Fagor CNC 8037 Programming Manual

CNC
8037 ·M·
Programming manual
Ref.1711
Soft: V02.2x
All rights reserved. No part of this documentation may be transmitted,
transcribed, stored in a backup device or translated into another language
without Fagor Automation’s consent. Unauthorized copying or distributing of this
software is prohibited.
It is possible that CNC can execute more functions than those described in its
associated documentation; however, Fagor Automation does not guarantee the
validity of those applications. Therefore, except under the express permission
from Fagor Automation, any CNC application that is not described in the
documentation must be considered as "impossible". In any case, Fagor
Automation shall not be held responsible for any personal injuries or physical
damage caused or suffered by the CNC if it is used in any way other than as
explained in the related documentation.
The information described in this manual may be subject to changes due to
technical modifications. Fagor Automation reserves the right to change the
contents of this manual without prior notice.
The content of this manual and its validity for the product described here has been
verified. Even so, involuntary errors are possible, hence no absolute match is
guaranteed. However, the contents of this document are regularly checked and
updated implementing the necessary corrections in a later edition. We appreciate
your suggestions for improvement.
All the trade marks appearing in the manual belong to the corresponding owners.
The use of these marks by third parties for their own purpose could violate the
rights of the owners.
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.
This product uses the following source code, subject to the terms of the GPL license. The applications busybox V0.60.2;
dosfstools V2.9; linux-ftpd V0.17; ppp V2.4.0; utelnet V0.1.1. The librarygrx V2.4.4. The linux kernel V2.4.4. The linux boot
ppcboot V1.1.3. If you would like to have a CD copy of this source code sent to you, send 10 Euros to Fagor Automation
for shipping and handling.
P r o gr a m m i ng m a n u a l
INDEX
About the product ......................................................................................................................... 7
Declaration of conformity and Warranty conditions ...................................................................... 9
Version history ............................................................................................................................ 11
Safety conditions ........................................................................................................................ 13
Returning conditions ................................................................................................................... 17
Additional notes .......................................................................................................................... 19
Fagor documentation.................................................................................................................. 21
CHAPTER 1
GENERAL CONCEPTS
1.1
1.1.1
1.2
1.3
CHAPTER 2
CREATING A PROGRAM
2.1
2.1.1
2.1.2
2.1.3
2.2
CHAPTER 3
Axis nomenclature ......................................................................................................... 36
Plane selection (G16, G17, G18, G19) .......................................................................... 37
Part dimensioning. Millimeters (G71) or inches (G70) ................................................... 39
Absolute/incremental programming (G90, G91) ............................................................ 40
Coordinate programming ............................................................................................... 41
Cartesian coordinates ................................................................................................ 42
Polar coordinates ....................................................................................................... 43
Cylindrical coordinates ............................................................................................... 45
Angle and Cartesian coordinate................................................................................. 46
Rotary axes.................................................................................................................... 47
Work zones .................................................................................................................... 48
Definition of the work zones ....................................................................................... 48
Using the work zones................................................................................................. 49
REFERENCE SYSTEMS
4.1
4.2
4.3
4.4
4.4.1
4.4.2
4.5
CHAPTER 5
Program structure at the CNC ....................................................................................... 30
Block header .............................................................................................................. 30
Program block ............................................................................................................ 31
End of block ............................................................................................................... 32
Local subroutines within a program ............................................................................... 33
AXES AND COORDINATE SYSTEMS
3.1
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
CHAPTER 4
Part programs ................................................................................................................ 24
Considerations regarding the Ethernet connection .................................................... 26
DNC connection............................................................................................................. 27
Communication protocol via DNC or peripheral device ................................................. 28
Reference points............................................................................................................ 51
Machine reference (Home) search (G74) ...................................................................... 52
Programming with respect to machine zero (G53) ........................................................ 53
Coordinate preset and zero offsets................................................................................ 54
Coordinate preset and S value limitation (G92) ......................................................... 55
Zero offsets (G54..G59 and G159) ............................................................................ 56
Polar origin preset (G93)................................................................................................ 60
ISO CODE PROGRAMMING
5.1
5.2
5.2.1
5.2.2
5.2.3
5.2.4
5.3
5.4
Preparatory functions..................................................................................................... 62
Feedrate F ..................................................................................................................... 64
Feedrate in mm/min or inches/min (G94)................................................................... 65
Feedrate in mm/rev.or inches/rev (G95) .................................................................... 66
Constant surface speed (G96) ................................................................................... 67
Constant tool center speed (G97) .............................................................................. 68
Spindle turning speed (S) .............................................................................................. 69
Tool number (T) and tool offset (D)................................................................................ 70
CNC 8037
SOFT: V02.2X
·3·
Prog ramm in g man u a l
5.5
Auxiliary function (M) ..................................................................................................... 71
5.5.1
M00. Program stop .................................................................................................... 72
5.5.2
M01. Conditional program stop.................................................................................. 72
5.5.3
M02. End of program ................................................................................................. 73
5.5.4
M30. End of program with return to the first block ..................................................... 73
5.5.5
M03. Clockwise spindle rotation ................................................................................ 74
5.5.6
M04. Counterclockwise spindle rotation .................................................................... 74
5.5.7
M05. Spindle stop ...................................................................................................... 75
5.5.8
M06. Tool change code ............................................................................................. 75
5.5.9
M19. Spindle orientation ............................................................................................ 76
5.5.10
M41, M42, M43, M44. Spindle gear change .............................................................. 77
CHAPTER 6
PATH CONTROL
6.1
6.2
6.3
6.4
6.5
6.6
6.7
6.8
6.9
6.10
6.11
6.12
6.13
6.14
6.15
CHAPTER 7
ADDITIONAL PREPARATORY FUNCTIONS
7.1
7.1.1
7.2
7.3
7.3.1
7.3.2
7.3.3
7.4
7.4.1
7.4.2
7.5
7.6
7.6.1
7.6.2
7.7
CHAPTER 8
CNC 8037
SOFT: V02.2X
·4·
Interruption of block preparation (G04) ........................................................................ 101
G04 K0: Block preparation interruption and coordinate update ............................... 103
Dwell (G04 K) .............................................................................................................. 104
Working with square (G07) and round (G05,G50) corners .......................................... 105
G07 (square corner)................................................................................................. 105
G05 (round corner) .................................................................................................. 106
Controlled round corner (G50) ................................................................................. 107
Look-ahead (G51)........................................................................................................ 108
Advanced look-ahead algorithm (integrating Fagor filters) ...................................... 110
Look-ahead operation with Fagor filters active ........................................................ 111
Mirror image (G10, G11. G12, G13, G14) ................................................................... 112
Scaling factor (G72)..................................................................................................... 113
Scaling factor applied to all axes. ............................................................................ 114
Scaling factor applied to one or more axes.............................................................. 115
Pattern rotation (G73) .................................................................................................. 117
TOOL COMPENSATION
8.1
8.1.1
8.1.2
8.1.3
8.1.4
8.2
8.3
CHAPTER 9
Rapid traverse (G00) ..................................................................................................... 80
Linear interpolation (G01) .............................................................................................. 81
Circular interpolation (G02, G03) ................................................................................... 82
Circular interpolation with absolute arc center coordinates (G06) ................................. 87
Arc tangent to previous path (G08)................................................................................ 88
Arc defined by three points (G09).................................................................................. 89
Helical interpolation ....................................................................................................... 90
Tangential entry at the beginning of a machining operation (G37) ................................ 91
Tangential exit at the end of a machining operator (G38) ............................................. 92
Automatic radius blend (G36) ........................................................................................ 93
Chamfer (G39) ............................................................................................................... 94
Threading (G33) ............................................................................................................ 95
Variable pitch threads (G34) .......................................................................................... 97
Move to hardstop (G52) ................................................................................................. 98
Feedrate "F" as an inverted function of time (G32)........................................................ 99
Tool radius compensation (G40, G41, G42) ................................................................ 120
Beginning of tool radius compensation .................................................................... 121
Sections of tool radius compensation ...................................................................... 124
Cancellation of tool radius compensation ................................................................ 125
Change of type of radius compensation while machining ........................................ 131
Tool length compensation (G43, G44, G15) ................................................................ 132
Collision detection (G41 N, G42 N) ............................................................................. 134
CANNED CYCLES
9.1
9.2
9.2.1
9.3
9.4
9.5
9.6
9.6.1
9.7
9.7.1
9.8
9.8.1
9.9
9.9.1
Canned cycle definition................................................................................................ 136
Influence zone of a canned cycle ................................................................................ 137
G79. Modification of the canned cycle parameters .................................................. 138
Canned cycle cancellation ........................................................................................... 140
Some general points to consider ................................................................................. 141
Machining canned cycles............................................................................................. 142
G69. Drilling canned cycle with variable peck ............................................................. 145
Basic operation ........................................................................................................ 147
G81. Drilling canned cycle ........................................................................................... 150
Basic operation ........................................................................................................ 151
G82. Drilling canned cycle with dwell .......................................................................... 153
Basic operation ........................................................................................................ 154
G83. Deep-hole drilling canned cycle with constant peck ........................................... 156
Basic operation ........................................................................................................ 158
P r o gr a m m i ng m a n u a l
9.10
9.10.1
9.11
9.11.1
9.12
9.12.1
9.13
9.13.1
9.14
9.14.1
9.15
9.15.1
9.16
9.16.1
9.17
9.17.1
9.18
9.18.1
CHAPTER 10
MULTIPLE MACHINING
10.1
10.1.1
10.2
10.2.1
10.3
10.3.1
10.4
10.4.1
10.5
10.5.1
10.6
10.6.1
CHAPTER 11
G60: Multiple machining in a straight line .................................................................... 194
Basic operation ........................................................................................................ 195
G61: Multiple machining in rectangular pattern ........................................................... 196
Basic operation ........................................................................................................ 198
G62: Multiple machining in grid pattern ....................................................................... 199
Basic operation ........................................................................................................ 201
G63: Multiple machining in a circular pattern............................................................... 202
Basic operation ........................................................................................................ 204
G64: Multiple machining in an arc................................................................................ 205
Basic operation ........................................................................................................ 207
G65: Machining programmed with an arc-chord.......................................................... 208
Basic operation ........................................................................................................ 209
PROBING
11.1
CHAPTER 12
G84. Tapping canned cycle ......................................................................................... 160
Basic operation ........................................................................................................ 162
G85. Reaming canned cycle........................................................................................ 165
Basic operation ........................................................................................................ 166
G86. Boring cycle with withdrawal in G00.................................................................... 167
Basic operation ........................................................................................................ 169
G87. Rectangular pocket canned cycle. ...................................................................... 170
Basic operation ........................................................................................................ 173
G88. Circular pocket canned cycle .............................................................................. 176
Basic operation ........................................................................................................ 180
G89. Boring cycle with withdrawal at work feedrate (G01) .......................................... 182
Basic operation ........................................................................................................ 183
G210. Bore milling canned cycle ................................................................................. 184
Basic operation ........................................................................................................ 186
G211. Inside thread milling cycle ................................................................................. 187
Basic operation ........................................................................................................ 189
G212. Outside thread milling cycle .............................................................................. 190
Basic operation ........................................................................................................ 192
Probing (G75, G76)...................................................................................................... 212
HIGH-LEVEL LANGUAGE PROGRAMMING
12.1
Lexical description ....................................................................................................... 213
12.2
Variables ...................................................................................................................... 215
12.2.1
General purpose parameters or variables................................................................ 216
12.2.2
Variables associated with tools. ............................................................................... 218
12.2.3
Variables associated with zero offsets. .................................................................... 221
12.2.4
Variables associated with machine parameters....................................................... 223
12.2.5
Variables associated with work zones ..................................................................... 224
12.2.6
Variables associated with feedrates......................................................................... 225
12.2.7
Variables associated with coordinates ..................................................................... 227
12.2.8
Variables associated with electronic handwheels .................................................... 230
12.2.9
Variables associated with feedback ......................................................................... 232
12.2.10 Variables associated with the main spindle ............................................................. 233
12.2.11 PLC related variables............................................................................................... 235
12.2.12 Variables associated with local parameters ............................................................. 237
12.2.13 Operating-mode related variables............................................................................ 238
12.2.14 Other variables......................................................................................................... 240
12.3
CONSTANTS............................................................................................................... 247
12.4
Operators ..................................................................................................................... 248
12.5
Expressions ................................................................................................................. 250
12.5.1
Arithmetic expressions ............................................................................................. 250
12.5.2
Relational expressions ............................................................................................. 251
CNC 8037
CHAPTER 13
PROGRAM CONTROL INSTRUCTIONS
13.1
13.2
13.3
13.4
13.5
13.5.1
13.6
13.7
13.8
Assignment instructions ............................................................................................... 254
Display instructions ...................................................................................................... 255
Enable-disable instructions .......................................................................................... 256
Flow control instructions .............................................................................................. 257
Subroutine instructions ................................................................................................ 259
Calls to subroutines using G functions..................................................................... 263
Interruption-subroutine instructions.............................................................................. 264
Program instructions .................................................................................................... 265
Screen customizing instructions .................................................................................. 268
SOFT: V02.2X
·5·
Prog ramm in g man u a l
CHAPTER 14
ANGULAR TRANSFORMATION OF AN INCLINE AXIS
14.1
14.2
Turning angular transformation on and off................................................................... 277
Freezing the angular transformation............................................................................ 278
A
B
C
D
E
ISO code programming................................................................................................ 281
Program control instructions ........................................................................................ 283
Summary of internal CNC variables. ........................................................................... 285
Key code...................................................................................................................... 291
Maintenance ................................................................................................................ 293
APPENDIX
CNC 8037
SOFT: V02.2X
·6·
ABOUT THE PRODUCT
BASIC CHARACTERISTICS
Monitor
7.5" Color LCD
Block processing time
Look-ahead
7 ms
75 blocks
RAM memory
1 Mb
Flash memory
128 MB
PLC cycle time
3 ms / 1000 instructions
Minimum position loop
4 ms
USB
Standard
RS-232 serial line
Standard
DNC ( via RS232 )
Standard
Ethernet
Option
5 V or 24 V probe inputs
Local digital inputs and outputs.
Feedback inputs for the axes and spindle
Feedback inputs for handwheels
Analog outputs
2
16 I / 8 O
40 I / 24 O
56 I / 32 O
4 TTL / 1Vpp inputs
2 TTL inputs
4 for axes and spindle
CAN servo drive system for Fagor servo drive connection.
Option
Remote CAN modules, for digital I/O expansion (RIO).
Option
Before start-up, verify that the machine that integrates this CNC meets the 89/392/CEE Directive.
CNC 8037
·7·
SOFTWARE OPTIONS
About the product
Model
CNC 8037
·8·
M
T
TC
Number of axes
3
2
2
Number of spindles
1
1
1
Electronic threading
Standard
Standard
Standard
Tool magazine management:
Standard
Standard
Standard
Machining canned cycles
Standard
Standard
Standard
Multiple machining
Standard
-----
-----
Rigid tapping
Standard
Standard
Standard
DNC
Standard
Standard
Standard
Tool radius compensation
Standard
Standard
Standard
Retracing
Standard
-----
-----
Jerk control
Standard
Standard
Standard
Feed forward
Standard
Standard
Standard
Oscilloscope function (Setup assistance)
Standard
Standard
Standard
Roundness test (Setup assistance)
Standard
Standard
Standard
DECLARATION OF CONFORMITY AND
WARRANTY CONDITIONS
DECLARATION OF CONFORMITY
The declaration of conformity for the CNC is available in the downloads section of FAGOR’S corporate
website at http://www.fagorautomation.com. (Type of file: Declaration of conformity).
WARRANTY TERMS
The warranty conditions for the CNC are available in the downloads section of FAGOR’s corporate website
at http://www.fagorautomation.com. (Type of file: General sales-warranty conditions).
CNC 8037
·9·
CNC 8037
·10·
Declaration of conformity and Warranty conditions
VERSION HISTORY
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
Operating manual
OPT-TC
Operating manual for the TC option.
Software V01.42
March 2012
First version.
Software V01.60
December 2013
List of features
Manual
Auto-adjustment of axis machine parameter DERGAIN
INST
New value for axis machine parameter ACFGAIN (P46)
INST
Value 120 of the OPMODE variable.
INST / PRG
Software V02.00
February 2014
List of features
Manual
Profile machining in segments. J parameter for G66 and G68 cycles.
PRG
Calls to subroutines using G functions.
INST / PRG
Anticipated tool management.
INST
New values for MAXGEAR1..4 (P2..5) and SLIMIT (P66) parameters.
INST
Quick block search.
OPT
Local subroutines within a program.
PRG
Avoid spindle stop with M30 or RESET. Spindle parameter SPDLSTOP (P87).
INST
Programming T and M06 with associated with a subroutine in the same line.
PRG
New values of the OPMODE variable.
INST / PRG
New variables: DISABMOD, GGSN, GGSO, GGSP, GGSQ, CYCCHORDERR.
INST / PRG
WRITE instruction: “$” character followed by “P”.
PRG
Cancel additive handwheel offset with G04 K0. General parameter ADIMPG (P176).
INST / PRG
Ethernet parameter NFSPROTO (P32). TCP or UDP protocol selection.
INST
API compliant thread.
OPT TC
Roughing by segments in inside profiling cycles 1 and 2.
INST / OPT TC
Programming the Z increment and the angle on threads.
INST / OPT TC
Manual tool calibration without stopping the spindle during each step.
INST / OPT TC
CNC 8037
·11·
Software V02.03
List of features
Manual
Set PAGE and SYMBOL instructions support PNG and JPG/JPEG formats.
PRG
New values for parameters MAXGEAR1..4 (P2..5), SLIMIT (P66) and DFORMAT (P1).
INST
Software V02.10
Version history
July 2014
November 2014
List of features
Manual
Incremental zero offset (G158).
INST / PRG
Programs identified with letters.
OPT
Variables PRGN and EXECLEV.
INST
Korean language.
INST
Change of default value for general machine parameters: MAINOFFS (P107), MAINTASF (P162)
and FEEDTYPE (P170).
INST
New variable EXTORG.
INST / PRG
Image handling via DNC.
PRG
Save/restore a trace of the oscilloscope.
OPT
Software V02.21
List of features
Manual
PLC library.
INST
Zero offsets table in ISO mode.
OPT
Compensation of the elastic deformation in the coupling of an axis.
INST
Machine axis parameter DYNDEFRQ (P103).
INST
Change of maximum value of axis and spindle parameter NPULSES.
INST
Software V02.22
CNC 8037
·12·
July 2015
March 2016
List of features
Manual
Axis filters for movements with the handwheel. General machine parameter HDIFFBAC (P129)
and machine axis parameter HANFREQ (P104).
INST
Change of maximum value of axis and spindle parameter NPULSES.
INST
SAFETY CONDITIONS
Read the following safety measures in order to prevent harming people or damage to this product and those
products connected to it.
The unit can only be repaired by personnel authorized by Fagor Automation.
Fagor Automation shall not be held responsible of any physical or material damage originated from not
complying with these basic safety rules.
PRECAUTIONS AGAINST PERSONAL HARM
• 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 electric shocks.
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 operate this unit in explosive environments.
In order to avoid risks, harm or damages, do not work in explosive environments.
CNC 8037
·13·
PRECAUTIONS AGAINST PRODUCT DAMAGE
• Work 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 that could suffer or cause when installed
under other conditions (residential or domestic environments).
Safety conditions
• Install this unit in the proper place.
It is recommended, whenever possible, to install the CNC away from coolants, chemical product, blows,
etc. that could damage it.
This unit meets 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 mains as the unit.
 Nearby portable transmitters (radio-telephones, Ham radio transmitters).
 Nearby radio / TC transmitters.
 Nearby arc welding machines.
 Nearby high voltage lines.
 Etc.
• Enclosures.
It is up to the manufacturer to guarantee that the enclosure where the unit has been installed meets
all the relevant directives of the European Union.
• Avoid disturbances coming from the machine tool.
The machine-tool must have all the interference generating elements (relay coils, contactors, motors,
etc.) uncoupled.
 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 y C=0,2 µF / 600 V.
 AC motors. RC connected between phases, with values of R=300  / 6 W y C=0,47 µF / 600 V.
• Use the proper power supply.
Use an external regulated 24 Vdc power supply for the inputs and outputs.
• Connecting the power supply to ground.
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 (8037 CNC).
Make sure that the needed gap is kept between the central unit and each wall of the enclosure. Use
a DC fan to improve enclosure ventilation.
CNC 8037
·14·
• 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.
PROTECTIONS OF THE UNIT ITSELF (8037)
• Central unit.
It has a 4 A 250V external fast fuse (F).
X8
X7
FUSES
+24V
0V
X9
X10
X11
X12
X2
X3
X4
X5
Safety conditions
X1
X6
• Inputs-Outputs.
All the digital inputs and outputs have galvanic isolation via optocouplers between the CNC circuitry
and the outside.
CNC 8037
·15·
PRECAUTIONS DURING REPAIRS
Safety conditions
Do not manipulate the inside of the unit. Only personnel authorized by Fagor Automation may access
the interior of this unit.
Do not handle the connectors with the unit connected to AC power. Before manipulating the connectors
(inputs/outputs, feedback, etc.) make sure that the unit is not connected to AC power.
SAFETY SYMBOLS
• Symbols that may appear in 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 could be caused by certain operations and the actions to take to prevent
them.
Mandatory symbol.
It indicates actions or operations that MUST be carried out.
i
CNC 8037
·16·
Information symbol.
It indicates notes, warnings and advises.
RETURNING CONDITIONS
When sending the central nit or the remote modules, pack them in its original package and packaging
material. If you do not have the original packaging material, pack it as follows:
1. Get a cardboard box whose 3 inside dimensions are at least 15 cm (6 inches) larger than those of the
unit itself. The cardboard being used to make the box must have a resistance of 170 kg. (375 pounds).
2. Attach a label indicating the owner of the unit, person to contact, type of unit and serial number.
3. In case of failure, also indicate the symptom and a short description of the failure.
4. Protect the unit wrapping it up with a roll of polyethylene or with similar material.
5. When sending the central unit, protect especially the screen.
6. Pad the unit inside the cardboard box with polyurethane foam on all sides.
7. Seal the cardboard box with packaging tape or with industrial staples.
CNC 8037
·17·
CNC 8037
·18·
Returning conditions
ADDITIONAL NOTES
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 made properly.
In case of a malfunction or failure, disconnect it and call the technical service. Do not get into the inside
of the unit.
CNC 8037
·19·
CNC 8037
·20·
Additional notes
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.
TC Manual
Directed to the end user.
It describes how to operate and program in TC mode.
It contains a self-teaching manual.
CNC 8037
·21·
CNC 8037
·22·
Fagor documentation
GENERAL CONCEPTS
1
The CNC may be programmed at the machine (from the front panel) and from a peripheral
(computer). 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 exchanged with a computer or peripheral device, using the RS232C serial
line.
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 8037
·M· MODEL
SOFT: V02.2X
·23·
Prog ramm in g man u a l
1.1
Part programs
The operating manual describes the different operating modes. Refer to that manual for further
information.
Editing a part-program
1.
Part programs
GENERAL CONCEPTS
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 part-programs may
be stored in the hard disk (KeyCF) at a PC connected through the serial line or in the USB disk.
To transmit a program to a PC through the serial, proceed as follows:
1. Execute the "WinDNC.exe" application program 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 hard disk (KeyCF), in a PC or in the USB 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 hard disk (KeyCF), in a PC or in the USB 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 line.
• From a program in execution, it is possible to execute another program located in RAM memory,
in the hard disk (KeyCF) or in a PC using the EXEC instruction.
The user customizing programs must be in RAM memory so the CNC can execute them.
–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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·24·
P r o gr a m m i ng m a n u a l
Operations that may be carried out with part-programs.
DNC
See the program directory of ...
See the subroutine directory of ...
Yes
Yes
Yes
No
Yes
No
Create the work directory from ...
Change the work directory from ...
No
No
No
No
No
Yes
Edit a program from ...
Modify a program from ...
Delete a program from ...
Yes
Yes
Yes
Yes
Yes
Yes
No
No
Yes
Copy from/to RAM memory to/from ...
Copy from/to HD to/from ...
Copy from/to DNC to/from ...
Yes
Yes
Yes
Yes
Yes
Yes
Yes
Yes
Yes
Rename a program from ...
Change the comment of a program from ...
Change the protections of a program from ...
Yes
Yes
Yes
Yes
Yes
Yes
No
No
No
Execute a part-program from ...
Execute a user program from ...
Execute a PLC program from ...
Execute programs with GOTO or RPT instructions from ...
Execute subroutines residing in ...
Execute programs with the EXEC instruction, in RAM from ...
Execute programs with the EXEC instruction, in HD from ...
Execute programs with the EXEC instruction, in DNC from ...
Yes
Yes
Yes
Yes
Yes
Yes
Yes
Yes
Yes
Yes
No
Yes
No
Yes
Yes
Yes
Yes
No
No
No
No
Yes
Yes
No
Open programs with the OPEN instruction, in RAM from ...
Open programs with the OPEN instruction, in HD from ...
Open programs with the OPEN instruction, in DNC from ...
Yes
Yes
Yes
Yes
Yes
Yes
Yes
Yes
No
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 ...
No
No
No
Yes
No
No
No
No
No
1.
Part programs
Hard
disk
GENERAL CONCEPTS
RAM
memory
(*) If it is not in RAM memory, it generates the executable code in RAM and it executes it.
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 (KeyCF).
• 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 8037
·M· MODEL
SOFT: V02.2X
·25·
Prog ramm in g man u a l
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 (KeyCF) may be edited and modified from any PC.
Instructions for setting up a PC to access CNC directories
1.
To set up the PC to access the CNC directories, we recommend to proceed as follows.
Part programs
GENERAL CONCEPTS
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.
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 two commas (,) the program attributes O (OEM), H (hidden), M
(modifiable), X (executable).
Examples:
%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.
CNC 8037
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.
·M· MODEL
SOFT: V02.2X
·26·
P r o gr a m m i ng m a n u a l
DNC connection
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.
DNC connection
1.
GENERAL CONCEPTS
1.2
CNC 8037
·M· MODEL
SOFT: V02.2X
·27·
Prog ramm in g man u a l
1.3
Communication protocol via DNC or peripheral device
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.
1.
GENERAL CONCEPTS
Communication protocol via DNC or peripheral device
Then, and separated by a comma ",", comes the protection of each file, read, write, etc. These
protections are optional, since their programming is not obligatory.
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
Image handling via DNC
While using WinDNC (version V6.01 or later), it is possible to send and receive PNG, JPG/JPEG
and BMP type images via DNC.
WinDNC software:
Version V6.01 of WinDNC supports files with extension bmp, png, jpg and jpeg. The maximum length
or the file name is 16 characters (including the dot and the extension).
The application scans all image type files in the work folder. When sending the files, if the name
of any file is too long, it will ask the user to enter a new shorter name (up to 16 characters). It must
also keep the original extension.
CNC 8037
·M· MODEL
SOFT: V02.2X
·28·
CREATING A PROGRAM
2
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 8037
·M· MODEL
SOFT: V02.2X
·29·
Prog ramm in g man u a l
2.1
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
CREATING A PROGRAM
Program structure at the CNC
2.
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 200 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.
200 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(0-99999999).
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 8 digits (0-99999999).
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.
Restrictions:
• Displaying the active block number at the top window on the screen:
 When executing a program in ISO mode, when the label number is higher than 9999, it
displays N**** .
 On the "DISPLAY / SUBROUTINES" window, when displaying an RPT that has a label higher
than 9999, it displays it with ****.
• Canned cycles G66, G67 and G68 (irregular pockets with islands) can only be edited using 4digit labels.
CNC 8037
·M· MODEL
SOFT: V02.2X
·30·
P r o gr a m m i ng m a n u a l
Program block
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.
• 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. Also, it allows the use of any type of arithmetic, relational
or logical expression.
Program structure at the CNC
2.
• Preparatory functions for movement, used to determine geometry and working conditions, such
as linear and circular interpolations, threading, etc.
CREATING A PROGRAM
2.1.2
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·31·
Prog ramm in g man u a l
2.1.3
End of block
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.
CREATING A PROGRAM
Program structure at the CNC
2.
CNC 8037
·M· MODEL
SOFT: V02.2X
·32·
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.
P r o gr a m m i ng m a n u a l
Local subroutines within a program
A subroutine is a part of a program which, being properly identified, can be called from any position
of a program to be executed.
Local subroutines may be defined within a program. These subroutines are executed from RAM or
hard disk memory.
The local subroutines are defined as part of a program. These subroutines may only be called upon
from the program where it has been defined.
The local subroutines are located at the beginning of the program, before the actual beginning of
the program. Local subroutines are defined by programming (LSUB n), where n indicates the
subroutine number. Followed by the contents of the subroutine.
The range of local subroutines is from 0 to 9999.
(LSUB 0)
(LSUB 9999)
The actual beginning of the program is identified with the % sign. Any text may follow this character.
A local subroutine may be called upon using the commands CALL, PCALL or MCALL. When
executing the calls, it first looks for the subroutines defined as local in that program and having
matching names. If there aren't any, it will look among the global subroutines.
2.
Local subroutines within a program
Programming
CREATING A PROGRAM
2.2
To execute a local subroutine directly, program (LL n). This way, only the local subroutine will be
executed. If this subroutine does not exist, it will not execute anything and it will issue an error
message indicating undefined subroutine.
Up to 100 local subroutines may be defined in a program. The maximum local subroutine nesting
level is 15.
Examples:
Example 1:
Example 2:
(LSUB9505)
X100
(RET)
(LSUB9505)
X100
(RET)
%**** ; beginning of program
(CALL 9505)
M30
%**** ; beginning of program
(LL9505)
M30
CNC 8037
·M· MODEL
SOFT: V02.2X
·33·
Prog ramm in g man u a l
Executing programs:
(LL n) Call to a local subroutine.
Parameters cannot be initialized with this command.
(CALL n) Call to a local or global subroutine.
Parameters cannot be initialized with this command.
(PCALL n ...) Call to a global or local subroutine.
Local parameters can be initialized with this command.
(MCALL n ...) Modal call to a local or global subroutine.
Local parameters can be initialized with this command.
CREATING A PROGRAM
Local subroutines within a program
2.
CNC 8037
·M· MODEL
SOFT: V02.2X
·34·
Limitations:
A local subroutine can call a global subroutine but a global subroutine cannot call a local subroutine
except if that local subroutine is defined in the root program; in other words, in the first program that
is executed.
Local subroutines defined inside a program that has been called with the "EXEC" command are
ignored. It only takes into account the ones defined in the root program.
It only takes into account local subroutines that are in programs that are executed from the CNC
execution channel, either in ISO mode or in conversational mode. Local subroutines cannot be
executed from the PLC channel.
AXES AND COORDINATE SYSTEMS
3
Given that the purpose 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 its coordinates.
The CNC allows you to use absolute, relative or incremental coordinates throughout the same
program.
CNC 8037
·M· MODEL
SOFT: V02.2X
·35·
Prog ramm in g man u a l
3.1
Axis nomenclature
The axes are named according to DIN 66217.
Axis nomenclature
AXES AND COORDINATE SYSTEMS
3.
Characteristics of the system of axes:
X and Y
main movements on the main work plane of the machine.
Z
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.
The drawing below shows an example of the nomenclature of the axes on a milling-profiling machine
with a tilted table.
CNC 8037
·M· MODEL
SOFT: V02.2X
·36·
P r o gr a m m i ng m a n u a l
Plane selection (G16, G17, G18, G19)
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.
• Rotation of the coordinate system.
• 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.
G17.
Selects the XY plane and the Z axis as longitudinal axis.
G18.
Selects the ZX plane and the Y axis as longitudinal axis.
G19.
Selects the YZ plane and the X axis as longitudinal axis.
Plane selection (G16, G17, G18, G19)
3.
• Machining canned cycles.
AXES AND COORDINATE SYSTEMS
3.2
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.
CNC 8037
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.
·M· MODEL
SOFT: V02.2X
·37·
Prog ramm in g man u a l
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.
Plane selection (G16, G17, G18, G19)
AXES AND COORDINATE SYSTEMS
3.
CNC 8037
·M· MODEL
SOFT: V02.2X
·38·
P r o gr a m m i ng m a n u a l
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.
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".
Part dimensioning. Millimeters (G71) or inches (G70)
3.
• G71. Programming in millimeters.
AXES AND COORDINATE SYSTEMS
3.3
CNC 8037
·M· MODEL
SOFT: V02.2X
·39·
Prog ramm in g man u a l
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.
3.
AXES AND COORDINATE SYSTEMS
Absolute/incremental programming (G90, G91)
The G90/G91 functions are modal and incompatible with each other.
Absolute coordinates:
G90
X0
Y0
; Point P0
X150.5
Y200
; Point P1
X300
X0
; Point P2
Y0
; Point P0
Incremental coordinates:
G90
X0
Y0
; Point P0
G91
X150.5
Y200
; Point P1
X149.5
X-300
; Point P2
Y-200
; 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".
CNC 8037
·M· MODEL
SOFT: V02.2X
·40·
P r o gr a m m i ng m a n u a l
Coordinate programming
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 :
• Polar coordinates
• Cylindrical coordinates
• Angle and Cartesian coordinate
Coordinate programming
3.
• Cartesian coordinates
AXES AND COORDINATE SYSTEMS
3.5
CNC 8037
·M· MODEL
SOFT: V02.2X
·41·
Prog ramm in g man u a l
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.
3.
Coordinate programming
AXES AND COORDINATE SYSTEMS
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·42·
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.
P r o gr a m m i ng m a n u a l
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 :
• 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.
Coordinate programming
3.
AXES AND COORDINATE SYSTEMS
3.5.2
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.
Programming example assuming that the Polar Origin is located at the Coordinate Origin.
Absolute coordinates:
G90
X0
Y0
; Point P0
G01
R100
Q0
; Point P1, in a straight line (G01)
G01
R50
Q30
; Point P2, in an arc (G03)
G01
R50
Q30
; Point P3, in a straight line (G01)
Q60
; Point P4, in an arc (G03)
Q60
; Point P5, in a straight line (G01)
Q90
; Point P6, in arc (G03)
Q90
; Point P0, in a straight line (G01)
G03
G01
R100
G03
G01
R0
CNC 8037
·M· MODEL
SOFT: V02.2X
·43·
Prog ramm in g man u a l
Incremental coordinates:
G90
X0
Y0
; Point P0
G91 G01
R100
Q0
; Point P1, in a straight line (G01)
G01
R50
Q30
; Point P2, in an arc (G03)
G01
R-50
Q0
; Point P3, in a straight line (G01)
Q30
; Point P2, in an arc (G03)
Q0
; Point P1, in a straight line (G01)
Q30
; Point P6, in arc (G03)
Q0
; Point P1, in a straight line (G01)
G03
G01
3.
R50
G03
Coordinate programming
AXES AND COORDINATE SYSTEMS
G01
CNC 8037
·M· MODEL
SOFT: V02.2X
·44·
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.
P r o gr a m m i ng m a n u a l
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 :
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
Coordinate programming
3.
AXES AND COORDINATE SYSTEMS
3.5.3
CNC 8037
·M· MODEL
SOFT: V02.2X
·45·
Prog ramm in g man u a l
3.5.4
Angle and Cartesian coordinate
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:
Coordinate programming
AXES AND COORDINATE SYSTEMS
3.
X10
Y20
; Point P0, starting point
Q45
X30
; Point P1
Q90
Y60
; Point P2
Q-45
X50
; Point P3
Q-135
Y20
; Point P4
Q180
X10
; Point P0
To represent a point in space, the rest of the coordinates may be programmed in Cartesian
coordinates.
CNC 8037
·M· MODEL
SOFT: V02.2X
·46·
P r o gr a m m i ng m a n u a l
Rotary axes
The types of rotary axes available are:
Normal rotary axis.
Positioning-only rotary axis.
Rotary HIRTH axis.
Each one of them can be divided into:
3.
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.
Rotary axes
Rollover
AXES AND COORDINATE SYSTEMS
3.6
Non-rollover axis programming.
In G90 and G91 like a linear axis.
Positioning-only rotary 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 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.
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·47·
Prog ramm in g man u a l
3.7
Work zones
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.
3.
Work zones
AXES AND COORDINATE SYSTEMS
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
Indicates the work zone you wish to define (1, 2, 3 or 4).
X...C
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).
For safety, the axis stops 0.1mm before the programmed limit.
It is not necessary to program all the axes, so only defined axes will be limited.
G20 K1 X20 Y20
G21 K1 X100 Y50
CNC 8037
·M· MODEL
SOFT: V02.2X
·48·
P r o gr a m m i ng m a n u a l
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).
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 set (1, 2, 3 or 4).
S
Indicates the enabling/disabling of the work zone.
Work zones
3.
AXES AND COORDINATE SYSTEMS
3.7.2
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 8037
·M· MODEL
SOFT: V02.2X
·49·
Prog ramm in g man u a l
Work zones
AXES AND COORDINATE SYSTEMS
3.
CNC 8037
·M· MODEL
SOFT: V02.2X
·50·
REFERENCE SYSTEMS
4.1
4
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 coordinate
system of the machine.
• Part zero or point of origin of the part. This is the origin point that is set for programming the
measurements of the part. It can be freely selected by the programmer, and its machine
reference zero 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".
M
Machine zero
W
Part zero
R
Machine reference point
XMW, YMW, ZMW...
Coordinates of the part zero
XMR, YMR, ZMR...
Coordinates of machine reference point ("REFVALUE")
CNC 8037
·M· MODEL
SOFT: V02.2X
·51·
Prog ramm in g man u a l
4.2
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.
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".
REFERENCE SYSTEMS
Machine reference (Home) search (G74)
4.
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 part zero will be maintained and the CNC will display the position values with
respect to that part zero.
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 8037
·M· MODEL
SOFT: V02.2X
·52·
P r o gr a m m i ng m a n u a l
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.
This function temporarily cancels radius and tool length compensation.
M
Machine zero
W
Part zero
4.
Programming with respect to machine zero (G53)
Function G53 is not modal, so it should be programmed every time you wish to indicate the
coordinates referred to machine zero.
REFERENCE SYSTEMS
4.3
CNC 8037
·M· MODEL
SOFT: V02.2X
·53·
Prog ramm in g man u a l
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
4.
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.
• Through the use of zero offsets (G54 ... G59, G159N1 ... G159N20); 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)
G54
G55
G56
G57
ORG*(58)
G58
G92
ORG*(59)
ORG*
CNC 8037
PLC Parameters.
Zero offsets
·M· MODEL
SOFT: V02.2X
·54·
PLCOF*
G59
P r o gr a m m i ng m a n u a l
Coordinate preset and S value limitation (G92)
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 :
; 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
Coordinate preset and zero offsets
4.
G92 X...C ±5.5
REFERENCE SYSTEMS
4.4.1
• 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 8037
·M· MODEL
SOFT: V02.2X
·55·
Prog ramm in g man u a l
4.4.2
Zero offsets (G54..G59 and G159)
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 types of zero offsets:
• Absolute zero offsets (G54 ... G57, G159N1 ... G159N20), must be referred to machine zero
(home).
4.
REFERENCE SYSTEMS
Coordinate preset and zero offsets
• 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.
Example: The zero offset table is initialized with the following values:
CNC 8037
·M· MODEL
SOFT: V02.2X
·56·
G54:
X200
Y100
G55:
X160
Y 60
G56:
X170
Y110
G58:
X-40
Y-40
G59:
X-30
Y 10
P r o gr a m m i ng m a n u a l
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
; 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
REFERENCE SYSTEMS
G54
Function G158 (incremental zero offset)
Coordinate preset and zero offsets
4.
Using incremental zero offsets:
The G158 instruction may be used to program and activate an incremental offset in a program. This
feature is used to define new part zeros in the same program without having to set them previously
in the offset table or use high level instructions.
When applying an incremental zero offset, the CNC adds it to the absolute zero offset active at a time.
Programming:
Incremental zero offset are defined by program using function G158 followed by the values of the
zero offset to be applied on each axis. To cancel the incremental zero offset, program function G158
without axes in the block. To cancel the incremental zero offset only on particular axes, program
a 0 (zero) incremental offset for each one of them.
Y
2
65
3
W
50
W
1
20
4
W
20
W
40
60
X
120
X
Y
G54 (G159N1)
20
20
G55 (G159N2)
120
20
CNC 8037
N100 G54
(It applies the first zero offset)
···
(Machining of profile 1)
N200 G158 X20 Y45
(Apply incremental zero offset)
···
(Machining of profile 2)
N300 G55
(It applies the second zero offset. G158 stays active)
···
(Machining of profile 3)
N400 G158
(Cancel incremental zero offset. G55 stays active)
···
(Machining of profile 4)
·M· MODEL
SOFT: V02.2X
·57·
Prog ramm in g man u a l
X
90
90
90
90
A4
A3
A2
A1
Z
150
240
330
G55
REFERENCE SYSTEMS
Coordinate preset and zero offsets
4.
G158
420
G54
G158
G158
X
Z
G54 (G159N1)
0
420
G55 (G159N2)
0
330
N100 G54
(It applies the first absolute zero offset)
···
(Machining of profile A1)
N200 G158 Z-90
(Apply incremental zero offset)
···
(Machining of profile A2)
N300 G55
(It applies the second absolute zero offset)
(The incremental zero offset stays active)
···
(Machining of profile A3)
N200 G158 Z-180
(It applies the second incremental zero offset)
···
(Machining of profile A4)
Only one incremental zero may be active at a time for each axis; therefore, applying an incremental
zero offset on an axis cancels the one that was active on that axis. The offsets on the rest of the
axes are not affected.
Y
80
W
50
20
M
G54 (G159N1)
CNC 8037
·M· MODEL
SOFT: V02.2X
·58·
W
W
W
20
W
40
70
120
X
Y
20
20
N100 G54
(Apply absolute zero offset)
N200 G158 X20 Y60
(It applies the first incremental zero offset)
N300 G158 X50 Y30
(It applies the second incremental zero offset)
N400 G158 X100
(It applies the third incremental zero offset)
N500 G158 Y0
(It applies the fourth incremental zero offset)
N600 G158 X0
(Cancel incremental zero offset)
X
P r o gr a m m i ng m a n u a l
The incremental zero offset is not canceled after applying a new absolute zero offset (G54-G57
or G159Nx).
As described earlier, only one incremental zero offset may be active; therefore, instructions G58
and G59 are incompatible with G158. This way, the last incremental zero offset programmed
cancels the incremental zero offset that is currently active.
Programming the G158 function alone in the block or G158 with a 0 value in the axes cancels the
incremental zero offset G158 activated earlier. Those instructions also cancel the incremental zero
offsets G58/G59 that are currently active.
When homing an axis in JOG mode, the incremental zero offset for that axis is canceled.
Function properties:
G158 is modal and incompatible with G53.
On power-up, the CNC assumes the incremental zero offset that was active when the CNC was
turned off. On the other hand, the incremental zero offset is neither affected by functions M02 and
M30 nor by RESETTING the CNC.
Display in the zero offset table:
In ISO mode and conversational mode, the zero offset table is one line over the the G54 position
where it identifies the G158 with its values X, Y, Z, etc.
REFERENCE SYSTEMS
An incremental zero offset, by itself, does not cause any axis movement.
Coordinate preset and zero offsets
4.
Considerations:
This line cannot be modified from the table, it can only be modified by programming G158.
Function G159
To apply any zero offset defined in the table.
The first six zero offsets are the same as programming G54 through G59, except that the values
of G58 and G59 are absolute. This is because function G159 cancels functions G54 through G57
and, consequently, there is no active zero offset to add the G58 or G59 to.
Function G159 is programmed as follows:
G159 Nn
Where n is a number from 1 to 20 that indicates the number of the zero offset being
applied.
Function G159 is modal, it is programmed alone in the block and is incompatible with functions G53,
G54, G55, G56, G57, G58, G59 and G92.
On power-up, the CNC assumes the zero offset that was active when the CNC was turned off. On
the other hand, the zero offset is neither affected by functions M02 and M30 nor by RESET.
This function is displayed in the history like G159Nn where the n is the active zero offset.
Examples:
G159 N1
It applies the first zero offset. It is the same as programming G54.
G159 N6
It applies the sixth zero offset. It is the same as programming G59, but it is applied
in absolute.
G159 N20
It applies the 20th zero offset.
CNC 8037
·M· MODEL
SOFT: V02.2X
·59·
Prog ramm in g man u a l
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.
4.
Polar origin preset (G93)
REFERENCE SYSTEMS
Example, assuming that the tool is at X0 Y0
G93
G90
G01
I35
J30
; Preset P3 as polar origin.
R25
Q0
; Point P1, in a straight line (G01).
Q90
; Point P2, in arc (G03).
Y0
; Point P0, in a straight line (G01)
G03
G01
X0
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.
i
CNC 8037
·M· MODEL
SOFT: V02.2X
·60·
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
5
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 8037
·M· MODEL
SOFT: V02.2X
·61·
Prog ramm in g man u a l
5.1
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.
5.
Preparatory functions
ISO CODE PROGRAMMING
Function
M
D
V
*
?
*
Rapid traverse
6.1
G01
*
?
*
Linear interpolation
6.2
G02
*
*
Clockwise circular (helical) interpolation
6.3 / 6.7
G03
*
*
Counterclockwise circular (helical) interpolation
6.3 / 6.7
Dwell/interruption of block preparation
7.1 / 7.2
G04
G05
*
?
*
Round corner
*
Circle center in absolute coordinates
G08
*
Arc tangent to previous path
6.5
G09
*
Arc defined by three points
6.6
G06
G07
*
G10
*
G11
*
?
Square corner
*
*
6.4
7.3.1
Mirror image cancellation
7.5
Mirror image on X axis
7.5
*
*
Mirror image on Y axis
7.5
G13
*
*
Mirror image on Z axis
7.5
G14
*
*
Mirror image in the programmed directions
7.5
G15
*
*
Longitudinal axis selection
8.2
G16
*
*
Main plane selection by two addresses and longitudinal axis
3.2
G17
*
?
*
Main plane X-Y and longitudinal Z
3.2
G18
*
?
*
Main plane Z-X and longitudinal Y
3.2
G19
*
*
Main plane Y-Z and longitudinal X
3.2
G20
Definition of lower work zone limits
3.7.1
G21
Definition of upper work zone limits.
3.7.1
Enable/disable work zones.
3.7.2
*
G32
*
*
Feedrate "F" as an inverted function of time.
6.15
G33
*
*
Electronic threading
6.12
Variable-pitch threading
6.13
G36
*
Corner rounding
6.10
G37
*
Tangential entry
6.8
G38
*
Tangential exit
6.9
G39
*
Chamfer
6.11
Cancellation of tool radius compensation
8.1
G40
·62·
7.3.2
G12
G34
·M· MODEL
SOFT: V02.2X
Section
G00
G22
CNC 8037
Meaning
*
*
G41
*
*
Left-hand tool radius compensation
8.1
G41 N
*
*
Collision detection
8.3
G42
*
*
Right-hand tool radius compensation
8.1
G42 N
*
*
Collision detection
8.3
G43
*
?
*
Tool length compensation
8.2
G44
*
?
G50
*
*
Controlled corner rounding
G51
*
*
Look-Ahead
7.4
6.14
Cancellation of tool length compensation
G52
*
Movement until making contact
G53
*
Programming with respect to machine zero
8.2
7.3.3
4.3
G54
*
*
Absolute zero offset 1
4.4.2
G55
*
*
Absolute zero offset 2
4.4.2
G56
*
*
Absolute zero offset 3
4.4.2
G57
*
*
Absolute zero offset 4
4.4.2
G58
*
*
Additive zero offset 1
4.4.2
G59
*
*
Additive zero offset 2
4.4.2
P r o gr a m m i ng m a n u a l
D
V
Meaning
Section
G60
*
Multiple machining in a straight line
10.1
G61
*
Multiple machining in rectangular pattern
10.2
I*
*
Grid pattern canned cycle
10.3
G63
*
Multiple machining in a circular pattern
10.4
G64
*
Multiple machining in an arc
10.5
G65
*
Machining programmed with an arc-chord
10.6
*
Drilling canned cycle with variable peck
9.6
*
Programming in inches
3.3
Programming in millimeters
3.3
G69
*
G70
*
?
G71
*
?
G72
*
*
General and specific scaling factor
7.6
G73
*
*
Rotation of the coordinate system
7.7
*
Machine reference (home) search
4.2
11.1
G74
G75
*
Probing move until touching
G76
*
Probing move while touching
11.1
Canned cycle parameter modification
9.2.1
G79
G80
*
Canned cycle cancellation
9.3
G81
*
*
*
Drilling canned cycle
9.7
G82
*
*
Drilling canned cycle with dwell
9.8
G83
*
*
Deep-hole drilling canned cycle with constant peck
9.9
G84
*
*
Tapping canned cycle
9.10
G85
*
*
Reaming canned cycle
9.11
G86
*
*
Boring canned cycle with withdrawal in G00
9.12
G87
*
*
Rectangular pocket canned cycle.
9.13
G88
*
*
Circular pocket canned cycle
9.14
G89
*
*
Boring canned cycle with withdrawal in G01
9.15
G90
*
?
Absolute programming:
3.4
G91
*
?
*
G92
Incremental programming
Coordinate preset / spindle speed limit
G93
Polar origin preset
3.4
4.4.1
4.5
G94
*
?
G95
*
?
G96
*
G97
*
*
G98
*
*
Withdrawal to the starting plane at the end of the canned cycle
9.5
G99
*
G159
*
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
*
5.
Preparatory functions
M
ISO CODE PROGRAMMING
Function
Withdrawal to the reference plane at the end of the canned cycle
9.5
Absolute zero offsets
4.4
G210
*
*
Bore milling canned cycle
9.16
G211
*
*
Inside thread milling canned cycle.
9.17
G212
*
*
Outside thread milling canned cycle.
9.18
M means modal, i.e. the G function, once programmed, remains active until another incompatible
G function is 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.
CNC 8037
The letter V means that the G code is displayed next to the current machining conditions in the
execution and simulation modes.
·M· MODEL
SOFT: V02.2X
·63·
Prog ramm in g man u a l
5.2
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.
Feedrate F
ISO CODE PROGRAMMING
5.
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 8037
·M· MODEL
SOFT: V02.2X
·64·
P r o gr a m m i ng m a n u a l
Feedrate in mm/min or inches/min (G94)
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 moving axis is rotary, the CNC interprets that the programmed feedrate is in degrees/minute.
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.
Feedrate F x Movement of axis
Feedrate component =
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:
Feedrate F
5.
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
5.2.1
F  x
10000  100
Fx = ----------------------------------------------------------- = ------------------------------------------------ = 3464 7946
 x  2 +  y  2 +  c  2
100 2 + 20 2 + 270 2
10000  20
F  y
Fy = ----------------------------------------------------------- = ------------------------------------------------ = 692 9589
2
2
2
100 2 + 20 2 + 270 2
 x  +  y  +  c 
F  c
10000  270
Fc = ----------------------------------------------------------- = ------------------------------------------------ = 9354 9455
2
2
2
 x  +  y  +  c 
100 2 + 20 2 + 270 2
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 8037
·M· MODEL
SOFT: V02.2X
·65·
Prog ramm in g man u a l
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.
Feedrate F
ISO CODE PROGRAMMING
5.
CNC 8037
·M· MODEL
SOFT: V02.2X
·66·
P r o gr a m m i ng m a n u a l
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.
Feedrate F
5.
On power-up, after executing M02, M30 or following EMERGENCY or RESET, the CNC assumes
function G97.
ISO CODE PROGRAMMING
5.2.3
CNC 8037
·M· MODEL
SOFT: V02.2X
·67·
Prog ramm in g man u a l
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.
Feedrate F
ISO CODE PROGRAMMING
5.
CNC 8037
·M· MODEL
SOFT: V02.2X
·68·
P r o gr a m m i ng m a n u a l
Spindle turning speed (S)
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.
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.
5.
Spindle turning speed (S)
This speed variation is made between the maximum and minimum values established by spindle
machine parameters "MINSOVR" and "MAXSOVR".
ISO CODE PROGRAMMING
5.3
CNC 8037
·M· MODEL
SOFT: V02.2X
·69·
Prog ramm in g man u a l
5.4
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
5.
ISO CODE PROGRAMMING
Tool number (T) and tool offset (D)
Magazine?
EZ
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.
YES
Selects the tool
YES
D?
If the "D" function has not be defined, it looks up the "Tool table"
to know the "D" offset associated with it.
EZ
The CNC takes the D
associated with the T in the
tool table
It examines the "tool offset table" and assumes the tool
dimensions corresponding to the "D" offset.
The CNC takes the
dimensions defined for the D
in the tool offset table
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.
T3
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.
Tool length and radius compensation.
The CNC looks up the "tool offset table" and assumes the tool dimensions corresponding to the
active "D" offset.
CNC 8037
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.
·M· MODEL
SOFT: V02.2X
·70·
For further information, refer to chapter 8 "tool compensation" in this manual..
P r o gr a m m i ng m a n u a l
5.5
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:
• 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.
ISO CODE PROGRAMMING
• The number of the subroutine which is required to associate to this miscellaneous function.
Auxiliary function (M)
5.
• The number (0-9999) of the defined miscellaneous M function.
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.
i
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 8037
·M· MODEL
SOFT: V02.2X
·71·
Prog ramm in g man u a l
5.5.1
M00. Program stop
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.
Auxiliary function (M)
ISO CODE PROGRAMMING
5.
CNC 8037
·M· MODEL
SOFT: V02.2X
·72·
5.5.2
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).
P r o gr a m m i ng m a n u a l
5.5.3
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.
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.
Auxiliary function (M)
5.5.4
ISO CODE PROGRAMMING
5.
CNC 8037
·M· MODEL
SOFT: V02.2X
·73·
Prog ramm in g man u a l
5.5.5
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.
Auxiliary function (M)
ISO CODE PROGRAMMING
5.
CNC 8037
·M· MODEL
SOFT: V02.2X
·74·
5.5.6
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.
P r o gr a m m i ng m a n u a l
5.5.7
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.
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.
The functions T and M06 may be programmed in the same block, regardless if they have an
associated subroutine or not. In a block where the functions T and M06 are programmed, nothing
else may be programmed.
Auxiliary function (M)
5.
M06. Tool change code
ISO CODE PROGRAMMING
5.5.8
CNC 8037
·M· MODEL
SOFT: V02.2X
·75·
Prog ramm in g man u a l
5.5.9
M19. Spindle orientation
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:
5.
Auxiliary function (M)
ISO CODE PROGRAMMING
• 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 "I0".
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.
i
CNC 8037
·M· MODEL
SOFT: V02.2X
·76·
During the M19 process the screen will display the warning: “M19 in execution"
P r o gr a m m i ng m a n u a l
5.5.10
M41, M42, M43, M44. Spindle gear change
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.
Auxiliary function (M)
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.
5.
ISO CODE PROGRAMMING
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 velocity
command value assigned to machine parameter "MAXVOLT" corresponds to the maximum speed
indicated for each one of the speed ranges (machine parameters "MAXGEAR1" thru
"MAXGEAR4").
CNC 8037
·M· MODEL
SOFT: V02.2X
·77·
Prog ramm in g man u a l
Auxiliary function (M)
ISO CODE PROGRAMMING
5.
CNC 8037
·M· MODEL
SOFT: V02.2X
·78·
PATH CONTROL
6
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
CNC 8037
·M· MODEL
SOFT: V02.2X
·79·
Prog ramm in g man u a l
6.1
Rapid traverse (G00)
The movements programmed after the G00 are executed using the rapid feedrate found in the
machine axis 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.
PATH CONTROL
Rapid traverse (G00)
6.
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 8037
·M· MODEL
SOFT: V02.2X
·80·
P r o gr a m m i ng m a n u a l
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.
Linear interpolation (G01)
6.
PATH CONTROL
6.2
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 8037
·M· MODEL
SOFT: V02.2X
·81·
Prog ramm in g man u a l
6.3
Circular interpolation (G02, G03)
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)
6.
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·82·
Axes X, U, A
==>
I
Axes Y, V, B
==>
J
Axes Z, W, C
==>
K
Programming format:
Plane XY:
G02(G03)
X±5.5
Y±5.5
I±6.5
J±6.5
Plane ZX:
G02(G03)
X±5.5
Z±5.5
I±6.5
K±6.5
Plane YZ:
G02(G03)
Y±5.5
Z±5.5
J±6.5
K±6.5
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±6.5
I±6.5
Plane XU:
G02(G03)
X±5.5
U±5.5
I±6.5
I±6.5
P r o gr a m m i ng m a n u a l
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:
I
Axes Y, V, B
==>
J
Axes Z, W, C
==>
K
6.
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:
G02(G03)
Q±5.5
I±6.5
J±6.5
Plane ZX:
G02(G03)
Q±5.5
I±6.5
K±6.5
Plane YZ:
G02(G03)
Q±5.5
J±6.5
K±6.5
Cartesian coordinates with radius programming
Circular interpolation (G02, G03)
==>
PATH CONTROL
Axes X, U, A
The coordinates of the endpoint of the arc and radius R are defined.
Programming format:
Plane XY:
G02(G03)
X±5.5
Y±5.5
R±6.5
Plane ZX:
G02(G03)
X±5.5
Z±5.5
R±6.5
Plane YZ:
G02(G03)
Y±5.5
Z±5.5
R±6.5
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 8037
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- ..
·M· MODEL
SOFT: V02.2X
·83·
Prog ramm in g man u a l
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.
In all these programming cases, the CNC checks that the center or radius coordinates do not exceed
214748.3647mm. Otherwise, the CNC will display the corresponding error.
PATH CONTROL
Circular interpolation (G02, G03)
6.
CNC 8037
·M· MODEL
SOFT: V02.2X
·84·
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.
P r o gr a m m i ng m a n u a l
Programming examples
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
Circular interpolation (G02, G03)
Various programming modes are analyzed below, point X60 Y40 being the starting point.
PATH CONTROL
6.
or:
G93 I60 J90
G03 Q0
G93 I160 J90
Q-90
; defines polar center
; defines new polar center
Cartesian coordinates with radius programming:
G90 G17 G03 X110 Y90 R50
X160 Y40 R50
CNC 8037
·M· MODEL
SOFT: V02.2X
·85·
Prog ramm in g man u a l
Programming of a (complete) circle in just one block:
PATH CONTROL
Circular interpolation (G02, G03)
6.
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
G02 Q360
; defines polar center
Cartesian coordinates with radius programming:
A complete circle cannot be programmed as there is an infinite range of solutions.
CNC 8037
·M· MODEL
SOFT: V02.2X
·86·
P r o gr a m m i ng m a n u a l
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.
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
Circular interpolation with absolute arc center coordinates (G06)
6.
PATH CONTROL
6.4
CNC 8037
·M· MODEL
SOFT: V02.2X
·87·
Prog ramm in g man u a l
6.5
Arc tangent to previous path (G08)
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)
6.
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
; Arc tangent to previous path.
G08 X110 Y60
; 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 8037
·M· MODEL
SOFT: V02.2X
·88·
P r o gr a m m i ng m a n u a l
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:
==>
I
Axes Y, V, B
==>
J
Axes Z, W, C
==>
K
6.
In Cartesian coordinates:
G17
G09
X±5.5
Y±5.5
I±5.5
J±5.5
G09
R±5.5
Q±5.5
I±5.5
J±5.5
Polar coordinates:
G17
Example:
Arc defined by three points (G09)
Axes X, U, A
PATH CONTROL
6.6
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.
Function G09 may not be used to programmed a full circle because all three points must be different.
The CNC displays the corresponding error code.
CNC 8037
·M· MODEL
SOFT: V02.2X
·89·
Prog ramm in g man u a l
6.7
Helical interpolation
A helical interpolation consists in a circular interpolation in the work plane while moving the rest of
the programmed axes.
PATH CONTROL
Helical interpolation
6.
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
G02
G03
G08
G09
XYIJZ
XYRZA
QIJAB
XYZ
XYIJZ
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
G02
G03
G08
G09
XYIJZK
XYRZK
QIJAI
XYBJ
XYIJZK
Example:
Z
Programming a helical interpolation
where the starting point is X0 Y0 Z0.
Y
(X, Y)
As the example shows, it is not necessary
to program the last point (X, Y):
Z=18
G03 I15 J0 Z18 K5
5
X
CNC 8037
15
·M· MODEL
SOFT: V02.2X
·90·
It is now possible to program helical interpolations while Look Ahead is active (G51). Thanks to this,
CAN/CAM programs that contain this type of paths may be executed while look-ahead is active.
P r o gr a m m i ng m a n u a l
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
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:
Tangential entry at the beginning of a machining operation (G37)
6.
PATH CONTROL
6.8
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.
CNC 8037
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.
·M· MODEL
SOFT: V02.2X
·91·
Prog ramm in g man u a l
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)
6.
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
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
CNC 8037
·M· MODEL
SOFT: V02.2X
·92·
P r o gr a m m i ng m a n u a l
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.
G90 G01 G36 R5 X35 Y60
X50 Y0
Automatic radius blend (G36)
6.
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.
PATH CONTROL
6.10
G90 G03 G36 R5 X50 Y50 I0 J30
G01 X50 Y0
CNC 8037
·M· MODEL
SOFT: V02.2X
·93·
Prog ramm in g man u a l
6.11
Chamfer (G39)
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.
Chamfer (G39)
PATH CONTROL
6.
CNC 8037
·M· MODEL
SOFT: V02.2X
·94·
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
P r o gr a m m i ng m a n u a l
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
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, if s.m.p. M19TYPE (P43) =0, and before making the servo-driven
thread, the CNC references the spindle (home search).
6.
Threading (G33)
X...C ±5.5
PATH CONTROL
6.12
Spindle machine parameter M19TYPE (P43) must be set to "1" in order to be able to program
parameter Q (angular spindle position).
When executing function G33 Q (s.m.p. M19TYPE (P43) =1), and before executing the thread, a
home search must be made for the spindle after the last power-up.
When executing function G33 Q (s.m.p. M19TYPE (P43) =1), and the s.m.p. DECINPUT (P31) =NO,
a home search is not needed for the spindle, since the CNC will be homed automatically after powerup when turning the spindle in M3 or in M4 for the first time.
This search will be carried out at the feedrate set by s.m.p. REFEED2 (P35). After finding home,
the spindle will speed up or slow down to the programmed speed without stopping.
If the spindle has motor feedback with a SINCOS encoder (without reference mark), the home
search will be done directly at the programmed S speed without going through the speed set by
s.m.p. REFEED2.
If after power-up, an M19 is executed before an M3 or M4, that M19 will be executed without homing
the spindle when executing the first M3 or M4.
If the feedback device does not have the reference mark synchronized, the home search in M3 might
not coincide with the home search in M4. This does not happen with FAGOR feedback.
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·95·
Prog ramm in g man u a l
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.
Threading (G33)
PATH CONTROL
6.
CNC 8037
·M· MODEL
SOFT: V02.2X
·96·
G90 G0 X Y Z
; Positioning
G33 Z -100 L5
; Threading
M19
; Spindle orientation
G00 X3
; Cutter withdrawal
Z30
; Withdrawal (exit the hole)
P r o gr a m m i ng m a n u a l
Variable pitch threads (G34)
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
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 references 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".
6.
Variable pitch threads (G34)
X...C ±5.5
PATH CONTROL
6.13
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.
Blending two variable-pitch threads (G34).
Two variable-pitch threads (G34) cannot be blended together.
CNC 8037
·M· MODEL
SOFT: V02.2X
·97·
Prog ramm in g man u a l
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.
6.
PATH CONTROL
Move to hardstop (G52)
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·98·
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.
P r o gr a m m i ng m a n u a l
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.
"F" units: 1/min
Example: G32 X22 F4
indicates that the movement must be executed in 1/4 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".
Feedrate "F" as an inverted function of time (G32)
6.
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.
PATH CONTROL
6.15
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·99·
·100·
PATH CONTROL
Feedrate "F" as an inverted function of time (G32)
Prog ramm in g man u a l
6.
CNC 8037
·M· MODEL
SOFT: V02.2X
ADDITIONAL PREPARATORY
FUNCTIONS
7.1
7
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
/1 G01 X10 Y20
.
.
; Interrupts block preparation
; 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 8037
·M· MODEL
SOFT: V02.2X
·101·
Prog ramm in g man u a l
Example:
The following program blocks are performed in a section with G41 compensation.
...
N10
N15
/1 N17
N20
N30
...
7.
X50 Y80
G04
M10
X50 Y50
X80 Y50
Interruption of block preparation (G04)
ADDITIONAL PREPARATORY FUNCTIONS
Block N15 interrupts block preparation and the execution of block N10 will finish at point A.
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".
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·102·
P r o gr a m m i ng m a n u a l
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 routines.
The PLC routines that require updating the coordinates of the axes of the channel are the following:
• PLC routine using the SWITCH* marks.
• PLC routines where an axis goes into DRO mode and then back into normal axis mode during
the execution of part programs.
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).
If bit 10 of the g.m.p. ADIMPG (P176) =1, with the instruction G04 K0, the coordinates are initialized
and the offset applied with the additive handwheel is eliminated on all the axes that had an offset.
The coordinates will be initialized to the real coordinates of the machine and the offset will be deleted
without moving any machine axis at all.
Interruption of block preparation (G04)
7.
G04 operation:
ADDITIONAL PREPARATORY FUNCTIONS
7.1.1
CNC 8037
·M· MODEL
SOFT: V02.2X
·103·
Prog ramm in g man u a l
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
7.
; Dwell of 50 hundredths of a second (0.5 seconds)
; Dwell of 200 hundredths of a second (2 seconds)
Dwell (G04 K)
ADDITIONAL PREPARATORY FUNCTIONS
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·104·
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 103.
P r o gr a m m i ng m a n u a l
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.
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.
Working with square (G07) and round (G05,G50) corners
G91 G01 G07 Y70 F100
X90
ADDITIONAL PREPARATORY FUNCTIONS
7.
CNC 8037
·M· MODEL
SOFT: V02.2X
·105·
Prog ramm in g man u a l
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.
ADDITIONAL PREPARATORY FUNCTIONS
Working with square (G07) and round (G05,G50) corners
7.
CNC 8037
·M· MODEL
SOFT: V02.2X
·106·
G91 G01 G05 Y70 F100
X90
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.
P r o gr a m m i ng m a n u a l
Controlled round corner (G50)
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.
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.
Working with square (G07) and round (G05,G50) corners
7.
G91 G01 G50 Y70 F100
X90
ADDITIONAL PREPARATORY FUNCTIONS
7.3.3
CNC 8037
·M· MODEL
SOFT: V02.2X
·107·
Prog ramm in g man u a l
7.4
Look-ahead (G51)
Programs consisting of very small movement blocks (CAM, etc.) tend to run very slowly. Those
programs may be executed at high machining speed using the "Look-Ahead" function.
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.
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.
Look-ahead (G51)
ADDITIONAL PREPARATORY FUNCTIONS
7.
Programming format:
The programming format is:
G51 [A] E B
A (0-255)
It 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.
E (5.5)
Maximum contouring error.
The lower this parameter value is, the lower the machining feedrate will be.
B (0-180)
It makes it possible to machine square corners using the Look-ahead function.
It indicates the angular value (in degrees) of the programmed corners, below which,
the machining operation will be carried out in square corner mode.
Block I
Block I+1
B
Parameter "A" permits using a standard working acceleration and another one to be used when
executing with Look-Ahead.
If parameter "B" is not programmed, the square corner management at the corners is canceled.
The square-corner management at the corners is valid for the look-ahead algorithm with jerk
management and for the look-ahead algorithm without jerk management.
Considerations for 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.
CNC 8037
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.
·M· MODEL
SOFT: V02.2X
• 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.
·108·
P r o gr a m m i ng m a n u a l
To prevent motionless blocks from causing a square-corner effect, change bit 0 of general machine
parameter MANTFCON (P189).
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.
G33
Electronic threading (G33)
G34
Variable-pitch threading.
G52
Move to hardstop.
G95
Feedrate per revolution.
Look-ahead (G51)
On the other hand, the CNC will issue Error 7 (Incompatible G functions) when programming any
of the following functions while G51 is active:
7.
ADDITIONAL PREPARATORY FUNCTIONS
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".
CNC 8037
·M· MODEL
SOFT: V02.2X
·109·
Prog ramm in g man u a l
7.4.1
Advanced look-ahead algorithm (integrating Fagor filters)
This mode is indicated when machining accuracy is required, especially if Fagor filters have been
set for the axes by machine parameters.
The advanced look-ahead algorithm calculates the feedrates at the corners so as to take the effect
of those filters into consideration. When programming G51 E, the contouring errors when machining
corners will be closer to the value programmed in that G51 function depending on the filters.
To activate the advanced look-ahead algorithm, use bit 15 of g.m.p. LOOKATYP (P160).
Look-ahead (G51)
ADDITIONAL PREPARATORY FUNCTIONS
7.
Considerations
• If there are no Fagor filters set by machine parameters in the axes of the main channel, activating
the advanced look-ahead algorithm will internally activate FIR filters of the 5th order and a
frequency of 30 Hz in all the axes of the channel.
• If there are Fagor filters set by machine parameters, activating the advanced look-ahead
algorithm will keep the values of those filters as long as their frequency is not higher than 30Hz
If their frequency is higher than 30 Hz, it will assume the values of 5th order and a frequency
of 30 Hz.
If there are several filters defined in the axes of the channel, the one with the lowest frequency
will be assumed as long as it is not higher than 30Hz.
• Even if the advanced look-ahead algorithm (using Fagor filters) is active with bit 15 of g.m.p.
LOOKATYP (P160), it will not start working in the following cases:
 If g.m.p. IPOTIME (P73) = 1.
 If any of the axes of the main channel has a.m.p. SMOTIME (P58) not equal to 0.
 If any of the axes of the main channel has defined by parameter a non-Fagor type filter, a.m.p.
TYPE (P71) not equal to 2.
In these cases, when activating G51, the CNC will issue the corresponding error message.
CNC 8037
·M· MODEL
SOFT: V02.2X
·110·
P r o gr a m m i ng m a n u a l
Look-ahead operation with Fagor filters active
This option makes it possible to use Fagor filters with Look-ahead (not advanced look-ahead
algorithm). It will only be considered if the advanced look-ahead algorithm is deactivated; that is,
if bit 15 of g.m.p. LOOKATYP (P160)=0.
To activate/deactivate this option, use bit 13 of g.m.p. LOOKATYP (P160).
Effect of Fagor filters when machining circles
Programmed movement.
Real (actual) movement using Fagor filters.
Real (actual) movement without using Fagor filters.
7.
Look-ahead (G51)
When machining circles, the error will be smaller when using Fagor filters than without using these
filters:
ADDITIONAL PREPARATORY FUNCTIONS
7.4.2
CNC 8037
·M· MODEL
SOFT: V02.2X
·111·
Prog ramm in g man u a l
7.5
Mirror image (G10, G11. G12, G13, G14)
The functions to activate the mirror image are the following.
7.
G10:
Cancel mirror image.
G11:
Mirror image on X axis.
G12:
Mirror image on the Y axis.
G13:
Mirror image on the Z axis
G14:
Mirror image on any axis (X..C), or in several at the same time.
Mirror image (G10, G11. G12, G13, G14)
ADDITIONAL PREPARATORY FUNCTIONS
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.
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
G11
Execution
G10 G12
Execution
G11
Execution
M30
of subroutine
of subroutine
of subroutine;
of subroutine;
; machines "a"
; Mirror image on X axis.
; machines "b"
; Mirror image on Y axis.
machines "c"
; Mirror image on X and Y axes.
Machines "d"
; End of program
Functions G11, G12, G13, and G14 are modal and incompatible with G10.
CNC 8037
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.
·M· MODEL
SOFT: V02.2X
·112·
On power-up, after executing M02, M30 or after EMERGENCY or RESET, the CNC assumes code
G10.
P r o gr a m m i ng m a n u a l
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 (G72)
7.
• Scaling factor applied to one or more axes.
ADDITIONAL PREPARATORY FUNCTIONS
7.6
CNC 8037
·M· MODEL
SOFT: V02.2X
·113·
Prog ramm in g man u a l
7.6.1
Scaling factor applied to all axes.
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 canceled.
Programming example (starting point X-30 Y10)
Scaling factor (G72)
ADDITIONAL PREPARATORY FUNCTIONS
7.
The following subroutine defines the machining of the part.
G90
G01
G02
G01
X-19 Y0
X0 Y10 F150
X0 Y-10 I0 J-10
X-19 Y0
The programming of the parts would be :
Execution of subroutine Machines "a".
G92 X-79 Y-30
G72 S2
; Coordinate preset
(zero offset)
; Applies a scaling factor of 2
Execution of subroutine Machines "b".
G72 S1
M30
; Cancel the scaling factor
; End of program
Examples of application of the scaling factor.
CNC 8037
·M· MODEL
SOFT: V02.2X
·114·
G90 G00 X0 Y0
N10 G91 G01 X20 Y10
Y10
X-10
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 X-10
X20 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.
P r o gr a m m i ng m a n u a l
7.6.2
Scaling factor applied to one or more axes.
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.
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.
i
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.
ADDITIONAL PREPARATORY FUNCTIONS
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.
Scaling factor (G72)
7.
2. It then applies the scaling factor indicated to the calculated movement of the corresponding axis
or axes.
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 8037
·M· MODEL
SOFT: V02.2X
·115·
Prog ramm in g man u a l
If a scaling factor equal to 360/2R 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.
Scaling factor (G72)
ADDITIONAL PREPARATORY FUNCTIONS
7.
CNC 8037
·M· MODEL
SOFT: V02.2X
·116·
P r o gr a m m i ng m a n u a l
Pattern rotation (G73)
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 rotation angle 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.
7.
Pattern rotation (G73)
Q
ADDITIONAL PREPARATORY FUNCTIONS
7.7
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 8037
·M· MODEL
SOFT: V02.2X
·117·
Prog ramm in g man u a l
Assuming that the starting point is X0 Y0, you get :
Pattern rotation (G73)
ADDITIONAL PREPARATORY FUNCTIONS
7.
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 8037
·M· MODEL
SOFT: V02.2X
·118·
TOOL COMPENSATION
8
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 8037
·M· MODEL
SOFT: V02.2X
·119·
Prog ramm in g man u a l
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.
8.
There are three preparatory functions for tool radius compensation:
TOOL COMPENSATION
Tool radius compensation (G40, G41, G42)
G40: Cancellation of tool radius compensation
G41: Left-hand tool radius compensation.
G42: Tool radius compensation to the right of the part.
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 8037
·M· MODEL
SOFT: V02.2X
·120·
P r o gr a m m i ng m a n u a l
Beginning of tool radius compensation
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: Left-hand tool radius compensation.
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.
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 the compensation without programmed 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.
8.
Tool radius compensation (G40, G41, G42)
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.
TOOL COMPENSATION
8.1.1
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 either linear or circular.
Y
X
Y
X
···
G90
G01 Y40
G91 G40 Y0 Z10
G02 X20 Y20 I20 J0
···
(X0 Y0)
···
G90
G01 X-30 Y30
G01 G41 X-30 Y30 Z10
G01 X25
···
(X0 Y0)
CNC 8037
·M· MODEL
SOFT: V02.2X
·121·
Prog ramm in g man u a l
STRAIGHT-STRAIGHT path
TOOL COMPENSATION
Tool radius compensation (G40, G41, G42)
8.
CNC 8037
·M· MODEL
SOFT: V02.2X
·122·
P r o gr a m m i ng m a n u a l
STRAIGHT-CURVED path
Tool radius compensation (G40, G41, G42)
TOOL COMPENSATION
8.
CNC 8037
·M· MODEL
SOFT: V02.2X
·123·
Prog ramm in g man u a l
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 shown with solid line and the compensated
path with dashed line.
TOOL COMPENSATION
Tool radius compensation (G40, G41, G42)
8.
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·124·
With an angle between paths of up 300º, it calculates the intersection. In the rest of the cases
it is compensated like COMPMODE = 0.
P r o gr a m m i ng m a n u a l
Cancellation of tool radius compensation
Tool radius compensation is canceled 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.
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.
(X0 Y0)
(X0 Y0)
Y
Tool radius compensation (G40, G41, G42)
End of the compensation without programmed movement:
8.
TOOL COMPENSATION
8.1.3
X
Y
X
···
G90
G01 X-30
G01 G40 X-30
G01 X25 Y-25
···
···
G90
G03 X-20 Y-20 I0 J-20
G91 G40 Y0
G01 X-20
···
CNC 8037
·M· MODEL
SOFT: V02.2X
·125·
Prog ramm in g man u a l
STRAIGHT-STRAIGHT path
TOOL COMPENSATION
Tool radius compensation (G40, G41, G42)
8.
CNC 8037
·M· MODEL
SOFT: V02.2X
·126·
P r o gr a m m i ng m a n u a l
CURVED-STRAIGHT path
Tool radius compensation (G40, G41, G42)
TOOL COMPENSATION
8.
CNC 8037
·M· MODEL
SOFT: V02.2X
·127·
Prog ramm in g man u a l
Example of machining with radius compensation:
TOOL COMPENSATION
Tool radius compensation (G40, G41, G42)
8.
CNC 8037
·M· MODEL
SOFT: V02.2X
·128·
The programmed path is shown with solid line and the compensated path with dashed line.
Tool radius
10mm
Tool number
T1
Tool offset number
D1
; 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
P r o gr a m m i ng m a n u a l
Example of machining with radius compensation:
Tool radius
10mm
Tool number
T1
Tool offset number
D1
; 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
Tool radius compensation (G40, G41, G42)
The programmed path is shown with solid line and the compensated path with dashed line.
TOOL COMPENSATION
8.
CNC 8037
·M· MODEL
SOFT: V02.2X
·129·
Prog ramm in g man u a l
Example of machining with radius compensation:
TOOL COMPENSATION
Tool radius compensation (G40, G41, G42)
8.
CNC 8037
·M· MODEL
SOFT: V02.2X
·130·
The programmed path is shown with solid line and the compensated path with dashed line.
Tool radius
10mm
Tool number
T1
Tool offset number
D1
; 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
P r o gr a m m i ng m a n u a l
Change of type of 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 the
following criteria:
A. The compensated paths cut each other.
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:
A
B
Tool radius compensation (G40, G41, G42)
8.
The programmed paths are compensated each on its corresponding side. The side change takes
place in the intersection point between both paths.
TOOL COMPENSATION
8.1.4
Straight - arc path:
A
B
Arc - straight path:
A
B
Arc - arc path:
CNC 8037
A
B
·M· MODEL
SOFT: V02.2X
·131·
Prog ramm in g man u a l
8.2
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
8.
TOOL COMPENSATION
Tool length compensation (G43, G44, G15)
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·132·
P r o gr a m m i ng m a n u a l
Example of machining with tool length compensation:
Tool length
-4mm
Tool number
T1
Tool offset number
D1
; 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
Tool length compensation (G43, G44, G15)
It is assumed that the tool used is 4 mm shorter than the programmed one.
TOOL COMPENSATION
8.
CNC 8037
·M· MODEL
SOFT: V02.2X
·133·
Prog ramm in g man u a l
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)
8.
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: 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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·134·
CANNED CYCLES
9
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
G210
Bore milling canned cycle
G211
Inside thread milling canned cycle.
G212
Outside thread milling canned cycle.
It also offers the following functions that can be used with the machining canned cycles:
G79
Change of 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 8037
·M· MODEL
SOFT: V02.2X
·135·
Prog ramm in g man u a l
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.
9.
CANNED CYCLES
Canned cycle definition
However, once a canned cycle has been defined in a block and following blocks, functions G02, G03,
G08 or G09 can be programmed.
CNC 8037
·M· MODEL
SOFT: V02.2X
·136·
P r o gr a m m i ng m a n u a l
Influence zone of a canned cycle
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, 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...
Definition and execution of the canned cycle (drilling).
G90 G1 X100
The X axis moves to X100, where the hole is to be drilled.
G91 X10 N3
The CNC runs the following operation 3 times.
Influence zone of a canned cycle
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.
9.
CANNED CYCLES
9.2
• Incremental move to X10.
• Runs the cycle defined above.
G91 X20 N0
Incremental move only to X20 (no drilling).
CNC 8037
·M· MODEL
SOFT: V02.2X
·137·
Prog ramm in g man u a l
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.
9.
CANNED CYCLES
Influence zone of a canned cycle
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:
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
CNC 8037
·M· MODEL
SOFT: V02.2X
·138·
P r o gr a m m i ng m a n u a l
Influence zone of a canned cycle
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
CANNED CYCLES
9.
CNC 8037
·M· MODEL
SOFT: V02.2X
·139·
Prog ramm in g man u a l
9.3
Canned cycle cancellation
A canned cycle can be canceled 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
9.
CNC 8037
·M· MODEL
SOFT: V02.2X
·140·
P r o gr a m m i ng m a n u a l
Some general points to consider
• 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 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.
9.
Some general points to consider
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.
CANNED CYCLES
9.4
CNC 8037
·M· MODEL
SOFT: V02.2X
·141·
Prog ramm in g man u a l
9.5
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.
CANNED CYCLES
Machining canned cycles
9.
• 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: Selects the withdrawal of the tool as far as the initial plane, once the indicated machining
has been done.
• G99: 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
FSTDM
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:
CNC 8037
·M· MODEL
SOFT: V02.2X
·142·
P r o gr a m m i ng m a n u a l
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 along
the longitudinal axis.
The following examples show how to drill in X and Y in both directions.
Function G81 defines the drilling canned cycle. It is defined with these parameters:
Y
Coordinate of the point to be machined along the ordinate axis.
I
Drilling depth.
K
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
9.
Machining canned cycles
Coordinate of the point to be machined along the abscissa axis.
CANNED CYCLES
X
Example 2:
G19
G1 X-25 F1000 S1000 M3
G81 X25 Y15 Z-2 I8 K1
Example 3:
G18
G1 Y25 F1000 S1000 M3
G81 X30 Y10 Z2 I-8 K1
CNC 8037
·M· MODEL
SOFT: V02.2X
·143·
Prog ramm in g man u a l
Example 4:
G18
G1 Y-25 F1000 S1000 M3
G81 X15 Y60 Z-2 I8 K1
CANNED CYCLES
Machining canned cycles
9.
CNC 8037
·M· MODEL
SOFT: V02.2X
·144·
P r o gr a m m i ng m a n u a l
9.6
G69. Drilling canned cycle with variable peck
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
[ 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.
G69. Drilling canned cycle with variable peck
CANNED CYCLES
9.
[ 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.
[ 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.
CNC 8037
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
·M· MODEL
SOFT: V02.2X
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.
·145·
Prog ramm in g man u a l
[ 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.
CANNED CYCLES
G69. Drilling canned cycle with variable peck
9.
When not programmed or programmed with a "0" value, it returns to the position indicated by H (relief
position) after each drilling peck.
• 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.
[ 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".
[ L5.5 ] Minimum drilling peck (step)
It defines the minimum value for the drilling peck. This paramater is used with "R" values other than
1. If not programmed or programmed with a 0 value, it assumes 1 mm.
[ R5.5 ] 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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·146·
If R is selected with a value other than 1, the CNC will not allow smaller steps than that programmed
in L.
P r o gr a m m i ng m a n u a l
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.
G69. Drilling canned cycle with variable peck
9.
CANNED CYCLES
9.6.1
3. First drilling operation. The drilling axis moves in G01 to the programmed incremental depth "B
+ D".
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.
·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)"
CNC 8037
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.
·M· MODEL
SOFT: V02.2X
·147·
Prog ramm in g man u a l
The first drilling penetration is done in G07 or G50 depending on the value assigned to the parameter
of the longitudinal axis "INPOSW2 (P51)" and to parameter "INPOSW1 (P19)". This is important
to join a drilling operation with another one in multiple drilling so the tool path is faster and smoother.
If INPOSW2 < INPOSW1 in G07 (square corner).
If INPOSW2 >= INPOSW1 in G50 (controlled round corner).
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
9.
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
Tool withdrawal
While machining, the CNC lets withdraw the tool to the starting plane stopping the spindle when
the tool reaches the starting plane.
Activating PLC mark RETRACYC (M5065) stops the main axis and the tool is withdrawn without
stopping the spindle. The spindle stops when the tool is retracted, once it reaches the starting plane.
Options after tool withdrawal
Once the tool has been retracted, the user will have the following options:
• Finish the hole.
• Go to the next hole.
• Go into tool inspection.
After this, the CNC will display the following message:
"To end the cycle, press START to skip to the next SKIPCYCL".
Finish the hole:
To finish the hole, press the [START] key.
CNC 8037
It goes down in G0 with spindle running to 1 mm before the coordinate where the hole stopped. From
then on, it continues at the F and S programmed in the cycle.
Go to the next hole:
To go to the next hole, activate the PLC mark SKIPCYCL.
·M· MODEL
SOFT: V02.2X
The CNC will display the following message:
"Press [START] to continue".
Pressing the [START] key, the CNC considers the cycle to be finished and continues with the next
block.
·148·
P r o gr a m m i ng m a n u a l
Go into tool inspection:
If you don't wish to finish the hole nor go to the next hole, it is possible to go into a standard tool
inspection.
In this case, a block must be selected and a standard repositioning must be done before resuming
the execution of the program.
After inspecting the tool, once repositioning is done, the following choices will be offered:
• Resume the interrupted cycle.
CANNED CYCLES
G69. Drilling canned cycle with variable peck
9.
• Skip the interrupted cycle and resume at the next block.
CNC 8037
·M· MODEL
SOFT: V02.2X
·149·
Prog ramm in g man u a l
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
9.
[ 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 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".
CNC 8037
·M· MODEL
SOFT: V02.2X
·150·
P r o gr a m m i ng m a n u a l
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.
3. Drill the hole. Movement of the longitudinal axis at work feedrate, to the bottom of the hole
programmed in "I".
4. Dwell K, in hundredths of a second, if it 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:
; 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
G81. Drilling canned cycle
9.
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.
CANNED CYCLES
9.7.1
CNC 8037
·M· MODEL
SOFT: V02.2X
·151·
Prog ramm in g man u a l
Tool withdrawal
While machining, the CNC lets withdraw the tool to the starting plane stopping the spindle when
the tool reaches the starting plane.
Activating PLC mark RETRACYC (M5065) stops the main axis and the tool is withdrawn without
stopping the spindle. The spindle stops when the tool is retracted, once it reaches the starting plane.
9.
CANNED CYCLES
G81. Drilling canned cycle
Options after tool withdrawal
Once the tool has been retracted, the user will have the following options:
• Finish the hole.
• Go to the next hole.
• Go into tool inspection.
After this, the CNC will display the following message:
"To end the cycle, press START to skip to the next SKIPCYCL".
Finish the hole:
To finish the hole, press the [START] key.
It goes down in G0 with spindle running to 1 mm before the coordinate where the hole stopped. From
then on, it continues at the F and S programmed in the cycle.
Go to the next hole:
To go to the next hole, activate the PLC mark SKIPCYCL.
The CNC will display the following message:
"Press [START] to continue".
Pressing the [START] key, the CNC considers the cycle to be finished and continues with the next
block.
Go into tool inspection
If you don't wish to finish the hole nor go to the next hole, it is possible to go into a standard tool
inspection.
In this case, a block must be selected and a standard repositioning must be done before resuming
the execution of the program.
After inspecting the tool, once repositioning is done, the following choices will be offered:
• Resume the interrupted cycle.
• Skip the interrupted cycle and resume at the next block.
CNC 8037
·M· MODEL
SOFT: V02.2X
·152·
P r o gr a m m i ng m a n u a l
9.8
G82. Drilling canned 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
[ 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.
G82. Drilling canned cycle with dwell
CANNED CYCLES
9.
[ 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 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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·153·
Prog ramm in g man u a l
9.8.1
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.
3. Drill the hole. Movement of the longitudinal axis at work feedrate, to the bottom of the hole
programmed in "I".
4. Dwell time K in hundredths of a second.
9.
CANNED CYCLES
G82. Drilling canned cycle with dwell
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.
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. 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 8037
Tool withdrawal
·M· MODEL
SOFT: V02.2X
·154·
While machining, the CNC lets withdraw the tool to the starting plane stopping the spindle when
the tool reaches the starting plane.
Activating PLC mark RETRACYC (M5065) stops the main axis and the tool is withdrawn without
stopping the spindle. The spindle stops when the tool is retracted, once it reaches the starting plane.
P r o gr a m m i ng m a n u a l
Options after tool withdrawal
Once the tool has been retracted, the user will have the following options:
• Finish the hole.
• Go to the next hole.
• Go into tool inspection.
After this, the CNC will display the following message:
To finish the hole, press the [START] key.
It goes down in G0 with spindle running to 1 mm before the coordinate where the hole stopped. From
then on, it continues at the F and S programmed in the cycle.
Go to the next hole:
To go to the next hole, activate the PLC mark SKIPCYCL.
The CNC will display the following message:
"Press [START] to continue".
Pressing the [START] key, the CNC considers the cycle to be finished and continues with the next
block.
CANNED CYCLES
Finish the hole:
G82. Drilling canned cycle with dwell
9.
"To end the cycle, press START to skip to the next SKIPCYCL".
Go into tool inspection
If you don't wish to finish the hole nor go to the next hole, it is possible to go into a standard tool
inspection.
In this case, a block must be selected and a standard repositioning must be done before resuming
the execution of the program.
After inspecting the tool, once repositioning is done, the following choices will be offered:
• Resume the interrupted cycle.
• Skip the interrupted cycle and resume at the next block.
CNC 8037
·M· MODEL
SOFT: V02.2X
·155·
Prog ramm in g man u a l
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
9.
[ 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 ] Depth of each drilling peck
Defines the value of each drilling step according to the axis longitudinal to the main plane.
CNC 8037
·M· MODEL
SOFT: V02.2X
·156·
P r o gr a m m i ng m a n u a l
[ J4 ] 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.
G83. Deep-hole drilling canned cycle with constant peck
CANNED CYCLES
9.
CNC 8037
·M· MODEL
SOFT: V02.2X
·157·
Prog ramm in g man u a l
9.9.1
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.
3. First drilling operation. The longitudinal axis moves in G01 to the programmed incremental depth
"I".
4. Drilling loop. The following steps will be repeated "J-1" times as in the previous step the first
programmed drilling was done.
9.
CANNED CYCLES
G83. Deep-hole drilling canned cycle with constant peck
·1·Withdrawal of the longitudinal axis in rapid (G00) to the reference plane.
CNC 8037
·M· MODEL
SOFT: V02.2X
·158·
·2·Longitudinal axis approach in rapid (G00):
If INPOSW2 < INPOSW1, down to 1mm off the previous drilling peck.
If not, down to twice the value of INPOSW2.
·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.
The first drilling penetration is done in G07 or G50 depending on the value assigned to the parameter
of the longitudinal axis "INPOSW2 (P51)" and to parameter "INPOSW1 (P19)". This is important
to join a drilling operation with another one in multiple drilling so the tool path is faster and smoother.
If INPOSW2 < INPOSW1 in G07 (square corner).
If INPOSW2 >= INPOSW1 in G50 (controlled round corner).
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:
P r o gr a m m i ng m a n u a l
While machining, the CNC lets withdraw the tool to the starting plane stopping the spindle when
the tool reaches the starting plane.
Activating PLC mark RETRACYC (M5065) stops the main axis and the tool is withdrawn without
stopping the spindle. The spindle stops when the tool is retracted, once it reaches the starting plane.
Options after tool withdrawal
Once the tool has been retracted, the user will have the following options:
• Finish the hole.
G83. Deep-hole drilling canned cycle with constant peck
Tool withdrawal
9.
CANNED CYCLES
; 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
• Go to the next hole.
• Go into tool inspection.
After this, the CNC will display the following message:
"To end the cycle, press START to skip to the next SKIPCYCL".
Finish the hole:
To finish the hole, press the [START] key.
It goes down in G0 with spindle running to 1 mm before the coordinate where the hole stopped. From
then on, it continues at the F and S programmed in the cycle.
Go to the next hole:
To go to the next hole, activate the PLC mark SKIPCYCL.
The CNC will display the following message:
"Press [START] to continue".
Pressing the [START] key, the CNC considers the cycle to be finished and continues with the next
block.
Go into tool inspection
CNC 8037
If you don't wish to finish the hole nor go to the next hole, it is possible to go into a standard tool
inspection.
In this case, a block must be selected and a standard repositioning must be done before resuming
the execution of the program.
After inspecting the tool, once repositioning is done, the following choices will be offered:
·M· MODEL
SOFT: V02.2X
• Resume the interrupted cycle.
• Skip the interrupted cycle and resume at the next block.
·159·
Prog ramm in g man u a l
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.
9.
CANNED CYCLES
G84. Tapping canned cycle
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.
Using parameters B and H, the threading may be done with relief for chip breakage.
The tapping with relief is done in successive approaches until the programmed total depth is
reached. After every approach, it withdraws for chip relief. In this case, the dwell (K) is only applied
on the last pass, not on the relief passes.
Working in Cartesian coordinates, the basic structure of the block is as follows:
G84 G98/G99 X Y Z I K R J B H
[ 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.
[ 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.
CNC 8037
If not programmed, it assumes as reference plane the current position of the tool.
[ I±5.5 ] 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.
·M· MODEL
SOFT: V02.2X
[ K5 ] 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".
·160·
P r o gr a m m i ng m a n u a l
[ R ] Type of tapping
Defines the type of tapping to be carried out.
Regular tapping.
R1
Rigid tapping. The CNC stops the spindle with M19 and orients it to begin tapping.
R1
Rigid tapping. If the spindle is turning in M3 or M4, the CNC does not stop it nor orient
it to begin tapping. This option does not allow thread repair, even if the part has not been
released because the thread start (entry) will coincide with the one machined earlier.
9.
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.
[ B5.5 ] Penetration step during tapping with relief.
It is optional and sets the penetration step during tapping with relief. This parameter is ignored when
programming R=0 or R=2. Tapping with relief is only possible when programming R=1.
CANNED CYCLES
[ J5.5 ] Withdrawal feedrate factor
G84. Tapping canned cycle
R0
When not programmed, tapping will be done in a single pass. When programmed with a 0 value,
it issues the corresponding error.
[ H5.5 ] Withdrawal distance after each penetration step.
This regress will be performed at a rate that takes into account the factor programmed for J. This
parameter will be ignored if R=0 or R=2 is programmed or if parameter B has not been programmed.
If not programmed or programmed with a 0 value, the withdrawal will be done to the Z reference
plane coordinate.
CNC 8037
·M· MODEL
SOFT: V02.2X
·161·
Prog ramm in g man u a l
9.10.1
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.
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.
CANNED CYCLES
G84. Tapping canned cycle
9.
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. The spindle reverses 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 8037
·M· MODEL
SOFT: V02.2X
·162·
P r o gr a m m i ng m a n u a l
While machining, the CNC lets withdraw the tool to the starting plane stopping the spindle when
the tool reaches the starting plane.
G84. Tapping canned cycle
Tool withdrawal
9.
CANNED CYCLES
; 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
Activating PLC mark RETRACYC (M5065) stops the main axis and the spindle, the tool is withdrawn
changing the direction of the axis and spindle while keeping the machining F and S values. This
withdrawal will be to the starting plane.
The stopping and starting sequence of the spindle and the axis when tapping keeps the same
synchronism and dwells as during the execution of the canned cycle.
Options after tool withdrawal
Once the tool has been retracted, the user will have the following options:
• Finish the hole.
• Go to the next hole.
• Go into tool inspection.
After this, the CNC will display the following message:
"To end the cycle, press START to skip to the next SKIPCYCL".
Finish the hole:
To finish the hole, press the [START] key.
The hole is repeated from the starting plane under the same F and S conditions without stopping
at the point where it stopped.
Go to the next hole:
To go to the next hole, activate the PLC mark SKIPCYCL.
The CNC will display the following message:
"Press [START] to continue".
Pressing the [START] key, the CNC considers the cycle to be finished and continues with the next
block.
CNC 8037
·M· MODEL
SOFT: V02.2X
·163·
Prog ramm in g man u a l
Go into tool inspection
If you don't wish to finish the hole nor go to the next hole, it is possible to go into a standard tool
inspection.
In this case, a block must be selected and a standard repositioning must be done before resuming
the execution of the program.
After inspecting the tool, once repositioning is done, the following choices will be offered:
• Resume the interrupted cycle.
9.
CANNED CYCLES
G84. Tapping canned cycle
• Skip the interrupted cycle and resume at the next block.
CNC 8037
·M· MODEL
SOFT: V02.2X
·164·
P r o gr a m m i ng m a n u a l
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
G85. Reaming canned cycle
CANNED CYCLES
9.
[ 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.
[ 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 ] 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".
CNC 8037
·M· MODEL
SOFT: V02.2X
·165·
Prog ramm in g man u a l
9.11.1
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.
3. Movement at the working feedrate (G01) of the longitudinal axis to the bottom of the machined
hole, and reaming.
4. Dwell, if parameter "K" has been programmed.
9.
CANNED CYCLES
G85. Reaming canned cycle
5. Withdrawal at working feedrate, of the longitudinal axis as far as the reference plane.
CNC 8037
·M· MODEL
SOFT: V02.2X
·166·
6. 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:
; 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
P r o gr a m m i ng m a n u a l
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.
After the quail has penetrated, it is possible to orient the spindle and retract the quail before the exit
movement, thus preventing the part from scratching. This is only available when using spindle
orientation.
Working in Cartesian coordinates, the basic structure of the block is as follows:
M03
M04
M03
M04
G98
G99
I
K
M05
CANNED CYCLES
G00
G01
G86. Boring cycle with withdrawal in G00
9.
G86 G98/G99 X Y Z I K Q D E
Q
D
E
[ 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.
[ 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 ] 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.
CNC 8037
[ 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".
[ Q±5.5 ] Spindle position for the withdrawal
·M· MODEL
SOFT: V02.2X
It defines the spindle position, in degrees, to separate the cutter from the wall of the hole.
If not programmed, the withdrawal will be done without separating the cutter from the wall of the
hole, the spindle stopped and in rapid.
·167·
Prog ramm in g man u a l
[ D±5.5 ] Gap between the cutter and the wall of the hole on the X axis
Defines the gap between the cutter and the wall of the hole on the X axis for the withdrawal.
If not programmed, the cutter does not separate from the wall of the hole along the X axis.
Both Q and D must be programmed for the cutter to separate from the wall of the hole.
[ E±5.5 ] Gap between the cutter and the wall of the hole on the Y axis
Defines the gap between the cutter and the wall of the hole on the Y axis for the withdrawal.
9.
If not programmed, the cutter does not separate from the wall of the hole along the Y axis.
CANNED CYCLES
G86. Boring cycle with withdrawal in G00
Both Q and E must be programmed for the cutter to separate from the wall of the hole.
CNC 8037
·M· MODEL
SOFT: V02.2X
·168·
P r o gr a m m i ng m a n u a l
9.12.1
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.
3. Movement at the working feedrate (G01) of the longitudinal axis to the bottom of the machined
hole, and boring.
4. Dwell, if parameter "K" has been programmed.
7. Tool withdrawal, in rapid (G00), to the starting plane or to the reference plane depending on
whether G98 or G99 has been programmed.
8. Tool movement, in a rapid interpolated movement, the distances programmed in parameters D
and E with opposite signs (undoing the movement made in step 6).
9. When done with the withdrawal, the spindle will start in the same direction as it was turning
before.
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.
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
CANNED CYCLES
6. The movement of the tool, for interpolated movements and slow feedrates, the distances
programmed for the parameters D and E. If the values are not programmed correctly it could
cause the blade to collide with the wall instead of pulling away from it.
G86. Boring cycle with withdrawal in G00
9.
5. Spindle orientation to the position programmed in parameter Q.
CNC 8037
·M· MODEL
SOFT: V02.2X
·169·
Prog ramm in g man u a l
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.
9.
Working in Cartesian coordinates, the basic structure of the block is as follows:
CANNED CYCLES
G87. Rectangular pocket canned cycle.
G87 G98/G99 X Y Z I J K B C D H L V
[ 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.
[ 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.
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·170·
P r o gr a m m i ng m a n u a l
[ I±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.).
[ J±5.5 ] 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.
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.
G87. Rectangular pocket canned cycle.
CANNED CYCLES
9.
[ 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.
[ 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.
CNC 8037
·M· MODEL
SOFT: V02.2X
If not programmed, it assumes a value of 3/4 of the diameter of the selected tool.
·171·
Prog ramm in g man u a l
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.
[ D5.5 ] 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
G87. Rectangular pocket canned cycle.
9.
[ 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.
[ L±5.5 ] 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).
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 8037
·M· MODEL
SOFT: V02.2X
·172·
P r o gr a m m i ng m a n u a l
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.
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.
G87. Rectangular pocket canned cycle.
9.
5. Finishing pass milling, "L" at the work feedrate defined by "H".
CANNED CYCLES
9.13.1
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 8037
·M· MODEL
SOFT: V02.2X
·173·
Prog ramm in g man u a l
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
G87. Rectangular pocket canned cycle.
9.
; 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 8037
·M· MODEL
SOFT: V02.2X
·174·
P r o gr a m m i ng m a n u a l
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.
; 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
G87. Rectangular pocket canned cycle.
CANNED CYCLES
9.
CNC 8037
·M· MODEL
SOFT: V02.2X
·175·
Prog ramm in g man u a l
9.14
G88. Circular pocket canned cycle
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
9.
[ 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.
[ 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 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 8037
·M· MODEL
SOFT: V02.2X
·176·
P r o gr a m m i ng m a n u a l
[ J±5.5 ] Pocket radius
Defines the radius of the pocket. The sign indicates the pocket machining direction.
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.
G88. Circular pocket canned cycle
J with "+" sign
CANNED CYCLES
9.
[ 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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·177·
Prog ramm in g man u a l
[ D5.5 ] 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
9.
[ H5.5 ] 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.
[ L5.5 ] 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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·178·
P r o gr a m m i ng m a n u a l
[ 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).
G88. Circular pocket canned cycle
CANNED CYCLES
9.
CNC 8037
·M· MODEL
SOFT: V02.2X
·179·
Prog ramm in g man u a l
9.14.1
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.
9.
CANNED CYCLES
G88. Circular pocket canned cycle
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.
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 8037
·M· MODEL
SOFT: V02.2X
·180·
P r o gr a m m i ng m a n u a l
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.
G88. Circular pocket canned cycle
CANNED CYCLES
9.
; 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
CNC 8037
·M· MODEL
SOFT: V02.2X
·181·
Prog ramm in g man u a l
9.15
G89. Boring cycle with withdrawal at work feedrate (G01)
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:
G89 G98/G99 X Y Z I K
CANNED CYCLES
G89. Boring cycle with withdrawal at work feedrate (G01)
9.
[ 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.
[ 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 ] 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 8037
·M· MODEL
SOFT: V02.2X
·182·
P r o gr a m m i ng m a n u a l
9.15.1
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.
3. Movement at the working feedrate (G01) of the longitudinal axis to the bottom of the machined
hole, and boring.
4. Dwell, if parameter "K" has been programmed.
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.
; 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
CANNED CYCLES
Programming example ·1·
G89. Boring cycle with withdrawal at work feedrate (G01)
9.
5. Withdrawal at working feedrate, of the longitudinal axis as far as the reference plane.
6. Withdrawal, at rapid feedrate (G00), of the longitudinal axis as far as the initial plane if G98 has
been programmed.
CNC 8037
·M· MODEL
SOFT: V02.2X
·183·
Prog ramm in g man u a l
9.16
G210. Bore milling canned cycle
This cycle may be used to increase the diameter of a hole through a helical movement of the tool.
Besides this, if the tool allows it, it is also possible to mill a hole without having to drill it first.
Working in Cartesian coordinates, the basic structure of the block is as follows:
G210 G98/G99 X Y Z D I J K B
M03
G01
M04
G98
G210. Bore milling canned cycle
CANNED CYCLES
9.
G00
Z
G99
D
I
K
J
[ G98/G99 ] Withdrawal plane
G98
The tool withdraws to the Initial Plane, once the hole has been milled.
G99
The tool withdraws to the Reference Plane, once the hole has been milled.
[X±5.5] Hole center coordinate along the abscissa axis.
It defines the hole center coordinate along the X axis. If not programmed, it will assume the current
tool position on that axis.
[ Y±5.5 ] Hole center coordinate along the ordinate axis
It defines the hole center coordinate along the Y axis. If not programmed, it will assume the current
tool position on that axis.
[ 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.
[D5] Safety distance
Defines the distance between the reference plane and the surface of the part where the milling is
to be done. If not programmed, it assumes 0.
[ 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 8037
If not programmed, the CNC issues the corresponding error.
[J±5.5 ] Hole diameter
Defines the nominal diameter of the hole. The sign indicates the direction of the helical path
associated with the machining of the hole (positive if clockwise and negative if counterclockwise).
·M· MODEL
SOFT: V02.2X
If not programmed or programmed with a value smaller than the diameter of the active tool, the CNC
issues the relevant error message.
[ K5.5 ] Pre-drilling diameter
Starting with a hole previously drilled, this parameter defines the diameter of that hole. If not
programmed or programmed with a 0 value, it means that no hole has been previously drilled.
·184·
P r o gr a m m i ng m a n u a l
The tool must meet the following conditions:
• The tool radius must be smaller than J/2.
• The tool radius must be equal to or larger than (J-K)/4.
If these two conditions are not met, the CNC issues the corresponding error.
[ B±5.5 ] Penetration step
It defines the penetration step when machining the hole.
• With a positive sign, it will mill the bottom of the hole.
CANNED CYCLES
If not programmed or programmed with a 0 value, the CNC will display the corresponding error
message.
G210. Bore milling canned cycle
9.
• With a negative sign, it will not mill the bottom of the hole.
CNC 8037
·M· MODEL
SOFT: V02.2X
·185·
Prog ramm in g man u a l
9.16.1
Basic operation
1. Rapid movement to the center of the hole (X, Y).
2. Rapid movement to the reference plane (Z).
3. Rapid movement to the tangential entry coordinate along the longitudinal axis.
4. Tangential entry to the helical path of the drilling.
5. Helical movement, with the pitch given by parameter B and in the direction given by parameter
J, down to the bottom of the hole.
9.
6. Milling of the bottom of the hole (this step is only carried out if parameter B has a positive sign).
CANNED CYCLES
G210. Bore milling canned cycle
7. Tangential exit movement to the helical path of the drilling to the center of the hole.
CNC 8037
·M· MODEL
SOFT: V02.2X
·186·
8. Rapid movement to the reference plane (G99) or to the starting plane (G98).
P r o gr a m m i ng m a n u a l
9.17
G211. Inside thread milling cycle
This cycle may be used to make an inside thread through a helical movement of the tool.
Working in Cartesian coordinates, the basic structure of the block is as follows:
G211 G98/G99 X Y Z D I J K B C L A E Q
A
M03
G01
M04
9.
G98
Z
K
D
G99
I
CANNED CYCLES
B
G00
G211. Inside thread milling cycle
L
J
[ G98/G99 ] Withdrawal plane
G98
The tool withdraws to the Initial Plane, once the hole has been milled.
G99
The tool withdraws to the Reference Plane, once the hole has been milled.
[X±5.5] Hole center coordinate along the abscissa axis.
It defines the hole center coordinate along the X axis. If not programmed, it will assume the current
tool position on that axis.
[ Y±5.5 ] Hole center coordinate along the ordinate axis
It defines the hole center coordinate along the Y axis. If not programmed, it will assume the current
tool position on that axis.
[ 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.
[D5] Safety distance
Defines the distance between the reference plane and the surface of the part where the milling is
to be done. If not programmed, it assumes 0.
[ I±5.5 ] Machining depth
Defines the threading depth. It may be programmed either in absolute or incremental coordinates,
in which case it will be referred to the reference plane.
CNC 8037
If not programmed, the CNC issues the corresponding error.
[ J±5.5 ] Thread diameter
Defines the nominal diameter of the thread The sign indicates the machining direction of the thread
(positive if clockwise and negative if counterclockwise).
If not programmed, the CNC issues the corresponding error.
·M· MODEL
SOFT: V02.2X
·187·
Prog ramm in g man u a l
[ K5.5 ] Thread depth
It defines the distance between the crest and the root of the thread. If not programmed, the CNC
issues the corresponding error.
[ B±5.5 ] Thread pitch
Defines the thread pitch.
• With a positive sign, the direction of the thread pitch is from the surface of the part to the bottom.
• With a negative sign, the direction of the thread pitch is from the bottom to the surface of the part.
9.
CANNED CYCLES
G211. Inside thread milling cycle
If not programmed or programmed with a 0 value, the CNC will display the corresponding error
message.
[ C1 ] Type of tapping
Defines the type of tapping to be carried out. This parameter depends on the type of tool being used.
• When programming C= 0, the threading will be done in a single pass.
• When programming C=1, it will make one thread per each pass (single-edge cutter).
• When programming C=n (where n is the number of cutting edges of the cutter), it will make n
threads per each pass.
If not programmed, a value of C=1 is assumed.
C=0
C=1
C>1
[ L5.5 ] Finishing stock
It defines the finishing stock at the bottom of the thread. If not programmed, a value of 0 is assumed.
[ A5.5 ] Maximum penetration step
Defines the maximum penetrating pass of the thread. If not programmed or programmed with a 0
value, it will run a single pass up to the finishing stock.
[ E5.5 ] Approach distance
Approach distance to the thread entry. If not programmed, it will enter the thread from the center
of the hole.
[ Q±5.5 ] Thread entry angle
Angle (in degrees) of the segment formed by the center of the hole and the thread entry point with
respect to the abscissa axis. If not programmed, a value of 0 is assumed.
CNC 8037
·M· MODEL
SOFT: V02.2X
·188·
P r o gr a m m i ng m a n u a l
Basic operation
1. Rapid movement to the center of the hole (X, Y).
2. Rapid movement to the reference plane (Z).
3. Rapid movement of the plane axes to the thread entry point (it only makes this movement if
parameter E has been programmed).
4. Rapid movement to the thread entry point coordinate along the longitudinal axis.
5. Thread entry with a helical movement tangent to the first helical threading path.
 If C=0:
·1·Helical movement, in the direction indicated in parameter J, to the bottom of the thread
(the movement will only be one revolution).
·2·Helical thread exiting movement, tangent to the previous helical path. If parameter E has
not been programmed, the exit point will correspond with the coordinates of the hole
center.
It must be borne in mind that in the exit tangent to the helical path, the exit point will exceed
the coordinate of the bottom of the thread along the longitudinal axis.
 If C=1:
·1·Helical movement, with the pitch and direction given in parameter J, to the bottom of the
thread.
G211. Inside thread milling cycle
9.
6. Making the thread according to the value of parameter C.
CANNED CYCLES
9.17.1
·2·Helical thread exiting movement, tangent to the previous helical path. If parameter E has
not been programmed, the exit point will correspond with the coordinates of the hole
center.
It must be borne in mind that in the exit tangent to the helical path, the exit point will exceed
the coordinate of the bottom of the thread along the longitudinal axis.
 If C=n:
·1·Helical movement, with the pitch and direction given in parameter J, (the movement will
be one revolution).
·2·Helical thread exiting movement, tangent to the previous helical path. If parameter E has
not been programmed, the exit point will correspond with the coordinates of the hole
center.
·3·Rapid movement to the thread entry point of the next threading path.
·4·Rapid movement to the Z coordinate of the thread entry point of the next threading path.
·5·Repetition of the previous 3 steps until reaching the bottom of the thread. It must be borne
in mind that in the last helical exit, the exit point will exceed the coordinate of the bottom
of the thread along the longitudinal axis.
7. Rapid movement to the center of the hole (X, Y).
8. Rapid movement to the thread entry coordinate along the longitudinal axis.
9. Repetition of steps 3 to 8 until reaching the depth of the finishing stock.
10.Repetition of steps 3 to 8 until reaching the bottom of the thread.
11.Rapid movement to the reference plane (G99) or to the starting plane (G98).
CNC 8037
·M· MODEL
SOFT: V02.2X
·189·
Prog ramm in g man u a l
9.18
G212. Outside thread milling cycle
This cycle may be used to make an outside thread through a helical movement of the tool.
Working in Cartesian coordinates, the basic structure of the block is as follows:
G212 G98/G99 X Y Z D I J K B C L A E Q
L
9.
CANNED CYCLES
G212. Outside thread milling cycle
B
G00
M03
G01
M04
G98
K
Z
G99
D
I
J
[ G98/G99 ] Withdrawal plane
G98
The tool withdraws to the Initial Plane, once the hole has been milled.
G99
The tool withdraws to the Reference Plane, once the hole has been milled.
[ X±5.5 ] Boss center coordinate along the abscissa axis.
It defines the boss center coordinate along the X axis. If not programmed, it will assume the current
tool position on that axis.
[ Y±5.5 ] Boss center coordinate along the ordinate axis.
It defines the boss center coordinate along the Y axis. If not programmed, it will assume the current
tool position on that axis.
[ 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.
[D5] Safety distance
Defines the distance between the reference plane and the surface of the part where the milling is
to be done. If not programmed, it assumes 0.
[ I±5.5 ] Machining depth
Defines the threading depth. It may be programmed either in absolute or incremental coordinates,
in which case it will be referred to the reference plane.
CNC 8037
If not programmed, the CNC issues the corresponding error.
[ J±5.5 ] Thread diameter
Defines the nominal diameter of the thread The sign indicates the machining direction of the thread
(positive if clockwise and negative if counterclockwise).
·M· MODEL
SOFT: V02.2X
If not programmed, the CNC issues the corresponding error.
[ K5.5 ] Thread depth
It defines the distance between the crest and the root of the thread. If not programmed, the CNC
issues the corresponding error.
·190·
P r o gr a m m i ng m a n u a l
[ B±5.5 ] Thread pitch
Defines the thread pitch.
• With a positive sign, the direction of the thread pitch is from the surface of the part to the bottom.
• With a negative sign, the direction of the thread pitch is from the bottom to the surface of the part.
If not programmed or programmed with a 0 value, the CNC will display the corresponding error
message.
[ C1 ] Type of tapping
• When programming C=1, it will make one thread per each pass (single-edge cutter).
• When programming C=n (where n is the number of cutting edges of the cutter), it will make n
threads per each pass.
If not programmed, a value of C=1 is assumed.
C=0
C=1
C>1
CANNED CYCLES
• When programming C= 0, the threading will be done in a single pass.
G212. Outside thread milling cycle
9.
Defines the type of tapping to be carried out. This parameter depends on the type of tool being used.
[ L5.5 ] Finishing stock
It defines the finishing stock at the bottom of the thread. If not programmed, a value of 0 is assumed.
[ A5.5 ] Maximum penetration step
Defines the maximum penetrating pass of the thread. If not programmed or programmed with a 0
value, it will run a single pass up to the finishing stock.
[ E5.5 ] Approach distance
Approach distance to the thread entry. If not programmed or programmed with a 0 value, the CNC
will display the corresponding error message.
[ Q±5.5 ] Thread entry angle
Angle (in degrees) of the segment formed by the center of the hole and the thread entry point with
respect to the abscissa axis. If not programmed, a value of 0 is assumed.
CNC 8037
·M· MODEL
SOFT: V02.2X
·191·
Prog ramm in g man u a l
9.18.1
Basic operation
1. Rapid movement to the center of the hole (X, Y).
2. Rapid movement to the reference plane (Z).
3. Rapid movement of the plane axes to the thread entry point (it only makes this movement if
parameter E has been programmed).
4. Rapid movement to the thread entry point coordinate along the longitudinal axis.
5. Rapid movement to the thread entry point (movement interpolated in 3 axes).
9.
6. Thread entry with a helical movement tangent to the first helical threading path.
CANNED CYCLES
G212. Outside thread milling cycle
7. Making the thread according to the value of parameter C.
 If C=0:
·1·Helical movement, in the direction indicated in parameter J, to the bottom of the thread
(the movement will only be one revolution).
·2·Helical thread exiting movement, tangent to the previous helical path.
It must be borne in mind that in the exit tangent to the helical path, the exit point will exceed
the coordinate of the bottom of the thread along the longitudinal axis.
 If C=1:
·1·Helical movement, with the pitch and direction given in parameter J, to the bottom of the
thread.
·2·Helical thread exiting movement, tangent to the previous helical path.
It must be borne in mind that in the exit tangent to the helical path, the exit point will exceed
the coordinate of the bottom of the thread along the longitudinal axis.
 If C=n:
·1·Helical movement, with the pitch and direction given in parameter J, (the movement will
be one revolution).
·2·Helical thread exiting movement, tangent to the previous helical path to the thread entry
point.
·3·Rapid movement to the Z coordinate of the thread entry point of the next threading path.
·4·Repetition of the previous 3 steps until reaching the bottom of the thread. It must be borne
in mind that in the last helical exit, the exit point will exceed the coordinate of the bottom
of the thread along the longitudinal axis.
8. Rapid movement to the reference plane (G99).
9. Repetition of steps 3 to 8 until reaching the depth of the finishing stock.
10.Repetition of steps 3 to 8 until reaching the bottom of the thread.
11.Rapid movement to the reference plane (G99) or to the starting plane (G98).
12.Rapid movement to the center of the hole (X, Y).
CNC 8037
·M· MODEL
SOFT: V02.2X
·192·
MULTIPLE MACHINING
10
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 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 8037
·M· MODEL
SOFT: V02.2X
·193·
Prog ramm in g man u a l
10.1
G60: Multiple machining in a straight line
The programming format for this cycle is:
radius
XI
XK
IK
PQRSTUV
MULTIPLE MACHINING
G60: Multiple machining in a straight line
10.
[ A±5.5 ] 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.
[ X5.5 ] Path length
Defines the length of the machining path.
[ I5.5 ] Step between machining operations.
Defines the pass between machining operations.
[ K5 ] 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.
[ P Q R S T U V ] 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.
CNC 8037
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:
·M· MODEL
SOFT: V02.2X
·194·
Proper programming
P5.006 Q12.015 R20.022
Correct programming
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.
P r o gr a m m i ng m a n u a l
10.1.1
Basic operation
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.
G60: Multiple machining in a straight line
; 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
10.
MULTIPLE MACHINING
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:
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
CNC 8037
·M· MODEL
SOFT: V02.2X
·195·
Prog ramm in g man u a l
10.2
G61: Multiple machining in rectangular pattern
The programming format for this cycle is:
G61 A B
XI
XK
IK
YJ
YD
JD
PQRSTUV
MULTIPLE MACHINING
G61: Multiple machining in rectangular pattern
10.
[ A±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.
[ B±5.5 ] 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.
[ X5.5 ] Length of the path along the abscissa axis
Defines the length of the machining path according to the abscissa axis.
[ I5.5 ] Machining pass along the abscissa axis
Defines the pass between machining operations along the abscissa axis.
[ K5 ] Number of machining operations along the abscissa axis
Defines the total number of 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.
[ Y5.5 ] Length of the path along the ordinate axis
Defines the length of the machining path according to the ordinate axis.
CNC 8037
[ J5.5 ] Machining pass along the ordinate axis
Defines the pass between machining operations according to the ordinate axis.
[ D5 ] Number of machining operations along the ordinate axis
·M· MODEL
SOFT: V02.2X
Defines the total number of 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.
·196·
P r o gr a m m i ng m a n u a l
[ P Q R S T U V ] 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.
Proper programming
P5.006 Q12.015 R20.022
Correct programming
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.
G61: Multiple machining in rectangular pattern
Example:
10.
MULTIPLE MACHINING
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·197·
Prog ramm in g man u a l
10.2.1
Basic operation
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.
MULTIPLE MACHINING
G61: Multiple machining in rectangular pattern
10.
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:
; 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 8037
·M· MODEL
SOFT: V02.2X
·198·
P r o gr a m m i ng m a n u a l
10.3
G62: Multiple machining in grid pattern
The programming format for this cycle is:
G62 A B
XI
XK
IK
YJ
YD
JD
PQRSTUV
[ A±5.5 ] Angle of the path with respect to the abscissa axis
G62: Multiple machining in grid pattern
MULTIPLE MACHINING
10.
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.
[ B±5.5 ] 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.
[ X5.5 ] Length of the path along the abscissa axis
Defines the length of the machining path according to the abscissa axis.
[ I5.5 ] Machining pass along the abscissa axis
Defines the pass between machining operations along the abscissa axis.
[ K5 ] Number of machining operations along the abscissa axis
Defines the total number of 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.
[ Y5.5 ] Length of the path along the ordinate axis
Defines the length of the machining path according to the ordinate axis.
[ J5.5 ] Machining pass along the ordinate axis
Defines the pass between machining operations according to the ordinate axis.
CNC 8037
[ D5 ] Number of machining operations along the ordinate axis
Defines the total number of 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.
·M· MODEL
SOFT: V02.2X
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.
·199·
Prog ramm in g man u a l
[ P Q R S T U V ] 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.
MULTIPLE MACHINING
G62: Multiple machining in grid pattern
10.
CNC 8037
·M· MODEL
SOFT: V02.2X
·200·
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
P5.006 Q12.015 R20.022
Correct programming
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.
P r o gr a m m i ng m a n u a l
10.3.1
Basic operation
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.
G62: Multiple machining in grid pattern
10.
MULTIPLE MACHINING
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:
; 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
CNC 8037
·M· MODEL
SOFT: V02.2X
·201·
Prog ramm in g man u a l
10.4
G63: Multiple machining in a circular pattern
The programming format for this cycle is:
G63 X Y
I
K
CFPQRSTUV
MULTIPLE MACHINING
G63: Multiple machining in a circular pattern
10.
[ 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.
[ K5 ] Total number of machining operations
Defines the total number of 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 not programmed, a value of C=0
is assumed.
CNC 8037
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)
[ F5.5 ] 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.
·M· MODEL
SOFT: V02.2X
·202·
P r o gr a m m i ng m a n u a l
[ P Q R S T U V ] 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.
Proper programming
P5.006 Q12.015 R20.022
Correct programming
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.
G63: Multiple machining in a circular pattern
Example:
10.
MULTIPLE MACHINING
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·203·
Prog ramm in g man u a l
10.4.1
Basic operation
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.
MULTIPLE MACHINING
G63: Multiple machining in a circular pattern
10.
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:
; 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 8037
·M· MODEL
SOFT: V02.2X
·204·
P r o gr a m m i ng m a n u a l
10.5
G64: Multiple machining in an arc
The programming format for this cycle is:
G64 X Y B
I
K
CFPQRSTUV
[ 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.
G64: Multiple machining in an arc
MULTIPLE MACHINING
10.
[ 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).
[ B5.5 ] Angular travel
Defines the angular stroke of the machining path and is expressed in degrees.
[ 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.
[ K5 ] Total number of machining operations
Defines the total number of 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 not programmed, a value of C=0
is assumed.
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 8037
[ F5.5 ] 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.
·M· MODEL
SOFT: V02.2X
·205·
Prog ramm in g man u a l
[ P Q R S T U V ] 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.
MULTIPLE MACHINING
G64: Multiple machining in an arc
10.
CNC 8037
·M· MODEL
SOFT: V02.2X
·206·
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
P5.006 Q12.015 R20.022
Correct programming
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.
P r o gr a m m i ng m a n u a l
10.5.1
Basic operation
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.
G64: Multiple machining in an arc
10.
MULTIPLE MACHINING
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:
; 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
CNC 8037
·M· MODEL
SOFT: V02.2X
·207·
Prog ramm in g man u a l
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
I
CF
MULTIPLE MACHINING
G65: Machining programmed with an arc-chord
10.
[ 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).
[ 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.
[ C0/1/2/3 ] Type of move from point to point
Indicates how movement is made between machining points. If not programmed, a value of C=0
is assumed.
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)
[ F5.5 ] Feedrate to move from point to point
CNC 8037
·M· MODEL
SOFT: V02.2X
·208·
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.
P r o gr a m m i ng m a n u a l
10.6.1
Basic operation
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:
; 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
G65: Machining programmed with an arc-chord
5
MULTIPLE MACHINING
444
.7
10.
It is also possible to write the multiple machining definition block in the following ways:
G65 X-280 Y-40 I444.75 C1 F200
CNC 8037
·M· MODEL
SOFT: V02.2X
·209·
Prog ramm in g man u a l
MULTIPLE MACHINING
G65: Machining programmed with an arc-chord
10.
CNC 8037
·M· MODEL
SOFT: V02.2X
·210·
PROBING
11
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·211·
Prog ramm in g man u a l
11.1
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:
PROBING
Probing (G75, G76)
11.
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 8037
·M· MODEL
SOFT: V02.2X
·212·
HIGH-LEVEL LANGUAGE
PROGRAMMING
12.1
12
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.
To assign the value 100000000 to the variable "TIMER", It can be done 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).
CNC 8037
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).
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.
·M· MODEL
SOFT: V02.2X
·213·
Prog ramm in g man u a l
Simbols
The symbols used in high-level language are:
()“=+-*/,
Lexical description
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
CNC 8037
·M· MODEL
SOFT: V02.2X
·214·
P r o gr a m m i ng m a n u a l
Variables
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.
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
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.
12.
Variables
ORG(X-C) -> ORGX
HIGH-LEVEL LANGUAGE PROGRAMMING
12.2
Example: Reading a variable that interrupts block preparation.
The following program blocks are performed in a section with G41 compensation.
...
N10
N15
N20
N30
...
X50 Y80
(P100 = POSX); Assigns the value of the real coordinate in X to parameter P100
X50 Y50
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.
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·215·
Prog ramm in g man u a l
12.2.1
General purpose parameters or 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.
Variables
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
Parameter type
Range
Local parameters
P0-P25
Global parameters
P100-P299
User parameters
P1000-P1255
OEM (manufacturer's) parameters
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...
GP0 XP1 Z100
(IF (P100 * P101 EQ P102) GOTO N100)
When executing...
G1 X-12.5 Z100
(IF (2 * 5 EQ 12) GOTO N100)
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.
CNC 8037
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.
·M· MODEL
SOFT: V02.2X
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.
·216·
P r o gr a m m i ng m a n u a l
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.
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
The CNC offers high level instructions for defining and using subroutines that may be called upon
from the main program (or a subroutine) and another subroutine from this one and so on, the CNC
limits the number of these calls to a maximum of 15 nesting levels. The CNC limitation is 20 nesting
levels.
HIGH-LEVEL LANGUAGE PROGRAMMING
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.
Variables
12.
Updating arithmetic parameter tables
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 8037
·M· MODEL
SOFT: V02.2X
·217·
Prog ramm in g man u a l
12.2.2
Variables associated with tools.
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).
Variables
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
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.
0
The magazine position is empty.
-1
The magazine position has been canceled.
The tool position in the magazine is represented as follows:
1.- Position number.
0
The tool is in the spindle.
-1
Tool not found
-2
The tool is in the change position.
Read-only variables
TOOL
Returns the number of the active tool.
(P100=TOOL)
Assigns the number of the active tool to parameter P100.
TOD
CNC 8037
Returns the number of the active tool offset.
NXTOOL
Returns the next tool number, which is selected but is awaiting the execution of M06 to be active.
NXTOD
·M· MODEL
SOFT: V02.2X
·218·
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.
P r o gr a m m i ng m a n u a l
TMZPn
Returns the position occupied in the tool magazine by the indicated tool (n).
PTOOL
Returns the magazine position to where the current tool is to be left. It matches the value that will
be received later on in the register "T2BCD" (R559) with the M6, but the latter will be in BCD format.
This variable is only accessible via the CNC.
This variable is only accessible via the CNC.
HTOR
The HTOR variable indicates the tool radius being used by the CNC to do the calculations.
Being a variable that can be read and written by the CNC and read-only from the PLC and DNC,
its value may be different from the one assigned in the table (TOR).
On power-up, after a T function, after a RESET or after an M30 function, it assumes the value of
the table (TOR).
Application example
To machine a profile with a residual stock of 0.5 mm running 0.1mm-passes with a tool whose radius
is 10 mm.
HIGH-LEVEL LANGUAGE PROGRAMMING
Returns the magazine position from where the next tool is to be picked up. It matches the value that
will be received later on in the register "TBCD" (R558) with the M6, but the latter will be in BCD format.
Variables
12.
PNXTOOL
Assign to the tool radius the value of:
10.5 mm in the table and execute the profile.
10.4 mm in the table and execute the profile.
10.3 mm in the table and execute the profile.
10.2 mm in the table and execute the profile.
10.1 mm in the table and execute the profile.
10.0 mm in the table and execute the profile.
However, if while machining, the program is interrupted or a reset occurs, the table assumes the
radius value assigned in that instant (e.g.: 10.2 mm). Its value has changed.
To avoid this, instead of modifying the tool radius in the (TOR) table, use the variable (HTOR) to
change the tool radius value used by the CNC to calculate.
Now, if the program is interrupted, the tool radius value initially assigned in the (TOR) table will be
correct because it has not changed.
Read-and-write variables
TORn
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.
TOLn
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·219·
Prog ramm in g man u a l
TOIn
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.
TOKn
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.
Variables
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
CNC 8037
·M· MODEL
SOFT: V02.2X
·220·
TLFDn
This variable allows the tool offset number of the indicated tool (n) to be read or modified in the tool
table.
TLFFn
This variable allows the family code of the indicated tool (n) to be read or modified in the tool table.
TLFNn
This variable allows the value assigned as the nominal life of the indicated tool (n) to be read or
modified in the tool table.
TLFRn
This variable allows the value corresponding to the real life of the indicated tool (n) to be read or
modified in the tool table.
TMZTn
This variable allows the contents of the indicated position (n) to be read or modified in the tool
magazine table.
P r o gr a m m i ng m a n u a l
12.2.3
Variables associated with zero offsets.
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).
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 the X and Z axes, it only allows the variables
ORGX and ORGZ in the case of ORG(X-C).
Read-only variables
ORG(X-C)
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".
HIGH-LEVEL LANGUAGE PROGRAMMING
If rotary axis in degrees (within ±99999.9999).
Variables
12.
If G71, in millimeters (within ±99999.9999).
PORGF
Returns the abscissa value of the polar coordinate origin with respect to the Cartesian origin.
PORGS
Returns the ordinate value of the polar coordinate origin with respect to the Cartesian origin.
ADIOF(X-C)
It returns the value of the zero offset generated by the additive handwheel in the selected axis.
ADDORG (X-C)
Returns the value of the active incremental zero offset corresponding to the axis selected at the time.
It is read-only variable that can be read from the CNC, PLC and DNC.
CNC 8037
·M· MODEL
SOFT: V02.2X
·221·
Prog ramm in g man u a l
EXTORG
Returns the active absolute zero offset. The values returned by the variable are identical for both
possible expressions of absolute zero offsets.
This read-only variable interrupts block preparation and may be read from the CNC, from the PLC
and from DNC.
The values of the EXTORG variables that correspond to the absolute zero offsets are:
EXTORG
Variables
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
Active zero offset
EXTORG
Active zero offset
0
G53 (there is no zero offset)
11
G159N11
1
G54 or G159N1
12
G159N12
2
G55 or G159N2
13
G159N13
3
G56 or G159N3
14
G159N14
4
G57 or G159N4
15
G159N15
5
G159N5
16
G159N16
6
G159N6
17
G159N17
7
G159N7
18
G159N18
8
G159N8
19
G159N19
9
G159N9
20
G159N20
10
G159N10
Considerations:
• When programming only an incremental zero offset (G58 or G59), the value of the EXTORG
variable will be 0.
• When programming an absolute and an incremental zero offset, the EXTORG variable will keep
the value of the absolute zero offset.
Example: If G54 + G58, EXTORG = 1 has been programmed.
Read-and-write variables
ORG(X-C)n
This variable allows the value of the selected axis to be read or modified in the table corresponding
to the indicated zero offset (n).
If G54-G59 is used:
(P110=ORGX 55)
Loads parameter P100 with the X value of G55 in the zero offset table.
(ORGY 54=100.8)
It assigns value 100.8 to the Y axis in the table for the G54 zero offset.
If G159N1-N20 is used:
(P110=ORGX 19)
Loads parameter P110 with the X value of G159N19 in the zero offset table.
(ORGY 19=100.8)
It assigns value 100.8 to the Y axis in the table for the G159N19 zero offset.
CNC 8037
PLCOF(X-C)
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.
·M· MODEL
SOFT: V02.2X
·222·
P r o gr a m m i ng m a n u a l
12.2.4
Variables associated with machine parameters
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).
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.
Read-only variables
MPGn
Returns the value assigned to general machine parameter (n).
HIGH-LEVEL LANGUAGE PROGRAMMING
If rotary axis in degrees (within ±99999.9999).
Variables
12.
If G71, in millimeters (within ±99999.9999).
(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.
MP(X-C)n
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.
MPSn
Returns the value assigned to the indicated machine parameter (n) of the main spindle.
MPLCn
Returns the value assigned to the indicated machine parameter (n) of the PLC.
CNC 8037
·M· MODEL
SOFT: V02.2X
·223·
Prog ramm in g man u a l
12.2.5
Variables associated with work zones
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).
Variables
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
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.
Read-only variables
FZONE
It returns the status of work zone 1.
FZLO(X-C)
FZUP(X-C)
Lower limit of zone 1 along the selected axis (X-C).
Upper limit of zone 1 along the selected axis (X-C).
(P100=FZONE)
; It assigns to parameter P100 the status of work zone 1.
(P101=FZOLOX)
; It assigns the lower limit of zone 1 to parameter P101.
(P102=FZUPZ)
; It assigns the upper limit of zone 1 to parameter P102.
SZONE
SZLO(X-C)
SZUP(X-C)
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).
TZONE
TZLO(X-C)
TZUP(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).
FOZONE
FOZLO(X-C)
FOZUP(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).
FIZONE
CNC 8037
FIZLO(X-C)
FIZUP(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).
·M· MODEL
SOFT: V02.2X
·224·
P r o gr a m m i ng m a n u a l
12.2.6
Variables associated with feedrates
Read-only variables associated with the real (actual) feedrate
FREAL
It returns the CNC's real feedrate. In mm/minute or inches/minute.
It returns the actual (real) CNC feedrate of the selected axis.
FTEO(X-C)
It returns the theoretical CNC feedrate of the selected axis.
Read-only variables associated with function G94
FEED
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.
HIGH-LEVEL LANGUAGE PROGRAMMING
FREAL(X-C)
Variables
12.
(P100=FREAL)
It assigns the real feedrate value of the CNC to parameter P100.
DNCF
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.
PLCF
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.
PRGF
It returns the feedrate, in mm/minute or inches/minute selected by program.
Read-only variables associated with function G95
FPREV
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.
CNC 8037
DNCFPR
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.
PLCFPR
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.
·M· MODEL
SOFT: V02.2X
·225·
Prog ramm in g man u a l
PRGFPR
It returns the feedrate, in mm/turn or inches/turn selected by program.
Read-only variables associated with function G32
PRGFIN
Variables
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
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.
Read-only variables associated with the override
FRO
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 from the front panel;
the CNC selects one of them, where the priority (from the highest to the lowest) is: by program, by
DNC, by PLC and from the switch.
DNCFRO
It returns the feedrate override % currently selected by the DNC. If it has a value of 0 it means that
it is not selected.
PLCFRO
It returns the feedrate override % currently selected by the PLC. If it has a value of 0 it means that
it is not selected.
CNCFRO
It returns the feedrate override % currently selected by the switch.
PLCCFR
It returns the feedrate percentage currently selected by the PLC's execution channel.
Read-write variables associated with the override
PRGFRO
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·226·
(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.
P r o gr a m m i ng m a n u a l
12.2.7
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).
PPOS(X-C)
Returns the programmed theoretical coordinate of the selected axis.
(P110=PPOSX)
It assigns to P100 the programmed theoretical position of the X axis.
POS(X-C)
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
HIGH-LEVEL LANGUAGE PROGRAMMING
Accessing any of the variables POS(X-C), TPOS(X-C), APOS(X-C), ATPOS(X-C), DPOS(X-C) or
FLWE(X-C) interrupts block preparation and the CNC waits for that command to be executed before
resuming block preparation.
Variables
12.
Read-only variables
TPOS(X-C)
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
APOS(X-C)
It returns the real tool base position value, referred to part zero, of the selected axis.
ATPOS(X-C)
It returns the theoretical position value (real coordinate + following error) of the tool base referred
to part zero.
DPOS(X-C)
The CNC updates this variable when probing, functions G75 and G76.
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·227·
Prog ramm in g man u a l
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.
FLWE(X-C)
It returns the following error of the selected axis.
Variables
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
CNC 8037
·M· MODEL
SOFT: V02.2X
·228·
DPLY(X-C)
It returns the position value (coordinate) shown on the screen for the selected axis.
GPOS(X-C)n p
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.
P r o gr a m m i ng m a n u a l
Read-and-write variables
DIST(X-C)
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.
LIMPL(X-C)
LIMMI(X-C)
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).
Variables
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.
12.
HIGH-LEVEL LANGUAGE PROGRAMMING
(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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·229·
Prog ramm in g man u a l
12.2.8
Variables associated with electronic handwheels
Read-only variables
HANPF
Variables
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
HANPS
HANPT
HANPFO
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.
HANDSE
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.
HANFCT
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
c
b
B
a
c
b
A
a
c
b
W
a
c
b
V
a
c
b
U
a
c
b
Z
a
c
b
Y
a
c
X
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.
c
b
a
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:
c
b
a
1
1
1
x1 factor
1
1
0
x10 factor
i
The screen always shows the value selected at the switch.
HBEVAR
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).
CNC 8037
C
* ^
B
A
W
V
U
Z
Y
X
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.
·M· MODEL
SOFT: V02.2X
·230·
0=
They are ignored.
1=
They are taken into account.
P r o gr a m m i ng m a n u a l
(^) 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 ignored the pulses from the individual handwheel.
(a, b, c) Indicate the axis to be moved and the selected multiplying factor.
a
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:
c
b
a
1
1
1
x1 factor
1
1
0
x10 factor
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.
12.
Variables
b
HIGH-LEVEL LANGUAGE PROGRAMMING
c
Read-and-write variables
MASLAN
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 8037
·M· MODEL
SOFT: V02.2X
·231·
Prog ramm in g man u a l
12.2.9
Variables associated with feedback
ASIN(X-C)
"A" signal of the CNC's sinusoidal feedback for the X-C axis.
BSIN(X-C)
"B" signal of the CNC's sinusoidal feedback for the X-C axis.
Variables
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
CNC 8037
·M· MODEL
SOFT: V02.2X
·232·
ASINS
"A" signal of the CNC's sinusoidal feedback for the spindle.
BSINS
"B" signal of the CNC's sinusoidal feedback for the spindle.
P r o gr a m m i ng m a n u a l
12.2.10 Variables associated with the main spindle
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.
Read-only variables
(P100=SREAL)
It assigns to P100 the real turning speed of the main spindle.
FTEOS
It returns the theoretical turning speed of the main spindle.
SPEED
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.
Variables
Returns the real main spindle turning speed in revolutions per minute. It interrupts block preparation.
HIGH-LEVEL LANGUAGE PROGRAMMING
SREAL
12.
DNCS
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.
PLCS
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.
PRGS
Returns the turning speed in revolutions per minute, selected by program.
SSO
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 panel frontal.
DNCSSO
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.
PLCSSO
CNC 8037
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.
CNCSSO
It returns the turning speed override % of the main spindle currently selected from the front panel.
·M· MODEL
SOFT: V02.2X
SLIMIT
It returns the value set in rpm at the CNC for the turning speed limit of the main spindle.
·233·
Prog ramm in g man u a l
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.
DNCSL
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.
PLCSL
Variables
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
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.
PRGSL
It returns the speed limit of the main spindle in rpm currently selected by program.
MDISL
Maximum machining spindle speed. This variable is also updated (refreshed) when programming
function G92 via MDI.
POSS
It returns the real position of the main spindle. Its value may be within ±99999.9999°. It interrupts
block preparation.
RPOSS
It returns the real position of the main spindle. Its value is given in 0.0001 degree units (between
-360º and 360º). It interrupts block preparation.
TPOSS
It returns the theoretical position of the main spindle (real position + lag). Its value may be within
±99999.9999º. It interrupts block preparation.
RTPOSS
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.
PRGSP
Position programmed in M19 via program for the main spindle. This variable may be read from the
CNC, from the PLC and from DNC.
FLWES
It returns the main spindle's following error in degrees (within ±99999.9999). It interrupts block
preparation.
Read-and-write variables
PRGSSO
CNC 8037
·M· MODEL
SOFT: V02.2X
·234·
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.
P r o gr a m m i ng m a n u a l
12.2.11 PLC related variables
It should be borne in mind that the PLC has the following resources:
(O1 thru O512)
Outputs.
M1 thru M5957)
Marks.
(R1 thru R499)
32-bit registers.
(T1 thru T512)
Timers with a timing count in 32 bits.
(C1 thru C256)
Counters with a count in 32 bits.
12.
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.
Read-only variables
PLCMSG
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.
Variables
Inputs.
HIGH-LEVEL LANGUAGE PROGRAMMING
(I1 thru I512)
Read-and-write variables
PLCIn
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.
PLCOn
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
PLCMn
This variable allows 32 PLC marks to be read or modified starting from the one indicated (n).
CNC 8037
PLCRn
This variable allows the status of 32 register bits to be read or modified starting from the one indicated
(n).
·M· MODEL
SOFT: V02.2X
PLCTn
This variable allows the timer count to be read or modified starting from the one indicated (n).
·235·
Prog ramm in g man u a l
PLCCn
This variable allows the counter count to be read or modified starting from the one indicated (n).
PLCMMn
This variable permits reading or modifying the PLC mark (n).
Variables
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
CNC 8037
·M· MODEL
SOFT: V02.2X
·236·
(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·
P r o gr a m m i ng m a n u a l
12.2.12 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.
Read-only variables
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)
...
...
HIGH-LEVEL LANGUAGE PROGRAMMING
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.
Variables
12.
CALLP
In parameter P100 the following will be obtained:
0000
0000
0000
0000
0000
0000
0000
1101
LSB
CNC 8037
·M· MODEL
SOFT: V02.2X
·237·
Prog ramm in g man u a l
12.2.13 Operating-mode related variables
Read-only variables related to the standard mode
OPMODE
It returns the code corresponding to the selected operating mode.
Variables
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
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.
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.
CNC 8037
53 = Tool magazine table.
54 = Global parameter table.
55 = Local parameter table.
56 = User parameter table.
57 = OEM parameter table.
·M· MODEL
SOFT: V02.2X
60 = Utilities.
70 = DNC status.
·238·
P r o gr a m m i ng m a n u a l
71 = CNC status.
80 = PLC file editing.
81 = PLC program compilation.
82 = PLC monitoring.
83 = Active PLC messages.
84 = Active PLC pages.
85 = Save PLC program.
88 = PLC statistics.
90 = Customizing.
100 = General machine parameter table.
101 = Axis machine parameter tables.
102 = Spindle machine parameter table.
103 = Serial line related 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.
HIGH-LEVEL LANGUAGE PROGRAMMING
87 = PLC usage maps.
Variables
12.
86 = Restore PLC program.
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.
120 = DERGAIN auto-adjustment.
CNC 8037
·M· MODEL
SOFT: V02.2X
·239·
Prog ramm in g man u a l
12.2.14 Other variables
Read-only variables
NBTOOL
Variables
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
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".
PRGN
Returns the program number being executed. If none is selected, a value of -1 is returned.
BLKN
It returns the label number of the last executed block.
GGSA
It returns the status of functions G00 through G24. The status of each one of the functions will be
given in the 25 least significant bits and it will be indicated by a 1 when active and a 0 when not active
or when not available in the current software version.
G24
G23
G22
G21
G20
...
G04
G03
G02
G01
G00
CNCRD (GGSA, R110, M10)
Loads register R110 with the status of functions G00 through G24.
GGSB
It returns the status of functions G25 through G49. The status of each one of the functions will be
given in the 25 least significant bits and it will be indicated by a 1 when active and a 0 when not active
or when not available in the current software version.
G49
G48
G47
G46
G45
...
G29
G28
G27
G26
G25
GGSC
It returns the status of functions G50 through G24. The status of each one of the functions will be
given in the 25 least significant bits and it will be indicated by a 1 when active and a 0 when not active
or when not available in the current software version.
G74
CNC 8037
·M· MODEL
SOFT: V02.2X
·240·
G73
G72
G71
G70
...
G54
G53
G52
G51
G50
P r o gr a m m i ng m a n u a l
GGSD
It returns the status of functions G5 through G99. The status of each one of the functions will be
given in the 25 least significant bits and it will be indicated by a 1 when active and a 0 when not active
or when not available in the current software version.
G99
G98
G97
G96
G95
...
G79
G78
G77
G76
G75
GGSE
It returns the status of functions G100 through G124. The status of each one of the functions will
be given in the 25 least significant bits and it will be indicated by a 1 when active and a 0 when not
active or when not available in the current software version.
G122
G121
G120
...
G104
G103
G102
G101
G100
GGSF
It returns the status of functions G125 through G149. The status of each one of the functions will
be given in the 25 least significant bits and it will be indicated by a 1 when active and a 0 when not
active or when not available in the current software version.
G149
G148
G147
G146
G145
...
G129
G128
G127
G126
G125
GGSG
It returns the status of functions G150 through G174. The status of each one of the functions will
be given in the 25 least significant bits and it will be indicated by a 1 when active and a 0 when not
active or when not available in the current software version.
G174
G173
G172
G171
G170
...
G154
G153
G152
G151
G150
Variables
G123
HIGH-LEVEL LANGUAGE PROGRAMMING
G124
12.
GGSH
It returns the status of functions G175 through G199. The status of each one of the functions will
be given in the 25 least significant bits and it will be indicated by a 1 when active and a 0 when not
active or when not available in the current software version.
G199
G198
G197
G196
G195
...
G179
G178
G177
G176
G175
GGSI
It returns the status of functions G200 through G224. The status of each one of the functions will
be given in the 25 least significant bits and it will be indicated by a 1 when active and a 0 when not
active or when not available in the current software version.
G224
G223
G222
G221
G220
...
G204
G203
G202
G201
G200
GGSJ
It returns the status of functions G225 through G249. The status of each one of the functions will
be given in the 25 least significant bits and it will be indicated by a 1 when active and a 0 when not
active or when not available in the current software version.
G249
G248
G247
G246
G245
...
G229
G228
G227
G226
G225
GGSK
It returns the status of functions G250 through G274. The status of each one of the functions will
be given in the 25 least significant bits and it will be indicated by a 1 when active and a 0 when not
active or when not available in the current software version.
G274
G273
G272
G271
G270
...
G254
G253
G252
G251
CNC 8037
G250
GGSL
It returns the status of functions G75 through G299. The status of each one of the functions will be
given in the 25 least significant bits and it will be indicated by a 1 when active and a 0 when not active
or when not available in the current software version.
G299
G298
G297
G296
G295
...
G279
G278
G277
G276
·M· MODEL
SOFT: V02.2X
G275
·241·
Prog ramm in g man u a l
GGSM
It returns the status of functions G300 through G324. The status of each one of the functions will
be given in the 25 least significant bits and it will be indicated by a 1 when active and a 0 when not
active or when not available in the current software version.
G324
G323
G322
G321
G320
...
G304
G303
G302
G301
G300
GGSN
Variables
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
It returns the status of functions G325 through G349. The status of each one of the functions will
be given in the 25 least significant bits and it will be indicated by a 1 when active and a 0 when not
active or when not available in the current software version.
G349
G348
G347
G346
G345
…
G329
G328
G327
G326
G325
GGSO
It returns the status of functions GG350 through G374. The status of each one of the functions will
be given in the 25 least significant bits and it will be indicated by a 1 when active and a 0 when not
active or when not available in the current software version.
G374
G373
G372
G371
G370
…
G354
G353
G352
G351
G350
GGSP
It returns the status of functions G375 through G399. The status of each one of the functions will
be given in the 25 least significant bits and it will be indicated by a 1 when active and a 0 when not
active or when not available in the current software version.
G399
G398
G397
G396
G395
…
G379
G378
G377
G376
G375
GGSQ
It returns the status of functions G400 through G424. The status of each one of the functions will
be given in the 25 least significant bits and it will be indicated by a 1 when active and a 0 when not
active or when not available in the current software version.
G424
G423
G422
G421
G420
…
G404
G403
G402
G401
G400
GSn
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.
MSn
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
and M44.
PLANE
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.
...
CNC 8037
...
...
...
...
...
7654
3210
Abscissa axis
lsb
Ordinate axis
The axes are coded in 4 bits and indicate the axis number according to the programming order.
·M· MODEL
SOFT: V02.2X
Example: If the CNC controls the X, Y and Z axes and the ZX plane (G18) is selected.
(P122 = PLANE) assigns the value of $31 to parameter P122.
0000
·242·
0000
0000
0000
0000
0000
0011
0001
LSB
P r o gr a m m i ng m a n u a l
Abscissa axis
= 3 (0011)
=> Z axis
Ordinate axis
= 1 (0001)
=> X axis
LONGAX
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:
MIRROR
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
Axis 3
Axis 2
Axis 1
LSB
The axis name corresponds to the number according to the programming order for them.
Example: If the CNC controls the X, Y and Z axes, axis1=X, axis2 = Y, axis 3=Z.
SCALE
It returns the general scaling factor being applied.
SCALE(X-C)
HIGH-LEVEL LANGUAGE PROGRAMMING
(P122 = LONGAX) assigns the value 3 to parameter P122.
Variables
12.
If the CNC controls the X, Y and Z axes and the Z axis is selected.
Returns the specific scaling factor of the indicated axis (X-C).
ORGROT
It returns the rotation angle of the coordinate system currently selected with G73. Its value is given
in degrees (within ±99999.9999).
ROTPF
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).
ROTPS
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).
PRBST
Returns probe status.
0 = the probe is not touching the part.
1 = the probe is touching the part.
CNC 8037
If this variable is accessed, block preparation is interrupted and the CNC waits for this command
to be executed to resume block preparation.
CLOCK
Returns the time in seconds indicated by the system clock. Possible values 0..4294967295.
·M· MODEL
SOFT: V02.2X
If this variable is accessed, block preparation is interrupted and the CNC waits for this command
to be executed to resume block preparation.
·243·
Prog ramm in g man u a l
TIME
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.
DATE
Returns the date in year-month-day format.
Variables
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
(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.
CYTIME
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.
FIRST
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.
ANAIn
It returns the status of the indicated analog input (n). The value given in Volts and in ±1.4 format.
It is possible to select one of the 8 analog inputs (1··8) available. The values returned will be within
the ±5 V range.
If this variable is accessed, block preparation is interrupted and the CNC waits for this command
to be executed to resume block preparation.
TIMEG
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.
RIP
Linear theoretical feedrate resulting from the next loop (in mm/min).
CNC 8037
The calculation of the resulting feedrate ignores the rotary axes, slave axes (gantry, coupled and
synchronized) as well as DRO axes.
Read-and-write variables
·M· MODEL
SOFT: V02.2X
TIMER
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.
·244·
P r o gr a m m i ng m a n u a l
PARTC
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.
KEY
If this variable is accessed, block preparation is interrupted and the CNC waits for this command
to be executed to resume block preparation.
KEYSRC
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.
ANAOn
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).
HIGH-LEVEL LANGUAGE PROGRAMMING
This variable may be used as a write variable only inside a customizing program (user channel).
Variables
12.
Returns the code of the last key accepted.
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.
SELPRO
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.
DIAM
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·.
CNC 8037
PRBMOD
It indicates whether a probing error is to issued or not in the following cases, even if general machine
parameter PROBERR (P119) =YES.
• When a G75 probing move finishes before the probe has touched part.
• When a G76 probing move finishes but the probe is still touching the part.
·M· MODEL
SOFT: V02.2X
·245·
Prog ramm in g man u a l
The PRBMOD variable takes the following values.
Value
Meaning
0
An error message is issued.
1
No error message is issued.
Default value 0.
Variables
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
The PRBMOD variable can be read and written from the CNC and the PLC an read from the DNC.
DISABMOD
This variable is used to disable some actions or modes by setting the corresponding bit value to
1. This variable may be written from the PLC and read from the PLC, DNC and CNC.
The following table shows the meaning of each bit:
Bit
Meaning
0
If 1, the PLC program cannot be displayed. The PLC in ladder (contacts) diagram cannot
be displayed either.
1
If 1, the date cannot be changed, although it displays the access softkey. It is valid for
the explorer and for "UTILITIES".
2
If 1, the passwords cannot be changed. The passwords cannot be seen or changed
although it displays the access softkey. It is valid for the explorer and for "UTILITIES".
CYCCHORDERR
This variable defines the chordal error of the canned cycles. It may be read and written from the
part-program.
The CYCCHORDERR variable lets modify the chordal error of the cycles so the user can increase
or decrease it for the parts as needed.
Using this variable is necessary, for example, on parts with curved areas using the 3D pocket cycle.
On these parts, if the radius is very large, the segments are noticeable. The parts get better by
decreasing the chordal error.
Using this variable, the user can decrease the chordal error on the part as needed. Decreasing the
chordal error can increase machining time.
Once the value of this variable has been changed, it remains active until the CNC is turned off.
Default value of the CYCCHORDERR variable (250 tenths of a micron).
Programming example:
(CYCCHORDERR = 25)
(PCALL 9986, P200=0)
M30
It is recommended to use a CYCCHORDERR value of 25 tenths of a micron. This value improves
part finish and it does not increase machining time too much.
CNC 8037
·M· MODEL
SOFT: V02.2X
·246·
P r o gr a m m i ng m a n u a l
CONSTANTS
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.
CONSTANTS
12.
HIGH-LEVEL LANGUAGE PROGRAMMING
12.3
CNC 8037
·M· MODEL
SOFT: V02.2X
·247·
Prog ramm in g man u a l
12.4
Operators
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.
+
add.
P1=3 + 4
P1=7
-
subtraction, also a negative value.
P2=5 - 2
P3= -(2 * 3)
P2=3
P3=-6
*
multiplication.
P4=2 * 3
P4=6
/
division.
P5=9 / 2
P5=4.5
MOD
Module or remainder of the division.
P6=7 MOD 4
P6=3
EXP
exponential.
P7=2 EXP 3
P7=8
Operators
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
Relational operators.
EQ
equal.
NE
different.
GT
greater than.
GE
greater than or equal to.
LT
Less than.
LE
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))
Trigonometric functions.
CNC 8037
·M· MODEL
SOFT: V02.2X
·248·
SIN
sine.
P1=SIN 30
P1=0.5
COS
cosine.
P2=COS 30
P2=0.8660
TAN
tangent.
P3=TAN 30
P3=0.5773
ASIN
arc sine.
P4=ASIN 1
P4=90
ACOS
arc cosine.
P5=ACOS 1
P5=0
ATAN
arc tangent.
P6=ATAN 1
P6=45
ARG
ARG(x,y) arctangent y/x.
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°.
P r o gr a m m i ng m a n u a l
Other functions.
P1=ABS -8
P1=8
LOG
decimal logarithm.
P2=LOG 100
P2=2
SQRT
square root.
P3=SQRT 16
P3=4
ROUND
rounding up an integer number.
P4=ROUND 5.83
P4=6
FIX
Integer.
P5=FIX 5.423
P5=5
FUP
if integer takes integer.
if not, takes entire part + 1.
P6=FUP 7
P6=FUP 5,423
P6=7
P6=6
BCD
converts given number to BCD.
P7=BCD 234
P7=564
0010
BIN
converts given number to binary.
P8=BIN $AB
0011
12.
0100
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
9C
Binary
0000 0000 0000 0000 0000 0000 1001 1100
BCD
0000 0000 0000 0000 0000 0001 0101 0110
Operators
absolute value.
HIGH-LEVEL LANGUAGE PROGRAMMING
ABS
CNC 8037
·M· MODEL
SOFT: V02.2X
·249·
Prog ramm in g man u a l
12.5
Expressions
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.
12.5.1
Expressions
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
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.
OR
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)
CNC 8037
·M· MODEL
SOFT: V02.2X
·250·
P r o gr a m m i ng m a n u a l
12.5.2
Relational expressions
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)
The result of these expressions is either true or false.
HIGH-LEVEL LANGUAGE PROGRAMMING
(IF ((P8 EQ 12.8) OR (ABS(SIN(P24)) GT SPEED)) AND (CLOCK LT (P9 * 10.99)) ...
Expressions
12.
At the same time these conditions can be joined by means of logic operators.
CNC 8037
·M· MODEL
SOFT: V02.2X
·251·
Prog ramm in g man u a l
Expressions
HIGH-LEVEL LANGUAGE PROGRAMMING
12.
CNC 8037
·M· MODEL
SOFT: V02.2X
·252·
PROGRAM CONTROL
INSTRUCTIONS
13
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.
• 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 8037
·M· MODEL
SOFT: V02.2X
·253·
Prog ramm in g man u a l
13.1
Assignment instructions
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.
Assignment instructions
PROGRAM CONTROL INSTRUCTIONS
13.
CNC 8037
·M· MODEL
SOFT: V02.2X
·254·
(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 ",".
P r o gr a m m i ng m a n u a l
Display instructions
(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).
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)
Display instructions
13.
(ERROR integer, "error text")
PROGRAM CONTROL INSTRUCTIONS
13.2
(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
CNC 8037
·M· MODEL
SOFT: V02.2X
·255·
Prog ramm in g man u a l
13.3
Enable-disable 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.
Enable-disable instructions
PROGRAM CONTROL INSTRUCTIONS
13.
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)
; Start of single block
G02 X20 Y20 I20 J-10
G01 X40 Y20
G01 X40 Y40 F10000
G01 X20 Y40 F8000
(DSBLK)
; Cancellation of single block
G01 X10 Y10
M30
(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 8037
·M· MODEL
SOFT: V02.2X
·256·
P r o gr a m m i ng m a n u a l
13.4
Flow control instructions
The GOTO and RPT instructions cannot be used in programs that are executed from a PC connected
through the serial line.
( GOTO N(expression) )
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.
X10
N22
(GOTO N22)
; Jump instruction
X15 Y20
; It is not executed
Y22 Z50
; It is not executed
G01 X30 Y40 Z40 F1000
; Continues execution in this block
G02 X20 Y40 I-5 J-5
...
( 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.
PROGRAM CONTROL INSTRUCTIONS
G00 X0 Y0 Z0 T2 D4
Flow control instructions
13.
The jump label can be addressed by means of a number or by any expression which results in a
number.
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.
i
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.
(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.
CNC 8037
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)
·M· MODEL
SOFT: V02.2X
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)
·257·
Prog ramm in g man u a l
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:
Flow control instructions
PROGRAM CONTROL INSTRUCTIONS
13.
CNC 8037
·M· MODEL
SOFT: V02.2X
·258·
(IF (E EQ 10) M10) ó (IF (P5 EQ 10) P12=10)
P r o gr a m m i ng m a n u a l
Subroutine instructions
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 hard disk (KeyCF) or in a PC connected through the serial line, copy it first
into the CNC's RAM memory.
(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
Range of OEM (manufacturer's) subroutines
SUB 10000 - SUB 20000
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.
13.
Subroutine instructions
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.
PROGRAM CONTROL INSTRUCTIONS
13.5
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
CNC 8037
·M· MODEL
SOFT: V02.2X
·259·
Prog ramm in g man u a l
( 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.
Subroutine instructions
PROGRAM CONTROL INSTRUCTIONS
13.
Programming example.
G90 G00 X30 Y20 Z10
(CALL 10)
G90 G00 X60 Y20 Z10
(CALL 10)
M30
CNC 8037
·M· MODEL
SOFT: V02.2X
·260·
(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)
(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)
; Drilling and threading
; Drilling and threading
; Drilling and threading
; Drilling and threading
; Drilling canned cycle
; Threading canned cycle
P r o gr a m m i ng m a n u a l
(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.
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
(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
G84 Z-8 I-22 K15 F500 S2000 T2 D2
G80
(RET)
Subroutine instructions
Programming example.
13.
PROGRAM CONTROL INSTRUCTIONS
Both the main program and each subroutine that is found on a parameter nesting level, will have
26 local parameters (P0-P25).
; Also (PCALL 10, A20, B10)
; Also (PCALL 10, A10, B20)
; Drilling canned cycle
; Threading canned cycle
CNC 8037
·M· MODEL
SOFT: V02.2X
·261·
Prog ramm in g man u a l
(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.
Subroutine instructions
PROGRAM CONTROL INSTRUCTIONS
13.
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.
G90 G00 X30 Y50 Z0
(PCALL 10, P0=20, P1=10)
G90 G00 X60 Y50 Z0
(PCALL 10, P0=10, P1=20)
M30
CNC 8037
·M· MODEL
SOFT: V02.2X
·262·
(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)
P r o gr a m m i ng m a n u a l
13.5.1
Calls to subroutines using G functions
Subroutine calls are made using the CALL and PCALL instructions. In addition to using these
statements, it is also possible to make subroutine calls using specific G functions. This way, the calls
to subroutines are more similar to machine tool language.
Functions G180-G189 and G380-G399 can call the associated OEM and user subroutine as long
as they are global subroutines. G functions cannot be used to call local subroutines.
Up to 30 subroutines may be defined and associated with functions G180-G189 and G380-G399,
and it is also possible to initialize local parameters for each subroutine.
Programming format
The programming format is the following:
G180 <P0..Pn>
<P0..Pn> Optional. Initializing parameters.
Example:
G183 P1=12.3 P2=6
G187 A12.3 B45.3 P10=6
PROGRAM CONTROL INSTRUCTIONS
Functions G180-G189 and G380-G399 are not modal.
Subroutine instructions
13.
When executing one of these functions, its associated subroutine will be executed.
Defining local parameters.
The values of the parameters are defined after the call function and they may be defined using the
name of the parameter (P0-P25) or using letters (A-Z) so "A" is the same as P0 and "Z" is the same
as P25.
Plus, parameters may also be programmed as follows:
• S=P100
• SP100
In either case, local parameter P18(S) would assume the established global parameter value P100.
The definitions described here may be combined in the same block.
Nesting levels
If the functions initialize local parameters, this instruction generates a new nesting level .
The maximum parameter nesting level is 6, within the 15 nesting level of the subroutines, just like
PCALL instructions.
Identification via PLC
All the G functions are identified through GGS* read-only variables . GGSH and GGSP read-only
variables are used to identify the new G functions via PLC; these variables return the status of the
G functions.
CNC 8037
Executing a call
Each function G180-G189 and G380-G399, has its corresponding subroutine associated with it.
Calling a G function means calling the subroutine of the same name.
·M· MODEL
SOFT: V02.2X
·263·
Prog ramm in g man u a l
13.6
Interruption-subroutine instructions
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)
Interruption-subroutine instructions
PROGRAM CONTROL INSTRUCTIONS
13.
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 XY axes, the Z axis is the longitudinal axis. To reposition first
the X and Y axes and finally the Z axis.
This repositioning move may be defined in any of the following ways:
(REPOS X, Y, Z)(REPOS X, Z)(REPOS 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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·264·
P r o gr a m m i ng m a n u a l
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.....)
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).
HD
in the Hard Disk (KeyCF).
DNC2
in a PC connected through the serial line.
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.
Program instructions
13.
( EXEC P(expression), (directory) )
PROGRAM CONTROL INSTRUCTIONS
13.7
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):
HD
in the Hard Disk (KeyCF).
DNC2
in a PC connected through the serial line.
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.
( 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.
CNC 8037
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).
HD
in the Hard Disk (KeyCF).
DNC2
in a PC connected through the serial line.
DNCE
in a PC connected through Ethernet.
·M· MODEL
SOFT: V02.2X
·265·
Prog ramm in g man u a l
Parameter A/D is used when the program to be edited already exists.
A
The CNC appends the new blocks after the ones already existing.
D
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
in the program directory.
To edit blocks, the WRITE instruction must be used as described next.
Program instructions
PROGRAM CONTROL INSTRUCTIONS
13.
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, or in the hard disk (KeyCF) 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)
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.
Using the character "$" in the WRITE instruction to write the number of a parameter:
While using the character "$" in the WRITE instruction, it will be possible to write the parameter
number directly. For that, use the "$" character followed by "P" as long is it is preceded by an axis.
For example, programming (WRITE X$P100) the result will be: XP100.
To show something in $, the value must be programmed after the $ sign. But, to take the value from
a parameter, put a space between the "$" sign and the parameter.
In short, these are the options:
• When programmed $P, it will output $P.
• When programmed $[space]P, it will output $[space] and the content of P.
• When programmed $[number], it will output $[number].
CNC 8037
Example:
Being parameter P100=22.
·M· MODEL
SOFT: V02.2X
·266·
Program
Result
(WRITE XP100)
X22
(WRITE X$P100)
XP100
(WRITE $ P100)
$ 22
(WRITE $3000)
$3000
P r o gr a m m i ng m a n u a l
Example of the creation of a program which contains several points of a cardioid:
| R = B cos (Q/2) |
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
Program instructions
Subroutine number 2 is used, its parameters having the following meaning:
PROGRAM CONTROL INSTRUCTIONS
13.
Program generating subroutine.
N100
(SUB 2)
(OPEN P12345)
(WRITE FP3)
(P10=P1*(ABS(COS(P0/2))))
(WRITE G01 G05 RP10 QP0)
(P0=P0+P2)
(IF (P0 LT 365) GOTO N100)
(WRITE M30)
(RET)
;
;
;
;
;
;
Starts editing of program P12345
Selects machining feedrate
Calculates R
Movement block
New angle
If angle smaller than 365º, calculates new
point
; End of program block
; End of subroutine
CNC 8037
·M· MODEL
SOFT: V02.2X
·267·
Prog ramm in g man u a l
13.8
Screen customizing instructions
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.
Screen customizing instructions
PROGRAM CONTROL INSTRUCTIONS
13.
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.
( 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.
From V02.03 and following versions, the JPG/JPEG formats are supported. This way, if there is an
"n.jpg", "n.jpeg" or "n.pan", the screen will display this file. When having several files, the order of
priorities will be the following:
1. "n.jpg".
2. "n.jpeg".
3. "n.pan".
The format of the JPG/JPEG files must be a 3 digit number. For example "001.jpg" for page 1. The
size of the page must be 638x335.
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.
From V02.03 and following versions, the PNG format is supported. This way, if there is an "n.png"
file, it will be displayed in the position indicated by the expressions 2 and 3. If it is missing, it will display
the "n.sim" file. The format of the PNG files must be a 3 digit 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).
(IB (expression) = INPUT "text", format)
CNC 8037
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.
·M· MODEL
SOFT: V02.2X
·268·
P r o gr a m m i ng m a n u a l
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.
PROGRAM CONTROL INSTRUCTIONS
Screen customizing instructions
13.
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.
CNC 8037
·M· MODEL
SOFT: V02.2X
·269·
Prog ramm in g man u a l
( 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).
Screen customizing instructions
PROGRAM CONTROL INSTRUCTIONS
13.
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:
N10
(ODW 1, 6, 33)
; Defines data window 1
(ODW 2, 14, 33)
; Defines data window 2
(DW1=DATE, DW2=TIME)
; Displays the date in window 1 and the time in 2
(GOTO N10)
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.
CNC 8037
(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.
·M· MODEL
SOFT: V02.2X
·270·
Expression 1, expression 2, expression 3, .... may contain a number or any expression which may
result in a number.
P r o gr a m m i ng m a n u a l
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")
MAXIMUN POINT
(SK 1="FEED", SK 2=" _ _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.
The pressed key will be recorded in the KEY variable.
...
(WKEY)
(IF KEY EQ $FC00 GOTO N1000)
...
13.
MAXIMUN POINT
; Wait for key
; If key F1 has been pressed, continue in N1000
PROGRAM CONTROL INSTRUCTIONS
FEED
Screen customizing instructions
HELP
( 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 entry 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
CNC 8037
·M· MODEL
SOFT: V02.2X
·271·
Prog ramm in g man u a l
• ( 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.
Screen customizing instructions
PROGRAM CONTROL INSTRUCTIONS
13.
(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.
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.
Displays the initial editing page (screen)
N0
(PAGE 10 )
Sets the softkeys to access the various modes and requests a choice
N5
CNC 8037
·M· MODEL
SOFT: V02.2X
·272·
(SK 1="CYCLE 1",SK 2="CYCLE 2",SK 7="EXIT")
(WKEY )
(IF KEY EQ $FC00 GOTO N10)
; Request a key
; Cycle 1
(IF KEY EQ $FC01 GOTO N20)
(IF KEY EQ $FC06 SYSTEM ELSE GOTO N5)
; Cycle 2
; Quit or request a key
P r o gr a m m i ng m a n u a l
CICLO 1
; Displays page 11 and defines 2 data entry windows
N10
(PAGE 11)
(ODW 1,10,60)
(ODW 2,15,60)
;Editing
(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.
(WBUF ")")
(WBUF )
; Adds ")" to the block being edited.
; Enters the edited block into memory.
; For example : (PCALL 1, X2, Y3)
(GOTO N0)
CICLO 2
; Displays page 12 and defines 3 data entry windows
N20
13.
Screen customizing instructions
; Adds "(PCALL 1," to the block being edited.
PROGRAM CONTROL INSTRUCTIONS
(WBUF "( PCALL 1,")
(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.
(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)
;
;
;
;
(WBUF ")")
; Adds ")" to the block being edited.
(WBUF )
; Enters the edited block into memory.
For example: (PCALL 2, A3, B1, C3).
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.
(GOTO N0)
CNC 8037
·M· MODEL
SOFT: V02.2X
·273·
Prog ramm in g man u a l
Screen customizing instructions
PROGRAM CONTROL INSTRUCTIONS
13.
CNC 8037
·M· MODEL
SOFT: V02.2X
·274·
ANGULAR TRANSFORMATION OF
AN INCLINE AXIS
14
With the angular transformation of an incline axis, it is possible to make 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 configured in a Cartesian way, they are not perpendicular to each
other. A typical case is the X axis of a lathe that for sturdiness reasons is not perpendicular to the
Z axis.
X
X'
X
Cartesian axis.
X'
Angular axis.
Z
Orthogonal axis.
Z
Programming in the Cartesian system (Z-X) requires activating an angular transformation of an
inclined plane that converts the movements of the real (non-perpendicular) axes (Z-X'). This way,
a movement programmed on the X axis is transformed into movements on the Z-X' axes; i.e. it then
moves along the Z axis and 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 the reset, turning the CNC off and of the 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 8037
·M· MODEL
SOFT: V02.2X
·275·
Prog ramm in g man u a l
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.
If the angular transformation is active, the coordinates displayed will be those of the Cartesian
system. Otherwise, it will display the coordinates of the real axes.
The following operations are possible while the transformation is active:
• Zero offsets.
ANGULAR TRANSFORMATION OF AN INCLINE AXIS
14.
CNC 8037
·M· MODEL
SOFT: V02.2X
·276·
• 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.
Machine reference zero (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.
P r o gr a m m i ng m a n u a l
Turning angular transformation on and off
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.
G46 S1
This instruction turns a "frozen" (suspended) transformation on again. See "14.2 Freezing the
angular transformation" on page 278.
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.
Turning angular transformation on and off
14.
The angular transformation is turned on using function G46 whose programming format is:
ANGULAR TRANSFORMATION OF AN INCLINE AXIS
14.1
CNC 8037
·M· MODEL
SOFT: V02.2X
·277·
Prog ramm in g man u a l
14.2
Freezing the angular transformation
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
Freezing the angular transformation
ANGULAR TRANSFORMATION OF AN INCLINE AXIS
14.
CNC 8037
·M· MODEL
SOFT: V02.2X
·278·
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".
P r o gr a m m i ng m a n u a l
APPENDIX
A. ISO code programming............................................................................ 281
B. Program control instructions.................................................................... 283
C. Summary of internal CNC variables........................................................ 285
D. Key code .................................................................................................. 291
E. Maintenance............................................................................................. 293
CNC 8037
SOFT: V02.2X
·279·
P r o gr a m m i ng m a n u a l
ISO CODE PROGRAMMING
Function
M
D
V
G00
*
?
*
Rapid traverse
G01
*
?
*
Linear interpolation
G02
*
*
Clockwise circular (helical) interpolation
6.3 / 6.7
G03
*
*
Counterclockwise circular (helical) interpolation
6.3 / 6.7
Dwell/interruption of block preparation
7.1 / 7.2
G05
*
?
G06
G07
*
*
Round corner
*
Circle center in absolute coordinates
?
Square corner
Section
6.1
6.2
7.3.2
6.4
7.3.1
G08
*
Arc tangent to previous path
6.5
G09
*
Arc defined by three points
6.6
G10
*
G11
*
G12
G13
*
Mirror image cancellation
7.5
*
Mirror image on X axis
7.5
*
*
Mirror image on Y axis
7.5
*
*
Mirror image on Z axis
7.5
G14
*
*
Mirror image in the programmed directions
7.5
G15
*
*
Longitudinal axis selection
8.2
G16
*
*
Main plane selection by two addresses and longitudinal axis
3.2
G17
*
?
*
Main plane X-Y and longitudinal Z
3.2
G18
*
?
*
Main plane Z-X and longitudinal Y
3.2
G19
*
*
Main plane Y-Z and longitudinal X
3.2
Definition of lower work zone limits
3.7.1
G20
G21
G22
Definition of upper work zone limits.
3.7.1
*
Enable/disable work zones.
3.7.2
G32
*
*
Feedrate "F" as an inverted function of time.
6.15
G33
*
*
Electronic threading
6.12
Variable-pitch threading
6.13
G34
G36
*
Corner rounding
6.10
G37
*
Tangential entry
6.8
G38
*
Tangential exit
6.9
G39
*
Chamfer
6.11
G40
*
Cancellation of tool radius compensation
8.1
G41
*
*
*
Left-hand tool radius compensation
8.1
G41 N
*
*
Collision detection
8.3
G42
*
*
Right-hand tool radius compensation
8.1
G42 N
*
*
Collision detection
8.3
G43
*
?
*
Tool length compensation
8.2
G44
*
?
G50
*
*
Controlled corner rounding
G51
*
*
Look-Ahead
7.4
*
Movement until making contact
6.14
G52
G53
Cancellation of tool length compensation
8.2
7.3.3
*
Programming with respect to machine zero
G54
*
*
Absolute zero offset 1
4.4.2
G55
*
*
Absolute zero offset 2
4.4.2
G56
*
*
Absolute zero offset 3
4.4.2
G57
*
*
Absolute zero offset 4
4.4.2
G58
*
*
Additive zero offset 1
4.4.2
G59
*
*
Additive zero offset 2
4.4.2
4.3
G60
*
Multiple machining in a straight line
10.1
G61
*
Multiple machining in rectangular pattern
10.2
I*
*
Grid pattern canned cycle
10.3
G63
*
Multiple machining in a circular pattern
10.4
G64
*
Multiple machining in an arc
10.5
G65
*
Machining programmed with an arc-chord
10.6
*
Drilling canned cycle with variable peck
9.6
*
Programming in inches
3.3
Programming in millimeters
3.3
G69
*
G70
*
?
G71
*
?
A.
ISO code programming
G04
Meaning
CNC 8037
·M· MODEL
SOFT: V02.2X
·281·
Prog ramm in g man u a l
Function
M
D
V
G72
*
*
General and specific scaling factor
7.6
G73
*
*
Rotation of the coordinate system
7.7
G74
*
Machine reference (home) search
4.2
G75
*
Probing move until touching
11.1
G76
*
Probing move while touching
11.1
Canned cycle parameter modification
9.2.1
G79
ISO code programming
A.
*
Meaning
Section
G80
*
Canned cycle cancellation
9.3
G81
*
*
Drilling canned cycle
9.7
G82
*
*
Drilling canned cycle with dwell
9.8
G83
*
*
Deep-hole drilling canned cycle with constant peck
9.9
G84
*
*
Tapping canned cycle
9.10
G85
*
*
Reaming canned cycle
9.11
G86
*
*
Boring canned cycle with withdrawal in G00
9.12
G87
*
*
Rectangular pocket canned cycle.
9.13
G88
*
*
Circular pocket canned cycle
9.14
G89
*
*
Boring canned cycle with withdrawal in G01
9.15
G90
*
?
Absolute programming:
3.4
G91
*
?
*
G92
Coordinate preset / spindle speed limit
G93
G94
Incremental programming
Polar origin preset
*
?
G95
*
?
G96
*
G97
*
*
G98
*
*
G99
*
3.4
4.4.1
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 cycle
9.5
M means modal, i.e. the G function, once programmed, remains active until another incompatible
G function is 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.
The letter V means that the G code is displayed next to the current machining conditions in the
execution and simulation modes.
CNC 8037
·M· MODEL
SOFT: V02.2X
·282·
P r o gr a m m i ng m a n u a l
PROGRAM CONTROL INSTRUCTIONS
Display instructions.
( section 13.2 )
(ERROR integer, "error text")
Stops the execution of the program and displays the indicated error.
(DGWZ expression 1, ..... expression 6)
Define the graphics area.
Enabling and disabling instructions.
( section 13.3 )
(ESBLK and DSBLK)
The CNC executes all the blocks between ESBLK and DSBLK as if it were a single block.
Program control instructions
B.
(MSG "message")
Displays the indicated message.
(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 13.4 )
( GOTO N(expression) )
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 13.5 )
(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.
CNC 8037
(MCALL (expression), (assignment instruction), (assignment instruction),...) )
Same as the PCALL instruction, but making the indicated subroutine modal.
( MDOFF )
Cancellation of modal subroutine.
·M· MODEL
SOFT: V02.2X
·283·
Prog ramm in g man u a l
Interruption-subroutine instructions.
( section 13.6 )
( 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.
Program instructions.
B.
Program control instructions
( section 13.7 )
( 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.
Screen customizing instructions.
( section 13.8 )
( 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 entry window.
CNC 8037
( 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.
·M· MODEL
SOFT: V02.2X
·284·
P r o gr a m m i ng m a n u a l
SUMMARY OF INTERNAL CNC VARIABLES.
• 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
( section 12.2.2 )
DNC
TOOL
R
R
R
Number of the active tool.
TOD
R
R
R
Number of active tool offset.
NXTOOL
R
R
R
Number of the next requested tool waiting for M06.
NXTOD
R
R
R
Number of the next tool’s offset.
TMZPn
R
R
-
(n) tool’s position in the tool magazine.
PTOOL
R
-
-
Magazine position to leave the current tool.
PNXTOOL
R
-
-
Magazine position to pick up the next tool.
TLFDn
R/W
R/W
-
(n) tool’s offset number.
TLFFn
R/W
R/W
-
(n) tool’s family code.
TLFNn
R/W
R/W
-
Nominal life assigned to tool (n).
TLFRn
R/W
R/W
-
Real life value of tool (n).
TMZTn
R/W
R/W
-
Contents of tool magazine position (n).
HTOR
R/W
R
R
Tool radius being used by the CNC to do the calculations.
TORn
R/W
R/W
-
Tool radius value of offset (n).
TOLn
R/W
R/W
-
Tool length value of offset (n).
TOIn
R/W
R/W
-
Tool radius wear of offset (n).
TOKn
R/W
R/W
-
Tool length wear of offset (n).
C.
Summary of internal CNC variables.
Variable
Variables associated with zero offsets.
Variable
( section 12.2.3 )
CNC
PLC
DNC
ORG(X-C)
R
R
-
Active zero offset on the selected axis. The value of the additive offset
indicated by the PLC is not included.
PORGF
R
-
R
Abscissa coordinate value of polar origin.
PORGS
R
-
R
Ordinate coordinate value of polar origin.
ORG(X-C)n
R/W
R/W
R
Zero offset (n) value of the selected axis.
PLCOF(X-C)
R/W
R/W
R
Value of the additive zero offset activated via PLC.
ADIOF(X-C)
R
R
R
Value for the selected axis of the zero offset with additive handwheel.
ADDORG (X-C)
R
R
R
Value of the active incremental zero offset corresponding to the selected
axis.
EXTORG
R
R
R
Value of the active absolute zero offset.
Variables associated with machine parameters.
Variable
( section 12.2.4 )
CNC
PLC
DNC
MPGn
R
R
-
MP(X-C)n
R
R
-
Value assigned to (X-C) axis machine parameter (n).
MPSn
R
R
-
Value assigned to machine parameter (n) of the main spindle.
MPLCn
R
R
-
Value assigned to machine parameter (n) of the PLC.
Value assigned to general machine parameter (n).
CNC 8037
·M· MODEL
SOFT: V02.2X
·285·
Prog ramm in g man u a l
Work zone related variables.
Summary of internal CNC variables.
C.
( section 12.2.5 )
Variable
CNC
PLC
DNC
FZONE
R
R/W
R
Status of work zone 1.
FZLO(X-C)
R
R/W
R
Work zone 1. Lower limit along the selected axis (X/C).
FZUP(X-C)
R
R/W
R
Work zone 1. Upper limit along the selected axis (X-C).
SZONE
R
R/W
R
Status of work zone 2.
SZLO(X-C)
R
R/W
R
Work zone 2. Lower limit along the selected axis (X/C).
SZUP(X-C)
R
R/W
R
Work zone 2. Upper limit along the selected axis (X-C).
TZONE
R
R/W
R
Status of work zone 3.
TZLO(X-C)
R
R/W
R
Work zone 3. Lower limit along the selected axis (X/C).
TZUP(X-C)
R
R/W
R
Work zone 3. Upper limit along the selected axis (X-C).
FOZONE
R
R/W
R
Status of work zone 4.
FOZLO(X-C)
R
R/W
R
Work zone 4. Lower limit along the selected axis (X/C).
FOZUP(X-C)
R
R/W
R
Work zone 4. Upper limit along the selected axis (X-C).
FIZONE
R
R/W
R
Status of work zone 5.
FIZLO(X-C)
R
R/W
R
Work zone 5. Lower limit along the selected axis (X/C).
FIZUP(X-C)
R
R/W
R
Work zone 5. Upper limit along the selected axis (X-C).
Feedrate related variables.
Variable
CNC
PLC
( section 12.2.6 )
DNC
FREAL
R
R
R
Real feedrate of the CNC in mm/min or inch/min.
FREAL(X-C)
R
R
R
Actual (real) CNC feedrate of the selected axis.
FTEO/X-C)
R
R
R
Theoretical CNC feedrate of the selected axis.
Variables associated with function G94.
FEED
R
R
DNCF
R
R
R
Active feedrate at the CNC in mm/min or inch/min.
PLCF
R
R/W
R
Feedrate selected via PLC.
PRGF
R
R
R
Feedrate selected by program.
R/W Feedrate selected via DNC.
Variables associated with function G94.
FPREV
R
R
DNCFPR
R
R
R
Active feedrate at CNC, in m/rev or inch/rev.
PLCFPR
R
R/W
R
Feedrate selected via PLC.
PRGFPR
R
R
R
Feedrate selected by program.
R/W Feedrate selected via DNC.
Variables associated with function G94.
PRGFIN
R
R
R
Feedrate selected by program, in 1/min.
Variables associated with feedrate override (%)
FRO
CNC 8037
·M· MODEL
SOFT: V02.2X
·286·
R
R
R
Feedrate Override (%) active at the CNC.
PRGFRO
R/W
R
R
Override (%) selected by program.
DNCFRO
R
R
PLCFRO
R
R/W
R
Override (%) selected via PLC.
CNCFRO
R
R
R
Override (%) selected from the front panel knob.
PLCCFR
R
R/W
R
Override (%) of the PLC execution channel.
R/W Override (%) selected via DNC.
P r o gr a m m i ng m a n u a l
Coordinate related variables.
CNC
PLC
( section 12.2.7 )
DNC
PPOS(X-C)
R
-
-
Programmed theoretical position value (coordinate).
POS(X-C)
R
R
R
Machine coordinates. Real coordinates of the tool base.
TPOS(X-C)
R
R
R
Machine coordinates. Theoretical coordinates of the tool base.
APOS(X-C)
R
R
R
Part coordinates. Real coordinates of the tool base.
ATPOS(X-C)
R
R
R
Part coordinates. Theoretical coordinates of the tool base.
DPOS(X-C)
R
R
R
Theoretical position of the probe when the probe touched the part.
FLWE(X-C)
R
R
R
Following error of the indicated axis.
DIST(X-C)
R/W
R/W
R
Distance traveled by the indicated axis.
LIMPL(X-C)
R/W
R/W
R
Second upper travel limit.
LIMMI(X-C)
R/W
R/W
R
Second lower travel limit.
DPLY(X-C)
R
R
R
Coordinate of the selected axis displayed on the screen.
GPOS(X-C)n p
R
-
-
Coordinate of the selected axis, programmed in the (n) block of the program
(p).
Variables associated with electronic handwheels.
Variable
CNC
PLC
( section 12.2.8 )
DNC
HANPF
R
R
-
Pulses received from 1st handwheel since the CNC was turned on.
HANPS
R
R
-
Pulses received from 2nd handwheel since the CNC was turned on.
HANPT
R
R
-
Pulses received from 3rd handwheel since the CNC was turned on.
HANPFO
R
R
-
Pulses received from 4th handwheel since the CNC was turned on.
HANDSE
R
R
HANFCT
R
R/W
R
Multiplying factor different for each handwheel (when having several).
HBEVAR
R
R/W
R
HBE handwheel. Reading enabled, axis being jogged and multiplying factor
(x1, x10, x100).
MASLAN
R/W
R/W
R/W
C.
Summary of internal CNC variables.
Variable
For handwheels with a selector button, it indicates whether that button has
been pressed or not.
Linear path angle for "Path handwheel" or "Path Jog" mode.
MASCFI
R/W
R/W
R/W
Arc center coordinates for "Path handwheel mode" or "Path jog".
MASCSE
R/W
R/W
R/W
Arc center coordinates for "Path handwheel mode" or "Path jog".
Feedback related variables.
Variable
( section 12.2.9 )
CNC
PLC
DNC
ASIN(X-C)
R
R
R
A signal of the CNC's sinusoidal feedback for the selected axis.
BSIN(X-C)
R
R
R
B signal of the CNC's sinusoidal feedback for the selected axis.
ASINS
R
R
R
"A" signal of the CNC's sinusoidal feedback for the spindle.
BSINS
R
R
R
"B" signal of the CNC's sinusoidal feedback for the spindle.
Variables associated with the main spindle.
( section 12.2.10 )
Variable
CNC
PLC
DNC
SREAL
R
R
R
Real spindle speed.
FTEOS
R
R
R
Theoretical spindle speed.
Variables associated with spindle speed.
SPEED
R
R
R
Active spindle speed at the CNC.
DNCS
R
R
R/W
Spindle speed selected via DNC.
PLCS
R
R/W
R
Spindle speed selected via PLC.
PRGS
R
R
R
Spindle speed selected by program.
CNC 8037
Variables associated with the spindle override.
SSO
PRGSSO
R
R
R
Spindle Speed Override (%) active at the CNC.
R/W
R
R
Override (%) selected by program.
DNCSSO
R
R
R/W
Override (%) selected via DNC.
PLCSSO
R
R/W
R
Override (%) selected via PLC.
CNCSSO
R
R
R
Spindle Speed Override (%) selected from front panel.
·M· MODEL
SOFT: V02.2X
·287·
Prog ramm in g man u a l
Speed limit related variables.
SLIMIT
R
R
DNCSL
R
R
PLCSL
R
R/W
R
Spindle speed limit active at the CNC.
R/W Spindle speed limit selected via DNC.
R
Spindle speed limit selected via PLC.
PRGSL
R
R
R
Spindle speed limit selected by program.
MDISL
R
R/W
R
Maximum machining spindle speed.
Position related variables.
Summary of internal CNC variables.
C.
POSS
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).
RPOSS
R
R
R
Real spindle position.
Reading from the PLC in ten-thousandths of a degree (between -3600000
and 3600000) and from the CNC in degrees (between -360 and 360).
TPOSS
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).
RTPOSS
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).
PRGSP
R
R
R
Position programmed in M19 via program for the main spindle.
Variables related to the following error.
FLWES
R
R
R
Spindle following error.
PLC related variables.
Variable
PLCMSG
CNC
PLC
DNC
( section 12.2.11 )
R
-
R
Number of the active PLC message with the highest priority.
PLCIn
R/W
-
-
32 PLC inputs starting from (n).
PLCOn
R/W
-
-
32 PLC outputs starting from (n).
PLCMn
R/W
-
-
32 PLC marks starting from (n).
PLCRn
R/W
-
-
(n) Register.
PLCTn
R/W
-
-
Indicated (n) Timer’s count.
PLCCn
R/W
-
-
Indicated (n) Counter’s count.
PLCMMn
R/W
-
-
Modifies the (n) mark of the PLC.
Variables associated with local and global parameters.
Variable
CNC
PLC
( section 12.2.12 )
DNC
GUP n
-
R/W
-
Global parameter (P100-P299) (n).
LUP (a,b)
-
R/W
-
Indicated local (P0-P25) parameter (b) of the nesting level (a).
CALLP
R
-
-
Indicates which local parameters have been defined by means of a PCALL
or MCALL instruction (calling a subroutine).
Operating-mode related variables.
Variable
OPMODE
CNC 8037
·M· MODEL
SOFT: V02.2X
·288·
CNC
PLC
DNC
R
R
R
( section 12.2.13 )
Operation mode.
P r o gr a m m i ng m a n u a l
Other variables.
CNC
PLC
( section 12.2.14 )
DNC
NBTOOL
R
-
R
Number of the tool being managed..
PRGN
R
R
R
Number of the program in execution.
BLKN
R
R
R
Label number of the last executed block.
GSn
R
-
-
Status of the indicated G function (n).
GGSA
-
R
R
Status of functions G00 thru G24.
GGSB
-
R
R
Status of functions G25 thru G49.
GGSC
-
R
R
Status of functions G50 thru G74.
GGSD
-
R
R
Status of functions G75 thru G99.
GGSE
-
R
R
Status of functions G100 thru G124.
GGSF
-
R
R
Status of functions G125 thru G149.
GGSG
-
R
R
Status of functions G150 thru G174.
GGSH
-
R
R
Status of functions G175 thru G199.
GGSI
-
R
R
Status of functions G200 thru G224.
GGSJ
-
R
R
Status of functions G225 thru G249.
GGSK
-
R
R
Status of functions G250 thru G274.
GGSL
-
R
R
Status of functions G275 thru G299.
GGSM
-
R
R
Status of functions G300 through G324.
GGSN
-
R
R
Status of functions G325 thru G349.
GGSO
-
R
R
Status of functions G350 thru G374.
GGSP
-
R
R
Status of functions G375 thru G399.
GGSQ
-
R
R
Status of functions G400 thru G424.
MSn
R
-
-
Status of the indicated M function (n)
GMS
-
-
R
Status of M functions: M (0..6, 8, 9, 19, 30, 41..44).
PLANE
R
R
R
Abscissa and ordinate axes of the active plane.
LONGAX
R
R
R
Axis affected by the tool length compensation (G15).
MIRROR
R
R
R
Active mirror images.
SCALE
R
R
R
General scaling factor applied. Reading from the PLC in ten-thousandths.
SCALE(X-C)
R
R
R
Scaling Factor applied only to the indicated axis. Reading from the PLC in
ten-thousandths.
ORGROT
R
R
R
Rotation angle (G73) of the coordinate system.
ROTPF
R
-
-
Abscissa of rotation center.
ROTPS
R
-
-
Ordinate of rotation center.
PRBST
R
R
R
Returns probe status.
CLOCK
R
R
R
System clock in seconds.
TIME
R
R
R/W
DATE
R
R
R/W
Date in year-month-day format.
R/W
R/W
R/W
Clock activated by PLC, in seconds.
CYTIME
R
R
R
PARTC
R/W
R/W
R/W
FIRST
R
R
R
KEY
R/W
R/W
R/W
keystroke code.
KEYSRC
R/W
R/W
R/W
Source of the keys.
TIMER
Time in hours-minutes-seconds format.
Time to execute a part in hundredths of a second.
Parts counter of the CNC.
First time a program is executed.
ANAIn
R
R
R
ANAOn
R/W
R/W
R/W
CNCERR
-
R
R
Active CNC error number.
PLCERR
-
-
R
Active PLC error number.
DNCERR
-
R
-
Number of the error generated during DNC communications.
Voltage (in volts) of the indicated analog input (n).
Voltage (in volts) to apply to the indicated output (n).
DNCSTA
-
R
-
DNC transmission status.
TIMEG
R
R
R
Remaining time to finish the dwell block (in hundredths of a second).
SELPRO
R/W
R/W
R
When having two probe inputs, it selects the active input.
DIAM
R/W
R/W
R
It changes the programming mode for X axis coordinates between radius
and diameter.
PRBMOD
R/W
R/W
R
Indicates whether a probing error must be displayed or not.
RIP
-
-
-
Linear theoretical feedrate resulting from the next loop (in mm/min).
DISABMOD
R
R/W
R
Disables some actions or modes.
R/W
-
-
Defines the chordal error of the canned cycles.
CYCCHORDERR
C.
Summary of internal CNC variables.
Variable
CNC 8037
·M· MODEL
SOFT: V02.2X
·289·
Prog ramm in g man u a l
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.
Summary of internal CNC variables.
C.
CNC 8037
·M· MODEL
SOFT: V02.2X
·290·
P r o gr a m m i ng m a n u a l
KEY CODE
Alphanumeric operator panel (M-T models)
b
c
e
101
f
j
k
107
l
o
111
p
q
112
113
u
117
v
118
w
119
98
i
103
h
104
105
106
m
109
n
110
ñ
164
r
s
115
t
116
y
z
122
g
114
x
120
121
99
d
100
97
102
65
66
67
68
69
70
108
71
72
73
74
75
76
77
78
79
80
81
82
83
84
85
86
87
88
89
90
91
32
65454
65456
64512
65522
64513
64514
65524
64515
027
64516
64517
61446
65453
65445
65460
65462
64518
65458
65455
013
61447
61452
35
40
61
37
93
33
60
43
61443
53
54
44
50
59
45
57
38
34
49
42
62
56
52
47
36
41
55
91
63
D.
Key code
a
51
58
48
46
65523
65521
65520
CNC 8037
·M· MODEL
SOFT: V02.2X
·291·
Prog ramm in g man u a l
Key code
D.
CNC 8037
·M· MODEL
SOFT: V02.2X
·292·
P r o gr a m m i ng m a n u a l
MAINTENANCE
Cleaning
The accumulated dirt inside the unit may act as a screen preventing the proper dissipation of the
heat generated by the internal circuitry which could result in a harmful overheating of the CNC and,
consequently, possible malfunctions.
To clean the operator panel and the monitor, a smooth cloth should be used which has been dipped
into de-ionized water and /or non abrasive dish-washer soap (liquid, never powder) or 75º alcohol.
Never use air compressed at high pressure to clean the unit because it could cause the accumulation
of electrostatic charges that could result in electrostatic shocks.
E.
Maintenance
On the other hand, accumulated dirt can sometimes act as an electrical conductor and short-circuit
the internal circuitry, especially under high humidity conditions.
The plastics used on the front panel are resistant to :
• Grease and mineral oils.
• Bases and bleach.
• Dissolved detergents.
• Alcohol.
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 manipulate the inside of the unit. Only personnel authorized by Fagor Automation may access
the interior of this unit.
Do not handle the connectors with the unit connected to AC power. Before handling these connectors
(I/O, feedback, etc.), make sure that the unit is not connected to main AC power.
CNC 8037
·M· MODEL
SOFT: V02.2X
·293·
Prog ramm in g man u a l
Maintenance
E.
CNC 8037
·M· MODEL
SOFT: V02.2X
·294·
P r o gr a m m i ng m a n u a l
E.
CNC 8037
SOFT: V02.2X
·295·
Prog ramm in g man u a l
E.
CNC 8037
SOFT: V02.2X
·296·
FAGOR AUTOMATION
Fagor Automation S. Coop.
Bº San Andrés, 19 - Apdo. 144
E-20500 Arrasate-Mondragón, Spain
Tel: +34 943 719 200
+34 943 039 800
Fax: +34 943 791 712
E-mail: [email protected]
www.fagorautomation.com