CNC 8040 - Programming manual

Fagor Automation S. Coop.

Google Docs
Google Drive
Download [pdf]

File Info : application/pdf, 418 Pages, 4.45MB

man 8040m prg

PROGRAMMING MANUAL

·M· Model (Soft V11.1x)

(ref 0612)

(REF 0612)
·M· MODEL (SOFT V11.1X)

CNC 8040

All rights reserved. No part of this documentation may be copied, transcribed, stored in a data backup system or translated into any language without Fagor Automation's explicit consent.
The information described in this manual may be modified for technical reasons. FAGOR AUTOMATION S. COOP. Reserves the right to modify the contents of this manual without having to communicate such modifications.
Microsoft and Windows are registered trademarks of Microsoft Corporation USA. The other commercial trademarks belong to their respective owners.

The content of this manual and its validity for the product described here has been verified. Even so, involuntary errors are possible, thus no absolute match is guaranteed. Anyway, the contents of the manual is periodically checked making and including the necessary corrections in a future edition.
The examples described in this manual are for learning purposes. Before using them in industrial applications, they must be properly adapted making sure that the safety regulations are fully met.

INDEX

Programming manual

CHAPTER 1 CHAPTER 2 CHAPTER 3
CHAPTER 4 CHAPTER 5

About the product ................................................................................................................... I Declaration of conformity...................................................................................................... III Version history (M) ................................................................................................................ V Safety conditions .................................................................................................................. XI Warranty terms................................................................................................................... XV Material returning terms ................................................................................................... XVII Additional remarks............................................................................................................. XIX Fagor documentation ........................................................................................................ XXI

GENERAL CONCEPTS

1.1 1.1.1 1.2 1.3

Part programs............................................................................................................ 2 Considerations regarding the Ethernet connection................................................ 4
DNC connection ........................................................................................................ 5 Communication protocol via DNC or peripheral device............................................. 5

CREATING A PROGRAM

2.1 2.1.1 2.1.2 2.1.3

Program structure at the CNC ................................................................................... 8 Block header.......................................................................................................... 8 Program block........................................................................................................ 9 End of block ......................................................................................................... 10

AXES AND COORDINATE SYSTEMS

3.1 3.1.1 3.2 3.3 3.4 3.5 3.5.1 3.5.2 3.5.3 3.5.4 3.6 3.7 3.7.1 3.7.2

Axis nomenclature ................................................................................................... 11 Axis selection....................................................................................................... 12
Plane selection (G16, G17, G18, G19).................................................................... 13 Part dimensioning. Millimeters (G71) or inches (G70)............................................. 15 Absolute/incremental programming (G90, G91)...................................................... 16 Coordinate programming......................................................................................... 17
Cartesian coordinates.......................................................................................... 17 Polar coordinates................................................................................................. 18 Cylindrical coordinates......................................................................................... 20 Angle and one Cartesian coordinate ................................................................... 21 Rotary axes ............................................................................................................. 22 Work zones.............................................................................................................. 23 Definition of the work zones................................................................................. 23 Using the work zones .......................................................................................... 24

REFERENCE SYSTEMS

4.1 4.2 4.3 4.4 4.4.1 4.4.2 4.5

Reference points ..................................................................................................... 25 Machine reference (Home) search (G74)................................................................ 26 Programming with respect to machine zero (G53) .................................................. 27 Coordinate preset and zero offsets ......................................................................... 28
Coordinate preset and S value limitation (G92)................................................... 29 Zero offsets (G54..G59)....................................................................................... 30 Polar origin preset (G93) ......................................................................................... 32

ISO CODE PROGRAMMING

5.1 5.2 5.2.1 5.2.2 5.2.3 5.2.4 5.3 5.4 5.5 5.6

Preparatory functions .............................................................................................. 34 Feedrate F ............................................................................................................... 36
Feedrate in mm/min or inches/min (G94) ............................................................ 37 Feedrate in mm/rev.or inches/rev (G95).............................................................. 38 Constant surface speed (G96)............................................................................. 38 Constant tool center speed (G97)........................................................................ 38 Spindle speed (S) .................................................................................................... 39 Spindle selection (G28, G29) .................................................................................. 40 Synchronized spindles (G30, G77S, G78S) ............................................................ 41 Tool number (T) and tool offset (D) ......................................................................... 42

CNC 8040
·M· MODEL (SOFT V11.1X)

Programming manual CHAPTER 6

CHAPTER 7

CHAPTER 8

CNC 8040
·M· MODEL (SOFT V11.1X)

CHAPTER 9

5.7 Auxiliary function (M) ............................................................................................... 44 5.7.1 M00. Program stop .............................................................................................. 45 5.7.2 M01. Conditional program stop ........................................................................... 45 5.7.3 M02. End of program........................................................................................... 45 5.7.4 M30. End of program with return to the first block ............................................... 45 5.7.5 M03 Clockwise spindle rotation ........................................................................... 45 5.7.6 M04. Counterclockwise spindle rotation .............................................................. 45 5.7.7 M05. Spindle stop................................................................................................ 45 5.7.8 M06. Tool change code ....................................................................................... 46 5.7.9 M19. Spindle orientation ...................................................................................... 46 5.7.10 M41, M42, M43, M44. Spindle gear change........................................................ 47 5.7.11 M45. Auxiliary spindle / Live tool ......................................................................... 47

PATH CONTROL
6.1 Rapid traverse (G00) ............................................................................................... 49 6.2 Linear interpolation (G01)........................................................................................ 50 6.3 Circular interpolation (G02, G03)............................................................................. 51 6.4 Circular interpolation with absolute arc center coordinates (G06)........................... 56 6.5 Arc tangent to previous path (G08) ......................................................................... 57 6.6 Arc defined by three points (G09) ........................................................................... 58 6.7 Helical interpolation ................................................................................................. 59 6.8 Tangential entry at the beginning of a machining operation (G37).......................... 60 6.9 Tangential exit at the end of a machining operator (G38) ....................................... 62 6.10 Automatic radius blend (G36).................................................................................. 64 6.11 Chamfer (G39) ........................................................................................................ 65 6.12 Threading (G33) ...................................................................................................... 66 6.13 Variable pitch threads (G34) ................................................................................... 67 6.14 Move to hardstop (G52) .......................................................................................... 68 6.15 Feedrate "F" as an inverted function of time (G32) ................................................. 69 6.16 Tangential control (G45).......................................................................................... 70 6.16.1 Considerations about the G45 function ............................................................... 72 6.17 G145. Temporary cancellation of tangential control ................................................ 73

ADDITIONAL PREPARATORY FUNCTIONS

7.1 7.1.1 7.2 7.3 7.3.1 7.3.2 7.3.3 7.4 7.5 7.6 7.6.1 7.6.2 7.7 7.8 7.8.1 7.8.2 7.9

Interruption of block preparation (G04).................................................................... 75 G04 K0: Block preparation interruption and coordinate update........................... 77
Dwell (G04 K) .......................................................................................................... 78 Working with square (G07) and round (G05,G50) corners...................................... 79
G07 (square corner) ............................................................................................ 79 G05 (round corner) .............................................................................................. 80 Controlled round corner (G50)............................................................................. 81 Look-ahead (G51) ................................................................................................... 82 Mirror image (G10, G11. G12, G13, G14) ............................................................... 84 Scaling factor (G72) ................................................................................................ 86 Scaling factor applied to all axes. ........................................................................ 87 Scaling factor applied to one or more axes. ........................................................ 89 Pattern rotation (G73).............................................................................................. 91 Electronic axis coupling/uncoupling......................................................................... 93 Electronic axis coupling, slaving, (G77)............................................................... 94 Cancellation of the electronic axis coupling, slaving, (G78) ................................ 95 Axes toggle G28-G29 .............................................................................................. 96

TOOL COMPENSATION

8.1 8.1.1 8.1.2 8.1.3 8.1.4 8.2 8.3

Tool radius compensation (G40, G41, G42)............................................................ 98 Beginning of tool radius compensation................................................................ 99 Sections of tool radius compensation ................................................................ 102 Cancellation of tool radius compensation .......................................................... 103 Change of type of tool radius compensation while machining........................... 109
Tool length compensation (G43, G44, G15).......................................................... 110 Collision detection (G41 N, G42 N) ....................................................................... 112

CANNED CYCLES

9.1 9.2 9.2.1 9.3 9.4 9.5 9.6 9.6.1

Canned cycle definition ......................................................................................... 114 Influence zone of a canned cycle .......................................................................... 115
G79. Modification of the canned cycle parameters ........................................... 116 Canned cycle cancellation..................................................................................... 118 General considerations ......................................................................................... 119 Machining canned cycles ...................................................................................... 120 G69. Drilling canned cycle with variable peck ....................................................... 123
Basic operation.................................................................................................. 126

CHAPTER 10 CHAPTER 11 CHAPTER 12

Programming manual
9.7 G81. Drilling canned cycle..................................................................................... 128 9.7.1 Basic operation .................................................................................................. 129 9.8 G82. Drilling cycle with dwell ................................................................................. 130 9.8.1 Basic operation .................................................................................................. 131 9.9 G83. Deep-hole drilling canned cycle with constant peck ..................................... 132 9.9.1 Basic operation .................................................................................................. 134 9.10 G84. Tapping canned cycle................................................................................... 136 9.10.1 Basic operation .................................................................................................. 138 9.11 G85. Reaming canned cycle ................................................................................. 140 9.11.1 Basic operation .................................................................................................. 141 9.12 G86. Boring cycle with withdrawal in G00 ............................................................. 142 9.12.1 Basic operation .................................................................................................. 143 9.13 G87. Rectangular pocket canned cycle................................................................. 144 9.13.1 Basic operation .................................................................................................. 148 9.14 G88. Circular pocket canned cycle........................................................................ 151 9.14.1 Basic operation .................................................................................................. 155 9.15 G89. Boring cycle with withdrawal at work feedrate (G01).................................... 157 9.15.1 Basic operation .................................................................................................. 158

MULTIPLE MACHINING
10.1 G60: Multiple machining in a straight line.............................................................. 160 10.1.1 Basic operation .................................................................................................. 162 10.2 G61: Multiple machining in a rectangular pattern .................................................. 163 10.2.1 Basic operation .................................................................................................. 165 10.3 G62: Multiple machining in a grid pattern. ............................................................. 166 10.3.1 Basic operation .................................................................................................. 168 10.4 G63: Multiple machining in a circular pattern ........................................................ 169 10.4.1 Basic operation .................................................................................................. 171 10.5 G64: Multiple machining in an arc ......................................................................... 172 10.5.1 Basic operation .................................................................................................. 174 10.6 G65: Machining programmed with an arc-chord ................................................... 175 10.6.1 Basic operation .................................................................................................. 176

IRREGULAR POCKET CANNED CYCLE
11.1 2D pockets............................................................................................................. 179 11.1.1 Drilling operation................................................................................................ 183 11.1.2 Roughing operation ........................................................................................... 184 11.1.3 Finishing operation ............................................................................................ 187 11.1.4 Profile programming syntax ............................................................................... 190 11.1.5 Profile intersection ............................................................................................. 191 11.1.6 Profile programming syntax ............................................................................... 195 11.1.7 Errors ................................................................................................................. 197 11.1.8 Programming examples..................................................................................... 199 11.2 3D pockets............................................................................................................. 203 11.2.1 Roughing operation ........................................................................................... 207 11.2.2 Semi-finishing operation .................................................................................... 210 11.2.3 Finishing operation ............................................................................................ 212 11.2.4 Geometry of the contours or profiles ................................................................. 215 11.2.5 Profile programming syntax ............................................................................... 217 11.2.6 Composite 3D profiles ....................................................................................... 222 11.2.7 Profile stacking .................................................................................................. 225 11.2.8 Profile programming syntax ............................................................................... 226 11.2.9 Programming examples..................................................................................... 228 11.2.10 Errors ................................................................................................................. 241

PROBING
12.1 Probing (G75, G76) ............................................................................................... 244 12.2 Probing canned cycles .......................................................................................... 245 12.3 PROBE 1. Tool length calibrating canned cycle.................................................... 246 12.3.1 Calibrate the length or measure the length wear of a tool. ................................ 248 12.3.2 Calibrate the radius or measure the radius wear of a tool ................................. 251 12.3.3 Measure or calibrate the tool radius wear and tool length wear. ....................... 254 12.4 PROBE 2. Probe calibration canned cycle. ........................................................... 257 12.4.1 Basic operation .................................................................................................. 259 12.5 PROBE 3. Surface measuring canned cycle......................................................... 261 12.5.1 Basic operation .................................................................................................. 263 12.6 PROBE 4. Outside corner measuring canned cycle.............................................. 265 12.6.1 Basic operation .................................................................................................. 266 12.7 PROBE 5. Inside corner measuring canned cycle. ............................................... 268 12.7.1 Basic operation .................................................................................................. 269

CNC 8040
·M· MODEL (SOFT V11.1X)

iii

Programming manual
CHAPTER 13
CHAPTER 14 CHAPTER 15 APPENDIX
CNC 8040
·M· MODEL (SOFT V11.1X)

12.8 PROBE 6. Angle measuring canned cycle ............................................................ 271 12.8.1 Basic operation.................................................................................................. 272 12.9 PROBE 7. Outside corner and angle measuring canned cycle............................. 274 12.9.1 Basic operation.................................................................................................. 275 12.10 PROBE 8. Hole measuring canned cycle.............................................................. 277 12.10.1 Basic operation.................................................................................................. 278 12.11 PROBE 9. Boss measuring canned cycle. ............................................................ 280 12.11.1 Basic operation.................................................................................................. 281 12.12 PROBE 10. Rectangular part centering canned cycle........................................... 283 12.13 PROBE 11. Circular part centering canned cycle.................................................. 286
HIGH-LEVEL LANGUAGE PROGRAMMING
13.1 Lexical description ................................................................................................. 289 13.2 Variables ............................................................................................................... 291 13.2.1 General purpose parameters or variables ......................................................... 293 13.2.2 Variables associated with tools. ....................................................................... 295 13.2.3 Variables associated with zero offsets. ............................................................ 297 13.2.4 Variables associated with machine parameters ............................................... 298 13.2.5 Variables associated with work zones .............................................................. 299 13.2.6 Variables associated with feedrates ................................................................. 300 13.2.7 Variables associated with coordinates ............................................................. 302 13.2.8 Variables associated with electronic handwheels ............................................ 304 13.2.9 Variables associated with feedback .................................................................. 306 13.2.10 Variables associated with the main spindle ...................................................... 307 13.2.11 Variables associated with the second spindle .................................................. 309 13.2.12 Variables associated with the live tool ............................................................... 311 13.2.13 PLC related variables ........................................................................................ 312 13.2.14 Variables associated with local parameters ...................................................... 314 13.2.15 Sercos variables ................................................................................................ 315 13.2.16 Software & hardware configuration variables ................................................... 316 13.2.17 Variables associated with telediagnosis ........................................................... 318 13.2.18 Operating-mode related variables ................................................................... 320 13.2.19 Other variables .................................................................................................. 323 13.3 Constants .............................................................................................................. 327 13.4 Operators .............................................................................................................. 327 13.5 Expressions ........................................................................................................... 329 13.5.1 Arithmetic expressions ...................................................................................... 329 13.5.2 Relational expressions ...................................................................................... 330
PROGRAM CONTROL INSTRUCTIONS
14.1 Assignment instructions ........................................................................................ 332 14.2 Display instructions ............................................................................................... 333 14.3 Enabling-disabling instructions .............................................................................. 334 14.4 Flow control instructions ........................................................................................ 335 14.5 Subroutine instructions .......................................................................................... 337 14.6 Probe related instructions...................................................................................... 342 14.7 Interruption-subroutine instructions ....................................................................... 343 14.8 Program instructions ............................................................................................. 344 14.9 Screen customizing instructions ............................................................................ 348
ANGULAR TRANSFORMATION OF AN INCLINE AXIS
15.1 Turning angular transformation on and off ............................................................ 357 15.2 Freezing the angular transformation...................................................................... 358

ISO code programming ......................................................................................... 361

Program control instructions.................................................................................. 363

Summary of internal CNC variables. .................................................................... 367

Key codes.............................................................................................................. 373

Programming assistance screens of the system. .................................................. 381

Maintenance .......................................................................................................... 385

ABOUT THE PRODUCT

Basic characteristics.
Block processing time RAM memory Memkey Card memory
Hardware options.
Hard disk / compact flash Ethernet RS-232 serial line. 16 digital inputs and 8 outputs (I1 to I16 and O1 to O8) Another 40 digital inputs and 24 outputs (I65 to I104 and O33 to O56) Probe inputs Spindle (feedback input and analog output) Electronic handwheels 4 axes (feedback and analog voltage) Remote CAN modules, for digital I/O expansion (RIO). Sercos servo drive system for Fagor servo drive connection. CAN servo drive system for Fagor servo drive connection. 1M RAM - 2M Flash

12 ms 256 Kb expandable to 1Mb 512 Kb expandable to 2 Mb

Analog Option Option Standard Standard Option Standard Standard Standard Option Option
- - - - Option

Digital Option Option Standard Standard Option Standard Standard Standard Option Option Option Option Option

Before start-up, check that machine carrying this CNC meets the 89/392/CEE ruling.

CNC 8040

About the product

Software options.
Number of axes with standard software Number of axes with optional software Electronic threading Tool magazine management: Machining canned cycles Multiple machining Solid graphics Rigid tapping Tool live monitoring Probing canned cycles DNC COCOM version Profile editor Tool radius compensation Tangential control Retracing Setup assistance Irregular pockets with islands Digitizing Telediagnosis

Model

MC MCO T

TC TCO

----- ----- ----- -----

----- Stand Stand Stand Stand Stand Stand

----- Stand Stand ----- Stand Stand -----

----- Stand Stand ----- ----- ----- -----

----- Stand Stand Stand Stand Stand Stand

Stand Stand Stand Stand Stand Stand Stand

----- Opt Opt Opt Opt Opt Opt

Stand Stand Stand Stand Stand Stand Stand

Opt Opt Opt Opt Opt Opt Opt

Stand Stand Stand Stand Stand Stand Stand

Opt Opt Opt Opt Opt Opt Opt

Stand Stand Stand Stand Stand Stand Stand

----- Stand Stand Stand ----- ----- -----

----- Opt Opt ----- ----- ----- -----

Opt Opt Opt Opt Opt Opt Opt

CNC 8040
II

DECLARATION OF CONFORMITY

The manufacturer: Fagor Automation, S. Coop. Barrio de San Andrés s/n, C.P. 20500, Mondragón -Guipúzcoa- (Spain).

We declare:

We declare under our exclusive responsibility the conformity of the product: Numerical Control Fagor 8040 CNC

Referred to by this declaration with following directives:

Safety regulations.

EN 60204-1

Machine safety. Electrical equipment of the machines.

Regulation on electromagnetic compatibility.

EN 61000-4-3 EN 55011

Generic regulation on emissions in industrial environments. Radiated. Class A, Group 1.

EN 61000-6-2 EN 61000-4-2 EN 61000-4-3 EN 61000-4-4 EN 61000-4-6 EN 61000-4-8 EN 61000-4-11 ENV 50204

Generic regulation on immunity in industrial environments. Electrostatic Discharges. Radiofrequency Radiated Electromagnetic Fields. Bursts and fast transients. Conducted disturbance induced by radio frequency fields. Magnetic fields to Mains frequency Voltage fluctuations and Outages. Fields generated by digital radio-telephones

As instructed by the European Community Directives: 73/23/CEE modified by 93/68/ EEC on Low Voltage and 89/336/CEE modified by 92/31/EEC and 93/68/EEC on Electromagnetic Compatibility and their updates.
In Mondragón, July 15th, 2005.

CNC 8040

III

VERSION HISTORY (M)
(mill model)

Here is a list of the features added in each software version and the manuals that describe them.

The version history uses the following abbreviations:

INST

Installation manual

PRG

Programming manual

OPT

Operation manual

OPT-MC Operation manual for the MC option.

OPT-CO Manual of the CO manual

Software V05.3x
List of features
New expansion board models for the 8055i. Bus CANOpen to control remote digital I/Os at the 8055i New PLC instructions. IREMRD and OREMWR. Leadscrew error compensation on rotary axes between 0-360 degrees. PLC statistic deletion in a single softkey. Show only the XY plane in top-view graphics Absolute reference mark management via Sercos (a.m.p. REFVALUE).

April 2002
Manual
INST / PRG INST / OPT INST INST OPT OPT INST

Software V07.0x

December 2002

List of features
New languages; Basque and Russian. Additional command pulse. Exponential backlash peak. Additional command pulse. Eliminate inside backlash peaks when changing quadrants. Improved non-random tool magazine management. Safety limit for the axis feedrate. Safety limit for the spindle speed. Execute the additional compensation block at the beginning of the next block. Jerk control in look-ahead. New graphics option. Mill graphics with changed line graphics. Path-jog mode. Update the variables of the machine parameters from the OEM program or subroutine. HARCON variable returns the type of LCD and turbo board. Variables to consult the actual (real) and theoretical feedrate of each axis. Variable to consult the coordinates shown on the screen for each axis. Variable to consult the position indicated by the Sercos drive of each axis. Variable to consult the coordinate programmed in a block of a program. Variable to consult the position indicated by the Sercos drive of the first and second spindles. Variable to consult the theoretical turning speed of the first and second spindles. Variable to consult the maximum spindle speed. Feedback related variables. Variable to consult a single PLC mark. Variable to consult the PROBE cycle being executed. Variable to know the number of the screen, created with WGDRAW, that is being consulted. Variable to know the number of the item (element), created with WGDRAW, that is being consulted. Machine safety. Hardware errors disable the [CYCLE START] key. Machine safety. Maximum machining feedrate.

Manual
INST INST INST INST INST INST INST INST INST INST / OPT INST / PRG INST / PRG INST / PRG INST / PRG INST / PRG INST / PRG INST / PRG INST / PRG INST / PRG INST / PRG INST / PRG INST / PRG INST / PRG INST / PRG
INST INST

CNC 8040
V

Version history (M)

List of features
Mandatory axis homing after feedback alarm when using direct feedback. The "SERCOS816" board is now recognized. Write-protect the user arithmetic parameters (P1000-P1255) and OEM arithmetic parameters (P2000-P2255). New command of the configuration language. UNMODIFIED command. Synchronize a PLC axis with a CNC axis. Axes (2) controlled by a drive. The direction of the command LOOPCHG is defined on both axes. Tool change via PLC. New user arithmetic parameters (P1000 - P1255). New OEM arithmetic parameters (P2000 - P2255). Improved PROBE 1 cycle. Calibrate and/or measure tool radius wear and/or tool length wear. RPT instruction. Execute blocks of a program located in RAM memory. Look-ahead. It analyzes up to 75 blocks in advance. OEM (manufacturer's) subroutines. Range SUB10000 - SUB20000. Oscilloscope function. Load the version without using an external microprocessor. The screen data (feedrates, coordinates, etc.) do not show their zeros to the left. Blackbox for registering errors. Telediagnosis through the RS232 serial line. Telediagnosis via WinDNC. Correct tool wear from tool inspection mode. Improvements to the profile editor. Save and load the parameters of the Sercos or CAN drive through the serial line. MC option. Restore the last F, S and Smax values on power-up. MC option. Possibility of hiding unused operations or cycles. MC option. There are auxiliary M functions in the cycles. MC option. Improvements for executing a part-program. MC option. It shows warning messages on a green stripe. MC option. Limitations to tool calibration when there is a program in execution or in tool inspection mode. MC option. Tool measuring and calibrating cycle. MC option. Icon to select between available options. MC option. Threading cycle. It is possible to indicate the type of thread defining the pitch and the speed (S) or the feedrate (F) and the speed (S). MC option. Milling cycle. When defining the points of the profile, when leaving a data blank, the cycle assumes that it is the repetition of the previous one. MC option. Milling cycle. It is possible to define the incremental points or coordinates. MC option. Multi-point multiple positioning cycle. When defining the points of the profile, when leaving a data blank, the cycle assumes that it is the repetition of the previous one. MC option. Multi-point multiple positioning cycle. It is possible to define the incremental points or coordinates.

Manual
INST
INST
INST INST INST INST PRG PRG PRG PRG PRG PRG OPT OPT
OPT OPT OPT OPT OPT INST INST INST INST OPT-MC OPT-MC OPT-MC
OPT-MC OPT-MC OPT-MC
OPT-MC
OPT-MC OPT-MC
OPT-MC

Software V07.1x

July 2003

CNC 8040

List of features
New 24-character validation codes. Pin ·9· of connector X1 (RS232 serial line) no longer supplies 5 V. Smooth stop of probing movement. Machining in round corner mode when changing the tool offset. Bi-directional leadscrew compensation. The management of the distance-coded reference mark via Sercos may be carried out through the drive's second feedback. The drive version must be V4.10 or V5.10 ( or greater). Machine parameters modifiable from an OEM program using variables General machine parameters modifiable from the oscilloscope: TLOOK. Axis machine parameters that may be modified from the oscilloscope: MAXFEED, JOGFEED. Improvements to look ahead. Machining feedrate variations are now smoother thanks to filtered acc/dec.

Manual
INST INST INST INST
INST / OEM OPT OPT

Version history (M)

Software V09.0x

February 2004

List of features
MEM CARD slot as floppy drive (CARD-A). Tandem axes Stop block preparation when executing a new "T". Execute the stop signal when done with the "T" change. Compact-flash type hard disk and Ethernet. Incline axis. Select the behavior of the feedrate for F0. On Gantry axes, cross compensation is also applied to the slave axis. Variable to select the active probe input. Variable to know the address of the I/O CAN. Variables to read the number of local and remote digital I/O available. The HARCON variable recognizes Ethernet and compact flash. While compiling the PLC program, the outputs are initialized to zero. New marks to park the spindles. Name the logic inputs and outputs with the axis name Parameter RAPIDEN assumes the value of ·2·. Rapid key controlled by PLC. Ending the execution of a block using a PLC mark (BLOABOR, BLOABORP). Additive coupling between axes. The EXEC and OPEN instructions may be used with Ethernet. G2/G3. The center coordinates may be left out if their value is zero. General parameters that may be modified from the oscilloscope or from an OEM program: CODISET. Axis parameters that may be modified from the oscilloscope or from an OEM program: MAXFLWE1, MAXFLWE2. Connection to a remote hard disk. Connection to a PC through WinDNC. Access the CNC's hard disk from a PC via FTP. Telediagnosis. Normal phone call. Telediagnosis. Disable the CNC screen and keyboard from the PC. Functions M41 through M44 admit subroutines when the gear change is automatic. MC option. Configuration as two and half axes. MC option. Accessing cycles and programs from the auxiliary screen. MC option. ISO programming assistance. MC option. Zero offset table management. MC option. After an execution or simulation error, it indicates the erroneous cycle. MC option. In execution or simulation, it indicates the cycle number. MC option. The CNC highlights the axis being moved in jog or with handwheels. MC option. Copying a profile. MC option. Select a program by indicating its number. MC option. Selection of the starting point in rectangular pockets and bosses. MC option. Pockets and bosses may be assigned to multiple positioning cycles. MC option. Configuration of two and half axes. CO option. Copying a profile.

Manual
INST / OPT INST INST INST INST INST / PRG INST INST INST / PRG INST / PRG INST / PRG INST / PRG
INST INST INST INST INST PRG PRG INST/PRG/OPT
INST/PRG/OPT
INST / OPT INST / OPT INST / OPT OPT OPT PRG INST INST OPT-MC OPT-MC OPT-MC OPT-MC OPT-MC OPT-MC OPT-MC OPT-MC OPT-MC OPT-MC OPT-CO

Software V09.1x

December 2004

List of features
Calculation of central unit heat dissipation . Frequency filters for axes and spindles. When activating tool radius compensation in the first motion block even if there is no movement of the plane axes. CAN servo system. 8055i model. New board "Axes2". Sercos transmission speed at 8 MHz and 16 MHz. Retracing function. If RETRACAC=2 , the retrace function does not stop at the M functions. Retracing function. The RETRACAC parameter is initialized with [SHIFT][RESET]. Retracing function. The number of blocks being retraced has been increased to 75. New variables for APOS(X-C) and ATPOS(X-C) to consult part coordinates. New variable DNCSTA to consult DNC communication status. New variable TIMEG to consult the status of the timer programmed with G4. Manual intervention with additive handwheel. A CNC emergency disables the SPENA signals and the Sercos drive brakes using the emergency ramps. Maintain G46 when the home search does not involve any axis of the angular transformation.

Manual
INST INST INST
INST INST INST INST
INST INST INST INST INST / OPT INST
INST / PRG

CNC 8040
VII

List of features
COMPMODE (P175). New tool radius compensation methods. Automatic keyboard type identification. Variable to indicate whether the handwheel selector button has been pressed or not. Protect the access from the network to the hard disk using a password. The HARCON variable recognizes the new axis board "Axes2". Variable to analog the value of the analog inputs. New MEXEC instruction. Execute a modal part-program. Look-ahead. Functions G74, G75 and G76 are possible. Up to 319 G functions now available. Machine parameters that may be modified from the oscilloscope or from an OEM program: REFVALUE, REFDIREC, FLIMIT, SLIMIT. Accessing the variables of the auxiliary spindle drive from the oscilloscope. The simulations without axis movement ignore the G4. Sharing the CNC's hard disk with password. Telediagnosis. Advanced phone call. Telediagnosis through the Internet. Telediagnosis. Disconnect the CNC from the Ethernet during telediagnosis. Maintain the feedrate selected in simulation.

Manual
INST / PRG INST INST INST INST / PRG INST / PRG PRG PRG PRG INST/PRG/OPT
OPT OPT INST / OPT OPT OPT OPT OPT

Version history (M)

Software V9.13
List of features
New table to define the Sercos power with the Sercos816 board. 600 µs delay at the Sercos bus for transmissions at 8 MHz and 16 MHz. Hirth axis pitch may be set in degrees via parameters. Rollover positioning axis. Movement in G53 via the shortest way.

April 2005
Manual
INST INST INST INST

Software V9.14x
List of features
New table to define the Sercos power with the Sercos816 board.

May 2005
Manual
INST

Software V11.01

Ref. 0508

CNC 8040

List of features
Analog I/O expansion and PT100 CAN bus speed with remote digital I/O modules The CNC supports Memkey Card + Compact Flash or KeyCF File explorer to show the contents of the storage devices Loading the version from the Memkey card o from the hard disk New way to search home that may be selected through g.m.p. I0TYPE=3 Improved block search. Switching from simulation to execution New repositioning mode that is activated by setting g.m.p. REPOSTY=1 Square-sine ramps on open-loop spindle Numbering of the local inputs/outputs of the expansion modules using plc machine parameters Default value of axis and spindle machine parameter ACFGAIN = YES Setting axis parameters FFGAIN and FFGAIN2 with two decimals Up to 400 (DEF) symbols now available at the PLC New HTOR variable that indicates the tool radius being used by the CNC Longitudinal axis definition with G16 Part centering with a probe Rectangular part centering cycle (PROBE 10) Circular part centering cycle (PROBE 11) Generating an ISO-coded program

Manual
INST INST OPT INST / OPT OPT INST INST / OPT INST/PRG/OPT INST INST INST INST INST INST INST / PRG OPT-MC PRG PRG OPT-MC

VIII

Version history (M)

Software V11.11

Ref. 0602

List of features
New G145. Temporary cancellation of tangential control Handwheel feedback taken to a free feedback connector New variables: RIP, GGSE, GGSF, GGSG, GGSH, GGSI, GGSJ, GGSK, GGSL, GGSM, PRGSP, SPRGSP and PRBMOD Automatic keyboard type identification Improved part centering with a probe (PROBE 10 - PROBE 11) G04 K0. Block preparation interruption and coordinate update Possibility to view all the active PLC messages Improved part centering with a probe

Manual
PRG INST INST
INST / PRG PRG PRG OPT-MC OPT-MC

Software V11.13
List of features
Smooth stop when homing the axes, it may be selected with a.m.p. I0TYPE

Ref. 0606
Manual
INST

Software V11.14
List of features
Selecting the additive handwheel as handwheel associated with the axis

Ref. 0608
Manual
INST

CNC 8040
IX

CNC 8040
X

Version history (M)

SAFETY CONDITIONS

Read the following safety measures in order to prevent damage to personnel, to this product and to those products connected to it.
This unit must only be repaired by personnel authorized by Fagor Automation.
Fagor Automation shall not be held responsible for any physical or material damage derived from the violation of these basic safety regulations.

Precautions against personal damage
Interconnection of modules Use the connection cables provided with the unit.
Use proper Mains AC power cables To avoid risks, use only the Mains AC cables recommended for this unit.
Avoid electrical overloads In order to avoid electrical discharges and fire hazards, do not apply electrical voltage outside the range selected on the rear panel of the central unit.
Ground connection. In order to avoid electrical discharges, connect the ground terminals of all the modules to the main ground terminal. Before connecting the inputs and outputs of this unit, make sure that all the grounding connections are properly made.
Before powering the unit up, make sure that it is connected to ground In order to avoid electrical discharges, make sure that all the grounding connections are properly made.
Do not work in humid environments In order to avoid electrical discharges, always work under 90% of relative humidity (non-condensing) and 45 ºC (113º F).
Do not work in explosive environments In order to avoid risks, damage, do no work in explosive environments.

Precautions against product damage
Working environment This unit is ready to be used in industrial environments complying with the directives and regulations effective in the European Community Fagor Automation shall not be held responsible for any damage suffered or caused when installed in other environments (residential or homes).

CNC 8040

Safety conditions

Install this unit in the proper place
It is recommended to install the CNC away from coolants, chemical products, possible blows etc. which could damage it.
This unit complies with the European directives on electromagnetic compatibility. Nevertheless, it is recommended to keep it away from sources of electromagnetic disturbance such as.
· Powerful loads connected to the same AC power line as this equipment.
· Nearby portable transmitters (Radio-telephones, Ham radio transmitters).
· Nearby radio / TC transmitters.
· Nearby arc welding machines
· Nearby High Voltage power lines
· Etc. Enclosures
The manufacturer is responsible of assuring that the enclosure involving the equipment meets all the currently effective directives of the European Community. Avoid disturbances coming from the machine tool
The machine tool must have decoupled all those elements capable of generating interference (relay coils, contactors, motors, etc.)
· DC relay coils. Diode type 1N4000.
· AC relay coils. RC connected as close to the coils as possible with approximate values of R=220 / 1 W and C=0,2 µF / 600 V.
· AC motors. RC connected between phases, with values of R=300 / 6 W and C=0,47 µF / 600 V
Use the proper power supply
Use an external regulated 24 Vdc power supply for the inputs and outputs. Grounding of the power supply
The zero volt point of the external power supply must be connected to the main ground point of the machine. Analog inputs and outputs connection
It is recommended to connect them using shielded cables and connecting their shields (mesh) to the corresponding pin. Ambient conditions
The working temperature must be between +5 ºC and +40 ºC (41ºF and 104º F)
The storage temperature must be between -25 ºC and +70 ºC. (-13 ºF and 158 ºF) Central unit enclosure (8055i CNC)
Guarantee the required gaps between the central unit and each wall of the enclosure. Use a DC fan to improve enclosure ventilation. Power switch
This power switch must be mounted in such a way that it is easily accessed and at a distance between 0.7 meters (27.5 inches) and 1.7 meters (5.5ft) off the floor.

XII

Protections of the unit itself
Central Unit It has a 4 A 250V external fast fuse (F).

Safety conditions

Inputs-Outputs All the digital inputs and outputs have galvanic isolation via optocouplers between the CNC circuitry and the outside.
Precautions during repair

Do not open this unit. Only personnel authorized by Fagor Automation may open this unit.
Do not handle the connectors with the unit connected to mains. Before manipulating the connectors (inputs/outputs, feedback, etc.) make sure that the unit is not connected to AC power.

Safety symbols
Symbols which may appear on the manual.
Symbol for danger or prohibition. It indicates actions or operations that may cause damage to people or to units.

Warning or caution symbol.
It indicates situations that may be caused by certain operations and the actions to be taken to prevent them.

Obligation symbol. It indicates actions and operations that must be carried out.

Information symbol. It indicates notes, warnings and suggestions.

CNC 8040

XIII

CNC 8040
XIV

Safety conditions

WARRANTY TERMS
All products manufactured or marketed by Fagor Automation has a warranty period of 12 months from the day they are shipped out of our warehouses. The mentioned warranty covers repair material and labor costs, at Fagor facilities, incurred in the repair of the products. Within the warranty period, Fagor will repair or replace the products verified as being defective. Fagor is committed to repairing or replacing its products from the time when the first such product was launched up to 8 years after such product has disappeared from the product catalog. It is entirely up to Fagor to determine whether a repair is to be considered under warranty. Excluding clauses The repair will take place at our facilities. Therefore, all shipping expenses as well as travelling expenses incurred by technical personnel are NOT under warranty even when the unit is under warranty. This warranty will be applied so long as the equipment has been installed according to the instructions, it has not been mistreated or damaged by accident or negligence and has been manipulated by personnel authorized by Fagor. If once the service call or repair has been completed, the cause of the failure is not to be blamed the FAGOR product, the customer must cover all generated expenses according to current fees. No other implicit or explicit warranty is covered and Fagor Automation shall not be held responsible, under any circumstances, of the damage which could be originated. Service agreements Service and Maintenance Contracts are available for the customer within the warranty period as well as outside of it.
CNC 8040
XV

CNC 8040
XVI

Warranty terms

MATERIAL RETURNING TERMS
When returning the remote modules or the central unit, pack it in its original package and with its original packaging material. If not available, pack it as follows: 1. Get a cardboard box whose three inside dimensions are at least 15 cm (6 inches)
larger than those of the unit. The cardboard being used to make the box must have a resistance of 170 kg (375 lb). 2. Attach the unit label indicating the owner of the unit, his/her address, the name of the contact person, the type of unit and the serial number. 3. In case of failure, also indicate the symptom and a short description. 4. Wrap the unit in a polyethylene roll or similar material to protect it. 5. When sending the central unit, above all protect the screen 6. Pad the unit inside the cardboard box with polyurethane foam on all sides. 7. Seal the cardboard box with packing tape or industrial staples.
CNC 8040
XVII

CNC 8040
XVIII

Material returning terms

ADDITIONAL REMARKS
Mount the CNC away from coolants, chemical products, blows, etc. which could damage it. Before turning the unit on, verify that the ground connections have been properly made. In case of a malfunction or failure, disconnect it and call the technical service. Do not open this unit.
CNC 8040
XIX

CNC 8040
XX

Additional remarks

FAGOR DOCUMENTATION

OEM Manual It is directed to the machine builder or person in charge of installing and starting-up the CNC.
USER-M manual Directed to the end user. It describes how to operate and program in M mode.
USER-T manual Directed to the end user. It describes how to operate and program in T mode.
MC Manual Directed to the end user. It describes how to operate and program in MC mode. It contains a self-teaching manual.
TC Manual Directed to the end user. It describes how to operate and program in TC mode. It contains a self-teaching manual.
MCO/TCO model Directed to the end user. It describes how to operate and program in MCO and TCO mode.
Examples-M manual Directed to the end user. It contains programming examples for the M mode.
Examples-T manual Directed to the end user. It contains programming examples for the T mode.
WINDNC Manual It is directed to people using the optional DNC communications software. It is supplied in a floppy disk with the application.
WGDRAW Manual Directed to people who use the WGDRAW to create screens. It is supplied in a floppy disk with the application.

CNC 8040

XXI

CNC 8040
XXII

Fagor documentation

GENERAL CONCEPTS

The CNC can be programmed both at the machine (from the front panel) or from external peripheral devices (tape reader/cassette recorder, computer, etc). Memory available to the user for carrying out the part programs is 1 Mbyte.
The part programs and the values in the tables which the CNC has can be entered from the front panel, from a pc (DNC) or from a peripheral.
Entering programs and tables from the front panel.
Once the editing mode or desired table has been selected, the CNC allows you to enter data from the keyboard.
Entering programs and tables from a Computer (DNC) or Peripheral Device.
The CNC allows data to be interchanged with a computer or peripheral device, using RS232C and RS422 cables.
If this is controlled from the CNC, it is necessary to preset the corresponding table or part program directory (utilities) you want to communicate with.
Depending on the type of communication required, the serial port machine parameter "PROTOCOL" should be set.
"PROTOCOL" = 0 if the communication is with a peripheral device. "PROTOCOL" = 1 if the communication is via DNC.

CNC 8040
·M· MODEL (SOFT V11.1X)
1

Programming manual
1.1 Part programs
The operating manual describes the different operating modes. Refer to that manual for further information.

GENERAL CONCEPTS Part programs

Editing a part-program
To create a part-program, access the Edit mode.
The new part-program edited is stored in the CNC's RAM memory. A copy of the partprograms may be stored in the "MemKey Card", at a PC connected through serial line 1 or 2 or in the hard disk.
To transmit a program to a PC through serial line 1 or 2, proceed as follows: 1. Execute the application "Fagor50.exe" or "WinDNC.exe" at the PC. 2. Activate DNC communications at the CNC. 3. Select the work directory at the CNC. It is selected from the Utilities mode,
option Directory \Serial L \Change directory
In Edit mode, it is possible to modify part-programs residing in the CNC's RAM memory. To modify a program stored in the "MemKey Card", in a PC or in the hard disk, it must be previously copied into RAM memory.

Executing and editing a part-program
Part-programs stored anywhere may be executed or simulated. Simulation is carried out in the Simulation mode, whereas the execution is done in the Automatic mode
When executing or simulating a part-program, bear in mind the following points: · Only subroutines stored in the CNC's RAM memory can be executed. Therefore, to execute a subroutine stored in the "MemKey Card", in a PC or in the hard disk, it must be first copied into the CNC's RAM memory. · The GOTO and RPT instructions cannot be used in programs that are executed from a PC connected through the serial lines. · From a program in execution, another program can be executed which is in RAM memory, in the "MemKey Card", in a PC or in the hard disk using the EXEC instruction.
The user customizing programs must be in RAM memory so the CNC can execute them.

CNC 8040

Utilities operating mode.
The Utilities mode, lets display the part-program directory of all the devices, make copies, delete, rename and even set the protections for any of them.

·M· MODEL (SOFT V11.1X)

Operations that may be carried out with part-programs.

Programming manual

RAM CARD A HD

DNC

See the program directory of ... See the subroutine directory of ...

Yes

Create the work directory from ... Change the work directory from ...

Yes

Edit a program from ... Modify a program from ... Delete a program from ...

Yes

Copy from/to RAM memory to/from ... Copy from/to CARD A to/from ... Copy from/to HD to/from ... Copy from/to DNC to/from ...

Yes

Rename a program from ... Change the comment of a program from ... Change the protections of a program from ...

Yes

Execute a part-program from ...

Yes

Execute a user program from ...

Yes

Execute a PLC program from ...

Yes

Execute programs with GOTO or RPT instructions from ...

Yes

Execute subroutines residing in ...

Yes

Execute programs with the EXEC instruction, in RAM from ...

Yes

Execute programs with the EXEC instruction, in CARD A from ...

Yes

Execute programs with the EXEC instruction, in HD from ...

Yes

Execute programs with the EXEC instruction, in DNC from ...

Yes

Open programs with the OPEN instruction, in RAM from ... Open programs with the OPEN instruction, in CARD A from ... Open programs with the OPEN instruction, in HD from ... Open programs with the OPEN instruction, in DNC from ...

Yes

Via Ethernet: See from a PC the program directory of ... See from a PC the subroutine directory of ... See from a PC, a directory in ...

Yes

(*) If it is not in RAM memory, it generates the executable code in RAM and it executes it.

GENERAL CONCEPTS Part programs

Ethernet
When having the Ethernet option and if the CNC is configured as another node within the computer network, the following operations are possible from any PC of the network:
· Access the part-program directory of the Hard Disk. · Edit, modify, delete, rename, etc. the programs stored on the hard disk. · Copy programs from the hard disk to the PC and vice versa.
To configure the CNC as another node within the computer network, see the installation manual.

CNC 8040

·M· MODEL (SOFT V11.1X)

Programming manual
1.1.1 Considerations regarding the Ethernet connection
When configuring the CNC as another node in the computer network, the programs stored in the hard disk module (HD) may be edited and modified from any PC.

GENERAL CONCEPTS Part programs

Instructions for setting up a PC to access CNC directories
To set up the PC to access the CNC directories, we recommend to proceed as follows. 1. Open the «Windows Explorer» 2. On the «Tools» menu, select the «Connect to Network Drives» option. 3. Select the drive, for example «D». 4. Indicate the path. The path will be the CNC name followed by the name of the
shared directory. For example: \\FAGORCNC\CNCHD
5. When selecting the option: «Connect again when initiating the session», the selected CNC will appear on each power-up as another path of the «Windows Explorer» without having to define it again.

CNC 8040
·M· MODEL (SOFT V11.1X)

Data format
This connection is established through Ethernet and, therefore, the CNC does not control the syntax of the programs while they are received or modified. However, whenever accessing the program directory of the Hard Disk (HD), the following verification takes place:
File name.
The file number must always have 6 digits and the extension PIM (for milling) or PIT (for lathe).
Examples: 001204.PIM 000100.PIM 123456.PIT 020150.PIT
If the file has been given the wrong name, for example: 1204.PIM or 100.PIT, the CNC will not change it, but it will display it with the comment "****************". The file name cannot be modified at the CNC; it must be edited from the PC to correct the error.
File size.
If the file is empty (size = 0) the CNC will display it with the comment "********************".
The file can be edited or deleted either from the CNC or from the PC.
First line of the program.
The first line of the program must have the % character, the comment associated with the file (up to 20 characters) and between the 2 commas (,) the program attributes O (OEM), H (hidden), M (modifiable), X (executable).
%Comment ,MX, % ,OMX,
If the first line does not exist, the CNC will display the program with an empty comment and with the modifiable (M) and executable (X) attributes.
When the format of the first line is wrong, the CNC does not modify it, but it displays it with the comment "****************". The file can be edited or deleted either from the CNC or from the PC.
The format is incorrect when the comment has more than 20 characters, a comma (,) is missing to group the attributes or there is a strange character in the attributes.

1.2 DNC connection

Programming manual

1.3

The CNC offers as optional feature the possibility of working in DNC (Distributed Numerical Control), enabling communication between the CNC and a computer to carry out the following functions:
· Directory and delete commands. · Transfer of programs and tables between the CNC and a computer. · Remote control of the machine. · The ability to supervise the status of advanced DNC systems.
Communication protocol via DNC or peripheral device

GENERAL CONCEPTS DNC connection

This type of communication enables program-and-table transfer commands, plus the organization of CNC directories such as the computer directory, for copying/deleting programs, etc. to be done either from the CNC or the computer.

When you want to transfer files, it is necessary to follow this protocol:
· The "%" symbol will be used to start the file, followed by the program comment (optional), of up to 20 characters.
Then, and separated by a comma ",", comes the protection of each file, read, write, etc. These protections are optional and need not be programmed.
To end the file header, RT (RETURN ) or LF (LINE FEED) characters should be sent separated by a comma (",").
Example: %Fagor Automation, MX, RT
· Following the header, the file blocks should be programmed. These will all be programmed according to the programming rules indicated in this manual. After each block, to separate it from the others, the RT (RETURN ) or LF (LINE FEED) characters should be used.
Example: N20 G90 G01 X100 Y200 F2000 LF
(RPT N10, N20) N3 LF

If communication is made with a peripheral device, you will need to send the `end of file' command. This command is selected via the machine parameter for the serial port: "EOFCHR", and can be one of the following characters :

ESC

ESCAPE

EOT

END OF TRANSMISSION

SUB

SUBSTITUTE

EXT

END OF TRANSMISSION

CNC 8040
·M· MODEL (SOFT V11.1X)
5

Programming manual
1.
CNC 8040
·M· MODEL (SOFT V11.1X)
6

GENERAL CONCEPTS Communication protocol via DNC or peripheral device

CREATING A PROGRAM

A CNC program consists of a series of blocks or instructions. These blocks or instructions are made of words composed of capital letters and numerical format.
The CNC's numerical format consists of : · The signs . (decimal points, + (plus), - (minus). · Digits 0 1 2 3 4 5 6 7 8 9.
Programming allows spaces between letters, numbers and symbols, in addition to ignoring the numerical format if it has zero value, or a symbol if it is positive.
The numeric format of a word may be replaced by an arithmetic parameter when programming. Later on, during execution, the CNC will replace the arithmetic parameter by its value. For example, if XP3 has been programmed, during execution the CNC will replace P3 by its numerical value, obtaining results such as X20, X20.567, X-0.003, etc.

CNC 8040
·M· MODEL (SOFT V11.1X)
7

Programming manual
2.1 Program structure at the CNC

CREATING A PROGRAM Program structure at the CNC

All the blocks which make up the program have the following structure: Block header + program block + end of block
2.1.1 Block header
The block header is optional, and may consist of one or more block skip conditions and by the block number or label. Both must be programmed in this order.
Block skip condition. "/", "/1", "/2", "/3".
These three block skip conditions, given that "/" and "/1" are the same, they are governed by the marks BLKSKIP1, BLKSKIP2 and BLKSKIP3 of the PLC. If any of these marks is active, the CNC will not execute the block or blocks in which it has been programmed; the execution takes place in the following block.
Up to 3 skip conditions can be programmed in one block; they will be evaluated one by one, respecting the order in which they have been programmed.
The control reads 20 blocks ahead of the one being executed in order to calculate in advance the path to be run. The condition for block skip will be analyzed at the time when the block is read i.e. 20 blocks before execution.
If the block skip needs to be analyzed at the time of execution, it is necessary to interrupt the block preparation, by programming G4 in the previous block.
Label or block number. N(0-9999).
This is used to identify the block, and is only used when block references or jumps are made. They are represented by the letter N followed by up to 4 digits (0-9999).
No particular order is required and the numbers need not be sequential. If two or more blocks with the same label number are present in the same program, the CNC will always give priority to the first number.
Although it is not necessary to program it, by using a softkey the CNC allows the automatic programming of labels. The programmer can select the initial number and the step between labels.

CNC 8040
·M· MODEL (SOFT V11.1X)
8

2.1.2 Program block

Programming manual

This is written with commands in ISO and high level languages. To prepare a program, blocks written in both languages will be used, although each one should be edited with commands in just one language.
ISO language.
This language is specially designed to control axis movement, as it gives information and movement conditions, in addition to data on feedrate. It offers the following types of functions.
· Preparatory functions for movement, used to determine geometry and working conditions, such as linear and circular interpolations, threading, etc.
· Control functions for axis feedrate and spindle speeds. · Tool control functions. · Complementary functions, with technological instructions.
High level language.
This enables access to general purpose variables and to system tables and variables.
It gives the user a number of control sentences which are similar to the terminology used in other languages, such as IF, GOTO, CALL, etc. It also allows the use of any type of expression (arithmetic, referential, or logical).
It also has instructions for the construction of loops, plus subroutines with local variables. A local variable is one that is only recognized by the subroutine in which it has been defined.
It is also possible to create libraries, grouping subroutines with useful and tested functions, which can be accessed from any program.

CREATING A PROGRAM Program structure at the CNC

CNC 8040
·M· MODEL (SOFT V11.1X)
9

Programming manual
2.1.3 End of block

CREATING A PROGRAM Program structure at the CNC

The end of block is optional and may consist of the indication of number of repetitions of the block and of the block comment. Both must be programmed in this order.
Number of block repetitions. N(0-9999)
This indicates the number of times the block will be executed. The number of repetitions is represented by the letter N followed by up to 4 digits (0-9999). The active machining operation does not take place if N0 is programmed; only the movement programmed within the block takes place.
Movement blocks can only be repeated which, at the time of their execution, are under the influence of a modal subroutine. In these cases, the CNC executes the programmed move and the active machining operation (canned cycle or modal subroutine) the indicated number of times.
Block comment
The CNC allows you to incorporate any kind of information into all blocks in the form of a comment. The comment is programmed at the end of the block, and should begin with the character ";" (semicolon).
If a block begins with ";" all its contents will be considered as a comment, and it will not be executed.
Empty blocks are not permitted. They should contain at least one comment.

CNC 8040
·M· MODEL (SOFT V11.1X)
10

AXES AND COORDINATE SYSTEMS

3.1

Given that the objective of the CNC is to control the movement and positioning of axes, it is necessary to determine the position of the point to be reached through the coordinates.
The CNC allows you to use absolute, relative or incremental coordinates throughout the same program.
Axis nomenclature

The axes are named according to DIN 66217.

Characteristics of the system of axes:

X and Y

main movements on the main work plane of the machine.

parallel to the main axis of the machine, perpendicular to the main XY

plane.

U, V, W

auxiliary axes parallel to X, Y, Z respectively.

A, B, C

Rotary axes on each axis X, Y, Z.

CNC 8040

·M· MODEL (SOFT V11.1X)

Programming manual

The drawing below shows an example of the nomenclature of the axes on a millingprofiling machine with a tilted table.

AXES AND COORDINATE SYSTEMS Axis nomenclature

3.1.1 Axis selection
Of the 9 possible axes that may exist, the CNC allows the manufacturer to select up to 7 of them. Moreover, all the axes should be suitably defined as linear/rotary, etc. through the axis machine parameters which appear in the Installation and Start-up Manual. There is no limitation to the programming of the axes, and interpolations can be made simultaneously with up to 7 axes.
CNC 8040
·M· MODEL (SOFT V11.1X)
12

3.2 Plane selection (G16, G17, G18, G19)

Programming manual

Plane selection should be made when the following are carried out : · Circular interpolations. · Controlled corner rounding. · Tangential entry and exit. · Chamfer. · Coordinate programming in Polar coordinates. · Machining canned cycles. · Pattern rotation. · Tool radius Compensation. · Tool length compensation.
The "G" functions which enable selection of work planes are as follows : G16 axis1 axis2 axis3.Enables selection of the desired work plane, plus the direction
of G02 G03 (circular interpolation), axis1 being programmed as the abscissa axis and axis2 as the ordinate axis. The axis3 is the longitudinal axis along which tool length compensation is applied.

AXES AND COORDINATE SYSTEMS Plane selection (G16, G17, G18, G19)

G17. G18. G19.

Selects the XY plane Selects the ZX plane Selects the YZ plane

CNC 8040
·M· MODEL (SOFT V11.1X)
13

Programming manual

The G16, G17, G18 and G19 functions are modal and incompatible among themselves. The G16 function should be programmed on its own within a block.

AXES AND COORDINATE SYSTEMS Plane selection (G16, G17, G18, G19)

The G17, G18, and G19 functions define two of the three main axes (X, Y, Z) as belonging to the work plane, and the other as the perpendicular axis to the same.
When radius compensation is done on the work plane, and length compensation on the perpendicular axis, the CNC does not allow functions G17, G18, and G19 if any one of the X, Y, or Z axes is not selected as being controlled by the CNC.
On power-up, after executing M02, M30 or after EMERGENCY or RESET, the CNC will assume that the plane defined by the general machine parameter as "IPLANE" is the work plane.

CNC 8040
·M· MODEL (SOFT V11.1X)
14

AXES AND COORDINATE SYSTEMS Part dimensioning. Millimeters (G71) or inches (G70)

Programming manual
3.3 Part dimensioning. Millimeters (G71) or inches (G70)

The CNC allows you to enter units of measurement with the programming, either in millimeters or inches.
It has a general machine parameter "INCHES" to define the unit of measurement of the CNC.
However, these units of measurement can be changed at any time in the program. Two functions are supplied for this purpose :
· G70. Programming in inches. · G71. Programming in millimeters.
Depending on whether G70 or G71 has been programmed, the CNC assumes the corresponding set of units for all the blocks programmed from that moment on.
The G70 and G71 functions are modal and are incompatible.
The CNC allows you to program figures from 0.00001 to 99999.9999 with or without sign, working in millimeters (G71), called format +/-5.4, or either from 0.00001 to 3937.00787 with or without sign if the programming is done in inches (G70), called format +/-4.5.
However, and to simplify the instructions, we can say that the CNC admits +/- 5.5 format, thereby admitting +/- 5.4 in millimeters and +/- 4.5 in inches.
On power-up, after executing M02, M30 or after EMERGENCY or RESET, the CNC will assume that the system of units of measurement is the one defined by the general machine parameter "INCHES".

CNC 8040
·M· MODEL (SOFT V11.1X)
15

Programming manual
3.4 Absolute/incremental programming (G90, G91)

The CNC allows the programming of the coordinates of one point either with absolute G90 or incremental G91 values.
When working with absolute coordinates (G90), the point coordinates refer to a point of origin of established coordinates, often the part zero (datum).
When working in incremental coordinates (G91), the numerical value programmed corresponds to the movement information for the distance to be traveled from the point where the tool is situated at that time. The sign in front shows the direction of movement.
The G90 and G91 functions are modal and are incompatible.

AXES AND COORDINATE SYSTEMS Absolute/incremental programming (G90, G91)

CNC 8040
·M· MODEL (SOFT V11.1X)
16

Absolute coordinates:

G90

X150.5

X300

Y0 Y200
Y0

; Point P0 ; Point P1 ; Point P2 ; Point P0

Incremental coordinates:

G90

G91

X150.5

Y200

X149.5

X-300

Y-200

; Point P0 ; Point P1 ; Point P2 ; Point P0

On power-up, after executing M02, M30 or after an EMERGENCY or RESET, the CNC will assume G90 or G91 according to the definition by the general machine parameter "ISYSTEM".

3.5 Coordinate programming

Programming manual

The CNC allows the selection of up to 7 of the 9 possible axes X, Y, Z, U, V, W, A, B, C.
Each of these may be linear, linear to position only, normal rotary, rotary to position only or rotary with hirth toothing (positioning in complete degrees), according to the specification in the machine parameter of each "AXISTYPE" axis.
With the aim of always selecting the most suitable coordinate programming system, the CNC has the following types :
· Cartesian coordinates · Polar coordinates · Cylindrical coordinates · Angle and one Cartesian coordinate
3.5.1 Cartesian coordinates
The Cartesian Coordinate System is defined by two axes on the plane, and by three or more axes in space.
The origin of all these, which in the case of the axes X Y Z coincides with the point of intersection, is called Cartesian Origin or Zero Point of the Coordinate System.
The position of the different points of the machine is expressed in terms of the coordinates of the axes, with two, three, four, or five coordinates.
The coordinates of the axes are programmed via the letter of the axis (X, Y, Z, U, V, W, A, B, C, always in this order) followed by the coordinate value.
The values of the coordinates are absolute or incremental, depending on whether it is working in G90 or G91, and its programming format is ±5.5.

AXES AND COORDINATE SYSTEMS Coordinate programming

CNC 8040
·M· MODEL (SOFT V11.1X)
17

Programming manual
3.5.2 Polar coordinates

In the event of the presence of circular elements or angular dimensions, the coordinates of the different points on the plane (2 axes at the same time), it may be easier to express them in polar coordinates.
The reference point is called Polar Origin, and this will be the origin of the Polar Coordinate System.
A point on this system would be defined by :

AXES AND COORDINATE SYSTEMS Coordinate programming

· The RADIUS (R), the distance between the polar origin and the point. · The ANGLE (Q), formed by the abscissa axis and the line which joins the polar
origin with the point. (In degrees)
The values R and Q are absolute or incremental depending on whether you are working with G90 or G91, and their programming format will be R5.5 Q±5.5. The radius value must always be positive.
The values R and Q are incremental and their programming format will be R±5.5 Q±5.5.
The R values may be negative when programming in incremental coordinates; but the resulting value assigned to the radius must always be positive.
When programming a "Q" value greater than 360º, the module will be assumed after dividing it by 360. Thus, Q420 is the same as Q60 and Q-420 is the same as Q-60.

CNC 8040
·M· MODEL (SOFT V11.1X)
18

Programming manual Programming example assuming that the Polar Origin is located at the Coordinate Origin.
3.

AXES AND COORDINATE SYSTEMS Coordinate programming

Absolute coordinates:

G90

G01

R100

G03

Q30

G01

R50

Q30

G03

Q60

G01

R100

Q60

G03

Q90

G01

Q90

; Point P0 ; Point P1, in a straight line (G01) ; Point P2, in an arc (G03) ; Point P3, in a straight line (G01) ; Point P4, in an arc (G03) ; Point P5, in a straight line (G01) ; Point P6, in arc (G03) ; Point P0, in a straight line (G01)

Incremental coordinates:

G90

G91 G01 R100

G03

Q30

G01

R-50

G03

Q30

G01

R50

G03

Q30

G01

R-100

The polar origin, apart from being able to be preset using function G93 (described later) can be modified in the following cases :
· On power-up, after executing M02, M30 EMERGENCY or RESET, the CNC will assume, as the polar origin, the coordinate origin of the work plane defined by the general machine parameter"IPLANE".
· Every time the work plane is changed (G16,G17,G18 or G19), the CNC assumes the coordinate origin of the new work plane selected as the polar origin.
· When executing a circular interpolation (G02 or G03), and if the general machine parameter "PORGMOVE" has a value of 1, the center of the arc will become the new polar origin.

CNC 8040

·M· MODEL (SOFT V11.1X)

AXES AND COORDINATE SYSTEMS Coordinate programming

Programming manual
3.5.3 Cylindrical coordinates
To define a point in space, the system of cylindrical coordinates can be used as well as the Cartesian coordinate system. A point on this system would be defined by :
3.
The projection of this point on the main plane, which should be defined in polar coordinates (R Q). Rest of axes in Cartesian coordinates. Examples:
R30 Q10 Z100 R20 Q45 Z10 V30 A20
CNC 8040
·M· MODEL (SOFT V11.1X)
20

3.5.4 Angle and one Cartesian coordinate

Programming manual

A point on the main plane can be defined via one of its cartesian coordinates, and the exit angle of the previous path.
Example of programming assuming that the main plane is XY:

AXES AND COORDINATE SYSTEMS Coordinate programming

X10

Y20

Q45

X30

Q90

Y60

Q-45

X50

Q-135

Y20

Q180

X10

; Point P0, starting point ; Point P1 ; Point P2 ; Point P3 ; Point P4 ; Point P0

If you wish to represent a point in space, the remaining coordinates can be programmed in Cartesian coordinates.

CNC 8040
·M· MODEL (SOFT V11.1X)
21

Programming manual
3.6 Rotary axes

3.
CNC 8040

AXES AND COORDINATE SYSTEMS Rotary axes

The types of rotary axes available are: Normal rotary axis. Positioning-only axis Rotary HIRTH axis.

Each one of them can be divided into:

Rollover

When it is displayed between 0º and 360º.

Non Rollover When it may be displayed between -99999º and 99999º.

They are all programmed in degrees. Therefore, their readings are not affected by the inch/mm conversion.

Normal rotary axes They can interpolate with linear axes.

Movement: in G00 and G01

Rollover axis programming:

G90

The sign indicates the turning direction and the target position

(between 0 and 359.9999).

G91

The sign indicates the turning direction. If the programmed

movement exceeds 360º, the axis will rotate more than one turn

before positioning at the desired point.

Non-rollover axis programming. In G90 and G91 like a linear axis.

Positioning-only axis

They cannot be interpolated with linear axes.

Movement: Always in G00 and they do not admit tool radius compensation (G41, G42).

Rollover axis programming:

G90

Always positive and in the shortest direction. End coordinate

between 0 & 359.9999

G91

The sign indicates the turning direction. If the programmed

movement exceeds 360º, the axis will rotate more than one turn

before positioning at the desired point.

Non-rollover axis programming. In G90 and G91 like a linear axis.

Rotary Hirth axis

They work like the positioning-only axis except that they do not admit decimal position values (coordinates).

More than one hirth axis can be used, but they can only be moved one at a time.

·M· MODEL (SOFT V11.1X)

3.7 Work zones

Programming manual

The CNC provides four work zones or areas, and also limits the tool movement in each of these.

3.7.1 Definition of the work zones

Within each work zone, the CNC allows you to limit the movement of the tool on each axis, with upper and lower limits being defined in each axis.
G20: Defines the lower limits in the desired zone.
G21: Defines the upper limits in the desired zone.

The format to program these functions is: G20 K X...C±5.5 G21 K X...C±5.5

Where: K X...C

Indicates the work zone you wish to define (1, 2, 3 or 4)
Indicates the coordinates (upper or lower) with which you wish to limit the axes. These coordinates will be programmed with reference to machine zero (home).

It is not necessary to program all the axes, so only defined axes will be limited.

AXES AND COORDINATE SYSTEMS Work zones

G20 K1 X20 Y20 G21 K1 X100 Y50

CNC 8040
·M· MODEL (SOFT V11.1X)
23

Programming manual
3.7.2 Using the work zones
Within each work zone, the CNC allows you to restrict the movement of the tool, either prohibiting its exit from the programmed zone (no exit zone) or its entry into the programmed zone (no entry zone).
3.

AXES AND COORDINATE SYSTEMS Work zones

S= 1 No entry zone

S = 2 No exit zone

The CNC will take the dimensions of the tool into account at all times (tool offset table) to avoid it exceeding the programmed limits.
The presetting of work zones is done via Function G22, the programming format being:
G22 K S
Where:
K Indicates the work zone you wish to define (1, 2, 3 or 4)
S Indicates the enabling/disabling of the work zone.
S=0 disabled. S=1 enabled as a no-entry zone. S=2 enabled as a no-exit zone.
On power-up, the CNC will disable all work zones. However, upper and lower limits for these zones will not undergo any variation, and they can be re-enabled through the G22 function.

CNC 8040
·M· MODEL (SOFT V11.1X)
24

REFERENCE SYSTEMS

4.1 Reference points
A CNC machine needs the following origin and reference points defined : · Machine Reference Zero or home. This is set by the manufacturer as the origin of the system of coordinates of the machine. · Part zero or point of origin of the part. This is the point of origin which is set for programming the measurements of the part. It can be freely selected by the programmer, and its zero machine reference can be set by the zero offset. · Machine Reference point. This is a point on the machine established by the manufacturer around which the synchronization of the system is done. The control positions the axis on this point, instead of moving it as far as the Machine Reference Zero, taking, at this point, the reference coordinates which are defined via the axis machine parameter "REFVALUE".

Machine zero

Part zero

Machine reference point

XMW, YMW, ZMW... Coordinates of part zero

XMR, YMR, ZMR... Coordinates of machine reference point ("REFVALUE")

CNC 8040

·M· MODEL (SOFT V11.1X)

Programming manual
4.2 Machine reference (Home) search (G74)

REFERENCE SYSTEMS Machine reference (Home) search (G74)

The CNC allows you to program the machine reference search in two ways :
· Machine reference (home) search of one or more axes in a particular order.
G74 is programmed followed by the axes in which you want to carry out the reference search. For example: G74 X Z C Y.
The CNC begins the movement of all the selected axes which have a machine reference switch (machine axis parameter "DECINPUT") and in the direction indicated by the axis machine parameter "REFDIREC".
This movement is carried out at the feedrate indicated by the axis machine parameter "REFEED1" for each axis until the home switch is hit.
Next, the home search (marker pulse or home) will be carried out in the programmed order.
This second movement will be carried out one axis at a time, at the feedrate indicated in the axis machine parameter "REFEED2" until the machine reference point is reached (i.e. the marker pulse is found).
· Home search using the associated subroutine.
The G74 function will be programmed alone in the block, and the CNC will automatically execute the subroutine whose number appears in the general machine parameter "REFPSUB". In this subroutine it is possible to program the machine reference searches required, and also in the required order.
In a block in which G74 has been programmed, no other preparatory function may appear.
If the machine reference search is done in JOG mode, the part zero selected is lost. The coordinates of the reference point indicated in the machine axis parameter "REFVALUE" is displayed. In all other cases, the active zero offset will be maintained and the CNC will display the position value with respect to the zero offset (or part zero) active before the home search.
If the G74 command is executed in MDI, the display of coordinates depends on the mode in which it is executed : Jog, Execution, or Simulation.

CNC 8040
·M· MODEL (SOFT V11.1X)
26

Programming manual
4.3 Programming with respect to machine zero (G53)

Function G53 can be added to any block that has path control functions.
It is only used when the programming of block coordinates relating to machine zero is required. These coordinates should be expressed in millimeters or inches, depending on how the general machine parameter "INCHES" is defined.
By programming G53 alone (without motion information) the current active zero offset is canceled regardless of whether it was originated by a G54-G59 or a G92 preset. This origin preset is described next.
Function G53 is not modal, so it should be programmed every time you wish to indicate the coordinates referred to machine zero.
This function temporarily cancels radius and tool length compensation.

REFERENCE SYSTEMS Programming with respect to machine zero (G53)

M Machine zero W Part zero

CNC 8040
·M· MODEL (SOFT V11.1X)
27

Programming manual
4.4 Coordinate preset and zero offsets

The CNC allows you to carry out zero offsets with the aim of using coordinates related to the plane of the part, without having to modify the coordinates of the different points of the part at the time of programming.
The zero offset is defined as the distance between the part zero (point of origin of the part) and the machine zero (point of origin of the machine).

REFERENCE SYSTEMS Coordinate preset and zero offsets

CNC 8040
·M· MODEL (SOFT V11.1X)
28

M Machine zero W Part zero

This zero offset can be carried out in one of two ways : · Via Function G92 (coordinate preset). The CNC accepts the coordinates of the programmed axes after G92 as new axis values. · Via the use of zero offsets (G54,G55,G56,G57,G58, G59); the CNC accepts as a new part zero the point located relative to machine zero at the distance indicated by the selected table(s).
Both functions are modal and incompatible, so if one is selected the other is disabled.
There is, moreover, another zero offset which is governed by the PLC. This offset is always added to the zero offset selected and is used (among other things) to correct deviations produced as a result of expansion, etc.

ORG*(54)

ORG*(55)

ORG*(56)

ORG*(57)

G94

G95

G96

G97

G92 ORG*

PLCOF* Offset of the PLC

ORG*(58) G58
ORG*(59) G59

Zero offset

4.4.1 Coordinate preset and S value limitation (G92)

Programming manual

Via Function G92 one can select any value in the axes of the CNC, in addition to limiting the spindle speed.
· Coordinate preset.
When carrying out a zero offset via Function G92, the CNC assumes the coordinates of the axes programmed after G92 as new axis values.
No other function can be programmed in the block where G92 is defined, the programming format being :
G92 X...C ±5.5

REFERENCE SYSTEMS Coordinate preset and zero offsets

; Positioning in P0 G90 X50 Y40 ; Preset P0 as part zero G92 X0 Y0 ; Programming according to part coordinates G91 X30 X20 Y20 X-20 Y20 X -30 Y -40 · Spindle speed limitation
When executing a "G92 S5.4" type block, the CNC limits the spindle speed from that instant on to the value set by S5.4. If later on, a block is to be executed at a greater "S", the CNC will execute that block at the maximum "S" set with function G92S. Neither is it possible to exceed this maximum value from the keyboard on the front panel.
CNC 8040
·M· MODEL (SOFT V11.1X)
29

Programming manual
4.4.2 Zero offsets (G54..G59)

REFERENCE SYSTEMS Coordinate preset and zero offsets

The CNC has a table of zero offsets, in which several zero offsets can be selected. The aim is to generate certain part zeros independently of the part zero active at the time.

Access to the table can be obtained from the front panel of the CNC (as explained in the Operating Manual), or via the program using high-level language commands.

There are two kinds of zero offsets :
· Absolute zero offsets (G54,G55,G56 & G57), which must be referred to machine zero.
· Incremental zero offsets (G58,G59).

Functions G54, G55, G56, G57, G58 & G59 must be programmed alone in the block, and work in the following way:

When one of the G54, G55, G56, G57 functions is executed, the CNC applies the zero offset programmed with respect to machine zero, canceling the possible active zero offsets.

If one of the incremental offsets G58 or G59 is executed, the CNC adds its values to the absolute zero offset active at the time. Previously canceling the additive offset which might be active.

You can see (in the following example) the zero offsets which are applied when the program is executed.

G54

Applies zero offsets G54

==> G54

G58

Applies zero offsets G58

==> G54+G58

G59

Cancels G58 and adds G59

==> G54+G59

G55

Cancels whatever and applies G55

==> G55

Once a Zero Offset has been selected, it will remain active until another one is selected or until a home search is carried out (G74) in JOG mode. This zero offset will remain active even after powering the CNC off and back on.

This kind of zero offsets established by program is very useful for repeated machining operations at different machine positions.

CNC 8040
·M· MODEL (SOFT V11.1X)
30

Programming manual

Example: The zero offset table is initialized with the following values:

G54:

X200

Y100

G55:

X160

Y 60

G56:

X170

Y110

G58:

X-40

Y-40

G59:

X-30

Y10

REFERENCE SYSTEMS Coordinate preset and zero offsets

Using absolute zero offsets:

G54

; Applies G54 offset

Profile execution

; Executes profile A1

G55

; Applies G55 offset

Profile execution

; Executes profile A2

G56

; Applies G56 offset

Profile execution

; Executes profile A3

Using incremental zero offsets:

G54

; Applies G54 offset

Profile execution

; Executes profile A1

G58

; Applies offsets G54+G58

Profile execution

; Executes profile A2

G59

; Applies offsets G54+G59

Profile execution

; Executes profile A3

CNC 8040
·M· MODEL (SOFT V11.1X)
31

Programming manual
4.5 Polar origin preset (G93)

Function G93 allows you to preset any point from the work plane as a new origin of polar coordinates.
This function must be programmed alone in the block, its programming format being : G93 I±5.5 J±5.5
Parameters I & J respectively define the abscissa and ordinate axes, of the new origin of polar coordinates referred to part zero.
Example, assuming that the tool is at X0 Y0

REFERENCE SYSTEMS Polar origin preset (G93)

CNC 8040
·M· MODEL (SOFT V11.1X)
32

G93

I35 J30 ; Preset P3 as polar origin.

G90 G01 R25 Q0 ; Point P1, in a straight line (G01).

G03

Q90 ; Point P2, in an arc (G03).

G01 X0 Y0 ; Point P0, in a straight line (G01)

If G93 is only programmed in a block, the point where the machine is at that moment becomes the polar origin.
On power-up; or after executing M02, M30; or after an EMERGENCY or RESET; the CNC assumes the currently active part zero as polar origin.
When selecting a new work plane (G16, G17, G18, G19), the CNC assumes as polar origin the part zero of that plane.

The CNC does not modify the polar origin when defining a new part zero; but it modifies the values of the variables: "PORGF" y "PORGS".

If, while selecting the general machine parameter "PORGMOVE" a circular interpolation is programmed (G02 or G03), the CNC assumes the center of the arc as the new polar origin.

ISO CODE PROGRAMMING

A block programmed in ISO language can consist of: · Preparatory (G) functions · Axis coordinates (X...C) · Feedrate (F) · Spindle speed (S) · Tool number (T) · Tool offset number (D) · Auxiliary functions (M)
This order should be maintained within each block, although it is not necessary for every block to contain the information.
The CNC allows you to program figures from 0.00001 to 99999.9999 with or without sign, working in millimeters (G71), called format +/-5.4, or either from 0.00001 to 3937.00787 with or without sign if the programming is done in inches (G70), called format +/-4.5.
However, and to simplify the instructions, we can say that the CNC admits +/- 5.5 format, thereby admitting +/- 5.4 in millimeters and +/- 4.5 in inches.
Any function with parameters can also be programmed in a block, apart from the number of the label or block. Thus, when the block is executed the CNC substitutes the arithmetic parameter for its value at that time.

CNC 8040
·M· MODEL (SOFT V11.1X)
33

Programming manual
5.1 Preparatory functions

5.
CNC 8040
·M· MODEL (SOFT V11.1X)
34

ISO CODE PROGRAMMING Preparatory functions

Preparatory functions are programmed using the letter G followed by up to 3 digits (G0 - G319).
They are always programmed at the beginning of the body of the block and are useful in determining the geometry and working condition of the CNC.
Table of G functions used in the CNC.

Function M D V

Meaning

G00

* ? * Rapid traverse

G01

* ? * Linear interpolation

G02

* Clockwise circular (helical) interpolation

G03

* Counterclockwise circular (helical) interpolation

G04

Dwell/interruption of block preparation

G05

* ? * Round corner

G06

* Arc center in absolute coordinates

G07

Square corner

G08

* Arc tangent to previous path.

G09

* Arc defined by three points

G10

Mirror image cancellation

G11

* Mirror image on X axis

G12

* Mirror image on Y axis

G13

* Mirror image on Z axis

G14

* Mirror image in the programmed directions

G15

* Longitudinal axis selection

G16

* Main plane selection by two addresses and longitudinal axis

G17

* ? * Main plane X-Y and longitudinal Z

G18

* ? * Main plane Z-X and longitudinal Y

G19

* Main plane Y-Z and longitudinal X

G20

Definition of lower work zone limits

G21

Definition of upper work zone limits.

G22

* Enable/disable work zones.

G28

* Second spindle selection

G29

Main spindle selection

G28 - G29

* Axis toggle

G30

* Spindle synchronization (offset)

G32

* Feedrate "F" as an inverted function of time.

G33

* Electronic threading

G34

Variable-pitch threading

G36

* Controlled corner rounding

G37

* Tangential entry

G38

* Tangential exit

G39

* Chamfer

G40

Cancellation of tool radius compensation

G41

* Left-hand tool radius compensation

G41 N *

* Collision detection

G42

* Right-hand tool radius compensation

G42 N *

* Collision detection

G43

* ? * Tool length compensation

G44

Cancellation of tool length compensation

G45

* Tangential control (G45)

G50

* Controlled corner rounding

G51

* Look-Ahead

G52

* Movement until making contact

G53

* Programming with respect to machine reference zero (home)

G54

* Absolute zero offset 1

G55

* Absolute zero offset 2

G56

* Absolute zero offset 3

G57

* Absolute zero offset 4

G58

* Additive zero offset 1

Section
6.1 6.2 6.3 / 6.7 6.3 / 6.7 7.1 / 7.2 7.3.2 6.4 7.3.1 6.5 6.6 7.5 7.5 7.5 7.5 7.5 8.2 3.2 3.2 3.2 3.2 3.7.1 3.7.1 3.7.2 5.4 5.4 7.9 5.5 6.15 6.12 6.13 6.10 6.8 6.9 6.11 8.1 8.1 8.3 8.1 8.3 8.2 8.2 6.16 7.3.3 7.4 6.14 4.3 4.4.2 4.4.2 4.4.2 4.4.2 4.4.2

Programming manual

Function M D V

Meaning

Section

G59 G60 G61 G62 G63 G64 G65 G66 G67 G68 G69 G70 G71 G72 G73 G74 G75 G76 G77 G77S G78 G78S G79 G80 G81 G82 G83 G84 G85 G86 G87 G88 G89 G90 G91 G92 G93 G94 G95 G96 G97 G98 G99
G145

* Additive zero offset 2

4.4.2

* Multiple machining in a straight line

10.1

* Multiple machining in a rectangular pattern

10.2

* Grid pattern canned cycle

10.3

* Multiple machining in a circular pattern

10.4

* Multiple machining in an arc

10.5

* Machining programmed with an arc-chord

10.6

* Irregular pocket canned cycle

11.1 / 11.2

* Irregular pocket roughing

11.1.2

* Irregular pocket finishing

11.1.3

* Drilling canned cycle with variable peck

9.6

* ? * Inch programming

3.3

Programming in millimeters

3.3

* General and specific scaling factor

7.6

* Pattern rotation

7.7

* Home search

4.2

* Probing move until touching

12.1

* Probing move while touching

12.1

* Axis coupling (slaving)

7.8.1

* Spindle synchronization

5.5

Cancellation of axis coupling (slaving)

7.8.2

Cancellation of spindle synchronization

5.5

Canned cycle parameter modification

9.2.1

Canned cycle cancellation

9.3

* Drilling canned cycle

9.7

* Drilling canned cycle with dwell

9.8

* Deep-hole drilling canned cycle with constant peck

9.9

* Tapping canned cycle

9.10

* Reaming canned cycle

9.11

* Boring canned cycle with withdrawal in G00

9.12

* Rectangular pocket canned cycle.

9.13

* Circular pocket canned cycle

9.14

* Boring canned cycle with withdrawal in G01

9.15

Absolute programming

3.4

* ? * Incremental programming

3.4

Coordinate preset / spindle speed limit

4.4.1

Polar origin preset

4.5

Feedrate in millimeters (inches) per minute

5.2.1

* ? * Feedrate in millimeters (inches) per revolution.

5.2.2

* Constant cutting point speed

5.2.3

Constant tool center speed

5.2.4

Withdrawal to the starting plane at the end of the canned cycle

9.5

* Withdrawal to the reference plane at the end of the canned

9.5

cycle

* Temporary cancellation of tangential control

6.17

M means modal, i.e. the G function, once programmed, remains active while another incompatible G function is not programmed or until an M02, M30, EMERGENCY or RESET is executed or the CNC is turned off and back on.

D means BY DEFAULT, i.e. they will be assumed by the CNC when it is powered on, after executing M02, M30 or after EMERGENCY or RESET.

In those cases indicated by ? , it should be understood that the DEFAULT of these G functions depends on the setting of the general machine parameters of the CNC.

V means that the G code is displayed next to the current machining conditions in the execution and simulation modes.

ISO CODE PROGRAMMING Preparatory functions

5.
CNC 8040
·M· MODEL (SOFT V11.1X)

Programming manual
5.2 Feedrate F

ISO CODE PROGRAMMING Feedrate F

The machining feedrate can be selected from the program. It remains active until another feedrate is programmed. It is represented by the letter F and Depending on whether it is working in G94 or G95, it is programmed in mm/minute (inches/minute) or in mm/revolution (inches/revolution).
Its programming format is 5.5; in other words, 5.4 when programmed in mm and 4.5 when programmed in inches.
The maximum operating feedrate of the machine, limited on each axis by the axis machine parameter "MAXFEED", may be programmed via code F0, or by giving F the corresponding value.
The programmed feedrate F is effective working in linear (G01) or circular (G02, G03) interpolation. If function F is not programmed, the CNC assumes the feedrate to be F0. When working in rapid travel (G00), the machine will move at the rapid feedrate indicated by the axis machine parameter "G00FEED", apart from the F programmed.
The programmed feedrate F may be varied between 0% and 255% via the PLC, or by DNC, or between 0% and 120% via the switch located on the Operator Panel of the CNC.
The CNC, however, is equipped with the general machine parameter "MAXFOVR" to limit maximum feedrate variation.
If you are working in rapid travel (G00), rapid feedrate will be fixed at 100%, alternatively it can be varied between 0% and 100%, depending on how the machine parameter "RAPIDOVR" is set.
When functions G33 (electronic threading), G34 (variable-pitch threading) or G84 (tapping canned cycle) are executed the feedrate cannot be modified; it works at 100% of programmed F.

CNC 8040
·M· MODEL (SOFT V11.1X)
36

5.2.1 Feedrate in mm/min or inches/min (G94)

Programming manual

From the moment the code G94 is programmed, the control takes that the feedrates programmed through F5.5 are in mm/min or inches/mm.
If the move corresponds to a rotary axis, the CNC will assume the feedrate to be programmed in degrees/min.
If an interpolation is made between a rotary and a linear axis, the programmed feedrate is taken in mm/min or inches/min, and the movement of the rotary axis (programmed in degrees) will be considered programmed in millimeters or inches.
The relationship between the feedrate of the axis component and the programmed feedrate "F" is the same as that between the movement of the axis and the resulting programmed movement.

ISO CODE PROGRAMMING Feedrate F

Feedrate component =

Feedrate F x Movement of axis Resulting programmed movement

Example:
On a machine which has linear X and Y axes and rotary C axis, all located at point X0 Y0 C0, the following movement is programmed :
G1 G90 X100 Y20 C270 F10000
You get:

Fx = -----------------------F------------x------------------------ = ----------1---0---0---0---0----×-----1---0---0----------- = 3464, 7946 (x)2 + (y)2 + (c)2 1002 + 202 + 2702

Fy = -----------------------F------------y------------------------ = -----------1---0---0---0---0-----×-----2---0------------ = 692, 9589 (x)2 + (y)2 + (c)2 1002 + 202 + 2702

Fc = -----------------------F------------c------------------------ = ----------1---0---0---0---0----×-----2---7---0----------- = 9354, 9455 (x)2 + (y)2 + (c)2 1002 + 202 + 2702

Function G94 is modal i.e. once programmed it stays active until G95 is programmed.
On power-up, after executing M02, M30 or following EMERGENCY or RESET, the CNC assumes function G94 or G95 according to how the general machine parameter "IFEED" is set.

CNC 8040
·M· MODEL (SOFT V11.1X)
37

Programming manual
5.2.2 Feedrate in mm/rev.or inches/rev (G95)

From the moment when the code G95 is programmed, the control assumes that the feedrates programmed through F5.5 are in mm/rev or inches/mm.
This function does not affect the rapid moves (G00) which will be made in mm/min or inch/min. By the same token, it will not be applied to moves made in the JOG mode, during tool inspection, etc.
Function G95 is modal i.e. once programmed it stays active until G94 is programmed.
On power-up, after executing M02, M30 or following EMERGENCY or RESET, the CNC assumes function G94 or G95 according to how the general machine parameter "IFEED" is set.

ISO CODE PROGRAMMING Feedrate F

5.2.3 Constant surface speed (G96)
When G96 is programmed the CNC takes the F5.5 feedrate as corresponding to the cutting point of the tool on the part.
By using this function, the finished surface is uniform in curved sections.
In this manner (working in function G96) the speed of the center of the tool in the inside or outside curved sections will change in order to keep the cutting point constant.
Function G96 is modal i.e. once programmed it stays active until G97 is programmed.
On power-up, after executing M02, M30 or following EMERGENCY or RESET, the CNC assumes function G97.

5.2.4 Constant tool center speed (G97)
When G97 is programmed the CNC takes the programmed F5.5 feedrate as corresponding to the feedrate of the center of the tool.
In this manner (working in function G97) the speed of the cutting point on the inside or outside curved sections is reduced, keeping the speed of the center of the tool constant.
Function G97 is modal i.e. once programmed it stays active until G96 is programmed.
On power-up, after executing M02, M30 or following EMERGENCY or RESET, the CNC assumes function G97.

CNC 8040
·M· MODEL (SOFT V11.1X)
38

5.3 Spindle speed (S)

Programming manual

The turning speed of the spindle is programmed directly in rpm via code S5.4.
The maximum value is limited by spindle machine parameters "MAXGEAR1", MAXGEAR2, MAXGEAR 3 and MAXGEAR4", in each case depending on the spindle range selected.
It is also possible to limit this maximum value from the program by using function G92 S5.4.
The programmed turning speed S may be varied from the PLC, DNC, or by the SPINDLE keys "+" and "-" on the Operator Panel of the CNC.
This speed variation is made between the maximum and minimum values established by spindle machine parameters "MINSOVR" and "MAXSOVR".
The incremental pitch associated with the SPINDLE keys "+" and "-" on the CNC Operator Panel in order to vary the programmed S value is fixed by the spindle machine parameter "SOVRSTEP".
When functions G33 (electronic threading), G34 (variable-pitch threading) or G84 (tapping canned cycle) are executed the programmed speed cannot be modified; it works at 100% of programmed S.

ISO CODE PROGRAMMING Spindle speed (S)

CNC 8040
·M· MODEL (SOFT V11.1X)
39

Programming manual
5.4 Spindle selection (G28, G29)

ISO CODE PROGRAMMING Spindle selection (G28, G29)

This CNC can govern two spindles: the main one and the second one. They both can be operative simultaneously, but only one can be controlled at a time.
This selection is made using functions G28 and G29. G28: Second spindle selection. G29: Main spindle selection.
Once the desired spindle has been selected, it can be acted upon from the keyboard or by means of the following functions:
M3, M4, M5, M19 S**** G33, G34, G94, G95, G96, G97
Both spindles can work in open and closed loop.
Functions G28 and G29 are modal and incompatible with each other.
Function G28 and G29 must be programmed alone in the block.
No more information can be programmed in that block. On power-up, after executing and M02, M30 or after an EMERGENCY or RESET, the CNC assumes function G29 (selects the main spindle).
Operating example for when 2 spindles are used.
On power-up, the CNC assumes function G29 selecting the main spindle. All the keyboard actions and by spindle related functions affect the main spindle. Example: S1000 M3 Main spindle clockwise at 1000 rpm.
To select the second spindle, execute function G28. From then on, All the keyboard actions and spindle related functions affect the second spindle. The main spindle remains in its previous status. Example: S1500 M4 Second spindle turns counterclockwise at 1500 rpm. The main spindle keeps turning at 1000 rpm.
To select the main spindle again, execute function G29. From then on, all the keyboard actions and spindle related functions affect the main spindle. The second spindle stays in its previous status. Example: S2000 The main spindle keeps turning clockwise but at 2000 rpm. The second spindle keeps turning at 1500 rpm.

CNC 8040

·M· MODEL (SOFT V11.1X)

5.5 Synchronized spindles (G30, G77S, G78S)

Programming manual

With function G77S, two spindles (main and secondary) may be synchronized in speed; this synchronism may be cancelled with function G78S. Always program G77S and G78S because functions G77, G78 to slave and unslave the axes.
When the spindles are synchronized in speed, the second one turns at the same speed as the main spindle.
Function G77S may be executed at any time, open loop (M3, M4) or closed loop (M19), the spindles may even have different ranges (gears).
General output "SYNSPEED (M5560)" will be high while the spindle are in synch (same speed).
When this synchronism is cancelled (G78S), the second spindle recovers its previous speed and status (M3, M4, M5, M19) and the main spindle stays in the current status.
If while in synchronism, an S is programmed greater than the maximum allowed, the CNC applies the maximum value while they are synchronized. When canceling this synchronism, the limit is no longer applied and the main spindle assumes the programmed speed.
While the spindles are synchronized in speed, function G77S active, with G30 they may also be synchronized in position and set an angular offset between them so the second spindle follows the main spindle at this set offset distance.
Programming format: G30 D ±359.9999 (offset in degrees)
For example, with G30 D90 the second spindle will turn 90º behind the main spindle.
Considerations
Before activating the synchronism, both spindles must be homed (referenced).
To synchronized the spindles in position (G30) they must be synchronized in speed already (G77S).
To synchronize two spindles, the SERVOSON and SERVOSO2 signals must be activated already. While the spindles are synchronized, only the signals of the main spindle will be attended to PLCCNTL, SPDLINH, SPDLREV, etc. On the other hand, when making a thread, only the feedback and reference pulses of the main spindle will be taken into account.
While the spindle synchronism is active, it is possible to: · Execute functions G94, G95, G96, G97, M3, M4, M5, M19 S*** · Change the spindle speed via DNC, PLC or CNC (S). · Change the spindle speed override via DNC, PLC, CNC or keyboard. · Change the spindle speed limit via DNC, PLC or CNC (G92 S)
But the following cannot be done: · Toggle the spindles: G28, G29. · Change gears: M41, M42, M43, M44.

ISO CODE PROGRAMMING Synchronized spindles (G30, G77S, G78S)

CNC 8040

·M· MODEL (SOFT V11.1X)

Programming manual
5.6 Tool number (T) and tool offset (D)
With the "T" function, it is possible to select the tool and with the "D" function it is possible to select the offset associated with it. When defining both parameters, the programming order is T D. For example: T6 D17

Magazine?
Yes Selects the tool

NO If the machine has a tool magazine, the CNC looks up the "Tool magazine table" to know the position occupied by the selected tool and the desired one.

ISO CODE PROGRAMMING Tool number (T) and tool offset (D)

CNC 8040

Yes D?

NO
The CNC takes the D associated with the T in
the tool table

If the "D" function has not be defined, it looks up the "Tool table" to know the "D" offset associated with it.

The CNC takes the dimensions defined for the D in the tool offset
table

It looks up the "tool offset table" and assumes the tool dimensions corresponding to the "D" offset.

To access, check and define these tables, refer to the operating manual.

How to use the T and D functions
· The "T" and "D" functions may be programmed alone or together as shown in the following example:

T5 D18 Selects tool 5 and assumes the dimensions of tool offset 18

D22

Tool 5 stays selected and it assumes the dimensions of tool offset 22.

Selects tool 3 and assumes the dimensions of the offset associated

with that tool.

· When having a tool magazine where the same position is occupied by more than one tool, do the following:
Use the "T" function to refer to the magazine position and the "D" function to the dimensions of the tool located in that position.
Thus, for example, programming T5 D23 means selecting the turret position 5 and assuming the geometry and dimensions of tool offset 23.

·M· MODEL (SOFT V11.1X)

Programming manual

Tool length and radius compensation.

The CNC looks up the "tool offset table" and assumes the tool dimensions corresponding to the active "D" offset.
Length compensation is applied at all times, whereas radius compensation must be selected by the operator by means of functions G40, G41, G42.

Length compensation is applied at all times, whereas tool length compensation must be selected by the operator by means of functions G43, G44.
If there is no tool selected or D0 is defined, neither tool length nor radius compensation is applied.
For further information, refer to chapter 8 "tool compensation" in this manual..

ISO CODE PROGRAMMING Tool number (T) and tool offset (D)

CNC 8040
·M· MODEL (SOFT V11.1X)
43

Programming manual
5.7 Auxiliary function (M)

ISO CODE PROGRAMMING Auxiliary function (M)

The miscellaneous functions are programmed by means of the M4 Code, it being possible to program up to 7 functions in the same block.
When more than one function has been programmed in one block, the CNC executes these correlatively to the order in which they have been programmed.
The CNC is provided with an M functions table with "NMISCFUN" (general machine parameter) components, specifying for each element:
· The number (0-9999) of the defined miscellaneous M function. · The number of the subroutine which is required to associate to this miscellaneous
function. · An indicator which determines if the M function is executed before or after the
movement block in which it is programmed. · An indicator which determines if the execution of the M function interrupts block
preparation or not. · An indicator which determines if the M function is executed or not, after the
execution of the associated subroutine. · An indicator which determines if the CNC must wait for the signal AUX END or
not (Executed M signal, coming from the PLC), to continue the execution of the program.
If, when executing the M miscellaneous function, this is not defined in the M functions table, the programmed function will be executed at the beginning of the block and the CNC will wait for the AUX END to continue the execution of the program.
Some of the miscellaneous functions are assigned an internal meaning in the CNC.
If, while executing the associated subroutine of an "M" miscellaneous function, there is a block containing the same "M", this will be executed but not the associated subroutine.

All the miscellaneous "M" functions which have an associated subroutine must be programmed alone in a block.

In the case of functions M41 through M44 with associated subroutine, the S that generates the gear change must be programmed alone in the block. Otherwise, the CNC will display error 1031.

CNC 8040
·M· MODEL (SOFT V11.1X)
44

5.7.1 M00. Program stop

Programming manual

When the CNC reads code M00 in a block, it interrupts the program. To start up again, press CYCLE START.
We recommend that you set this function in the table of M functions, in such a way that it is executed at the end of the block in which it is programmed.

5.7.2 M01. Conditional program stop
This is identical to M00, except that the CNC only takes notice of it if the signal M01 STOP from the PLC is active (high logic level).

ISO CODE PROGRAMMING Auxiliary function (M)

5.7.3 M02. End of program
This code indicates the end of program and carries out a "General Reset" function of the CNC (returning it to original state). It also carries out the M05 function.
We recommend that you set this function in the table of M functions, in such a way that it is executed at the end of the block in which it is programmed.

5.7.4 M30. End of program with return to the first block
Identical to M02 except that the CNC returns to the first block of the program.

5.7.5 M03 Clockwise spindle rotation
This code represents clockwise spindle start. As explained in the corresponding section, the CNC automatically executes this code in the machining canned cycles.
It is recommended to set this function in the table of M functions, so that it is executed at the beginning of the block in which it is programmed.

5.7.6 M04. Counterclockwise spindle rotation
This code represents counterclockwise spindle start. We recommend that you set this function in the table of M functions, so that it is executed at the beginning of the block in which it is programmed.

5.7.7 M05. Spindle stop
We recommend that you set this function in the table of M functions, in such a way that it is executed at the end of the block in which it is programmed.

CNC 8040

·M· MODEL (SOFT V11.1X)

Programming manual
5.7.8 M06. Tool change code

If the general machine parameter "TOFFM06" (indicating that it is a machining center) is active, the CNC sends instructions to the tool changer and updates the table corresponding to the tool magazine. It is recommended to set this function in the table of M functions, so that the subroutine corresponding to the tool changer installed in the machine is executed.
5.7.9 M19. Spindle orientation

ISO CODE PROGRAMMING Auxiliary function (M)

CNC 8040

With this CNC it is possible to work with the spindle in open loop (M3, M4) and with the spindle in closed loop (M19).
In order to work in closed loop, it is necessary to have a rotary encoder installed on the spindle of the machine.
To switch from open loop to closed loop, execute function M19 or M19 S±5.5. The CNC will act as follows:
· If the spindle has a home switch, the CNC modifies the spindle speed until it reaches the one set by spindle machine parameter "REFEED1". It then searches for actual marker pulse (Io) of the spindle encoder at the turning speed set by spindle machine parameter REFEED2. And, finally, it positions the spindle at the programmed S±5.5 point.
· If the spindle does not have a home switch, it searches the encoder marker pulse at the turning speed set by spindle machine parameter REFEED2. And, then, it positions the spindle at the programmed S±5.5 point.
If only M19 is executed, the spindle is oriented to position "S0" after having "found" the home switch.
To, now, orient the spindle to another position, program M19 S±5.5, the CNC will not perform the home search since it is already in closed loop and it will orient the spindle to the indicated position. (S±5.5).
The S±5.5 code indicates the spindle position, in degrees, from the spindle reference point (marker pulse).
The sign indicates the counting direction and the 5.5 value is always considered to be absolute coordinates regardless of the type of units currently selected.
Example: S1000 M3 Spindle in open loop. M19 S100 The spindle switches to closed loop. Home search and positioning (orientation) at 100º. M19 S -30 The spindle orients to -30º, passing through 0º. M19 S400 The spindle turns a whole revolution and positions at 40º.

·M· MODEL (SOFT V11.1X)

5.7.10 M41, M42, M43, M44. Spindle gear change

Programming manual

The CNC offers 4 spindle speed ranges M41, M42, M43 and M44 with maximum speed limits set by the spindle machine parameters "MAXGEAR1", MAXGEAR2", "MAXGEAR3" and "MAXGEAR4".
If machine parameter "AUTOGEAR" is set so the CNC executes the range change automatically, M41 thru M44 will be sent out automatically by the CNC without having to be programmed.
If this machine parameter is set for non-automatic gear change, M41 thru M44 will have to be programmed every time a gear change is required. Bear in mind that the maximum voltage value assigned to machine parameter "MAXVOLT" corresponds to the maximum speed indicated for each one of the speed ranges (machine parameters "MAXGEAR1" thru "MAXGEAR4").
Regardless of whether the gear change is automatic or not, functions M41 through M44 may have an associated subroutine. If the function M41 through M44 is programmed and then an S corresponding to that gear, it does not generate the automatic gear change and it does not execute the associated subroutine.

ISO CODE PROGRAMMING Auxiliary function (M)

5.7.11 M45. Auxiliary spindle / Live tool
In order to use this miscellaneous function, it is necessary to set one of the axes of the machine as auxiliary spindle or live tool (general machine parameter P0 thru P7).
To use the auxiliary spindle or live tool, execute the command: M45 S±5.5 where S indicates the turning speed in rpm and the sign indicates the turning direction.
The CNC will output the analog voltage corresponding to the selected speed according to the value assigned to the machine parameter "MAXSPEED" for the auxiliary spindle.
To stop the auxiliary spindle, program M45 or M45 S0.
Whenever the auxiliary spindle or live tool is active, the CNC will let the PLC know by activating the general logic output "DM45" (M5548).
Also, it is possible to set the machine parameter for the auxiliary spindle "SPDLOVR" so the Override keys of the front panel can modify the currently active turning speed of the auxiliary spindle.

CNC 8040
·M· MODEL (SOFT V11.1X)
47

ISO CODE PROGRAMMING Auxiliary function (M)

Programming manual
5.
CNC 8040
·M· MODEL (SOFT V11.1X)
48

PATH CONTROL

6.1

The CNC allows you to program movements on one axis only or several at the same time. Only those axes which intervene in the required movement are programmed. The programming order of the axes is as follows : X, Y, Z, U, V, W, A, B, C
Rapid traverse (G00)

The movements programmed after G00 are executed at the rapid feedrate indicated in the axis machine parameter "G00FEED".
Independently of the number of axis which move, the resulting path is always a straight line between the starting point and the final point.

X100 Y100; Starting point G00 G90 X400 Y300; Programmed path
It is possible, via the general machine parameter "RAPIDOVR", to establish if the feedrate override % switch (when working in G00) operates from 0% to 100%, or whether it stays constant at 100%.
When G00 is programmed, the last "F" programmed is not cancelled i.e. when G01, G02 or G03 are programmed again "F" is recovered.
G00 is modal and incompatible with G01, G02, G03, G33 G34 and G75. Function G00 can be programmed as G or G0.
On power-up, after executing M02, M30 or after EMERGENCY or RESET, the CNC assumes code G00 or G01, depending on how general machine parameter "IMOVE" has been set.

CNC 8040

·M· MODEL (SOFT V11.1X)

Programming manual
6.2 Linear interpolation (G01)

The movements programmed after G01 are executed according to a straight line and at the programmed feedrate "F".
When two or three axes move simultaneously the resulting path is a straight line between the starting point and the final point.
The machine moves according to this path to the programmed feedrate "F". The CNC calculates the feedrates of each axis so that the resulting path is the "F" value programmed.

PATH CONTROL Linear interpolation (G01)

G01 G90 X650 Y400 F150 The programmed feedrate "F" may vary between 0% and 120% via the switch located on the Control Panel of the CNC, or by selecting between 0% and 255% from the PLC, or via the DNC or the program. The CNC, however, is equipped with the general machine parameter "MAXFOVR" to limit maximum feedrate variation. With this CNC, it is possible to program a positioning-only axis in a linear interpolation block. The CNC will calculate the feedrate for this positioning-only axis so it reaches the target coordinate at the same time as the interpolating axes. Function G01 is modal and incompatible with G00, G02, G03, G33 and G34. Function G01 can be programmed as G1. On power-up, after executing M02, M30 or after EMERGENCY or RESET, the CNC assumes code G00 or G01, depending on how general machine parameter "IMOVE" has been set.
CNC 8040
·M· MODEL (SOFT V11.1X)
50

6.3 Circular interpolation (G02, G03)

Programming manual

There are two ways of carrying out circular interpolation: G02: Clockwise circular interpolation G03: Counterclockwise circular interpolation
Movements programmed after G02 and G03 are executed in the form of a circular path and at the programmed feedrate "F".
Clockwise (G02) and counterclockwise (G03) definitions are established according to the system of coordinates shown below:

PATH CONTROL Circular interpolation (G02, G03)

This system of coordinates refers to the movement of the tool on the part. Circular interpolation can only be executed on a plane. The form of definition of circular interpolation is as follows :
Cartesian coordinates
The coordinates of the endpoint of the arc and the position of the center with respect to the starting point are defined according to the axes of the work plane. The center coordinates are defined in radius by the letters I, J, or K, each one of these being associated to the axes as follows: When not defining the center coordinates, the CNC assumes that their value is zero.

Axes X, U, A Axes Y, V, B Axes Z, W, C

==> I ==> J ==> K

Programming format:

Plane XY: Plane ZX: Plane YZ:

G02(G03) G02(G03) G02(G03)

X±5.5 X±5.5 Y±5.5

Y±5.5 Z±5.5 Z±5.5

I±5.5 I±5.5 J±5.5

J±5.5 K±5.5 K±5.5

CNC 8040
·M· MODEL (SOFT V11.1X)

PATH CONTROL Circular interpolation (G02, G03)

Programming manual
6.

The programming order of the axes is always maintained regardless of the plane selected,, as are the respective center coordinates.
Plane AY: G02(G03) Y±5.5 A±5.5 J±5.5 I±5.5 Plane XU: G02(G03) X±5.5 U±5.5 I±5.5 I±5.5

Polar coordinates

It is necessary to define the angle to be traveled Q and the distance from the starting point to the center (optional), according to the axes of the work plane.

The center coordinates are defined by the letters I, J, or K, each one of these being associated to the axes as follows:

Axes X, U, A Axes Y, V, B Axes Z, W, C

==> I ==> J ==> K

If the center of the arc is not defined, the CNC will assume that it coincides with the current polar origin.

Programming format:

Plane XY: Plane ZX: Plane YZ:

G02(G03) G02(G03) G02(G03)

Q±5.5 Q±5.5 Q±5.5

I±5.5 I±5.5 J±5.5

J±5.5 K±5.5 K±5.5

Cartesian coordinates with radius programming

The coordinates of the endpoint of the arc and radius R are defined.

Programming format:

Plane XY: Plane ZX: Plane YZ:

G02(G03) G02(G03) G02(G03)

X±5.5 X±5.5 Y±5.5

Y±5.5 Z±5.5 Z±5.5

R±5.5 R±5.5 R±5.5

If a complete circle is programmed, with radius programming, the CNC will show the corresponding error, as infinite solutions exist.
If an arc is less than 180o, the radius is programmed with a plus sign, and a minus sign if it is more than 180o.

CNC 8040

·M· MODEL (SOFT V11.1X)

Programming manual

PATH CONTROL Circular interpolation (G02, G03)

If P0 is the starting point and P1 the endpoint, there are 4 arcs which have the same value passing through both points.

Depending on the circular interpolation G02 or G03, and on the radius sign, the relevant arc is defined. Thus the programming format of the sample arcs is as follows:

Arc 1

G02 X.. Y.. R- ..

Arc 2

G02 X.. Y.. R+..

Arc 3

G03 X.. Y.. R+..

Arc 4

G03 X.. Y.. R- ..

Execution of the circular interpolation
The CNC calculates, depending on the programmed arc, the radii of the starting point and endpoint. Although both of them should be "exactly" the same, general parameter "CIRINERR" allows a certain calculation tolerance by establishing the maximum difference between these two radii. When exceeding this value, the CNC will issue the corresponding error message.
The programmed feedrate "F" may vary between 0% and 120% via the switch located on the Control Panel of the CNC, or by selecting between 0% and 255% from the PLC, or via the DNC or the program.
The CNC, however, is equipped with the general machine parameter "MAXFOVR" to limit maximum feedrate variation.
If the general machine parameter "PORGMOVE" has been selected and a circular interpolation (G02 or G03) is programmed, the CNC assumes the center of the arc to be a new polar origin.
Functions G02 and G03 are modal and incompatible both among themselves and with G00, G01, G33 and G34. Functions G02 and G03 can be programmed as G2 and G3.
Also, function G74 (home search) and G75 (probing) cancel the G02 and G03 functions.
On power-up, after executing M02, M30 or after EMERGENCY or RESET, the CNC assumes code G00 or G01, depending on how general machine parameter "IMOVE" has been set.

CNC 8040
·M· MODEL (SOFT V11.1X)

Programming manual

Programming examples

PATH CONTROL Circular interpolation (G02, G03)

Various programming modes are analyzed below, point X60 Y40 being the starting point.
Cartesian coordinates: G90 G17 G03 X110 Y90 I0 J50 X160 Y40 I50 J0
Polar coordinates: G90 G17 G03 Q0 I0 J50 Q-90 I50 J0
or: G93 I60 J90 ; defines polar center G03 Q0 G93 I160 J90 ; defines new polar center Q-90
Cartesian coordinates with radius programming: G90 G17 G03 X110 Y90 R50 X160 Y40 R50

CNC 8040
·M· MODEL (SOFT V11.1X)
54

Programming of a (complete) circle in just one block:

Programming manual

PATH CONTROL Circular interpolation (G02, G03)

Various programming modes analyzed below, point X170 Y80 being the starting Point.
Cartesian coordinates: G90 G17 G02 X170 Y80 I-50 J0
or: G90 G17 G02 I-50 J0
Polar coordinates. G90 G17 G02 Q36 0I-50 J0
or: G93 I120 J80 ; defines polar center G02 Q360
Cartesian coordinates with radius programming: A complete circle cannot be programmed as there is an infinite range of solutions.

CNC 8040
·M· MODEL (SOFT V11.1X)
55

Programming manual
6.4 Circular interpolation with absolute arc center coordinates (G06)

By adding function G06 to a circular interpolation block you can program the coordinates of the center of the arc (I,J, or K) in absolute coordinates i.e. with respect to the zero origin and not to the beginning of the arc.
Function G06 is not modal, so it should be programmed any time the coordinates of the center of the arc are required in absolute coordinates. G06 can be programmed as G6.

PATH CONTROL Circular interpolation with absolute arc center coordinates (G06)

Various programming modes are analyzed below, point X60 Y40 being the starting point. Cartesian coordinates:
G90 G17 G06 G03 X110 Y90 I60 J90 G06 X160 Y40 I160 J90 Polar coordinates: G90 G17 G06 G03 Q0 I60 J90 G06 Q-90 I160 J90
CNC 8040
·M· MODEL (SOFT V11.1X)
56

6.5 Arc tangent to previous path (G08)

Programming manual

Via function G08 you can program an arc tangential to the previous path without having to program the coordinates (I.J &K) of the center.
Only the coordinates of the endpoint of the arc are defined, either in polar coordinates or in Cartesian coordinates according to the axes of the work plane.

PATH CONTROL Arc tangent to previous path (G08)

Supposing that the starting point is X0 Y40, you wish to program a straight line, then an arc tangential to the line and finally an arc tangential to the previous one.

G90 G01 X70 G08 X90 Y60 G08 X110 Y60

; Arc tangent to previous path. ; Arc tangent to previous path.

Function G08 is not modal, so it should always be programmed if you wish to execute an arc tangential to the previous path. Function G08 can be programmed as G8.
Function G08 enables the previous path to be a straight line or an arc and does not alter its history. The same function G01, G02 or G03 stays active after the block is finished.

When using function G08 it is not possible to execute a complete circle, as an infinite range of solutions exists. The CNC displays the corresponding error code.

CNC 8040
·M· MODEL (SOFT V11.1X)
57

Programming manual
6.6 Arc defined by three points (G09)

PATH CONTROL Arc defined by three points (G09)

Through function G09 you can define an arc by programming the endpoint and an intermediate point (the starting point of the arc is the starting point of the movement). In other words, instead of programming the coordinates of the center, you program any intermediate point.

The endpoint of the arc is defined in Cartesian or polar coordinates, and the intermediate point is always defined in Cartesian coordinates by the letters I,J, or K, each one being associated to the axes as follows:

Axes X, U, A Axes Y, V, B Axes Z, W, C

==> I ==> J ==> K

In Cartesian coordinates:

G17

G09

X±5.5

Y±5.5

I±5.5

J±5.5

Polar coordinates:

G17

G09

R±5.5 Q±5.5 I±5.5

J±5.5

Example:

CNC 8040
·M· MODEL (SOFT V11.1X)
58

Being initial point X-50 Y0. G09 X35 Y20 I-15 J25
Function G09 is not modal, so it should always be programmed if you wish to execute an arc defined by three points. Function G09 can be programmed as G9.
When G09 is programmed it is not necessary to program the direction of movement (G02 or G03).
Function G09 does not alter the history of the program. The same G01, G02 or G03 function stays active after finishing the block.
When using function G09 it is not possible to execute a complete circle, as you have to program three different points. The CNC displays the corresponding error code.

6.7 Helical interpolation

Programming manual

A helical interpolation consists in a circular interpolation in the work plane while moving the rest of the programmed axes.

PATH CONTROL Helical interpolation

The helical interpolation is programmed in a block where the circular interpolation must be programmed by means of functions: G02, G03, G08 or G09.
G02 X Y I J Z G02 X Y R Z A G03 Q I J A B G08 X Y Z G09 X Y I J Z
If the helical interpolation is supposed to make more than one turn, the linear movement of another axis must also be programmed (one axis only).
On the other hand, the pitch along the linear axis must also be set (format 5.5) by means of the I, J and K letters. Each one of these letters is associated with the axes as follows:
Axes X, U, A ==> I Axes Y, V, B ==> J Axes Z, W, C ==> K
G02 X Y I J Z K G02 X Y R Z K G03 Q I J A I G08 X Y B J G09 X Y I J Z K
Example:
Programming in Cartesian and polar coordinates, the starting point being X0 Y0 Z0.

Cartesian coordinates: G03 X0 Y0 I15 J0 Z50 K5
Polar coordinates: G03 Q180 I15 J0 Z50 K5

CNC 8040
·M· MODEL (SOFT V11.1X)

PATH CONTROL Tangential entry at the beginning of a machining operation (G37)

Programming manual
6.8 Tangential entry at the beginning of a machining operation (G37)

Via function G37 you can tangentially link two paths without having to calculate the intersection points.
Function G37 is not modal, so it should always be programmed if you wish to start a machining operation with tangential entry:

If the starting point is X0 Y30 and you wish to machine an arc (the path of approach being straight) you should program:
G90 G01 X40
G02 X60 Y10 I20 J0

CNC 8040
·M· MODEL (SOFT V11.1X)
60

PATH CONTROL Tangential entry at the beginning of a machining operation (G37)

Programming manual If, however, in the same example you require the entrance of the tool to the part to be machined tangential to the path and describing a radius of 5 mm, you should program:
6.
G90 G01 G37 R5 X40 G02 X60 Y10 I20 J0 As can be seen in the figure, the CNC modifies the path so that the tool starts to machine with a tangential entry to the part. You have to program Function G37 plus value R in the block which includes the path you want to modify. R5.5 should appear in all cases following G37, indicating the radius of the arc which the CNC enters to obtain tangential entry to the part. This R value must always be positive. Function G37 should only be programmed in the block which includes a straight-line movement (G00 or G01). If you program in a block which includes circular movement (G02 or G03), the CNC displays the corresponding error.
CNC 8040
·M· MODEL (SOFT V11.1X)
61

Programming manual
6.9 Tangential exit at the end of a machining operator (G38)

Function G38 enables the ending of a machining operation with a tangential exit of the tool. The path should be in a straight line (G00 or G01). Otherwise, the CNC will display the corresponding error.
Function G38 is not modal, so it should be programmed whenever a tangential exit of the tool is required.
Value R 5.5 should always appear after G38. It also indicates the radius of the arc which the CNC applies to get a tangential exit from the part. This R value must always be positive.

PATH CONTROL Tangential exit at the end of a machining operator (G38)

If the starting point is X0 Y30 and you wish to machine an arc (with the approach and exit paths in a straight line), you should program :
G90 G01 X40 G02 X80 I20 J0 G00 X120

CNC 8040
·M· MODEL (SOFT V11.1X)
62

PATH CONTROL Tangential exit at the end of a machining operator (G38)

Programming manual If, however, in the same example you wish the exit from machining to be done tangentially and describing a radius of 5 mm, you should program :
G90 G01 X40 G02 G38 R5 X80 I20 J0 G00 X120
6.
CNC 8040
·M· MODEL (SOFT V11.1X)
63

Programming manual
6.10 Automatic radius blend (G36)

In milling operations, it is possible to round a corner via function G36 with a determined radius, without having to calculate the center nor the start and end points of the arc.
Function G36 is not modal, so it should be programmed whenever controlled corner rounding is required.
This function should be programmed in the block in which the movement the end you want to round is defined.
The R5.5 value should always follow G36. It also indicates the rounding radius which the CNC applies to get the required corner rounding. This R value must always be positive.
G90 G01 G36 R5 X35 Y60 X50 Y0

PATH CONTROL Automatic radius blend (G36)

G90 G03 G36 R5 X50 Y50 I0 J30 G01 X50 Y0

CNC 8040
·M· MODEL (SOFT V11.1X)
64

6.11 Chamfer (G39)

Programming manual

In machining operations it is possible (using G39) to chamfer corners between two straight lines, without having to calculate intersection points.
Function G39 is not modal, so it should be programmed whenever the chamfering of a corner is required.
This function should be programmed in the block in which the movement whose end you want to chamfer is defined.
The R5.5 value should always follow G39. It also indicates the distance from the end of the programmed movement as far as the point where you wish to carry out the chamfering. This R value must always be positive.
G90 G01 G39 R15 X35 Y60 X50 Y0

PATH CONTROL Chamfer (G39)

CNC 8040
·M· MODEL (SOFT V11.1X)
65

Programming manual
6.12 Threading (G33)

PATH CONTROL Threading (G33)

If the machine spindle is equipped with a rotary encoder, you can thread with a tool tip via function G33.
Although this threading is often done along the entire length of an axis, the CNC enables threading to be done interpolating more than one axis at a time.
Programming format: G33 X.....C L Q
X...C ±5.5 End point of the thread
L 5.5 Thread pitch
Q ±3.5 Optional. It indicates the spindle angular position (±359.9999) of the thread's starting point. If not programmed, a value of "0" is assumed.

Considerations

Whenever G33 is executed and before making the thread, the CNC referenced the spindle (home search) and positions the spindle at the angular position indicated by parameter Q.

Parameter "Q" is available when spindle machine parameter "M19TYPE" has been set to "1".

If the threads are blended together in round corner, only the first one can have an entry angle (Q).

While function G33 is active, neither the programmed feedrate "F" nor the programmed Spindle speed "S" can be varied. They will both be set to 100%.

Function G33 is modal and incompatible with G00, G01, G02, G03, G34 and G75.
On power-up, after executing M02, M30 or after EMERGENCY or RESET, the CNC assumes code G00 or G01, depending on how general machine parameter "IMOVE" has been set.

Example
We would like to a make a thread in a single pass in X0 Y0 Z0, with a depth of 100 mm and a pitch of 5 mm using a threadcutting tool located in Z10.

G90 G0 X Y Z G33 Z -100 L5 M19 G00 X3 Z30

; Positioning ; Roscado ; Spindle orientation ; Cutter withdrawal ; Withdrawal (exit the hole)

CNC 8040

·M· MODEL (SOFT V11.1X)

6.13 Variable pitch threads (G34)

Programming manual

To make variable-pitch threads, the spindle of the machine must have a rotary encoder.

Although this threading is often done along the entire length of an axis, the CNC enables threading to be done interpolating more than one axis at a time.

Programming format: G34 X.....C L Q K

X...C ±5.5 End point of the thread

L 5.5

Thread pitch

Q ±3.5

Optional. It indicates the spindle angular position (±359.9999) of the thread's starting point. If not programmed, a value of "0" is assumed.

K ±5.5

Thread pitch increase or decrease per spindle turn.

Considerations
Whenever G34 is executed and before making the thread, the CNC referenced the spindle (home search) and positions the spindle at the angular position indicated by parameter Q.
Parameter "Q" is available when spindle machine parameter "M19TYPE" has been set to "1".
When working in round corner mode (G05), it is possible to blend different threads in the same part.
While function G34 is active, neither the programmed feedrate "F" nor the programmed Spindle speed "S" can be varied. They will both be set to 100%.
Function G34 is modal and incompatible with G00, G01, G02, G03, G33 and G75.
On power-up, after executing M02, M30 or after EMERGENCY or RESET, the CNC assumes code G00 or G01, depending on how general machine parameter "IMOVE" has been set.
Blending a fixed-pitch thread (G33) with a variable-pitch thread (G34).
The starting thread pitch (L) of the G34 must coincide with the thread pitch of the G33.
The pitch increase in the first turn of the spindle in variable pitch will be half and increment (K/2) and in the rest of the turns it will be the full increment K.
Blending a variable-pitch thread (G34) with a fixed-pitch thread.
It is used to finish a variable-pitch thread (G34) with a portion of the thread keeping the final pitch of the previous thread.
Since it is very complicated to calculate the final thread pitch, the fixed-pitch thread is not programmed with G33 but with G34 ... L0 K0. The CNC calculates the pitch.
Two variable-pitch threads (G34) cannot be blended together.

PATH CONTROL Variable pitch threads (G34)

6.
CNC 8040

·M· MODEL (SOFT V11.1X)

Programming manual
6.14 Move to hardstop (G52)

By means of function G52 it is possible to program the movement of an axis until running into an object. This feature may be interesting for forming machines, live tailstocks, bar feeders, etc.
The programming format is: G52 X..C ±5.5
After G52, program the desired axis as well as the target coordinate of the move.
The axis will move towards the programmed target coordinate until running into something. If the axis reaches the programmed target coordinate without running into the hardstop it will stop.
Function G52 is not modal; therefore, it must be programmed every time this operation is to be carried out.
Also, it assumes functions G01 and G40 modifying the program history. It is incompatible with functions G00, G02, G03, G33, G34, G41, G42, G75 and G76.

PATH CONTROL Move to hardstop (G52)

CNC 8040
·M· MODEL (SOFT V11.1X)
68

Programming manual
6.15 Feedrate "F" as an inverted function of time (G32)

There are instances when it is easier to define the time required by the various axes of the machine to reach the target point instead of defining a common feedrate for all of them.
A typical case may be when a linear axis (X, Y, Z) has to move together (interpolated) with a rotary axis programmed in degrees.
Function G32 indicates that the "F" functions programmed next set the time it takes to reach the target point.
In order for a greater value of "F" to indicate a greater feedrate, the value assigned to "F" is defined as "Inverted function of time" and it is assumed as the activation of this feature.
"F" units: 1/min Example: G32 X22 F4 indicates that the movement must be executed in ¼ minute; i.e. in 0.25 minutes.
Function G32 is modal and incompatible with G94 and G95.
On power-up, after executing M02, M30 or after an Emergency or Reset, the CNC assumes G94 or G95 depending on the setting of general machine parameter "IFFED".
Considerations
The CNC variable PROGFIN will show the feedrate programmed as an inverted function of time and variable FEED will show the resulting feedrate in mm/min or inches/min.
If the resulting feedrate of any axis exceeds the maximum value set by machine parameter "MAXFEED", the CNC will apply this maximum value.
The programmed "F" is ignored on G00 movements. All the movements will be carried out at the feedrate set by axis machine parameter "G00FEED".
When programming "F0" the movement will be carried out at the feedrate set by axis machine parameter "MAXFEED".
Function G32 may be programmed and executed in the PLC channel.
Function G32 is canceled in JOG mode.

PATH CONTROL Feedrate "F" as an inverted function of time (G32)

CNC 8040
·M· MODEL (SOFT V11.1X)
69

Programming manual
6.16 Tangential control (G45)
With the "Tangential control" feature, the axis may maintain the same orientation with respect to the programmed path.

PATH CONTROL Tangential control (G45)

Orientation parallel to the path

Orientation perpendicular to the path

The path is defined by the axes of the active plane. The axis maintaining the orientation must be a rotary rollover axis (A, B or C).

Programming format: G45 Axis Angle

Axis Angle

Axis maintaining the orientation (A, B or C)
Indicates the angular position in degrees with respect to the path (±359.9999). If not programmed, "0" will be assumed.

CNC 8040
·M· MODEL (SOFT V11.1X)
70

To cancel this function, program G45 alone (without defining the axis). Every time G45 (tangential control) is activated, the CNC acts as follows: 1. Positions the tangential axis, with respect to the first section in the programmed
position.
2. The interpolation of the axes in the plane starts once the tangential axis has been positioned.
3. On linear sections, the orientation of the tangential axis is maintained and in circular interpolations, the programmed orientation is maintained for the whole path.

Programming manual
4. If the joint of sections requires a new orientation of the tangential axis, the following takes place: 1. Ends the current section. 2. Orients the tangential axis with respect to the next section. 3. Resumes the execution.

When working in round corner (G05), the tool orientation is not maintained at the corners since it begins before ending the current section.
It is recommended to work in square corner (G07). However, to work in round corner (G05), function G36 (automatic radius blend) should be used in order to also maintain tool orientation at the corners.
5. To cancel this function, program G45 alone (without defining the axis).
Even when the tangential axis takes the same orientation by programming 90° or 270°, the turning direction in a direction change depends on the programmed value.

PATH CONTROL Tangential control (G45)

CNC 8040
·M· MODEL (SOFT V11.1X)
71

Programming manual
6.16.1 Considerations about the G45 function

PATH CONTROL Tangential control (G45)

Tangential control, G45, is optional. It can only be executed in the main channel and is compatible with:
· Tool radius and length compensation (G40, 41, 42, 43, 44) · Mirror image (G10, 11, 12, 13 14) · Gantry axes , including the gantry axis associated with the tangential rotary axis.
The maximum feedrate while orienting the tangential axis is defined by machine parameter MAXFEED for that axis.
While tangential control is active, tool inspection is also possible. When accessing tool inspection, the tangential control is deactivated, the axes are free and when quitting tool inspection, tangential control may be activated again.
While in JOG mode, tangential control may be activated in MDI mode and the axes may be moved by programming blocks in MDI.
Tangential control is canceled when jogging the axes with the jog keys (not in MDI). Once the movement is over, tangential control is recovered.
Likewise, the following is NOT possible: · To define as tangential axis, one of the plane axes, the longitudinal axis or any other axis which is not rotary. · To jog the tangential axis in JOG mode or by program using another G code while tangential control is active. · Incline planes.
The TANGAN variable is read-only, from the CNC, PLC and DNC, associated with function G45. It indicates the angular position, in degrees, referred to the programmed path.
Also, general logic output TANGACT (M5558) indicates to the PLC that function G45 is active.
Function G45 is modal and is canceled when executing G45 alone (without defining the axis), on power-up, after executing an M02 or M30 or after an EMERGENCY or RESET.

CNC 8040
·M· MODEL (SOFT V11.1X)
72

Programming manual
6.17 G145. Temporary cancellation of tangential control

Function G145 may be used to cancel the tangential control (G45) temporarily:

G145 K0

It cancels the tangential control temporarily. Function G45 stays in the history and the new function G145 comes up in it.
If no G45 has been programmed, G145 is ignored. If K is not programmed, K0 will be assumed.

G145 K1 It resumes the tangential control of the axis with the angle it had before it was canceled. Then, G145 disappears from history.

PATH CONTROL G145. Temporary cancellation of tangential control

CNC 8040
·M· MODEL (SOFT V11.1X)
73

Programming manual
6.
CNC 8040
·M· MODEL (SOFT V11.1X)
74

PATH CONTROL G145. Temporary cancellation of tangential control

ADDITIONAL PREPARATORY FUNCTIONS

7.1 Interruption of block preparation (G04)

The CNC reads up to 20 blocks ahead of the one it is executing, with the aim of calculating beforehand the path to be followed.

Each block is evaluated (in its absence) at the time it is read, but if you wish to evaluate it at the time of execution of the block you use function G04.

This function holds up the preparation of blocks and waits for the block in question to be executed in order to start the preparation of blocks once more.

A case in point is the evaluation of the "status of block-skip inputs" which is defined in the block header.

Example:

G04

; Interrupts block preparation

/1 G01 X10 Y20 ; block-skip condition "/1"

Function G04 is not modal, so it should be programmed whenever you wish to interrupt block preparation.

It should be programmed on its own and in the block previous to the one in which the evaluation in execution is required. Function G04 can be programmed as G4.

Every time G04 is programmed, active radius and length compensation are cancelled.

For this reason, care needs to be taken when using this function, because if it is introduced between machining blocks which work with compensation, unwanted profiles may be produced.

CNC 8040
·M· MODEL (SOFT V11.1X)
75

Programming manual
7.

Example: The following program blocks are performed in a section with G41 compensation.
... N10 X50 Y80 N15 G04
/1 N17 M10 N20 X50 Y50 N30 X80 Y50
...
Block N15 interrupts block preparation and the execution of block N10 will finish at point A.

ADDITIONAL PREPARATORY FUNCTIONS Interruption of block preparation (G04)

Once the execution of block N15 has been carried out, the CNC continues preparing blocks starting from block N17.
As the next point corresponding to the compensated path is point "B", the CNC will move the tool to this point, executing path "A-B".

CNC 8040
·M· MODEL (SOFT V11.1X)
76

As you can see, the resulting path is not the required one, so we recommend avoiding the use of function G04 in sections which work with compensation.

Programming manual
7.1.1 G04 K0: Block preparation interruption and coordinate update

The function associated with G04 K0 may be used to update the coordinates of the axes of the channel after finishing particular PLC maneuvers.

The PLC maneuvers that require updating the coordinates of the axes of the channel are the following:
· PLC maneuver using the SWITCH* marks.
· PLC maneuvers where an axis goes into DRO mode and then back into normal axis mode during the execution of part programs.

G04 operation:

Function

Description

G04

Interrupts block preparation.

G04 K50

It executes a dwell 50 hundredths of a second.

G04 K0 or G04 K It interrupts block preparation and updates the CNC coordinates to the current position.
(G4 K0 works in the CNC and PLC channel).

ADDITIONAL PREPARATORY FUNCTIONS Interruption of block preparation (G04)

CNC 8040
·M· MODEL (SOFT V11.1X)
77

Programming manual
7.2 Dwell (G04 K)

A dwell can be programmed via function G04 K.

The dwell value is programmed in hundredths of a second via format K5 (1..99999).

Example: G04 K50 G04 K200

; Dwell of 50 hundredths of a second (0.5 seconds) ; Dwell of 200 hundredths of a second (2 seconds)

Function G04 K is not modal, so it should be programmed whenever a dwell is required. Function G04 K can be programmed as G4 K.

The dwell is executed at the beginning of the block in which it is programmed.

Note: When programming G04 K0 or G04 K, instead of applying a delay, it only interrupts block preparation and it will refresh the coordinates. See "7.1.1 G04 K0: Block preparation interruption and coordinate update" on page 77.

ADDITIONAL PREPARATORY FUNCTIONS Dwell (G04 K)

CNC 8040
·M· MODEL (SOFT V11.1X)
78

Programming manual
7.3 Working with square (G07) and round (G05,G50) corners

7.3.1 G07 (square corner)
When working in G07 (square corner) the CNC does not start executing the following program block until the position programmed in the current block has been reached.
The CNC considers that the programmed position has been reached when the axis is within the "INPOSW" (in-position zone or dead band) from the programmed position.

G91 G01 G07 Y70 F100 X90

ADDITIONAL PREPARATORY FUNCTIONS Working with square (G07) and round (G05,G50) corners

The theoretical and real profile coincide, obtaining square corners, as seen in the figure.
Function G07 is modal and incompatible with G05, G50 and G51. Function G07 can be programmed as G7.
On power-up, after executing M02, M30 or after EMERGENCY or RESET, the CNC assumes code G05 or G07 depending on how the general machine parameter "ICORNER" is set.

CNC 8040
·M· MODEL (SOFT V11.1X)
79

Programming manual
7.3.2 G05 (round corner)

When working in G05 (round corner), the CNC starts executing the following block of the program as soon as the theoretical interpolation of the current block has concluded. It does not wait for the axes to physically reach the programmed position.
The distance prior to the programmed position where the CNC starts executing the next block depends on the actual axis feedrate.

G91 G01 G05 Y70 F100 X90

ADDITIONAL PREPARATORY FUNCTIONS Working with square (G07) and round (G05,G50) corners

Via this function round corners can be obtained, as shown in the figure.
The difference between the theoretical and real profiles depends on the programmed feedrate value "F". The higher the feedrate, the greater the difference between both profiles.
Function G05 is modal and incompatible with G07, G50 and G51. Function G05 can be programmed as G5.
On power-up, after executing M02, M30 or after EMERGENCY or RESET, the CNC assumes code G05 or G07 depending on how the general machine parameter "ICORNER" is set.

CNC 8040
·M· MODEL (SOFT V11.1X)
80

7.3.3 Controlled round corner (G50)

Programming manual

When working in G50 (controlled round corner); once the theoretical interpolation of the current block has concluded, the CNC waits for the axis to enter the area defined by machine parameter "INPOSW2" and it then starts executing the following block of the program.

G91 G01 G50 Y70 F100 X90

ADDITIONAL PREPARATORY FUNCTIONS Working with square (G07) and round (G05,G50) corners

Function G50 assures that the difference between the theoretical and actual paths stays smaller than what was set by machine parameter "INPOSW2".
On the other hand, when working in G05, the difference between the theoretical and real profiles depends on the programmed feedrate value "F". The higher the feedrate, the greater the difference between both profiles.
Function G50 is modal and incompatible with G07, G05 and G51.
On power-up, after executing M02, M30 or after EMERGENCY or RESET, the CNC assumes code G05 or G07 depending on how the general machine parameter "ICORNER" is set.

CNC 8040
·M· MODEL (SOFT V11.1X)
81

Programming manual
7.4 Look-ahead (G51)

7.
CNC 8040
·M· MODEL (SOFT V11.1X)

ADDITIONAL PREPARATORY FUNCTIONS Look-ahead (G51)

Programs consisting of very small movement blocks (CAM, etc.) tend to run very slowly. With look-ahead, high speed machining is possible for this type of programs.

The look-ahead function analyzes in advance the path to be machined (up to 75 blocks) in order to calculate the maximum feedrate for each section of the path. This function provides smoother and faster machining in programs with very small movements, even in the order of microns.
It is recommended to have the CPU-TURBO option when using the look-ahead function.
When operating with "Look-Ahead", it is a good idea to adjust the axes so their following error (lag) is as small as possible because the contouring error will be at least equal to the minimum following error.

Programming format. The programming format is:
G51 [A] E

A (0-255) E (5.5)

Is optional and it defines the percentage of acceleration to be applied. When not programmed or programmed with a "0" value, the CNC assumes the acceleration value set by machine parameter for each axis.
Maximum contouring error. The lower this parameter value is, the lower the machining feedrate will be.

Parameter "A" permits using a standard working acceleration and another one to be used when executing with Look-Ahead.
Considerations for the execution.
When calculating the feedrate, the CNC takes the following into account: · The programmed feedrate. · The curvature and the corners. · The maximum feedrate of the axes. · The maximum accelerations. · The jerk.
If any of the circumstances listed below occurs while executing with Look-Ahead, the CNC slows down to "0" at the previous block and it recovers the machining conditions for Look-Ahead in the next motion block.
· Motionless block. · Execution of auxiliary functions (M, S, T). · Single block execution mode. · MDI mode. · Tool inspection mode.
If a Cycle Stop, Feed-Hold, etc. occurs while executing in Look-Ahead mode, the machine may not stop at the current block, several additional blocks will be necessary to stop with the permitted deceleration.
Function properties.
Function G51 is modal and incompatible with G05, G07 and G50. Should any of them be programmed, function G51 will be canceled and the new one will be selected.
Function G51 must be programmed alone in a block and there must be no more information in that block.

Programming manual

On power-up, after executing an M02, M30, of after an EMERGENCY or RESET, the CNC will cancel G51, if it was active, and it will assume G05 or G07 according to the setting of general machine parameter "ICORNER".

On the other hand, the CNC will issue Error 7 (Incompatible G functions) when programming any of the following functions while G51 is active:

G33

Electronic threading (G33)

G34

Variable-pitch threading.

G52

Move to hardstop.

G95

Feedrate per revolution.

ADDITIONAL PREPARATORY FUNCTIONS Look-ahead (G51)

CNC 8040
·M· MODEL (SOFT V11.1X)
83

Programming manual
7.5 Mirror image (G10, G11. G12, G13, G14)

The functions to activate the mirror image are the following.

G10:

Cancel mirror image.

G11:

Mirror image on X axis

G12:

Mirror image on Y axis.

G13:

Mirror image on Z axis

G14:

Mirror image on any axis (X..C), or in several at the same time.

Examples:

G14 W

G14 X Z A B

When the CNC works with mirror images, it executes the movements programmed in the axes that have mirror image selected, with the sign changed.

ADDITIONAL PREPARATORY FUNCTIONS Mirror image (G10, G11. G12, G13, G14)

CNC 8040
·M· MODEL (SOFT V11.1X)
84

The following subroutine defines the machining of part "a". G91 G01 X30 Y30 F100 Y60 X20 Y-20 X40 G02 X0 Y-40 I0 J-20 G01 X-60 X-30 Y-30

The programming of all parts would be :

Execution of subroutine ; machines "a"

G11

; Mirror image on X axis.

Execution of subroutine ; machines "b"

G10 G12

; Mirror image on Y axis.

Execution of subroutine ; machines "c"

G11

; Mirror image on X and Y axes.

Execution of subroutine ; Machines "d"

M30

; End of program

Programming manual

Functions G11, G12, G13, and G14 are modal and incompatible with G10.
G11, G12, and G13 can be programmed in the same block, because they are not incompatible with each other. Function G14 must be programmed alone in the block.

If function G73 (pattern rotation) is also active in a mirror image program, the CNC first applies the mirror image function and then the pattern rotation.

If while one of the mirror imaging functions (G11, G12, G13, and G14) is active, a new coordinate origin (part zero) is preset with G92, this new origin will not be affected by the mirror imaging function.
On power-up, after executing M02, M30 or after EMERGENCY or RESET, the CNC assumes code G10.

ADDITIONAL PREPARATORY FUNCTIONS Mirror image (G10, G11. G12, G13, G14)

CNC 8040
·M· MODEL (SOFT V11.1X)
85

Programming manual
7.6 Scaling factor (G72)

By using function G72 you can enlarge or reduce programmed parts.
In this way, you can produce families of parts which are similar in shape but of different sizes with a single program.
Function G72 should be programmed on its own in a block. There are two formats for programming G72 :
· Scaling factor applied to all axes. · Scaling factor applied to one or more axes.

ADDITIONAL PREPARATORY FUNCTIONS Scaling factor (G72)

CNC 8040
·M· MODEL (SOFT V11.1X)
86

7.6.1 Scaling factor applied to all axes.

Programming manual

The programming format is: G72 S5.5
Following G72 all coordinates programmed are multiplied by the value of the scaling factor defined by S until a new G72 scaling factor definition is read or the definition is cancelled.
Programming example (starting point X-30 Y10)

ADDITIONAL PREPARATORY FUNCTIONS Scaling factor (G72)

The following subroutine defines the machining of the part. G90 X-19 Y0 G01 X0 Y10 F150 G02 X0 Y-10 I0 J-10 G01 X-19 Y0

The programming of the parts would be :

Execution of subroutine Machines "a".

G92 X-79 Y-30

; Coordinate preset

(zero offset)

G72 S2

; Applies a scaling factor of 2

Execution of subroutine Machines "b".

G72 S1

; Cancel the scaling factor

M30

; End of program

CNC 8040
·M· MODEL (SOFT V11.1X)
87

Programming manual

Examples of application of the scaling factor.

ADDITIONAL PREPARATORY FUNCTIONS Scaling factor (G72)

G90 G00 X0 Y0 N10 G91 G01 X20 Y10 Y10 X-10 X-10 X20 N20 X-10 Y-20
; Scaling factor G72 S0.5
; Repeats from block 10 to block 20 (RPT N10,20) M30

G90 G00 X20 Y20 N10 G91 G01 X-10 Y -20 Y10 N20 Y10
; Scaling factor G72 S0.5
; Repeats from block 10 to block 20 (RPT N10,20) M30

Function G72 is modal and is cancelled when another scaling factor with a value of S1 is programmed, or on power-up, after executing M02, M30 or after EMERGENCY or RESET.

CNC 8040
·M· MODEL (SOFT V11.1X)
88

ADDITIONAL PREPARATORY FUNCTIONS Scaling factor (G72)

7.6.2 Scaling factor applied to one or more axes.

Programming manual

The programming format is: G72 X...C 5.5
After G72 the axis or axes and the required scaling factor are programmed.
All blocks programmed after G72 are treated by the CNC as follows : 1. The CNC calculates the movement of all the axes in relation to the programmed
path and compensation. 2. It then applies the scaling factor indicated to the calculated movement of the
corresponding axis or axes.
If the scaling factor is applied on one or more axes, the CNC will apply the scaling factor indicated both to the movement of the corresponding axis or axes and to their feedrate.
If, within the same program, both scaling factor types are applied, the one applied to all the axes and the one for one or several axes, the CNC applies a scaling factor equal to the product of the two scaling factors programmed for this axis to the axis or axes affected by both types.
Function G72 is modal and will be cancelled when the CNC is turned on, after executing M02, M30 or after an EMERGENCY or RESET.

This type of scaling factor is ignored when simulating without moving the axes.

Application of the scaling factor to a plane axis, working with tool radius compensation.

As it can be observed, the tool path does not coincide with the required path, as the scaling factor is applied to the calculated movement.
CNC 8040
·M· MODEL (SOFT V11.1X)
89

Programming manual

If a scaling factor equal to 360/2R is applied to a rotary axis, R being the radius of the cylinder on which you wish to machine, this axis can be considered linear, and any figure with tool radius compensation can be programmed on the cylindrical surface.

ADDITIONAL PREPARATORY FUNCTIONS Scaling factor (G72)

CNC 8040
·M· MODEL (SOFT V11.1X)
90

7.7 Pattern rotation (G73)

Programming manual

Function G73 enables you to turn the system of coordinates, taking either the coordinates origin or the programmed rotation center as the active rotation center.

The format which defines the rotation is the following : G73 Q+/5.5 I±5.5 J±5.5

Where:

Indicates the angle of rotation in degrees

I, J:

The are optional and define the abscissa and ordinate respectively of

the rotation center. If they are not defined, the coordinate origin will be

taken as the rotation center.

The "I" and "J" values are defined in absolute coordinates and referred to the coordinate origin of the work plane. These coordinates are affected by the active scaling factor and mirror images.

ADDITIONAL PREPARATORY FUNCTIONS Pattern rotation (G73)

You should remember that G73 is incremental i.e. the different Q values programmed add up.

Function G73 should be programmed on its own in a block.

CNC 8040
·M· MODEL (SOFT V11.1X)
91

Programming manual

Assuming that the starting point is X0 Y0, you get :

ADDITIONAL PREPARATORY FUNCTIONS Pattern rotation (G73)

N10 G01 X21 Y0 F300 G02 Q0 I5 J0 G03 Q0 I5 J0 Q180 I-10 J0 N20 G73 Q45 (RPT N10, N20) N7 M30

; Positioning at starting point
; Coordinate (pattern) rotation ; Repeat from block 10 to 20 seven times ; End of program

In a program which rotates the coordinate system, if any mirror image function is also active the CNC first applies the mirror image function and then the turn.
The pattern rotation function can be cancelled either by programming G72 (on its own, without angle value) or via G16, G17, G18, or G19, or on power-up, after executing M02, M30 or after EMERGENCY or RESET.

CNC 8040
·M· MODEL (SOFT V11.1X)
92

7.8 Electronic axis coupling/uncoupling

Programming manual

The CNC enables two or more axes to be coupled together. The movement of all axes is subordinated to the movement of the axis to which they were coupled.
There are three possible ways of coupling axes :
· Mechanical coupling. This is imposed by the manufacturer of the machine, and is selected via the axis machine parameter "GANTRY".
· By PLC. This enables the coupling and uncoupling of each axis through logic input on the CNC "SYNCHRO1", "SYNCHRO2", "SYNCHRO3", "SYNCHRO4", and "SYNCHRO5". Each axis is coupled to the one indicated in the axis machine parameter "SYNCHRO".
· By program. This enables electronic coupling and uncoupling between two or more axes, through functions G77 and G78.

ADDITIONAL PREPARATORY FUNCTIONS Electronic axis coupling/uncoupling

CNC 8040
·M· MODEL (SOFT V11.1X)
93

Programming manual
7.8.1 Electronic axis coupling, slaving, (G77)

ADDITIONAL PREPARATORY FUNCTIONS Electronic axis coupling/uncoupling

Function G77 allows the selection of both the master axis and the slaved axis (axes). The programming format is as follows :
G77 <Axis 1> <Axis 2> <Axis 3> <Axis 4> <Axis 5>
Where <Axis 2>, <Axis 3>, <Axis 4> and <Axis 5> will indicate the axes to be coupled to <Axis 1>. You have to define <Axis 1> and <Axis 2>, the programming of the rest of the axes being optional.

Example: G77 X Y U ; Couples the Y and U axes to the X axis

The following rules should be observed when slaving axes electronically:

· You may use one or two different electronic couplings.

G77 X Y U ; Couples the Y and U axes to the X axis

G77 V Z

; Couples the Z axis to the V axis.

· You cannot couple one axis to two others at the same time.

G77 V Y ; Couples the Y axis to the V axis.

G77 X Y ; Gives an error signal, because the Y axis is coupled to the V axis.

· You can couple several axes to one in successive steps.

G77 X Z

; Couples the Z axis to the X axis.

G77 X U ; Couples the U axis to the X axis --> Z U coupled to X.

G77 X Y ; Couples the Y axis to the X axis --> Y Z U coupled to X.

· A pair of axes which are already coupled to each other cannot be coupled to another axis.

G77 Y U ; Couples the U axis to the Y axis.

G77 X Y ; Issues an error because Y axis is coupled to U axis.

CNC 8040
·M· MODEL (SOFT V11.1X)
94

Programming manual
7.8.2 Cancellation of the electronic axis coupling, slaving, (G78)

Function G78 enables you to uncouple all the axes that are coupled (slaved), or only uncouple indicated axes.

G78

Uncouples all slaved axes.

G78 <Axis 1> <Axis 2> <Axis 3> <Axis 4> Only uncouples the indicated axes.

Example. G77 X Y U G77 V Z G78 Y G78

; Couples the Y and U axes to the X axis ; Couples the Z axis to the V axis ; uncouples Y axis, but U stays coupled to X and Z to V. ; Uncouples all axes

ADDITIONAL PREPARATORY FUNCTIONS Electronic axis coupling/uncoupling

CNC 8040
·M· MODEL (SOFT V11.1X)
95

Programming manual
7.9 Axes toggle G28-G29
With this feature, on machines having two machining tables, it is possible to use a single part-program to make the same parts on both tables.

ADDITIONAL PREPARATORY FUNCTIONS Axes toggle G28-G29

With function G28 the axes can be toggled from one to the other in such way that after that instruction all the movements associated with the first axis next to G28 will take place on the second axis next to G28 and vice versa.
Programming format: G28 (axis 1) (axis 2)
To cancel the toggle, execute function G29 followed by one of the axes to be toggled back. Up to three pairs of axes may be toggled at the same time.
On power-up, after executing M30 or following an emergency or a reset, the axes are toggled back.
Example. Let us suppose that the part program is defined for table 1. 1. Execute the part-program on table 1 2. G28 BC. Toggle the "B" and "C" axes 3. Zero offset to machine on table 2 4. Execute the part-program.
· It will be executed on table 2. · In the meantime, replace the part made on table 1 with a new one. 5. G29 B. Toggle the "B" and "C" axes back. 6. Cancel zero offset to machine on table 1. 7. Execute the part-program. · It will be executed on table 1. · In the meantime, replace the part made on table 2 with a new one.

CNC 8040
·M· MODEL (SOFT V11.1X)
96

TOOL COMPENSATION

The CNC has a tool offset table, its number of components being defined via the general machine parameter "NTOFFSET". The following is specified for each tool offset:
· Tool radius, in work units, in R±5.5 format. · Tool length, in work units, in L±5.5 format. · Wear of tool radius, in work units, in I±5.5 format. The CNC adds this value to the
theoretical radius (R) to calculate the real radius (R+I). · Wear of tool length, in work units, in K±5.5 format. The CNC adds this value to
the theoretical length (L) to calculate the real length (L+K).
When tool radius compensation is required (G41 or G42), the CNC applies the sum of R+I values of the selected tool offset as the compensation value.
When tool length compensation is required (G43), the CNC applies the sum of L+K values of the selected tool offset as the compensation value.

CNC 8040
·M· MODEL (SOFT V11.1X)
97

Programming manual
8.1 Tool radius compensation (G40, G41, G42)

In normal milling operations, it is necessary to calculate and define the path of the tool taking its radius into account so that the required dimensions of the part are achieved.
Tool radius compensation allows the direct programming of part contouring and of the tool radius without taking the dimensions of the tool into account.
The CNC automatically calculates the path the tool should follow based on the contour of the part and the tool radius value stored in the tool offset table.
There are three preparatory functions for tool radius compensation: G40: Cancellation of tool radius compensation G41: Tool radius compensation to the left of the part. G42: Tool radius compensation to the right of the part.

TOOL COMPENSATION Tool radius compensation (G40, G41, G42)

G41

The tool is to the left of the part, depending on the machining

direction.

G42

The tool is to the right of the part, depending on the machining

direction.

Tool values R, L, I, K should be stored in the tool offset table before starting machining, or should be loaded at the beginning of the program via assignments to variables TOR, TOL, TOI, TOK.

Once the plane in which compensation will be applied has been chosen via codes G16, G17, G18, or G19, this is put into effect by G41 or G42, assuming the value of the tool offset selected via code D, or (in its absence) by the tool offset shown in the tool table for the selected tool (T).

Functions G41 and G42 are modal and incompatible to each other. They are cancelled by G40, G04 (interruption of block preparation), G53 (programming with reference to machine zero), G74 (home search), machining canned cycles (G81, G82, G83, G84, G85, G86, G87, G88, G89) and also on power-up, after executing M02, M30 or after EMERGENCY or RESET.

CNC 8040
·M· MODEL (SOFT V11.1X)
98

8.1.1 Beginning of tool radius compensation

Programming manual

Once the plane in which tool radius compensation has been selected (via G16, G17, G18, or G19), functions G41 or G42 must be used to activate it.
G41: Tool radius compensation to the left of the part. G42: Tool radius compensation to the right of the part.
In the same block (or a previous one) in which G41 or G42 is programmed, functions T, D, or only T must be programmed so that the tool offset value to be applied can be selected from the tool offset table. If no tool offset is selected, the CNC takes D0 with R0 L0 I0 K0.
When the new selected tool has function M06 associated with it and this, in turn, has an associated subroutine, the CNC will first process the motion block of that subroutine as the starting block of the compensation.
If in that subroutine, a block is executed that contains function G53 (programming in machine coordinates), the previously programmed G41 or G42 is canceled.
The selection of tool radius compensation (G41 or G42) can only be made when functions G00 or G01 are active (straight-line movements).
If the compensation is selected while G02 or G03 are active, the CNC will display the corresponding error message.
The following pages show different cases of starting tool radius compensation, in which the programmed path is represented by a solid line and the compensated path with a dotted line.
Beginning of compensation without programming a movement
After activating the compensation, it could happen that the plane axes do not get involved in the first motion block either because they have not been programmed or because the same point as the tool position has been programmed or because a null incremental move has been programmed.
In this case, the compensation is applied in the current tool position; depending on the first movement programmed in the plane, the tool moves perpendicular to the path on its starting point.
The first movement programmed in the plane may be linear or circular.

TOOL COMPENSATION Tool radius compensation (G40, G41, G42)

(X0 Y0)

· · · G90 G01 X-30 Y30 G01 G41 X-30 Y30 Z10 G01 X25 · · ·

Y
X
· · · G90 G01 Y40 G91 G40 Y0 Z10 G02 X20 Y20 I20 J0 · · ·
(X0 Y0)

CNC 8040
·M· MODEL (SOFT V11.1X)

Programming manual

STRAIGHT-STRAIGHT path

TOOL COMPENSATION Tool radius compensation (G40, G41, G42)

CNC 8040
·M· MODEL (SOFT V11.1X)
100

STRAIGHT-CURVED path

Programming manual
8.

TOOL COMPENSATION Tool radius compensation (G40, G41, G42)

CNC 8040
·M· MODEL (SOFT V11.1X)
101

Programming manual
8.1.2 Sections of tool radius compensation

The CNC reads up to 20 blocks ahead of the one it is executing, with the aim of calculating beforehand the path to be followed. When working with tool radius compensation, the CNC needs to know the next programmed movement to calculate the path to follow; therefore, no more than 17 blocks can be programmed in a row.
The diagrams (below) show the different paths followed by a tool controlled by a programmed CNC with tool radius compensation. The programmed path is represented by a solid line and the compensated path by a dotted line.

TOOL COMPENSATION Tool radius compensation (G40, G41, G42)

CNC 8040
·M· MODEL (SOFT V11.1X)
102

The way the various paths are blended (joined) depends on the setting of machine parameter COMPMODE.
· If it is set to ·0·, the compensation method depends on the angle between paths.
With an angle between paths of up to 300º, both paths are joined with straight sections. In the rest of the cases, both paths are joined with arcs.
· If it is set to ·1·, both paths are joined with arcs.
· If it is set to ·2·, the compensation method depends on the angle between paths.
With an angle between paths of up 300º, it calculates the intersection. In the rest of the cases it is compensated like COMPMODE = 0.

8.1.3 Cancellation of tool radius compensation

Programming manual

Tool radius compensation is cancelled by using function G40.
It should be remembered that canceling radius compensation (G40) can only be done in a block in which a straight-line movement is programmed (G00 or G01).
If G40 is programmed while functions G02 or G03 are active, the CNC displays the corresponding error message.
The following pages show different cases of canceling tool radius compensation, in which the programmed path is represented by a solid line and the compensated path with a dotted line.
End of compensation without programming a movement
After cancelling the compensation, it could happen that the plane axes do not get involved in the first motion block either because they have not been programmed or because the same point as the tool position has been programmed or because a null incremental move has been programmed.
In this case, the compensation is canceled in the current tool position; depending on the last movement executed in the plane, the tool moves to the end point without compensating the programmed path.

TOOL COMPENSATION Tool radius compensation (G40, G41, G42)

Y
X
· · · G90 G01 X-30 G01 G40 X-30 G01 X25 Y-25 · · ·

(X0 Y0)

(X0 Y0)
Y
X
· · · G90 G03 X-20 Y-20 I0 J-20 G91 G40 Y0 G01 X-20 · · ·

CNC 8040
·M· MODEL (SOFT V11.1X)
103

Programming manual

STRAIGHT-STRAIGHT path

TOOL COMPENSATION Tool radius compensation (G40, G41, G42)

CNC 8040
·M· MODEL (SOFT V11.1X)
104

CURVED-STRAIGHT path

Programming manual
8.

TOOL COMPENSATION Tool radius compensation (G40, G41, G42)

CNC 8040
·M· MODEL (SOFT V11.1X)
105

Programming manual

Example of machining with radius compensation

TOOL COMPENSATION Tool radius compensation (G40, G41, G42)

The programmed path is represented by a solid line and the compensated path by a dotted line.

Tool radius

10mm

Tool number

Tool offset number

; Preset G92 X0 Y0 Z0
; Tool, offset and spindle start at S100 G90 G17 S100 T1 D1 M03
; Begins compensation G41 G01 X40 Y30 F125Y70 X90 Y30 X40
; Cancels compensation G40 G00 X0 Y0 M30

CNC 8040
·M· MODEL (SOFT V11.1X)
106

Example of machining with radius compensation

Programming manual

TOOL COMPENSATION Tool radius compensation (G40, G41, G42)

The programmed path is represented by a solid line and the compensated path by a dotted line.

Tool radius

10mm

Tool number

Tool offset number

; Preset G92 X0 Y0 Z0
; Tool, offset and spindle start at S100 G90 G17 F150 S100 T1 D1 M03
; Begins compensation G42 G01 X30 Y30 X50 Y60 X80 X100 Y40 X140 X120 Y70 X30 Y30
; Cancels compensation G40 G00 X0 Y0 M30

CNC 8040

·M· MODEL (SOFT V11.1X)

107

Programming manual

Example of machining with radius compensation

8.
CNC 8040
·M· MODEL (SOFT V11.1X)
108

TOOL COMPENSATION Tool radius compensation (G40, G41, G42)

The programmed path is represented by a solid line and the compensated path by a dotted line.

Tool radius

10mm

Tool number

Tool offset number

; Preset G92 X0 Y0 Z0
; Tool, offset and spindle start at S100 G90 G17 F150 S100 T1 D1 M03
; Begins compensation G42 G01 X20 Y20 X50 Y30 X70 G03 X85Y45 I0 J15 G02 X100 Y60 I15 J0 G01 Y70 X55 G02 X25 Y70 I-15 J0 G01 X20 Y20
; Cancels compensation G40 G00 X0 Y0 M5 M30

Programming manual
8.1.4 Change of type of tool radius compensation while machining

The compensation may be changed from G41 to G42 or vice versa without having to cancel it with G40. It may be changed in any motion block and even in a motionless one, i.e. without moving the axes of the plane or by programming the same point twice.
It compensates independently the last movement before the change and the first one after the change. To change the type of compensation, the different cases are solved according to these criteria:
A. The compensated paths cut each other.
The programmed paths are compensated each on its corresponding side. The change of sides takes place at the intersection point of both paths.
B. The compensated paths do not cut each other.
An additional section is inserted between the two paths. From the point perpendicular to the first path at the end point up to the point perpendicular to the second path at the starting point. Both points are located at a distance R from the programmed path.
Here is a summary of the different cases:

Straight - straight path:

TOOL COMPENSATION Tool radius compensation (G40, G41, G42)

A
Straight - arc path:
A
Arc - straight path:
A
Arc - arc path:
A

B B B
B

CNC 8040
·M· MODEL (SOFT V11.1X)
109

Programming manual
8.2 Tool length compensation (G43, G44, G15)

8.
CNC 8040

TOOL COMPENSATION Tool length compensation (G43, G44, G15)

With this function it is possible to compensate possible differences in length between the programmed tool and the tool being used.
The tool length compensation is applied on to the axis indicated by function G15 or, in its absence, to the axis perpendicular to the main plane.
If G17, tool length compensation on the Z axis. If G18, tool length compensation on the Y axis If G19, tool length compensation on the X axis.
Whenever one of functions G17, G18 or G19 is programmed, the CNC assumes as new longitudinal axis (upon which tool length compensation will be applied) the one perpendicular to the selected plane.
On the other hand, if function G15 is executed while functions G17, G18 or G19 are active, the new longitudinal axis (selected with G15) will replace the previous one.
The function codes used in length compensation are as follows: G43: Tool length compensation. G44: Cancellation of tool length compensation.
Function G43 only indicates that a longitudinal compensation is to be applied. The CNC starts applying it when the longitudinal (perpendicular) axis starts moving.
; Preset G92 X0 Y0 Z50
; Tool, offset ... G90 G17 F150 S100 T1 D1 M03
; Selects compensation G43 G01 X20 Y20 X70
; Begins compensation Z30
When G43 is programmed, the CNC compensates the length in accordance with the value of the tool offset selected with code D, or (in its absence) the tool offset shown in the tool table for the selected tool (T).
Tool values R, L, I, K should be stored in the tool offset table before starting machining, or should be loaded at the beginning of the program via assignments to variables TOR, TOL, TOI, TOK.
If no tool offset is selected, the CNC takes D0 with R0 L0 I0 K0.
Function G43 is modal and can be canceled via G44 and G74 (home search). If general machine parameter "ILCOMP=0", it is also canceled on power-up, after executing M02, M30 or after EMERGENCY or RESET.
G53 (programming with respect to machine zero) temporarily cancels G43 only while executing a block which contains a G53.
Length compensation can be used together with canned cycles, although here care should be taken to apply this compensation before starting the cycle.

·M· MODEL (SOFT V11.1X)

110

Example of machining with tool length compensation

Programming manual

TOOL COMPENSATION Tool length compensation (G43, G44, G15)

It is assumed that the tool used is 4 mm shorter than the programmed one.

Tool length

-4mm

Tool number

Tool offset number

; Preset G92 X0 Y0 Z0
; Tool, offset ... G91 G00 G05 X50 Y35 S500 M03
; Begins compensation G43 Z-25 T1 D1 G01 G07 Z-12 F100 G00 Z12 X40 G01 Z-17
; Cancels compensation G00 G05 G44 Z42 M5 G90 G07 X0 Y0 M30

CNC 8040
·M· MODEL (SOFT V11.1X)
111

Programming manual
8.3 Collision detection (G41 N, G42 N)

Using this option, the CNC analyzes in advance the blocks to be executed in order to detect loops (profile intersections with itself) or collisions of the programmed profile. The number of blocks to be analyzed (up to 50) may be defined by the user.
The example shows machining errors (E) due to a collision in the programmed profile. This type of errors may be avoided using collision detection.

TOOL COMPENSATION Collision detection (G41 N, G42 N)

CNC 8040
·M· MODEL (SOFT V11.1X)
112

When detecting a loop or a collision, the blocks that caused it will not be executed and a warning will be issued for each loop or collision eliminated.
Possible cases: a step on a straight path, a step in a circular path and tool radius compensation too large.
The information contained in the eliminated blocks, not being the moving in the active plane, will be executed (including the movements of the axes).
Block detection is defined and activated with tool radius compensation functions G41 and G42. A new parameter N (G41 N y G42 N) has been added to activate the feature and define the number of blocks to analyze.
Possible values from N3 to N50. Without "N", or with N0, N1 and N2 , it behaves like in older versions.
In CAD generated programs that are made up of lots of very short blocks, it is recommended to use very low N values (around 5) so as not to jeopardize block processing time.
When this function is active, the history of active G functions shows G41 N or G42 N.

CANNED CYCLES

These canned cycles can be performed on any plane, the depth being along the axis selected as longitudinal via function G15 or, in its absence, along the axis perpendicular to this plane.

The CNC offers the following machining canned cycles :

G69

Complex deep hole drilling

G81

Drilling canned cycle.

G82

Drilling cycle with dwell.

G83

Deep hole drilling canned cycle with constant peck (drilling step).

G84

Tapping canned cycle.

G85

Reaming canned cycle.

G86

Boring cycle with withdrawal in G00

G87

Rectangular pocket canned cycle.

G88

Circular pocket canned cycle.

G89

Boring cycle with withdrawal in G01

It also offers the following functions that can be used with the machining canned cycles:

G79

Modification of the canned cycle parameters

G98

Return to the starting plane at the end of the canned cycle

G99

Return to the reference plane at the end of the canned cycle.

CNC 8040
·M· MODEL (SOFT V11.1X)
113

Programming manual
9.1 Canned cycle definition

A canned cycle is defined by the G function indicating the canned cycle and its corresponding parameters.
A canned cycle cannot be defined in a block which has nonlinear movements (G02, G03, G08, G09, G33 or G34).
Also, a canned cycle cannot be executed while function G02, G03, G33 or G34 is active. The CNC will issue the corresponding error message.
However, once a canned cycle has been defined in a block and following blocks, functions G02, G03, G08 or G09 can be programmed.

CANNED CYCLES Canned cycle definition

CNC 8040
·M· MODEL (SOFT V11.1X)
114

9.2 Influence zone of a canned cycle

Programming manual

Once a canned cycle has been defined it remains active, and all blocks programmed after this block are under its influence while it is not cancelled.

In other words, every time a block is executed in which some axis movement has been programmed, the CNC will carry out (following the programmed movement) the machining operation which corresponds to the active canned cycle.

If, in a movement block within the area of influence of a canned cycle, the number of times a block is executed (repetitions) "N" is programmed at the end of the block, the CNC repeats the programmed positioning and the machining operation corresponding to the canned cycle the indicated number of times.

If a number of repetitions (times) "N0" is programmed, the machining operation corresponding to the canned cycle will not be performed. The CNC will only carry out the programmed movement.

If, within the area of influence of a canned cycle, there is a block which does not contain any movement, the machining operation corresponding to the defined canned cycle will not be performed, except in the calling block.

G81... G90 G1 X100 G91 X10 N3
G91 X20 N0

Definition and execution of the canned cycle (drilling).
The X axis moves to X100, where the hole is to be drilled.
The CNC runs the following operation 3 times. · Incremental move to X10. · Runs the cycle defined above.
Incremental move only to X20 (no drilling).

CANNED CYCLES Influence zone of a canned cycle

CNC 8040
·M· MODEL (SOFT V11.1X)
115

Programming manual
9.2.1 G79. Modification of the canned cycle parameters

The CNC allows one or several parameters of an active canned cycle to be modified by programming the G79 function, without any need for redefining the canned cycle.
The CNC will continue to maintain the canned cycle active and will perform the following machinings of the canned cycle with the updated parameters.
The G79 function must be programmed alone in a block, and this block must not contain any more information.
Next 2 programming examples are shown assuming that the work plane is formed by the X and Y axes, and that the longitudinal axis (perpendicular) is the Z axis:

CANNED CYCLES Influence zone of a canned cycle

CNC 8040
·M· MODEL (SOFT V11.1X)
116

T1 M6 ; Starting point. G00 G90 X0 Y0 Z60 ; Defines drilling cycle. Drills in A. G81 G99 G91 X15 Y25 Z-28 I-14 ; Drills in B. G98 G90 X25 ; Modifies reference plane and machining depth. G79 Z52 ; Drills in C. G99 X35 ; Drills in D. G98 X45 ; Modifies reference plane and machining depth. G79 Z32 ; Drills in E. G99 X55 ; Drills in F. G98 X65 M30

T1 M6
; Starting point. G00 G90 X0 Y0 Z60
; Defines drilling cycle. Drills in A. G81 G99 X15 Y25 Z32 I18
; Drills in B. G98 X25
; Modifies reference plane. G79 Z52
; Drills in C. G99 X35
; Drills in D. G98 X45
; Modifies reference plane. G79 Z32
; Drills in E. G99 X55
; Drills in F. G98 X65 M30

Programming manual
9.
CNC 8040
·M· MODEL (SOFT V11.1X)
117

CANNED CYCLES Influence zone of a canned cycle

Programming manual
9.3 Canned cycle cancellation

A canned cycle can be cancelled via : · Function G80, which can be programmed in any block. · After defining a new canned cycle. This will cancel and replace any other that may be active. · After executing M02, M30, or after EMERGENCY or RESET. · When searching home with function G74. · Selecting a new work plane via functions G16, G17, G18, or G19.

CANNED CYCLES Canned cycle cancellation

CNC 8040
·M· MODEL (SOFT V11.1X)
118

9.4 General considerations

Programming manual

· A canned cycle may be defined anywhere in the program, that is, in the main program as well as in a subroutine.
· Calls to subroutines can be made from a block within the influence of a canned cycle without implying the cancellation of the canned cycle.
· The execution of a canned cycle will not alter the history of previous "G" functions.
· Nor will the spindle turning direction be altered. A canned cycle can be entered with any turning direction (M03 or M04), leaving in the same direction in which the cycle was entered.
Should a canned cycle be entered with the spindle stopped, it will start in a clockwise direction (M03), and maintain the same turning direction until the cycle is completed.
· Should it be required to apply a scaling factor when working with canned cycles, it is advisable that this scale factor be common to all the axes involved.
· The execution of a canned cycle cancels radius compensation (G41 and G42). It is equivalent to G40.
· If tool length compensation (G43) is to be used, this function must be programmed in the same block or in the one before the definition of the canned cycle.
The CNC applies the tool length compensation when the longitudinal (perpendicular) axis starts moving. Therefore, it is recommended to position the tool outside the canned cycle area when defining function G43 for the canned cycle.
· The execution of any canned cycle will alter the global parameter P299.

CANNED CYCLES General considerations

CNC 8040
·M· MODEL (SOFT V11.1X)
119

Programming manual
9.5 Machining canned cycles

9.
CNC 8040

CANNED CYCLES Machining canned cycles

In all machining cycles there are three coordinates along the longitudinal axis to the work plane which, due to their importance, are discussed below:
· Initial plane coordinate. This coordinate is given by the position which the tool occupies with respect to machine zero when the cycle is activated.
· Coordinate of the reference plane. This is programmed in the cycle definition block and represents an approach coordinate to the part. It can be programmed in absolute coordinates or in incremental, in which case it will be referred to the initial plane.
· Machining depth coordinate. This is programmed in the cycle definition block. It can be programmed in absolute coordinates or in incremental coordinates, in which case it will be referred to the reference plane.

There are two functions which allow to select the type of withdrawal of the longitudinal axis after machining.
· G98: G98 Selects the withdrawal of the tool as far as the initial plane, once the indicated machining has been done.
· G99: G98 Selects the withdrawal of the tool as far as the reference plane, once the indicated machining has been done.

These functions can be used both in the cycle definition block and the blocks which are under the influence of the canned cycle. The initial plane will always be the coordinate which the longitudinal axis had when the cycle was defined.

The structure of a canned cycle definition block is as follows:

G** Machining point

Parameters

F S T D M N****

It is possible to program the starting point in the canned cycle definition block (except the longitudinal axis), both in polar coordinates and in Cartesian coordinates.
After defining the point at which it is required to carry out the canned cycle (optional), the functions and parameters corresponding to the canned cycle will be defined, and afterwards, if required, the complementary functions F S T D M are programmed.
When programming, at the end of the block, the number of times a block is to be executed "N", the CNC performs the programmed move and the machining operation corresponding to the active canned cycle the indicated number of times.
If "N0" is programmed, it will not execute the machining operation corresponding to the canned cycle. The CNC will only carry out the programmed movement.
The general operation for all the cycles is as follows: 1. If the spindle was previously running, it maintains the turning direction. If it was
not in movement, it will start by turning clockwise (M03). 2. Positioning (if programmed) at the starting point for the programmed cycle. 3. Rapid movement of the longitudinal axis from the initial plane to the reference
plane. 4. Execution of the programmed machining cycle. 5. Rapid withdrawal of the longitudinal axis to the initial plane or reference plane,
depending on whether G98 or G99 has been programmed. The explanation of each cycle assumes that the work plane is formed by the X and Y axes, and that the longitudinal axis (perpendicular) is the Z axis:

·M· MODEL (SOFT V11.1X)

Programming in other planes
The programming format is always the same, it does not depend on the work plane. Parameters XY indicate the coordinate in the work plane ( X = abscissa, Y = ordinate) and the penetration takes place along the longitudinal axis.
The following examples show how to drill in X and Y in both directions.

120

Programming manual

Function G81 defines the drilling canned cycle. It is defined with parameters:

Coordinate of the point to be machined along the abscissa axis.

Coordinate of the point to be machined along the ordinate axis.

Drilling depth.

Dwell at the bottom.

In the following examples, the part surface has a 0 coordinate, the holes are 8 mm deep and the reference coordinate is 2 mm above the surface.

Example 1:

G19 G1 X25 F1000 S1000 M3 G81 X30 Y20 Z2 I-8 K1

CANNED CYCLES Machining canned cycles

Example 2:

G19 G1 X-25 F1000 S1000 M3 G81 X25 Y15 Z-2 I8 K1

CNC 8040
·M· MODEL (SOFT V11.1X)
121

CANNED CYCLES Machining canned cycles

Programming manual

Example 3:

9.
Example 4:

G18 G1 Y25 F1000 S1000 M3 G81 X30 Y10 Z2 I-8 K1
G18 G1 Y-25 F1000 S1000 M3 G81 X15 Y60 Z-2 I8 K1

CNC 8040
·M· MODEL (SOFT V11.1X)
122

9.6 G69. Drilling canned cycle with variable peck

Programming manual

This cycle makes successive drilling steps until the final coordinate is reached. The tool withdraws a fixed amount after each drilling operation, it being possible to select that every J drillings it withdraws to the reference plane. A dwell can also be programmed after every drilling.
Working in Cartesian coordinates, the basic structure of the block is as follows:
G69 G98/G99 X Y Z I B C D H J K L R

CANNED CYCLES G69. Drilling canned cycle with variable peck

[ G98/G99 ] Withdrawal plane

G98

The tool withdraws to the Initial Plane, once the hole has been drilled.

G99

The tool withdraws to the Reference Plane, once the hole has been

drilled.

[ X/Y±5.5 ] Machining coordinates
These are optional and define the movement of the axes of the main plane to position the tool at the machining point.
This point can be programmed in Cartesian coordinates or in polar coordinates, and the coordinates may be absolute or incremental, according to whether the machine is operating in G90 or G91.

[ Z±5.5 ]

Reference plane
Defines the reference plane coordinate. It can be programmed in absolute coordinates or incremental coordinates, in which case it will be referred to the initial plane.
If not programmed, it assumes as reference plane the current position of the tool.

[ I±5.5 ]

Drilling depth.
Defines the total drilling depth. It can be programmed in absolute coordinates or incremental coordinates and in this case will be referred to the part surface.

[ B5.5 ]

Drilling peck (step) Defines the drilling step in the axis longitudinal to the main plane.

CNC 8040
·M· MODEL (SOFT V11.1X)

123

Programming manual

[ C5.5 ]

Approach to the previous drilling
Defines the approach distance the longitudinal axis will move in rapid (G00) from the previous drilling step to start the next drilling step.
If not programmed, a value of 1 mm is assumed. If programmed with a 0 value, the CNC will display the corresponding error message.

[ D5.5 ]

Reference plane
Defines the distance between the reference plane and the surface of the part where the drilling is to be done.
In the first drilling, this amount will be added to "B" drilling step. If not programmed, a value of 0 is assumed.

CANNED CYCLES G69. Drilling canned cycle with variable peck

[ H±5.5 ]

Withdrawal after drilling
Distance or coordinate the longitudinal axis returns to, in rapid (G00), after each drilling step.
"J" other than 0 means the distance and "J=0" indicates the relief coordinate or absolute coordinate it withdraws to.
If not programmed, the longitudinal axis returns to the reference plane.

[ J4 ]

Drilling passes to withdraw to the starting plane
Defines after how many drilling pecks the tool returns to the reference plane in G00. A value between 0 and 9999 may be programmed.
When not programmed or programmed with a "0" value, it returns to the position indicated by H (relief position) after each drilling peck.

CNC 8040
·M· MODEL (SOFT V11.1X)

[ K5 ]

· With "J" greater than 1, after each peck, the tool returns the distance indicated by "H" and every "J" pecks to the reference plane (RP).
· With J1, it will return to the reference plane (RP) after each peck . · With J0, it will return to the relief position indicated by H.
Dwell
Defines the dwell, in hundredths of a second, after each drilling peck until the withdrawal begins. If not programmed, the CNC will take the value of "K0".

124

[ L5.5 ] [ R5.5 ]

Programming manual

Minimum drilling peck (step).
It defines the minimum value for the drilling peck. This parameter is used with "R" values other than 1. If not programmed or programmed with a 0 value, it assumes the value of 1 mm.

Reduction factor for the drilling pecks.
Factor that reduces the drilling peck (step) "B". If it is not programmed or is programmed with a value of "0", it assumes a value of "1".
If R =1, all the drilling pecks will be the same (the programmed "B" value).
If R is other than 1, the first drilling peck will be "B", the second one "R B", The third one "R (RB)" and so on. In other words, from the second peck on, the new peck will be the product of the R factor times the previous peck.
If R is selected with a value other than 1, the CNC will not allow smaller steps than that programmed in L.

CANNED CYCLES G69. Drilling canned cycle with variable peck

CNC 8040
·M· MODEL (SOFT V11.1X)
125

Programming manual
9.6.1 Basic operation
1. If the spindle was previously running, it maintains the turning direction. If it was not in movement, it will start by turning clockwise (M03).
2. Rapid movement of the longitudinal axis from the initial plane to the reference plane.
9.

CANNED CYCLES G69. Drilling canned cycle with variable peck

CNC 8040
·M· MODEL (SOFT V11.1X)
126

3. First drilling operation. The drilling axis moves in G01 to the programmed incremental depth "B + D".
This movement will be carried out either in G07 or G50 depending on the value assigned to the longitudinal axis "INPOSW2(P51)"
· If P51=0, in G7 (square corner)
· If P51=1, in G50 (controlled round corner).
4. Drilling loop. The following steps will be repeated until the programmed machining depth "I" is reached.
·1· Dwell K, in hundredths of a second, if it has been programmed.
·2· Withdrawal of the longitudinal axis in rapid (G00) as far as the reference plane, if the number of drillings programmed in J were made, otherwise it withdraws the distance programmed in "H".
·3· Rapid approach (G00) of the longitudinal axis to a "C" distance from the next peck.

Programming manual

·4· New drilling step. G1 move of the longitudinal axis to the next incremental depth "B and R". This movement will be carried out either in G07 or G50 depending on the value assigned to the longitudinal axis "INPOSW2(P51)" If P51=0, in G7 (square corner). If P51=1, in G50 (controlled round corner).
5. Dwell K, in hundredths of a second, if it has been programmed. 6. Withdrawal at rapid feedrate (G00) of the longitudinal axis to the initial or
reference plane, depending on whether G98 or G99 has been programmed.
If a scaling factor is applied to this cycle, it should be borne in mind that this scaling factor will only affect the reference plane coordinates and drilling depth.

Therefore, and due to the fact that parameter "D" is not affected by the scaling factor, the surface coordinate of the part will not be proportional to the programmed cycle.

CANNED CYCLES G69. Drilling canned cycle with variable peck

Programming example assuming that the work plane is formed by the X and Y axes, that the Z axis is the longitudinal axis and that the starting point is X0 Y0 Z0:
; Tool selection. T1 M6
; Starting point. G0 G90 X0 Y0 Z0
; Canned cycle definition. G69 G98 G91 X100 Y25 Z-98 I-52 B12 C2 D2 H5 J2 K150 L3 R0.8 F100 S500 M8
; Cancels the canned cycle. G80
; Positioning. G90 X0 Y0
; End of program. M30

CNC 8040
·M· MODEL (SOFT V11.1X)
127

Programming manual
9.7 G81. Drilling canned cycle

This cycle drills at the point indicated until the final programmed coordinate is reached. It is possible to program a dwell at the bottom of the drill hole.
Working in Cartesian coordinates, the basic structure of the block is as follows: G81 G98/G99 X Y Z I K

CANNED CYCLES G81. Drilling canned cycle

CNC 8040
·M· MODEL (SOFT V11.1X)

[ G98/G99 ] Withdrawal plane

G98

The tool withdraws to the Initial Plane, once the hole has been drilled.

G99

The tool withdraws to the Reference Plane, once the hole has been

drilled.

[ Z±5.5 ]

[ I±5.5 ]

Drilling depth.
Defines the total drilling depth. It can be programmed in absolute coordinates or incremental coordinates and in this case will be referred to the reference plane.

[ K5 ]

Dwell
Defines the dwell, in hundredths of a second, after each drilling peck until the withdrawal begins. If not programmed, the CNC will take the value of "K0".

128

9.7.1 Basic operation

Programming manual

CANNED CYCLES G81. Drilling canned cycle

; Tool selection. T1 M6
; Starting point. G0 G90 X0 Y0 Z0
; Canned cycle definition. G81 G98 G00 G91 X250 Y350 Z-98 I-22 F100 S500
; Polar coordinate origin. G93 I250 J250
; Turn and canned cycle, 3 times Q-45 N3
; Cancels the canned cycle. G80
; Positioning. G90 X0 Y0
; End of program. M30

CNC 8040
·M· MODEL (SOFT V11.1X)
129

Programming manual
9.8 G82. Drilling cycle with dwell

This cycle drills at the point indicated until the final programmed coordinate is reached. Then it executes a dwell at the bottom of the drill hole.
Working in Cartesian coordinates, the basic structure of the block is as follows: G82 G98/G99 X Y Z I K

CANNED CYCLES G82. Drilling cycle with dwell

CNC 8040
·M· MODEL (SOFT V11.1X)

[ G98/G99 ] Withdrawal plane

G98

The tool withdraws to the Initial Plane, once the hole has been drilled.

G99

The tool withdraws to the Reference Plane, once the hole has been

drilled.

[ Z±5.5 ]

[ I±5.5 ]

Drilling depth.
Defines the total drilling depth. It can be programmed in absolute coordinates or incremental coordinates and in this case will be referred to the reference plane.

[ K5 ]

Dwell
Defines the dwell, in hundredths of a second, after each drilling until the withdrawal begins. Should this not be programmed, the CNC will take a value of K0.

130

9.8.1 Basic operation

Programming manual

CANNED CYCLES G82. Drilling cycle with dwell

; Tool selection. T1 M6
; Starting point. G0 G90 X0 Y0 Z0
; Canned cycle definition. Three machining operations are carried out. G82 G99 G91 X50 Y50 Z-98 I-22 K15 F100 S500 N3
; Positioning and canned cycle G98 G90 G00 X500 Y500
; Cancels the canned cycle. G80
; Positioning. G90 X0 Y0
; End of program. M30

CNC 8040
·M· MODEL (SOFT V11.1X)
131

Programming manual
9.9 G83. Deep-hole drilling canned cycle with constant peck

This cycle makes successive drilling steps until the final coordinate is reached. The tool withdraws as far as the reference plane after each drilling step. Working in Cartesian coordinates, the basic structure of the block is as follows:
G83 G98/G99 X Y Z I J

CANNED CYCLES G83. Deep-hole drilling canned cycle with constant peck

CNC 8040

[ G98/G99 ] Withdrawal plane

G98

The tool withdraws to the Initial Plane, once the hole has been drilled.

G99

The tool withdraws to the Reference Plane, once the hole has been

drilled.

[ Z±5.5 ]

[ I±5.5 ]

Depth of each drilling peck
Defines the value of each drilling step according to the axis longitudinal to the main plane.

·M· MODEL (SOFT V11.1X)

132

[ J4 ]

Programming manual
Drilling passes to withdraw to the starting plane
Defines the number of steps which the drill is to make. A value between 1 and 9999 may be programmed.

CANNED CYCLES G83. Deep-hole drilling canned cycle with constant peck

CNC 8040
·M· MODEL (SOFT V11.1X)
133

Programming manual
9.9.1 Basic operation

CANNED CYCLES G83. Deep-hole drilling canned cycle with constant peck

1. If the spindle was previously running, it maintains the turning direction. If it was not in movement, it will start by turning clockwise (M03).
2. Rapid movement of the longitudinal axis from the initial plane to the reference plane.
3. First drilling operation. The longitudinal axis moves in G01 to the programmed incremental depth "I". This movement will be carried out either in G07 or G50 depending on the value assigned to the longitudinal axis "INPOSW2(P51)" If P51=0, in G7 (square corner) Otherwise, in G50 (controlled round corner).
4. Drilling loop. The following steps will be repeated "J-1" times as in the previous step the first programmed drilling was done. ·1· Withdrawal of the longitudinal axis in rapid (G00) to the reference plane. ·2· Longitudinal axis approach in rapid (G00): If INPOSW2=0 up to 1mm from the previous drilling peck. Otherwise, up to "INPOSW2 +0.02 MM of the previous drilling peck. ·3· New drilling step. G01 movement of the longitudinal axis to the incremental depth programmed in "I". If INPOSW2=0 in G7. If not, in G50.
5. Withdrawal at rapid feedrate (G00) of the longitudinal axis to the initial or reference plane, depending on whether G98 or G99 has been programmed.
If a scaling factor is applied to this cycle, drilling will be performed proportional to that programmed, with the same step "I" programmed, but varying the number of steps "J".
Programming example assuming that the work plane is formed by the X and Y axes, that the Z axis is the longitudinal axis and that the starting point is X0 Y0 Z0:

CNC 8040
·M· MODEL (SOFT V11.1X)
134

; Tool selection. T1 M6
; Starting point. G0 G90 X0 Y0 Z0
; Canned cycle definition. G83 G99 X50 Y50 Z-98 I-22 J3 F100 S500 M4
; Positioning and canned cycle G98 G90 G00 X500 Y500
; Cancels the canned cycle. G80
; Positioning. G90 X0 Y0
; End of program. M30

Programming manual
9.

CANNED CYCLES G83. Deep-hole drilling canned cycle with constant peck

CNC 8040
·M· MODEL (SOFT V11.1X)
135

Programming manual
9.10 G84. Tapping canned cycle

This cycle taps at the point indicated until the final programmed coordinate is reached. General logic output "TAPPING" (M5517) stays active while executing this cycle.
Due to the fact that the tapping tool turns in two directions (one when tapping and the other when withdrawing from the thread), by means of the machine parameter of the spindle "SREVM05" it is possible to select whether the change in turning direction is made with the intermediate spindle stop, or directly.
General machine parameter "STOPAP(P116)" indicates whether general inputs / STOP, /FEEDHOL and /XFERINH are enabled or not while executing function G84.
It is possible to program a dwell before each reversal of the spindle turning direction, i.e., at the bottom of the thread hole and when returning to the reference plane.
Working in Cartesian coordinates, the basic structure of the block is as follows: G84 G98/G99 X Y Z I K R J

CANNED CYCLES G84. Tapping canned cycle

CNC 8040
·M· MODEL (SOFT V11.1X)

[ G98/G99 ] Withdrawal plane

G98

The tool withdraws to the Initial Plane, once the hole has tapped.

G99

The tool withdraws to the Reference Plane, once the hole has tapped.

[ Z±5.5 ]

136

[ I±5.5 ] [ K5 ] [ R ] [ J5.5 ]

Programming manual

Thread depth.
Defines tapping depth. It can be programmed in absolute coordinates or incremental coordinates and in this case will be referred to the reference plane.

Dwell Defines the dwell, in hundredths of a second, after the tapping until the withdrawal begins. If not programmed, the CNC will take the value of "K0".
Type of tapping Defines the type of tapping cycle to be performed: normal if "R0" and rigid if "R1".

CANNED CYCLES G84. Tapping canned cycle

Withdrawal feedrate factor
When rigid tapping, the returning feedrate will be J times the tapping feedrate. When not programmed or programmed J1, they will both be the same.
In order to execute a rigid tapping, the spindle must be ready to operate in closed loop; in other words, that it must have a servo drive-motor system with rotary encoder.
When rigid tapping, the CNC interpolates the movement of the longitudinal axis with the spindle rotation.

CNC 8040
·M· MODEL (SOFT V11.1X)
137

Programming manual
9.10.1 Basic operation

CANNED CYCLES G84. Tapping canned cycle

1. If the spindle was previously running, it maintains the turning direction. If it was not in movement, it will start by turning clockwise (M03).
2. Rapid movement of the longitudinal axis from the initial plane to the reference plane.
3. Movement of the longitudinal axis and at the working feedrate, to the bottom of the machined section, producing the threaded hole. The canned cycle will execute this movement and all later movements at 100% of F feedrate and the programmed S speed.
If rigid tapping is selected (parameter R=1), the CNC will activate the general logic output "RIGID" (M5521) to indicate to the PLC that a rigid tapping block is being executed.
4. Spindle stop (M05). This will only be performed when the spindle machine parameter "SREVM05" is selected and parameter "K" has a value other than "0"..
5. Dwell, if parameter "K" has been programmed.
6. Reverse the spindle turning direction.
7. Withdrawal, at J times the working feedrate, of the longitudinal axis to the reference plane. Once this coordinate has been reached, the canned cycle will assume the selected FEEDRATE OVERRIDE and the SPINDLE OVERRIDE.
If rigid tapping is selected (parameter R=1), the CNC will activate the general logic output "RIGID" (M5521) to indicate to the PLC that a rigid tapping block is being executed.
8. Spindle stop (M05). This will only be performed if the spindle machine parameter "SREVM05" is selected.
9. Dwell, if parameter "K" has been programmed.
10.Reverse the spindle turning direction restoring the initial turning direction.
11.Withdrawal, at rapid feedrate (G00), of the longitudinal axis as far as the initial plane if G98 has been programmed.
Programming example assuming that the work plane is formed by the X and Y axes, that the Z axis is the longitudinal axis and that the starting point is X0 Y0 Z0:

CNC 8040
·M· MODEL (SOFT V11.1X)
138

Programming manual

; Tool selection. T1 M6
; Starting point. G0 G90 X0 Y0 Z0
; Canned cycle definition. Three machining operations are carried out. G84 G99 G91 X50 Y50 Z-98 I-22 K150 F350 S500 N3
; Positioning and canned cycle G98 G90 G00 X500 Y500
; Cancels the canned cycle. G80
; Positioning. G90 X0 Y0
; End of program. M30

CANNED CYCLES G84. Tapping canned cycle

CNC 8040
·M· MODEL (SOFT V11.1X)
139

Programming manual
9.11 G85. Reaming canned cycle

This cycle reams at the point indicated until the final programmed coordinate is reached.
It is possible to program a dwell at the bottom of the machined hole.
Working in Cartesian coordinates, the basic structure of the block is as follows: G85 G98/G99 X Y Z I K

CANNED CYCLES G85. Reaming canned cycle

CNC 8040
·M· MODEL (SOFT V11.1X)

[ G98/G99 ] Withdrawal plane

G98

The tool withdraws to the Initial Plane, once the hole has been reamed.

G99

The tool withdraws to the Reference Plane, once the hole has been

reamed.

[ Z±5.5 ]

[ I±5.5 ]

Reaming depth.
Defines reaming depth. It can be programmed in absolute coordinates or incremental coordinates and in this case will be referred to the reference plane.

[ K5 ]

Dwell
Defines the dwell, in hundredths of a second, after the reaming until the withdrawal begins. If not programmed, the CNC will take the value of "K0".

140

9.11.1 Basic operation

Programming manual

CANNED CYCLES G85. Reaming canned cycle

; Tool selection. T1 M6
; Starting point. G0 G90 X0 Y0 Z0
; Canned cycle definition. G85 G98 G91 X250 Y350 Z-98 I-22 F100 S500
; Cancels the canned cycle. G80
; Positioning. G90 X0 Y0
; End of program. M30

CNC 8040
·M· MODEL (SOFT V11.1X)
141

Programming manual
9.12 G86. Boring cycle with withdrawal in G00

This cycle bores at the point indicated until the final programmed coordinate is reached.
It is possible to program a dwell at the bottom of the machined hole.
Working in Cartesian coordinates, the basic structure of the block is as follows: G86 G98/G99 X Y Z I K

CANNED CYCLES G86. Boring cycle with withdrawal in G00

CNC 8040
·M· MODEL (SOFT V11.1X)

[ G98/G99 ] Withdrawal plane

G98

The tool withdraws to the Initial Plane, once the hole has been bored.

G99

The tool withdraws to the Reference Plane, once the hole has been

bored.

[ Z±5.5 ]

[ I±5.5 ]

Reaming depth.
Defines boring depth. It can be programmed in absolute coordinates or incremental coordinates and in this case will be referred to the reference plane.

[ K5 ]

Dwell
Defines the dwell, in hundredths of a second, after boring until the withdrawal begins. If not programmed, the CNC will take the value of "K0".

142

9.12.1 Basic operation

Programming manual

CANNED CYCLES G86. Boring cycle with withdrawal in G00

; Tool selection. T1 M6
; Starting point. G0 G90 X0 Y0 Z0
; Canned cycle definition. G86 G98 G91 X250 Y350 Z-98 I-22 K20 F100 S500
; Cancels the canned cycle. G80
; Positioning. G90 X0 Y0
; End of program. M30

CNC 8040
·M· MODEL (SOFT V11.1X)
143

Programming manual
9.13 G87. Rectangular pocket canned cycle.

This cycle executes a rectangular pocket at the point indicated until the final programmed coordinate is reached.
It is possible to program, in addition to milling pass and feedrate, a final finishing step with its corresponding milling feedrate.
In order to obtain a good finish in the machining of the pocket walls, the CNC will apply a tangential entry and exit to the last milling step during each cutting operation.
Working in Cartesian coordinates, the basic structure of the block is as follows: G87 G98/G99 X Y Z I J K B C D H L V

CANNED CYCLES G87. Rectangular pocket canned cycle.

CNC 8040
·M· MODEL (SOFT V11.1X)

[ G98/G99 ] Withdrawal plane

G98

The tool withdraws to the Initial Plane, once the pocket has been made.

G99

The tool withdraws to the Reference Plane, once the pocket has been

made.

[ Z±5.5 ]

Reference plane
Defines the reference plane coordinate.
When programmed in absolute coordinates, it will be referred to the part zero and when programmed in incremental coordinates, it will be referred to the starting plane (P.P.).
If not programmed, it assumes as reference plane the current position of the tool. Thus, the starting plane (P.P.) and the reference plane (P.R.) will be the same.

144

Programming manual

[ I±5.5 ] [ J±5.5 ]

Machining depth.
Defines the machining depth.
When programmed in absolute coordinates, it will be referred to the part zero and when programmed in incremental coordinates, it will be referred to the starting plane (P.P.).
Half the width of the pocket along the abscissa axis
Defines the distance from the center to the edge of the pocket according to the abscissa axis. The sign indicates the pocket machining direction.

CANNED CYCLES G87. Rectangular pocket canned cycle.

J with "+" sign

J with "-" sign

[ K5.5 ]

Half the width of the pocket along the ordinate axis
Defines the distance from the center to the edge of the pocket according to the ordinate axis.

[ B±5.5 ]

Penetration step
Defines the cutting depth according to the longitudinal axis.
If this is programmed with a positive sign, the entire cycle will be executed with the same machining pass, this being equal to or less than that programmed.
If programmed with a negative sign, the whole pocket is machined with the given pass (step) except the last pass that machines the rest.

CNC 8040
·M· MODEL (SOFT V11.1X)

145

Programming manual
[ C±5.5 ]
9.

Milling pass
Defines the milling pass along the main plane.
If the value is positive, the entire cycle will be executed with the same milling step, this being equal to or less than that programmed.
If the value is negative, the entire pocket will be executed with the given step, except for the last step which will machine whatever remains.

CANNED CYCLES G87. Rectangular pocket canned cycle.

[ D5.5 ]

If not programmed, it assumes a value of 3/4 of the diameter of the selected tool.
If programmed with a value greater than the tool diameter, the CNC issues the relevant error message.
If programmed with a 0 value, the CNC will display the corresponding error message.
Reference plane
Defines the distance between the reference plane and the surface of the part where the pocket is to be made.
During the first deepening operation this amount will be added to incremental depth "B". If not programmed, a value of 0 is assumed.

CNC 8040

[ H.5.5 ]

Feedrate for the finishing pass
Defines the working feedrate during the finishing pass.
If not programmed or programmed with a 0 value, it assumes the value of the machining feedrate.

·M· MODEL (SOFT V11.1X)

146

[ L±5.5 ]

Programming manual
Finishing stock. Defines the value of the finishing pass, along the main plane. If the value is positive, the finishing pass is made on a square corner (G07). If the value is negative, the finishing pass is made on a rounded corner (G05).

CANNED CYCLES G87. Rectangular pocket canned cycle.

[ V.5.5 ]

If not programmed or programmed with a 0 value, it does not run the finishing pass.
Tool penetrating feedrate. Defines the tool penetrating feedrate. If not programmed or programmed with a 0 value, it assumes 50% of the feedrate in the plane (F).

CNC 8040
·M· MODEL (SOFT V11.1X)
147

Programming manual
9.13.1 Basic operation

1. If the spindle was previously running, it maintains the turning direction. If it was not in movement, it will start by turning clockwise (M03).
2. Rapid movement (G0) of the longitudinal axis from the starting plane to the reference plane.
3. First penetrating operation. Movement of longitudinal axis at the feedrate indicated by "V" to the incremental depth programmed in "B+D".
4. Milling of the pocket surface at work feedrate in the passes defined by "C" up to a distance "L" (finishing pass) from the pocket wall.
5. Finishing pass milling, "L" at the work feedrate defined by "H".
6. Once the finishing pass has been completed, the tool withdraws at the rapid feedrate (G00) to the center of the pocket, the longitudinal axis being separated 1 mm (0.040 inch) from the machined surface.

CANNED CYCLES G87. Rectangular pocket canned cycle.

7. New milling surfaces until reaching the total depth of the pocket.
·1· Movement of the longitudinal axis at the feedrate indicated by "V", up to a distance "B" from the previous surface.
·2· Milling of the new surface following the steps indicated in points 4, 5 and 6.
8. Withdrawal at rapid feedrate (G00) of the longitudinal axis to the initial or reference plane, depending on whether G98 or G99 has been programmed.

CNC 8040
·M· MODEL (SOFT V11.1X)
148

Programming manual
Programming example ·1· Let us suppose a work plane formed by the X and Y axis, Z being the longitudinal axis and the starting point X0 Y0 Z0.
9.

CANNED CYCLES G87. Rectangular pocket canned cycle.

; Tool selection. (TOR1=6, TOI1=0) T1 D1 M6
; Starting point G0 G90 X0 Y0 Z0
; Canned cycle definition G87 G98 X90 Y60 Z-48 I-90 J52.5 K37.5 B12 C10 D2 H100 L5 V100 F300 S1000 M03
; Cancels the canned cycle G80
; Positioning G90 X0 Y0
; End of program M30

CNC 8040
·M· MODEL (SOFT V11.1X)

149

Programming manual

Programming example ·2·
Let us suppose a work plane formed by the X and Y axis, Z being the longitudinal axis and the starting point X0 Y0 Z0.

CANNED CYCLES G87. Rectangular pocket canned cycle.

CNC 8040
·M· MODEL (SOFT V11.1X)
150

; Tool selection. (TOR1=6, TOI1=0) T1 D1 M6
; Starting point G0 G90 X0 Y0 Z0
; Work plane. G18
; Canned cycle definition N10 G87 G98 X200 Y-48 Z0 I-90 J52.5 K37.5 B12 C10 D2 H100 L5 V50 F300
; Coordinate rotation N20 G73 Q45
; Repeats the select blocks 7 times. (RPT N10,N20) N7
; Cancels the canned cycle. G80
; Positioning G90 X0 Y0
; End of program M30

9.14 G88. Circular pocket canned cycle

Programming manual

This cycle executes a circular pocket at the point indicated until the final programmed coordinate is reached.
It is possible to program, in addition to milling pass and feedrate, a final finishing step with its corresponding milling feedrate.
Working in Cartesian coordinates, the basic structure of the block is as follows: G88 G98/G99 X Y Z I J B C D H L V

CANNED CYCLES G88. Circular pocket canned cycle

[ G98/G99 ] Withdrawal plane

G98

The tool withdraws to the Initial Plane, once the pocket has been made.

G99

The tool withdraws to the Reference Plane, once the pocket has been

made.

[ Z±5.5 ]

Reference plane
Defines the reference plane coordinate.
It may be programmed either in absolute or incremental coordinates, in which case it will be referred to the starting plane. If not programmed, it assumes as reference plane the current position of the tool.

[ I±5.5 ]

Machining depth.
Defines the machining depth. It may be programmed either in absolute or incremental coordinates, in which case it will be referred to the reference plane.

CNC 8040
·M· MODEL (SOFT V11.1X)

151

Programming manual
[ J±5.5 ]

Pocket radius Defines the radius of the pocket. The sign indicates the pocket machining direction.

J with "+" sign

J with "-" sign

[ B±5.5 ]

Penetration step
Defines the cutting pass along the longitudinal axis to the main plane. · If this value is positive, the entire cycle will be executed with the same machining pass, this being equal to or less than that programmed. · If the value is negative, the entire pocket will be executed with the given step, except for the last step which will machine whatever remains.

CANNED CYCLES G88. Circular pocket canned cycle

CNC 8040

[ C±5.5 ]

Milling pass
Defines the milling pass along the main plane. · If the value is positive, the entire cycle will be executed with the same milling step, this being equal to or less than that programmed. · If the value is negative, the entire pocket will be executed with the given step, except for the last step which will machine whatever remains.
If not programmed, it assumes a value of 3/4 of the diameter of the selected tool.
If programmed with a value greater than the tool diameter, the CNC issues the relevant error message.
If programmed with a 0 value, the CNC will display the corresponding error message.

·M· MODEL (SOFT V11.1X)

152

[ D5.5 ]

Programming manual
Reference plane
Defines the distance between the reference plane and the surface of the part where the pocket is to be made.
During the first deepening operation this amount will be added to incremental depth "B". If not programmed, a value of 0 is assumed.

CANNED CYCLES G88. Circular pocket canned cycle

[ H5.5 ] [ L5.5 ]

Feedrate for the finishing pass Defines the working feedrate during the finishing pass. If not programmed or programmed with a 0 value, it assumes the value of the machining feedrate.
Finishing stock Defines the value of the finishing pass, along the main plane. If not programmed or programmed with a 0 value, it does not run the finishing pass.

[ V.5.5 ]

Tool penetrating feedrate.
Defines the tool penetrating feedrate.
If not programmed or programmed with a 0 value, it assumes 50% of the feedrate in the plane (F).

CNC 8040

·M· MODEL (SOFT V11.1X)

153

CANNED CYCLES G88. Circular pocket canned cycle

Programming manual
9.
CNC 8040
·M· MODEL (SOFT V11.1X)
154

9.14.1 Basic operation

Programming manual

1. If the spindle was previously running, it maintains the turning direction.
If it was not in movement, it will start by turning clockwise (M03).
2. Rapid movement (G0) of the longitudinal axis from the starting plane to the reference plane.
3. First penetrating operation. Movement of longitudinal axis at the feedrate indicated by "V" to the incremental depth programmed in "B+D".
4. Milling of the pocket surface at work feedrate in the passes defined by "C" up to a distance "L" (finishing pass) from the pocket wall.
5. Finishing pass milling, "L" at the work feedrate defined by "H".
6. Once the finishing pass has been completed, the tool withdraws at the rapid feedrate (G00) to the center of the pocket, the longitudinal axis being separated 1 mm (0.040 inch) from the machined surface.

CANNED CYCLES G88. Circular pocket canned cycle

7. New milling surfaces until reaching the total depth of the pocket.
· Movement of the longitudinal axis at the feedrate indicated by "V", up to a distance "B" from the previous surface.
· Milling of the new surface following the steps indicated in points 4, 5 and 6.
8. Withdrawal at rapid feedrate (G00) of the longitudinal axis to the initial or reference plane, depending on whether G98 or G99 has been programmed.

CNC 8040
·M· MODEL (SOFT V11.1X)
155

Programming manual

Programming example ·1·
Let us suppose a work plane formed by the X and Y axis, Z being the longitudinal axis and the starting point X0 Y0 Z0.

CANNED CYCLES G88. Circular pocket canned cycle

CNC 8040
·M· MODEL (SOFT V11.1X)
156

; Tool selection. (TOR1=6, TOI1=0) T1 D1 M6
; Starting point G0 G90 X0 Y0 Z0
; Canned cycle definition G88 G98 G00 G90 X90 Y80 Z-48 I-90 J70 B12 C10 D2 H100 L5 V100 F300 S1000 M03
; Cancels the canned cycle. G80
; Positioning G90 X0 Y0
; End of program M30

Programming manual
9.15 G89. Boring cycle with withdrawal at work feedrate (G01)

CANNED CYCLES G89. Boring cycle with withdrawal at work feedrate (G01)

[ G98/G99 ] Withdrawal plane

G98

The tool withdraws to the Initial Plane, once the hole has been bored.

G99

The tool withdraws to the Reference Plane, once the hole has been

bored.

[ Z±5.5 ]

[ I±5.5 ]

Machining depth.
Defines boring depth. It can be programmed in absolute coordinates or incremental coordinates and in this case will be referred to the reference plane.

[ K5 ]

Dwell
Defines the dwell, in hundredths of a second, after boring until the withdrawal begins. If not programmed, the CNC will take the value of "K0".

CNC 8040
·M· MODEL (SOFT V11.1X)

157

Programming manual
9.15.1 Basic operation

CANNED CYCLES G89. Boring cycle with withdrawal at work feedrate (G01)

; Tool selection. T1 D1 M6
; Starting point G0 G90 X0 Y0 Z0
; Canned cycle definition G89 G98 G91 X250 Y350 Z-98 I-22 K20 F100 S500
; Cancels the canned cycle. G80
; Positioning G90 X0 Y0
; End of program M30

CNC 8040
·M· MODEL (SOFT V11.1X)
158

MULTIPLE MACHINING

Multiple machining is defined as a series of functions which allow a machining operation to be repeated along a given path.
The programmer will select the type of machining, which can be a canned cycle or a subroutine (which must be programmed as a modal subroutine) defined by the user.
Machining paths are defined by the following functions: G60: Multiple machining in a straight line G61: Multiple machining in a rectangular pattern. G62: Multiple machining in a grid pattern. G63: Multiple machining in a circular pattern. G64: Multiple machining in an arc G65: Machining programmed with an arc-chord
These functions can be performed on any work plane and must be defined every time they are used, as they are not modal.
It is absolutely essential for the machining which it is required to repeat to be active. In other words, these functions will only make sense if they are under the influence of a canned cycle or under the influence of a modal subroutine.
To perform multiple machining, follow these steps: 1. Move the tool to the first point of the multiple machining operation. 2. Define the canned cycle or modal subroutine to be repeated at all the points. 3. Define the multiple operation to be performed.
All machining operations programmed with these functions will be done under the same working conditions (T,D,F,S) which were selected when defining the canned cycle or modal subroutine.
Once the multiple machining operation has been performed, the program will recover the history it had before starting this machining, even when the canned cycle or modal subroutine will remain active. Now feedrate F corresponds to the feedrate programmed for the canned cycle or modal subroutine.
Likewise, the tool will be positioned at the last point where the programmed machining operation was done.
If multiple machining of a modal subroutine is performed in the Single Block mode, this subroutine will be performed complete (not block by block) after each programmed movement.
A detailed explanation is given on the next page of multiple machining operations, assuming in each case, that the work plane is formed by X and Y axes.

CNC 8040

·M· MODEL (SOFT V11.1X)

159

Programming manual
10.1 G60: Multiple machining in a straight line

10.

The programming format is as follows:

G60 A

XI PQRSTUV X K I K

MULTIPLE MACHINING G60: Multiple machining in a straight line

CNC 8040
·M· MODEL (SOFT V11.1X)

A (±5.5) X (±5.5) I (5.5) K (5)
P Q R S T U V

Angle of the path
Defines the angle that forms the machining path with the abscissa axis. It is expressed in degrees and if not programmed, the value A=0 will be taken.
Length of the path
Defines the length of the machining path.
Machining pass
Defines the pass between machining operations.
Number of machining operations
Defines the number of total machining operations in the section, including the machining definition point.
Due to the fact that machining may be defined with any two points of the X I K group, the CNC allows the following definition combinations: XI, XK, IK.
Nevertheless, if format XI is defined, care should be taken to ensure that the number of machining operations is an integer number, otherwise the CNC will show the corresponding error code.
Points where no drilling takes place
These parameters are optional and are used to indicate at which points or between which of those programmed points it is not required to machine.
Thus, programming P7 indicates that it is not required to do machining at point 7, and programming Q10.013 indicates that machining is not required from point 10 to 13, or expressed in another way, that no machining is required at points 10, 11, 12 and 13.
When it is required to define a group of points (Q10.013), care should be taken to define the final point with three digits, as if Q10.13 is programmed, multiple machining understands Q10.130.
The programming order for these parameters is P Q R S T U V, it also being necessary to maintain the order in which the points assigned to these are numbered, i.e., the numbering order of the points assigned to Q must be greater than that assigned to P and less than that assigned to R.

160

Programming manual

Example: Proper programming Correct programming

P5.006 Q12.015 R20.022 P5.006 Q12.015 R20.022

If these parameters are not programmed, the CNC understands that it must perform machining at all the points along the programmed path.

10.

MULTIPLE MACHINING G60: Multiple machining in a straight line

CNC 8040
·M· MODEL (SOFT V11.1X)
161

Programming manual
10.1.1 Basic operation

10.

1. Multiple machining calculates the next point of those programmed where it is wished to machine.
2. Rapid traverse (G00) to this point. 3. Multiple machining will perform the canned cycle or modal subroutine selected
after this movement. 4. The CNC will repeat steps 1-2-3 until the programmed path has been completed.
After completing multiple machining, the tool will be positioned at the last point along the programmed path where machining was performed.
Programming example assuming that the work plane is formed by the X and Y axes, that the Z axis is the longitudinal axis and that the starting point is X0 Y0 Z0:

MULTIPLE MACHINING G60: Multiple machining in a straight line

CNC 8040
·M· MODEL (SOFT V11.1X)
162

; Canned cycle positioning and definition. G81 G98 G00 G91 X200 Y300 Z-8 I-22 F100 S500 ; Defines multiple machining. G60 A30 X1200 I100 P2.003 Q6 R12 ; Cancels the canned cycle. G80 ; Positioning. G90 X0 Y0 ; End of program. M30
It is also possible to write the multiple machining definition block in the following ways: G60 A30 X1200 K13 P2.003 Q6 R12 G60 A30 I100 K13 P2.003 Q6 R12

Programming manual
10.2 G61: Multiple machining in a rectangular pattern

The programming format is as follows:
G61 A B X I Y J P Q R S T U V XK YD IK JD

10.

MULTIPLE MACHINING G61: Multiple machining in a rectangular pattern

A (±5.5) B (±5.5) X (5.5) I (5.5) K (5)
Y (5.5) J (5.5)

Angle of the path with respect to the abscissa axis Defines the angle that forms the machining path with the abscissa axis. It is expressed in degrees and if not programmed, the value A=0 will be taken.
Angle between paths Defines the angle formed by the two machining paths. It is expressed in degrees and if not programmed, the value B=90 will be taken.
Length of the path along the abscissa axis Defines the length of the machining path according to the abscissa axis.
Machining pass along the abscissa axis Defines the pass between machining operations along the abscissa axis.
Number of machining operations along the abscissa axis Defines the number of total machining operations in the abscissa axis, including the machining definition point. Due to the fact that machining may be defined according to the abscissa axis with any two points of the X I K group, the CNC allows the following definition combinations: XI, XK, IK. Nevertheless, if format XI is defined, care should be taken to ensure that the number of machining operations is an integer number, otherwise the CNC will show the corresponding error code.
Length of the path along the ordinate axis Defines the length of the machining path according to the ordinate axis.
Machining pass along the ordinate axis Defines the pass between machining operations according to the ordinate axis.

CNC 8040
·M· MODEL (SOFT V11.1X)

163

MULTIPLE MACHINING G61: Multiple machining in a rectangular pattern

Programming manual
D (5)

10.

P Q R S T U V

Number of machining operations along the ordinate axis

Defines the number of total machining operations in the ordinate axis, including the machining definition point.

Due to the fact that machining may be defined according to the ordinate axis with any two points of the Y J D group, the CNC allows the following definition combinations: YJ, YD, JD.
Nevertheless, if format YJ is defined, care should be taken to ensure that the number of machining operations is an integer number, otherwise the CNC will show the corresponding error code.

Points where no drilling takes place
These parameters are optional and are used to indicate at which points or between which of those programmed points it is not required to machine.
Thus, programming P7 indicates that it is not required to do machining at point 7, and programming Q10.013 indicates that machining is not required from point 10 to 13, or expressed in another way, that no machining is required at points 10, 11, 12 and 13.
When it is required to define a group of points (Q10.013), care should be taken to define the final point with three digits, as if Q10.13 is programmed, multiple machining understands Q10.130.

The programming order for these parameters is P Q R S T U V, it also being necessary to maintain the order in which the points assigned to these are numbered, i.e., the numbering order of the points assigned to Q must be greater than that assigned to P and less than that assigned to R.

Example: Proper programming Correct programming

P5.006 Q12.015 R20.022 P5.006 Q12.015 R20.022

If these parameters are not programmed, the CNC understands that it must perform machining at all the points along the programmed path.

CNC 8040
·M· MODEL (SOFT V11.1X)
164

10.2.1 Basic operation

Programming manual

10.

MULTIPLE MACHINING G61: Multiple machining in a rectangular pattern

; Canned cycle positioning and definition. G81 G98 G00 G91 X100 Y150 Z-8 I-22 F100 S500 ; Defines multiple machining. G61 X700 I100 Y180 J60 P2.005 Q9.011 ; Cancels the canned cycle. G80 ; Positioning. G90 X0 Y0 ; End of program. M30 It is also possible to write the multiple machining definition block in the following ways:
G61 X700 K8 J60 D4 P2.005 Q9.011 G61 I100 K8 Y180 D4 P2.005 Q9.011
CNC 8040
·M· MODEL (SOFT V11.1X)
165

Programming manual
10.3 G62: Multiple machining in a grid pattern.

10.

The programming format is as follows:
G62 A B X I Y J P Q R S T U V XK YD IK JD

MULTIPLE MACHINING G62: Multiple machining in a grid pattern.

CNC 8040
·M· MODEL (SOFT V11.1X)

A (±5.5) B (±5.5) X (5.5) I (5.5) K (5)
Y (5.5) J (5.5)

166

D (5) P Q R S T U V

Programming manual

Number of machining operations along the ordinate axis

Defines the number of total machining operations in the ordinate axis, including the machining definition point.
Due to the fact that machining may be defined according to the ordinate axis with any two points of the Y J D group, the CNC allows the following definition combinations: YJ, YD, JD.

Nevertheless, if format YJ is defined, care should be taken to ensure that the number of machining operations is an integer number, otherwise the CNC will show the corresponding error code.

10.

MULTIPLE MACHINING G62: Multiple machining in a grid pattern.

Points where no drilling takes place

These parameters are optional and are used to indicate at which points or between which of those programmed points it is not required to machine.

When it is required to define a group of points (Q10.013), care should be taken to define the final point with three digits, as if Q10.13 is programmed, multiple machining understands Q10.130.
The programming order for these parameters is P Q R S T U V, it also being necessary to maintain the order in which the points assigned to these are numbered, i.e., the numbering order of the points assigned to Q must be greater than that assigned to P and less than that assigned to R.

Example: Proper programming Correct programming

P5.006 Q12.015 R20.022 P5.006 Q12.015 R20.022

If these parameters are not programmed, the CNC understands that it must perform machining at all the points along the programmed path.

CNC 8040
·M· MODEL (SOFT V11.1X)
167

Programming manual
10.3.1 Basic operation

10.

MULTIPLE MACHINING G62: Multiple machining in a grid pattern.

CNC 8040
·M· MODEL (SOFT V11.1X)
168

; Canned cycle positioning and definition. G81 G98 G00 G91 X100 Y150 Z-8 I-22 F100 S500 ; Defines multiple machining. G62 X700 I100 Y180 J60 P2.005 Q9.011 R15.019 ; Cancels the canned cycle. G80 ; Positioning. G90 X0 Y0 ; End of program. M30
It is also possible to write the multiple machining definition block in the following ways: G62 X700 K8 J60 D4 P2.005 Q9.011 R15.019 G62 I100 K8 Y180 D4 P2.005 Q9.011 R15.019

10.4 G63: Multiple machining in a circular pattern
The programming format is as follows: G63 X Y I C F P Q R S T U V K

Programming manual

10.

MULTIPLE MACHINING G63: Multiple machining in a circular pattern

X (±5.5)

Distance from the first machining point to the center along the abscissa axis
Defines the distance from the starting point to the center along the abscissa axis.

Y (±5.5)

Distance from the first machining point to the center along the ordinate axis
Defines the distance from the starting point to the center along the ordinate axis.
With parameters X and Y the center of the circle is defined in the same way that I and J do this in circular interpolations (G02, G03).

I (±5.5)

Angular pass between machining operations
Defines the angular pass between machining operations. When moving from point to point in G00 or G01, the sign indicates the direction, "+" counterclockwise, "-" clockwise.

K (5)

Total number of machining operations
Defines the number of total machining operations along the circle, including the machining definition point.
It will be enough to program I or K in the multiple machining definition block. Nevertheless, if K is programmed in a multiple machining operation in which movement between points is made in G00 or G01, machining will be done counterclockwise.

C (0/1/2/3) Type of move from point to point.

Indicates how movement is made between machining points. If it is not programmed, the value C=0 will be taken.

C=0:

Movement is made in rapid feedrate (G00).

C=1:

Movement is made in linear interpolation (G01).

C=2:

Movement is made in clockwise circular interpolation (G02)

C=3:

Movement is made in counterclockwise circular interpolation (G03)

CNC 8040
·M· MODEL (SOFT V11.1X)

169

MULTIPLE MACHINING G63: Multiple machining in a circular pattern

Programming manual
F (5.5)

10.

P Q R S T U V

Feedrate to move from point to point

Defines the feedrate that is used for moving from point to point. Obviously, it will only apply for "C" values other than zero. If it is not programmed, the value F0 will be taken, maximum feedrate selected by the "MAXFEED" axis machine parameter.

Points where no drilling takes place
These parameters are optional and are used to indicate at which points or between which of those programmed points it is not required to machine.

Thus, programming P7 indicates that it is not required to do machining at point 7, and programming Q10.013 indicates that machining is not required from point 10 to 13, or expressed in another way, that no machining is required at points 10, 11, 12 and 13.
When it is required to define a group of points (Q10.013), care should be taken to define the final point with three digits, as if Q10.13 is programmed, multiple machining understands Q10.130.

Example: Proper programming Correct programming

P5.006 Q12.015 R20.022 P5.006 Q12.015 R20.022

If these parameters are not programmed, the CNC understands that it must perform machining at all the points along the programmed path.

CNC 8040
·M· MODEL (SOFT V11.1X)
170

10.4.1 Basic operation

Programming manual

1. Multiple machining calculates the next point of those programmed where it is wished to machine.
2. Movement at the feedrate programmed by "C" (G00,G01,G02 or G03) to this point.
3. Multiple machining will perform the canned cycle or modal subroutine selected after this movement.
4. The CNC will repeat steps 1-2-3 until the programmed path has been completed.
After completing multiple machining, the tool will be positioned at the last point along the programmed path where machining was performed.
Programming example assuming that the work plane is formed by the X and Y axes, that the Z axis is the longitudinal axis and that the starting point is X0 Y0 Z0:

10.

MULTIPLE MACHINING G63: Multiple machining in a circular pattern

; Canned cycle positioning and definition. G81 G98 G01 G91 X280 Y130 Z-8 I-22 F100 S500 ; Defines multiple machining. G63 X200 Y200 I30 C1 F200 P2.004 Q8 ; Cancels the canned cycle. G80 ; Positioning. G90 X0 Y0 ; End of program. M30 It is also possible to write the multiple machining definition block in the following ways:
G63 X200 Y200 K12 C1 F200 P2.004 Q8
CNC 8040
·M· MODEL (SOFT V11.1X)
171

Programming manual
10.5 G64: Multiple machining in an arc
The programming format is as follows: G64 X Y B I C F P Q R S T U V K
10.

MULTIPLE MACHINING G64: Multiple machining in an arc

CNC 8040
·M· MODEL (SOFT V11.1X)
172

X (±5.5)

Distance from the first machining point to the center along the abscissa axis
Defines the distance from the starting point to the center along the abscissa axis.

Y (±5.5)

B (5.5)

Angular path Defines the angular stroke of the machining path and is expressed in degrees.

I (±5.5)

K (5)

C (0/1/2/3) Type of move from point to point.

Indicates how movement is made between machining points. If it is not programmed, the value C=0 will be taken.

C=0:

Movement is made in rapid feedrate (G00).

C=1:

Movement is made in linear interpolation (G01).

C=2:

Movement is made in clockwise circular interpolation (G02)

C=3:

Movement is made in counterclockwise circular interpolation (G03)

F (5.5) P Q R S T U V

Programming manual

Feedrate to move from point to point

Points where no drilling takes place

These parameters are optional and are used to indicate at which points or between which of those programmed points it is not required to machine.

When it is required to define a group of points (Q10.013), care should be taken to define the final point with three digits, as if Q10.13 is programmed, multiple machining understands Q10.130.

Example: Proper programming Correct programming

P5.006 Q12.015 R20.022 P5.006 Q12.015 R20.022

If these parameters are not programmed, the CNC understands that it must perform machining at all the points along the programmed path.

MULTIPLE MACHINING G64: Multiple machining in an arc

10.

CNC 8040
·M· MODEL (SOFT V11.1X)
173

Programming manual
10.5.1 Basic operation

10.

MULTIPLE MACHINING G64: Multiple machining in an arc

CNC 8040
·M· MODEL (SOFT V11.1X)
174

; Canned cycle positioning and definition. G81 G98 G01 G91 X280 Y130 Z-8 I-22 F100 S500 ; Defines multiple machining. G64 X200 Y200 B225 I45 C3 F200 P2 ; Cancels the canned cycle. G80 ; Positioning. G90 X0 Y0 ; End of program. M30
It is also possible to write the multiple machining definition block in the following ways: G64 X200 Y200 B225 K6 C3 F200 P2

Programming manual
10.6 G65: Machining programmed with an arc-chord

This function allows activated machining to be performed at a point programmed by means of an arc chord. Only one machining operation will be performed, its programming format being:
G65 X Y A C F I

10.

MULTIPLE MACHINING G65: Machining programmed with an arc-chord

X (±5.5)

Distance from the first machining point to the center along the abscissa axis
Defines the distance from the starting point to the center along the abscissa axis.

Y (±5.5)

A (±5.5)

Angle of the chord
Defines the angle formed by the perpendicular bisector of the chord with the abscissa axis and is expressed in degrees.

I (±5.5)

Angular pass between machining operations
Defines the chord length. When moving from point to point in G00 or G01, the sign indicates the direction, "+" counterclockwise, "-" clockwise.

C (0/1/2/3) Type of move from point to point.

Indicates how movement is made between machining points. If it is not programmed, the value C=0 will be taken.

C=0:

Movement is made in rapid feedrate (G00).

C=1:

Movement is made in linear interpolation (G01).

C=2:

Movement is made in clockwise circular interpolation (G02)

C=3:

Movement is made in counterclockwise circular interpolation (G03)

F (5.5)

Feedrate to move from point to point
Defines the feedrate that is used for moving from point to point. Obviously, it will only apply for "C" values other than zero. If it is not programmed, the value F0 will be taken, maximum feedrate selected by the "MAXFEED" axis machine parameter.

CNC 8040
·M· MODEL (SOFT V11.1X)

175

Programming manual
10.6.1 Basic operation

10.

1. Multiple machining calculates the next point of those programmed where it is wished to machine.
2. Movement at the feedrate programmed by "C" (G00,G01,G02 or G03) to this point.
3. Multiple machining will perform the canned cycle or modal subroutine selected after this movement.
After completing multiple machining, the tool will be positioned at the programmed point.
Programming example assuming that the work plane is formed by the X and Y axes, that the Z axis is the longitudinal axis and that the starting point is X0 Y0 Z0:

MULTIPLE MACHINING G65: Machining programmed with an arc-chord

CNC 8040
·M· MODEL (SOFT V11.1X)
176

; Canned cycle positioning and definition. G81 G98 G01 G91 X890 Y500 Z-8 I-22 F100 S500 ; Defines multiple machining. G65 X-280 Y-40 A60 C1 F200 ; Cancels the canned cycle. G80 ; Positioning. G90 X0 Y0 ; End of program. M30
It is also possible to write the multiple machining definition block in the following ways: G65 X-280 Y-40 I430 C1 F200

11 IRREGULAR POCKET CANNED
CYCLE
What is an irregular pocket with islands?
A pocket with islands is composed by an external contour or profile and a series of internal contours or profiles called islands.

(1) Outside contour or profile of the pocket. (2) Inside contour or profile of the pocket.
There are two types of pockets with islands, namely 2D and 3D pockets.
2D pocket.
In a 2D pocket, all the walls of the outside profile and of the islands are vertical. To define the contours of a 2D pocket, the plane profile for all the contours must be defined.

3D pocket.

In a 3D pocket, one, several or all the walls of the outside pocket and/or of the islands are not vertical. To define the contours of a 2D pocket, the plane profile and the depth profile for all the contours must be defined (even if they are vertical).

(A) Plane profile.

(B) Depth profile.

CNC 8040
·M· MODEL (SOFT V11.1X)
177

Programming manual
11.

Programming the irregular pocket canned cycle

The call function for a 2D or 3D irregular pocket canned cycle is G66. The machining of a pocket may consist of the following operations, each one is programmed with its relevant ·G· function.

Function Machining operation

G69 G81 G82 Drilling operation, prior to machining. G83

G67

Roughing operation.

G67

Semi-finishing operation.

G68

Finishing operation.

Pocket
2D
2D / 3D 3D
2D / 3D

G66 defines the operations that make up the machining of the pocket and where they are defined in the program. This function also indicates where the various profiles of the pocket are defined.

IRREGULAR POCKET CANNED CYCLE

CNC 8040
·M· MODEL (SOFT V11.1X)
178

11.1 2D pockets

Programming manual

The G66 function is not modal, therefore it must be programmed whenever it is required to perform a 2D pocket. In a block defining an irregular pocket canned cycle, no other function can be programmed, its structure definition being:
G66 D H R I F K S E Q

D (0-9999) / H (0-9999) Drilling operation

Label number of the first block (D) and last block (H) defining the drilling operation. · When not setting (H) only block (D) is executed. · When not setting (D) there is no drilling operation.

R (0-9999) / I (0-9999) Roughing operation
Label number of the first block (R) and last block (I) defining the roughing operation. · When not setting (I) only block (r) is executed. · When not setting (R) there is no roughing operation.

F (0-9999) / K (0-9999) Finishing operation

Label number of the first block (F) and last block (K) defining the finishing operation. · When not setting (K) only block (F) is executed. · When not setting (F) there is no finishing operation.

S (0-9999) / E (0-9999) Geometry description of the profiles
Label number of the first block (S) and last block (E) defining the geometry of the profiles forming the pocket. Both parameters must be set.

Q (0-999999)

Program that contains the definition of the geometrical description of the profiles
Number of the program containing the geometry definition, parameters S and E. If it is in the same program, (Q) need not be defined.

IRREGULAR POCKET CANNED CYCLE 2D pockets

11.

CNC 8040
·M· MODEL (SOFT V11.1X)
179

IRREGULAR POCKET CANNED CYCLE 2D pockets

Programming manual
11.

Programming example:
; Initial positioning. G00 G90 X100 Y200 Z50 F5000 T1 D2 M06 ; Definition of irregular pocket canned cycle. G66 D100 R200 I210 F300 S400 E500 ; End of program. M30
; Defines the drilling operation. N100 G81... ; Roughing operation. N200... G67... N210 ... ; Finishing operation. N300 G68... ; Geometrical description. N400 G0 G90 X300 Y50 Z3 ... ... N500 G2 G6 X300 Y50 I150 J0
Basic operation
1. Drilling operation. Only if it has been programmed. After analyzing the geometry of the pocket with islands, the tool radius and the angle of the path programmed in the roughing operation, the CNC will calculate the coordinates of the point where the selected drilling operation must be performed.
2. Roughing operation. Only if it has been programmed. It consists of several surface milling passes, until the total depth programmed has been reached. On each surface milling pass, the steps below will be followed depending on the type of machining that has been programmed: Case A: When the machining paths are linear and maintain a certain angle with the abscissa axis. It first contours the external profile of the part. If the finishing operation has been selected on the cycle call, this contouring is performed leaving the finishing stock programmed for the finishing pass.

CNC 8040
·M· MODEL (SOFT V11.1X)
180

Programming manual
Next the milling operation, with the programmed feed and steps. If, while milling, an island is run into for the first time, it will be contoured.

After the contouring and the remaining times, the tool will pass over the island, withdrawing along the longitudinal axis, to the reference plane, and will continue machining once the island has been cleared.

11.

IRREGULAR POCKET CANNED CYCLE 2D pockets

Case B: When the machining paths are concentric.
The roughing operation is carried out along paths concentric to the profile. The machining will be done as fast as possible avoiding (when possible) going over the islands.

3. Finishing operation. Only if it has been programmed. This operation can be done on a single pass or on several, as well as following the profiles in the programmed direction or in the opposite. The CNC will machine both the external profile and the islands, making tangential approaches and exits to these with a constant surface speed.
Reference coordinates
In the pocket canned cycle with islands, there are four coordinates along the longitudinal axis (selected with G15), which, due to their importance, are discussed below: ·1· Initial plane coordinate. This coordinate is given by the position which the tool
occupies when the cycle is called. ·2· Coordinate of the reference plane. This represents an approach coordinate to the
part, and must be programmed in absolute coordinates. ·3· Part surface coordinate. This is programmed in absolute coordinates and in the
first profile definition block. ·4· Machining depth coordinate. It must be programmed in absolute values.

CNC 8040
·M· MODEL (SOFT V11.1X)

181

Programming manual

Conditions after finishing the cycle
Once the canned cycle has ended, the active feedrate will be the last one programmed, i.e. the one corresponding to the roughing operation or the finishing operation. The CNC will assume functions G00, G40 and G90.

11.

IRREGULAR POCKET CANNED CYCLE 2D pockets

CNC 8040
·M· MODEL (SOFT V11.1X)
182

11.1.1 Drilling operation

Programming manual

This operation is optional and in order to be executed it is necessary to also program a roughing operation.
It is mainly used when the tool programmed in the roughing operation does not machine along the longitudinal axis, allowing, by means of this operation, the access of this tool to the surface to be roughed off.
It will be programmed in a block which will need to bear a label number in order to indicate to the canned cycle the block where the drilling operation is defined.
; Definition of irregular pocket canned cycle. G66 D100 R200 F300 S400 E500 ; Defines the drilling operation. N100 G81...

11.

IRREGULAR POCKET CANNED CYCLE 2D pockets

The drilling canned cycles that can be programmed are:

G69

Complex deep hole drilling

G81

Drilling canned cycle.

G82

Drilling cycle with dwell.

G83

Deep hole drilling canned cycle with constant peck (drilling step).

When defining the drilling operation, the corresponding definition parameters must be programmed together with the required function.

In a block of this type, only cycle definition parameters must be programmed, without defining XY positioning, as the canned cycle itself will calculate the coordinate of the point or points to be drilled according to the programmed profile and the roughing angle.

After the definition parameters, auxiliary F S T D M functions can be programmed, if so wished. No M function can be programmed if it has an associated subroutine.

It is possible to program the M06 function in this block (if it does not have an associated subroutine), to make the tool change. Otherwise, the CNC will show the corresponding error. If the M06 has an associated subroutine, the drilling tool "T" must be selected before calling the cycle.

N100 G69 G98 G91 Z-4 I-90 B1.5 C0.5 D2 H2 J4 K100 F500 S3000 M3 N120 G81 G99 G91 Z-5 I-30 F400 S2000 T3 D3 M3 N220 G82 G99 G91 Z-5 I-30 K100 F400 S2000 T2 D2 M6 N200 G83 G98 G91 Z-4 I-5 J6 T2 D4

CNC 8040
·M· MODEL (SOFT V11.1X)
183

Programming manual
11.1.2 Roughing operation

11.

This is the main operation in the machining of an irregular pocket, and its programming is optional.
This operation will be performed keeping the square corner mode (G07) or round corner mode (G05) that is currently active. However, the canned cycle will assign the G07 format to the necessary movements.
It will be programmed in a block which will need to bear a label number in order to indicate to the canned cycle the block where the roughing operation is defined.
; Definition of irregular pocket canned cycle. G66 D100 R200 F300 S400 E500 ; Definition of the roughing operation. N200 G67...

A (±5.5)

The function for the roughing operation is G67 and its programming format: G67 A B C I R K V Q F S T D M
Angle of the path with respect to the abscissa axis It defines the angle of the machining path with respect to the abscissa axis.

IRREGULAR POCKET CANNED CYCLE 2D pockets

If parameter "A" is not programmed, the roughing operation is carried out following concentric paths. It will be machined as fast as possible since it does not have to go over the islands.

CNC 8040
·M· MODEL (SOFT V11.1X)
184

B (±5.5)

Programming manual

Pass depth

Defines the machining pass along the longitudinal axis (depth of the roughing pass). It must be defined and it must have a value other than 0; otherwise, the roughing operation will be cancelled.
· If programmed with a positive sign, all the roughing will be performed with the same machining pass, and the canned cycle calculates a pass equal to or smaller than the programmed pass.
· If programmed with a negative sign, all the roughing will be performed with the programmed pass, and the canned cycle will adjust the last pass to obtain the total programmed depth.

11.

C (5.5)

Milling pass
Defines the milling pass in roughing along the main plane, the entire pocket being performed with the given pass, and the canned cycle adjusts the last milling pass.

IRREGULAR POCKET CANNED CYCLE 2D pockets

I (±5.5) R (±5.5)

If not programmed or programmed with a 0 value, it assumes a value of 3/4 of the diameter of the selected tool. If programmed with a value greater than the tool diameter, the CNC issues the relevant error message.
Pocket depth
Defines the total depth of the pocket and is programmed in absolute coordinates. It must be programmed.
Reference plane
Defines the reference plane coordinate and is programmed in absolute coordinates. It must be programmed.

CNC 8040
·M· MODEL (SOFT V11.1X)
185

Programming manual
K (1)

11.

V (5.5) Q (5.5)

Type of profile intersection

Defines the type of profile intersection to be used.

K=0

Basic profile intersection.

K=1

Advanced profile intersection.

If not programmed, a value of 0 will be assumed. Both intersection types will be discussed later on.

Penetration feedrate
Defines the tool penetrating feedrate.
If not programmed or programmed with a 0 value, it assumes 50% of the feedrate in the plane (F).

Penetration angle Optional. Tool penetration angle.

IRREGULAR POCKET CANNED CYCLE 2D pockets

CNC 8040

F (5.5) S (5.5) T (4) D (4) M

If not programmed or programming the value of 90, it means that the penetration is vertical. When programming a value lower than 0 or greater than 90, it issues the error "wrong parameter value in canned cycle".
Machining feedrate Optional. It sets the machining feedrate in the plane.
Spindle speed Optional. It sets the spindle speed.
Tool number Defines the tool used for the roughing operation. It must be programmed.
Tool offset Optional. Defines the tool offset number.
Auxiliary (miscellaneous) functions Optional. Up to 7 miscellaneous M functions can be programmed. This operation allows M06 with an associated subroutine to be defined, and the tool change is performed before beginning the roughing operation.

·M· MODEL (SOFT V11.1X)

186

11.1.3 Finishing operation

Programming manual

This operation is optional.
It will be programmed in a block that will need to bear a label number in order to indicate to the canned cycle the block where the finishing operation is defined.

; Definition of irregular pocket canned cycle. G66 D100 R200 F300 S400 E500 ; Defines the finishing operation. N300 G68...

11.

IRREGULAR POCKET CANNED CYCLE 2D pockets

B (±5.5)

The function for the finishing operation is G68 and its programming format: G68 B L Q I R K V F S T D M
Pass depth
Defines the machining pass along the longitudinal axis (depth of the finishing pass). · If it is programmed with a value of 0, the CNC will perform a single finishing pass with the total depth of the pocket. · If programmed with a positive sign, all the roughing will be performed with the same machining pass, and the canned cycle calculates a pass equal to or lower than the programmed pass. · If programmed with a negative sign, all the roughing will be performed with the programmed pass, and the canned cycle will adjust the last pass to obtain the total programmed depth.

L (±5.5)

lateral finishing stock
Defines the value of the finishing stock left on the side walls of the pocket before the finishing operation.

· If programmed with a positive value, the finishing pass will be carried out in square corner (G07).
· If a negative value is programmed, the finishing pass will be carried out in G5 (round corner).
· If not programmed or programmed with a 0 value, the cycle does not run the finishing pass.

CNC 8040
·M· MODEL (SOFT V11.1X)

187

Programming manual

11.

Q (0/1/2)

Direction of the finishing pass

Indicates the direction of the finishing pass on the outside profile. The finishing pass on the islands is always run in the opposite direction.

Q = 0

The finishing pass is carried out in the same direction as the outside profile was programmed.

Q = 1

The finishing pass is carried out in the opposite direction to the one programmed.

Q = 2

Reserved.

Any other value will generate the corresponding error message. If parameter "Q" is not programmed, the cycle assumes Q0.

IRREGULAR POCKET CANNED CYCLE 2D pockets

I (±5.5)

Pocket depth
Defines the total depth of the pocket and is programmed in absolute coordinates. · If the island has a roughing operation, it is not necessary to define this parameter since it has been programmed in that operation. However, if programmed in both operations, the canned cycle will assume the particular depth indicated for each operation. · If the island has no roughing operation, it is necessary to define this parameter.

R (±5.5)

Reference plane
Defines the reference plane coordinate and is programmed in absolute coordinates. · If the island has a roughing operation, it is not necessary to define this parameter since it has been programmed in that operation. However, if programmed in both operations, the canned cycle will assume the particular depth indicated for each operation. · If the island has no roughing operation, it is necessary to define this parameter.

CNC 8040
·M· MODEL (SOFT V11.1X)

K (1) V (5.5)

Type of profile intersection

Defines the type of profile intersection to be used.

K=0

Basic profile intersection.

K=1

Advanced profile intersection.

If the island has a roughing operation, it is not necessary to define this parameter since it has been programmed in that operation. However, if programmed in both operations, the canned cycle will assume the one defined for the roughing operation.

If no roughing operation has been defined and this parameter is not programmed, the canned cycle will assume a K0 value. Both types of intersection are described later on.

Penetration feedrate
Defines the tool penetrating feedrate.
If not programmed or programmed with a 0 value, it assumes 50% of the feedrate in the plane (F).

188

F (5.5) S (5.5) T (4) D (4) M

Programming manual

Machining feedrate Optional. It sets the machining feedrate in the plane.

Spindle speed Optional. It sets the spindle speed.

Tool number Defines the tool used for the roughing operation. It must be programmed. Tool offset Optional. Defines the tool offset number.

11.

Auxiliary (miscellaneous) functions
Optional. Up to 7 miscellaneous M functions can be programmed.
This operation allows M06 with an associated subroutine to be defined, and the tool change is performed before beginning the roughing operation.

IRREGULAR POCKET CANNED CYCLE 2D pockets

CNC 8040
·M· MODEL (SOFT V11.1X)
189

IRREGULAR POCKET CANNED CYCLE 2D pockets

Programming manual
11.1.4 Profile programming syntax

11.

When outside and inside profiles of an irregular pocket are programmed the following programming rules must be followed: The canned cycle will verify all these geometry rules before beginning to make the pocket adapting the profile of the pocket to them and displaying the error message when necessary.
· All types of programmed profiles must be closed. The following examples cause a geometry error.

· No profile must intersect itself. The following examples cause a geometry error.

· When more than one outside profile has been programmed, the canned cycle assumes the one occupying the largest surface.

· It is not required to program inside profiles. Should these be programmed, they must be partially or totally internal with respect to the outside profile. Some examples are given below.

CNC 8040
·M· MODEL (SOFT V11.1X)
190

· An internal profile totally contained within another internal profile cannot be programmed. In this case, only the most external profile will be considered.

11.1.5 Profile intersection

Programming manual

In order to facilitate the programming of profiles, the canned cycle allows the profiles to intersect one another and the external profile.
The two available types of intersection can be selected by parameter "K"

Basic profile intersection (K=0)
When selecting this type, the following profile intersecting rules are to be followed: · The intersection of islands generates a new inside profile which is their Boolean union.

11.

IRREGULAR POCKET CANNED CYCLE 2D pockets

· The intersection between an internal and an external profile generates a new external profile as a result of the difference between the external and the internal profiles.

· If there is an inside profile which has an intersection with another inside profile and with the external profile, the canned cycle first makes the intersection between the inside profiles and then the intersection of these with the external profile.

· As a result of the intersection of the inside profiles with the outside one, a single pocket will be obtained which corresponds to the outside profile having the largest surface. The rest will be ignored.

· If the finishing operation has been programmed, the profile of the resulting pocket must comply with all the tool compensation rules, since if a profile is programmed which cannot be machined by the programmed finishing tool, the CNC will show the corresponding error.

CNC 8040

·M· MODEL (SOFT V11.1X)

191

Programming manual
11.

Advanced profile intersection (K=1)
When selecting this type, the following profile intersecting rules are to be followed: 1. The initial point of each contour determines the section to be selected.
In a profile intersection, each contour is divided into several lines that could be grouped as:
· Lines external to the other contour. · Lines internal to the other contour. This type of profile intersection selects in each contour the group of lines where the profile defining point is included. The following example shows the explained selection process. The solid lines indicate the lines external to the other contour and the dashes indicate the internal lines. The initial point of each contour is indicated with an "x".

IRREGULAR POCKET CANNED CYCLE 2D pockets

Examples of profile intersections: Boolean addition
Boolean subtraction

Boolean intersection

CNC 8040
·M· MODEL (SOFT V11.1X)
192

IRREGULAR POCKET CANNED CYCLE 2D pockets

Programming manual 2. The programming sequence for the different profiles is determinant when having
an intersection of more than 3 profiles. The profile intersection process is performed according to the order in which the profiles have been programmed. This way, the result of the intersection between the first two will be intersected with the third one and so forth. The initial point of the resulting profiles always coincides with the initial point that defined the first profile.
11.
CNC 8040
·M· MODEL (SOFT V11.1X)
193

Programming manual
11.

Resulting profile
Once the profiles of the pocket and islands have been obtained, the canned cycle calculates the remaining profiles according to the radius of the roughing tool and the programmed finishing stock.
It may occur that in this process intersections are obtained which do not appear among the programmed profiles.

If there is an area in which the roughing tool cannot pass, when the intersection is made between the offset of the profiles, several pockets will be obtained as a result, all of which will be machined.

IRREGULAR POCKET CANNED CYCLE 2D pockets

CNC 8040
·M· MODEL (SOFT V11.1X)
194

11.1.6 Profile programming syntax

Programming manual

The outside profile and the inside profiles or islands which are programmed must be defined by simple geometrical elements such as straight lines or arcs.
The first definition block (where the external profile starts) and the last (where the last profile defined ends) must be provided with the block label number. These label numbers will indicate the beginning and end of the profile geometry definition for the profiles that make up the pocket.
; Definition of irregular pocket canned cycle. G66 D100 R200 F300 S400 E500 ; Geometrical description. N400 G0 G90 X300 Y50 Z3 ... N500 G2 G6 X300 Y50 I150 J0

11.

IRREGULAR POCKET CANNED CYCLE 2D pockets

The profile programming syntax must follow these rules:
· The external profile must begin in the first definition block of the geometric description of the part profiles. This block will be assigned a label number in order to indicate canned cycle G66 the beginning of the geometric description.
· The part surface coordinate will be programmed in this block.
· All the internal profiles which are required may be programmed, one after the other. Each of these must commence with a block containing the G00 function (indicating the beginning of the profile).

Care must be taken to program G01, G02 or G03 in the block following the definition of the beginning, as G00 is modal, thus preventing the CNC from

interpreting the following blocks as the beginnings of a new profile.

· Once the definition of the profiles has been completed, a label number must be assigned to the last block programmed, in order to indicate the canned cycle G66 the end of the geometric description.

G0 G17 G90 X-350 Y0 Z50 ; Definition of irregular pocket canned cycle. G66 D100 R200 F300 S400 E500 G0 G90 X0 Y0 Z50 M30

; Defines the first profile. N400 G0 G90 X-260 Y-190 Z4.5 --- --- --- --; Defines another profile. G0 X230 Y170 G1 --- ----- --- --- --; Defines another profile. G0 X-120 Y90 G2 --- ----- --- --- --; End of geometric description. N500 G1 X-120 Y90

CNC 8040
·M· MODEL (SOFT V11.1X)

195

IRREGULAR POCKET CANNED CYCLE 2D pockets

Programming manual
11.

· Profiles are described as programmed paths, it being possible to include corner rounding, chamfers, etc., following the syntax rules defined for this purpose.
· The profile description must not contain: mirror images, scaling factor changes, pattern rotation, zero offsets, etc.
· It must not contain high level blocks such as jumps, calls to subroutines or parametric programming.
· It must not contain other canned cycles.

In addition to the G00 function, which has a special meaning, the irregular pocket canned cycle allows the use of the following functions for the definition of profiles.

G01

Linear interpolation.

G02

Clockwise circular interpolation.

G03

Counter-clockwise circular interpolation.

G06

Circle center in absolute coordinates.

G08

Arc tangent to previous path.

G09

Arc defined by three points.

G36

Corner rounding, radius blend.

G39

Chamfer.

G53

Programming with respect to machine zero.

G70

Programming in inches.

G71

Programming in millimeters.

G90

Absolute programming.

G91

Incremental programming.

G93

Polar origin preset.

CNC 8040
·M· MODEL (SOFT V11.1X)
196

11.1.7 Errors

Programming manual

ERROR 1023 ERROR 1024 ERROR 1025 ERROR 1026 ERROR 1041
ERROR 1042
ERROR 1044 ERROR 1046 ERROR 1047 ERROR 1048

The CNC will issue the following errors:
G67. Tool radius too large.
When selecting a wrong roughing tool.
G68. Tool radius too large.
When selecting a wrong finishing tool.
A tool with no radius has been programmed
When using a tool with "0" radius while machining a pocket.
A step has been programmed that is larger than the tool diameter
When parameter "C" of the roughing operation is greater than the diameter of the roughing tool.
A parameter required in the canned cycle has not been programmed.
It comes up in the following instances: · When parameters "I" and "R" have not been programmed in the roughing operation. · When not using a roughing operation and not programming the "I" and "R" parameters for the finishing operation.
Wrong parameter value in the canned cycle
It comes up in the following instances: · When parameter "Q" of the finishing operation has the wrong value. · When parameter "B" of the finishing operation has a "0" value. · When parameter "J" of the finishing operation has been programmed with a value greater than the finishing tool radius.
The plane profile intersects itself in an irregular pocket with islands.
It comes up when any of the plane profiles of the programmed contours intersects itself.
Wrong tool position prior to the canned cycle
It comes up when calling the G66 cycle if the tool is positioned between the reference plane and the depth coordinate (bottom) of any of the operations.
Open plane profile in an irregular pocket with islands
It comes up when any of the programmed contours does not begin and end at the same point. It may be because G1 has not been programmed after the beginning, with G0, on any of the profiles.
Part surface coordinate not programmed in pocket with islands
It comes up when the first point of the geometry does not include the pocket top coordinate.

IRREGULAR POCKET CANNED CYCLE 2D pockets

11.
CNC 8040

·M· MODEL (SOFT V11.1X)

197

Programming manual ERROR 1049

ERROR 1084

11.

ERROR 1227

Wrong reference plane coordinate for the canned cycle.
It comes up when the coordinate of the reference plane is located between the part's "top" and "bottom" in any of the operations.
Arc programmed wrong'
It comes up when any of the paths programmed in the geometry definition of the pocket is wrong.
Wrong profile intersection in a pocket with islands.
It comes up in the following instances: · When two plane profiles have a common section (drawing on the left). · When the initial points of two profiles in the main plane coincide (drawing on the right).

IRREGULAR POCKET CANNED CYCLE 2D pockets

CNC 8040
·M· MODEL (SOFT V11.1X)
198

11.1.8 Programming examples
Programming example ·1· Programming example, without automatic tool changer

Programming manual
11.

IRREGULAR POCKET CANNED CYCLE 2D pockets

; Tool dimensions. (TOR1=5, TOI1=0, TOL1=25, TOK1=0) (TOR2=3, TOI2=0, TOL2=20, TOK2=0) (TOR3=5, TOI3=0, TOL3=25, TOK3=0)
; Initial positioning and programming of a pocket with islands. G0 G17 G43 G90 X0 Y0 Z25 S800 G66 D100 R200 F300 S400 E500 M30
; Definition of drilling operation. N100 G81 Z5 I-40 T3 D3 M6
; Definition of roughing operation. N200 G67 B20 C8 I-40 R5 K0 V100 F500 T1 D1 M6
; Definition of finishing operation. N300 G68 B0 L0.5 Q0 V100 F300 T2 D2 M6
; Definition of pocket profiles. N400 G0 G90 X-260 Y-190 Z0 ; External contour. G1 X-200 Y30 X-200 Y210 G2 G6 X-120 Y290 I-120 J210 G1 X100 Y170 G3 G6 X220 Y290 I100 J290 G1 X360 Y290 G1 X360 Y-10 G2 G6 X300 Y-70 I300 J-10 G3 G6 X180 Y-190 I300 J-190 G1 X-260 Y-190

CNC 8040
·M· MODEL (SOFT V11.1X)
199

Programming manual
11.

; Contour of the first island. G0 X230 Y170 G1 X290 Y170 G1 X230 Y50 G1 X150 Y90 G3 G6 X230 Y170 I150 J170
; Contour of the second island. G0 X-120 Y90 G1 X20 Y90 G1 X20 Y-50 G1 X-120 Y-50
; End of contour definition. N500 G1 X-120 Y90

IRREGULAR POCKET CANNED CYCLE 2D pockets

CNC 8040
·M· MODEL (SOFT V11.1X)
200

Programming manual
Programming example ·2· Programming example, with automatic tool changer. The "x" of the figure indicates the initial points of each profile:
11.

IRREGULAR POCKET CANNED CYCLE 2D pockets

; Tool dimensions. (TOR1=9, TOI1=0, TOL1=25, TOK1=0) (TOR2=3.6, TOI2=0, TOL2=20, TOK2=0) (TOR3=9, TOI3=0, TOL3=25, TOK3=0)
; Initial positioning and programming of a pocket with islands. G0 G17 G43 G90 X0 Y0 Z25 S800 G66 D100 R200 F300 S400 E500 M30
; Definition of drilling operation. N100 G81 Z5 I-40 T3 D3 M6
; Definition of roughing operation. N200 G67 B10 C5 I-40 R5 K1 V100 F500 T1 D1 M6
; Definition of finishing operation. N300 G68 Q1 L0.5 Q0 V100 F300 T2 D2 M6
; Definition of pocket profiles. N400 G0 G90 X-300 Y50 Z3

CNC 8040
·M· MODEL (SOFT V11.1X)
201

IRREGULAR POCKET CANNED CYCLE 2D pockets

Programming manual
11.
CNC 8040
·M· MODEL (SOFT V11.1X)

; External contour. G1 Y190 G2 G6 X-270 Y220 I-270 J190 G1 X170 X300 Y150 Y50 G3 G6 X300 Y-50 I300 J0 G1 G36 R50 Y-220 X -30 G39 R50 X-100 Y-150 X-170 Y-220 X -270 G2 G6 X-300 Y-190 I-270 J-190 G1 Y-50 X -240 Y50 X -300
; Contour of the first island. G0 X-120 Y80 G2 G6 X-80 Y80 I-100 J80; (Contour a) G1 Y-80 G2 G6 X-120 Y-80 I-100 J-80 G1 Y80 G0 X-40 Y0; (Contour b) G2 G6 X-40 Y0 I-100 J0 G0 X-180 Y20; (Contour c) G1 X-20 G2 G6 X-20 Y-20 I-20 J0 G1 X-180 G2 G6 X-180 Y20 I-180 J0
; Contour of the second island. G0 X150 Y140 G1 X170 Y110; (Contour d) Y -110 X150 Y-140 X130 Y-110 Y110 X150 Y140 G0 X110 Y0; (Contour e)
; End of contour definition. N500 G2 G6 X110 Y0 I150 J0

202

11.2 3D pockets

Programming manual

The cycle calling function G66 is not modal; therefore, it must be programmed every time a 3D pocket is to be executed.
In a block defining an irregular pocket canned cycle, no other function can be programmed, its structure definition being:
G66 R I C J F K S E
R (0-9999) / I (0-9999) Roughing operation
Label number of the first block (R) and last block (I) defining the roughing operation. · When not setting (I) only block (r) is executed. · When not setting (R) there is no roughing operation.
C (0-9999) / J (0-9999) Semi-finishing operation
Label number of the first block (C) and last block (J) defining the semi-finishing operation.
· When not setting "J" only block "c" is executed. · When not setting (C) there is no semi-finishing operation.
F (0-9999) / K (0-9999) Finishing operation
Label number of the first block (F) and last block (K) defining the finishing operation. · When not setting (K) only block (F) is executed. · When not setting (F) there is no finishing operation.
S (0-9999) / E (0-9999) Geometry description of the profiles
Label number of the first block (S) and last block (E) defining the geometry of the profiles forming the pocket. Both parameters must be set.

IRREGULAR POCKET CANNED CYCLE 3D pockets

11.

CNC 8040
·M· MODEL (SOFT V11.1X)
203

IRREGULAR POCKET CANNED CYCLE 3D pockets

Programming manual
11.

Programming example:
; Initial positioning. G00 G90 X100 Y200 Z50 F5000 T1 D2 M06 ; Definition of irregular pocket canned cycle. G66 R100 C200 J210 F300 S400 E500 ; End of program. M30
; Roughing operation. N100 G67... ; Semi-finishing operation. N200... G67... N210 ... ; Finishing operation. N300 G68... ; Geometrical description. N400 G0 G90 X300 Y50 Z3 ... ... N500 G2 G6 X300 Y50 I150 J0
Basic operation
1. Roughing operation. Only if it has been programmed. It consists of several surface milling passes, until the total depth programmed has been reached. On each surface milling pass, the steps below will be followed depending on the type of machining that has been programmed: Case A: When the machining paths are linear and maintain a certain angle with the abscissa axis. It first contours the external profile of the part. If the finishing operation has been selected on the cycle call, this contouring is performed leaving the finishing stock programmed for the finishing pass.

CNC 8040
·M· MODEL (SOFT V11.1X)
204

IRREGULAR POCKET CANNED CYCLE 3D pockets

Programming manual Next the milling operation, with the programmed feed and steps. If, while milling, an island is run into for the first time, it will be contoured.
11.
After the contouring and the remaining times, the tool will pass over the island, withdrawing along the longitudinal axis, to the reference plane, and will continue machining once the island has been cleared.
Case B: When the machining paths are concentric. The roughing operation is carried out along paths concentric to the profile. The machining will be done as fast as possible avoiding (when possible) going over the islands.
2. Semi-finishing operation. Only if it has been programmed. After the roughing, some ridges appear on the external profile as well as on the islands themselves as shown in the illustration below:
CNC 8040
·M· MODEL (SOFT V11.1X)
205

Programming manual

With the semi-finishing operation, it is possible to minimize these ridges by running several contouring passes at different depths.

11.

3. Finishing operation. Only if it has been programmed.
It runs consecutive finishing passes in 3D. Either inward or outward machining direction may be selected or both may be alternated.

IRREGULAR POCKET CANNED CYCLE 3D pockets

The CNC will machine both the external profile and the islands, making tangential approaches and exits to these with a constant surface speed.
Conditions after finishing the cycle
Once the canned cycle has ended, the active feedrate will be the last one programmed, i.e. the one corresponding to the roughing operation or the finishing operation. The CNC will assume functions G00, G40 and G90.
Reference coordinates
In the pocket canned cycle with islands, there are four coordinates along the longitudinal axis (selected with G15), which, due to their importance, are discussed below: ·1· Initial plane coordinate. This coordinate is given by the position which the tool
occupies when the cycle is called. ·2· Coordinate of the reference plane. This represents an approach coordinate to the
part, and must be programmed in absolute coordinates. ·3· Part surface coordinate. This is programmed in absolute coordinates and in the
first profile definition block. ·4· Machining depth coordinate. It must be programmed in absolute values.

CNC 8040
·M· MODEL (SOFT V11.1X)
206

11.2.1 Roughing operation

Programming manual

This is the main operation in the machining of an irregular pocket, and its programming is optional.
It will be programmed in a block which will need to bear a label number in order to indicate to the canned cycle the block where the roughing operation is defined.

; Definition of irregular pocket canned cycle. G66 R100 C200 F300 S400 E500 ; Definition of the roughing operation. N100 G67...

11.

A (±5.5)

The function for the roughing operation is G67 and it cannot be executed independently from the G66. Its programming format is:
G67 A B C I R V F S T D M
Angle of the path with respect to the abscissa axis It defines the angle of the machining path with respect to the abscissa axis.

IRREGULAR POCKET CANNED CYCLE 3D pockets

If parameter "A" is not programmed, the roughing operation is carried out following concentric paths. It will be machined as fast as possible since it does not have to go over the islands.

CNC 8040
·M· MODEL (SOFT V11.1X)
207

Programming manual
B (±5.5)

Pass depth
Defines the machining pass along the longitudinal axis (depth of the roughing pass). It must be defined and it must have a value other than 0; otherwise, the roughing operation will be cancelled.

11.

· If programmed with a positive sign, all the roughing will be performed with the same machining pass, and the canned cycle calculates a pass equal to or smaller than the programmed pass.
· If programmed with a negative sign, all the roughing will be performed with the programmed pass, and the canned cycle will adjust the last pass to obtain the total programmed depth.
If done with "B(+)", the ridges will appear only on the pocket walls; but, if done with "B(-)", they could also show up above the islands.

IRREGULAR POCKET CANNED CYCLE 3D pockets

C (5.5)

Milling pass
Defines the milling pass in roughing along the main plane, the entire pocket being performed with the given pass, and the canned cycle adjusts the last milling pass.

CNC 8040
·M· MODEL (SOFT V11.1X)

I (±5.5)

If not programmed or programmed with a 0 value, it assumes a value of 3/4 of the diameter of the selected tool.
If programmed with a value greater than the tool diameter, the CNC issues the relevant error message.
Pocket depth
Defines the total depth of the pocket and is programmed in absolute coordinates. It must be programmed.

208

R (±5.5)

Programming manual
Reference plane
Defines the reference plane coordinate and is programmed in absolute coordinates. It must be programmed.

V (5.5)
F (5.5) S (5.5) T (4) D (4) M

Penetration feedrate Defines the tool penetrating feedrate. If not programmed or programmed with a 0 value, it assumes 50% of the feedrate in the plane (F).
Machining feedrate Optional. It sets the machining feedrate in the plane.
Spindle speed Optional. It sets the spindle speed.
Tool number Defines the tool used for the roughing operation. It must be programmed.
Tool offset Optional. Defines the tool offset number.
Auxiliary (miscellaneous) functions Optional. Up to 7 miscellaneous M functions can be programmed. This operation allows M06 with an associated subroutine to be defined, and the tool change is performed before beginning the roughing operation.

IRREGULAR POCKET CANNED CYCLE 3D pockets

11.

CNC 8040
·M· MODEL (SOFT V11.1X)
209

Programming manual
11.2.2 Semi-finishing operation

This operation is optional.
It will be programmed in a block which will need to bear a label number in order to indicate to the canned cycle the block where the roughing operation is defined.

11.

; Definition of irregular pocket canned cycle. G66 R100 C200 F300 S400 E500 ; Definition of the semi-finish operation. N200 G67...

IRREGULAR POCKET CANNED CYCLE 3D pockets

B (±5.5)

The function for the semi-finishing operation is G67 and it cannot be executed independently from the G66.
Both the roughing and the semi-finishing operations are defined with G67; but, in different blocks. It is function G66 who indicates which is which by means of parameters "R" and "C".
Its programming format is: G67 B I R V F S T D M
Pass depth
Defines the machining step along the longitudinal axis (semi-finishing pass). It must be programmed and with a value other than "0". Otherwise, the semi-finishing operation will be canceled.

CNC 8040
·M· MODEL (SOFT V11.1X)

I (±5.5) R (±5.5)

· If programmed with a positive sign, the whole semi-finish operation will be carried out with the same machining pass and the canned cycle will calculate a pass equal or smaller than the one programmed.
· If programmed with a negative sign, the whole semi-finish operation will be run with the programmed pass. The canned cycle will adjust the last pass to obtain the total programmed depth.
Pocket depth
Defines the total depth of the pocket and is programmed in absolute coordinates.
If there is a roughing operation and it is not programmed, the CNC takes the value defined for the roughing operation.
If there is no roughing operation, it must be programmed.
Reference plane
Defines the reference plane coordinate and is programmed in absolute coordinates.
If there is a roughing operation and it is not programmed, the CNC takes the value defined for the roughing operation.
If there is no roughing operation, it must be programmed.

210

V (5.5)
F (5.5) S (5.5)
D (4) M

Programming manual

Penetration feedrate
Defines the tool penetrating feedrate.
If not programmed or programmed with a 0 value, it assumes 50% of the feedrate in the plane (F).

Machining feedrate Optional. It sets the machining feedrate in the plane. Spindle speed Optional. It sets the spindle speed. T (4) Tool number Defines the tool used for the semi-finishing operation. It must be programmed.

11.

IRREGULAR POCKET CANNED CYCLE 3D pockets

Tool offset Optional. Defines the tool offset number.

Auxiliary (miscellaneous) functions
Optional. Up to 7 miscellaneous M functions can be programmed. They will be executed at the beginning of the semi-finishing operation.
This operation allows M06 with an associated subroutine to be defined, and the tool change is performed before beginning the semi-finishing operation.

CNC 8040
·M· MODEL (SOFT V11.1X)
211

Programming manual
11.2.3 Finishing operation

This operation is optional.
It will be programmed in a block that will need to bear a label number in order to indicate to the canned cycle the block where the finishing operation is defined.

11.

; Definition of irregular pocket canned cycle. G66 R100 C200 F300 S400 E500 ; Defines the finishing operation. N300 G68...

B (5.5)

The function for the finishing operation is G68 and it cannot be executed independently from the G66.
Its programming format is: G68 B L Q J I R V F S T D M
Machining pass
Defines the pass in the plane between two 3D paths of the finishing operation. It must be defined and with a value other than "0".

IRREGULAR POCKET CANNED CYCLE 3D pockets

L (±5.5)

lateral finishing stock
Defines the value of the finishing stock on the side walls of the pocket left by the roughing and semi-finishing operations. There is no finishing stock left on top of the islands nor on the bottom of the pocket.
If programmed with a positive value, the finishing pass will be carried out in square corner (G07). If a negative value is programmed, the finishing pass will be carried out in G5 (round corner). If not programmed, the cycle assumes "L0".

CNC 8040
·M· MODEL (SOFT V11.1X)

Q (0/1/2)

Direction of the finishing pass

Indicates the direction of the finishing pass.

Q= 1:

All the passes will be inward from the top of the pocket to its bottom

Q= 2:

All the passes will be outward from the bottom of the pocket to the top.

Q=0:

Alternating direction for every 2 consecutive paths.

Any other value will generate the corresponding error message. If parameter "Q" is not programmed, the cycle assumes Q0.

212

J (5.5)

Programming manual

Tool tip radius

Indicates the tool tip radius and, therefore, the type of finishing tool being used.

Depending on the radius assigned to the tool in the tool offset table (of the CNC variables: "TOR" + "TOI") and the value of assigned to this parameter, three tool types may be defined.

FLAT

If J is not programmed or J = 0.

SPHERICAL If J = R.

TORIC

If J other than 0 and J smaller than R.

11.

IRREGULAR POCKET CANNED CYCLE 3D pockets

I (±5.5)
R (±5.5)
V (5.5) F (5.5) S (5.5) T (4)

Pocket depth
Defines the total depth of the pocket and is programmed in absolute coordinates. · If defined, the cycle will take it into account during the finishing operation. · If not defined and the pocket has a roughing operation, the cycle will assume the value defined for the roughing operation. · If not defined and the pocket has no roughing operation, but it has a semi-finishing operation, the cycle will assume the one define in the semi-finishing operation. · If the pocket has neither roughing nor semi-finishing operation, this parameter must be defined.
Reference plane
Defines the reference plane coordinate and is programmed in absolute coordinates. · If defined, the cycle will take it into account during the finishing operation. · If not defined and the pocket has a roughing operation, the cycle will assume the value defined for the roughing operation. · If not defined and the pocket has no roughing operation, but it has a semi-finishing operation, the cycle will assume the one define in the semi-finishing operation. · If the pocket has neither roughing nor semi-finishing operation, this parameter must be defined.
Penetration feedrate
Defines the tool penetrating feedrate.
If not programmed or programmed with a 0 value, it assumes 50% of the feedrate in the plane (F).
Machining feedrate
Optional. It sets the machining feedrate in the plane.
Spindle speed
Optional. It sets the spindle speed.
Tool number
Defines the tool used for the finishing operation. It must be programmed.

CNC 8040
·M· MODEL (SOFT V11.1X)

213

Programming manual
D (4) M
11.

Tool offset Optional. Defines the tool offset number.
Auxiliary (miscellaneous) functions Optional. Up to 7 miscellaneous M functions can be programmed. This operation allows M06 with an associated subroutine to be defined, and the tool change is performed before beginning the finishing operation.

IRREGULAR POCKET CANNED CYCLE 3D pockets

CNC 8040
·M· MODEL (SOFT V11.1X)
214

11.2.4 Geometry of the contours or profiles

Programming manual

To define the contours of a 2D pocket, the plane profile (3) and the depth profile (4) for all the contours must be defined (even if they are vertical).

11.

IRREGULAR POCKET CANNED CYCLE 3D pockets

Since the canned cycle applies the same depth profile to the whole contour, the same start point must be used to define the plane profile as for the depth profile.
CNC 8040
·M· MODEL (SOFT V11.1X)
215

Programming manual

3D contours with more than one depth profile are also possible. These contours are called "composite 3D profiles" and will be described later on.

11.

IRREGULAR POCKET CANNED CYCLE 3D pockets

CNC 8040
·M· MODEL (SOFT V11.1X)
216

11.2.5 Profile programming syntax

Programming manual

When programming inside or outside contours of an irregular 3D pocket (with islands) , the following rules must be complied with: 1. The profile in the main plane indicates the shape of the contour.
Since a 3D contour has an infinite number of different profiles (1 per each depth coordinate), the following must be programmed:
· For the outside contour of the pocket, the one for the surface coordinate (1). · For the inside contours: the one corresponding to the base or bottom (2).

11.

IRREGULAR POCKET CANNED CYCLE 3D pockets

2. The profile in the plane must be closed (same starting and end points) and it must not intersect itself. Examples:

The following examples cause a geometry error.

3. The depth profile (vertical cross section) must be programmed with any of the axes of the active plane. If the active plane is the XY and the perpendicular axis is the Z axis, one must program: G16XZ or G16YZ. All profiles, plane and depth, must start with the definition of the plane containing it.
G16 XY ; Beginning of the outside profile definition. ; - - Plane profile definition - G16 XZ ; - - Depth profile definition - -
G16 XY ; Beginning of the island definition. ; - - Plane profile definition - G16 XZ ; - - Depth profile definition - -

CNC 8040

·M· MODEL (SOFT V11.1X)

217

Programming manual
11.

4. The depth profile must be defined after having defined the plane profile. The beginning points of the plane profile and depth profile must be the same one. Nevertheless, the depth profile must be programmed: · For the outside contour of the pocket starting from the top or surface coordinate (1). · For the inside contours, islands, starting from the bottom or base coordinate (2).

IRREGULAR POCKET CANNED CYCLE 3D pockets

5. The depth profile must be open and without direction changes along its path. In other words, it cannot zig-zag.
The following examples cause a geometry error.

CNC 8040
·M· MODEL (SOFT V11.1X)
218

Programming example. 3D pocket without islands.

Programming manual

(TOR1=2.5,TOL1=20,TOI1=0,TOK1=0) G17 G0 G43 G90 Z50 S1000 M4 G5 ; Defines the 3D pocket. G66 R200 C250 F300 S400 E500 M30
; Roughing operation. N200 G67 B5 C4 I-30 R5 V100 F400 T1 D1 M6 ; Semi-finishing operation. N250 G67 B2 I-30 R5 V100 F550 T2 D1 M6 ; Finishing operation. N300 G68 B1.5 L0.75 Q0 I-30 R5 V80 F275 T3 D1 M6
; Definition of pocket geometry. N400 G17 ; Plane profile. G90 G0 X10 Y30 Z0 G1 Y90 X130 Y10 X10 Y30 ; Depth profile. G16 G0 X10 Z0 N500 G3 X40 Z-30 I30 K0

IRREGULAR POCKET CANNED CYCLE 3D pockets

11.
CNC 8040
·M· MODEL (SOFT V11.1X)
219

IRREGULAR POCKET CANNED CYCLE 3D pockets

Programming manual
11.

Programming examples. Profile definition.
Pyramid island
; Plane profile G17 G0 G90 X17 Y4 G1 X30 G1 Y30 G1 X4 G1 Y4 G1 X17
; Depth profile G16 YZ G0 G90 Y4 Z4 G1 Y17 Z35

Conic island

; Plane profile G17 G0 G90 X35 Y8 G2 X35 Y8 I0 J27
; Depth profile G16 YZ G0 G90 Y8 Z14 G1 Y35 Z55

Semi-spherical island

; Plane profile G17 G0 G90 X35 Y8 G2 X35 Y8 I0 J27
; Depth profile G16 YZ G0 G90 Y8 Z14 G2 Y35 Z41 R27

CNC 8040

·M· MODEL (SOFT V11.1X)

220

Programming example. 3D pocket without islands.

Programming manual

11.

IRREGULAR POCKET CANNED CYCLE 3D pockets

(TOR1=2.5,TOL1=20,TOI1=0,TOK1=0) G17 G0 G43 G90 Z50 S1000 M4 G5 ; Defines the 3D pocket. G66 R200 C250 F300 S400 E500 M30
; Roughing operation. N200 G67 B5 C4 I9 R25 V100 F400 T1D1 M6 ; Semi-finishing operation. N250 G67 B2 I9 R25 V100 F550 T2D1 M6 ; Finishing operation. N300 G68 B1.5 L0.75 Q0 I9 R25 V50 F275 T3D1 M6
; Definition of pocket geometry. N400 G17 ; External contour. Plane profile. G90 G0 X10 Y30 Z24 G1 Y50 X70 Y10 X10 Y30 ; Depth profile. G16 XZ G0 X10 Z24 G1 X15 Z9 ; Island definition. Plane profile. G17 G90 G0 X30 Y30 G2 X30 Y30 I10 K0 ; Depth profile. G16 XZ G90 G0 X30 Z9 N500 G1 X35 Z20

CNC 8040
·M· MODEL (SOFT V11.1X)
221

Programming manual
11.2.6 Composite 3D profiles
A "composite 3D profile" is a 3D contour with more than one depth profile.

11.

IRREGULAR POCKET CANNED CYCLE 3D pockets

It is defined by means of the intersection of several contours with different depth profiles.
Each contour is defined by a profile in the plane and a depth profile. All the contours must meet the following conditions:
· The plane profile must contain the corresponding sides completely. · Only a depth profile per contour must be defined. · The plane profile and the depth profile of the contour gathering several sides must
start at the same point.
The resulting plane profile will be formed by the intersection of the plane profiles of each element or contour.

Each wall of the resulting profile will assume the corresponding depth profile.

CNC 8040
·M· MODEL (SOFT V11.1X)
222

Profile intersection syntax

Programming manual

The plane profile intersecting rules are:
1. At a profile intersection, each contour is divided into several lines which could be grouped as:
· Lines external to the other contour.
· Lines internal to the other contour.
The starting point of each contour (x) determines the group of lines to be selected.
The following example shows the explained selection process. The solid lines indicate the lines external to the other contour and the dashes indicate the internal lines.

11.

IRREGULAR POCKET CANNED CYCLE 3D pockets

Examples of profile intersections: Boolean addition
Boolean subtraction

Boolean intersection

CNC 8040
·M· MODEL (SOFT V11.1X)
223

Programming manual
11.

2. The programming sequence for the different profiles is determinant when having an intersection of more than 3 profiles.
The profile intersection process is performed according to the order in which the profiles have been programmed. This way, the result of the intersection between the first two will be intersected with the third one and so forth.
The initial point of the resulting profiles always coincides with the initial point that defined the first profile.

IRREGULAR POCKET CANNED CYCLE 3D pockets

CNC 8040
·M· MODEL (SOFT V11.1X)
224

11.2.7 Profile stacking

Programming manual

When 2 or more profiles stack on top of each other, the following considerations must be taken into account.

For clarity sakes, refer to the drawing on the right that consists of 2 stacked profiles: 1 and 2.

11.

The base coordinate of the top profile (2) must coincide with the surface coordinate of the bottom profile (1).

IRREGULAR POCKET CANNED CYCLE 3D pockets

If there is a gap between them, the cycle will consider that they are 2 different profiles and it will eliminate the top profile when executing the bottom one.
If the profiles mix, the canned cycle will make a groove around the top profile when running the finishing pass.

CNC 8040
·M· MODEL (SOFT V11.1X)
225

Programming manual
11.2.8 Profile programming syntax

11.

The outside profile and the inside profiles or islands which are programmed must be defined by simple geometrical elements such as straight lines or arcs.
The first definition block (where the external profile starts) and the last (where the last profile defined ends) must be provided with the block label number. These label numbers will indicate the beginning and end of the profile geometry definition for the profiles that make up the pocket.
; Definition of irregular pocket canned cycle. G66 R100 C200 F300 S400 E500 ; Geometrical description. N400 G17 ... N500 G2 G6 X300 Y50 I150 J0

IRREGULAR POCKET CANNED CYCLE 3D pockets

CNC 8040
·M· MODEL (SOFT V11.1X)

The profile programming syntax must follow these rules: · The first profile defining block must have a label number to indicate to the G66 canned cycle the beginning of the geometry description. · First, the outside pocket contour must be defined and, then, the contour of each island. · When a contour has more than one depth profile, the contours must be defined one by one indicating, on each one, the plane profile and, then, its depth profile. · The first profile defining block of the plane profile as well as that of the depth profile must contain function G00 (indicative of the beginning of the profile). Care must be taken to program G01, G02 or G03 in the block following the definition of the beginning, as G00 is modal, thus preventing the CNC from interpreting the following blocks as the beginnings of a new profile. · The last profile defining block must have a label number to indicate to the G66 canned cycle the end of the geometry description.
; Definition of irregular pocket canned cycle. G66 R200 C250 F300 S400 E500
; Beginning of the definition of pocket geometry. N400 G17 ; External contour. Plane profile. G0 G90 X5 Y-26 Z0 --- --- --- --; Depth profile. G16 XZ G0 --- ----- --- --- --; Island definition G17 ; Plane profile. G0 X30 Y-6 --- --- --- --; Depth profile. G16 XZ G0 --- --- --- --; End of geometric description. N500G3 Y-21 Z0 J-5 K0

226

Programming manual

In addition to the G00 function, which has a special meaning, the irregular pocket canned cycle allows the use of the following functions for the definition of profiles.

G01

Linear interpolation.

G02

Clockwise circular interpolation.

G03

Counter-clockwise circular interpolation.

G06

Circle center in absolute coordinates.

G08

Arc tangent to previous path.

G09

Arc defined by three points.

G16

Main plane selection by two addresses and longitudinal axis.

G17

Main plane X-Y, and longitudinal axis Z.

G18

Main plane Z-X, and longitudinal axis Y.

G19

Main plane Y-Z, and longitudinal axis X.

G36

Corner rounding, radius blend.

G39

Chamfer.

G53

Programming with respect to machine zero.

G70

Programming in inches.

G71

Programming in millimeters.

G90

Absolute programming.

G91

Incremental programming.

G93

Polar origin preset.

IRREGULAR POCKET CANNED CYCLE 3D pockets

11.

CNC 8040
·M· MODEL (SOFT V11.1X)
227

Programming manual
11.2.9 Programming examples
Programming example ·1·
11.

IRREGULAR POCKET CANNED CYCLE 3D pockets

In this example, the island has 3 types of depth profiles: A, B and C. 3 contours are used to define the island: A-type contour, B-type contour and C-type contour.

CNC 8040
·M· MODEL (SOFT V11.1X)
228

; Tool dimensions. (TOR1=2.5,TOL1=20,TOI1=0,TOK1=0)
; Initial positioning and definition of the 3D pocket. G17 G0 G43 G90 Z50 S1000 M4 G5 G66 R200 C250 F300 S400 E500 M30
; Definition of roughing operation. N200 G67 B5 C4 I-20 R5 V100 F400 T1D1 M6
; Definition of the semi-finishing operation N250 G67 B2 I-20 R5 V100 F550 T2D1 M6
; Definition of finishing operation. N300 G68 B1.5 L0.75 Q0 I-20 R5 V80 F275 T3 D1 M6

; Definition of pocket geometry. Blocks N400 through N500. N400 G17
; Definition of A-type contour. Plane profile. G0 G90 X50 Y90 Z0 G1 X0 Y10 X100 Y90 X50
; Depth profile. G16 YZ G0 G90 Y90 Z0 G1 Z-20
; Definition of B-type contour. Plane profile. G17 G0 G90 X10 Y50 G1 Y100 X -10 Y0 X10 Y50 ; Depth profile. G16 XZ G0 G90 X10 Z0 G1 X20 Z-20
; Definition of C-type contour. Plane profile. G17 G0 G90 X90 Y50 G1 Y100 X110 Y0 X90 Y50 ; Depth profile. G16 XZ G0 G90 X90 Z0 N500 G2 X70 Z-20 I-20 K0

Programming manual
11.
CNC 8040

IRREGULAR POCKET CANNED CYCLE 3D pockets

·M· MODEL (SOFT V11.1X)

229

Programming manual

Programming example ·2·

11.

IRREGULAR POCKET CANNED CYCLE 3D pockets

CNC 8040
·M· MODEL (SOFT V11.1X)
230

In this example, the island has 3 types of depth profiles: A, B and C. 3 contours are used to define the island: A-type contour, B-type contour and C-type contour.
; Tool dimensions. (TOR1=7.5,TOI1=0,TOR2=5,TOI2=0,TOR3=2.5,TOI3=0) ; Initial positioning and definition of the 3D pocket. G17 G0 G43 G90 Z50 S1000 M4 G5 G66 R200 C250 F300 S400 E500 M30 ; Definition of roughing operation. N200 G67 B7 C14 I-25 R3 V100 F500 T1 D1 M6 ; Definition of the semi-finishing operation N250 G67 B3 I-25 R3 V100 F625 T2 D2 M6 ; Definition of finishing operation. N300 G68 B1 L1 Q0 J0 I-25 R3 V100 F350 T3 D3 M6 ; Definition of pocket geometry. Blocks N400 through N500. N400 G17

; Definition of outside contour. Plane profile. G0 G90 X0 Y0 Z0 G1 X150 Y100 X0 Y0 ; Depth profile. G16 XZ G0 G90 X0 Z0 G1 X10 Z-10
; Definition of A-type contour. Plane profile. G17 G0 G90 X50 Y30 G1 X70 Y70 X35 Y30 X50 ; Depth profile. G16 YZ G0 G90 Y30 Z-25 G2 Y50 Z-5 J20 K0
; Definition of B-type contour. Plane profile. G17 G0 G90 X40 Y50 G1 Y25 X65 Y75 X40 Y50 ; Depth profile. G16 XZ G0 G90 X40 Z-25 G1 Z-5
; Definition of C-type contour. Plane profile. G17 G90 X80 Y40 G0 X96 G1 Y60 X60 Y40 X80 ; Depth profile. G16 YZ G0 G90 Y40 Z-25 N500 G2 Y50 Z-15 J10 K0

Programming manual
11.
CNC 8040
·M· MODEL (SOFT V11.1X)
231

IRREGULAR POCKET CANNED CYCLE 3D pockets

Programming manual

Programming example ·3·

11.

In this example, the island has 3 types of depth profiles: A, B and C. 3 contours are used to define the island: A-type contour, B-type contour and C-type contour.

IRREGULAR POCKET CANNED CYCLE 3D pockets

CNC 8040
·M· MODEL (SOFT V11.1X)
232

; Tool dimensions. (TOR1=4,TOI1=0,TOR2=2.5,TOI2=0)
; Initial positioning and definition of the 3D pocket. G17 G0 G43 G90 Z25 S1000 M3 G66 R200 C250 F300 S400 E500 M30
; Definition of roughing operation. N200 G67 B5 C4 I-20 R5 V100 F700 T1 D1 M6
; Definition of the semi-finishing operation N250 G67 B2 I-20 R5 V100 F850 T1 D1 M6
; Definition of finishing operation. N300 G68 B1.5 L0.25 Q0 I-20 R5 V100 F500 T2 D2 M6

; Definition of pocket geometry. Blocks N400 through N500. N400 G17
; Definition of outside contour. Plane profile. G0 G90 X0 Y0 Z0 G1 X105 Y62 X0 Y0 ; Depth profile. G16 XZ G0 X0 Z0 G2 X5 Z-5 I0 K-5 G1 X7.5 Z-20
; Definition of A-type contour. Plane profile. G17 G90 G0 X37 Y19 G2 I0 J12 ; Depth profile. G16 YZ G0 Y19 Z-20 G1 Z-16 G2 Y31 Z-4 R12
; Definition of B-type contour. Plane profile. G17 G90 G0 X60 Y37 G1 X75 Y25 X40 Y37 ; Depth profile. G16 YZ G0 Y37 Z-20 G1 Z-13 G3 Y34 Z-10 J-3 K0
; Definition of C-type contour. Plane profile. G17 G0 X70 Y31 G1 Y40 X80 Y20 X70 Y31 ; Depth profile. G16 XZ G0 X70 Z-20 N500 G1 X65 Z-10

Programming manual
11.
CNC 8040
·M· MODEL (SOFT V11.1X)
233

IRREGULAR POCKET CANNED CYCLE 3D pockets

Programming manual

Programming example ·4·

11.

To define the island 10 contours are used as shown here:

IRREGULAR POCKET CANNED CYCLE 3D pockets

CNC 8040
·M· MODEL (SOFT V11.1X)
234

Programming manual
11.

IRREGULAR POCKET CANNED CYCLE 3D pockets

; Tool dimensions. (TOR1=4,TOI1=0,TOR2=2.5,TOI2=0)
; Initial positioning and definition of the 3D pocket. G17 G0 G43 G90 Z25 S1000 M3 G66 R200 C250 F300 S400 E500 M30
; Definition of roughing operation. N200 G67 B5 C0 I-30 R5 V100 F700 T1 D1 M6
; Definition of the semi-finishing operation N250 G67 B1.15 I-29 R5 V100 F850 T1 D1 M6
; Definition of finishing operation. N300 G68 B1.5 L0.25 Q0 I-30 R5 V100 F500 T2 D2 M6
; Definition of pocket geometry. Blocks N400 through N500. N400 G17
; Definition of outside contour. Plane profile. G90 G0 X-70 Y20 Z0 G1 X70 Y -90 X -70 Y20

CNC 8040
·M· MODEL (SOFT V11.1X)
235

IRREGULAR POCKET CANNED CYCLE 3D pockets

Programming manual
11.
CNC 8040
·M· MODEL (SOFT V11.1X)

; Definition of contour 1. Plane profile. G17 G90 G0 X42.5 Y5 G1 G91 X-16 Y -60 X32 Y60 X -16 ; Depth profile. G16 YZ G0 G90 Y5 Z-30 G3 Y-25 Z0 J-30 K0 ; Definition of contour 2. G17 G0 X27.5 Y-25 G1 G91 Y31 G1 X-2 Y -62 X2 Y31 ; Depth profile. G16 XZ G0 G90 X27.5 Z-30 G1 Z0 ; Definition of contour 3. G17 G0 X57.5 Y-25 G1 G91 Y-31 X2 Y62 X -2 Y -31 ; Depth profile. G16 XZ G0 G90 X57.5 Z-30 G1 Z0 ; Definition of contour 4. G17 G0 X0 Y-75 G1 G91 X-31 Y -2 X62 Y2 X -31 ; Depth profile. G16 YZ G0 G90 Y-75 Z-30 G1 Z0

236

; Definition of contour 5. G17 G0 X-30 Y-60 G1 G91 Y-16 X60 Y32 X -60 Y -16 ; Depth profile. G16 XZ G0 G90 X-30 Z-30 G2 X0 Z0 I30 K0 ; Definition of contour 6. G17 G0 X0 Y-45 G1 G91 X31 Y2 X -62 Y -2 X31 ; Depth profile. G16 YZ G0 G90 Y-45 Z-30 G1 Z0 ; Definition of contour 7. G17 G0 X-57.5 Y-25 G1 G91 Y31 X -2 Y -62 X2 Y31 ; Depth profile. G16 XZ G0 G90 X-57.5 Z-30 G1 Z0 ; Definition of contour 8. G17 G0 X-42.5 Y5 G1 G91 X-16 Y -60 X32 Y60 X -16 ; Depth profile. G16 YZ G0 G90 Y5 Z-30 G3 Y-25 Z0 J-30 K0

Programming manual
11.
CNC 8040
·M· MODEL (SOFT V11.1X)
237

IRREGULAR POCKET CANNED CYCLE 3D pockets

Programming manual
11.

; Definition of contour 9. G17 G0 X-27.5 Y-25 G1 G91 Y-31 X2 Y62 X -2 Y -31 ; Depth profile. G16 XZ G0 G90 X27.5 Z-30 G1 Z0 ; Definition of contour 10. G17 G0 X0 Y0 G1 X-28 Y -50 X28 Y0 X0 ; Depth profile. G16 YZ G0 Y0 Z-30 N500 G3 Y-25 Z-5 J-25 K0

CNC 8040
·M· MODEL (SOFT V11.1X)
238

Programming example ·5·

Programming manual
11.

IRREGULAR POCKET CANNED CYCLE 3D pockets

In this example, the island has 2 types of depth profiles: A and B. 2 contours are used to define the island: the low contour (A-type) and the high contour (B-type).

; Tool dimensions. (TOR1=2.5,TOL1=20,TOI1=0,TOK1=0)
; Initial positioning and definition of the 3D pocket. G17 G0 G43 G90 Z50 S1000 M4 G5 G66 R200 C250 F300 S400 E500 M30
; Definition of roughing operation. N200 G67 B5 C4 I-25 R5 V100 F400 T1 D1 M6
; Definition of the semi-finishing operation N250 G67 B2 I-25 R5 V100 F550 T2 D1 M6
; Definition of finishing operation. N300 G68 B1.5 L0.75 Q0 I-25 R5 V100 F275 T3 D1 M6
; Definition of pocket geometry. Blocks N400 through N500. N400 G17

CNC 8040
·M· MODEL (SOFT V11.1X)
239

IRREGULAR POCKET CANNED CYCLE 3D pockets

Programming manual
11.

; Definition of outside contour. Plane profile. G90 G0 X5 Y-26 Z0 G1 Y25 X160 Y -75 X5 Y -26
; Definition of the low (A-type) contour. Plane profile. G17 G90 G0 X30 Y-6 G1 Y-46 X130 Y -6 X30 ; Depth profile. G16 XZ G0 X30 Z-25 G1 Z-20 G2 X39 Z-11 I9 K0
; Definition of the high (B-type) contour. Plane profile. G17 G90 G0 X80 Y-16 G2 I0 J-10 ; Depth profile. G16 YZ G0 Y-16 Z-11 G1 Y-16 Z-5 N500 G3 Y-21 Z0 J-5 K0

CNC 8040
·M· MODEL (SOFT V11.1X)
240

11.2.10 Errors

Programming manual

ERROR 1025 ERROR 1026 ERROR 1041
ERROR 1042
ERROR 1043
ERROR 1044 ERROR 1046 ERROR 1047 ERROR 1048 ERROR 1049

The CNC will issue the following errors:
A tool with no radius has been programmed
It comes up when using a tool with "0" radius while machining a 3D pocket.
A step has been programmed that is larger than the tool diameter
When parameter "C" of the roughing operation is greater than the diameter of the roughing tool.
A parameter required in the canned cycle has not been programmed.
It comes up in the following instances: · When parameters "I" and "R" have not been programmed in the roughing operation. · When not using a roughing operation and not programming the "I" and "R" parameters for the semi-finishing operation. · When not using a semi-finishing operation and not programming the "I" and "R" parameters for the finishing operation. · When parameter "B" has not been programmed in the finishing operation.
Wrong parameter value in the canned cycle
It comes up in the following instances: · When parameter "Q" of the finishing operation has the wrong value. · When parameter "B" of the finishing operation has a "0" value. · When parameter "J" of the finishing operation has been programmed with a value greater than the finishing tool radius.
Wrong depth profile in a pocket with islands.
It comes up in the following instances: · When the depth profiles of 2 sections of the same contour (simple or composite) cross each other · When the finishing operation cannot be performed with the programmed tool. A typical case is a spherical mold with a non-spherical tool (parameter "J" not equal to the radius).
The plane profile intersects itself in an irregular pocket with islands.
It comes up when any of the plane profiles of the programmed contours intersects itself.
Wrong tool position prior to the canned cycle
It comes up when calling the G66 cycle if the tool is positioned between the reference plane and the depth coordinate (bottom) of any of the operations.
Open plane profile in an irregular pocket with islands
It comes up when any of the programmed contours does not begin and end at the same point. It may be because G1 has not been programmed after the beginning, with G0, on any of the profiles.
Part surface coordinate not programmed in pocket with islands
It comes up when the first point of the geometry does not include the pocket top coordinate.
Wrong reference plane coordinate for the canned cycle.
It comes up when the coordinate of the reference plane is located between the part's "top" and "bottom" in any of the operations.

IRREGULAR POCKET CANNED CYCLE 3D pockets

11.
CNC 8040
·M· MODEL (SOFT V11.1X)

241

Programming manual ERROR 1084
ERROR 1227
11.

Arc programmed wrong'
It comes up when any of the paths programmed in the geometry definition of the pocket is wrong.
Wrong profile intersection in a pocket with islands.
It comes up in the following instances: · When two plane profiles have a common section (drawing on the left). · When the initial points of two profiles in the main plane coincide (drawing on the right).

IRREGULAR POCKET CANNED CYCLE 3D pockets

CNC 8040
·M· MODEL (SOFT V11.1X)
242

PROBING

The CNC has two probe inputs, one for TTL-type 5Vdc signals and another for 24 Vdc signals.
The connection of the different types of probes to these inputs are explained in the appendix to the Installation manual.
This control allows the following operations to be performed, by using probes: · Programming probing blocks with functions G75 and G76. · Execution of the various tool calibration, part-measurement and part centering cycles by means of high-level language programming.

CNC 8040
·M· MODEL (SOFT V11.1X)
243

Programming manual
12.1 Probing (G75, G76)

12.

PROBING Probing (G75, G76)

The G75 function allows movements to be programmed that will end after the CNC receives the signal from the measuring probe used.
The G76 function allows movements to be programmed that will end after the CNC no longer receives the signal from the measuring probe used.
Their definition format is: G75 X..C ±5.5 G76 X..C ±5.5
After G75 or G76, the required axis or axes will be programmed, as well as the coordinates of these axes that will define the end point of the programmed movement.
The machine will move according to the programmed path until it receives the signal from the probe (G75) or until it no longer receives the probe signal (G76). At this time, the CNC will consider the block finished, taking as the theoretical position of the axes the real position they have at that time.
If the axes reach the programmed position before receiving or while receiving the external signal from the probe, the CNC will stop the movement of the axes.
This type of movement with probing blocks are very useful when it is required to generate measurement or verification programs for tools and parts.
Functions G75 and G76 are not modal and, therefore, must be programmed whenever it is wished to probe.
Functions G75 and G76 are incompatible with each other and with G00, G02, G03, G33, G34, G41 and G42 functions. In addition, once this has been performed, the CNC will assume functions G01 and G40.
During G75 or G76 moves, the operation of the feedrate override switch depends on the setting of OEM machine parameter FOVRG75.

CNC 8040
·M· MODEL (SOFT V11.1X)
244

12.2 Probing canned cycles

Programming manual

The CNC has the following probing canned cycles: · Tool calibrating canned cycle. · Probe calibrating canned cycle. · Surface measuring canned cycle. · Outside corner measuring canned cycle. · Inside corner measuring canned cycle. · Angle measuring canned cycle. · Corner and angle measuring canned cycle. · Hole measuring canned cycle. · Boss measuring canned cycle. · Rectangular part centering canned cycle. · Circular part centering canned cycle.
All the movements of these probing canned cycles will be performed in the X, Y, Z axes and the work plane must be formed by 2 of these axes (XY, XZ, YZ, YX, ZX, ZY). The other axis must be perpendicular and it must be selected as the longitudinal axis.
Canned cycles will be programmed by means of the high level mnemonic, PROBE, which has the following programming format:
(PROBE (expression), (assignment instruction),...)
This instruction PROBE calls the probing cycle indicated by means of a number or any expression which results in a number. Besides, it allows the parameters of this cycle to be initialized with the values required to perform it, by means of assignment instructions.
General considerations
Probing canned cycles are not modal, and therefore must be programmed whenever it is required to perform any of them.
The probes used in the performance of these cycles are: · Probe placed on a fixed position on the machine, used for calibrating tools. · Probe placed in the spindle, will be treated as a tool and will be used in the different measuring cycles.
The execution of a probing canned cycle does not alter the history of previous "G" functions, except for the radius compensation functions G41 and G42.

PROBING Probing canned cycles

12.

CNC 8040
·M· MODEL (SOFT V11.1X)
245

Programming manual
12.3 PROBE 1. Tool length calibrating canned cycle

12.

PROBING PROBE 1. Tool length calibrating canned cycle

This is used to calibrate the length and radius of the selected tool. The following operations are possible with this cycle.
· To calibrate the tool length. · To calibrate the tool radius. · To calibrate the tool radius and length. · Measure the tool length wear. · Measure the tool radius wear. · Measure the tool radius wear and length wear.
To perform this cycle it is necessary to have a table-top probe, installed in a fixed position on the machine and with its faces parallel to axes X, Y, Z. Its position will be indicated in absolute coordinates with respect to machine zero by means of the general machine parameters:
PRBXMIN Indicates the minimum coordinate occupied by the probe along the X axis.
PRBXMAX Indicates the maximum coordinate occupied by the probe along the X axis.
PRBYMIN Indicates the minimum coordinate occupied by the probe along the Y axis.
PRBYMAX Indicates the maximum coordinate occupied by the probe along the Y axis.
PRBZMIN Indicates the minimum coordinate occupied by the probe along the Z axis.
PRBZMAX Indicates the maximum coordinate occupied by the probe along the Z axis.

CNC 8040
·M· MODEL (SOFT V11.1X)
246

If it is the first time that the tool length has been calibrated, it is advisable to include an approximate value of its length (L) in the tool offset table.

Programming format

Programming manual

The programming format of this cycle is as follows. (PROBE 1, B, I, F, J, K, L, C, D, E, S, M, C, N, X, U, Y, V, Z, W)
Certain parameters are only relevant in certain type of measurement. Later sections describe the various options of this cycle and the parameters to be set in each one.
Parameters X, U, Y, V, Z, W.
Define the probe position. They are optional parameters that are not usually necessary. On certain machines, due to lack of mechanical positioning repeatability of the probe's, the probe must be calibrated before each tool calibration.
Instead of redefining machine parameters PRBXMIN, PRBXMAX, PRBYMIN, PRBYMAX, PRBZMAX, PRBZMIN every time the probe is calibrated, those coordinates may be indicated in parameters X, U, Y, V, Z, W, respectively.
The CNC does not modify the machine parameters. The CNC only takes into account the coordinates indicated in X, U, Y, V, Z, W during this calibration. If any of the X, U, Y, V, Z is left out, the CNC takes the value assigned to the corresponding machine parameter.

12.

PROBING PROBE 1. Tool length calibrating canned cycle

CNC 8040
·M· MODEL (SOFT V11.1X)
247

Programming manual
12.3.1 Calibrate the length or measure the length wear of a tool.

12.

PROBING PROBE 1. Tool length calibrating canned cycle

B5.5 I

The type of operation (calibration or measurement) is selected when calling the cycle.
The calibration or measurement may be done on the tool shaft or on its tip. It is selected when calling the canned cycle.
The programming format depends on the operation to carry out: · Tool length calibration along its shaft. (PROBE 1, B, I0, F, J0, X, U, Y, V, Z, W) · Tool length calibration at its tip. (PROBE 1, B, I1, F, J0, D, S, N, X, U, Y, V, Z, W) · Measurement of the tool length wear along its shaft. (PROBE 1, B, I0, F, J1, L, C, X, U, Y, V, Z, W) · Measurement of the tool length wear at its tip. (PROBE 1, B, I1, F, J1, L, D, S, C, N, X, U, Y, V, Z, W)

Safety distance It must be programmed with a positive value greater than 0.

Type of calibration or wear measurement

The calibration may be done on the tool shaft or on its tip.

I = 0

Calibration of the tool length or measurement of the tool length

wear along its shaft.

I = 1

Calibration of the tool length or measurement of the tool length

wear on its tip.

If not programmed, the cycle will assume the IO value.

I = 0. Tool calibration along its shaft. It is useful for drilling tools, ball end-mills, or tools whose diameter is smaller than the probe's probing surface. This type of calibration is carried out with the spindle stopped.

CNC 8040

I = 1. Tool calibration at its tip.
It is useful for calibrating tools with several cutting edges (endmills), or tools whose diameter is larger than the probe's probing surface.
This type of calibration may be carried out either with the spindle stopped or turning in the opposite direction to the cutting direction.

F5.5

Probing feedrate It sets the probing feedrate. It must be programmed in mm/minute or inches/minute.

·M· MODEL (SOFT V11.1X)

248

J L5.5 D5.5 S±5.5 C N X U Y V Z W

Programming manual

Type of operation

The calibration may be done on the tool shaft or on its tip.

J = 0

Tool calibration.

J = 1

Tool wear measurement.

Maximum length wear allowed
When set to 0, the tool is not rejected due to length wear. The tool is rejected when measuring a wear greater than the one defined.
Only if J1 has been defined and tool life monitoring is being used. If this is not programmed, the canned cycle will take the value of L0.

12.

PROBING PROBE 1. Tool length calibrating canned cycle

Distance from the tool shaft to the probing point It sets the radius or distance referred to the tool shaft being probed. If not defined, probing is carried out on the tool tip.

Speed and turning direction of the tool
To probe with the spindle running, the tool must be turning in the opposite direction to the cutting direction.
· When set to 0, probing is carried out with the spindle stopped. · When set with a positive value, the spindle starts in M3. · When set with a negative value, the spindle starts in M4.

Behavior when exceeding the amount of wear allowed

Only if "L" has been set to other than zero.

C = 0

Interrupts the execution for the user to select another tool.

C = 1

The cycle replaces the tool with another one of the same family.

If not programmed, the cycle will assume the C0 value.

Number of edges to measure
When set to zero, it only takes one measurement. If not programmed, the cycle will assume the N0 value.
To measure each cutting edge when the spindle has feedback and s.m.p. M19TYPE (P43) =1.

Probe position Optional parameters. See "Programming format" on page 247.

Actions after finishing the cycle

Once the calibration cycle has ended

It updates global arithmetic parameter P299 and assigns the measured length to the tool offset selected in the tool offset table.

P299

"Measured length" - "Previous length (L+K)".

Measured length.

CNC 8040
·M· MODEL (SOFT V11.1X)

249

Programming manual
12.

Once the wear measuring cycle has ended
· When using tool live monitoring.
In this case, it compares the measured value with the theoretical length assigned in the table. If the maximum allowed is exceeded, it issues a "tool rejected" message and acts as follows:

C0 It interrupts the execution for the user to select another tool.

C1 The cycle replaces the tool with another one of the same family. It sets the "rejected tool" indicator (Status = R) It activates the general logic output PRTREJEC (M5564).

· If tool life monitoring is not available or the measuring difference does not exceed the maximum allowed.

In this case, it updates global arithmetic parameter P299 and the length wear value of the tool offset selected in the tool offset table.

P299

"Measured length" - "Theoretical length (L)".

Theoretical length. It maintains the previous value.

"Measured length" - "Theoretical length (L)". New wear value.

If the dimension of each cutting edge was requested ("N" parameter) the measured values are assigned to global arithmetic parameters P271 and on.

PROBING PROBE 1. Tool length calibrating canned cycle

CNC 8040
·M· MODEL (SOFT V11.1X)
250

Programming manual
12.3.2 Calibrate the radius or measure the radius wear of a tool

B5.5 I F5.5 J K
E5.5

The type of operation (calibration or measurement) is selected when calling the cycle.
The programming format depends on the operation to carry out: · Tool radius Calibration. (PROBE 1, B, I2, F, J0, K, E, S, N, X, U, Y, V, Z, W) · Radius wear measurement. (PROBE 1, B, I2, F, J1, K, E, S, M, C, N, X, U, Y, V, Z, W)

Safety distance It must be programmed with a positive value greater than 0.

Type of calibration or wear measurement

The calibration may be done on the tool shaft or on its tip.

I = 2

Calibrate the radius or measure the radius wear of a tool.

If not programmed, the cycle will assume the IO value.

Probing feedrate It sets the probing feedrate. It must be programmed in mm/minute or inches/minute.

Type of operation

J = 0

Tool calibration.

J = 1

Tool wear measurement.

Probe side used

It sets the probe side being used to probe the radius.

K = 0

Side X+.

K = 1

Side X-.

K = 2

Side Y+.

K = 3

Side Y-.

Distance from the tool tip to the probing point. Distance referred to the theoretical tool tip being probed. This parameter may be very useful with cutters whose bottom is not horizontal. If not programmed, the cycle will assume the E0 value.

PROBING PROBE 1. Tool length calibrating canned cycle

12.

CNC 8040
·M· MODEL (SOFT V11.1X)
251

Programming manual
S±5.5

PROBING PROBE 1. Tool length calibrating canned cycle

12.

M5.5

N X U Y V Z W

Maximum radius wear allowed
When set to 0, the tool is not rejected due to radius wear. The tool is rejected when measuring a wear greater than the one defined.
Only if J1 has been defined and tool life monitoring is being used. If not programmed, a value of M0 will be assumed.

Behavior when exceeding the amount of wear allowed

Only if "M" has been set to other than zero.

C = 0

Interrupts the execution for the user to select another tool.

C = 1

The cycle replaces the tool with another one of the same family.

If not programmed, the cycle will assume the C0 value.

Probe position Optional parameters. See "Programming format" on page 247.

Actions after finishing the cycle

Once the calibration cycle has ended

It updates global arithmetic parameter P298 and assigns the measured radius to the tool offset selected in the tool offset table.

P298

"Measured radius" - "Previous radius (R+I)".

Measured radius.

CNC 8040
·M· MODEL (SOFT V11.1X)
252

Programming manual

Once the wear measuring cycle has ended
· When using tool live monitoring.
In this case, it compares the measured value with the theoretical radius assigned in the table. If the maximum allowed is exceeded, it issues a "tool rejected" message and acts as follows:

C0 It interrupts the execution for the user to select another tool.

C1 The cycle replaces the tool with another one of the same family. It sets the "rejected tool" indicator (Status = R) It activates the general logic output PRTREJEC (M5564).

· If tool life monitoring is not available or the measuring difference does not exceed the maximum allowed.

In this case, it updates global arithmetic parameter P298 and the radius wear value of the tool offset selected in the tool offset table.

P298

"Measured radius" - "Theoretical radius (R)".

Theoretical radius. It maintains the previous value.

"Measured radius" - "Theoretical radius (R)". New wear value.

If the dimension of each cutting edge was requested ("N" parameter) the measured values are assigned to global arithmetic parameters P251 and on.

12.

PROBING PROBE 1. Tool length calibrating canned cycle

CNC 8040
·M· MODEL (SOFT V11.1X)
253

Programming manual
12.3.3 Measure or calibrate the tool radius wear and tool length wear.

12.

PROBING PROBE 1. Tool length calibrating canned cycle

B5.5 I F5.5 J K
L5.5
D5.5

The type of operation (calibration or measurement) is selected when calling the cycle.
The programming format depends on the operation to carry out: · Tool radius Calibration. (PROBE 1, B, I3, F, J0, K, D, E, S, N, X, U, Y, V, Z, W) · Radius wear measurement. (PROBE 1, B, I3, F, J1, K, L, D, E, S, M, C, N, X, U, Y, V, Z, W)

Safety distance It must be programmed with a positive value greater than 0.

Type of calibration or wear measurement

The calibration may be done on the tool shaft or on its tip.

I = 3

Measure or calibrate the tool radius wear and tool length wear.

If not programmed, the cycle will assume the IO value.

Probing feedrate It sets the probing feedrate. It must be programmed in mm/minute or inches/minute.

Type of operation

J = 0

Tool calibration.

J = 1

Tool wear measurement.

Probe side used

It sets the probe side being used to probe the radius.

K = 0

Side X+.

K = 1

Side X-.

K = 2

Side Y+.

K = 3

Side Y-.

Distance from the tool shaft to the probing point It sets the radius or distance referred to the tool shaft being probed. If not defined, probing is carried out on the tool tip.

CNC 8040

·M· MODEL (SOFT V11.1X)

254

E5.5

Programming manual
Distance from the tool tip to the probing point. Distance referred to the theoretical tool tip being probed. This parameter may be very useful with cutters whose bottom is not horizontal. If not programmed, the cycle will assume the E0 value.

S±5.5 M5.5 C N X U Y V Z W

Behavior when exceeding the amount of wear allowed

Only if "M" or "L" has been set to other than zero.

C = 0

Interrupts the execution for the user to select another tool.

C = 1

The cycle replaces the tool with another one of the same family.

If not programmed, the cycle will assume the C0 value.

Probe position Optional parameters. See "Programming format" on page 247.

PROBING PROBE 1. Tool length calibrating canned cycle

12.

CNC 8040
·M· MODEL (SOFT V11.1X)

255

PROBING PROBE 1. Tool length calibrating canned cycle

Programming manual
12.

Actions after finishing the cycle

Once the calibration cycle has ended

It updates global arithmetic parameter P298 and assigns the measured radius to the tool offset selected in the tool offset table.

P298

"Measured radius" - "Previous radius (R+I)".

P299

"Measured length" - "Previous length (L+K)".

Measured radius.

Measured length.

Once the wear measuring cycle has ended
· When using tool live monitoring.
In this case, it compares the measured radius and length with the theoretical values in the table. If the maximum allowed is exceeded, it issues a "tool rejected" message and acts as follows:

C0 It interrupts the execution for the user to select another tool.

C1 The cycle replaces the tool with another one of the same family. It sets the "rejected tool" indicator (Status = R) It activates the general logic output PRTREJEC (M5564).

· If tool life monitoring is not available or the measuring difference does not exceed the maximum allowed.

In this case, it updates global arithmetic parameters P298 and P299 as well as the radius wear and length wear value of the tool offset selected in the tool offset table.

P298

"Measured radius" - "Theoretical radius (R)".

P299

"Measured length" - "Theoretical length (L)".

Theoretical radius. It maintains the previous value.

"Measured radius" - "Theoretical radius (R)". New wear value.

Theoretical length. It maintains the previous value.

"Measured length" - "Theoretical length (L)". New wear value.

If the dimension of each cutting edge was requested, parameter "N", the lengths are assigned to global arithmetic parameters P271 and on; the radii are assigned to global arithmetic parameters P251 and on.

CNC 8040
·M· MODEL (SOFT V11.1X)
256

12.4 PROBE 2. Probe calibration canned cycle.

Programming manual

This is used to calibrate the probe located in the tool holding spindle. This probe which previously must be calibrated in length, will be the one used in probe measuring canned cycles.
The cycle measures the deviation which the probe ball axis has with respect to the tool holder axis, using a previously machined hole with known center and dimensions for its calibration.

12.

PROBING PROBE 2. Probe calibration canned cycle.

The CNC will treat each measuring probe used as just one more tool. The tool offset table fields corresponding to each probe will have the following meaning:

Radius of the sphere (ball) of the probe. This value will be loaded

into the table manually.

Length of the probe. This value will be indicated by the tool length

calibration cycle.

Deviation of the probe ball with respect to the tool-holder axis,

along the abscissa axis. This value will be indicated by the cycle.

Deviation of the probe ball with respect to the tool-holder axis,

along the ordinate axis. This value will be indicated by the cycle.

The following steps will be followed for its calibration:
1. Once the characteristics of the probe have been consulted, the value for the sphere radius (R) will be entered manually in the corresponding tool offset.
2. After selecting the corresponding tool number and tool offset the Tool Length Calibration Cycle will be performed, the value of (L) will be updated and the value of (K) will be initialized to 0.
3. Execution of the probe calibration canned cycle, updating the "I" and "K" values.

CNC 8040
·M· MODEL (SOFT V11.1X)
257

Programming manual

12.

PROBING PROBE 2. Probe calibration canned cycle.

X±5.5 Y±5.5 Z±5.5 B5.5 J5.5
E5.5
H5.5
F5.5

The programming format for this cycle is: (PROBE 2, X, Y, Z, B, J, E, H, F)
Real coordinate, along the X axis, of the hole center.
Real coordinate, along the Y axis, of the hole center.
Real coordinate, along the Z axis, of the hole center.
Safety distance Defines the safety distance. Must be programmed with a positive value and over 0.
Real diameter of the hole. Defines the real diameter of the hole. Must be programmed with a positive value and over 0.
Withdrawal distance Defines the distance which the probe moves back after initial probing. Must be programmed with a positive value and over 0.
Initial probing feedrate Defines the feedrate for the initial probing movement. It must be programmed in mm/ minute or inches/minute.
Probing feedrate It sets the probing feedrate. It must be programmed in mm/minute or inches/minute.

CNC 8040
·M· MODEL (SOFT V11.1X)
258

12.4.1 Basic operation

Programming manual
12.

PROBING PROBE 2. Probe calibration canned cycle.

1. Approach movement. Movement of the probe in rapid (G00) from the point where the cycle is called to the center of the hole. The approaching movement is made in two stages: ·1· Movement in the main work plane. ·2· Movement along the longitudinal axis.
2. Probing. This movement consists of: · Movement of the probe along the ordinate axis at the indicated feedrate (H), until the probe signal is received. The maximum distance to be traveled in the probing movement is "B+(J/2)"; if, after travelling that distance, the CNC does not receive the probe signal, it will display the corresponding error code and stop the movement of the axes. · Return of the probe in rapid (G00) the distance indicated in (E). · Movement of the probe along the ordinate axis at the indicated feedrate (F), until the probe signal is received.
3. Withdrawal. Movement of the probe in rapid (G00) from the point where it probed to the real center of the hole.
4. Second probing movement. Same as above.
5. Withdrawal. Movement of the probe in rapid (G00) from the point where it probed to the real center of the hole along the ordinate axis.
6. Third probing movement. Same as above.
7. Withdrawal. Movement of the probe in rapid (G00) from the point where it probed to the real center of the hole.
8. Fourth probing movement. Same as above.
9. Withdrawal.

CNC 8040
·M· MODEL (SOFT V11.1X)

259

Programming manual
12.

This movement consists of: · Movement of the probe in rapid (G00) from the point where it probed to the real center of the hole. · Movement along the longitudinal axis to the coordinate of the point (along this axis) from where the cycle was called. · Movement in the main work plane to the point where the cycle is called.
Correction of the tool offset.
Once the cycle has been completed, the CNC will have updated the "I" and "K" values corresponding to the tool offset selected at the time on the tool offset table.
Arithmetic parameters modified by the cycle
The cycle returns in arithmetic parameter P299 the best value to be assigned to general machine parameter PRODEL.

PROBING PROBE 2. Probe calibration canned cycle.

CNC 8040
·M· MODEL (SOFT V11.1X)
260

12.5 PROBE 3. Surface measuring canned cycle.

Programming manual

X±5.5 Y±5.5 Z±5.5 B5.5
K

A probe placed in the spindle will be used, which must be previously calibrated by means of canned cycles:
Tool length calibrating canned cycle. Probe calibrating canned cycle.
This cycle allows correcting the value of the tool offset of the tool that has been used in the surface machining process. This correction will be used only when the measurement error exceeds a programmed value.
The programming format for this cycle is: (PROBE 3, X, Y, Z, B, K, F, C, D, L)

Theoretical coordinate, along the X axis, of the point over which it is required to measure.

Theoretical coordinate, along the Y axis, of the point over which it is required to measure.

Theoretical coordinate, along the Z axis, of the point over which it is required to measure.

Probing axis

Defines the axis with which it is required to measure the surface and will be defined by means of the following code:

K = 0

With the abscissa axis of the work plane.

K = 1

With the ordinate axis of the work plane.

K = 2

With the longitudinal axis of the work plane.

If this is not programmed, the canned cycle will take the value of K0.

PROBING PROBE 3. Surface measuring canned cycle.

12.

F5.5

CNC 8040

Probing feedrate It sets the probing feedrate. It must be programmed in mm/minute or inches/minute.

·M· MODEL (SOFT V11.1X)

261

Programming manual
C

12.

L5.5

Actions after finishing the probing operation

Indicates where the probing cycle must finish.

C = 0

Will return to the same point where the call to the cycle was made.

C = 1

The cycle will finish over the measured point returning the longitudinal axis to the cycle calling point.

If this is not programmed, the canned cycle will take the value of C0.

Tool offset
Defines the number of the tool offset to be corrected, once the measurement cycle is completed. If this is not programmed or is programmed with a value of 0, the CNC will understand that it is not required to make this correction.

Error tolerance
Defines the tolerance that will be applied to the error measured. It will be programmed with an absolute value and the tool offset will be corrected only when the error exceeds this value.
If this is not programmed, the canned cycle will take the value of 0.

PROBING PROBE 3. Surface measuring canned cycle.

CNC 8040
·M· MODEL (SOFT V11.1X)
262

12.5.1 Basic operation

Programming manual
12.

PROBING PROBE 3. Surface measuring canned cycle.

1. Approach movement.
Movement of the probe in rapid (G00) from the point where the cycle is called to the approach point.
This point is to be found opposite the point where it is wished to measure, at a safety distance (B) from this and along the probing axis (K).
The approaching movement is made in two stages:
·1· Movement in the main work plane.
·2· Movement along the longitudinal axis.
2. Probing.
Movement of the probe along the selected axis (K) at the indicated feedrate (F), until the probe signal is received.
The maximum distance to be traveled in the probing movement is 2B; if, after travelling that distance, the CNC does not receive the probe signal, it will display the corresponding error code and stop the movement of the axes.
Once probing has been made, the CNC will assume as their theoretical position the real position of the axes when the probe signal is received .
3. Withdrawal.
Movement of the probe in rapid (G00) from the point where it probed to the point where the cycle was called.
The withdrawal movement is made in three stages:
·1· Movement along the probing axis to the approach point.
·2· Movement along the longitudinal axis to the coordinate of the point (along this axis) from where the cycle was called.
·3· When (C0) is programmed, movement is made in the main work plane to the point where the cycle is called.

Arithmetic parameters modified by the cycle

Once the cycle has been completed, the CNC will return the real values obtained after measurement, in the following global arithmetic parameters.

P298 P299

Real surface coordinate.
Error detected. Difference between the real coordinate of the surface and the theoretical programmed coordinate.

CNC 8040
·M· MODEL (SOFT V11.1X)

263

Programming manual
12.

Correction of the tool offset.
If the Tool Offset Number (D) was selected, the CNC will modify the values of this tool offset, whenever the measurement error is equal to or greater than the tolerance (L).
Depending on the axis the measurement is made with (K), the correction will be made on the length or radius value.
· If the measurement is made with the axis longitudinal to the work plane, the length wear (K) of the indicated tool offset (D) will be modified.
· If the measurement is made with one of the axes that make up the work plane, the radius wear (I) of the indicated tool offset (D) will be modified.

PROBING PROBE 3. Surface measuring canned cycle.

CNC 8040
·M· MODEL (SOFT V11.1X)
264

Programming manual
12.6 PROBE 4. Outside corner measuring canned cycle

X±5.5 Y±5.5 Z±5.5

A probe placed in the spindle will be used, which must be previously calibrated by means of canned cycles:
Tool length calibrating canned cycle. Probe calibrating canned cycle. The programming format for this cycle is: (PROBE 4, X, Y, Z, B, F)
Theoretical coordinate, along the X axis, of the corner to be measured.
Theoretical coordinate, along the Y axis, of the corner to be measured.
Theoretical coordinate, along the Z axis, of the corner to be measured.
Depending on the corner of the part it is required to measure, the probe must be placed in the corresponding shaded area (see figure) before calling the cycle.

12.

PROBING PROBE 4. Outside corner measuring canned cycle

B5.5 F5.5

Safety distance Defines the safety distance. Must be programmed with a positive value and over 0. The probe must be placed, with respect to the point to be measured, at a distance greater than this value when the cycle is called.
Probing feedrate It sets the probing feedrate. It must be programmed in mm/minute or inches/minute.

CNC 8040
·M· MODEL (SOFT V11.1X)
265

Programming manual
12.6.1 Basic operation
12.

PROBING PROBE 4. Outside corner measuring canned cycle

CNC 8040
·M· MODEL (SOFT V11.1X)
266

1. Approach movement. Movement of the probe in rapid (G00) from the point where the cycle is called to the first approach point, situated at a distance (B) from the first face to be probed. The approaching movement is made in two stages: ·1· Movement in the main work plane. ·2· Movement along the longitudinal axis.
2. Probing. Movement of the probe along the abscissa axis at the indicated feedrate (F), until the probe signal is received. The maximum distance to be traveled in the probing movement is 2B; if, after travelling that distance, the CNC does not receive the probe signal, it will display the corresponding error code and stop the movement of the axes.
3. Withdrawal. Movement of the probe in rapid (G00) from the point where it probed to the first approach point
4. Second approach. Movement of the probe in rapid (G00) from the first approach point to the second. The approaching movement is made in two stages: ·1· Movement along the ordinate plane. ·2· Movement along the abscissa axis.
5. Second probing movement. Movement of the probe along the abscissa axis at the indicated feedrate (F), until the probe signal is received. The maximum distance to be traveled in the probing movement is 2B; if, after travelling that distance, the CNC does not receive the probe signal, it will display the corresponding error code and stop the movement of the axes.
6. Withdrawal. Movement of the probe in rapid (G00) from the point where it probed for the second time to the point where the cycle was called. The withdrawal movement is made in three stages: ·1· Movement along the probing axis to the second approach point. ·2· Movement along the longitudinal axis to the coordinate of the point (along this axis) from where the cycle was called. ·3· Movement in the main work plane to the point where the cycle is called.

Programming manual

Arithmetic parameters modified by the cycle
Once the cycle has been completed, the CNC will return the real values obtained after measurement, in the following global arithmetic parameters.

P296 P297 P298
P299

Real coordinate of the corner along the abscissa axis.
Real coordinate of the corner along the ordinate axis.
Error detected along the abscissa axis. Difference between the real coordinate of the corner and the theoretical programmed coordinate.
Error detected along the ordinate axis. Difference between the real coordinate of the corner and the theoretical programmed coordinate.

12.

PROBING PROBE 4. Outside corner measuring canned cycle

CNC 8040
·M· MODEL (SOFT V11.1X)
267

Programming manual
12.7 PROBE 5. Inside corner measuring canned cycle.

12.

X±5.5 Y±5.5 Z±5.5

PROBING PROBE 5. Inside corner measuring canned cycle.

B5.5 F5.5

CNC 8040
·M· MODEL (SOFT V11.1X)
268

12.7.1 Basic operation

Programming manual
12.

PROBING PROBE 5. Inside corner measuring canned cycle.

1. Approach movement.
Movement of the probe in rapid (G00) from the point where the cycle is called to the first approach point, situated at a distance (B) from both faces to be probed.
The approaching movement is made in two stages:
·1· Movement in the main work plane.
·2· Movement along the longitudinal axis.
2. Probing.
Movement of the probe along the abscissa axis at the indicated feedrate (F), until the probe signal is received.
The maximum distance to be traveled in the probing movement is 2B; if, after travelling that distance, the CNC does not receive the probe signal, it will display the corresponding error code and stop the movement of the axes.
3. Withdrawal.
Movement of the probe in rapid (G00) from the point where it probed to the approach point
4. Second probing movement.
Movement of the probe along the abscissa axis at the indicated feedrate (F), until the probe signal is received.
The maximum distance to be traveled in the probing movement is 2B; if, after travelling that distance, the CNC does not receive the probe signal, it will display the corresponding error code and stop the movement of the axes.
5. Withdrawal.
Movement of the probe in rapid (G00) from the point where it probed for the second time to the point where the cycle was called.
The withdrawal movement is made in three stages:
·1· Movement along the probing axis to the approach point.
·2· Movement along the longitudinal axis to the coordinate of the point (along this axis) from where the cycle was called.
·3· Movement in the main work plane to the point where the cycle is called.

CNC 8040

·M· MODEL (SOFT V11.1X)

269

Programming manual
12.

Arithmetic parameters modified by the cycle

Once the cycle has been completed, the CNC will return the real values obtained after measurement, in the following global arithmetic parameters.

P296 P297 P298
P299

PROBING PROBE 5. Inside corner measuring canned cycle.

CNC 8040
·M· MODEL (SOFT V11.1X)
270

12.8 PROBE 6. Angle measuring canned cycle

Programming manual

X±5.5 Y±5.5 Z±5.5 B5.5
F5.5

A probe placed in the spindle will be used, which must be previously calibrated by means of canned cycles:
Tool length calibrating canned cycle. Probe calibrating canned cycle.
The programming format for this cycle is: (PROBE 6, X, Y, Z, B, F)
Theoretical coordinate, along the X axis, of the vertex of the angle to be measured.
Theoretical coordinate, along the Y axis, of the vertex of the angle to be measured.
Theoretical coordinate, along the Z axis, of the vertex of the angle to be measured.
Safety distance
Defines the safety distance. Must be programmed with a positive value and over 0.
The probe must be placed, with respect to the point to be measured, at a distance greater than double this value when the cycle is called.
Probing feedrate
It sets the probing feedrate. It must be programmed in mm/minute or inches/minute.

PROBING PROBE 6. Angle measuring canned cycle

12.

CNC 8040
·M· MODEL (SOFT V11.1X)
271

Programming manual
12.8.1 Basic operation
12.

PROBING PROBE 6. Angle measuring canned cycle

CNC 8040
·M· MODEL (SOFT V11.1X)
272

1. Approach movement.
Movement of the probe in rapid (G00) from the point where the cycle is called to the first approach point, situated at a distance (B) from the programmed vertex and at (2B) from the face to be probed.
The approaching movement is made in two stages:
·1· Movement in the main work plane.
·2· Movement along the longitudinal axis.
2. Probing.
Movement of the probe along the abscissa axis at the indicated feedrate (F), until the probe signal is received.
The maximum distance to be traveled in the probing movement is 3B; if, after travelling that distance, the CNC does not receive the probe signal, it will display the corresponding error code and stop the movement of the axes.
3. Withdrawal.
Movement of the probe in rapid (G00) from the point where it probed to the first approach point
4. Second approach.
Movement of the probe in rapid (G00) from the first approach point to the second. It is at a distance (B) from the first one.
5. Second probing movement.
Movement of the probe along the abscissa axis at the indicated feedrate (F), until the probe signal is received.
The maximum distance to be traveled in the probing movement is 4B; if, after travelling that distance, the CNC does not receive the probe signal, it will display the corresponding error code and stop the movement of the axes.
6. Withdrawal.
Movement of the probe in rapid (G00) from the point where it probed for the second time to the point where the cycle was called.
The withdrawal movement is made in three stages:
·1· Movement along the ordinate axis to the second approach point.
·2· Movement along the longitudinal axis to the coordinate of the point (along this axis) from where the cycle was called.
·3· Movement in the main work plane to the point where the cycle is called.

Programming manual
Arithmetic parameters modified by the cycle Once the cycle has been completed, the CNC will return the real values obtained after measurement, in the following global arithmetic parameter. P295 Inclination angle which the part has in relation to the abscissa axis.

Considerations for the cycle
This cycle allows angles between ±45º to be measured. · If the angle to be measured is > 45º, the CNC will display the corresponding error. · If the angle to be measured is < -45º, the probe will collide with the part.

12.

PROBING PROBE 6. Angle measuring canned cycle

CNC 8040
·M· MODEL (SOFT V11.1X)
273

Programming manual
12.9 PROBE 7. Outside corner and angle measuring canned cycle

12.

X±5.5 Y±5.5 Z±5.5

A probe placed in the spindle will be used, which must be previously calibrated by means of canned cycles:
Tool length calibrating canned cycle. Probe calibrating canned cycle. The programming format for this cycle is: (PROBE 7, X, Y, Z, B, F)
Theoretical coordinate, along the X axis, of the corner to be measured.
Theoretical coordinate, along the Y axis, of the corner to be measured.
Theoretical coordinate, along the Z axis, of the corner to be measured.
Depending on the corner of the part it is required to measure, the probe must be placed in the corresponding shaded area (see figure) before calling the cycle.

PROBING PROBE 7. Outside corner and angle measuring canned cycle

B5.5 F5.5

Safety distance Defines the safety distance. Must be programmed with a positive value and over 0. The probe must be placed, with respect to the point to be measured, at a distance greater than double this value when the cycle is called.
Probing feedrate It sets the probing feedrate. It must be programmed in mm/minute or inches/minute.

CNC 8040
·M· MODEL (SOFT V11.1X)
274

12.9.1 Basic operation

Programming manual
12.

PROBING PROBE 7. Outside corner and angle measuring canned cycle

1. Approach movement.
Movement of the probe in rapid (G00) from the point where the cycle is called to the first approach point, situated at a distance (2B) from the first side to be probed.
The approaching movement is made in two stages:
·1· Movement in the main work plane.
·2· Movement along the longitudinal axis.
2. Probing.
Movement of the probe along the abscissa axis at the indicated feedrate (F), until the probe signal is received.
The maximum distance to be traveled in the probing movement is 3B; if, after travelling that distance, the CNC does not receive the probe signal, it will display the corresponding error code and stop the movement of the axes.
3. Withdrawal.
Movement of the probe in rapid (G00) from the point where it probed to the first approach point
4. Second approach.
Movement of the probe in rapid (G00) from the first approach point to the second, situated at a distance (2B) from the second side to be probed.
The approaching movement is made in two stages:
·1· Movement along the ordinate plane.
·2· Movement along the abscissa axis.
5. Second probing movement.
Movement of the probe along the abscissa axis at the indicated feedrate (F), until the probe signal is received.
The maximum distance to be traveled in the probing movement is 3B; if, after travelling that distance, the CNC does not receive the probe signal, it will display the corresponding error code and stop the movement of the axes.
6. Withdrawal.
Movement of the probe in rapid (G00) from the point where it probed to the second point of approach.
7. Third approach.
Movement of the probe in rapid (G00) from the second approach point to the third. It is at a distance (B) from the previous one.
8. Third probing movement.
Movement of the probe along the abscissa axis at the indicated feedrate (F), until the probe signal is received.

CNC 8040
·M· MODEL (SOFT V11.1X)

275

PROBING PROBE 7. Outside corner and angle measuring canned cycle

Programming manual
12.

The maximum distance to be traveled in the probing movement is 4B; if, after travelling that distance, the CNC does not receive the probe signal, it will display the corresponding error code and stop the movement of the axes.
9. Withdrawal.
Movement of the probe in rapid (G00) from the third probing point to the point where the cycle was called.
The withdrawal movement is made in three stages:
·1· Movement along probing axis to the third approach point.
·2· Movement along the longitudinal axis to the coordinate of the point (along this axis) from where the cycle was called.
·3· Movement in the main work plane to the point where the cycle is called.

Arithmetic parameters modified by the cycle
Once the cycle has been completed, the CNC will return the real values obtained after measurement, in the following global arithmetic parameters.

P295 P296 P297 P298
P299

Inclination angle which the part has in relation to the abscissa axis.
Real coordinate of the corner along the abscissa axis.
Real coordinate of the corner along the ordinate axis.
Error detected along the abscissa axis. Difference between the real coordinate of the corner and the theoretical programmed coordinate.
Error detected along the ordinate axis. Difference between the real coordinate of the corner and the theoretical programmed coordinate.

CNC 8040
·M· MODEL (SOFT V11.1X)
276

12.10 PROBE 8. Hole measuring canned cycle.

Programming manual

X±5.5 Y±5.5 Z±5.5 B5.5 J5.5
E5.5 C
H5.5 F5.5

Theoretical coordinate, along the X axis, of the hole center.

Theoretical coordinate, along the Y axis, of the hole center.

Theoretical coordinate, along the Z axis, of the hole center.

Safety distance Defines the safety distance. Must be programmed with a positive value and over 0.

Theoretical diameter of the hole.
Defines the theoretical diameter of the hole. Must be programmed with a positive value and over 0.
This cycle allows holes to be measured with diameters of no more than (J+B).

Withdrawal distance
Defines the distance which the probe moves back after initial probing. Must be programmed with a positive value and over 0.

Actions after finishing the probing operation

Indicates where the probing cycle must finish.

C = 0

Will return to the same point where the call to the cycle was made.

C = 1

The cycle will finish at the real center of the hole.

If this is not programmed, the canned cycle will take the value of C0.

Initial probing feedrate
Defines the feedrate for the initial probing movement. It must be programmed in mm/ minute or inches/minute.

Probing feedrate It sets the probing feedrate. It must be programmed in mm/minute or inches/minute.

PROBING PROBE 8. Hole measuring canned cycle.

12.

CNC 8040
·M· MODEL (SOFT V11.1X)

277

Programming manual
12.10.1 Basic operation
12.

PROBING PROBE 8. Hole measuring canned cycle.

CNC 8040
·M· MODEL (SOFT V11.1X)
278

1. Approach movement. Movement of the probe in rapid (G00) from the point where the cycle is called to the center of the hole. The approaching movement is made in two stages: ·1· Movement in the main work plane. ·2· Movement along the longitudinal axis.
2. Probing. This movement consists of:
· Movement of the probe along the ordinate axis at the indicated feedrate (H), until the probe signal is received. The maximum distance to be traveled in the probing movement is "B+(J/2)"; if, after travelling that distance, the CNC does not receive the probe signal, it will display the corresponding error code and stop the movement of the axes.
· Return of the probe in rapid (G00) the distance indicated in (E). · Movement of the probe along the abscissa axis at the indicated feedrate (F), until
the probe signal is received. 3. Withdrawal.
Movement of the probe in rapid (G00) from the point where it probed to the theoretical center of the hole. 4. Second probing movement. Same as above. 5. Withdrawal. Movement of the probe in rapid (G00) from the point where it probed to the real center (calculated) of the hole along the ordinate axis. 6. Third probing movement. Same as above. 7. Withdrawal. Movement of the probe in rapid (G00) from the point where it probed to the theoretical center of the hole. 8. Fourth probing movement. Same as above. 9. Withdrawal. This movement consists of:

Programming manual

·1· Movement of the probe in rapid (G00) from the point where it probed to the real center (calculated) of the hole.
·2· Should (C0) be programmed, the probe will be moved to the point where the cycle was called.
Movement along the longitudinal axis to the coordinate of the point (along this axis) from where the cycle was called.
Movement in the main work plane to the point where the cycle is called.

Arithmetic parameters modified by the cycle
Once the cycle has been completed, the CNC will return the real values obtained after measurement, in the following global arithmetic parameters.

12.

P294 P295
P296 P297 P298
P299

Hole diameter.
Hole diameter error. Difference between the real diameter and programmed diameter.
Real coordinate of the center along the abscissa axis.
Real coordinate of the center along the ordinate axis.
Error detected along the abscissa axis. Difference between the real coordinate of the center and the programmed theoretical coordinate.
Error detected along the ordinate axis. Difference between the real coordinate of the center and the programmed theoretical coordinate.

PROBING PROBE 8. Hole measuring canned cycle.

CNC 8040
·M· MODEL (SOFT V11.1X)
279

Programming manual
12.11 PROBE 9. Boss measuring canned cycle.

12.

PROBING PROBE 9. Boss measuring canned cycle.

X±5.5 Y±5.5 Z±5.5 B5.5 J5.5
E5.5 C
H5.5 F5.5

Theoretical coordinate, along the X axis, of the boss center.

Theoretical coordinate, along the Y axis, of the boss center.

Theoretical coordinate, along the Z axis, of the boss center.

Safety distance Defines the safety distance. Must be programmed with a positive value and over 0.

Theoretical diameter of the boss.
Defines the theoretical diameter of the boss. Must be programmed with a positive value and over 0.
This cycle allows bosses to be measured with diameters of no more than (J+B).

Withdrawal distance
Defines the distance which the probe moves back after initial probing. Must be programmed with a positive value and over 0.

Actions after finishing the probing operation

Indicates where the probing cycle must finish.

C = 0

Will return to the same point where the call to the cycle was made.

C = 1

The cycle will finish by positioning the probe over the center of the boss, at a distance (B) from the programmed theoretical coordinate.

If this is not programmed, the canned cycle will take the value of C0.

Initial probing feedrate
Defines the feedrate for the initial probing movement. It must be programmed in mm/ minute or inches/minute.

Probing feedrate It sets the probing feedrate. It must be programmed in mm/minute or inches/minute.

CNC 8040

·M· MODEL (SOFT V11.1X)

280

12.11.1 Basic operation

Programming manual
12.

PROBING PROBE 9. Boss measuring canned cycle.

1. Positioning over the center of the boss. Movement of the probe in rapid (G00) from the point where the cycle is called to the center of the boss. The approaching movement is made in two stages: ·1· Movement in the main work plane. ·2· Movement along the longitudinal axis up to a distance (B) from the programmed surface.
2. Movement to the first approach point. This movement of the probe that is made in rapid (G00) consists of: ·1· Movement along the ordinate plane. ·2· Movement of the longitudinal axis the distance (2B).
3. Probing. This movement consists of:
· Movement of the probe along the ordinate axis at the indicated feedrate (H), until the probe signal is received. The maximum distance to be traveled in the probing movement is "B+(J/2)"; if, after travelling that distance, the CNC does not receive the probe signal, it will display the corresponding error code and stop the movement of the axes.
· Return of the probe in rapid (G00) the distance indicated in (E). · Movement of the probe along the abscissa axis at the indicated feedrate (F), until
the probe signal is received. 4. Movement to second approach point.
This movement of the probe that is made in rapid (G00) consists of: · Withdrawal to the first approach point. · Movement to a distance (B) above the boss, to the second approach point.
5. Second probing movement. Same as the first probing.
6. Third approach movement. Same as above.
7. Third probing movement. Same as above.
8. Fourth approach movement. Same as above.
9. Fourth probing movement.

CNC 8040
·M· MODEL (SOFT V11.1X)
281

PROBING PROBE 9. Boss measuring canned cycle.

Programming manual
12.

Same as above. 10.Withdrawal.
This movement consists of: ·1· Withdrawal to the fourth approach point. ·2· Movement of the probe in rapid (G00) and at a distance (B) above the boss
to the real center (calculated) of the boss. ·3· Should (C0) be programmed, the probe will be moved to the point where the
cycle was called. Movement along the longitudinal axis to the coordinate of the point (along this axis) from where the cycle was called. Movement in the main work plane to the point where the cycle is called.

Arithmetic parameters modified by the cycle
Once the cycle has been completed, the CNC will return the real values obtained after measurement, in the following global arithmetic parameters.

P294 P295
P296 P297 P298
P299

Boss diameter.
Boss diameter error. Difference between the real diameter and programmed diameter.
Real coordinate of the center along the abscissa axis.
Real coordinate of the center along the ordinate axis.
Error detected along the abscissa axis. Difference between the real coordinate of the center and the programmed theoretical coordinate.
Error detected along the ordinate axis. Difference between the real coordinate of the center and the programmed theoretical coordinate.

CNC 8040
·M· MODEL (SOFT V11.1X)
282

Programming manual
12.12 PROBE 10. Rectangular part centering canned cycle
Cycle that, with a digital probe, minimizes the preparation time of rectangular part calculating the real coordinates of the center, of the surface and of the part inclination.
(PROBE 10, I, J, X, Y, Z, K, L, B, D, E, H, F, Q)

Initial conditions
· The probe must properly calibrated in radius and length. · The probe position before the first probing movement must be as centered as
possible in X and Y.

12.

PROBING PROBE 10. Rectangular part centering canned cycle

Considerations for the cycle
· After the probing movements, the probe withdraws from the part in G0 before moving to the safety Z position.
· Depending on the PRBMOD variable, no error is issued in the following cases, even if machine parameter PROBERR=YES. ·1· When a G75 probing move finishes before the probe has touched part. ·2· When a G76 probing move finishes but the probe is still touching the part.

Parameters

X+-5.5: Y+-5.5: Z+-5.5: I 5.5: J 5.5: K 1:
L 1:
B 5.5: D+-5.5: E+-5.5:

X coordinate of the probe position where the first probing move will start. If not programmed, it will assume the current X position of the probe. Y coordinate of the probe position where the first probing move will start. If not programmed, it will assume the current Y position of the probe. Z coordinate of the probe position where the first probing move will start. If not programmed, it will assume the current Z position of the probe. X length of the rectangular part. If not programmed or programmed with a 0 value, it generates the corresponding error message. Y length of the rectangular part. If not programmed or programmed with a 0 value, it generates the corresponding error message. Axis and direction of the first probing movement. The values are:
· For X+ : 0
· For X- : 1
· For Y+ : 2
· For Y- : 3
· If not programmed, it assumes 0. It indicates whether the part surface is measured or not:
· 0 Value: It is not measured
· 1 Value: It is measured
· If not programmed, it assumes 0 Part approaching distance in each probing movement. If not programmed or programmed as 0, it assumes the approach distance value from the probe position to the part. Distance for the probe to go up in Z for its movements over the part. If not programmed or programmed with a 0 value, it generates the corresponding error message. Distance the probe retracts after finding the part, to make the measurement. If not programmed or programmed with a 0 value, it generates the corresponding error message.

CNC 8040
·M· MODEL (SOFT V11.1X)
283

Programming manual H 5: F 5: Q 5: T: D:
12.

Probing feedrate for searching the part. If not programmed or programmed with a 0 value, it generates the corresponding error message.
Probing feedrate for measuring. If not programmed or programmed with a 0 value, it generates the corresponding error message.
Probe feedrate when going to the approach points. If not programmed, it assumes rapid traverse (G0).
Probe's tool number. If not programmed or programmed with a 0 value, it generates the corresponding error message.
Tool offset number. If not programmed, it assumes the offset number assigned to T in the tool table.

PROBING PROBE 10. Rectangular part centering canned cycle

Operation

CNC 8040
·M· MODEL (SOFT V11.1X)

1. Approach movement (according to the value given in Q), first in the axes of the plane and then in the longitudinal axis, to the position of the first probing (only if X or Y or Z has been programmed).
2. Probing movement (at the feedrate given in H), in the given axis and direction until touching the first side.
3. Withdrawal (distance given in E) for the measuring probing movement.
4. Probing movement (at the feedrate given in F) until touching the same side again.
5. Withdrawal to the starting position.
6. Movement parallel to the probed side to touch a different point of the same side.
7. Probing movement (at the feedrate given in F), in the given axis and direction until touching the first side again. This calculates the part inclination angle with respect to the table and it is saved in parameter P296.
8. Rapid up movement in Z (distance given in D) up to the Safety Z coordinate.
9. Movement (according to the value given in Q) up to the approach point of the opposite side considering the length of the part, the calculated inclination angle and the value of parameter B.
10.Probing movement (at the feedrate given in H) to go down to the probing Z coordinate. If it touches the part, the probe goes back up to the safety Z position and moves the distance indicated by parameter B (in the same direction) until clearing the part.
11.Probing movement (at the feedrate given in H), considering the calculated inclination angle until touching that side.
12.Withdrawal (distance given in E) for the measuring probing movement.
13.Probing movement (at the feedrate given in F) until touching the same side again.
14.Rapid up movement to the safety Z coordinate.
15.Movement (according to the value given in Q) up to approach point in the middle of one of the remaining sides considering half the lengths and the calculated inclination angle.
16.Probing movement (at the feedrate given in H) to go down to the probing Z coordinate. If it touches the part, the probe goes back up to the safety Z position and moves the distance indicated by parameter B (in the same direction) until clearing the part.
17.Probing movement (at the feedrate given in H), considering the calculated inclination angle until touching that side.
18.Withdrawal (distance given in E) for the measuring probing movement.
19.Probing movement (at the feedrate given in F) until touching the same side again.
20.Rapid up movement to the safety Z coordinate.
21.If part surface measuring has not been programmed, it goes on to point 26; and if it has been programmed, movement (according to the value given in Q) up to the center of the part.
22.Probing movement (at the feedrate given in H) until touching the surface of the part.
23.Withdrawal (distance given in E) for the measuring probing movement.

284

Programming manual

24.Probing movement (at the feedrate given in F) until touching the surface of the part again. This measures the coordinate of the part surface and it is saved in parameter P297.
25.Rapid up movement to the safety Z coordinate.
26.Movement (according to the value given in Q) up to the approach point of the opposite side considering the length of the part, the calculated inclination angle.
27.Probing movement (at the feedrate given in H) to go down to the probing Z coordinate. If it touches the part, the probe goes back up to the safety Z position and moves the distance indicated by parameter B (in the same direction) until clearing the part.
28.Probing movement (at the feedrate given in H), considering the calculated inclination angle until touching that side.
29.Withdrawal (distance given in E) for the measuring probing movement.
30.Probing movement (at the feedrate given in F) until touching the same side again. This calculates the real center of the rectangular part and it is saved in parameters P298 and P299.
31.Rapid up movement to the safety Z coordinate.
32.Rapid movement up to the calculated center.

12.

PROBING PROBE 10. Rectangular part centering canned cycle

CNC 8040
·M· MODEL (SOFT V11.1X)
285

Programming manual
12.13 PROBE 11. Circular part centering canned cycle.
Cycle that, with a digital probe, minimizes the preparation time of circular part calculating the real coordinates of the center and of the surface of the part.
(PROBE 11, J, X, Y, Z, K, L, B, D, E, H, F, Q)

12.

Initial conditions
· The probe must properly calibrated in radius and length. · The probe position before the first probing movement must be as centered as
possible in X and Y.

PROBING PROBE 11. Circular part centering canned cycle.

CNC 8040
·M· MODEL (SOFT V11.1X)

Parameters

X+-5.5: Y+-5.5: Z+-5.5: J 5.5: K 1:
L 1:
B 5.5: D+-5.5: E+-5.5:

X coordinate of the probe position where the first probing move will start. If not programmed, it will assume the current X position of the probe. Y coordinate of the probe position where the first probing move will start. If not programmed, it will assume the current Y position of the probe. Z coordinate of the probe position where the first probing move will start. If not programmed, it will assume the current Z position of the probe. Diameter of the circular part. If not programmed or programmed with a 0 value, it generates the corresponding error message. Axis and direction of the first probing movement. The values are:
· For X+ : 0
· For X- : 1
· For Y+ : 2
· For Y- : 3
· If not programmed, it assumes 0. It indicates whether the part surface is measured or not:
· 0 Value: It is not measured
· 1 Value: It is measured
· If not programmed, it assumes 0 Part approaching distance in each probing movement. If not programmed or programmed as 0, it assumes the approach distance value from the probe starting position to the part. Distance for the probe to go up in Z for its movements over the part. If not programmed or programmed with a 0 value, it generates the corresponding error message. Distance the probe retracts after finding the part, to make the measurement. If not programmed or programmed with a 0 value, it generates the corresponding error message.

286

Programming manual

H 5:

Probing feedrate for searching the part. If not programmed or programmed with a

0 value, it generates the corresponding error message.

F 5:

Probing feedrate for measuring. If not programmed or programmed with a 0 value,

it generates the corresponding error message.

Q 5:

Probe feedrate when going to the approach points. If not programmed, it assumes

in G0.

Probe's tool number. If not programmed or programmed with a 0 value, it generates

the corresponding error message.

Tool offset number. If not programmed, it assumes the offset number assigned to

T in the tool table.

12.

PROBING PROBE 11. Circular part centering canned cycle.

Operation
1. Approach movement (according to the value given in Q), first in the axes of the plane and then in the longitudinal axis, to the position of the first probing (only if X or Y or Z has been programmed).
2. Probing movement (at the feedrate given in H), in the given axis and direction until touching the part.
3. Withdrawal (distance given in E) for the measuring probing movement.
4. Probing movement (at the feedrate given in F) until touching the same side again.
5. Rapid up movement in Z (distance given in D) up to the Safety Z coordinate.
6. Movement (according to the value given in Q) up to the opposite approach point considering the diameter of the part.
7. Probing movement (at the feedrate given in H) to go down to the probing Z coordinate. If it touches the part, the probe goes back up to the safety Z position and moves the distance indicated by parameter B (in the same direction) until clearing the part.
8. Probing movement (at the feedrate given in H) until touching the part.
9. Withdrawal (distance given in E) for the measuring probing movement.
10.Probing movement (at the feedrate given in F) until touching the part again. This calculates one of the coordinates of the real center of the part.
11.Rapid up movement to the safety Z coordinate.
12.Movement (according to the value given in Q) up to the approach point of the remaining axis considering the calculated center coordinate.
13.Probing movement (at the feedrate given in H) to go down to the probing Z coordinate. If it touches the part, the probe goes back up to the safety Z position and moves the distance indicated by parameter B (in the same direction) until clearing the part.
14.Probing movement (at the feedrate given in H) until touching the part.
15.Withdrawal (distance given in E) for the measuring probing movement.
16.Probing movement (at the feedrate given in F) until touching the part again.
17.Rapid up movement to the safety Z coordinate.
18.If part surface measuring has not been programmed, it goes on to point 23; and if it has been programmed, movement (according to the value given in Q) up to the center of the part.
19.Probing movement (at the feedrate given in H) until touching the surface of the part.
20.Withdrawal (distance given in E) for the measuring probing movement.
21.Probing movement (at the feedrate given in F) until touching the surface of the part again. This measures the coordinate of the part surface and it is saved in parameter P297.
22.Rapid up movement to the safety Z coordinate.
23.Movement (according to the value given in Q) up to the opposite approach point considering the diameter of the part.
24.Probing movement (at the feedrate given in H) to go down to the probing Z coordinate. If it touches the part, the probe goes back up to the safety Z position

CNC 8040
·M· MODEL (SOFT V11.1X)
287

Programming manual
12.

and moves the distance indicated by parameter B (in the same direction) until clearing the part.
25.Probing movement (at the feedrate given in H) until touching the part.
26.Withdrawal (distance given in E) for the measuring probing movement.
27.Probing movement (at the feedrate given in F) until touching the part again. This calculates the real center of the circular part and it is saved in parameters P298 and P299.
28.Rapid up movement to the safety Z coordinate.
29.Rapid movement up to the calculated center.

PROBING PROBE 11. Circular part centering canned cycle.

CNC 8040
·M· MODEL (SOFT V11.1X)
288

HIGH-LEVEL LANGUAGE PROGRAMMING

13.1 Lexical description
All the words that make up the high-level language of the numerical control must be written in capital letters except for associated texts which may be written in upper and lower case letters.
The following elements are available for high-level programming: · Reserved words. · Numerical constants. · Symbols.

Reserved words
Reserved words are those that the CNC uses in high-level programming for naming system variables, operators, control instructions, etc.
All the letters of the alphabet A-Z are also reserved words, as they can make up a high-level language word when used alone.

Numerical constants
Blocks programmed in high-level language admit numbers in decimal format and in hexadecimal format.
· The numbers in decimal format must not exceed the ±6.5 format (6 digits to the left of the decimal point and 5 decimals).
· The numbers in hexadecimal format must be preceded by the $ symbol and they must not have more than 8 digits.
A constant higher than the format ±6,5 must be assigned to a variable by means of arithmetic parameters by means of arithmetic expressions or by means of constants in hexadecimal format.
The value 100000000 may be assigned to the variable "TIMER" in one of the following ways:
(TIMER = $5F5E100) (TIMER = 10000 * 10000) (P100 = 10000 * 10000) (TIMER = P100)
If the CNC operates in the metric system (millimeters), the resolution is a tenth of a micron and the figures will be programmed in the ±5.4 format (positive or negative with 5 digits to the left of the decimal point and 4 decimals).
If the CNC operates in inches, the resolution is a hundred-thousandths of an inch (ten millionths of an inch) and the figures will be programmed in the ±4.5 format (positive or negative with 4 digits to the left of the decimal point and 5 decimals).

CNC 8040
·M· MODEL (SOFT V11.1X)

289

Programming manual
13.

For the convenience of the programmer, this control always allows the format ±5.5 (positive or negative, with 5 integers and 5 decimals), adjusting each number appropriately to the working units every time they are used.
Symbols
The symbols used in high-level language are: ( ) " = + - * / ,

HIGH-LEVEL LANGUAGE PROGRAMMING Lexical description

CNC 8040
·M· MODEL (SOFT V11.1X)
290

13.2 Variables

Programming manual

The CNC has a number of internal variables that may be accessed from the user program, from the PLC program or via DNC. Depending on how they are used, these variables may be read-only or read-write.

These variables may be accessed from the user program using high-level commands. Each one of these variables is referred to by its mnemonic that must be written in upper-case (capital) letters.

· Mnemonics ending in (X-C) indicate a set of 9 elements formed by the corresponding root followed by X, Y, Z, U, V, W, A, B and C.

ORG(X-C) -> ORGX

ORGY

ORGZ

ORGU

ORGV

ORGW

ORGA

ORGB

ORGC

· Mnemonics ending in n indicate that the variables are grouped in tables. To access an element of any of these tables, indicate the field of the desired table using the relevant mnemonic followed by the desired element.

TORn -> TOR1

TOR3

TOR11

13.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

The variables and block preparation
The variables that access the real values of the CNC interrupt block preparation. The CNC waits for that command to be executed before resuming block preparation. Thus, precaution must be taken when using this type of variable, because if they are inserted between machining blocks that are working with compensation, undesired profiles may be obtained.
Example: Reading a variable that interrupts block preparation.
The following program blocks are performed in a section with G41 compensation. ... N10 X50 Y80 N15 (P100 = POSX); Assigns the value of the real coordinate in X to parameter P100 N20 X50 Y50 N30 X80 Y50 ...
Block N15 interrupts block preparation and the execution of block N10 will finish at point A.
Once the execution of block N15 has ended, the CNC will resume block preparation from block N20 on.

CNC 8040

·M· MODEL (SOFT V11.1X)

291

Programming manual
13.

As the next point corresponding to the compensated path is point "B", the CNC will move the tool to this point, executing path "A-B".
As can be observed, the resulting path is not the desired one, and therefore it is recommended to avoid the use of this type of variable in sections having tool compensation active.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

CNC 8040
·M· MODEL (SOFT V11.1X)
292

13.2.1 General purpose parameters or variables

Programming manual

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

General purpose variables are referred to with the letter "P" followed by an integer number. The CNC has four types of general purpose variables.

Parameter type Local parameters Global parameters User parameters OEM (manufacturer's) parameters

Range P0-P25 P100-P299 P1000-P1255 P2000 - P2255

Blocks programmed in ISO code allow associating parameters to the G F S T D M fields and coordinates of the axes. The block label number must be defined with a numeric value. If parameters are used in blocks programmed in high-level language, they can be programmed within any expression.
Programmers may use general purpose variables when editing their own programs. Later on, during execution, the CNC will replace these variables with the values assigned to them at the time.

When programming...

When executing...

GP0 XP1 Z100

G1 X-12.5 Z100

(IF (P100 * P101 EQ P102) GOTO N100) (IF (2 * 5 EQ 12) GOTO N100)

13.

Using these general purpose variables will depend on the type of block in which they are programmed and the channel of execution. Programs that are executed in the user channel may contain any global, OEM or user parameter, but may not use local parameters.

Types of arithmetic parameters
Local parameters
Local parameters can only be accessed from the program or subroutine where they have been programmed. There are seven groups of parameters.
Local parameters used in high-level language may be defined either using the above format or by using the letter A-Z, except for Ñ, so that A is equal to P0 and Z to P25.
The following example shows these two methods of definition: (IF ((P0+P1)* P2/P3 EQ P4) GOTO N100) (IF ((A+B)* C/D EQ E) GOTO N100)
When using a parameter name (letter) for assigning a value to it (A instead of P0, for example), if the arithmetic expression is a constant, the instruction can be abbreviated as follows:
(P0=13.7) ==> (A=13.7) ==> (A13.7)
Be careful when using parenthesis since M30 is not the same as (M30). The CNC interprets (M30) as a high level instruction meaning (P12 = 30) and not the execution of the miscellaneous M30 function.
Global parameters
Global parameters can be accessed from any program and subroutine called from a program.
Global parameters may be used by the user, by the OEM or by the CNC cycles.
User parameters
These parameters are an expansion of the global parameters but they are not used by the CNC cycles.

CNC 8040
·M· MODEL (SOFT V11.1X)
293

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

Programming manual
13.

OEM (manufacturer's) parameters
OEM parameters and subroutines with OEM parameters can only be used in OEM programs; those defined with the [O] attribute. Modifying one of these parameters in the tables requires an OEM password.
Using arithmetic parameters by the cycles
Multiple machining cycles (G60 through G65) and the machining canned cycles (G69, G81 to G89) use the sixth nesting level of local parameters when they are active.
Machining canned cycles use the global parameter P299 for internal calculations and probing canned cycles use global parameters P294 to P299.
Updating arithmetic parameter tables
The CNC will update the parameter table after processing the operations indicated in the block that is in preparation. This operation is always done before executing the block and for this reason, the values shown in the table do not necessarily have to correspond to the block being executed.
If the execution mode is abandoned after interrupting the execution of the program, the CNC will update the parameter tables with values corresponding to the block that was being executed.
When accessing the local parameter and global parameter table, the value assigned to each parameter may be expressed in decimal notation (4127.423) or in scientific notation (0.23476 E-3).
Arithmetic parameters in the subroutines
This CNC has high level instructions that allow the definition and use of subroutines that can be called from the main program, or from another subroutine, it also being possible to call a second subroutine, from the second to a third, etc. The CNC limits these calls to a maximum of 15 nesting levels.
Up to 26 (P0-P25) local parameters may be assigned to a subroutine. These parameters, that will be unknown for blocks outside the subroutine, may be referred to by the blocks that make up the subroutine.
Local parameters may be assigned to more than one subroutine up to 6 parameter nesting levels within the 15 subroutine nesting levels.

CNC 8040
·M· MODEL (SOFT V11.1X)
294

13.2.2 Variables associated with tools.

Programming manual

These variables are associated with the tool offset table, tool table and tool magazine table, so the values which are assigned to or read from these fields will comply with the formats established for these tables.

Tool Offset table

The radius (R), length (L) and wear offset (I, K) values of the tool are given in the active units.
If G70, in inches (within ±3937.00787). If G71, in millimeters (within ±99999.9999). If rotary axis in degrees (within ±99999.9999).

Tool table

The tool offset number is an integer between 0 and 255. The maximum number of tool offsets is limited by g.m.p. NTOFFSET.

The family code is a number between 0 and 255.

0 to 199

if it is a normal tool.

200 to 255 if it is a special tool.

The nominal life is given either in minutes or in operations (0··65535).
The real (actual) life is given either in hundredths of a minute (0··9999999) or in operations (0··999999).

Tool magazine table

Each magazine position is represented as follows:

1··255

Tool number.

The magazine position is empty.

-1

The magazine position has been canceled.

The tool position in the magazine is represented as follows:

1··255

Position number.

The tool is in the spindle.

-1

Tool not found.

-2

The tool is in the change position.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

13.

TOOL
TOD NXTOOL NXTOD TMZPn

Read-only variables
Returns the number of the active tool.
(P100=TOOL) Assigns the number of the active tool to parameter P100.
Returns the number of the active tool offset. Returns the next tool number, which is selected but is awaiting the execution of M06 to be active. Returns the number of the tool offset corresponding to the next tool, which is selected but is awaiting the execution of M06 to be active. Returns the position occupied in the tool magazine by the indicated tool (n).

CNC 8040
·M· MODEL (SOFT V11.1X)

295

Programming manual TORn

13.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

TOLn TOIn TOKn TLFDn TLFFn TLFNn TLFRn TMZTn

Read-and-write variables
This variable allows the value assigned to the radius of the indicated tool offset (n) in the tool offset table to be read or modified.
(P110=TOR3) Assigns the radius value of tool offset ·3· to parameter P110.
(TOR3=P111) Assigns the value indicated in parameter P111 to the radius of tool offset 3.
This variable allows the value assigned to the length of the indicated tool offset (n) to be read or modified in the tool offset table.
This variable allows the value assigned to the wear in radius (I) of the indicated tool offset (n) to be read or modified in the tool offset table.
This variable allows the value assigned to the wear in length (K) of the indicated tool offset (n) to be read or modified in the tool offset table.
This variable allows the tool offset number of the indicated tool (n) to be read or modified in the tool table.
This variable allows the family code of the indicated tool (n) to be read or modified in the tool table.
This variable allows the value assigned as the nominal life of the indicated tool (n) to be read or modified in the tool table.
This variable allows the value corresponding to the real life of the indicated tool (n) to be read or modified in the tool table.
This variable allows the contents of the indicated position (n) to be read or modified in the tool magazine table.

CNC 8040
·M· MODEL (SOFT V11.1X)
296

13.2.3 Variables associated with zero offsets.

Programming manual

These variables are associated with the zero offsets and may correspond to the table values or to those currently preset either by means of function G92 or manually in the JOG mode.
The possible zero offsets in addition to the additive offset indicated by the PLC, are G54, G55, G56, G57, G58 and G59.
The values for each axis are given in the active units: If G70, in inches (within ±3937.00787). If G71, in millimeters (within ±99999.9999). If rotary axis in degrees (within ±99999.9999).
Although there are variables which refer to each axis, the CNC only allows those referring to the axes selected at the CNC. Thus, if the CNC controls axes X, Y, Z, U and B, it only allows the variables ORGX, ORGY, ORGZ,. ORGU and ORGB in the case of ORG(X-C).

13.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

ORG(X-C)
PORGF PORGS ADIOF(X-C)

Read-only variables
Returns the value of the active zero offset in the selected axis. The value of the additive offset indicated by the PLC or by the additive handwheel is not included in this value.
(P100=ORGX) It assigns to P100 the X value of the part zero active for the X axis. This value could have been set either manually, by means of function G92 or by the variable "ORG(X-C)n".
Returns the abscissa value of the polar coordinate origin with respect to the Cartesian origin.
Returns the ordinate value of the polar coordinate origin with respect to the Cartesian origin.
It returns the value of the zero offset generated by the additive handwheel in the selected axis.

ORG(X-C)n PLCOF(X-C)

Read-and-write variables
This variable allows the value of the selected axis to be read or modified in the table corresponding to the indicated zero offset (n).
(P110=ORGX 55) Loads parameter P100 with the X value of G55 in the zero offset table.
(ORGY 54=P111) It assigns parameter P111 to the Y axis in the table for the G54 offset.
This variable allows the value of the selected axis to be read or modified in the table of additive offsets indicated by the PLC. Accessing any of the PLCOF(X-C) variables interrupts block preparation and the CNC waits for that command to be executed before resuming block preparation.

CNC 8040
·M· MODEL (SOFT V11.1X)

297

Programming manual
13.2.4 Variables associated with machine parameters

13.

These variables associated with machine parameters are read-only variables. These variables may be read and written when executed inside an OEM program or subroutine.
Refer to the installation and start-up manual to know the format of the values returned. The values of 1/0 correspond to the parameters that are set as YES/NO, +/- or ON/ OFF.
The coordinate and feedrate values are given in the active units: If G70, in inches (within ±3937.00787). If G71, in millimeters (within ±99999.9999). If rotary axis in degrees (within ±99999.9999).
Modify the machine parameters from an OEM program or subroutine.
These variables may be read and written when executed inside an OEM program or subroutine. In this case, these variables can be used to modify the value of certain machine parameters. Refer to the installation manual for the list of machine parameters that may be modified.
In order to be able to modify these parameters via PLC, an OEM subroutine containing the relevant variables must be executed using the CNCEX command.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

MPGn
MP(X-C)n
MPSn MPSSn MPASn MPLCn

Read-only variables
Returns the value assigned to general machine parameter (n).
(P110=MPG8) It assigns the value of the general machine parameter P8 "INCHES" to parameter P110, if millimeters P110=0 and if inches P110=1.
Returns the value assigned to the machine parameter (n) of the indicated axis (X-C).
(P110=MPY 1) Assigns the value of Y axis machine parameter P1 "DFORMAT" to parameter P110.
Returns the value assigned to the indicated machine parameter (n) of the main spindle. Returns the value assigned to the indicated machine parameter (n) of the second spindle. Returns the value of the indicated machine parameter (n) of the auxiliary spindle. Returns the value assigned to the indicated machine parameter (n) of the PLC.

CNC 8040

·M· MODEL (SOFT V11.1X)

298

13.2.5 Variables associated with work zones

Programming manual

Variables associated with work zones are read-only variables.
The values of the limits are given in the active units: If G70, in inches (within ±3937.00787). If G71, in millimeters (within ±99999.9999). If rotary axis in degrees (within ±99999.9999).
The status of the work zones are defined according to the following code: 0 = Disabled. 1 = Enabled as no-entry zone. 2 = Enabled as no-exit zone.

13.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

FZONE FZLO(X-C) FZUP(X-C)
SZONE SZLO(X-C) SZUP(X-C) TZONE TZLO(X-C) TZUP(X-C) FOZONE FOZLO(X-C) FOZUP(X-C) FIZONE FIZLO(X-C): FIZUP(X-C)

Read-only variables

It returns the status of work zone 1. Lower limit of zone 1 along the selected axis (X-C). Upper limit of zone 1 along the selected axis (X-C).

(P100=FZONE) (P101=FZOLOX) (P102=FZUPZ)

; It assigns to parameter P100 the status of work zone 1. ; It assigns the lower limit of zone 1 to parameter P101. ; It assigns the upper limit of zone 1 to parameter P102.

Status of work zone 2. Lower limit of zone 2 along the selected axis (X-C). Upper limit of zone 2 along the selected axis (X-C).
Status of work zone 3. Lower limit of zone 3 along the selected axis (X-C) Upper limit of zone 3 along the selected axis (X-C).
Status of work zone 4. Lower limit of zone 4 along the selected axis (X-C). Upper limit of zone 4 along the selected axis (X-C).
Status of work zone 5. Lower limit of zone 5 along the selected axis (X-C). Upper limit of zone 5 along the selected axis (X-C).

CNC 8040
·M· MODEL (SOFT V11.1X)
299

Programming manual
13.2.6 Variables associated with feedrates

13.

FREAL
FREAL(X-C) FTEO(X-C)

Read-only variables associated with the real (actual) feedrate
It returns the CNC's real feedrate. In mm/minute or inches/minute. (P100=FREAL)
It assigns the real feedrate value of the CNC to parameter P100. It returns the actual (real) CNC feedrate of the selected axis. It returns the theoretical CNC feedrate of the selected axis.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

FEED
DNCF PLCF PRGF

Read-only variables associated with function G94
It returns the feedrate selected at the CNC by function G94. In mm/minute or inches/ minute.
This feedrate may be indicated by program, by PLC or by DNC; the CNC selects one of them, the one indicated by DNC has the highest priority and the one indicated by program has the lowest priority.
It returns the feedrate, in mm/minute or inches/minute selected by DNC. If it has a value of 0 it means that it is not selected.
It returns the feedrate, in mm/minute or inches/minute selected by PLC. If it has a value of 0 it means that it is not selected.
It returns the feedrate, in mm/minute or inches/minute selected by program.

FPREV
DNCFPR PLCFPR PRGFPR

Read-only variables associated with function G95
It returns the feedrate selected at the CNC by function G95. In mm/turn or inches/turn.
This feedrate may be indicated by program, by PLC or by DNC; the CNC selects one of them, the one indicated by DNC has the highest priority and the one indicated by program has the lowest priority.
It returns the feedrate, in mm/turn or inches/turn selected by DNC. If it has a value of 0 it means that it is not selected.
It returns the feedrate, in mm/turn or inches/turn selected by PLC. If it has a value of 0 it means that it is not selected.
It returns the feedrate, in mm/turn or inches/turn selected by program.

CNC 8040

PRGFIN

·M· MODEL (SOFT V11.1X)

Read-only variables associated with function G32
It returns the feedrate selected by program, in 1/min. Likewise, the CNC variable FEED, associated with G94, indicates the resulting feedrate in mm/min or inches/min.

300

FRO
DNCFRO PLCFRO CNCFRO PLCCFR
PRGFRO

Read-only variables associated with the override

Programming manual

It returns the feedrate override (%) currently selected at the CNC. It is given in integer values between 0 and "MAXFOVR" (maximum 255).
This feedrate percentage may be indicated by program, by PLC, by DNC or by the front panel; the CNC selects one of them and the priority (from the highest to the lowest) is: by program, by DNC, by PLC and from the front panel switch.
It returns the feedrate override % currently selected by the DNC. If it has a value of 0 it means that it is not selected.
It returns the feedrate override % currently selected by the PLC. If it has a value of 0 it means that it is not selected.
It returns the feedrate override % currently selected by the switch.
It returns the feedrate percentage currently selected by the PLC's execution channel.

13.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

Read-write variables associated with the override
This variable may be used to read or modify the feedrate override percentage currently selected by program. It is given in integer values between 0 and "MAXFOVR" (maximum 255). If it has a value of 0 it means that it is not selected.
(P110=PRGFRO) It assigns to P110 the % of feedrate override selected by program.
(PRGFRO=P111) It sets the feedrate override % selected by program to the value of P111.

CNC 8040
·M· MODEL (SOFT V11.1X)
301

Programming manual
13.2.7 Variables associated with coordinates
The coordinate values for each axis are given in the active units: If G70, in inches (within ±3937.00787). If G71, in millimeters (within ±99999.9999). If rotary axis in degrees (within ±99999.9999).

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

13.
PPOS(X-C) POS(X-C)
TPOS(X-C)
APOS(X-C) ATPOS(X-C) DPOS(X-C)
CNC 8040

Read-only variables

Accessing any of the variables POS(X-C), TPOS(X-C), APOS(X-C), ATPOS(X-C), DPOS(X-C), FLWE(X-C), DEFLEX, DEFLEY or DEFLEZ interrupts block preparation and the CNC waits for that command to be executed before resuming block preparation.
Returns the programmed theoretical coordinate of the selected axis.

(P110=PPOSX) It assigns to P100 the programmed theoretical position of the X axis.

It returns the real tool base position value referred to machine reference zero (home).

On limit-less rotary axes, this variable takes into account the value of the active zero offset. The values of the variable are between the active zero offset and ±360º (ORG* ± 360º).

If ORG* = 20º

it displays between 20º and 380º / displays between -340º and 20º.

If ORG* = -60º

it displays between -60º and 300º / displays between -420 and -60º

It returns the theoretical position value (real coordinate + following error) of the tool base referred to machine reference zero (home).

On limit-less rotary axes, this variable takes into account the value of the active zero offset. The values of the variable are between the active zero offset and ±360º (ORG* ± 360º).

If ORG* = 20º

it displays between 20º and 380º / displays between -340º and 20º.

If ORG* = -60º

it displays between -60º and 300º / displays between -420 and -60º

It returns the real tool base position value, referred to part zero, of the selected axis.

It returns the theoretical position value (real coordinate + following error) of the tool base referred to part zero.

The CNC updates this variable whenever probing operations "G75, G76" and probing cycles "PROBE are carried out.

When the digital probe communicates with the CNC via infrared beams, there could be some delay (milliseconds) from the time the probe touches the part to the instant the CNC receives the probe signal.

·M· MODEL (SOFT V11.1X)

302

FLWE(X-C) DEFLEX DEFLEY DEFLEZ DPLY(X-C) DRPO(X-C)
GPOS(X-C)n p

Programming manual

Although the probe keeps moving until the CNC receives the probing signal, the CNC takes into account the value assigned to general machine parameter PRODEL and provides the following information in the variables TPOS(X-C) and DPOS(X-C).
TPOS(X-C) Actual position of the probe when the CNC receives the probe signal.
DPOS(X-C) Theoretical position of the probe when the probe touched the part.

It returns the following error of the selected axis.
They return the amount of deflection obtained at the time by the Renishaw probe SP2 on each axis X, Y, Z.

13.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

It returns the position value (coordinate) shown on the screen for the selected axis.
It returns the position indicated by the Sercos drive of the selected axis (variable PV51 or PV53 of the drive).
Programmed coordinate for a particular axis in the indicated (n) block of the (p) program.
(P80=GPOSX N99 P100) It assigns to parameter P88 the value of the coordinate programmed for the X axis in the block having the label N99 and located in program P100.
Only programs located in the CNC's RAM memory may be consulted.
If the defined program or block does not exist, it shows the relevant error message. If the indicated block does not contain the requested axis, it returns the value 100000.0000.

DIST(X-C)
LIMPL(X-C) LIMMI(X-C)

Read-and-write variables
These variables may be used to read or modify the distance traveled by the selected axis. This value is accumulative and is very useful when it is required to perform an operation which depends on the distance traveled by the axes, their lubrication for example.
(P110=DISTX) It assigns to P110 the distance traveled by the X axis
(DISTX=P111) It presets the variable indicating the distance traveled by the Z axis with the value of arithmetic parameter P111.
Accessing any of the DIST(X-C) variables interrupts block preparation and the CNC waits for that command to be executed before resuming block preparation.
With these variables, it is possible to set a second travel limit for each axis: LIMPL for the upper limit and LIMMI for the lower one.
Since the second limits are activated or deactivated from the PLC, through general logic input ACTLIM2 (M5052), besides setting the limits, an auxiliary M code must be executed to let it know.
It is also recommended to execute function G4 after the change so the CNC executes the following blocks with the new limits.
The second travel limit will be taken into account if the first one has been set using axis machine parameters LIMIT+ (P5) and LIMIT- (P6).

CNC 8040
·M· MODEL (SOFT V11.1X)

303

Programming manual
13.2.8 Variables associated with electronic handwheels

13.
CNC 8040
·M· MODEL (SOFT V11.1X)

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

HANPF HANPS HANPT HANPFO
HANDSE
HANFCT

Read-only variables
They return the pulses of the first (HANPF), second (HANPS), third (HANPT) or fourth (HANPFO) handwheel received since the CNC was turned on. It is irrelevant to have the handwheel connected to the feedback inputs or to the PLC inputs.

For handwheels with axis selector button, it indicates whether that button has been pressed or not. A value of ·0· means that it has not been pressed.

It returns the multiplying factor set by PLC for each handwheel.

It must be used when using several electronic handwheels or when using a single handwheel but different multiplying factors (x1, x10, x100) are to be applied to each axis.

c b a c b a c b a c b a c b a c b a c b a c b a c b a lsb

Once the switch has been turned to one of the handwheel positions, the CNC checks this variable and, depending on the values assigned to each axis bit (c, b, a) it applies the multiplying factor selected for each one of them.
cba 0 0 0 The value indicated at the front panel or keyboard switch. 0 0 1 x1 factor 0 1 0 x10 factor 1 0 0 x100 factor

If there are more than one bit set to "1" for an axis, the least significant bit will be considered. Thus:
cba 1 1 1 x1 factor 1 1 0 x10 factor

i
HBEVAR

The screen always shows the value selected at the switch.

It must be used when having a Fagor HBE handwheel.

It indicates whether the HBE handwheel is enabled or not, the axis to be jogged and the multiplying factor to be applied (x1, x10, x100).

c b a c b a c b a c b a c b a c b a c b a c b a c b a lsb

(*) Indicates whether the HBE handwheel pulses will be taken into account or not in jog mode.
0 = They are ignored.
1 = They are taken into account.
(^) When the machine has a general handwheel and individual handwheels (associated with an axis), it indicates which handwheel has priority when both are turned at the same time.
0 = The individual handwheel has priority. The relevant axis ignores the pulses from the general handwheel, the rest of the axes don't.
1 = The general handwheel has priority. It ignores the pulses from the individual handwheel.

304

MASLAN

Programming manual

(a, b, c) Indicate the axis to be moved and the selected multiplying factor. cba 0 0 0 The value indicated at the front panel or keyboard switch. 0 0 1 x1 factor 0 1 0 x10 factor 1 0 0 x100 factor

If several axes are selected, the following order of priority is applied: X, Y, Z, U, V, W, A, B, C.
If there are more than one bit set to "1" for an axis, the least significant bit will be considered. Thus:
cba 1 1 1 x1 factor 1 1 0 x10 factor

13.

The HBE handwheel has priority. That is, regardless of the mode selected at the CNC switch (continuous or incremental JOG, handwheel), HBEVAR is set to other than "0", the CNC goes into handwheel mode.
It shows the selected axis in reverse video and the multiplying factor selected by the PLC. When the HBEVAR variable is set to "0", it shows the mode selected by the switch again.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

Read-and-write variables
It must be used when the path-handwheel or the path-jog is selected. Indicates the angle of the linear path.

MASCFI MASCSE

They must be used when the path-handwheel or the path-jog is selected.
On circular paths (arcs), they indicate the center coordinates.

CNC 8040
·M· MODEL (SOFT V11.1X)
305

Programming manual
13.2.9 Variables associated with feedback

13.

ASIN(X-C) BSIN(X-C) ASINS BSINS SASINS SBSINS

"A" signal of the CNC's sinusoidal feedback for the X-C axis. "B" signal of the CNC's sinusoidal feedback for the X-C axis. "A" signal of the CNC's sinusoidal feedback for the spindle. "B" signal of the CNC's sinusoidal feedback for the spindle. "A" signal of the CNC sinusoidal feedback for the second spindle. "B" signal of the CNC sinusoidal feedback for the second spindle.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

CNC 8040
·M· MODEL (SOFT V11.1X)
306

13.2.10 Variables associated with the main spindle

Programming manual

In these variables associated with the spindle, their values are given in revolutions per minute and the main spindle override values are given in integers from 0 to 255.
Certain variables interrupt block preparation (it is indicated in each one) and the CNC waits for that command to be executed before resuming block preparation.

SREAL
FTEOS SPEED
DNCS PLCS PRGS SSO
DNCSSO PLCSSO CNCSSO SLIMIT
DNCSL PLCSL PRGSL MDISL

Read-only variables
Returns the real main spindle turning speed in revolutions per minute. It interrupts block preparation.
(P100=SREAL) It assigns to P100 the real turning speed of the main spindle.
It returns the theoretical turning speed of the main spindle.
Returns, in revolutions per minute, the main spindle speed selected at the CNC.
This turning speed may be indicated by program, by PLC or by DNC; the CNC selects one of them, the one indicated by DNC has the highest priority and the one indicated by program has the lowest priority.
Returns the turning speed in revolutions per minute, selected by DNC. If it has a value of 0 it means that it is not selected.
Returns the turning speed in revolutions per minute selected by PLC. If it has a value of 0 it means that it is not selected.
Returns the turning speed in revolutions per minute, selected by program.
It returns the turning speed override (%) of the main spindle currently selected at the CNC. It is given in integer values between 0 and "MAXFOVR" (maximum 255).
This turning speed percentage of the main spindle may be indicated by program, by PLC, by DNC or by the front panel; the CNC selects one of them and the priority (from the highest to the lowest) is: by program, by DNC, by PLC and from the front panel.
It returns the turning speed override % of the main spindle currently selected via DNC. If it has a value of 0 it means that it is not selected.
It returns the turning speed override % of the main spindle currently selected by PLC. If it has a value of 0 it means that it is not selected.
It returns the turning speed override % of the main spindle currently selected from the front panel.
It returns the value set in rpm at the CNC for the turning speed limit of the main spindle.
This limit may be indicated by program, by PLC or by DNC; the CNC selects one of them, the one indicated by DNC has the highest priority and the one indicated by program has the lowest priority.
It returns the speed limit of the main spindle in rpm currently selected via DNC. If it has a value of 0 it means that it is not selected.
It returns the speed limit of the main spindle in rpm currently selected by PLC. If it has a value of 0 it means that it is not selected.
It returns the speed limit of the main spindle in rpm currently selected by program.
Maximum machining spindle speed. This variable is also updated (refreshed) when programming function G92 via MDI.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

13.
CNC 8040
·M· MODEL (SOFT V11.1X)

307

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

Programming manual POSS

RPOSS

TPOSS

13.

RTPOSS
DRPOS FLWES

SYNCER

PRGSSO

It returns the real position of the main spindle. Its value may be within ±99999.9999°. It interrupts block preparation.
It returns the real position of the main spindle in 360º module. Its value may be between 0 and 360º. It interrupts block preparation.
It returns the theoretical position of the main spindle (real position + lag). Its value may be within ±99999.9999º. It interrupts block preparation.
It returns the theoretical position of the main spindle (real position + lag) in 360º module. Its value may be between 0 and 360º. It interrupts block preparation.
Position indicated by the Sercos drive of the main spindle.
It returns the main spindle's following error in degrees (within ±99999.9999). It interrupts block preparation.
It returns, in degrees (within ±99999.9999), the following error of the second spindle with respect to the main spindle when they are synchronized in position.
Read-and-write variables
This variable may be used to read or modify the speed override percentage of the main spindle currently selected by program. It is given in integer values between 0 and "MAXFOVR" (maximum 255). If it has a value of 0 it means that it is not selected.
(P110=PRGSSO) It assigns to P110 the % of the main spindle speed selected by program.
(PRGSSO=P111) It sets the value indicating the main spindle speed % selected by program to the value of arithmetic parameter P111.

CNC 8040
·M· MODEL (SOFT V11.1X)
308

13.2.11 Variables associated with the second spindle

Programming manual

In these variables associated with the spindle, their values are given in revolutions per minute and the 2nd spindle override values are given in integers from 0 to 255.

SSREAL
SFTEOS SSPEED
SDNCS SPLCS SPRGS SSSO
SDNCSO SPLCSO SCNCSO SSLIMI
SDNCSL SPLCSL SPRGSL SPOSS

Read-only variables
Returns the real 2nd spindle turning speed in revolutions per minute.
(P100=SSREAL) It assigns to P100 the real turning speed of the second spindle.
If this variable is accessed, block preparation is interrupted and the CNC waits for this command to be executed to resume block preparation.
It returns the theoretical turning speed of the second spindle.
Returns, in revolutions per minute, the 2nd spindle speed selected at the CNC.
This turning speed may be indicated by program, by PLC or by DNC; the CNC selects one of them, the one indicated by DNC has the highest priority and the one indicated by program has the lowest priority.
Returns the turning speed in revolutions per minute, selected by DNC. If it has a value of 0 it means that it is not selected.
Returns the turning speed in revolutions per minute selected by PLC. If it has a value of 0 it means that it is not selected.
Returns the turning speed in revolutions per minute, selected by program.
It returns the turning speed override (%) of the second spindle currently selected at the CNC. It is given in integer values between 0 and "MAXFOVR" (maximum 255).
This turning speed percentage of the second spindle may be indicated by program, by PLC, by DNC or by the front panel; the CNC selects one of them and the priority (from the highest to the lowest) is: by program, by DNC, by PLC and from the front panel.
It returns the turning speed override % of the second spindle currently selected via DNC. If it has a value of 0 it means that it is not selected.
It returns the turning speed override % of the second spindle currently selected by PLC. If it has a value of 0 it means that it is not selected.
It returns the turning speed override % of the second spindle currently selected from the front panel.
It returns the value set in rpm at the CNC for the turning speed limit of the second spindle.
This limit may be indicated by program, by PLC or by DNC; the CNC selects one of them, the one indicated by DNC has the highest priority and the one indicated by program has the lowest priority.
It returns the speed limit of the second spindle in rpm currently selected via DNC. If it has a value of 0 it means that it is not selected.
It returns the speed limit of the second spindle in rpm currently selected by PLC. If it has a value of 0 it means that it is not selected.
It returns the speed limit of the second spindle in rpm currently selected by program.
It returns the real position of the second spindle. Its value will be given within ±99999.9999°

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

13.
CNC 8040
·M· MODEL (SOFT V11.1X)
309

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

Programming manual SRPOSS

STPOSS

SRTPOS

13.

SDRPOS SFLWES

SPRGSO

It returns the real position of the second spindle in 360º module. Its value will be given between 0 and 360º.
It returns the theoretical position of the second spindle (real position + lag). Its value may be within ±99999.9999º.
Returns the second spindle's theoretical position value (real coordinate+ following error) in a 360º module. Its value may be between 0 and 360º.
Position indicated by the Sercos drive of the second spindle.
It returns the second spindle's following error in degrees (within ±99999.9999).
When accessing one of these variables SPOSS, SRPOSS, STPOSS, SRTPOSS or SFLWES, block preparation is interrupted and the CNC waits for that command to be executed before resuming block preparation.
Read-and-write variables
This variable may be used to read or modify the speed override percentage of the second spindle currently selected by program. It is given in integer values between 0 and "MAXFOVR" (maximum 255). If it has a value of 0 it means that it is not selected.
(P110=SPRGSO) It assigns to P110 the % of the second spindle speed selected by program.
(SPRGSO=P111) It sets the value indicating the second spindle speed % selected by program to the value of arithmetic parameter P111.

CNC 8040
·M· MODEL (SOFT V11.1X)
310

13.2.12 Variables associated with the live tool

Programming manual

ASPROG

Read-only variables
It must be used inside the subroutine associated with function M45. It returns the rpm programmed by M45 S. When programming M45 alone, the variable takes the value of "0". The ASPROG variable is updated just before executing the M45 function so it is already updated when executing its associated subroutine.

13.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

CNC 8040
·M· MODEL (SOFT V11.1X)
311

Programming manual
13.2.13 PLC related variables

13.

It should be borne in mind that the PLC has the following resources:

(I1 thru I256)

Inputs.

(O1 thru O256)

Outputs.

M1 thru M5957) Marks.

(R1 thru R499)

32-bit registers.

(T1 thru T256)

Timers with a timing count in 32 bits.

(C1 thru C256)

Counters with a count in 32 bits.

If any variable is accessed which allows the status of a PLC variable to be read or modified (I,O,M,R,T,C), block preparation is interrupted and the CNC waits for this command to be executed in order to restart block preparation.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

PLCMSG

Read-only variables
Returns the number of the active PLC message with the highest priority and will coincide with the number displayed on screen (1··128). If there is none, it returns 0.
(P110=PLCMSG) It assigns to P100 the number of the active PLC message with the highest priority.

PLCIn PLCOn

CNC 8040
·M· MODEL (SOFT V11.1X)

PLCMn PLCRn PLCTn PLCCn

Read-and-write variables
This variable allows 32 PLC inputs to be read or modified starting with the one indicated (n).
The value of the inputs which are used by the electrical cabinet cannot be modified as their values are determined by it. Nevertheless, the status of the remaining inputs can be modified.
This variable allows 32 PLC outputs to be read or modified starting from the one indicated (n).
(P110=PLCO 22) It assigns to parameter P110 the value of outputs O22 through O53 (32 outputs) of the PLC.
(PLCO 22=$F) It sets outputs O22 through O25 to "1" and outputs O26 through O53 to "0".

Bit Output

31 30 29 28 27 26 25 24 23 22 ... 5 4 3 2 1 0 0 0 0 0 0 0 0 0 0 0 .... 0 0 1 1 1 1 53 52 51 50 49 48 47 46 45 44 .... 27 26 25 24 23 22

This variable allows 32 PLC marks to be read or modified starting from the one indicated (n).
This variable allows the status of 32 register bits to be read or modified starting from the one indicated (n).
This variable allows the timer count to be read or modified starting from the one indicated (n).
This variable allows the counter count to be read or modified starting from the one indicated (n).

312

PLCMMn

This variable permits reading or modifying the PLC mark (n).

Programming manual

(PLMM4=1) It sets mark M4 to ·1· and leaves the rest untouched.
(PLCM4=1) It sets mark M4 to ·1· and the following 31 marks (M5, through M35) to ·0·

13.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

CNC 8040
·M· MODEL (SOFT V11.1X)
313

Programming manual
13.2.14 Variables associated with local parameters
The CNC allows 26 local parameters (P0-P25) to be assigned to a subroutine, by using mnemonics PCALL and MCALL. In addition to performing the required subroutine these mnemonics allow local parameters to be initialized.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

13.

CALLP

Read-only variables

Allows us to know which local parameters have been defined and which have not, in the call to the subroutine by means of the PCALL or MCALL mnemonic.

The information will be given in the 26 least significant bits (bits 0··25), each of these corresponding to the local parameter of the same number; thus bit 12 corresponds to P12.

Each bit will indicate whether the corresponding local parameter has been defined (=1) or not (0).

Bit

31 30 29 28 27 26 25 24 23 22 ... 5 4 3 2 1 0

0 0 0 0 0 0 * * * * ... * * * * * *

Example: ;Call to subroutine 20. (PCALL 20, P0=20, P2=3, P3=5) ... ... ;Beginning of subroutine 20. ( SUB 20) (P100 = CALLP) ... ...
In parameter P100 the following will be obtained:
0000 0000 0000 0000 0000 0000 0000 1101 LSB

CNC 8040
·M· MODEL (SOFT V11.1X)
314

13.2.15 Sercos variables

Programming manual

They are used in the data exchange via Sercos between the CNC and the drives.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

TSVAR(X-C) TSVARS TSSVAR

Read-only variables
It returns the third attribute of the Sercos variable corresponding to the "identifier". The third attribute is used in particular software applications and its information is coded according to the Sercos standard.
TSVAR(X-C) identifier ... for the axes. TSVARS identifier ... for the main spindle. TSSVAR identifier ... for the second spindle.
(P110=SVARX 40) It assigns to parameter P110 the third attribute of the Sercos variable of identifier 40 of the X axis which corresponds to "VelocityFeedback"

13.

SETGE(X-C) SETGES SSETGS

Write variables
The drive may have up to 8 gear ratios (0 through 7). Sercos identifier 218, GearRatioPreselection.
It may also have up to 8 parameter sets (0 through 7). Sercos identifier 217, ParameterSetPreselection.
With these variables the work range or gear ratio and the parameter set of each drive may be modified.
SETGE(X-C) ... for the axes. SETGES ... for the main spindle. SSETGS ... for the second spindle
The 4 least significant bits of these variables indicate the gear ratio and the other 4 the parameter set to be selected.

SVAR(X-C) SVARS SSVARS

Read-and-write variables

They permit reading or modifying the value of the Sercos variable corresponding to the axis identifier.

SVAR(X-C) identifier ... for the axes.

SVARS

identifier ... for the main spindle.

SSVARS identifier ... for the second spindle.

CNC 8040

·M· MODEL (SOFT V11.1X)

315

Programming manual
13.2.16 Software & hardware configuration variables

13.

HARCON

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

HARCOA
CNC 8040

Read-only variables

It indicates, with bits, the CNC's hardware configuration. The bit will be "1" when the relevant configuration is available.

Bit

Meaning

Turbo board.

4, 3, 2, 1

0100 8040 model

Sercos (digital model).

Reserved.

9, 8, 7

000

Expansion board missing.

001

"Feedback + I/O" expansion board.

010

Feedback-only expansion board.

011

I/O-only expansion board.

101

"Axes 2" board for expansion of "feedback + I/O".

110

"Axes 2" board for expansion of feedback only.

111

"Axes 2" board for expansion of I/O only.

Axis board with 12-bit (=0) or 16-bit (=1) Digital/Analog converter.

14, 13, 12, 11 Reserved.

It has CAN (digital module).

18,17,16

Keyboard type (technical service department).

20,19

CPU type (technical service department).

23,22,21

000

Memkey card (4 Mb).

010

Memkey card (24 Mb).

110

Memkey card (512 Kb).

111

Memkey card (2 Mb).

26,25,24

000

Color LCD Monitor.

001

Monochrome LCD monitor.

28,27

Turbo board at 25 MHz

Turbo board at 40 MHz

Ethernet.

Compact flash.

It indicates, with bits, the CNC's hardware configuration. The bit will be "1" when the relevant configuration is available.

Bit

Meaning

"Axes 2" board.

It has a connector for compact flash.

Bit ·1· only indicates whether the hardware has a connector for the compact flash or not, it does not indicate whether the compact flash is inserted or not.

·M· MODEL (SOFT V11.1X)

316

IDHARH IDHARL
SOFCON
HDMEGA KEYIDE

Programming manual
They return, in BCD code, the hardware identification number corresponding to the memkey card. It is the number appearing on the software diagnosis screen.
Since the identification number has 12 digits, the IDHARL variable shows the 8 least significant bits and the IDHARH the 4 most significant bits.
Example:

29ADEE020102

000029AD EE020102

IDHART IDHARL

13.

They return the software version numbers for the CNC and the hard disk. Bits 15-0 return the CNC software version (4 digits) Bits 31-16 return the software version of the hard disk (HD) (4 digits)

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

... 31 30 29 ... 18 17 16 15 14 13 ... 2 1 0
LSB

HD Software

CNC Software

For example, SOFCON 01010311 indicates: Hard disk (HD) software version CNC software version

0101 0311

Hard disk size (in megabytes).

Keyboard code, according to the auto-identification system.

KEYIDE 0
130 131 132 133 135 136 137 138

CUSTOMY (P92) - - 254 254 254 254 252 0 0 0

Keyboard Keyboard without auto-identification. Mill model keyboard. Lathe model keyboard. Conversational mill model keyboard. Conversational lathe model keyboard. Operator panel: OP.8040/55.ALFA Operator panel: OP.8040/55.MC Operator panel: OP.8040/55.TC Operator panel: OP.8040/55.MCO/TCO

CNC 8040

·M· MODEL (SOFT V11.1X)

317

Programming manual
13.2.17 Variables associated with telediagnosis

13.

HARSWA HARSWB

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

HARTST

CNC 8040

Read-only variables

They return, in 4 bits, the central unit configuration, a value of "1" if it is present and "0" if not.

HARSWA

HARSWB

Bits

Board

31 - 28 Large sercos

27 - 24 I/O 4

23 - 20 I/O 3

19 - 16 I/O 2

15 - 12 I/O 1

11- 8

Axes:

7 -4

Turbo

3 - 0 (LSB) CPU

Bits

Board

31 - 28

27 - 24

23 - 20

19 - 16

15 - 12

0 - CAN board missing 1 - CAN board in COM1 2 - CAN board in COM2 3 - Board in both COM

11- 8

Small sercos

7 -4

3 - 0 (LSB) HD

There may be two types of CAN boards (value of ·0001· if it is an SJ1000 type and value of ·0010· if it is an OKI9225 type).

It returns the result of the hardware test. The data comes at the least significant bits with a "1" if it failed and with a "0" if OK or if the relevant board is missing.

Bits

Inside temperature

I/O 3

I/O 2

I/O 1

Axes:

+3.3 V

GND

GNDA

-15 V

+15 V

Battery

-5 V

0 (LSB) +5 V

(Board voltage) (Board voltage) (Board voltage)
(Board voltage) (Power supply) (Power supply) (Power supply) (Power supply) (Power supply) (Power supply) (Power supply) (Power supply)

·M· MODEL (SOFT V11.1X)

318

MEMTST
NODE VCHECK IONODE IOSLOC IOSREM

Programming manual
It returns the result of the memory test. Each data uses 4 bits that will be at "1" if the test is OK and will have a value other than "1" if there is an error.

Bits 30 ... ... 19 - 16

Test Test status ... ... Caché

Bits

Test

15 - 12

Sdram

11- 8

7 -4

Flash

3 - 0 (LSB) Ram

Bit 30 stays at "1" during the test.

It returns the number of the node assigned to the CNC in the Sercos ring.

It returns the checksum of the code for the software version installed. It is the value appearing on the code test.

It returns in 16 bits the position of the "ADDRESS" switch of the CAN of the I/O. If it is not connected, it returns the value 0xFFFF.

They may be used to read the number of local digital I/O available.

Bit
0 - 15 16 - 31

Meaning
Number of inputs. Number of outputs.

They may be used to read the number of remote digital I/O available.

Bit
0 - 15 16 - 31

Meaning
Number of inputs. Number of outputs.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

13.

CNC 8040
·M· MODEL (SOFT V11.1X)
319

Programming manual
13.2.18 Operating-mode related variables

13.

OPMODE

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

CNC 8040
·M· MODEL (SOFT V11.1X)
320

Read-only variables related to the standard mode
It returns the code corresponding to the selected operating mode. 0 = Main menu.
10 = Automatic execution. 11 = Single block execution. 12 = MDI in EXECUTION. 13 = Tool inspection. 14 = Repositioning. 15 = Block search executing G. 16 = Block search executing G, M, S, T.
20 = Theoretical path simulation. 21 = G function simulation. 22 = G, M, S and T function simulation. 23 = Simulation with movement in the main plane. 24 = Simulation with rapid movement. 25 = Rapid simulation with S=0.
30 = Normal editing. 31 = User editing. 32 = TEACH-IN editing. 33 = Interactive editor. 34 = Profile editor.
40 = Movement in continuous JOG. 41 = Movement in incremental JOG. 42 = Movement with electronic handwheel. 43 = HOME search in JOG. 44 = Position preset in JOG. 45 = Tool calibration. 46 = MDI in JOG. 47 = User JOG operation.
50 = Zero offset table. 51 = Tool offset table. 52 = Tool table. 53 = Tool magazine table. 54 = Global parameter table. 55 = Local parameter table. 56 = User parameter table. 57 = OEM parameter table.
60 = Utilities.
70 = DNC status. 71 = CNC status.

OPMODE

Programming manual

80 = PLC file editing. 81 = PLC program compilation. 82 = PLC monitoring. 83 = Active PLC messages. 84 = Active PLC pages. 85 = Save PLC program. 86 = Restore PLC program. 87 = PLC usage maps. 88 = PLC statistics.
90 = Customizing.
100 = General machine parameter table. 101 = Axis machine parameter tables. 102 = Spindle machine parameter table. 103 = Serial port machine parameter tables. 104 = PLC machine parameter table. 105 = M function table. 106 = Leadscrew error compensation tables and cross compensation tables. 107 = Machine parameter table for Ethernet.
110 = Diagnosis: configuration. 111 = Diagnosis: hardware test. 112 = Diagnosis: RAM memory test. 113 = Diagnosis: Flash memory test. 114 = User diagnosis. 115 = Hard disk diagnosis (HD). 116 = Circle geometry test. 117 = Oscilloscope.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

13.

Read-only variables related to the conversational mode (MC, MCO) and configurable mode M, ([SHIFT]-[ESC]).
In these work modes, it is recommended to use variables OPMODA, OPMODB and OPMODC. The OPMODE variable is generic and contains different values to those of the standard mode.
It returns the code corresponding to the selected operating mode. 0 = CNC starting up. 10 = In execution mode. In execution or waiting for the [CYCLE START] key (drawing of the [CYCLE START] on top). 21 = In graphic simulation mode. 30 = Cycle editing. 40 = In Jog mode (standard screen). 45 = In tool calibration mode. 60 = Managing parts. PPROG mode.

CNC 8040
·M· MODEL (SOFT V11.1X)

321

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

Programming manual OPMODA
13.
OPMODB
OPMODC
CNC 8040
·M· MODEL (SOFT V11.1X)

Indicates the operating mode currently selected when working with the main channel.

Use the OPMODE variable to know at any time the selected operating mode (main channel, user channel, PLC channel).

This information is given at the least significant bits with a "1" when active and with a "0" when not active or when it is not available in the current version.

Bit 0

Program in execution.

Bit 1

Program in simulation.

Bit 2

Block in execution via MDI, JOG.

Bit 3

Repositioning in progress.

Bit 4

Program interrupted by CYCLE STOP.

Bit 5

MDI, JOG block interrupted.

Bit6

Repositioning interrupted.

Bit 7

In tool inspection.

Bit 8

Block in execution via CNCEX1.

Bit 9

CNCEX1 block interrupted.

Bit 10

CNC ready to accept JOG movements: jog, handwheel, teach-in, inspection.

Bit 11

CNC ready to receive the CYCLE START command: execution, simulation and MDI modes.

Bit 12

The CNC is not ready to execute anything involving axis or spindle movement.

Bit 13

It identifies the block search.

Indicates the type of simulation currently selected. This information is given at the least significant bits indicating with a "1" the one currently selected.

Bit 0

Theoretical path.

Bit 1

G functions.

Bit 2

G M S T functions.

Bit 3

Main plane.

Bit 4

Rapid.

Bit 5

Rapid (S=0).

Indicates the axes selected by handwheel. This information is given at the least significant bits indicating with a "1" the one currently selected.

Bit 0

Axis 1.

Bit 1

Axis 2.

Bit 2

Axis 3.

Bit 3

Axis 4.

Bit 4

Axis 5.

Bit 5

Axis 6.

Bit 6

Axis 7.

Bit 7

Bit 8

The axis name corresponds to the number according to the programming order for them.

Example: If the CNC controls axes X, Y, Z, U, B, C, axis 1=X, axis2=Y, axis3=Z, axis4=U, axis5=B, axis6=C.

322

13.2.19 Other variables

Programming manual

NBTOOL
PRGN BLKN GSn MSn PLANE

Read-only variables
Indicates the tool number being managed. This variable can only be used within the tool change subroutine. Example: There is a manual tool changer. Tool T1 is currently selected and the operator requests tool T5. The subroutine associated with the tools may contain the following instructions:
(P103 = NBTOOL) (MSG "SELECT T?P103 AND PRESS CYCLE START") Instruction (P103 = NBTOOL) assigns the number of the tool currently being managed to parameter P103. Therefore, P103=5 The message displayed by the CNC will be ""SELECT T5 AND PRESS CYCLE START".
Returns the program number being executed. Should none be selected, a value of -1 is returned.
It returns the label number of the last executed block.
Returns the status of the G function indicated (n). 1 if it is active and 0 if not.
(P120=GS17) It assigns the value 1 to parameter P120 if the G17 function is active and 0 if not.
Returns the status of the M function indicated (n). 1 if it is active and 0 if not. These functions are M00, M01, M02, M03, M04, M05, M06, M08, M09, M19, M30, M41, M42, M43, M44 and M45.
Returns data on the abscissa axis (bits 4 to 7) and the ordinate axis (bits 0 to 3) of the active plane in 32 bits and in binary.
... ... ... ... ... ... 7654 3210 lsb

Abscissa axis

Ordinate axis

The axes are coded in 4 bits and indicate the axis number according to the programming order.
Example: If the CNC controls the X,Y,Z,U,B,C axes and the ZX plane (G18) is selected.
(P122 = PLANE) assigns the value of $31 to parameter P122.

0000 0000 0000 0000 0000 0000 0011 0001 LSB

Abscissa axis Ordinate axis

= 3 (0011) = 1 (0001)

=> Z axis => X axis

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

13.
CNC 8040

·M· MODEL (SOFT V11.1X)

323

Programming manual LONGAX

13.

MIRROR

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

SCALE SCALE(X-C) ORGROT ROTPF
ROTPS
PRBST
CLOCK
TIME
CNC 8040
·M· MODEL (SOFT V11.1X)

It returns the number according to the programming order corresponding to the longitudinal axis. This will be the one selected with the G15 function and by default the axis perpendicular to the active plane, if this is XY, ZX or YZ.
Example:
If the CNC controls the X, Y, Z, U, B, C axes and the U axis is selected.
(P122 = LONGAX) assigns the value 4 to parameter P122.
Returns in the least significant bits of the 32-bit group, the status of the mirror image of each axis, 1 in the case of being active and 0 if not.
Bit 8 Bit 7 Bit 6 Bit 5 Bit 4 Bit 3 Bit 2 Bit 1 Bit 0 LSB Axis 7 Axis 6 Axis 5 Axis 4 Axis 3 Axis 2 Axis 1
The axis name corresponds to the number according to the programming order for them.
Example: If the CNC controls axes X, Y, Z, U, B, C, axis 1=X, axis2=Y, axis3=Z, axis4=U, axis5=B, axis6=C.
It returns the general scaling factor being applied.
Returns the specific scaling factor of the indicated axis (X-C).
It returns the rotation angle of the coordinate system currently selected with G73. Its value is given in degrees (within ±99999.9999).
Returns the abscissa value of the rotation center with respect to the Cartesian coordinate origin. It is given in the active units:
If G70, in inches (within ±3937.00787). If G71, in millimeters (within ±99999.9999).
Returns the ordinate value of the rotation center with respect to the Cartesian coordinate origin. It is given in the active units:
If G70, in inches (within ±3937.00787). If G71, in millimeters (within ±99999.9999).
Returns probe status. 0 = the probe is not touching the part. 1 = the probe is touching the part.
If this variable is accessed, block preparation is interrupted and the CNC waits for this command to be executed to resume block preparation.
Returns the time in seconds indicated by the system clock. Possible values 0..4294967295.
If this variable is accessed, block preparation is interrupted and the CNC waits for this command to be executed to resume block preparation.
Returns the time in hours-minutes-seconds format.
(P150=TIME) Loads P150 with hh-mm-ss. For example if the time is: 34sec. P150 = 182234.
If this variable is accessed, block preparation is interrupted and the CNC waits for this command to be executed to resume block preparation.

324

DATE
CYTIME FIRST
ANAIn AXICOM
TANGAN TPIOUT(X-C) TIMEG TIPPRB PANEDI DATEDI

Returns the date in year-month-day format.

Programming manual

(P151=DATE)
It assigns to P151 the year-month-day. For example if the date is April 25th 1992, P151 = 920425.

If this variable is accessed, block preparation is interrupted and the CNC waits for this command to be executed to resume block preparation.

It returns the amount of time (in hundredths of a second) elapsed executing the part. It ignores the time the execution has been interrupted. Possible values 0..4294967295.
If this variable is accessed, block preparation is interrupted and the CNC waits for this command to be executed to resume block preparation.

Indicates whether it is the first time that a program has been run or not. It returns a value of 1 if it is the first time and 0 if not.
A first-time execution is considered as being one which is done: · After turning on the CNC. · After pressing [SHIFT]+[RESET]. · Every time a new program is selected.

Returns in volts and in ±1.4 format (values ±5 Volts), the status of the analog input indicated (n), it being possible to select one among eight (1··8) analog inputs.
If this variable is accessed, block preparation is interrupted and the CNC waits for this command to be executed to resume block preparation.

It returns in the 3 least significant bits the axis pairs switched with function G28.

Pair 3

Pair 2

Pair 1

Axis 2 Axis 1 Axis 2 Axis 1 Axis 2 Axis 1 LSB

The axes are coded in 4 bits and indicate the axis number (1 to 7) according to their programming order.

If the CNC controls the X, Y, Z, B, C axes and G28BC has been programmed, the AXICOM variable will show:

Pair 3 0000 0000

Pair 2 0000 0000

Pair 1

0101 0100 LSB

Variable associated with the tangential control function, G45. It indicates the programmed angular position.
Output of the PI of the tandem master axis in rpm.
It shows the timing status of the timer programmed with G4 K in the CNC channel. This variable, returns the time remaining to end the timing block in hundredths of a second.
It indicates the PROBE cycle being executed at the CNC.
WGDRAW application. Number of the screen created by the user or the manufacturer and is being consulted.
WGDRAW application. Number of the element (item) being consulted.

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

13.
CNC 8040
·M· MODEL (SOFT V11.1X)

325

HIGH-LEVEL LANGUAGE PROGRAMMING Variables

Programming manual TIMER PARTC
13.
KEY
KEYSRC
ANAOn
SELPRO DIAM
CNC 8040
·M· MODEL (SOFT V11.1X)

Read-and-write variables
This variable allows reading or modifying the time, in seconds, indicated by the clock enabled by the PLC. Possible values 0..4294967295.
If this variable is accessed, block preparation is interrupted and the CNC waits for this command to be executed to resume block preparation.
The CNC has a part counter whose count increases, in all modes except simulation, every time M30 or M02 is executed and this variable allows its value to be read or modified. This value will be between 0 and 4294967295
If this variable is accessed, block preparation is interrupted and the CNC waits for this command to be executed to resume block preparation.
Returns the code of the last key accepted.
This variable may be used as a write variable only inside a customizing program (user channel).
If this variable is accessed, block preparation is interrupted and the CNC waits for this command to be executed to resume block preparation.
This variable allows reading or modifying the source of keystrokes, possible values being:
0 = Keyboard. 1 = PLC. 2 = DNC.
The CNC only allows modification of this variable if this is at 0.
This variable allows the required analog output (n) to be read or modified. The value assigned will be expressed in volts and in the ±2.4 format (±10 V).
The analog outputs which are free among the eight (1 through 8) available at the CNC may be modified, the corresponding error being displayed if an attempt is made to write in one which is occupied.
If this variable is accessed, block preparation is interrupted and the CNC waits for this command to be executed to resume block preparation.
When having two probe inputs, it allows selecting the active input.
On power-up, it assumes the value of ·1· thus selecting the first probe input. To select the second probe input, set it to a value of ·2·.
Accessing this variable from the CNC interrupts block preparation.
It changes the programming mode for X axis coordinates between radius and diameter. When changing the value of this variable, the CNC assumes the new way to program the following blocks.
When the variable is set to ·1·, the programmed coordinates are assumed in diameter; when is set to ·0·, the programmed coordinates are assumed in radius.
This variable affects the display of the real value of the X axis in the coordinate system of the part and the reading of variables PPOSX, TPOSX and POSX.
On power-up, after executing an M02 or M30 and after an emergency or a reset, the variable is initialized according to the value of the DFORMAT parameter of the X axis. If this parameter has a value equal to or greater than 4, the variable takes a value of 1; otherwise, it takes the value of ·0·.

326

13.3 Constants

Programming manual

Constants are defined as being all those fixed values which cannot be altered by a program. The following are considered as constants:
· Numbers expressed in the decimal system. · Hexadecimal numbers. · PI constant. · Read-only tables and variables as their value cannot be altered with a program.
13.4 Operators

13.

HIGH-LEVEL LANGUAGE PROGRAMMING Constants

An operator is a symbol that indicates the mathematical or logic operations to carry out. The CNC has arithmetic, relational, logic, binary, trigonometric operators and special operators.

Arithmetic operators.

+ -
* / MOD EXP

add.

P1=3 + 4

subtraction, also a negative value.

P2=5 - 2 P3= -(2 * 3)

multiplication.

P4=2 * 3

division.

P5=9 / 2

Module or remainder of the division. P6=7 MOD 4

exponential.

P7=2 EXP 3

P1=7 P2=3 P3=-6 P4=6 P5=4.5 P6=3 P7=8

Relational operators.

equal.

different.

greater than.

greater than or equal to.

Less than.

Less than or equal to.

Logic and binary operators.
NOT, OR, AND, XOR: The act as logic operators between conditions and as binary operators between variables and constants.
IF (FIRST AND GS1 EQ 1) GOTO N100 P5 = (P1 AND (NOT P2 OR P3))

CNC 8040

·M· MODEL (SOFT V11.1X)

327

HIGH-LEVEL LANGUAGE PROGRAMMING Operators

Programming manual
13.

Trigonometric functions.

SIN COS TAN ASIN ACOS ATAN ARG

sine. cosine. tangent. arc sine. arc cosine. arc tangent. ARG(x,y) arctangent y/x.

P1=SIN 30 P1=0.5 P2=COS 30 P2=0.8660 P3=TAN 30 P3=0.5773 P4=ASIN 1 P4=90 P5=ACOS 1 P5=0 P6=ATAN 1 P6=45 P7=ARG(-1,-2) P7=243.4349

There are two functions for calculating the arc tangent ATAN which returns the result between ±90° and ARG given between 0 and 360°.

Other functions.

ABS

absolute value.

LOG

decimal logarithm.

SQRT square root.

ROUND rounding up an integer number.

FIX

Integer.

FUP

if integer takes integer. if not, takes entire part + 1.

BCD

converts given number to BCD.

P1=ABS -8

P1=8

P2=LOG 100

P2=2

P3=SQRT 16

P3=4

P4=ROUND 5.83 P4=6

P5=FIX 5.423

P5=5

P6=FUP 7 P6=FUP 5,423

P6=7 P6=6

P7=BCD 234

P7=564

0010 0011 0100

BIN

converts given number to binary.

P8=BIN $AB

P8=171

1010 1011

Conversions to binary and BCD are made in 32 bits, it being possible to represent the number 156 in the following formats:

decimal

156

Hexadecimal

Binary

0000 0000 0000 0000 0000 0000 1001 1100

BCD

0000 0000 0000 0000 0000 0001 0101 0110

CNC 8040
·M· MODEL (SOFT V11.1X)
328

13.5 Expressions

Programming manual

An expression is any valid combination of operators, constants, parameters and variables.
All expressions must be placed between brackets, but if the expression is reduced to an integer, the brackets can be removed.

13.5.1 Arithmetic expressions

These are formed by combining functions and arithmetic, binary and trigonometric operators with the constants and variables of the language.

The priorities of the operators and the way they can be associated determine how these expressions are calculated:

Priority from highest to lowest To be associated

NOT, functions, - (negative)

from right to left.

EXP, MOD

from left to right.

* , /

from left to right.

+,- (add, subtract)

from left to right.

Relational operators

from left to right.

AND, XOR

from left to right.

Brackets should be used in order to clarify the order in which the expression is to be evaluated.
(P3 = P4/P5 - P6 * P7 - P8/P9 )
(P3 = (P4/P5)-(P6 * P7)-(P8/P9))

Using redundant or additional brackets will neither cause errors nor slow down the execution.

In functions, brackets must be used except when these are applied to a numerical constant, in which case they are optional.

(SIN 45) (SIN (45)) they're both valid and equivalent.

(SIN 10+5)

the same as ((SIN 10)+5).

Expressions can be used also to reference parameters and tables:

(P100 = P9)

(P100 = P(P7))

(P100 = P(P8 + SIN(P8 * 20)))

(P100 = ORGX 55)

(P100 = ORGX (12+P9))

(PLCM5008 = PLCM5008 OR 1) ; Selects single block execution mode (M5008=1)

(PLCM5010 = PLCM5010 AND $FFFFFFFE) ; Frees feedrate override (M5010=0)

HIGH-LEVEL LANGUAGE PROGRAMMING Expressions

13.
CNC 8040
·M· MODEL (SOFT V11.1X)

329

Programming manual
13.5.2 Relational expressions

13.

These are arithmetic expressions joined by relational operators.
(IF (P8 EQ 12.8) ; It checks if the value of P8 is equal to 12.8.
(IF (ABS(SIN(P24)) GT SPEED) ;Analyzes if the sine is greater than the spindle speed.
(IF (CLOCK LT (P9 * 10.99)) ; Analyzes if the clock count is less than (P9 * 10.99)

At the same time these conditions can be joined by means of logic operators. (IF ((P8 EQ 12.8) OR (ABS(SIN(P24)) GT SPEED)) AND (CLOCK LT (P9 * 10.99)) ... The result of these expressions is either true or false.

HIGH-LEVEL LANGUAGE PROGRAMMING Expressions

CNC 8040
·M· MODEL (SOFT V11.1X)
330

PROGRAM CONTROL INSTRUCTIONS

The control instructions available to high-level programming can be grouped as follows:
· Assignment instructions. · Display instructions. · Enable-disable instructions. · Flow control instructions. · Subroutine instructions. · Probe related instructions. · Interruption-subroutine instructions. · Program instructions. · Screen customizing instructions.
Only one instruction can be programmed in each block, and no other additional information may be programmed in this block.

CNC 8040
·M· MODEL (SOFT V11.1X)
331

Programming manual
14.1 Assignment instructions

14.

This is the simplest type of instruction and can be defined as: (target = arithmetic expression)
A local or global parameter or a read-write variable may be selected as target. The arithmetic expression may be as complex as required or a simple numerical constant.
(P102 = FZLOY) (ORGY 55 = (ORGY 54 + P100))
In the specific case of designating a local parameter using its name (A instead of P0, for example) and the arithmetic expression being a numerical constant, the instruction can be abbreviated as follows:
(P0=13.7) ==> (A=13.7) ==> (A13.7)
Within a single block, up to 26 assignments can be made to different targets, a single assignment being interpreted as the set of assignments made to the same target.
(P1=P1+P2, P1=P1+P3, P1=P1*P4, P1=P1/P5) It is the same as saying:
(P1=(P1+P2+P3)*P4/P5).
The different assignments which are made in the same block will be separated by commas ",".

PROGRAM CONTROL INSTRUCTIONS Assignment instructions

CNC 8040
·M· MODEL (SOFT V11.1X)
332

14.2 Display instructions

Programming manual

(ERROR integer, "error text")
This instruction stops the execution of the program and displays the indicated error, it being possible to select this error in the following ways:
(ERROR integer) This will display the error number indicated and the text associated to this number according to the CNC error code (should there be one).
(ERROR integer, "error text") This will display the number and the error text indicated, it being necessary to write the text between quote marks "".
(ERROR "error text"). This will display the error text only.

The error number may be defined by means of a numerical constant or an arithmetic parameter. When using a local parameter, its numeric format must be used (P0 thru P25 instead of A thru Z).
Programming examples: (ERROR 5) (ERROR P100) (ERROR "User error") (ERROR 3, "User error") (ERROR P120, "User error)

(MSG "message") This instruction will display the message indicated between quote marks.

The CNC screen is provided with an area for displaying DNC or user program messages, and always displays the last message received irrespective of where it has come from.
Example: (MSG "Check tool")

(DGWZ expression 1, expression 2, expression 3, expression 4, expression 5, expression 6)

The DGWZ instruction (Define Graphic Work Zone) defines the graphics area.

Each expression forming the instruction syntax correspond to one of the limits and they must be defined in millimeters or inches.

expression 1

X minimum

expression 2

X maximum

expression 3

Y minimum

expression 4

Y maximum

expression 5

Z minimum

expression 6

Z maximum

PROGRAM CONTROL INSTRUCTIONS Display instructions

14.
CNC 8040

·M· MODEL (SOFT V11.1X)

333

Programming manual
14.3 Enabling-disabling instructions

14.

PROGRAM CONTROL INSTRUCTIONS Enabling-disabling instructions

(ESBLK and DSBLK)
After executing the mnemonic ESBLK, the CNC executes all the blocks that come after as if it were dealing with a single block.
This single block treatment is kept active until it is cancelled by executing the mnemonic DSBLK.
In this way, should the program be executed in the SINGLE BLOCK operating mode, the group of blocks which are found between the mnemonics ESBLK and DSBLK will be executed in a continuous cycle, i.e., execution will not be stopped at the end of a block but will continue by executing the following one.

G01 X10 Y10 F8000 T1 D1 (ESBLK) G02 X20 Y20 I20 J-10 G01 X40 Y20 G01 X40 Y40 F10000 G01 X20 Y40 F8000 (DSBLK) G01 X10 Y10 M30

; Start of single block ; Cancellation of single block

(ESTOP and DSTOP)
After executing the mnemonic DSTOP, the CNC enables the Stop key, as well as the Stop signal from the PLC.
It will remain disabled until it is enabled once again by means of the mnemonic ESTOP.
(EFHOLD and DFHOLD)
After executing the mnemonic DFHOLD, the CNC enables the Feed-Hold input from the PLC.
It will remain disabled until it is enabled once again by means of the mnemonic EFHOLD.

CNC 8040
·M· MODEL (SOFT V11.1X)
334

14.4 Flow control instructions

Programming manual

The GOTO and RPT instructions cannot be used in programs that are executed from a PC connected through the serial lines.
( GOTO N(expresión) )
The mnemonic GOTO causes a jump within the same program, to the block defined by the label N(expression). The execution of the program will continue after the jump, from the indicated block.
The jump label can be addressed by means of a number or by any expression which results in a number.

G00 X0 Y0 Z0 T2 D4 X10 (GOTO N22) X15 Y20 Y22 Z50 N22 G01 X30 Y40 Z40 F1000 G02 X20 Y40 I-5 J-5 ...

; Jump instruction ; It is not executed ; It is not executed ; Continues execution in this block

( RPT N(expression), N(expression), P(expression) )
The mnemonic RPT executes the part of the program between the blocks defined by means of the labels N(expression). The blocks to be executed may be in the execution program or in a RAM memory program.
The label P(expression) indicates the number of the program containing the blocks to be executed. If not defined, the CNC interprets that the portion to be repeated is located in the same program.
All the labels can be indicated by means of a number or by any expression which results in a number. The part of the program selected by means of the two labels must belong to the same program, by first defining the initial block and then the final block.
The execution of the program will continue in the block following the one in which the mnemonic RPT was programmed, once the selected part of the program has been executed.
N10 G00 X10 Z20 G01 X5 G00 Z0
N20 X0 N30 (RPT N10, N20) N3 N40 G01 X20
M30 When reaching block N30, the program will execute section N10-N20 three times. Once this has been completed, the program will continue execution in block N40.

PROGRAM CONTROL INSTRUCTIONS Flow control instructions

14.
CNC 8040

Since the RPT instruction does not interrupt block preparation or tool compensation, it may be used when using the EXEC instruction and while

needing to maintain tool compensation active.

·M· MODEL (SOFT V11.1X)

335

PROGRAM CONTROL INSTRUCTIONS Flow control instructions

Programming manual
14.

(IF condition <action1> ELSE <action2>)
This instruction analyzes the given condition that must be a relational expression. If the condition is true (result equal to 1), <action1> will be executed, otherwise (result equal to 0) <action2> will be executed.
Example: (IF (P8 EQ 12.8) CALL 3 ELSE PCALL 5, A2, B5, D8) If P8 = 12.8 executes the mnemonic (CALL3) If P8<>12.8 executes the mnemonic (PCALL 5, A2, B5, D8)
The instruction can lack the ELSE part, i.e., it will be enough to program IF condition <action1>.
Example: (IF (P8 EQ 12.8) CALL 3)
Both <action1> and <action2> can be expressions or instructions, except for mnemonics IF and SUB.
Due to the fact that in a high level block local parameters can be named by means of letters, expressions of this type can be obtained:
(IF (E EQ 10) M10)
If the condition of parameter P5 (E) having a value of 10 is met, the miscellaneous function M10 will not be executed, since a high level block cannot have ISO code commands. In this case M10 represents the assignment of value 10 to parameter P12, i.e., one can program either:
(IF (E EQ 10) M10) or (IF (P5 EQ 10) P12=10)

CNC 8040
·M· MODEL (SOFT V11.1X)
336

14.5 Subroutine instructions

Programming manual

A subroutine is a part of a program which, being properly identified, can be called from any position of a program to be executed.

A subroutine can be kept in the memory of the CNC as an independent part of a program and be called one or several times, from different positions of a program or different programs.

Only subroutines stored in the CNC's RAM memory can be executed. Therefore, to execute a subroutine stored in the Memkey Card, HD or in a PC connected through the serial lines, it must be copied first into the CNC's RAM memory.
If the subroutine is too large to be copied into RAM, it must be converted into a program and then the EXEC instruction must be used.

(SUB integer)
The SUB instruction defines as subroutine the set of program blocks programmed next until reaching the RET subroutine. The subroutine is identified with an integer which also defines the type of subroutine; either general or OEM.

Range of general subroutines

SUB 0000 - SUB 9999

R a n g e o f O E M ( m a n u f a c t u r e r ' s ) SUB 10000 - SUB 20000 subroutines

The OEM subroutines are treated like the general ones, but with the following restrictions:
· They can only be defined in OEM programs, having the [O] attribute. Otherwise, the CNC will display the corresponding error. Error 63 : Program subroutine number 1 thru 9999.
· To execute an OEM subroutine using CALL, PCALL or MCALL, it must be inside an OEM program. Otherwise, the CNC will display the corresponding error. Error 1255 : Subroutine restricted to an OEM program.
There can not be two subroutines with the same identification number in the CNC memory, even when they belong to different programs.
(RET)
The mnemonic RET indicates that the subroutine which was defined by the mnemonic SUB, finishes in this block.

( SUB 12) G91 G01 XP0 F5000 YP1 X-P0 Y-P1 (RET)

; Definition of subroutine 12 ; End of subroutine

(CALL (expression))
The mnemonic CALL makes a call to the subroutine indicated by means of a number or by means of any expression that results in a number.
As a subroutine may be called from a main program, or a subroutine, from this subroutine to a second one, from the second to a third, etc..., the CNC limits these calls to a maximum of 15 nesting levels, it being possible to repeat each of the levels 9999 times.

PROGRAM CONTROL INSTRUCTIONS Subroutine instructions

14.
CNC 8040
·M· MODEL (SOFT V11.1X)

337

Programming manual

14.

Programming example.

PROGRAM CONTROL INSTRUCTIONS Subroutine instructions

CNC 8040
·M· MODEL (SOFT V11.1X)
338

G90 G00 X30 Y20 Z10 (CALL 10) G90 G00 X60 Y20 Z10 (CALL 10) M30

( SUB 10) G91 G01 X20 F5000 (CALL 11) G91 G01 Y10 (CALL 11) G91 G01 X-20 (CALL 11) G91 G01 Y-10 (CALL 11) (RET)

; Drilling and threading ; Drilling and threading ; Drilling and threading ; Drilling and threading

( SUB 11) G81 G98 G91 Z-8 I-22 F1000 S5000 T1 D1
; Drilling canned cycle

Programming manual

G84 Z-8 I-22 K15 F500 S2000 T2 D2 ; Threading canned cycle
G80 (RET)

(PCALL (expression), (assignment instruction), (assignment instruction),...) )
The mnemonic PCALL calls the subroutine indicated by means of a number or any expression that results in a number. In addition, it allows up to a maximum of 26 local parameters of this subroutine to be initialized.
These local parameters are initialized by means of assignment instructions. Example: (PCALL 52, A3, B5, C4, P10=20)
In this case, in addition to generating a new subroutine nesting level, a new local parameter nesting level will be generated, there being a maximum of 6 levels of local parameter nesting, within the 15 levels of subroutine nesting.
Both the main program and each subroutine that is found on a parameter nesting level, will have 26 local parameters (P0-P25).
Programming example.

14.

PROGRAM CONTROL INSTRUCTIONS Subroutine instructions

G90 G00 X30 Y50 Z0

(PCALL 10, P0=20, P1=10)

; Also (PCALL 10, A20, B10)

G90 G00 X60 Y50 Z0

(PCALL 10, P0=10, P1=20)

; Also (PCALL 10, A10, B20)

M30

( SUB 10)

G91 G01 XP0 F5000

(CALL 11)

G91 G01 YP1

(CALL 11)

G91 G01 X-P0

(CALL 11)

G91 G01 Y-P1

(CALL 11)

(RET)

( SUB 11)

G81 G98 G91 Z-8 I-22 F1000 S5000 T1 D1

; Drilling canned cycle

CNC 8040
·M· MODEL (SOFT V11.1X)
339

PROGRAM CONTROL INSTRUCTIONS Subroutine instructions

Programming manual
14.

G84 Z-8 I-22 K15 F500 S2000 T2 D2 ; Threading canned cycle
G80 (RET)
(MCALL (expression), (assignment instruction), (assignment instruction),...) )
By means of the mnemonic MCALL, any user-defined subroutine (SUB integer) acquires the category of canned cycle.
The execution of this mnemonic is the same as the mnemonic PCALL, but the call is modal, i.e., if another block with axis movement is programmed at the end of this block, after this movement, the subroutine indicated will be executed and with the same call parameters.
If, when a modal subroutine is selected, a movement block with a number of repetitions is executed, for example X10 N3, the CNC will execute the movement only once (X10) and after the modal subroutine, as many times as the number of repetitions indicates.
Should block repetitions be chosen, the first execution of the modal subroutine will be made with updated call parameters, but not for the remaining times, which will be executed with the values which these parameters have at that time.
If, when a subroutine is selected as modal, a block containing the MCALL mnemonic is executed, the present subroutine will lose its modal quality and the new subroutine selected will be changed to modal.
(MDOFF)
The MDOFF instruction indicates that the mode assumed by a subroutine with the MCALL instruction or a part-program with MEXEC ends in that block.
The use of modal subroutines simplifies programming.
Programming example.

CNC 8040
·M· MODEL (SOFT V11.1X)
340

G90 G00 X30 Y50 Z0 (PCALL 10, P0=20, P1=10) G90 G00 X60 Y50 Z0 (PCALL 10, P0=10, P1=20) M30
( SUB 10) G91 G01 XP0 F5000 (MCALL 11)

G91 G01 YP1 G91 G01 X-P0 G91 G01 Y-P1 (MDOFF) (RET) ( SUB 11) G81 G98 G91 Z-8 I-22 F1000 S5000 T1 D1 G84 Z-8 I-22 K15 F500 S2000 T2 D2 G80 (RET)

Programming manual
14.

PROGRAM CONTROL INSTRUCTIONS Subroutine instructions

CNC 8040
·M· MODEL (SOFT V11.1X)
341

Programming manual
14.6 Probe related instructions

14.

(PROBE (expression), (assignment instruction), (assignment instruction),...) )
The mnemonic PROBE calls the probe cycle indicated by means of a number or any expression that results in a number. In addition, it allows the local parameters of this subroutine to be initialized by means of assignment instructions.
This instruction also generates a new subroutine nesting level.

PROGRAM CONTROL INSTRUCTIONS Probe related instructions

CNC 8040
·M· MODEL (SOFT V11.1X)
342

14.7 Interruption-subroutine instructions

Programming manual

Whenever one of the general interruption logic input is activated, "INT1" (M5024), "INT2" (M5025), "INT3" (M5026) or "INT4 (M5027), the CNC temporarily interrupts the execution of the program in progress and starts executing the interruption subroutine whose number is indicated by the corresponding general parameter.
With INT1 (M5024) the one indicated by machine parameter INT1SUB (P35) With INT2 (M5025) the one indicated by machine parameter INT2SUB (P36) With INT3 (M5026) the one indicated by machine parameter INT3SUB (P37) With INT4 (M5027) the one indicated by machine parameter INT4SUB (P38)
The interruption subroutines are defined like any other subroutine by using the instructions: "(SUB integer)" and "(RET)".
These interruption subroutines do not change the nesting level of local parameters, thus only global parameters must be used in them.
Within an interruption subroutine, it is possible to use the "(REPOS X, Y, Z, ...)" instruction described next.
Once the execution of the subroutine is over, the CNC resumes the execution of the program which was interrupted.
( REPOS X, Y, Z, ... )
The REPOS instruction must always be used inside an interruption subroutine and facilitates the repositioning of the machine axes to the point of interruption.
When executing this instruction, the CNC moves the axes to the point where the program was interrupted.
Inside the REPOS instruction, indicate the order the axes must move to the point where the program was interrupted.
· The axes move one by one. · It is not necessary to define all the axes, only those to be repositioned. · The axes that make up the main plane of the machine move together.
Both axes need not be defined because the CNC moves the first one. The movement is not repeated when defining the second one, it is ignored.
Example: The main plane is formed by the X and Y axes, the Z axis is the longitudinal (perpendicular) axis and the machine uses the C and W axes as auxiliary axes. It is desired to first move the C axis, then the X and Y axes and finally the Z axis. This repositioning move may be defined in any of the following ways: (REPOS C, X, Y, Z)(REPOS C, X, Z)(REPOS C, Y, Z)
If the REPOS instruction is detected while executing a subroutine not activated by an interruption input, the CNC will issue the corresponding error message.

PROGRAM CONTROL INSTRUCTIONS Interruption-subroutine instructions

14.

CNC 8040

·M· MODEL (SOFT V11.1X)

343

Programming manual
14.8 Program instructions

14.
CNC 8040
·M· MODEL (SOFT V11.1X)

PROGRAM CONTROL INSTRUCTIONS Program instructions

With this CNC, from a program in execution, it is possible to: · Execute another program. Instruction (EXEC P.....) · Execute another program in modal mode. Instruction (MEXEC P.....) · Generate a new program. Instruction (OPEN P.....) · Add blocks to an existing program. Instruction (WRITE P.....)

( EXEC P(expression), (directory) ) The EXEC P instruction executes the part-program of the indicated directory

The part-program may be defined by a number or any expression resulting in a number.

By default, the CNC interprets that the part-program is in the CNC's RAM memory. If it is in another device, it must be indicated in (directory).

CARD A in the "Memkey CARD".

in the Hard Disk.

DNC1

in a PC connected through serial line 1.

DNC2

in a PC connected through serial line 2.

DNCE

in a PC connected through Ethernet.

(MEXEC P(expression), (directory))
The MEXEC instruction executes the part-program of the indicated directory and it also becomes modal; i.e. if after this block, another one is programmed with axis movement; after this movement, it will execute the indicated program again.

The part-program may be defined with a number or with an expression whose result is a number.

By default, the CNC interprets that the part-program is in the CNC's RAM memory. If it is in another device, it must be so indicated in (directory):

CARD A in the "Memkey CARD".

in the Hard Disk.

DNC1

in a PC connected through serial line 1.

DNC2

in a PC connected through serial line 2.

DNCE

in a PC connected through Ethernet.

If while the modal part-program is selected, a motion block is executed with a number of repetitions (for example X10 N3), the CNC ignores the number of repetitions and executes the movement and the modal part-program only once.

If while a part-program is selected as modal, a block containing the MEXEC instruction is executed from the main program, the current part-program stops being modal and the part-program called upon with MEXEC will then become modal.
If within the modal part-program, an attempt is made to execute a block using the MEXEC instruction, it will issue the relevant error message.
1064: The program cannot be executed.

(MDOFF)
The MDOFF instruction indicates that the mode assumed by a subroutine with the MCALL instruction or a part-program with MEXEC ends in that block.

344

Programming manual

(OPEN P(expression), (destination directory), A/D, "program comment")
The OPEN instruction begins editing a part-program. The part-program number may be indicated by a number or any expression resulting in a number.

By default, the new part-program edited will be stored in the CNC's RAM memory. To store it another device, it must be indicated in (destination directory).

CARD A in the "Memkey CARD".

in the Hard Disk.

DNC1

in a PC connected through serial line 1.

DNC2

in a PC connected through serial line 2.

DNCE

in a PC connected through Ethernet.

14.

PROGRAM CONTROL INSTRUCTIONS Program instructions

Parameter A/D is used when the program to be edited already exists.

The CNC appends the new blocks after the ones already existing.

The CNC deletes the existing program and starts editing a new

one.

A program comment may also be associated with it. This comment will later be displayed next to it on the program directory.

The OPEN instruction allows generating a program from a program already in execution. That generated program will depend on the values assumed by the program being executed.

To edit blocks, the WRITE instruction must be used as described next.

Notes:
If the program to be edited already exists and the A/D parameters are not defined, the CNC will display an error message when executing the block.
The program opened with the OPEN instruction is closed when executing an M30, or another OPEN instruction and after an Emergency or Reset.
From a PC, only programs stored in the CNC'S RAM memory, in the CARD A, or in the Hard Disk module can be opened

(WRITE <block text> )
The mnemonic WRITE adds, after the last block of the program which began to be edited by means of the mnemonic OPEN P, the information contained in <block text> as a new program block.
When it is an ISO coded parametric block, all the parameters (global and local) are replaced by the numeric value they have at the time.
(WRITE G1 XP100 YP101 F100) => G1 X10 Y20 F100
When it is a parametric block edited in high level, use the "?" character to indicate that the parameter is supposed to be replaced by the numeric value it has at the time.

(WRITE (SUB P102)) (WRITE (SUB ?P102))

=> (SUB P102) => ( SUB 55)

(WRITE (ORGX54=P103)) (WRITE (ORGX54=?P103))

=> (ORGX54=P103) => (ORGX54=222)

(WRITE (PCALL P104)) (WRITE (PCALL ?P104))

=> (PCALL P104) => (PCALL 25)

CNC 8040
·M· MODEL (SOFT V11.1X)

345

Programming manual
14.

If the mnemonic WRITE is programmed without having programmed the mnemonic OPEN previously, the CNC will display the corresponding error, except when editing a user customized program, in which case a new block is added to the program being edited. Example of the creation of a program which contains several points of a cardioid:
| R = B cos (Q/2) |

PROGRAM CONTROL INSTRUCTIONS Program instructions

Subroutine number 2 is used, its parameters having the following meaning:

A or P0

Value of angle Q.

B or P1

Value of B.

C or P2

Angular increment for calculation.

D or P3

The maximum feedrate of the axes.

A way to use this example could be: G00 X0 Y0 G93 (PCALL 2, A0, B30, C5, D500) M30

CNC 8040
·M· MODEL (SOFT V11.1X)
346

Program generating subroutine.

Programming manual

N100

( SUB 2)

(OPEN P12345)

; Starts editing of program P12345

(WRITE FP3)

; Selects machining feedrate

(P10=P1 * (ABS(COS(P0/2))))

; Calculates R

(WRITE G01 G05 RP10 QP0)

; Movement block

(P0=P0+P2)

; New angle

(IF (P0 LT 365) GOTO N100)

; If angle smaller than 365º, calculates new point

(WRITE M30)

; End of program block

(RET)

; End of subroutine

14.

PROGRAM CONTROL INSTRUCTIONS Program instructions

CNC 8040
·M· MODEL (SOFT V11.1X)
347

Programming manual
14.9 Screen customizing instructions

14.

Customizing instructions may be used only when customizing programs made by the user.
These customizing programs must be stored in the CNC'S RAM memory and they may utilize the "Programming Instructions" and they will be executed in the special channel designed for this use; the program selected in each case will be indicated in the following general machine parameters.
In "USERDPLY" the program to be executed in the Execution Mode will be indicated.
In "USEREDIT" the program to be executed in the Editing Mode will be indicated.
In "USERMAN" the program to be executed in the Manual (JOG) Mode will be indicated.
In "USERDIAG" the program to be executed in the Diagnosis Mode will be indicated.
The customizing programs may have up to five nesting levels besides their current one. Also, the customizing instructions do not allow local parameters, nevertheless all global parameters may be used to define them.

PROGRAM CONTROL INSTRUCTIONS Screen customizing instructions

( PAGE (expression) )
The mnemonic PAGE displays the page number indicated by means of a number or by means of any expression resulting in a number.
User-defined pages will be from page 0 to page 255 and will be defined from the CNC keyboard in the Graphic Editor mode and as indicated in the Operating Manual.
System pages will be defined by a number greater than 1000. See the corresponding appendix.

( SYMBOL (expression 1), (expression 2), (expression 3) )
The mnemonic SYMBOL displays the symbol whose number is indicated by means of the value of expression 1 once this has been evaluated.
Its position on screen is also defined by expression 2 (column) and by expression 3 (row).
Expression 1, expression 2 and expression 3 may contain a number or any expression resulting in a number.
The CNC allows displaying any user-defined symbol (0-255) defined at the CNC keyboard in the Graphic Editor mode such as is indicated in the Operating Manual.
In order to position it within the display area its pixels must be defined, 0-639 for columns (expression 2) and 0-335 for rows (expression 3).

CNC 8040

·M· MODEL (SOFT V11.1X)

348

Programming manual

(IB (expression) = INPUT "text", format)
The CNC has 26 data entry variables (IBO-1B25)
The IB mnemonic displays the text indicated in the data input window and stores the data input by the user in the entry variable indicated by means of a number or by means of any expression resulting in a number.

The wait for data entry will only occur when programming the format of the requested data. This format may have a sign, integer part and decimal part.
If it bears the "-" sign, it will allow positive and negative values, and if it does not have a sign, it will only allow positive values.
The integer part indicates the maximum number of digits (0-6) desired to the left of the decimal point.
The decimal part indicates the maximum number of digits (0-5) desired to the right of the decimal point.

14.

If the numerical format is not programmed; for example: (IB1 =INPUT "text"), the mnemonic will only display the indicated text without waiting for the data to be entered.

PROGRAM CONTROL INSTRUCTIONS Screen customizing instructions

( ODW (expression 1), (expression 2), (expression 3) )
The mnemonic ODW defines and draws a white window on the screen with fixed dimensions (1 row and 14 columns).
Each mnemonic has an associated number which is indicated by the value of expression 1 once this has been evaluated.
Likewise, its position on screen is defined by expression 2 (row) and by expression 3 (column).
Expression 1, expression 2 and expression 3 may contain a number or any expression resulting in a number.
The CNC allows 26 windows (0-25) to be defined and their positioning within the display area, providing 21 rows (0-20) and 80 columns (0-79).

( DW(expression 1) = (expression 2), DW (expression 3) = (expression 4), ... )
The instruction DW displays in the window indicated by the value for expression 1, expression 3, .. once they have been evaluated, the numerical data indicated by expression 2, expression 4, ...
Expression 1, expression 2, expression 3, .... may contain a number or any expression which may result in a number.
The following example shows a dynamic variable display: (ODW 1, 6, 33) ; Defines data window 1 (ODW 2, 14, 33) ; Defines data window 2
N10 (DW1=DATE, DW2=TIME) ; Displays the date in window 1 and the time in 2
(GOTO N10)

CNC 8040

·M· MODEL (SOFT V11.1X)

349

Programming manual
14.

The CNC allows displaying the data in decimal, hexadecimal and binary format; the following instructions are available:
(DW1 = 100) Decimal format. Value "100" displayed in window 1.
(DWH2 = 100) Hexadecimal format. Value "64" displayed in window 2.
(DWB3 = 100) Binary format. Value "01100100" displayed in window 3.
When using the binary format, the display is limited to 8 digits in such a way that a value of "11111111" will be displayed for values greater than 255 and the value of "10000000" for values more negative than -127.
Besides, the CNC allows the number stored in one of the 26 data input variables (IB0-IB25) to be displayed in the requested window.
The following example shows a request and later displays the axis feedrate:
(ODW 3, 4, 60) ; Defines data window 3.
(IB1=INPUT "Axis feed: ", 5.4) ; Axis feedrate request.
(DW3=IB1) ; Displays feedrate in window 3.

PROGRAM CONTROL INSTRUCTIONS Screen customizing instructions

CNC 8040
·M· MODEL (SOFT V11.1X)
350

(SK (expression 1) = "text1" (expression 2) = "text 2", .... )

The instruction SK defines and displays the new softkey menu indicated.

Each of the expressions will indicate the softkey number which it is required to modify (1-7, starting from the left) and the texts which it is required to write in them.

Expression 1, expression 2, expression 3, .... may contain a number or any expression which may result in a number.

Each text will allow a maximum of 20 characters that will be shown in two lines of 10 characters each. If the text selected has less than 10 characters, the CNC will center it on the top line, but if it has more than 10 characters the programmer will center it.

Examples: (SK 1="HELP", SK 2="MAXIMUN POINT")

HELP

MAXIMUN POINT

(SK 1="FEED", SK 2=" _ _MAXIMUN_ _ _POINT")

FEED

MAXIMUN POINT

If while a standard CNC softkey menu is active, one or more softkeys are selected via high level language instruction: "SK", the CNC will clear all existing softkeys and it will only show the selected ones. If while a user softkey menu is active, one or more softkeys are selected via high level language instruction "SK", the CNC will only replace the selected softkeys leaving the others intact.
( WKEY )
The mnemonic WKEY stops execution of the program until the key is pressed.

PROGRAM CONTROL INSTRUCTIONS Screen customizing instructions

The pressed key will be recorded in the KEY variable.

Programming manual

... ( WKEY ) (IF KEY EQ $FC00 GOTO N1000)
...

; Wait for key
; If key F1 has been pressed, continue in N1000

( WBUF "text", (expression) )

The WBUF instruction can only be used when editing a program in the user channel.

This instruction may be programmed in two ways:

· ( WBUF "text", (expression) ) It adds the text and value of the expression, once it has been evaluated, to the block that is being edited and within the data input window. (Expression) may contain a number or any expression resulting in a number. It will be optional to program the expression, but it will be required to define the text. If no text is required, "" must be programmed. Examples for P100=10:

(WBUF "X", P100) (WBUF "X P100")

=> X10 => X P100

14.

· ( WBUF ) Enters into memory, adding to the program being edited and after the cursor position, the block being edited by means of (WBUF "text", (expression)). It also clears the editing buffer in order to edit a new block. This allows the user to edit a complete program without having to quit the user editing mode after each block and press ENTER to "enter" it into memory.
(WBUF "(PCALL 25, ") ; Adds "(PCALL 25, " to the block being edited.
(IB1=INPUT "Parameter A:",-5.4) ; Request of Parameter A.
(WBUF "A=", IB1) ; Adds "A=(value entered)" to the block being edited.
(IB2=INPUT "Parameter B: ", -5.4) ; Request of Parameter B.
(WBUF ", B=", IB2) ; Adds "B=(value entered)" to the block being edited.
(WBUF ")") ; Adds ")" to the block being edited.
( WBUF ) ; Enters the edited block into memory.
...
After executing this program the block being edited contains: (PCALL 25, A=23.5, B=-2.25)
( SYSTEM ) The mnemonic SYSTEM stops execution of the user customized program and returns to the corresponding standard menu of the CNC.

CNC 8040
·M· MODEL (SOFT V11.1X)

351

Programming manual

Customizing program example:

The following customizing program must be selected as user program associated to the Editing Mode.
After selecting the Editing Mode and pressing the USER softkey, this program starts executing and it allows assisted editing of 2 user cycles. This editing process is carried out a cycle at a time and as often as desired.

14.

Displays the initial editing page (screen) N0 ( PAGE 10 )

PROGRAM CONTROL INSTRUCTIONS Screen customizing instructions

Sets the softkeys to access the various modes and requests a choice

(SK 1="CYCLE 1",SK 2="CYCLE 2",SK 7="EXIT")

N5 ( WKEY )

; Request a key

(IF KEY EQ $FC00 GOTO N10)

; Cycle 1

(IF KEY EQ $FC01 GOTO N20)

; Cycle 2

(IF KEY EQ $FC06 SYSTEM ELSE GOTO N5) ; Quit or request a key

CYCLE 1 ; Displays page 11 and defines 2 data entry windows N10 ( PAGE 11 )
(ODW 1,10,60) (ODW 2.15,60)

;Editing (WBUF "(PCALL 1, ")

; Adds "(PCALL 1," to the block being edited.

(IB 1=INPUT "X:",-6.5) (DW 1=IB1) (WBUF "X",IB1)

; Requests the value of X. ; Data window 1 shows the entered value. ; Adds X (entered value) to the block being edited.

(WBUF ",")

; Adds "," to the block being edited.

(IB 2=INPUT "Y:",-6.5) (DW 2=IB2) (WBUF "Y",IB2)

; Requests the value of Y. ; Data window 2 shows the entered value. ; Adds Y (entered value) to the block being edited.

CNC 8040

(WBUF ")") ( WBUF )
(GOTO N0)

; Adds ")" to the block being edited.
; Enters the edited block into memory. ; For example : (PCALL 1, X2, Y3)

·M· MODEL (SOFT V11.1X)

352

CYCLE 2 ; Displays page 12 and defines 3 data entry windows N20 ( PAGE 12 )
(ODW 1,10,60) (ODW 2.13,60) (ODW 3.16,60)

;Editing (WBUF "(PCALL 2, ")

; Adds "(PCALL 2, " to the block being edited.

Programming manual
14.

PROGRAM CONTROL INSTRUCTIONS Screen customizing instructions

(IB 1=INPUT "A:",-6.5) (DW 1=IB1) (WBUF "A",IB1)

; Requests the value of A. ; Data window 1 shows the entered value. ; Adds A (entered value) to the block being edited.

(WBUF ",")

; Adds "," to the block being edited.

(IB 2=INPUT "B:",-6.5) (DW 2=IB2) (WBUF "B",IB2)

; Requests the value of B. ; Data window 2 shows the entered value. ; Adds B (entered value) to the block being edited.

(WBUF ",") (IB 3=INPUT "C:",-6.5) (DW 3=IB3) (WBUF "C",IB3)

; Adds "," to the block being edited. ; Requests the value of C. ; Data window 3 shows the entered value. ; Adds C (entered value) to the block being edited.

(WBUF ")")

; Adds ")" to the block being edited.

( WBUF ) (GOTO N0)

; Enters the edited block into memory. For example: (PCALL 2, A3, B1, C3).

CNC 8040
·M· MODEL (SOFT V11.1X)
353

Programming manual
14.
CNC 8040
·M· MODEL (SOFT V11.1X)
354

PROGRAM CONTROL INSTRUCTIONS Screen customizing instructions

15 ANGULAR TRANSFORMATION
OF AN INCLINE AXIS
Using the angular transformation of the incline axis it is possible to carry out movements along an axis that is not perpendicular to another. The movements are programmed in the Cartesian system and to make the movements, they are transformed into movements on the real axes. On certain machines, the axes are not configured as Cartesian, they form angles other than 90º between them, instead. A typical case is the X axis of a lathe that, for sturdiness, it is not at 90º of the Z axis, but at another angle.
X X' X Cartesian axis. X' Angular axis. Z orthogonal axis.
Z

In order to program it in the Cartesian system (Z-X), activate the incline axis angular transformation to convert the movements to the non-perpendicular real axes (Z-X'). This way, a movement programmed on the X axis is transformed into movements on the Z-X0 axes; in other words, it moves along the Z axis and along the angular X' axis.
Turning angular transformation on and off.
The CNC assumes no transformation on power-up; the angular transformations are activated via part-program using the instruction G46.
The angular transformations are turned off via part-program using function G46. Optionally, a transformation may be "frozen" (suspended) to move angular axis by programming in Cartesian coordinates.
Influence of RESET, of powering off and of function M30.
The angular transformation of an incline axis stays active after a RESET, M30 and even after turning the CNC off and back on.

CNC 8040

·M· MODEL (SOFT V11.1X)

355

ANGULAR TRANSFORMATION OF AN INCLINE AXIS

Programming manual
15.

Considerations for the angular transformation of an incline axis.
The axes involved in an angular transformation must be linear. Both axes may have Gantry axes associated with them, the may be slaved (coupled) or synchronized by PLC.
If the angular transformation is active, the coordinates displayed will be those of the Cartesian system. Otherwise, the coordinates of the real axes will be displayed.
The following operations are possible while the transformation is active: · Zero offsets. · Coordinate preset. · Movements in continuous / incremental jog and handwheels.
The following operations are not possible while the transformation is active: · Movement until making contact (against a hard stop). · Coordinate rotation. · Surface feedrate in milling.
Home search
Function G46 is canceled when homing an axis that is involved in the angular transformation (machine parameters ANGAXNA and ORTAXNA). When homing the axes that are not involved in the angular axis transformation, function G46 stays active.
While searching home, only the real axes move.
Jogging and handwheel movements.
Either the real or the Cartesian axes may be jogged depending on how they've been set by the manufacturer. It is selected via PLC (MACHMOVE) and it may be available, for example, from a user key.

CNC 8040
·M· MODEL (SOFT V11.1X)
356

15.1 Turning angular transformation on and off

Programming manual

Turn angular transformation on
When the transformation is on, the movements are programmed in the Cartesian system and to make the movements, the CNC transforms them into movements on the real axes. The coordinates displayed on the screen will be those of the Cartesian system.
The angular transformation is turned on using function G46 whose programming format is:
G46 S1
This instruction turns a "frozen" (suspended) transformation on again. See "15.2 Freezing the angular transformation" on page 358.
Turning the angular transformation off
If the transformation is off, the movements are programmed and executed in the system of the real axes. The coordinates displayed on the screen will be those of the real axes.
The angular transformation is turned off using function G46 whose programming format is:
G46 S0 G46
The angular transformation of an incline axis stays active after a RESET, M30 and even after turning the CNC off and back on.

ANGULAR TRANSFORMATION OF AN INCLINE AXIS Turning angular transformation on and off

15.

CNC 8040
·M· MODEL (SOFT V11.1X)
357

Programming manual
15.2 Freezing the angular transformation

15.

Freezing the angular transformation is a special way to make movements along the angular axis, but programming it in the Cartesian system. The angular transformation cannot be "frozen" (suspended) while jogging.
The angular transformation is "frozen" (suspended) using function G46 whose programming format is:
G46 S2
Programming movements after "freezing" the angular transformation.
If an angular transformation is "frozen" (suspended), only the coordinate of the angular axis must be programmed in the motion block. If the coordinate of the orthogonal axis is programmed, the movement is carried out according to the normal angular transformation.
Canceling the freezing of a transformation.
The "freezing" of an angular transformation is canceled after a reset or an M30. Turning the transformation on (G46 S1) also cancels the "freezing".

ANGULAR TRANSFORMATION OF AN INCLINE AXIS Freezing the angular transformation

CNC 8040
·M· MODEL (SOFT V11.1X)
358

APPENDIX

Programming manual

A. ISO code programming ...................................................361 B. Program control instructions..........................................363 C. Summary of internal CNC variables. .............................367 D. Key codes .........................................................................373 E. Programming assistance screens of the system..........381 F. Maintenance .....................................................................385

CNC 8040
·M· MODEL (SOFT V11.1X)
359

ISO CODE PROGRAMMING

Programming manual

Function M D V

Meaning

G00

* ? * Rapid traverse

G01

* ? * Linear interpolation

G02

* Clockwise circular (helical) interpolation

G03

* Counterclockwise circular (helical) interpolation

G04

Dwell/interruption of block preparation

G05

* ? * Round corner

G06

* Arc center in absolute coordinates

G07

Square corner

G08

* Arc tangent to previous path.

G09

* Arc defined by three points

G10

Mirror image cancellation

G11

* Mirror image on X axis

G12

* Mirror image on Y axis

G13

* Mirror image on Z axis

G14

* Mirror image in the programmed directions

G15

* Longitudinal axis selection

G16

* Main plane selection by two addresses and longitudinal axis

G17

* ? * Main plane X-Y and longitudinal Z

G18

* ? * Main plane Z-X and longitudinal Y

G19

* Main plane Y-Z and longitudinal X

G20

Definition of lower work zone limits

G21

Definition of upper work zone limits.

G22

* Enable/disable work zones.

G28

* Second spindle selection

G29

Main spindle selection

G28 - G29

* Axis toggle

G30

* Spindle synchronization (offset)

G32

* Feedrate "F" as an inverted function of time.

G33

* Electronic threading

G34

Variable-pitch threading

G36

* Controlled corner rounding

G37

* Tangential entry

G38

* Tangential exit

G39

* Chamfer

G40

Cancellation of tool radius compensation

G41

* Left-hand tool radius compensation

G41 N *

* Collision detection

G42

* Right-hand tool radius compensation

G42 N *

* Collision detection

G43

* ? * Tool length compensation

G44

Cancellation of tool length compensation

G45

* Tangential control (G45)

G50

* Controlled corner rounding

G51

* Look-Ahead

G52

* Movement until making contact

G53

* Programming with respect to machine reference zero (home)

G54

* Absolute zero offset 1

G55

* Absolute zero offset 2

G56

* Absolute zero offset 3

G57

* Absolute zero offset 4

G58

* Additive zero offset 1

G59

* Additive zero offset 2

G60

* Multiple machining in a straight line

G61

* Multiple machining in a rectangular pattern

G62

* Grid pattern canned cycle

G63

* Multiple machining in a circular pattern

APPENDIX ISO code programming

A.
CNC 8040
·M· MODEL (SOFT V11.1X)
361

Programming manual

A.
CNC 8040

APPENDIX ISO code programming

Function M D V

Meaning

Section

G64 G65 G66 G67 G68 G69 G70 G71 G72 G73 G74 G75 G76 G77 G77S G78 G78S G79 G80 G81 G82 G83 G84 G85 G86 G87 G88 G89 G90 G91 G92 G93 G94 G95 G96 G97 G98 G99
G145

* Multiple machining in an arc

10.5

* Machining programmed with an arc-chord

10.6

* Irregular pocket canned cycle

11.1 / 11.2

* Irregular pocket roughing

11.1.2

* Irregular pocket finishing

11.1.3

* Drilling canned cycle with variable peck

9.6

* ? * Inch programming

3.3

Programming in millimeters

3.3

* General and specific scaling factor

7.6

* Pattern rotation

7.7

* Home search

4.2

* Probing move until touching

12.1

* Probing move while touching

12.1

* Axis coupling (slaving)

7.8.1

* Spindle synchronization

5.5

Cancellation of axis coupling (slaving)

7.8.2

Cancellation of spindle synchronization

5.5

Canned cycle parameter modification

9.2.1

Canned cycle cancellation

9.3

* Drilling canned cycle

9.7

* Drilling canned cycle with dwell

9.8

* Deep-hole drilling canned cycle with constant peck

9.9

* Tapping canned cycle

9.10

* Reaming canned cycle

9.11

* Boring canned cycle with withdrawal in G00

9.12

* Rectangular pocket canned cycle.

9.13

* Circular pocket canned cycle

9.14

* Boring canned cycle with withdrawal in G01

9.15

Absolute programming

3.4

* ? * Incremental programming

3.4

Coordinate preset / spindle speed limit

4.4.1

Polar origin preset

4.5

Feedrate in millimeters (inches) per minute

5.2.1

* ? * Feedrate in millimeters (inches) per revolution.

5.2.2

* Constant cutting point speed

5.2.3

Constant tool center speed

5.2.4

Withdrawal to the starting plane at the end of the canned cycle

9.5

* Withdrawal to the reference plane at the end of the canned

9.5

cycle

* Temporary cancellation of tangential control

6.17

D means BY DEFAULT, i.e. they will be assumed by the CNC when it is powered on, after executing M02, M30 or after EMERGENCY or RESET.

In those cases indicated by ? , it should be understood that the DEFAULT of these G functions depends on the setting of the general machine parameters of the CNC.

V means that the G code is displayed next to the current machining conditions in the execution and simulation modes.

·M· MODEL (SOFT V11.1X)

362

PROGRAM CONTROL INSTRUCTIONS

Programming manual

Display instructions.
(ERROR integer, "error text") Stops the execution of the program and displays the indicated error.
(MSG "message") Displays the indicated message.
(DGWZ expression 1, ..... expression 6) Define the graphics area.

( section 14.2 )

Enabling and disabling instructions.
( section 14.3 ) (ESBLK and DSBLK)
The CNC executes all the blocks between ESBLK and DSBLK as if it were a single block. (ESTOP and DSTOP)
Enabling (ESTOP) and disabling (DSTOP) of the Stop key and the external Stop signal (PLC). (EFHOLD and DFHOLD)
Enabling (EFHOLD) and disabling (DFHOLD) of the Feed-hold input (PLC).

Flow control instructions.
( section 14.4 )
( GOTO N(expresión) ) It causes a jump within the same program, to the block defined by the label N(expression).
( RPT N(expression), N(expression), P(expression) ) It repeats the execution of the portion of the program between the blocks defined by means of the labels N(expression).
(IF condition <action1> ELSE <action2>) It analyzes the given condition that must be a relational expression. If the condition is true (result equal to 1), <action1> will be executed, otherwise (result equal to 0) <action2> will be executed.

Subroutine instructions.
( section 14.5 )
(SUB integer) Subroutine definition.
(RET) End of subroutine.
(CALL (expression)) Call to a subroutine.
(PCALL (expression), (assignment instruction), (assignment instruction),...) ) Call to a subroutine. In addition, using assignment instructions, it is possible to initialize up to a maximum of 26 local parameters of this subroutine.
(MCALL (expression), (assignment instruction), (assignment instruction),...) ) Same as the PCALL instruction, but making the indicated subroutine modal
(MDOFF) Cancellation of modal subroutine.

APPENDIX Program control instructions

B.
CNC 8040
·M· MODEL (SOFT V11.1X)

363

Programming manual
Probe related instructions. ( section 14.6 )
(PROBE (expression), (assignment instruction), (assignment instruction),...) ) It executes a probing canned cycle initializing its parameters by means of assignment instructions.

Interruption-subroutine instructions.
( section 14.7 ) ( REPOS X, Y, Z, .... )
It must always be used inside an interruption subroutine and facilitates the repositioning of the machine axes to the point of interruption.

APPENDIX Program control instructions

Program instructions.
( section 14.8 )
( EXEC P(expression), (directory) ) Starts program execution..
(MEXEC P(expression), (directory)) Starts program execution in modal mode.
(OPEN P(expression), (destination directory), A/D, "program comment") It begins editing a new program being possible to associate a comment with the program.
(WRITE <block text> ) It adds, after the last block of the program which began to be edited by means of the mnemonic OPEN P, the information contained in <block text> as a new program block.

CNC 8040

Screen customizing instructions.
( section 14.9 )
( PAGE (expression) ) The screen displays the indicated user page number (0-255) or system page (1000).
( SYMBOL (expression 1), (expression 2), (expression 3) ) The screen displays the symbol (0-255) indicated by the expression 1. Its position on the screen is defined by expression 2 (row, 0-639) and by expression 3 (column 0-335).
(IB (expression) = INPUT "text", format) It displays the text indicated in the data input window and stores in the input variable (IBn) the data entered by the user.
( ODW (expression 1), (expression 2), (expression 3) ) It defines and draws a white window on the screen (1 row and 14 columns). Its position on screen is defined by expression 2 (row) and by expression 3 (column).
( DW(expression 1) = (expression 2), DW (expression 3) = (expression 4), ... ) It displays in the windows indicated by the value of the expression 1, 3,.. , the numerical data indicated by the expression 2,4,..
(SK (expression 1) = "text1" (expression 2) = "text 2", .... ) It defines and displays the new softkey menu indicated.
( WKEY ) It stops the execution of the program until a key is pressed.
( WBUF "text", (expression) ) It adds the text and value of the expression, once it has been evaluated, to the block that is being edited and within the data input window.

·M· MODEL (SOFT V11.1X)

364

Programming manual

( section 14.9 )
( WBUF ) Enters the block being edited into memory. It can only be used in the screen customizing program to be executed in the Editing mode.
( SYSTEM ) It ends the execution of the user screen customizing program and returns to the corresponding standard menu of the CNC.

APPENDIX Program control instructions

CNC 8040
·M· MODEL (SOFT V11.1X)
365

APPENDIX Program control instructions

Programming manual
B.
CNC 8040
·M· MODEL (SOFT V11.1X)
366

SUMMARY OF INTERNAL CNC VARIABLES.

Programming manual

Variable
TOOL TOD NXTOOL NXTOD TMZPn TLFDn TLFFn TLFNn TLFRn TMZTn TORn TOLn TOIn TOKn
Variable
ORG(X-C)
PORGF PORGS ORG(X-C)n PLCOF(X-C) ADIOF(X-C)
Variable
MPGn MP(X-C)n MPSn MPSSn MPASn MPLCn
Variable
FZONE FZLO(X-C) FZUP(X-C) SZONE SZLO(X-C) SZUP(X-C) TZONE TZLO(X-C) TZUP(X-C) FOZONE FOZLO(X-C) FOZUP(X-C) FIZONE FIZLO(X-C): FIZUP(X-C)

· The R symbol indicates that the variable can be read. · The W symbol indicates that the variable can be modified.

Variables associated with tools.

CNC PLC DNC

( section 13.2.2 )

R R R Number of active tool.

R R R Number of active tool offset.

R R R Number of the next requested tool waiting for M06.

R R R Number of the next tool's offset.

- (n) tool's position in the tool magazine.

R/W R/W - (n) tool's offset number.

R/W R/W - (n) tool's family code.

R/W R/W - Nominal life assigned to tool (n).

R/W R/W - Real life value of tool (n).

R/W R/W - Contents of tool magazine position (n).

R/W R/W - Tool radius value of offset (n)

R/W R/W - Tool length value of offset (n)

R/W R/W - Tool radius wear of offset (n).

R/W R/W - Tool length wear of offset (n).

Variables associated with zero offsets..

CNC PLC DNC

( section 13.2.3 )

- Active zero offset on the selected axis. The value of the additive offset

indicated by the PLC is not included in this value.

R Abscissa coordinate value of polar origin.

R Ordinate coordinate value of polar origin.

R/W R/W R Zero offset (n) value of the selected axis.

R/W R/W R Value of the additive Zero Offset activated via PLC.

R R R Value for the selected axis of the zero offset with additive handwheel.

Variables associated with machine parameters.

CNC PLC DNC

( section 13.2.4 )

- Value assigned to general machine parameter (n).

- Value assigned to axis machine parameter (n) (X-C)

- Value assigned to machine parameter (n) of the main spindle.

- Value assigned to machine parameter (n) of the second spindle.

- Value assigned to machine parameter (n) of the auxiliary spindle.

- Value assigned to machine parameter (n) of the PLC.

Variables associated with work zones.

CNC PLC DNC

( section 13.2.5 )

R R/W R Status of work zone 1.

R R/W R Work zone 1. Lower limit along the selected axis (X/C).

R R/W R Work zone 1. Upper limit along the selected axis (X/C).

R R/W R Status of work zone 2.

R R/W R Work zone 2. Lower limit along the selected axis (X/C).

R R/W R Work zone 2. Upper limit along the selected axis (X/C).

R R/W R Status of work zone 3.

R R/W R Work zone 3. Lower limit along the selected axis (X/C).

R R/W R Work zone 3. Upper limit along the selected axis (X/C).

R R/W R Status of work zone 4.

R R/W R Work zone 4. Lower limit along the selected axis (X/C).

R R/W R Work zone 4. Upper limit along the selected axis (X/C).

R R/W R Status of work zone 5.

R R/W R Work zone 5. Lower limit along the selected axis (X/C).

R R/W R Work zone 5. Upper limit along the selected axis (X/C).

APPENDIX Summary of internal CNC variables.

C.
CNC 8040
·M· MODEL (SOFT V11.1X)

367

Programming manual

APPENDIX Summary of internal CNC variables.

Variable
FREAL FREAL(X-C) FTEO/X-C)
FEED DNCF PLCF PRGF
FPREV DNCFPR PLCFPR PRGFPR
PRGFIN
FRO PRGFRO DNCFRO PLCFRO CNCFRO PLCCFR

Feedrate related variables.
CNC PLC DNC
R R R Real feedrate of the CNC in mm/min or inch/min. R R R Actual (real) CNC feedrate of the selected axis. R R R Theoretical CNC feedrate of the selected axis.

( section 13.2.6 )

Variables associated with function G94.
R R R Active feedrate at the CNC in mm/min or inch/min. R R R/W Feedrate selected via DNC. R R/W R Feedrate selected via PLC. R R R Feedrate selected by program.

Variables associated with function G95.
R R R Active feedrate at CNC, in m/rev or inch/rev. R R R/W Feedrate selected via DNC. R R/W R Feedrate selected via PLC. R R R Feedrate selected by program.

Variables associated with function G32.
R R R Feedrate selected by program, in 1/min.

Variables associated with feedrate override (%)
R R R Feedrate Override (%) active at the CNC. R/W R R Override (%) selected by program.
R R R/W Override (%) selected via DNC. R R/W R Override (%) selected via PLC. R R R Override (%) selected from the front panel knob. R R/W R Override (%) of the PLC execution channel.

Variable
PPOS(X-C) POS(X-C) TPOS(X-C) APOS(X-C) ATPOS(X-C) DPOS(X-C) FLWE(X-C) DEFLEX DEFLEY DEFLEZ DIST(X-C) LIMPL(X-C) LIMMI(X-C) DPLY(X-C) DRPO(X-C) GPOS(X-C)n p

Coordinate related variables.

CNC PLC DNC

( section 13.2.7 )

- Programmed theoretical position value (coordinate).

R R R Machine coordinates. Real coordinates of the tool base.

R R R Machine coordinates. Theoretical coordinates of the tool base. R R R Part coordinates. Real coordinates of the tool base.

R R R Part coordinates. Theoretical coordinates of the tool base. R R R Theoretical position of the probe when the probe touched the part.

R R R Following error of the indicated axis.

R R R Probe deflection along X axis. R R R Probe deflection along Y axis.

RR R/W R/W

R Probe deflection along Z axis. R Distance travelled by the indicated axis.

R/W R/W R/W R/W

R Second upper travel limit. R Second lower travel limit.

R R R Coordinate of the selected axis displayed on the screen.

R R R Position indicated by the Sercos drive of the selected axis.

- Coordinate of the selected axis, programmed in the (n) block of the program

(p).

CNC 8040
·M· MODEL (SOFT V11.1X)

Variable
HANPF HANPS HANPT HANPFO HANDSE
HANFCT HBEVAR
MASLAN MASCFI MASCSE

Variables associated with electronic handwheels.

CNC PLC DNC

( section 13.2.8 )

- Pulses received from 1st handwheel since the CNC was turned on.

- Pulses received from 2nd handwheel since the CNC was turned on.

- Pulses received from 3rd handwheel since the CNC was turned on.

- Pulses received from 4th handwheel since the CNC was turned on.

For handwheels with a selector button, it indicates whether that button has

been pressed or not.

R R/W R Multiplying factor different for each handwheel (when having several).

R R/W R HBE handwheel. Reading enabled, axis being jogged and multiplying factor (x1, x10, x100).

R/W R/W R/W Linear path angle for "Path handwheel" or "Path Jog" mode. R/W R/W R/W Arc center coordinates for "Path handwheel mode" or "Path jog".

R/W R/W R/W Arc center coordinates for "Path handwheel mode" or "Path jog".

368

Variable
ASIN(X-C) BSIN(X-C) ASINS BSINS SASINS SBSINS
Variable
SREAL FTEOS
SPEED DNCS PLCS PRGS
SSO PRGSSO DNCSSO PLCSSO CNCSSO
SLIMIT DNCSL PLCSL PRGSL MDISL
POSS
RPOSS
TPOSS
RTPOSS
DRPOS
FLWES SYNCER
Variable
SSREAL SFTEOS
SSPEED SDNCS SPLCS SPRGS

Programming manual

Variables associated with feedback.

CNC PLC DNC

( section 13.2.9 )

R R R A signal of the CNC's sinusoidal feedback for the selected axis.

R R R B signal of the CNC's sinusoidal feedback for the selected axis.

R R R A signal of the CNC's sinusoidal feedback for the spindle.

R R R B signal of the CNC's sinusoidal feedback for the spindle.

R R R "A" signal of the CNC sinusoidal feedback for the second spindle.

R R R "B" signal of the CNC sinusoidal feedback for the second spindle.

Variables associated with the main spindle.
CNC PLC DNC
R R R Real spindle speed R R R Theoretical spindle speed.

( section 13.2.10 )

APPENDIX Summary of internal CNC variables.

Variables associated with spindle speed.
R R R Active spindle speed at the CNC. R R R/W Spindle speed selected via DNC. R R/W R Spindle speed selected via PLC. R R R Spindle speed selected by program.

Speed limit related variables.
R R R Spindle speed limit active at the CNC. R R R/W Spindle speed limit selected via DNC. R R/W R Spindle speed limit selected via PLC. R R R Spindle speed limit selected by program. R R/W R Maximum machining spindle speed.

Position related variables.
R R R Real Spindle position. Reading from the PLC in ten-thousandths of a degree (within ±999999999) and from the CNC in degrees (within ±99999.9999).
R R R Real Spindle position. Reading from the PLC in ten-thousandths of a degree (between 0 and 3600000) and from the CNC in degrees (between 0 and 360).
R R R Theoretical spindle position. Reading from the PLC in ten-thousandths of a degree (within ±999999999) and from the CNC in degrees (within ±99999.9999).
R R R Theoretical spindle position. Reading from the PLC in ten-thousandths of a degree (between 0 and 3600000) and from the CNC in degrees (between 0 and 360).
R R R Position indicated by the Sercos drive.

Variables related to the following error.
R R R Spindle following error. R R R Error of second spindle (synchronized) following the main spindle.

Variables associated with the second spindle.
CNC PLC DNC
R R R Real spindle speed R R R Theoretical spindle speed.
Variables associated with spindle speed.
R R R Active spindle speed at the CNC. R R R/W Spindle speed selected via DNC. R R/W R Spindle speed selected via PLC. R R R Spindle speed selected by program.

( section 13.2.11 )

CNC 8040
·M· MODEL (SOFT V11.1X)

369

Programming manual

SSSO SPRGSO SDNCSO SPLCSO SCNCSO

SSLIMI SDNCSL SPLCSL SPRGSL

APPENDIX Summary of internal CNC variables.

SPOSS SRPOSS STPOSS SRTPOS SDRPOS

SFLWES

Variable
ASPROG

Variable
PLCMSG PLCIn PLCOn PLCMn PLCRn PLCTn PLCCn PLCMMn

CNC 8040

Variable
GUP n LUP (a,b) CALLP

Variables associated with the spindle override.
R R R Spindle Speed Override (%) active at the CNC. R/W R R Override (%) selected by program.
R R R/W Override (%) selected via DNC. R R/W R Override (%) selected via PLC. R R R Spindle Speed Override (%) selected from front panel.
Speed limit related variables.
R R R Spindle speed limit active at the CNC. R R R/W Spindle speed limit selected via DNC. R R/W R Spindle speed limit selected via PLC. R R R Spindle speed limit selected by program.
Position related variables.
R R R Real Spindle position. Reading from the PLC in ten-thousandths of a degree (within ±999999999) and from the CNC in degrees (within ±99999.9999).
R R R Real Spindle position. Reading from the PLC in ten-thousandths of a degree (between 0 and 3600000) and from the CNC in degrees (between 0 and 360).
R R R Theoretical spindle position. Reading from the PLC in ten-thousandths of a degree (within ±999999999) and from the CNC in degrees (within ±99999.9999).
R R R Theoretical spindle position. Reading from the PLC in ten-thousandths of a degree (between 0 and 3600000) and from the CNC in degrees (between 0 and 360).
R R R Position indicated by the Sercos drive.
Variables related to the following error.
R R R Spindle following error.

Variables associated with the live tool.

CNC PLC DNC

( section 13.2.12 )

- Speed programmed in M45 S (within the associated subroutine).

PLC related variables.

CNC PLC DNC

( section 13.2.13 )

R/W -

R Number of the active PLC message with the highest priority. - 32 PLC inputs starting from (n).

R/W R/W -

- 32 PLC outputs starting from (n). - 32 PLC marks starting from (n).

R/W R/W -

- (n) Register. - Indicated (n) Timer's count.

R/W R/W -

- Indicated (n) Counter's count. - Modifies the (n) mark of the PLC.

Variables associated with local and global parameters.

CNC PLC DNC

( section 13.2.14 )

- R/W - Global parameter (P100-P299) (n).

- R/W - Indicated local (P0-P25) parameter (b) of the nesting level (a).

- Indicates which local parameters have been defined by means of a PCALL or MCALL instruction (calling a subroutine).

·M· MODEL (SOFT V11.1X)

370

Variable
SETGE(X-C) SETGES SSETGS SVAR(X-C) id SVARS id SSVARS id TSVAR(X-C) id TSVARS id TSSVAR id

Programming manual

Sercos variables.

CNC PLC DNC

( section 13.2.15 )

W W - Gear ratio and parameter set of the (X-C) axis drive

W W - Gear ratio and parameter set of the main spindle

W W - Gear ratio and parameter set of the second spindle

R/W -

- Sercos variable sercos for the (X-C) axis "id"

R/W -

- Sercos variable sercos for the main spindle "id"

R/W -

- Sercos variable sercos for the second spindle "id"

- Third attribute of the sercos variable for the (X-C) axis "id"

- Third attribute of the sercos variable for the main spindle "id"

- Third attribute of the sercos variable for the second spindle "id"

APPENDIX Summary of internal CNC variables.

Variable
HARCON HARCOA IDHARH IDHARL SOFCON HDMEGA KEYIDE

Software & hardware configuration variables.

CNC PLC DNC

( section 13.2.16 )

R R R It indicates, with bits, the CNC's hardware configuration.

R R R Hardware identifier (8 least significant bits).

R R R Hardware identifier (4 most significant bits).

R R R Software version of the CNC (bits 15-0) and HD (bits 31-16)

R R R Hard disk size (in megabytes).

R R R Keyboard code, according to the auto-identification system.

Variable
HARSWA HARSWB HARTST MEMTST NODE VCHECK IONODE IOSLOC IOSREM

Variables associated with telediagnosis.

CNC PLC DNC

( section 13.2.17 )

R R R Hardware configuration. R R R Hardware configuration.

R R R Hardware test. R R R Memory test.

R R R Node number in the Sercos ring. R R R Software version checksum.

R R R Position of the "ADDRESS" switch of the I/O CAN bus.

R R R Number of local I/O available. R R R Number of remote I/O available.

Variable
OPMODE OPMODA OPMODB OPMODC

Operating-mode related variables.

CNC PLC DNC

( section 13.2.18 )

R R R Operating mode. R R R Operating mode when working in the main channel.

R R R Type of simulation. R R R Axes selected by handwheel.

Variable
NBTOOL PRGN BLKN GSn GGSA GGSB GGSC GGSD MSn GMS PLANE LONGAX MIRROR SCALE SCALE(X-C)
ORGROT ROTPF ROTPS PRBST

Other variables.

CNC PLC DNC

( section 13.2.19 )

R Number of the tool being managed..

R R R Number of the program in execution.

R R R Label number of the last executed block.

- Status of the indicated G function (n).

R R Status of functions G00 thru G24.

R R Status of functions G25 thru G49.

R R Status of functions G50 thru G74.

R R Status of functions G75 thru G99.

- Status of the indicated M function (n)

R Status of M functions: M (0..6, 8, 9, 19, 30, 41..44).

R R R Abscissa and ordinate axes of the active plane.

R R R Axis affected by the tool length compensation (G15). R R R Active mirror images.

R R R General scaling factor applied. Reading from the PLC in ten-thousandths.

R R R Scaling Factor applied only to the indicated axis. Reading from the PLC in ten-thousandths.
R R R Rotation angle (G73) of the coordinate system.

- Abscissa of rotation center.

- Ordinate of rotation center.

R R R Returns probe status.

CNC 8040
·M· MODEL (SOFT V11.1X)

371

Programming manual

APPENDIX Summary of internal CNC variables.

Variable
CLOCK TIME DATE TIMER CYTIME PARTC FIRST KEY KEYSRC ANAIn ANAOn CNCERR PLCERR DNCERR AXICOM TANGAN TPIOUT(X-C) DNCSTA TIMEG SELPRO DIAM
TIPPRB PANEDI DATEDI

CNC PLC DNC

( section 13.2.19 )

R R R System clock in seconds.

R R R/W Time in Hours, minutes and seconds.

R R R/W Date in Year-Month-Day format

R/W R/W R/W Clock activated by PLC, in seconds.

R R R Time to execute a part in hundredths of a second.

R/W R/W R/W Parts counter of the CNC.

R R R First time a program is executed.

R/W R/W R/W keystroke code.

R/W R/W R/W Source of the keys.

R R R Voltage (in volts) of the indicated analog input (n).

R/W R/W R/W Voltage (in volts) to apply to the indicated output (n).

R R Active CNC error number.

R Active PLC error number.

- Number of the error generated during DNC communications.

R R R Pairs of axes switched with function G28.

R R R Angular position with respect to the path (G45).

R R R Output of the PI of the tandem master axis in rpm.

- DNC transmission status.

R R R Remaining time to finish the dwell block (in hundredths of a second).

R/W R/W R When having two probe inputs, it selects the active input.

R/W R/W R It changes the programming mode for X axis coordinates between radius and diameter.

R R R PROBE cycle being executed.

R R R WGDRAW application. Number of screen being executed.

R R R WGDRAW application. Number of element (item) being executed.

The "KEY" variable can be "written" at the CNC only via the user channel. The "NBTOOL" variable can only be used within the tool change subroutine.

CNC 8040
·M· MODEL (SOFT V11.1X)
372

KEY CODES
Alpha-numeric keyboard and monitor

Programming manual
D.

APPENDIX Key codes

CNC 8040
·M· MODEL (SOFT V11.1X)
373

Programming manual

Alphanumeric operator panel

APPENDIX Key codes

CNC 8040
·M· MODEL (SOFT V11.1X)
374

MC operator panel

Programming manual
D.

APPENDIX Key codes

CNC 8040
·M· MODEL (SOFT V11.1X)
375

APPENDIX Key codes

Programming manual
D.
CNC 8040
·M· MODEL (SOFT V11.1X)
376

APPENDIX Key codes

Programming manual
D.
CNC 8040
·M· MODEL (SOFT V11.1X)
377

Programming manual

MCO/TCO operator panel

APPENDIX Key codes

CNC 8040
·M· MODEL (SOFT V11.1X)
378

Alphanumeric keyboard

Programming manual
D.

APPENDIX Key codes

CNC 8040
·M· MODEL (SOFT V11.1X)
379

Programming manual

11" LCD Monitor

APPENDIX Key codes

CNC 8040
·M· MODEL (SOFT V11.1X)
380

Programming manual
PROGRAMMING ASSISTANCE SCREENS OF THE SYSTEM.

These screens (pages) may be displayed using the high level instruction "PAGE". They all belong to the CNC system and are used as help screens of the corresponding functions.

Syntax-graphics help screens

Page 1000

Preparatory functions G00-G09.

Page 1001

Preparatory functions G10-G19.

Page 1002

Preparatory functions G20-G44.

Page 1003

Preparatory functions G53-G59.

Page 1004

Preparatory functions G60-G69.

Page 1005

Preparatory functions G70-G79.

Page 1006

Preparatory functions G80-G89.

Page 1007

Preparatory functions G90-G99.

Page 1008

Auxiliary (miscellaneous) M functions.

Page 1009

Auxiliary (miscellaneous) M functions with the "next page" symbol.

Page 1010

Same as number 250 of the directory if there is one.

Page 1011

Same as number 251 of the directory if there is one.

Page 1012

Same as number 252 of the directory if there is one.

Page 1013

Same as number 253 of the directory if there is one.

Page 1014

Same as number 254 of the directory if there is one.

Page 1015

Same as number 255 of the directory if there is one.

Page 1016

High level language dictionary (from A to G).

Page 1017

High level language dictionary (from H to N).

Page 1018

High level language dictionary (from O to S).

Page 1019

High level language dictionary (from T to Z).

Page 1020

Variables that may be accessed through high level language (part 1).

Page 1021

Variables that may be accessed through high level language (part 2).

Page 1022

Variables that may be accessed through high level language (part 3).

Page 1023

Variables that may be accessed through high level language (part 4).

Page 1024

Variables that may be accessed through high level language (part 5).

Page 1025

Variables that may be accessed through high level language (part 6).

Page 1026

Variables that may be accessed through high level language (part 7).

Page 1027

Variables that may be accessed through high level language (part 8).

Page 1028

Variables that may be accessed through high level language (part 9).

Page 1029

Variables that may be accessed through high level language (part 10).

Page 1030

Variables that may be accessed through high level language (part 11).

APPENDIX Programming assistance screens of the system.

E.
CNC 8040
·M· MODEL (SOFT V11.1X)

381

Programming manual

Page 1031 Page 1032

Variables that may be accessed through high level language (part 12).
Mathematical operators.

APPENDIX Programming assistance screens of the system.

CNC 8040
·M· MODEL (SOFT V11.1X)
382

Programming manual

Syntax help: ISO language

Page 1033

Structure of a program block.

Page 1034

Positioning and linear interpolation: G00, G01 (part 1).

Page 1035

Positioning and linear interpolation: G00, G01 (part 2).

Page 1036

Circular-helical interpolation: G02, G03 (part 1).

Page 1037

Circular-helical interpolation: G02, G03 (part 2).

Page 1038

Circular-helical interpolation: G02, G03 (part 3).

Page 1039

Circular tangent path: G08 (part 1).

Page 1040

Circular tangent path: G08 (part 2).

Page 1041

Circular path through 3 points: G09 (part 1).

Page 1042

Circular path through 3 points: G09 (part 2).

Page 1043

Electronic threading: G33

Page 1044

Rounding: G36.

Page 1045

Tangential entry: G37.

Page 1046

Tangential exit: G38.

Page 1047

Chamfer: G39.

Page 1048

Dwell/interruption of block preparation: G04, G04K.

Page 1049

Square/round corner: G07, G05.

Page 1050

Mirror image: G11, G12, G13, G14.

Page 1051

Programming of planes and longitudinal axis. G16, G17, G18, G19, G15.

Page 1052

Work zones: G21, G22.

Page 1053

Tool radius compensation: G40, G41, G42.

Page 1054

Tool length compensation: G43, G44.

Page 1055

Zero offsets.

Page 1056

Millimeters/inches G71, G70.

Page 1057

Scaling factor: G72.

Page 1058

Pattern rotation: G73.

Page 1059

Home search: G74.

Page 1060

Probing: G75.

Page 1061

Axis coupling (slaving): G77, G78

Page 1062

Absolute/incremental: G90, G91.

Page 1063

Coordinate preset and Polar origin: G92, G93.

Page 1064

Feedrate programming: G94, G95.

Page 1065

Preparatory G functions associated with the canned cycles: G79, G80, G98 and G99.

Page 1066

Programming of auxiliary functions F, S, T and D.

Page 1067

Programming of auxiliary (miscellaneous) M functions.

APPENDIX Programming assistance screens of the system.

Syntax help: CNC tables

Page 1090

Tool offset table.

Page 1091

Tool table.

Page 1092

Tool magazine table.

Page 1093

Auxiliary (miscellaneous) M function table.

Page 1094

Zero offset table.

Page 1095

Leadscrew error compensation tables.

Page 1096

Cross compensation table.

Page 1097

Machine parameter tables.

CNC 8040
·M· MODEL (SOFT V11.1X)

383

APPENDIX Programming assistance screens of the system.

Programming manual
E.
CNC 8040
·M· MODEL (SOFT V11.1X)

Page 1098 Page 1099

User parameter tables. Passwords table.

Syntax help: High level language

Page 1100

ERROR and MSG instructions.

Page 1101

GOTO and RPT instructions.

Page 1102

OPEN and WRITE instructions.

Page 1103

SUB and RET instructions.

Page 1104

CALL, PCALL, MCALL, MDOFF and PROBE instructions.

Page 1105

DSBLK, ESBLK, DSTOP, ESTOP, DFHOLD and EFHOLD instructions.

Page 1106

IF instruction.

Page 1107

Assignment blocks.

Page 1108

Mathematical expressions.

Page 1109

PAGE instruction.

Page 1110

ODW instruction.

Page 1111

DW instruction.

Page 1112

IB instruction.

Page 1113

SK instruction.

Page 1114

WKEY and SYSTEM instructions.

Page 1115

KEYSRC instruction.

Page 1116

WBUF instruction.

Page 1117

SYMBOL instruction.

Syntax help: Canned cycles

Page 1070

Multiple machining in a straight line: G60.

Page 1071

Multiple machining in a rectangular pattern: G61.

Page 1072

Multiple machining in a grid pattern: G62.

Page 1073

Multiple machining in a circular pattern: G63.

Page 1074

Multiple machining in an arc: G64.

Page 1075

Machining programming by means of an arc chord: G65.

Page 1076

Irregular pocket canned cycle: G66.

Page 1077

Irregular-pocket roughing: G67.

Page 1078

Irregular-pocket finishing: G68.

Page 1079

Deep hole drilling canned cycle with variable peck: G69.

Page 1080

Drilling canned cycle: G81.

Page 1081

Drilling cycle with dwell: G82.

Page 1082

Deep hole drilling cycle with constant peck: G83.

Page 1083

Tapping canned cycle: G84.

Page 1084

Reaming canned cycle: G85.

Page 1085

Boring cycle with withdrawal in G00: G86.

Page 1086

Rectangular pocket canned cycle: G87.

Page 1087

Circular pocket canned cycle: G88.

Page 1088

Boring cycle with withdrawal in G01: G89.

384

MAINTENANCE

Programming manual

Cleaning
The dirt accumulated in the unit could act as a layer that hampers the dissipation of the heat generated by the internal electronic circuitry with the risk of overheating and damaging the CNC.
Also, accumulated dirt
To clean the operator panel and the monitor's front panel, a soft cloth should be used soaked in de-ionized water and home non-abrasive dishwasher soap (liquid, never powder) or with 75º alcohol.
Do not use air at high pressure to clean the unit because it could cause grease to accumulate which in turn may cause electrostatic discharges.
The plastics used on the front panel of the units are resistant to: · Grease and mineral oil. · Bases and bleach. · Dissolved detergents. · Alcohol.

APPENDIX Maintenance

Fagor Automation shall not be held responsible for any material or physical damage derived from the violation of these basic safety requirements.
To check the fuses, first unplug the unit from mains. If the CNC does not turn on when flipping the power switch, check that the fuses are the right ones and they are in good condition.
Avoid solvents. The action of solvents such as chlorine hydrocarbons, benzole, esters and ether may damage the plastics used to make the front panel of the unit.
Do not open this unit. Only personnel authorized by Fagor Automation may open this unit.
Do not handle the connectors with the unit connected to mains. Before manipulating the connectors (inputs/outputs, feedback, etc.) make sure that the unit is not connected to AC power.

CNC 8040
·M· MODEL (SOFT V11.1X)
385

APPENDIX

Programming manual
F.
CNC 8040
·M· MODEL (SOFT V11.1X)
386

Programming manual
F.
CNC 8040
·M· MODEL (SOFT V11.1X)
387

Programming manual
F.
CNC 8040
·M· MODEL (SOFT V11.1X)
388

Acrobat Distiller 6.0 (Windows)