10 Series CNC
Programming Manual
Code: 45004457K
Rev. 18
PUBLICATION ISSUED BY:
PRIMA ELECTRO S.p.A.
Strada Carignano, 48/2 - 10024 Moncalieri (To) - Italy
Tel. +39-011 9899800
Web: www.osai.it; www.primaelectro.com
e-mail: it.sales@primaelectro.com
Copyright 2011 by PRIMA ELECTRO
All rights reserved
Edition: September 2011
IMPORTANT USER INFORMATION
PRIMA ELECTRO reserves the right to modify and improve the product described in this manual at any time and without prior notice.
This document has been drafted by PRIMA ELECTRO in order to be used by its customers and this is the most updated document related to this product at time of publication.
The application of this manual is under customer responsibility. No further guarantees will be given by PRIMA ELECTRO, in particular for any possible faults, incompleteness and/or difficulties in the operation. In no event will PRIMA ELECTRO responsible or liable for indirect or consequential damages that may result by the use of such documentation.
UPDATE
10 Series CNC Programming Manual
SUMMARY OF CHANGES
General
This publication is issued with reference to Software Release 7.6 (E69).
PAGE |
UPDATING TYPE |
|
|
INDEX |
Updated |
|
|
CHAPTER 2
p. 30-35 Changed paragraphs UDA, SDA, XDA
p.42-45 Changed paragraphs
-Defining/Changing the following ratio
-Activating the following function
-Deactivating the following function
p. 48 |
New paragraph added, ACCESSING AXIS/DRIVE PARAMETERS |
pp.49-54 New paragraphs added
-CPA – Read/Write of a CNC parameter related to an axis
-CPD – Drive Parameter Read/Write
p. 65 |
Changed DYM paragraph |
p. 67 |
Changed MDA paragraph |
p. 69 |
Changed VEF paragraph |
p. 70 |
New paragraph added, CRV – Curve – Velocity Optimization Parameter |
p. 72 |
New paragraph added, MOA – Motion Auxiliary |
p. 74 |
Changed MOV paragraph |
p. 81 |
New value added |
p.92 |
New paragraph added, MOMManual Operating Modality |
p.108 |
Changed ROT paragraph |
p.125 |
Changed UPR paragraph |
p.153 |
New value added in the table |
p.187 New paragraph added, TCP - Tool Centre Point for machines with rotary axis plus balancing axis (Mixed)
p.192 |
New paragraph added, TCP - Tool Centre Point for machines with double |
|
rotary axis on the table (Machine Bed) |
p. 200 |
New paragraph added, REMARKS ON TCP PARAMETERS |
CHAPTER 3 |
|
p. 3 |
Changed description |
CHAPTER 4 |
|
pp. 1-13 |
Changed Cutter diameter compensation paragraph |
p. 22 |
Changed paragraph TPO - Path optimisation on bevels with G41/G42 |
p. 28 |
Added TPO=2 and TPO=3 modes |
p. 31 |
Added TPO=4, TPO=8 and TPO=16 modes |
CHAPTER 9 |
|
p. 8 |
Changed description |
p. 11 |
New paragraph added, DGM – Disable Paramacro scrolling |
10 Series CNC Programming Manual
UPDATE
10 Series CNC Programming Manual
CHAPTER 14 |
|
p. 7 |
Changed SND paragraph |
CHAPTER 17 |
|
p. 5 |
New paragraph added, ERF – Error form |
APP. B |
|
p. 11 |
Changed description for NC133 |
10 Series CNC Programming Manual
Preface
10 Series CNC Programming Manual
PREFACE
This manual describes the procedures used for writing part programs with the 10 Series CNC system. It provides programmers with all the information they need for creating machine control programs.
REFERENCES
For further information:
10 Series CNC - AMP Software Characterization Manual
10 Series CNC - User Guide
The chapters in this manual are organised in sections. They describe the language elements (commands and functions) used for managing a specific task, e.g. axis programming, tool programming, probe management. Programming examples have been introduced in the command description.
SUMMARY
1.Programming with 10 Series System
This chapter contains the general programming rules of the International Standards Organization (ISO) standard. The chapter also provides an overview of the programming environment and a summary of the most used codes.
2.Programming the Axes
This chapter describes axis programming. The G codes and extended commands involved in this activity are provided with their characteristics. Several examples complete the command description and give suggestions for programming the major types of movements.
3.Programming Tools and tool offsets
This chapter describes tool programming and provides the functions and instructions used in tool operation.
10 Series CNC Programming Manual |
1 |
Preface
10 Series CNC Programming Manual
4.Cutter Diameter Compensation
This chapter describes cutter compensation. T functions and G codes used in tool compensation are provided with characteristics and several examples.
5.Programming the Spindle
This chapter describes spindle programming. The G codes and extended commands involved in this activity are provided with their characteristics. Several examples complete the command description and give hints for solving the main cases of spindle programming.
6.Miscellaneous Functions
This chapter describes miscellaneous functions and provides a list of M functions with their meaning and characteristics.
7.Parametric Programming
This chapter deals with special programming applications that use local and system variables.
8.Canned Cycles
This chapter provides a description of the canned cycles available with the control. The G codes and extended commands used in this activity are provided with their characteristics. Several examples complete the command description.
9.Paramacros
This chapter describes how paramacros can be used in programs.
10.Probing Cycles
This chapter provides a description of the probing cycles available with the control. The G codes and extended commands involved in probe management are provided complete with examples.
11.Managing the Screen
This chapter discusses the commands used to handle the system screen from a part programs. Examples are given to complete the command description.
12.Modifying the Program Execution Sequence
This chapter contains the commands used for modifying the sequence of execution of a part program. It describes commands for branching, repeating blocks and executing subprograms, as well as commands for putting the part program on hold and releasing it.
13.High Speed Machining
This chapter describes the high-speed milling features on machine tools with 3 axes.
14.Multiprocess management commands
This chapter shows 10 Series CNC's multi process potentials.
2 |
10 Series CNC Programming Manual |
Preface
10 Series CNC Programming Manual
15.High level geometric programming (GTL)
This chapter discusses the set of programming instructions available with the GTL utility.
16.Working Cycles for Turning Systems
This chapter provides the instructions for programming macro-cycles of rough-shaping, threading and groove cutting.
17.Filters
This chapter describes the various types of filters that can be configured and hence applied in OSAI control units, designed to improve machine tool performances from the geometric and dynamic points of view and hence the finishing quality of the parts produced.
A.Characters and Commands
Appendix A provides a summary of all the characters allowed in the system and gives lists of G codes, mathematical functions and extended commands.
B.Error Messages
Appendix B provides a list of all the error messages that can occur during programming..
C.Error management
10 Series CNC Programming Manual |
3 |
Preface
10 Series CNC Programming Manual
COMMANDS
Commands are dealt with in the chapters that describe the specific task. A common structure has been adopted in the command description. For each command, the following information is provided:
Command name
Command function
Command syntax
Parameters
Characteristics and notes
Examples
Where possible, examples consist of a portion of program and a diagram that shows how the commands in that portion work.
Syntax conventions
Use these conventions with the commands:
SYMBOL |
MEANING |
|
|
[ ] |
Brackets enclose optional entries. Do not enter the brackets. |
{ } |
Braces enclose entries which may be repeated more than once. This could |
|
also be described as a series of alternative entries, i.e. only one of these may |
|
be entered. Alternative entries are separated by a (|). Do not enter the braces |
|
in the command itself. |
| |
A vertical bar separates alternative entries. Do not enter the bar. |
|
|
Key-words are written in bold. They must be entered exactly as they are represented in the syntax description.
Parameters that must be passed with commands are indicated by a mnemonic written in italics. Appropriate values must be entered in place of the mnemonic. Leading zeros can be omitted. For example, you can program G00 as G, G01 as G1.
Example: (SCF,[value])
SCF, the comma and parenthesis are key-words and must be written as described. value is a parameter name and must be replaced by an appropriate value. The brackets indicate that value is an optional value.
4 |
10 Series CNC Programming Manual |
Preface
10 Series CNC Programming Manual
Warnings
For correct control operation, it is important to follow the information given in this manual. Take particular care with topics bearing one of the mentions: WARNING, CAUTION or IMPORTANT, which indicate the following types of information:
Draws attention to facts or circumstances that may cause damage to the control, to the machine or to operators.
WARNING
Indicates information to be followed in order to avoid damage to equipment in
general.
CAUTION
IMPORTANT |
Indicates information that must be followed carefully in order to ensure full |
|
success of the application. |
||
|
Terminology
Some terms appearing throughout the manual are explained below.
Control |
Refers to the 10 Series numerical control unit comprising front panel unit and |
|
basic unit. |
Front Panel |
Is the interface module between machine and operator; it has a monitor on |
|
which messages are output and a keyboard to input the data. It is connected to |
|
the basic unit. |
Basic Unit |
Is the hardware-software unit handling all the machine functions. It is connected |
|
to the front panel and to the machine tool. |
10 Series CNC Programming Manual |
5 |
Preface
10 Series CNC Programming Manual
END OF PREFACE
6 |
10 Series CNC Programming Manual |
Index
10 Series CNC Programming Manual
INDEX
PROGRAMMING WITH 10 SERIES SYSTEMS
THE PROGRAM FILES ................................................................................................... |
1-1 |
Program Components............................................................................................ |
1-2 |
Blocks .................................................................................................................... |
1-2 |
Block Types ........................................................................................................... |
1-4 |
Programmable Functions....................................................................................... |
1-6 |
G Codes................................................................................................................. |
1-9 |
SYNCHRONISATION AND PROGRAM EXECUTION ................................................... |
1-13 |
Default Synchronisation ......................................................................................... |
1-13 |
Overriding Default Synchronisation ....................................................................... |
1-14 |
Part Program Interpreter........................................................................................ |
1-14 |
Sequence of execution .......................................................................................... |
1-15 |
Programming restrictions for long real (double) formats ....................................... |
1-15 |
PROGRAMMING THE AXES
AXIS MOTION CODES.................................................................................................... |
2-1 |
|
Defining Axis Motion .............................................................................................. |
2-1 |
|
G00 |
- Rapid Axes Positioning ................................................................................ |
2-2 |
G01 |
- Linear Interpolation ...................................................................................... |
2-3 |
G02 |
G03 - Circular Interpolation ............................................................................ |
2-4 |
CET (PRC) - Circular Endpoint Tolerance............................................................. |
2-7 |
|
FCT - Full Circle Threshold.................................................................................... |
2-8 |
|
ARM - Defining Arc Normalisation Mode ............................................................... |
2-9 |
|
CRT - Circular interpolation speed reduction threshold ......................................... |
2-13 |
|
CRK - Circular interpolation speed reduction constant .......................................... |
2-13 |
|
Helical Interpolation ............................................................................................... |
2-16 |
|
G33 |
- Constant or Variable Pitch Threading .......................................................... |
2-18 |
Rotary Axes ........................................................................................................... |
2-22 |
|
Axes with Rollover ................................................................................................. |
2-24 |
|
G90 |
- Absolute mode ............................................................................................. |
2-24 |
G91 |
- Incremental mode ........................................................................................ |
2-26 |
Pseudo Axes.......................................................................................................... |
2-27 |
|
Diameter Axes ....................................................................................................... |
2-27 |
|
UDA - Dual Axes.................................................................................................... |
2-30 |
|
SDA - Special Dual Axes ....................................................................................... |
2-32 |
|
XDA - Master/Slave axes....................................................................................... |
2-34 |
|
Master/Slave Association....................................................................................... |
2-34 |
|
10 Series CNC Programming Manual |
i |
Index
10 Series CNC Programming Manual
Syntax .............................................................................................................................. |
2-34 |
Mode 0 ................................................................................................................... |
2-36 |
Mode 1 ................................................................................................................... |
2-37 |
Mode 2 ................................................................................................................... |
2-38 |
Mode 3 ................................................................................................................... |
2-40 |
Releasing the Slave(s) from the Master................................................................. |
2-41 |
Syntax .............................................................................................................................. |
2-41 |
Defining/Changing the following ratio..................................................................... |
2-42 |
Syntax .............................................................................................................................. |
2-42 |
Activating the following function ............................................................................. |
2-43 |
Syntax .............................................................................................................................. |
2-43 |
Deactivating the following function ......................................................................... |
2-44 |
Syntax .............................................................................................................................. |
2-44 |
AXF – Definition of axes with dynamic following function ...................................... |
2-46 |
ACCESSING AXIS/DRIVE PARAMETERS ..................................................................... |
2-48 |
CPA – Read/Write of a CNC parameter related to an axis .................................... |
2-49 |
CPD – Drive Parameter Read/Write ...................................................................... |
2-53 |
ORIGINS AND COORDINATE CONTROL CODES........................................................ |
2-55 |
G17 G18 G19 - Selecting the Interpolation Plane .................................................. |
2-56 |
G16 - Defining the Interpolation Plane ................................................................... |
2-57 |
G27 G28 G29 - Defining the Dynamic Mode ......................................................... |
2-58 |
AUTOMATIC DECELERATION ON BEVELS IN G27 MODE......................................... |
2-63 |
DLA - Deceleration Look Ahead............................................................................. |
2-64 |
DYM - Dynamic Mode ............................................................................................ |
2-65 |
MDA - Maximum Deceleration Angle ..................................................................... |
2-67 |
VEF - Velocity Factor ............................................................................................. |
2-68 |
CRV – Curve – Velocity Optimization Parameter................................................... |
2-70 |
MOA – Motion Auxiliary.......................................................................................... |
2-72 |
Jerk Limitation ........................................................................................................ |
2-73 |
MOV - Enable Jerk Limitation ................................................................................ |
2-74 |
JRK - Jerk Time Constant ...................................................................................... |
2-83 |
JRS - Jerk Smooth Constant.................................................................................. |
2-85 |
ODH - Online Debug Help...................................................................................... |
2-87 |
MBA – MultiBlock retrace Auxiliary functions ......................................................... |
2-89 |
REM – Automatic return to profile at end of move ................................................. |
2-90 |
IPB (DTL) - In Position Band .................................................................................. |
2-91 |
MOMManual Operating Modality ......................................................................... |
2-92 |
G70 G71 - Measuring Units ................................................................................... |
2-95 |
G90 G91 G79 - Absolute, Incremental and Zero Programming............................. |
2-96 |
G92 G98 G99 - Axis Presetting.............................................................................. |
2-98 |
G04 G09 - Dynamic Mode Attributes ..................................................................... |
2-99 |
t - Block Execution Time ........................................................................................ |
2-100 |
DWT (TMR) - Dwell Time....................................................................................... |
2-100 |
G93 - V/D Feedrate ................................................................................................ |
2-101 |
VFF - Velocity Feed Forward ................................................................................. |
2-102 |
CODES THAT MODIFY THE AXES REFERENCE SYSTEM ......................................... |
2-103 |
SCF - Scale Factors ............................................................................................... |
2-104 |
MIR - Using Mirror Machining................................................................................. |
2-105 |
ROT (URT) - Interpolation Plane Rotation ............................................................. |
2-108 |
UAO - Using Absolute Origins................................................................................ |
2-113 |
UTO (UOT) - Using Temporary Origins ................................................................. |
2-114 |
UIO - Using Incremental Origins ............................................................................ |
2-116 |
RQO - Requalifying Origins.................................................................................... |
2-118 |
OVERTRAVELS AND PROTECTED AREAS ................................................................. |
2-119 |
SOL (DLO) - Software Overtravel Limits................................................................ |
2-120 |
DPA (DSA) - Define Protected Areas..................................................................... |
2-121 |
ii |
10 Series CNC Programming Manual |
|
Index |
|
10 Series CNC Programming Manual |
|
|
|
|
|
PAE (ASC) - Protected Area Enable...................................................................... |
2-123 |
|
PAD (DSC) - Protected Area Disable .................................................................... |
2-123 |
|
VIRTUAL AXES MANAGEMENT .................................................................................... |
2-124 |
|
Virtual Axes............................................................................................................ |
2-124 |
|
Virtual modes available on 10 Series CNC............................................................ |
2-124 |
|
UPR - Rotation of Cartesian axes.......................................................................... |
2-125 |
|
Using UPR ............................................................................................................. |
2-131 |
|
UVP - Programming polar coordinates .................................................................. |
2-136 |
|
Programming examples with polar coordinates..................................................... |
2-138 |
|
UVC - Programming cylindrical coordinates .......................................................... |
2-140 |
|
UVA - Programming non orthogonal axes ........................................................... |
2-142 |
|
Example of programming with polar coordinates .................................................. |
2-143 |
|
TCP - Tool Center Point for machines with "Double Twist" head ......................... |
2-144 |
|
Programming the "m" and "n" parameters (angles)............................................... |
2-160 |
|
Programming the "m", "n", "o" and “u”, “v”, “w” parameters (vectors) ................... |
2-161 |
|
TCP - Tool Center Point for generic 5-axis machines ........................................... |
2-163 |
|
Programming ......................................................................................................... |
2-168 |
|
TCP - Tool Center Point for machines with fixed tool and rotary table .................. |
2-172 |
|
Programming ......................................................................................................... |
2-178 |
|
TCP - Tool Center Point for machines with Prismatic Head .................................. |
2-179 |
|
Programming ......................................................................................................... |
2-186 |
|
TCP - Tool Center Point for machines with rotary axis plus balancing |
|
|
axis (Mixed)............................................................................................................ |
2-187 |
|
Rotary axes table .............................................................................................. |
2-189 |
|
TCP - Tool Center Point for machines with double rotary axis on the |
|
|
table (MachineBed)................................................................................................ |
2-192 |
|
TCP on multi-processor ......................................................................................... |
2-198 |
|
REMARKS ON TCP PARAMETERS .............................................................................. |
2-200 |
|
Dynamic Mode – L356 ........................................................................................... |
2-200 |
|
Operational Limits Mode – L367 ............................................................................ |
2-200 |
|
|
|
|
PROGRAMMING TOOLS AND TOOL OFFSETS |
|
|
T address for programming tools........................................................................... |
3-2 |
|
T address for multi-tool programming.................................................................... |
3-3 |
|
h address ............................................................................................................... |
3-5 |
|
TTR – Toroidal Tool Radius................................................................................... |
3-7 |
|
AXO - Axis Offset Definition................................................................................... |
3-8 |
|
RQT (RQU) - Requalifying Tool Offset .................................................................. |
3-10 |
|
RQP - Requalifying Tool Offset ............................................................................. |
3-11 |
|
TOU (TOF) - Tool Expiry Declaration .................................................................... |
3-12 |
|
LOA - Table loading ............................................................................................... |
3-13 |
|
|
|
|
CUTTER DIAMETER COMPENSATION |
|
|
TTC – Tool Type Compensation............................................................................ |
4-3 |
|
G40 G41 G42 – Tool Compensation ..................................................................... |
4-4 |
|
Enabling Tool Compensation................................................................................. |
4-5 |
|
Tool Diameter Compensation ................................................................................ |
4-5 |
|
Tool Thickness Compensation (TTC, 1)............................................................... |
4-6 |
|
Notes on using tool compensation......................................................................... |
4-10 |
|
Tool path optimisation (TPO)................................................................................. |
4-10 |
|
Disabling Cutter Diameter Compensation ............................................................. |
4-11 |
|
Disabling Compensation with TPO active.............................................................. |
4-12 |
|
10 Series CNC Programming Manual |
iii |
Index
10 Series CNC Programming Manual
Disabling disc thickness compensation.................................................................. |
4-13 |
TOOL DIAMETER COMPENSATION CHANGE............................................................. |
4-14 |
Linear/Linear tool path............................................................................................ |
4-14 |
Linear/Circular, Circular/Linear, Circular/Circular tool paths .................................. |
4-16 |
r - Radiuses in Compensated Profiles.................................................................... |
4-18 |
b - Bevels in Compensated Profiles ....................................................................... |
4-19 |
TPO - Path optimisation on bevels with G41/G42.................................................. |
4-22 |
TPO=1, TPO=33 and TPO=65 Modes ................................................................... |
4-23 |
Examples of profile optimisation with TPO=1 ........................................................ |
4-26 |
TPO=2 mode.......................................................................................................... |
4-28 |
TPO=3 mode.......................................................................................................... |
4-28 |
Examples of TPO=2 mode..................................................................................... |
4-29 |
TPO=4 mode.......................................................................................................... |
4-31 |
TPO=8 and TPO=16 modes .................................................................................. |
4-31 |
TPO=32 mode and 64 mode.................................................................................. |
4-31 |
TPA – Threshold angle for TPO............................................................................. |
4-32 |
TPT - Tool Path Threshold..................................................................................... |
4-33 |
u v w - Paraxial Compensation............................................................................... |
4-35 |
Examples of compensation factor applications u, v, w .......................................... |
4-36 |
UVW – Definition of axes for paraxial compensation............................................. |
4-40 |
MSA (UOV) - Defining a Machining Stock Allowance ............................................ |
4-41 |
AUTOMATIC CONTOUR MILLING................................................................................. |
4-42 |
Limits to use of automatic contour miling............................................................... |
4-42 |
GTP - Get Point...................................................................................................... |
4-43 |
Determining the approach point ............................................................................. |
4-44 |
CCP - Cutter Compensation Profile ....................................................................... |
4-46 |
PROGRAMMING THE SPINDLE
SPINDLE FUNCTIONS .................................................................................................... |
5-1 |
G96 G97 - CSS and RPM Programming ............................................................... |
5-1 |
SSL - Spindle Speed Limit ..................................................................................... |
5-3 |
M19 - Oriented Spindle Stop .................................................................................. |
5-4 |
GTS – Spindle sharing ........................................................................................... |
5-5 |
MISCELLANEOUS FUNCTIONS
Standard M functions ............................................................................................. |
6-1 |
PARAMETRIC PROGRAMMING
LOCAL VARIABLES........................................................................................................ |
7-4 |
E Parameters ......................................................................................................... |
7-4 |
! - User Variables ................................................................................................... |
7-6 |
SYSTEM VARIABLES ..................................................................................................... |
7-8 |
SN - System Number ............................................................................................. |
7-8 |
SC - System Character .......................................................................................... |
7-9 |
TIM - System Timer................................................................................................ |
7-11 |
@ - PLUS Variables ............................................................................................... |
7-12 |
L Variables ............................................................................................................. |
7-13 |
Multiple Assignments ............................................................................................. |
7-14 |
iv |
10 Series CNC Programming Manual |
|
|
Index |
|
|
10 Series CNC Programming Manual |
|
|
|
|
|
|
|
|
|
|
CANNED CYCLES |
|
|
|
CANNED CYCLES G8N .................................................................................................. |
8-1 |
|
|
Canned Cycle Features ......................................................................................... |
8-2 |
|
|
Canned Cycle Moves ............................................................................................. |
8-3 |
|
|
G81 |
- Drilling Cycle ................................................................................................ |
8-5 |
|
G82 |
- Spot Facing Cycle........................................................................................ |
8-7 |
|
G83 |
- Deep Drilling Cycle ...................................................................................... |
8-9 |
|
DRP – G83 hole reworking distance...................................................................... |
8-12 |
|
|
G84 |
- Tapping Cycle with no Transducer .............................................................. |
8-13 |
|
G84 |
- Tapping Cycle with Transducer ................................................................... |
8-16 |
|
G84 |
- Rigid tapping cycle with a transducer mounted on the spindle .................... |
8-17 |
|
TRP (RMS) - Tapping Return Percentage............................................................. |
8-18 |
|
|
G85 |
- Reaming Cycle (or Tapping by Tapmatic) ................................................... |
8-19 |
|
G86 |
- Boring Cycle................................................................................................. |
8-20 |
|
G89 |
- Boring Cycle with Spot Facing ..................................................................... |
8-21 |
|
Using two R dimensions in a canned cycle............................................................ |
8-22 |
|
|
Updating Canned Cycle Dimensions ..................................................................... |
8-23 |
|
|
Updating R dimensions (upper limit and lower limit) during execution .................. |
8-24 |
|
|
|
|
|
|
PARAMACRO |
|
|
|
Paramacro Definition ............................................................................................. |
9-1 |
|
|
HC Parameters ...................................................................................................... |
9-3 |
|
|
DAN - Define Axis Name ....................................................................................... |
9-6 |
|
|
PMS – S as a paramacro....................................................................................... |
9-7 |
|
|
PMT – T as a paramacro ....................................................................................... |
9-7 |
|
|
PMM – M as a paramacro ..................................................................................... |
9-7 |
|
|
Syntax.............................................................................................................................. |
|
9-7 |
|
S, T, M ANCILLARY FUNCTIONS EXECUTED AS PARAMACROS ............................ |
9-8 |
|
|
Syntax: ............................................................................................................................ |
|
9-8 |
|
DGM – Disable Paramacro scrolling...................................................................... |
9-11 |
|
|
|
|
|
|
PROBING CYCLES |
|
|
|
MANAGING AN ELECTRONIC PROBE ......................................................................... |
10-1 |
|
|
PRESETTING A PROBING CYCLE................................................................................ |
10-3 |
|
|
DPP (DPT) - Defining Probing Parameters ........................................................... |
10-3 |
|
|
Dynamic Measurement of the Ball Diameter ......................................................... |
10-4 |
|
|
Probe Requalification............................................................................................. |
10-4 |
|
|
Dynamic Measurement of the Probe Length ......................................................... |
10-4 |
|
|
Probe Presetting .................................................................................................... |
10-4 |
|
|
PROBING CYCLES......................................................................................................... |
10-6 |
|
|
G72 |
- Point Measurement with Compensation ...................................................... |
10-7 |
|
G73 |
- Hole Probing Cycle ...................................................................................... |
10-9 |
|
G74 |
- Tool Requalification Cycle ........................................................................... |
10-11 |
|
UPA (RTA) - Update Probe Abscissa .................................................................... |
10-13 |
|
|
UPO (RTO) - Update Probe Ordinate.................................................................... |
10-13 |
|
|
ERR - Managing Probing Errors ............................................................................ |
10-13 |
|
|
OPERATIONS WITH A NON-FIXED PROBE ................................................................. |
10-14 |
|
|
Requalifying Origins by Probing Reference Surfaces............................................ |
10-14 |
|
|
Requalifying Origins by Centring on a Hole ........................................................... |
10-16 |
|
|
Checking Diameters .............................................................................................. |
10-16 |
|
|
Checking Plane Dimensions and Hole Depths ...................................................... |
10-18 |
|
|
10 Series CNC Programming Manual |
v |
Index
10 Series CNC Programming Manual
OPERATIONS THAT USE A FIXED PROBE .................................................................. |
10-19 |
MANAGING THE SCREEN
GRAPHICS VISUALIZATION .......................................................................................... |
11-1 |
UGS (UCG) - Use Graphic Scale (Machine plot) ................................................... |
11-2 |
UGS (UCG) - Use 3D Graphic Scale ..................................................................... |
11-3 |
CGS (CLG) - Clear Graphic Screen....................................................................... |
11-3 |
DGS (DCG) - Disable Graphic Scale ..................................................................... |
11-4 |
DIS - Displaying a Variable..................................................................................... |
11-4 |
MODIFYING THE PROGRAM EXECUTION SEQUENCE
GENERAL ........................................................................................................................ |
12-1 |
COMMAND FOR PROGRAM BLOCKS REPETITION ................................................... |
12-4 |
RPT - ERP.............................................................................................................. |
12-4 |
COMMANDS FOR SUBROUTINE EXECUTION ............................................................ |
12-8 |
CLS – CLD - CLT - Call Subroutine ....................................................................... |
12-8 |
PTH - Declaration of the default pathname............................................................ |
12-14 |
EPP - Executing a Portion of a Program ................................................................ |
12-15 |
EPB - Execute Part-Program Block ....................................................................... |
12-17 |
BRANCHING AND DELAY COMMANDS ....................................................................... |
12-19 |
GTO - Branch Command ....................................................................................... |
12-19 |
IF ELSE ENDIF .................................................................................................... |
12-23 |
DLY - Defining Delay Time..................................................................................... |
12-24 |
DSB - Disable Slashed Blocks ............................................................................... |
12-25 |
REL - Releasing the part program ......................................................................... |
12-25 |
WOS - WAIT on signal........................................................................................... |
12-26 |
DEVICE DEFINING COMMANDS ................................................................................... |
12-27 |
GDV - Definition of the device for file access......................................................... |
12-27 |
RDV - Release device ............................................................................................ |
12-28 |
HIGH SPEED MACHINING
GENERAL CONSIDERATIONS....................................................................................... |
13-1 |
PROGRAMMING POINTS AND CHARACTERISTICS OF THE PROFILE .................... |
13-3 |
Considerations on the use of the G62,G63,G66 and G67 functions |
|
(transition codes).................................................................................................... |
13-6 |
GENERAL HIGH SPEED MACHINING PROGRAMMING STRUCTURE ...................... |
13-7 |
Interaction with Machine Logic ............................................................................... |
13-7 |
POINT DEFINING CONVENTIONS................................................................................. |
13-8 |
Points and machining coordinates ......................................................................... |
13-8 |
Tool Direction: IJK .................................................................................................. |
13-9 |
Normal to the Surface Direction: MNO................................................................... |
13-9 |
Tool Radius Application Direction: PQD................................................................. |
13-10 |
Paraxial Compensation Factors: UVW .................................................................. |
13-11 |
Tangential Axis....................................................................................................... |
13-12 |
FEATURES PROVIDED BY HIGH SPEED MACHINING ............................................... |
13-13 |
Tool Radius and Length Compensation................................................................. |
13-13 |
Tool Length Compensation .................................................................................... |
13-14 |
No Tool Compensation .......................................................................................... |
13-15 |
Tangential Axis Management................................................................................. |
13-15 |
SETUP.............................................................................................................................. |
13-16 |
vi |
10 Series CNC Programming Manual |
|
Index |
|
10 Series CNC Programming Manual |
|
|
|
|
|
Type of points described in the part program ........................................................ |
13-17 |
|
Versor management methods ............................................................................... |
13-18 |
|
Look Ahead management...................................................................................... |
13-20 |
|
Thresholds ............................................................................................................. |
13-22 |
|
Tool definition......................................................................................................... |
13-24 |
|
Tool direction (3D) ................................................................................................. |
13-25 |
|
Change in curvature management ........................................................................ |
13-26 |
|
Edge management ................................................................................................ |
13-27 |
|
Axis definition......................................................................................................... |
13-28 |
|
Axis parameters..................................................................................................... |
13-30 |
|
Axis dynamics ........................................................................................................ |
13-31 |
|
Example ................................................................................................................. |
13-32 |
|
|
|
|
MULTIPROCESS MANAGEMENT COMMANDS |
|
|
GENERAL........................................................................................................................ |
14-1 |
|
SYNCHRONIZATION AMONG PROCESSES ................................................................ |
14-2 |
|
Notes On The "Wait" Function:.............................................................................. |
14-2 |
|
Notes On The "Send" Function:............................................................................. |
14-2 |
|
Exchanging data .................................................................................................... |
14-3 |
|
Resetting synchronised processes ........................................................................ |
14-3 |
|
Channels table ....................................................................................................... |
14-3 |
|
DCC - Definition of the communication channel .................................................... |
14-4 |
|
PVS - PLUS channel selection .............................................................................. |
14-5 |
|
PRO - Definition of the process ............................................................................. |
14-6 |
|
SND - Send a synchronisation message ............................................................... |
14-7 |
|
WAI - Wait for a synchronisation message ........................................................... |
14-10 |
|
EXE - Automatic part program execution .............................................................. |
14-12 |
|
ECM - Manual block execution in a process.......................................................... |
14-13 |
|
Example of synchronisation of two process using EXE:........................................ |
14-14 |
|
SHARED AXES................................................................................................................ |
14-15 |
|
General .................................................................................................................. |
14-15 |
|
Conditions for axis acquisition ............................................................................... |
14-15 |
|
GTA - Axes acquisition .......................................................................................... |
14-16 |
|
SYSTEM PARAMETERS AFTER GTA ................................................................. |
14-17 |
|
INFORMATION RETAINED AFTER A GTA COMMAND...................................... |
14-18 |
|
Error Management ................................................................................................. |
14-27 |
|
|
|
|
HIGH LEVEL GEOMETRIC PROGRAMMING (GTL) |
|
|
ORIENTED GEOMETRY................................................................................................. |
15-2 |
|
DEFINING GEOMETRIC ELEMENTS ............................................................................ |
15-5 |
|
DEFINITION OF A REFERENCE ORIGIN ...................................................................... |
15-8 |
|
DEFINITION OF POINTS ................................................................................................ |
15-9 |
|
DEFINITION OF STRAIGHT LINES................................................................................ |
15-15 |
|
DEFINITION OF CIRCLES.............................................................................................. |
15-26 |
|
DEFINITION OF A PROFILE........................................................................................... |
15-40 |
|
Profile types ........................................................................................................... |
15-40 |
|
Connecting the elements ....................................................................................... |
15-45 |
|
EXAMPLES OF GTL PROGRAMMING.......................................................................... |
15-49 |
|
|
|
|
10 Series CNC Programming Manual |
vii |
Index
10 Series CNC Programming Manual
WORKING CYCLES FOR TURNING SYSTEMS........................... |
16-1 |
|
PROFILE PROGRAMMING............................................................................................. |
16-1 |
|
Restrictions to the definition of a profile to be recalled by the macro- |
|
|
instructions of roughing/finishing. ........................................................................... |
16-2 |
|
SPECIAL CYCLES PROGRAMMING ............................................................................. |
16-3 |
|
MACRO-INSTRUCTIONS OF PARA-AXIAL ROUGHING WITHOUT PRE- |
|
|
FINISHING ....................................................................................................................... |
16-3 |
|
MACRO-INSTRUCTIONS OF PARA-AXIAL ROUGHING WITH PRE-FINISHING................ |
16-7 |
|
MACRO-INSTRUCTION OF ROUGHING PARALLEL TO THE PROFILE .................... |
16-9 |
|
MACRO-INSTRUCTION OF A PROFILE FINISHING..................................................... |
16-11 |
|
THREADING CYCLE ....................................................................................................... |
16-12 |
|
GROOVE CUTTING CYCLE ........................................................................................... |
16-16 |
|
|
|
|
FILTERS |
|
|
GENERAL ........................................................................................................................ |
17-1 |
|
FLT – Filter programming....................................................................................... |
17-2 |
|
ERF – Error Form................................................................................................... |
17-5 |
|
|
|
|
CHARACTERS AND COMMANDS |
|
|
TABLE OF CHARACTERS.............................................................................................. |
100-1 |
|
G CODES ......................................................................................................................... |
100-5 |
|
MATHEMATICAL FUNCTIONS....................................................................................... |
100-6 |
|
LOCAL AND SYSTEM VARIABLES ............................................................................... |
100-6 |
|
THREE-LETTER CODES ................................................................................................ |
100-7 |
|
ASCII CODES .................................................................................................................. |
100-10 |
|
|
|
|
ERROR MESSAGES |
|
|
Description of error messages and remedial actions............................................. |
200-1 |
|
|
|
|
ERROR MANAGEMENT |
|
|
GENERAL ........................................................................................................................ |
300-1 |
|
ERR - Enable/disables error management from part program .............................. |
300-2 |
|
Probing cycle errors ............................................................................................... |
300-3 |
|
Shared axes errors................................................................................................. |
300-4 |
|
Errors in multiprocess management ...................................................................... |
300-5 |
|
viii |
10 Series CNC Programming Manual |
Index
10 Series CNC Programming Manual
END OF INDEX
10 Series CNC Programming Manual |
ix |
Chapter 1
PROGRAMMING WITH 10 SERIES SYSTEMS
10 Series part programs are written with a specific language defined by the ISO standard. This chapter describes the language elements and discusses programming techniques and rules.
THE PROGRAM FILES
The 10 Series part programs are stored in files which may be identified with 10 SERIES names or with DOS names.
10 SERIES names are a maximum of 48 characters in length; they identify the programs stored in the logic directories configured on the machine.
Logic directories are configured during the installation stage (PPDIR config - human interface menu in AMP characterization).
DOS names are a maximum of 8 characters in length, plus an extension and path where applicable; they identify files resident in DOS type directories.
Using the Windows Editors, remember to give the “enter” command on the last line entered in the program. Quitting the program without this command might cause errors during program execution.
Mixed management of part programs is not allowed; in fact if a program is activated after being called by a DOS type name, all it subroutines must be identified with DOS names.
Similarly, programs with 10 SERIES names can use only subroutines identified in the same way.
NOTE:
Part programs can also be resident on remote devices, defined in advance through the triliteral GDV (see chap. 12).
10 Series CNC Programming Manual |
1-1 |
Chapter 1
Programming with 10 Series Systems
Program Components
Address
An address is a letter that identifies the type of instruction. For example, these are addresses:
G, X, Y, F
Word
A word is an address followed by a numerical value. For example, these are words:
G1 X50.5 Z-3.15 F200 T1.1
When you assign a numeric value to a word, no zeroes must preceed or follow the value. Insert decimal values after the decimal point.
Block
A program block comprises a set of words that identify an operation or a series of operations to be performed. The maximum length of a block is 126 characters.
A technological program is a sequence of blocks that describe a machining operation.
Each block must end with: <CR> <LF>.
Blocks
Blocks may include one or several fields.
When several fields are used in the same block, they must appear in the order shown in the following table:
block |
label |
sequence |
synchronisation |
words |
delete |
|
number |
asynchronisation |
codes |
|
|
|
|
|
/ |
LABEL |
NUMBER |
# or & |
ALL ALLOWED |
|
|
|
|
CHARACTERS |
|
|
|
|
|
Comment blocks
It can be inserted in any position within the current block. Any character after ";" is considered as a comment.
1-2 |
10 Series CNC Programming Manual |
Chapter 1
Programming with 10 Series Systems
Block delete
The block delete field is optional. It allows the operator to choose whether to execute program blocks that begin with the "/" character that are called slashed blocks.
Example:
/N100 G00 X100
The block shown in the example can be enabled or disabled using the PROGRAM SET UP softkey, or typing the three-letter code DSB on the keyboard.
Label
The label field is optional. It allows the programmer to assign a symbolic name to a block. A label can have up to six alphanumeric characters which must be between quotes. In case of a slashed block, the label must be inserted after the slash.
Example: "START" /"END"
When a label field is used in a 'GTO' command, the label defines the block that the control should jump to.
Sequence number
The "sequence number" field is optional. It allows the programmer to number each program block. A sequence number begins with the letter N and is followed by up to six digits (N0N999999).
The sequence number must appear in front of the first operand and after the label.
Example:
N125 X0 "START" N125 X0 "END" N125 X0
Synchronisation/asynchronisation
Characters & and # are used to override the default synchronisation/asynchronisation status. For further information on synchronisation, see "Synchronisation and Program Execution".
Example: #(GTO,START, @PL1=1)
10 Series CNC Programming Manual |
1-3 |
Chapter 1
Programming with 10 Series Systems
Block Types
Four types of blocks can be used in a part program:
Comment blocks
Motion blocks
Assignment blocks
Three-letter command blocks
Comment blocks
A comment block allows the programmer to insert free sentences in the program. These sentences may describe the function to be executed or provide other pieces of information that make the program more understandable and documented.
A comment block does not produce messages for the operator. The control ignores a comment block during execution of the program.
The first character of a comment block must be a semicolon (;). The rest of the comment block is a sequence of alphanumeric characters. For example:
;THIS IS AN EXAMPLE OF COMMENT BLOCK
A comment can be inserted not only in a single block, but also in other types of blocks after the character ";".All characters after a ; considered as a comment. For example:
G1 X100 Y50 ; Motion block E1=10 ; Local variable E (ROT,45) ; Rotation command
Motion blocks
Motion blocks conform to ISO and ASCII standards for programming blocks. There is no particular order for programming the components of a motion block.
Example:
G1 X500 Y20 F200
Assignment blocks
Assignment blocks are used to write variables' values directly from the program. Several types of assignments are possible as shown in the following table:
TYPE OF ASSIGNMENT |
EXAMPLE |
|
|
|
|
Simple assignment |
E10=123.567 |
|
Multiple assignment |
E1=10, 15.5, 123.467 |
|
|
In multiple assignments values are loaded as follows: |
|
|
10 |
to E1 |
|
15.5 |
to E2 |
|
123.467 |
to E3 |
Math expression assignment |
E20=(E10+125*SQR(E23)) |
|
System number |
SN=1.5 |
|
|
|
|
Three-letter command blocks
1-4 |
10 Series CNC Programming Manual |
Chapter 1
Programming with 10 Series Systems
Three-letter command blocks define an operation with a three-letter instruction in conformity with the RS-447 standard. For example:
(ROT,45) (DIS,"message text")
For the sake of compatibility between 10 Series and Series 8600 certain commands may be programmed with either of the following three-letter codes.
UGS UCG
CGS CLG
DGS DCG
RQT RQU
DPA DSA
PAE ASC
PAD DSC
DPP DPT
IPB DTL
ROT URT
SOL DLO
UTO UOT
TOU TOF
10 Series CNC Programming Manual |
1-5 |
Chapter 1
Programming with 10 Series Systems
Programmable Functions
Axis coordinates
Axis coordinates can be named with letters ABCUVWXYZPQD (according to the configuration set in AMP) and can be programmed in the following ranges:
-99999.99999 |
-0.00001 |
mm/inch |
|
|
|
+0.00001 |
+99999.99999 |
mm/inch |
|
|
|
NOTE:
It is impossible to program coordinates in the +0.00001 range because 0.00001 is the minimum value accepted by the control.
R coordinate
In a circular interpolation (G02 G03) R represents the radius of the circle.
In a standard canned cycle (G81-G89), the R coordinate defines the initial position value and retract value. This function is programmable in the following ranges:
-99999.99999 |
-0.00001 |
mm/inch |
|
|
|
+0.00001 |
+99999.99999 |
mm/inch |
|
|
|
NOTE:
It is impossible to program values in the +0.00001 range because 0.00001 is the minimum value accepted by the control.
In a threading block (G33), the R coordinate represents the offset from the zero angular position of the spindle for multi-start threads.
I J coordinates
In circular interpolation (G02-G03), I and J specify the coordinates of the center of an arc. I specifies the abscissa (typically X) and J the ordinate of the center (typically Y). I and J always specify the center coordinates regardless of the active interpolation plane.
This function is programmable in the following ranges:
-99999.99999 |
-0.00001 |
mm/inch |
|
|
|
+0.00001 |
+99999.99999 |
mm/inch |
|
|
|
NOTE:
It is impossible to program values in the +0.00001 range because 0.00001 is the minimum value accepted by the control.
When the values of the corresponding axis are expressed in diametrical units (according to the configuration set in AMP), the values of the center coordinates (I and J) are also expressed in diametrical units.
I and J coordinates are also used in the deep hole drilling cycle (G83).
In a threading block (G33), the I address defines the pitch variation for variable pitch threads:
I+ |
Increasing pitch |
I- |
Decreasing pitch |
K function |
|
1-6 |
10 Series CNC Programming Manual |
Chapter 1
Programming with 10 Series Systems
In the deep hole drilling cycle (G83), K defines the incremental value to be applied to the minimum depth value (J) in order to reduce the initial pitch depth (I).
This function is programmable in the following ranges:
-99999.99999 |
-0.00001 |
mm/inch |
|
|
|
+0.00001 |
+99999.99999 |
mm/inch |
|
|
|
NOTE:
It is impossible to program values in the +0.00001 range because 0.00001 is the minimum value accepted by the control.
In a threading block (G33) or a tapping cycle (G84), K defines the thread pitch. In helical interpolation (G02-G03), K defines the helix pitch.
F and t function
The F function defines the axes feedrate. This function is programmable in the following range:
+0.00001 |
+99999.99999 |
mm/inch |
|
|
|
In G94, F function defines the feedrate in millimetres per minute (G71) or inches per minute (G70).
A "t" value can be programmed in a block to specify the time in seconds needed to complete the move defined in the block. In this case the block feedrate will be:
F = |
totaldistance |
* 60 |
||
time |
|
|||
|
|
|||
A "t" value is valid only in the block in which it is programmed.
In G93, the F function defines the inverse of the necessary time in minutes to complete the movement:
F = |
speed |
= 1/t (minutes) |
||
|
|
|||
totaldistance |
||||
|
|
|||
The F function is mandatory in the blocks when G93 is active and only affects that block.
In G95, F specifies the axes feedrate in millimetres per revolution (G71) or inches per revolution of the spindle (G70).
a Function
The a function defines the acceleration to use on the part program block and may be programmed in the range:
+0.00001 |
+99999.99999 |
mm/sec2 or inches/sec2 |
The a function is considered in mm/sec2 in presence of G71 and in inches/sec2 in presence of G70. This function is active only in the block it is programmed in and is in any case limited to the acceleration on the profile as calculated by the system in function of the accelerations configured.
M function
10 Series CNC Programming Manual |
1-7 |
Chapter 1
Programming with 10 Series Systems
The M address can activate various machine operations. The programmable range goes from 0 to 999. See Chapter 6 for further information about these functions.
S function
The S function specifies the spindle rotation speed. It is programmable in the following range:
+0.001 |
999999.999 |
rpm/fpm |
|
|
|
In G97, the S function defines spindle rotation speed expressed in revolutions per minute.
In G96, the S function defines the cutting surface speed expressed in metres per minute (G71) or feet per minute (G70). The above cutting speed remains constant on the surface.
Refer to Chapter 5 for further information about S function programming.
T function
The T function defines the tool and tool offset needed for machining. It is programmable in the 0.0 to 999999999999.300 range. The 12 digits on the left of the decimal point represent the tool identifier code and the three digits on the right represent the tool offset number.
Chapter 3 provides a detailed description of T functions.
IMPORTANT
h functions
M, S and T functions vary according to their characterisation in AMP.
From SW release 3.1 it is possible for the system to execute these functions inside a continuous move (G27-G28).
When planning an application the manufacturer must:
configure the desired function as "ALLOWED IN CONTINUOUS" in AMP. write a machine logic to handle such a function.
In turn, the programmer must remember that these functions produce different effects depending on how they are programmed:
in continuous mode a function configured as "ALLOWED IN CONTINUOUS" will be executed in the sequence in which it has been programmed. In order not to lock the program the function will be executed in "NO WAIT" mode.
in point-to-point mode a function configured as "ALLOWED IN CONTINUOUS" will be executed in standard mode.
h functions permit to alter an offset during both continuous and point to point moves.
An h function must be programmed by itself in a block. Its value may range from 0 through 300 and may be either an integer or an E variable.
G functions
G codes program machining preparatory functions for machining. The following section deal with this codes.
1-8 |
10 Series CNC Programming Manual |
Chapter 1
Programming with 10 Series Systems
G Codes
This section shows how to write preparatory G codes in part program blocks. A preparatory G code is identified by the G address followed by one or two digits (G00-G99). At present, only some of the 100 possible G codes are available.
Paramacro subroutines can be called with a three-digit G code. This class of G codes is described in Chapter 9. Three-digit G codes are classified as follows:
G100 - G299 Reserved
G300 - G699 Non modal paramacro range
G700 - G998 Modal paramacro range
G999 |
Reset modal paramacro |
The G code must be programmed after the sequence number (if defined) and before any other operand in the block. For example:
N100 G01 X0 - operand
It is possible to program several G codes in the same block, provided they are compatible with each other. The table that follows defines compatibility between G codes. Zero indicates that the G codes are compatible and can be programmed in the same block; 1 means that the G codes are not compatible and cannot be programmed in the same block without generating an error.
10 Series CNC Programming Manual |
1-9 |
Chapter 1
Programming with 10 Series Systems
Compatible G Codes
G |
00 |
01 |
02 |
33 |
81 |
80 |
72 |
93 |
96 |
41 |
40 |
27 |
29 |
04 |
09 |
90 |
79 |
70 |
16 |
92 |
20 |
21 |
60 |
|
|
|
03 |
|
89 |
|
73 |
94 |
97 |
42 |
|
28 |
|
|
|
91 |
|
71 |
17 |
99 |
|
|
61 |
|
|
|
|
|
|
|
74 |
95 |
|
|
|
|
|
|
|
|
|
|
18 |
98 |
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
|
19 |
|
|
|
|
G00 |
1 |
1 |
1 |
1 |
0 |
1 |
1 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
G01 |
1 |
1 |
1 |
1 |
0 |
1 |
1 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
G02 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
G03 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
G04 |
0 |
0 |
0 |
1 |
1 |
0 |
1 |
0 |
0 |
0 |
0 |
1 |
0 |
1 |
1 |
0 |
0 |
0 |
1 |
1 |
0 |
0 |
1 |
G09 |
0 |
0 |
0 |
0 |
1 |
0 |
1 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
0 |
0 |
0 |
1 |
1 |
0 |
0 |
1 |
G16 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
G17 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
G18 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
G19 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
G20 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
0 |
1 |
1 |
1 |
1 |
1 |
G21 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
0 |
1 |
1 |
1 |
1 |
1 |
G27 |
0 |
0 |
0 |
0 |
1 |
0 |
1 |
0 |
0 |
0 |
0 |
1 |
1 |
1 |
0 |
0 |
0 |
0 |
1 |
1 |
0 |
0 |
1 |
G28 |
0 |
0 |
0 |
0 |
1 |
0 |
1 |
0 |
0 |
0 |
0 |
1 |
1 |
1 |
0 |
0 |
0 |
0 |
1 |
1 |
0 |
0 |
1 |
G29 |
0 |
0 |
0 |
0 |
1 |
0 |
1 |
0 |
0 |
0 |
0 |
1 |
1 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
0 |
0 |
1 |
G33 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
0 |
0 |
1 |
1 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
G40 |
0 |
0 |
0 |
1 |
1 |
1 |
1 |
0 |
0 |
1 |
1 |
0 |
0 |
0 |
0 |
0 |
1 |
0 |
1 |
1 |
0 |
0 |
1 |
G41 |
0 |
0 |
0 |
1 |
1 |
1 |
1 |
0 |
0 |
1 |
1 |
0 |
0 |
0 |
0 |
0 |
1 |
0 |
1 |
1 |
1 |
0 |
1 |
G42 |
0 |
0 |
0 |
1 |
1 |
1 |
1 |
0 |
0 |
1 |
1 |
0 |
0 |
0 |
0 |
0 |
1 |
0 |
1 |
1 |
1 |
0 |
1 |
G60 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
G61 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
G70 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
1 |
0 |
0 |
1 |
G71 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
1 |
0 |
0 |
1 |
G72 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
G73 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
G74 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
G79 |
0 |
0 |
0 |
0 |
1 |
1 |
1 |
0 |
0 |
1 |
1 |
0 |
0 |
0 |
0 |
1 |
1 |
0 |
1 |
1 |
1 |
1 |
1 |
G80 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
0 |
0 |
1 |
1 |
0 |
0 |
0 |
0 |
0 |
1 |
0 |
1 |
1 |
1 |
1 |
1 |
G81 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
1 |
0 |
1 |
0 |
1 |
1 |
1 |
1 |
1 |
G82 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
0 |
0 |
1 |
1 |
1 |
1 |
0 |
0 |
0 |
1 |
0 |
1 |
1 |
1 |
1 |
1 |
G83 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
0 |
0 |
1 |
1 |
1 |
1 |
0 |
0 |
0 |
1 |
0 |
1 |
1 |
1 |
1 |
1 |
G84 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
0 |
0 |
1 |
1 |
1 |
1 |
0 |
0 |
0 |
1 |
0 |
1 |
1 |
1 |
1 |
1 |
G85 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
0 |
0 |
1 |
1 |
1 |
1 |
0 |
0 |
0 |
1 |
0 |
1 |
1 |
1 |
1 |
1 |
G86 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
0 |
0 |
1 |
1 |
1 |
1 |
0 |
0 |
0 |
1 |
0 |
1 |
1 |
1 |
1 |
1 |
G89 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
0 |
0 |
1 |
1 |
1 |
1 |
0 |
0 |
0 |
1 |
0 |
1 |
1 |
1 |
1 |
1 |
G90 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
0 |
1 |
1 |
0 |
0 |
1 |
G91 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
0 |
1 |
1 |
0 |
0 |
1 |
G92 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
G93 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
G94 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
G95 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
G96 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
0 |
1 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
G97 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
0 |
1 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
0 |
1 |
1 |
1 |
1 |
1 |
G98 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
G99 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
1 |
NOTE:
0 means compatible G codes
1 means incompatible G codes
1-10 |
10 Series CNC Programming Manual |
Chapter 1
Programming with 10 Series Systems
The following table gives a summary of the G codes available in the control. This default configuration can be modified through the AMP utility.
G code summary
CODE |
GROUP |
MODAL |
DESCRIPTION |
POWER UP |
|
|
|
|
|
MILL |
GRINDING |
|
|
|
|
|
|
G00 |
a |
yes |
Rapid axes positioning |
yes |
yes |
G01 |
a |
yes |
Linear interpolation |
no |
no |
G02 |
a |
yes |
Circular interpolation CW |
no |
no |
G03 |
a |
yes |
Circular interpolation CCW |
no |
no |
G33 |
a |
yes |
Constant or variable pitch thread |
no |
no |
|
|
|
|
|
|
G16 |
b |
yes |
Circular interpolation and cutter |
no |
no |
|
|
|
diameter compensation on a defined |
|
|
|
|
|
plane |
|
|
G17 |
b |
yes |
Circular interpolation and cutter |
yes |
no |
|
|
|
diameter compensation on 1st-2nd axes |
|
|
|
|
|
plane |
|
|
G18 |
b |
yes |
Circular interpolation and cutter |
no |
yes |
|
|
|
diameter compensation on 3rd-1st axes |
|
|
|
|
|
plane |
|
|
G19 |
b |
yes |
Circular interpolation and cutter |
no |
no |
|
|
|
diameter compensation on 2nd-3rd axes |
|
|
|
|
|
plane |
|
|
|
|
|
|
|
|
G27 |
c |
yes |
Continuous sequence operation with |
yes |
yes |
|
|
|
automatic speed reduction on corners |
|
|
G28 |
c |
yes |
Continuous sequence operation |
no |
no |
|
|
|
without speed reduction on corners |
|
|
G29 |
c |
yes |
Point-to-point operation |
no |
no |
|
|
|
|
|
|
G92 |
d |
no |
Axis presetting without mirror |
no |
no |
G98 |
d |
no |
Axis presetting with mirror |
no |
no |
G99 |
d |
yes |
Delete G92 |
yes |
yes |
|
|
|
|
|
|
G40 |
e |
yes |
Cutter diameter compensation disable |
yes |
yes |
G41 |
e |
yes |
Cutter diameter compensation-tool left |
no |
no |
G42 |
e |
yes |
Cutter diameter compensation-tool right |
no |
no |
G20 |
|
yes |
Closes GTL profile |
|
|
G21 |
|
yes |
Opens GTL profile |
|
|
|
|
|
|
|
|
G60 |
|
yes |
Closes the HSM profile |
no |
no |
G61 |
|
yes |
Opens the HSM profile |
no |
no |
G62 |
|
no |
Splits the HSM profile in two with |
no |
no |
|
|
|
continuity |
|
|
G63 |
|
no |
Splits the HSM profile in tw with link |
no |
no |
G66 |
|
no |
Splits the HSM profile in two with edge |
no |
no |
G67 |
|
no |
Splits the HSM profile in two with |
no |
no |
|
|
|
reduced speed on edge |
|
|
|
|
|
|
|
|
10 Series CNC Programming Manual |
1-11 |
Loading...