OSAI 10 CNC User Manual

10 Series CNC
Programming Manual

Code: 45004457K
Rev. 17

PUBLICATION ISSUED BY:

OSAI S.p.A.
Via Torino, 14 - 10010 Barone Canavese (TO) – Italy

Phone: [phone]

Web: www.osai.it

e-mail: [e-mail]

[e-mail]

Copyright  2001-2006 by OSAI
All rights reserved

Edition: December 2006

IMPORTANT USER INFORMATION

This document has been prepared in order to be used by OSAI. It describes the latest release of
the product.
OSAI reserves the right to modify and improve the product described by this document at any time
and without prior notice.
Actual application of this product is up to the user. In no event will OSAI be responsible or liable for
indirect or consequential damages that may result from installation or use of the equipment
described in this text.

abc

10 Series CNC Programming Manual

SUMMARY OF CHANGES

General

This publication is issued with reference to Software Release 7.6 (E69).

PAGE UPDATING TYPE

UPDATE

INDEX

CHAPTER 1

p. 1
p. 11

CHAPTER 2

p. 13

p. 44

p. 56
p. 57
pp. 58-59
p. 61
p. 70
p. 135
p. 161

CHAPTER 3

p. 8-9

CHAPTER 4

p. 5

p. 16
p. 26
p. 34

Updated

Added description
Added code G98

Changed paragraph “CRT – Circular interpolation speed reduction
threshold. CRK – Circular interpolation speed reduction constants”
Added new paragraph “AXF – Definition of axes with dynamic following
function”
Added description
Added description
Added description
Changed paragraph “MOV – Movement modalities”
Changed paragraph “JRK – Jerk Constant”
Added description in table of “operational limit modes”
Added new paragraph “TCP – Tool Center Point for machines with
prismatic head”

Added description

Changed description in paragraph “Notes on using cutter diameter
compensation”
Changed paragraph “TPO – Tool path optimisation in G41/G42”
Added new paragraph “TPA – Threshold angle for TPO”
Added new paragraph “UVW – Definition of axes for paraxial
compensation”

CHAPTER 12

p. 23

CHAPTER 14

p. 11
pp. 12-13
pp. 18-24

CHAPTER 16

p. 9

10 Series CNC Programming Manual (17)

Changed description

Added description
Added description
Added description

Corrected description n_pass

UPDATE

10 Series CNC Programming Manual

CHAPTER 17

Added new chapter “Filters”

APP. B

p. 1
p. 4

APP. C

p. 5

Added description for NC008
Changed description for NC042

Added new paragraph “Errors in multiprocess management”

10 Series CNC Programming Manual (17)

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 (17) 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 (17)

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..

Preface

C. Error management

10 Series CNC Programming Manual (17) 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.

|

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.

A vertical bar separates alternative entries. Do not enter the bar.

4 10 Series CNC Programming Manual (17)

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

CAUTION

in general.

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 (17) 5

Preface

10 Series CNC Programming Manual

END OF PREFACE

6 10 Series CNC Programming Manual (17)

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

Index

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 (17) i

Index

10 Series CNC Programming Manual

Syntax.............................................................................................................................. 2-34

Mode 0 ...................................................................................................................2-35

Mode 1 ...................................................................................................................2-36

Mode 2 ...................................................................................................................2-37

Mode 3 ...................................................................................................................2-39

Releasing the Slave(s) from the Master ................................................................ 2-40

Syntax.............................................................................................................................. 2-40

Defining/Changing the following ratio ....................................................................2-41

Syntax.............................................................................................................................. 2-41

Activating the following function............................................................................. 2-42

Syntax.............................................................................................................................. 2-42

Deactivating the following function......................................................................... 2-43

Syntax.............................................................................................................................. 2-43

AXF – Definition of axes with dynamic following function...................................... 2-44

ORIGINS AND COORDINATE CONTROL CODES ....................................................... 2-46

G17 G18 G19 - Selecting the Interpolation Plane .................................................2-47

G16 - Defining the Interpolation Plane................................................................... 2-48

G27 G28 G29 - Defining the Dynamic Mode ......................................................... 2-49

AUTOMATIC DECELERATION ON BEVELS IN G27 MODE........................................ 2-54

DLA - Deceleration Look Ahead ............................................................................2-55

DYM - Dynamic Mode ............................................................................................ 2-56

MDA - Maximum Deceleration Angle..................................................................... 2-57

VEF - Velocity Factor ............................................................................................. 2-58

Jerk Limitation ........................................................................................................ 2-60

MOV - Enable Jerk Limitation ................................................................................ 2-61

JRK - Jerk Time Constant...................................................................................... 2-70

JRS - Jerk Smooth Constant .................................................................................2-72

ODH - Online Debug Help .....................................................................................2-74

MBA – MultiBlock retrace Auxiliary functions ........................................................ 2-76

REM – Automatic return to profile at end of move................................................. 2-77

IPB (DTL) - In Position Band.................................................................................. 2-78

G70 G71 - Measuring Units ................................................................................... 2-79

G90 G91 G79 - Absolute, Incremental and Zero Programming ............................ 2-80

G92 G98 G99 - Axis Presetting .............................................................................2-82

G04 G09 - Dynamic Mode Attributes..................................................................... 2-83

t - Block Execution Time ........................................................................................2-84

DWT (TMR) - Dwell Time....................................................................................... 2-84

G93 - V/D Feedrate................................................................................................ 2-85

VFF - Velocity Feed Forward ................................................................................. 2-86

CODES THAT MODIFY THE AXES REFERENCE SYSTEM......................................... 2-87

SCF - Scale Factors............................................................................................... 2-88

MIR - Using Mirror Machining ................................................................................ 2-89

ROT (URT) - Interpolation Plane Rotation............................................................. 2-92

UAO - Using Absolute Origins ...............................................................................2-95

UTO (UOT) - Using Temporary Origins ................................................................. 2-96

UIO - Using Incremental Origins ............................................................................ 2-98

RQO - Requalifying Origins ...................................................................................2-100

OVERTRAVELS AND PROTECTED AREAS ................................................................2-101

SOL (DLO) - Software Overtravel Limits ............................................................... 2-102

DPA (DSA) - Define Protected Areas ....................................................................2-103

PAE (ASC) - Protected Area Enable...................................................................... 2-105

PAD (DSC) - Protected Area Disable ....................................................................2-105

VIRTUAL AXES MANAGEMENT.................................................................................... 2-106

Virtual Axes ............................................................................................................ 2-106

Virtual modes available on 10 Series CNC............................................................ 2-106

ii 10 Series CNC Programming Manual (17)

UPR - Rotation of Cartesian axes ......................................................................... 2-107

Using UPR ............................................................................................................. 2-113

UVP - Programming polar coordinates.................................................................. 2-118

Programming examples with polar coordinates .................................................... 2-120

UVC - Programming cylindrical coordinates.......................................................... 2-122

UVA - Programming non orthogonal axes........................................................... 2-124

Example of programming with polar coordinates .................................................. 2-125

TCP - Tool Center Point for machines with "Double Twist" head ........................ 2-126

Programming the "m" and "n" parameters (angles) .............................................. 2-142

Programming the "m", "n", "o" and “u”, “v”, “w” parameters (vectors) ................... 2-143

TCP - Tool Center Point for generic 5-axis machines........................................... 2-145

Programming ......................................................................................................... 2-150

TCP - Tool Center Point for machines with fixed tool and rotary table ................. 2-154

Programming ......................................................................................................... 2-160

TCP - Tool Center Point for machines with Prismatic Head ................................. 2-161

Programming ......................................................................................................... 2-168

TCP on multi-processor......................................................................................... 2-169

PROGRAMMING TOOLS AND TOOL OFFSETS

Index

10 Series CNC Programming Manual

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

G40 G41 G42 - Cutter Diameter Compensation ................................................... 4-2

Enabling Cutter Diameter Compensation.............................................................. 4-3

Notes on using cutter diameter compensation ...................................................... 4-5

Tool path optimisation (TPO)................................................................................. 4-5

Disabling Cutter Diameter Compensation ............................................................. 4-6

Disabling Compensation with TPO active ............................................................. 4-7

TOOL DIAMETER COMPENSATION CHANGE............................................................ 4-8

Linear/Linear tool path........................................................................................... 4-8

Linear/Circular, Circular/Linear, Circular/Circular tool paths................................. 4-10

r - Radiuses in Compensated Profiles................................................................... 4-12

b - Bevels in Compensated Profiles ...................................................................... 4-13

TPO - Path optimisation on bevels with G41/G42................................................. 4-16

Examples of profile optimisation with TPO=1........................................................ 4-20

Examples of TPO=2 mode .................................................................................... 4-23

TPA – Threshold angle for TPO ............................................................................ 4-26

TPT - Tool Path Threshold .................................................................................... 4-27

u v w - Paraxial Compensation.............................................................................. 4-29

Examples of compensation factor applications u, v, w.......................................... 4-30

UVW – Definition of axes for paraxial compensation ............................................ 4-34

MSA (UOV) - Defining a Machining Stock Allowance ........................................... 4-35

AUTOMATIC CONTOUR MILLING ................................................................................ 4-36

Limits to use of automatic contour miling .............................................................. 4-36

10 Series CNC Programming Manual (17) iii

Index

10 Series CNC Programming Manual

GTP - Get Point...................................................................................................... 4-37

Determining the approach point............................................................................. 4-38

CCP - Cutter Compensation Profile....................................................................... 4-40

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

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

iv 10 Series CNC Programming Manual (17)

10 Series CNC Programming Manual

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

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

OPERATIONS THAT USE A FIXED PROBE................................................................. 10-19

Index

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

10 Series CNC Programming Manual (17) v

Index

10 Series CNC Programming Manual

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

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

vi 10 Series CNC Programming Manual (17)

10 Series CNC Programming Manual

PRO - Definition of the process ............................................................................. 14-6

SND - Send a synchronisation message............................................................... 14-7

WAI - Wait for a synchronisation message ........................................................... 14-9

EXE - Automatic part program execution .............................................................. 14-11

ECM - Manual block execution in a process ......................................................... 14-12

Example of synchronisation of two process using EXE: ....................................... 14-13

SHARED AXES ............................................................................................................... 14-14

General .................................................................................................................. 14-14

Conditions for axis acquisition ............................................................................... 14-14

GTA - Axes acquisition .......................................................................................... 14-15

SYSTEM PARAMETERS AFTER GTA................................................................. 14-16

INFORMATION RETAINED AFTER A GTA COMMAND ..................................... 14-17

Error Management................................................................................................. 14-26

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

Index

WORKING CYCLES FOR TURNING SYSTEMS

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

CHARACTERS AND COMMANDS

TABLE OF CHARACTERS............................................................................................. A-1

G CODES.........................................................................................................................A-5

MATHEMATICAL FUNCTIONS...................................................................................... A-6

LOCAL AND SYSTEM VARIABLES .............................................................................. A-6

10 Series CNC Programming Manual (17) vii

Index

10 Series CNC Programming Manual

THREE-LETTER CODES ................................................................................................ A-7

ASCII CODES .................................................................................................................. A-10

ERROR MESSAGES

Description of error messages and remedial actions ............................................ B-1

ERROR MANAGEMENT

GENERAL........................................................................................................................ C-1

ERR - Enable/disables error management from part program .............................. C-2

Probing cycle errors ............................................................................................... C-3

Shared axes errors................................................................................................. C-4

Errors in multiprocess management ...................................................................... C-5

END OF INDEX

viii 10 Series CNC Programming Manual (17)

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 (17) 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
delete

/ LABEL NUMBER # or & ALL ALLOWED

♦ Comment blocks

It can be inserted in any position within the current block. Any character after ";" is considered
as a comment.

label sequence

number

synchronisation
asynchronisation

words
codes

CHARACTERS

1-2 10 Series CNC Programming Manual (17)

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 (17) 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 (17)

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 (17) 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 (17)

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

time

distance total

*

60

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

distance total

(minutes)1/t =

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/sec

The a function is considered in mm/sec

2

or inches/sec

2

in presence of G71 and in inches/sec

2

2

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 (17) 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.

M, S and T functions vary according to their characterisation in AMP.

IMPORTANT

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

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 (17)

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 (17) 1-9

Chapter 1

Programming with 10 Series Systems

Compatible G Codes

20 21 60
17
18
19

92
99
98

9697414240 272829 04 09 909179 707116
73
74

93
94
95

G0001020333 818980 72

G00 11110110000000000011111
G01 11110110000000000011111
G02 11111110000000000011111
G03 11111110000000000011111
G04 00011010000101100011001
G09 00001010000001100011001
G16 11111111111111111111111
G17 11111111111111111111111
G18 11111111111111111111111
G19 11111111111111111111111
G20 11111111110000001011111
G21 11111111100000001011111
G27 00001010000111000011001
G28 00001010000111000011001
G29 00001010000110000011001
G33 11111110011000000011111
G40 00011110011000001011001
G41 00011110011000001011101
G42 00011110011000001011101
G60 11111111111111111111111
G61 11111111111111111111111
G70 00000010000000000111001
G71 00000010000000000111001
G72 11111111111111111111111
G73 11111111111111111111111
G74 11111111111111111111111
G79 00001110011000011011111
G80 11111110011000001011111
G81 00111110011111101011111
G82 00111110011110001011111
G83 00111110011110001011111
G84 00111110011110001011111
G85 00111110011110001011111
G86 00111110011110001011111
G89 00111110011110001011111
G90 00000010000000011011001
G91 00000010000000011011001
G92 11111111111111111111111
G93 00000011000000000011111
G94 00000011000000000011111
G95 00000011000000000011111
G96 00000010100000000011111
G97 00000010100000000011111
G98 11111111111111111111111
G99 11111111111111111111111

61

NOTE:

0 means compatible G codes
1 means incompatible G codes

1-10 10 Series CNC Programming Manual (17)

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

diameter compensation on 1

st-2nd

axes

yes no

plane

G18 b yes Circular interpolation and cutter

diameter compensation on 3

rd-1st

axes

no yes

plane

G19 b yes Circular interpolation and cutter

diameter compensation on 2

nd-3rd

axes

no no

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
G21

yes
yes

Closes GTL profile
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 (17) 1-11

Chapter 1

Programming with 10 Series Systems

CODE GROUP MODAL DESCRIPTION POWER UP

MILL GRINDING

G70 f yes Programming in inches no no
G71 f yes Programming in millimetres yes yes

G80 g yes Disable canned cycles yes yes
G81 g yes Drilling cycle no no
G82 g yes Spot-facing cycle no no
G83 g yes Deep hole drilling cycle no no
G84 g yes Tapping cycle no no
G85 g yes Reaming cycle no no
G86 g yes Boring cycle no no
G89 g yes Boring cycle with dwell no no

G90 h yes Absolute programming yes yes
G91 h yes Incremental programming no no

G79 i no Programming referred to axis no no

home switch

G04 j no Dwell at end of block no no
G09 j no Deceleration at end of block no no

G72 k no Point probing with probe tip no no

radius compensation

G73 k no Hole probing with probe tip no no

radius compensation

G74 k no Probing for theoretical deviation from a

no no
point without probe tip radius
compensation

G93 l yes Inverse time (V/D) feedrate no no

programming mode

G94 l yes Feedrate programming in ipm or

yes no

mmpm

G95 l yes Feedrate programming in ipr or mmpr no yes

G96 m yes Constant surface speed (feet per no yes

minute or metres per minute)

G97 m yes Spindle speed programming in rpm yes no

1-12 10 Series CNC Programming Manual (17)

Chapter 1

Programming with 10 Series Systems

SYNCHRONISATION AND PROGRAM EXECUTION

The terms "synchronised" and "asynchronised" apply only to part program blocks that do not imply
a movement, that is, assignment or calculation blocks. A motion block is any block containing axes
motion together with other actions:

• Axis moves

• M codes

• S codes

• T codes

A synchronisation block is taken into consideration and executed only after the motion block that
precedes it in the program is completed, that is after the axis move has been executed.

On there other hand, a non-synchronised block is executed as soon as it is read by the part
program interpreter, i.e. when perhaps the previous move is still in progress.

The advantage of asynchronous block execution is that variable assignments and complex
calculations can be made between moves. This allows to reduce waiting time between two motion
blocks caused by calculations.

Default Synchronisation

At power up, the following commands and codes are automatically synchronised:

• UDA, SCF, RQO, IPB, DLY, WOS, WAI, SND, GTA, REL, UPR, TCP, UVP, UVC

• G16, G17, G18, G19, G72, G73, G74

All the other commands are not synchronised.

This default assignment can be changed. This means that the commands that are synchronised by
default at power-up can become asynchronous and that the commands that are not synchronised
by default at power-up can become synchronous. The next section explains how to override default
synchronisation.

NOTE:

Default synchronisation cannot be modified for GTA, UPR, TCP, UVP, and UVC instructions.

10 Series CNC Programming Manual (17) 1-13

Chapter 1

Programming with 10 Series Systems

Overriding Default Synchronisation

Under certain circumstances, the part program may request to modify the default synchronisation.

If the command is synchronised by default and the programmer wants it to be executed by the
interpreter as soon as it is read (asynchronous operation), an "&" must be programmed in the first
position of the block, immediately after the "n" number.

If the command is asynchronous and you wish to activate synchronous operation, the first
character in the block must be #.

Both # and & are active only in the block where they are programmed.

To avoid possible damage to the workpiece, note that programming
synchronised blocks between contouring blocks clears the motion buffer at
each synchronised block. This will result in dwells while the buffer is reloaded

WARNING

and all the calculations are performed.

Part Program Interpreter

When the system reads a part program block it executes various activities, depending on the type
of block:

• A motion block will be loaded in the motion buffer queue. If the move is defined by a variable,
the stored move values stored are those of the variable. The buffer size is configurable from 2
to 128 blocks through AMP.

• An asynchronous assign or calculation block will be executed.

Three factors cause the part program interpreter to stop reading blocks:

• The motion buffer is full. When the active motion block is completed, the interpreter will read
another motion block and load it in the buffer queue.

• A non-motion block that contains a synchronised command or a code that forces
synchronisation is read. The interpreter does not start again until the last loaded motion block is
completed. At this point the block calling for synchronisation is executed and the interpreter
starts reading the following blocks.

• Error conditions

1-14 10 Series CNC Programming Manual (17)

Programming with 10 Series Systems

Sequence of execution

1. Diameter axes

2. Scale factors (SCF)

3. Measuring units (G70 G71)

4. Paraxial compensation ( u v w )

5. Inch/metric programming (G90 G91)

6. Mirror machining (MIR)

7. Plane rotation (ROT)

8. Origins (UAO UTO UIO G92)

Programming restrictions for long real (double) formats

The following restrictions apply to long real programming:

Chapter 1

• Max. 15 numbers in total

• Max. 12 integer digits

• Max. 9 decimal digits

The system will display an error if more than 12 integer digits are programmed.

If more than 9 decimal numbers are programmed, the system does not display any error but cuts
off the programmed number at the last allowed digit.

10 Series CNC Programming Manual (17) 1-15

Chapter 1

Programming with 10 Series Systems

END OF CHAPTER

1-16 10 Series CNC Programming Manual (17)

Chapter 2

PROGRAMMING THE AXES

AXIS MOTION CODES

Defining Axis Motion

In this manual axes motion directions are defined in compliance with EIA standard RS-267. By
convention, we always assume that the tool moves towards the part, no matter whether the tool
moves towards the part or the part moves towards the tool in the actual process.

Basic movements can be defined with the motion G codes listed in the following table:

G CODE FUNCTION

G00 Rapid axes positioning

G01 Linear interpolation

G02 Circular interpolation clockwise

G03 Circular interpolation counter clockwise

G33 Constant or variable pitch threading

10 Series CNC Programming Manual (17) 2-1

Chapter 2

Programming the Axes

G00 - Rapid Axes Positioning

G00 defines a linear movement at rapid feedrate that is simultaneous and coordinated for all the
axes programmed in the block.

Syntax

G00 [G-codes] [axes] [offset ] [F..] [a] [auxiliary]

where:

G-codes Other G codes that are compatible with G00 (See "Compatible G codes" table in

Chapter 1).

axes Axis name followed by a numerical value. The numerical value can be programmed

directly with a decimal value or indirectly with an E parameter. Up to nine axes can be
written in a block.

offset Offset factors on the profile. For the X, Y, Z axes these factors are entered with u, v,

and w respectively. See "Paraxial compensation" in Chapter 4 for further information.

F Feedrate for coordinated moves. It is given with the F address followed by the

feedrate value. This parameter does not affect the move of the axes programmed in
the G00 block, but is retained for subsequent feedrate moves. The rapid feedrate
forced by G00 is a velocity along the vector of the axes programmed in the block. The
maximum rapid feedrate is defined during characterisation with the AMP utility.

a Acceleration to be used on the profile.

auxiliary Programmable M, S, and T auxiliary functions. Up to four M functions, one S (spindle

speed) and one T (tool selection) can be programmed in the block.

2-2 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

G01 - Linear Interpolation

G01 defines a linear move at machining feedrate that is simultaneous and coordinated on all the
axes programmed in the block.

Syntax

G01 [G-codes] [axes] [offset ] [F..] [a] [auxiliary]

where:

G-codes Other G codes that are compatible with G01 (See "Compatible G codes" table in

Chapter 1).

axes Axis name followed by a numerical value. The numerical value can be programmed

directly with a decimal value or indirectly with an E parameter. Up to nine axes can be
written in a block.

offset Offset factors on the profile. These factors are entered for the X, Y, Z axes with the

characters u, v, w respectively. See "Paraxial compensation" in Chapter 4 for further
information.

F Feedrate used for the move. It is given with the F address followed by the feedrate

value. If omitted, the system will use the previously programmed feedrate. If no
feedrate has been programmed the control will generate an error.

a Acceleration to be used on the profile.

auxiliary Programmable M, S, T auxiliary functions. Up to four M functions, one S (spindle

speed) and one T (tool selection) can be programmed in the block.

Example:

This example shows how to program a G01 code.

Y

40

Program:

N60 (UGS,X,-10,100,Y,-10,50)
N70 G0 X10 Y10
N80 G01 X90 Y40 F200

10

0

0

10

90

x

10 Series CNC Programming Manual (17) 2-3

Chapter 2

Programming the Axes

G02 G03 - Circular Interpolation

These codes define the following circular movements:

G02 Circular interpolation clockwise (CW)

G03 Circular interpolation counter clockwise (CCW)

The circular move is performed at machining feedrate and is coordinated and simultaneous with all
the axes programmed in the block.

Syntax

G02 [G-codes] [axes] I.. J.. [F..] [a] [auxiliary]

or

G02 [G-codes] [axes] R.. [F..] [a] [auxiliary]

G03 [G-codes] [axes] I.. J.. [F..] [a] [auxiliary]

or
G03 [G-codes] [axes] R.. [F..] [a] [auxiliary]

where:

G-codes Other G codes that are compatible with G02 and G03 (See "Compatible G codes"

table in Chapter 1).

axes Axis name followed by a numerical value programmed directly with a decimal value or

indirectly with an E parameter.

If axes are not programmed in the block, the move is a complete circle in the active
interpolation plane.

I Abscissa of the circle centre. This is a value in millimetres that can be programmed

directly or indirectly with an E parameter. The abscissa is expressed as a diameter
unit when the corresponding axis is a diameter axis. No matter what interpolation
plane you are using, the symbol for the abscissa is always I.

J Ordinate of the circle centre. This is a value in millimetres that can be programmed

directly or indirectly with an E parameter. The ordinate is expressed as a diameter unit
when the corresponding axis is a diameter axis. No matter what interpolation plane
you are using, the symbol for the ordinate is always J.

NOTE: The parameter R cannot be used for arcs of 360 degrees..

2-4 10 Series CNC Programming Manual (17)

Chapter 2

Z

Programming the Axes

R Circle radius alternative to the I and J coordinates. If the arc of a circle is less than or

equal to 180 degrees, the radius must be programmed with positive sign; if the arc of
a circle is greater than 180 degrees the radius must be programmed with negative
sign.

NOTA: R is not allowed with arc of 360 degrees.

F Feedrate used for the move. It is given with the F address followed by the feedrate

value. If omitted, the system will use the programmed value. If no feedrate has been
programmed an error will occur.

a Acceleration to be used on the profile.

auxiliary Programmable auxiliary functions M, S, T. Up to four M functions, one S (spindle

speed) and one T (tool selection) can be programmed in the block.

Characteristics:

The maximum programmable arc is 360 degrees, i.e. a full circle. Before programming a circular
interpolation block, the interpolation plane must be defined with G16, G17, G18, G19. G17 is
automatically active after power up.
The coordinates of the start point (determined from the previous block), the end point and the
centre of the move must be calculated so that the difference between start and end radius is less
than the default value (0.01 mm or 0.00039 inches). If this difference is equal or greater than the
default value, the control displays an error message and the circular move is not performed.

Incremental programming (G91) can be used in conjunction with circular interpolation. With G91
the end point and the centre point of the circular move are referenced to the start point
programmed in the previous block.
The direction (CW or CCW) of a circular interpolation is defined by looking in the positive direction
of the axis that is perpendicular to the active interpolation plane.The following examples show the
directions for circular interpolation on the active planes.

G02

XY

G02

G03

G03

Y

G02

G03

Z

ZX

Y

X

Directions of a circular interpolation

10 Series CNC Programming Manual (17) 2-5

Chapter 2

Y

Programming the Axes

Circular interpolation in absolute programming with the I and J coordinates of the centre of the
circle.

N14 X10 Y20
N15 G2 X46 Y20 I28 J20 F200
N16 G3 X64 Y38 I46 J38

G02

G03

0

28

46

64

38

20

0

X

Circular interpolation in absolute programming with the value R of the radius of the circle.

N14 X10 Y20
N15 G2 X46 Y20 R18 F200
N16 G3 X64 Y38 R18

Circular interpolation in incremental programming with the coordinates J and I.

N14 X10 Y20
N15 G2 G91 X36 I18 J0 F200
N16 G3 X18 Y18 I0 J18

Circular interpolation in incremental programming with the value of the radius R.

N14 X10 Y20
N15 G2 G91 X36 R18 F200
N16 G3 X18 Y18 R18

2-6 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

CET (PRC) - Circular Endpoint Tolerance

In circular interpolations, CET defines the tolerance for the variance between the starting and final
radiuses of the circle arc.

Syntax

CET=value

where:

value Tolerance expressed in millimetres. The default value is 0.01 mm.

Characteristics:

If the difference between starting and final radius is smaller than the tolerance but not zero, the
system normalises the circle data according to the values specified in CET and ARM.

If the difference is equal to or greater than the value assigned to CET, an error occurs and the
programmed final points will not be executed. In this case, you must either modify the program or
increase the CET tolerance.

The value assigned to CET can be modified as follows:

• In the AMP configuration

• By means of a specific data entry

• By writing a new CET in the part program.

The CET tolerance is always expressed in the characterised measuring unit (G70/G71 apply).

If the variance between programmed start and final radius is higher than the CET value, the circle
arc can be executed as follows:

• By making the CET value greater than the actual variance

• By programming the arc with the circle radius rather than with the centre using this format:

G2/G3, final point and R radius

A RESET re-establishes the default tolerance.

Example:

CET=0.02 defines a 0.02 mm tolerance

10 Series CNC Programming Manual (17) 2-7

Chapter 2

Programming the Axes

FCT - Full Circle Threshold

In a circular interpolation, the FCT instruction defines a threshold for the distance between the first
and the last point in an arc. Within this distance the arc is considered a full circle.

Syntax

FCT=value

where:

value Threshold expressed in millimetres. The default value is 0.001 mm.

Characteristics:

The FCT command allows to deal with inaccurate program data that would otherwise prevent the
system from forcing a complete circle. In other words, if the distance from the first to the last point
is less than FCT, the system uses the points as if they were overlapping and forces a full circle.

FCT thresholds can be modified as follows:

• In the AMP configuration

• By means of a specific data entry

• By writing a new CET in the part program.

The FCT threshold is always expressed in the characterised measuring unit (G70/G71 apply).

A RESET re-establishes the default threshold.

Example:

G71
FCT=0.005
In this example, FCT defines a threshold 0.005 millimetres.

2-8 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

ARM - Defining Arc Normalisation Mode

The ARM code defines the method with which the system normalises an arc (programmed with the
centre coordinates I and J, and a final point) in order to render it geometrically congruent.

An arc is normalised when the variance between initial and final radius is less than the
characterised accuracy tolerance or than the tolerance programmed with the CET command.

Before executing an arc, the system calculates the difference between initial and final radiuses.

• If the difference is zero, the control will execute the programmed arc without normalising it.

• If the difference is greater than the CET value, the control will stop without executing the move,

and display a profile error message.

• If the difference is less than the CET value, the control will execute the move normalising the

arc with the method specified by ARM.

• If the distance is less than the FCT threshold, the system will force the complete circle. For ISO

blocks with radius compensation, the system checks the difference twice: first on the base
profile without compensation (normalisation stage) and then on the compensated profile (motion
generation stage).

Syntax

ARM=arc mode

where:

arc mode Is the numerical value that defines the arc normalisation mode.

Valid values are:

0 displaced centre within the CET tolerance (default mode)
1 displaced starting point displaced the CET tolerance
2 displaced centre independent from the CET tolerance
3 centre beyond the CET tolerance range

The default value is zero.

Characteristics:

The arc normalisation mode can be modified as follows:

• In the AMP configuration

• By means of a specific data entry

• By writing a new CET in the part program.

The examples that follow illustrate ARC normalisation modes.

10 Series CNC Programming Manual (17) 2-9

Chapter 2

Programming the Axes

ARM=0

This is an arc through the initial and final programmed points whose centre is displaced within the
tolerance defined by CET. The arc is executed with averaged radius.

starting point

CET

averaged radius

CS

C

CET

final point

C = programmed center

CS= displaced center

ARM=1

This is an arc through the programmed final point and the starting point displaced within the CET
tolerance. The arc is executed with final radius.

starting point

CET

C

final point

C= programmed center

2-10 10 Series CNC Programming Manual (17)

Chapter 2

A

Programming the Axes

ARM=2

This is an arc whose centre is displaced irrespective of the tolerance defined with CET. In this case
the arc is executed with averaged radius.

CET

CET

C

starting point

CS

arc with averaged radius

final point

C= programmed center

CS = displaced center

ARM=3

If the displacement of the centre arc is within the CET tolerance defined with CET, the arc centre
will be displaced and the arc will pass through the programmed starting and final points. If the
displacement of the centre is not within the CET tolerance, the arc will have the programmed
centre and pass through the displaced starting and final points (both points are displaced within the
CET/2 tolerance).
In this case the arc is executed with averaged radius.

CET

CS

starting point

CET

C

C = programmed center

CS = displaced center

averaged radius

final point

CET

CET

B

starting point

arc with averaged
radius plus initial
and final steps

C

CS

final point

10 Series CNC Programming Manual (17) 2-11

Chapter 2

Programming the Axes

IMPORTANT

With ARM = 1 or ARM = 3 the resultant profile can show inaccuracies ("steps"):

With ARM = 1 there will be a step at circle start equal to the difference between
starting and final radiuses.

In case of ARM = 3 there will be a step both at circle arc start and end.

To prevent these steps from causing a servo error, we suggest that you program
a CET value smaller than the characterised servo error threshold.

2-12 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

CRT - Circular interpolation speed reduction threshold CRK - Circular interpolation speed reduction constant

The variables CRT (Circle Reduction Threshold) and CRK (Circle Reduction K-Constant) are used
for reducing the speed on circular elements by applying different reduction algorithms depending
on the sign of the CRT parameter. Speed reduction will be:

- as a function of the radius of the element only, if CRT > 0

- as a function of the radius and centrifugal acceleration, if CRT = 0

- as a function of the radius and tolerated interlocking error, if CRT < 0

Syntax

CRT = value

where:

value If value > 0 => value, it is the threshold radius below which the reduction must be

applied. A value of 0 (zero), which is the default value, cancels this operation.

If value < 0 => abs(value), it is the maximum departure in mm desired between
the programmed and the actual path. A value of 0 (zero), which is the default
value, cancels this operation.

CRK = value

where:

value if CRT > 0 => is a constant for modulating the reduction in speed. The value

set by default is 1.

if CRT = 0 => Is a constant for modulating the reduction in speed depending

on centrifugal acceleration.

if CRT < 0 => Is the axis position interlocking gain (Kv). The value to be

specified must be the same as configured in AMP in the
corresponding axis field.

If both CRT and CRK are nil, then no reduction speed is applied to the circular elements.

10 Series CNC Programming Manual (17) 2-13

Chapter 2

R

Programming the Axes

Characteristics:

CRT is the variable identifying the type of strategy to be adopted to reduce speed on circles. If:

• CRT > 0 =>

By assigning any value positive to the variable CRT, the speed is reduced on
all circular elements with a smaller radius than the value set. The value
assigned to the variable CRK enables this reduction to be modulated. The
speed is reduced as shown in the graph below, in which it is assumed that
the programmed speed Vp is equal to 1 and the variable CRT is equal to 1.

V

Vp = 1

Crk

0.606

0,271

2.718

0.135

0.018

0.5

1

2

4

• CRT = 0 =>

Crt = 1

When CRT becomes 0, the CRK value (if other than zero) is used, in circular
movements, in order to recalculate processing speed. In circular movements,
in fact, processing speed is generally limited by the radius of the
circumference (centrifugal acceleration) according to the following
relationship:

V lav = Min ( √ a radius, V Prog )

where a is the minimum acceleration between the two axes involved in the
circular movement.

CRK changes this relationship as follows

V lav = Min ( CRK * √ a radius, V Prog )

and therefore makes it possible to increase (CRK > 1.0) or decrease (CRK <

1.0) the limitation associated with the centrifugal acceleration. With a value of

1.0 the standard calculation is retained.

2-14 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

• CRT < 0 =>

By assigning any value negative to the variable CRT, the speed is reduced on
all circular elements as a function of the curvature radius of the path in order
to make sure the error does not exceed the limit specified in CRT.

Hence, maximum admissible speed will be a function of the radius, the error
specified by the absolute value of CRT and the interlocking gain CRK,
according to the following formula:

Vmax

=

CRK *

2 * R * abs(CRT) * f(VFF,FLT_2)

Where f(VFF,FLT_2) is a function that depends on the Velocity Feed Forward
(VFF) set and the type 2 filter, if any, activated (centripetal acceleration
compensation filter). For further details, see the Chapter on filters in this
manual.

NOTE:

Since speed on circles is limited as a function of the percentage of VFF, it is
necessary, when working with VFF, to have enabled the process variable
VFF and configured the same percentage value both on the drives and on the
axes.

The values assigned to the variables CRT and CRK may be modified as follows

• by means of the AMP command during configuration

• from the part program with the specified syntax.

The values assigned to CRT are always expressed in the current unit of measurement of the
process (the G70/G71 functions are applied).

The RESET command restores the characterization values.

10 Series CNC Programming Manual (17) 2-15

Chapter 2

Programming the Axes

Helical Interpolation

G02 and G03 program a helical path in only one block. The system performs the helical path by
moving the plane axes in a circular interpolation while the axis that is perpendicular to the
interpolation plane moves linearly.

To program a helical path, simply add a depth coordinate and the helix pitch (K) to the parameters
specified in the circular interpolation block.

Syntax

G02 [G-codes] [axes] I.. J.. K.. [F..] [auxiliary]

or

G02 [G-codes] [axes] R.. K.. [F..] [auxiliary]

G03 [G-codes] [axes ] I.. J.. K.. [F..] [auxiliary]

or
G03 [G-codes] [axes ] R.. K.. [F..] [auxiliary]

where:

G-codes Other G codes that are compatible with G02 and G03 (See "Compatible G

codes" table in Chapter 1).

axes An axis letter followed by a numerical value programmed (either decimal value

or E parameter).

If no axes are programmed in the block, the move will generate a full circle on
the active interpolation plane.

I Abscissa of the circle centre. This is a value in millimetres (decimal number or E

parameter). The abscissa is expressed as a diameter unit when the
corresponding axis is a diameter axis. No matter what the interpolation plane,
the symbol for the abscissa is always I.

J Ordinate of the circle centre. This is a value in millimetres (decimal number or E

parameter). The ordinate is expressed as a diameter unit when the
corresponding axis is a diameter axis. No matter what the interpolation plane,
the symbol for the ordinate is always J.

2-16 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

R Circle radius. It is specified with the R address followed by a length value, and

is alternative to the I and J coordinates.

K Helix pitch. This parameter is specified with the K address followed by the pitch

value. It can be omitted if the helix depth is less than one pitch.

F Feedrate. It is specified by the F address followed by a value. If it is omitted, the

system will use the previously programmed feedrate. If no feedrate has been
programmed, the system will signal an error.

auxiliary Programmable M, S, and T functions. Up to four M functions, one S (spindle

speed) and one T (tool selection) can be programmed in the block.

Characteristics:

If Z is a multiple of K, it is not necessary to program the final point

If the depth is not an integer number of pitches, i.e. if Z is not equal to n * K), the length of the circle
arc must be calculated with the decimal remainder of the pitch number. For example, if Z = 2.7 * K,
then the arc that must be programmed is 360 * (2.7 - 2) = 252 degrees.

Example:

G2 X . . Y. . Z . . I . . J . . K . . F. .

In this example, addresses X, Y, I, and J refer to circle programming; addresses Z and K refer to
helix programming and are respectively the depth and the helix pitch. The figure below shows the
typical dimensions of a helical interpolation.

Dimensions Helix

10 Series CNC Programming Manual (17) 2-17

Chapter 2

Programming the Axes

G33 - Constant or Variable Pitch Threading

G33 defines a cylindrical, taper, or face threading movement with constant or variable pitch. The
threading move is synchronised to spindle rotation. The parameters programmed in the block
identify the type of thread.

Syntax

G33 [axes] K.. [I..] [R..]

where:

axes An axis letter followed by a numerical value.

K Thread pitch (mandatory). For variable pitch threads, K is the initial pitch.

I Pitch variation for variable pitch threading. For increasing pitch threading, I must

be positive; for decreasing pitch threading I must be negative.

R Deviation from the zero spindle angular position in degrees. R is used in

multistart threading to avoid displacing the starting point.

Characteristics:

All these numerical values can be programmed directly with decimal numbers or indirectly with E
parameters.

In decreasing pitch threads, the initial pitch, the pitch variation, and the thread length must be
calculated so that the pitch is greater than zero before reaching the final coordinate. Use the
following formula:

2

I <

where:
I Is the maximum pitch variation

K Is the initial pitch

(Zf - Zi) Is the thread length.

K

2 (Zf - Zi)

IMPORTANT

2-18 10 Series CNC Programming Manual (17)

During the threading cycle the control ignores the CYCLE STOP button and the
FEEDRATE OVERRIDE selector/softkey, whereas the SPINDLE SPEED
OVERRIDE selector must be disabled by the machine logic.

VFF may be disabled with the dedicated softkey or with a VFF command.

Chapter 2

Programming the Axes

Constant Pitch Threading

The figures that follow illustrate examples of constant pitch threading. Note that the U axis is a
diameter axis.

Cylindrical threading

U

Conical threading

U

Z

K2

Z-100

Z

K3

Z-80

U40

Part program block: G33 Z-100 K2

Part program block: G33 U40 Z-80 K3

Cylindrical-conical threading

Part program blocks: G33 Z-95 K2 .5

Z-100 U52 K2.5

U52

10 Series CNC Programming Manual (17) 2-19

Chapter 2

Z

Programming the Axes

Variable Pitch Threading

The figures that follow illustrate variable pitch threading. Note that the U axis is a diameter axis.

Cylindrical threading with increasing pitch

Z

4

5

6

7

8

9

Part program block: G33 Z-50 K4 I1

Conical threading with increasing pitch

Z

U

4

5

6

7

8

9

Part program block: G33 U50 Z-40 K4 I1

Cylindrical thread with decreasing pitch

U

10

9

8

7

6

5

4

Part program block: G33 Z-50 K10 I-1

2-20 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

Multi-start threading

An R word in a G33 block makes the control start moving the axes from an angular position that
varies according to the programmed R value.

This permits to program the same start point for all threads, rather than move the start point of
each thread by a distance equal to the pitch divided by the number of starts.

Example:

Three-start threading

N37 G33 Z3 K6 1st thread

.
.
.

N41 G33 Z3 K6 R120 2nd thread

.
.
.

N45 G33 Z3 K6 R240 3rd thread

10 Series CNC Programming Manual (17) 2-21

Chapter 2

Programming the Axes

Rotary Axes

In the system characterisation, axes can be configured as rotary axes, i.e. a rotary table.

To program rotary axis moves simultaneous to and coordinated with the other axes programmed in
the same block:

• Always use decimal degrees (from +0.00001 to +99999.99999 degrees) starting from a pre­selected origin.

• Select either the rapid rate (G00) or the feedrate (G01). In a rotary move rates are always
expressed in degrees per minute (dpm, F5.5 format). For example, with F75.5 the axis moves
at 75.5 dpm.

To perform milling operations on a circle with a rotary table, calculate the rotary rate with the
following formula.

360

F =

A

*

D

= 114,64

pi

*

A
D

where:

F Is the rotary rate in dpm

A Is the linear rate on the arc in millimetres or inches per minute

D Is the diameter on which the milling operation is performed (in mm or inches).

To move rotary and linear axes simultaneously in the same block, you may calculate the feedrate
with one of the following formulas.

With G94:

F = A *

where:

F Is the feedrate

A Is the feedrate on the part (in mm/min or inches/min)

X Y Z B C Is the actual travel performed by each axis (in mm or inches for linear axes, in

degrees for rotary axes)

L Is the resultant path length (in mm or inches).

X2+Y2+Z2+B2+C

L

2

2-22 10 Series CNC Programming Manual (17)

With G93:

Chapter 2

Programming the Axes

F =

A

X2 + Y2 + B

2

where:

F Is the feedrate

A Is the desired feedrate (in mm/min or inches/min) on the part

X Is the X axis incremental distance

Y Is the Y axis incremental distance

B Is the B axis incremental distance

The control cannot calculate the desired tool feedrate directly because the radius is not
programmed. In these cases, the feedrate can be specified as inverse time with G93.

A block moving only the rotary axes generates an arc. If rotary and linear moves are combined, the
resulting path may be an Archimedean spiral, a cylindrical helix or more complex curves,
depending on the programmed number of linear axes.

10 Series CNC Programming Manual (17) 2-23

Chapter 2

Programming the Axes

Axes with Rollover

Axes with rollover axis are rotary or linear axes whose position is controlled between zero and a
positive value configured in the rollover pitch parameter.

In the following description the axsi with rollover is rotary and has a 360 degree rollover pitch. We
assume that the axis position is controlled in the 0 to 359.9999 degree range. That is, when the
axis reaches 360 degrees, the displayed position rolls over to zero degrees.

An axis with rollover can be programmed in a block or in a MDI in two different modes:

absolute mode (G90) programs the move in degrees.

incremental mode (G91) programs the move as increments in degrees from the current

axis position.

G90 - Absolute mode

In this mode:

• Displayed position is from 0 to +359.99999 degrees

• Programmed range is from 0 to ± 359.99999 degrees

• Direction of axis rotation depends on the sign of the programmed move. By convention, a

positive move is clockwise and a negative move is counter clockwise.

2-24 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

For example, let's assume that rotary axis B is positioned at 90 degrees and the following block is
written in the part program or in an MDI:

G90 B45

180

90

Clockwise Rotation

The B axis rotates by 315 degrees clockwise from the 90 degree position to reach the absolute
position of 45 degrees (the sign of the move is positive).

Now let's assume that the B rotary axis is at 90 degrees and, the following block is written in the
part program or in an MDI:

G90 B-0

359.999

0

45

0

90

Counter clockwise Rotation

The B axis rotates by 90 degrees counterclockwise to absolute position 0 degrees because the
sign of the move is negative.

10 Series CNC Programming Manual (17) 2-25

Chapter 2

Programming the Axes

G91 - Incremental mode

When an axis with rollover is programmed in incremental (G91) mode, the following conditions
apply:

• Displayed position is from 0 to +359.99999 degrees.

• Program range is from +/-0.00001 to +/-99999.99999 degrees.

• Direction of axis rotation depends upon the sign of the programmed move. By convention, a

positive move is clockwise and a negative move is counter clockwise.

IMPORTANT

range is greater than +359.999 degrees.

For example, if the absolute zero position of the B rotary axis is 0 degrees and the following block
is written in the part program or in an MDI:

G91 B765

0

45

The displayed position is beyond the programmed range when the programmed

90

Incremental clockwise rotation

The B axis makes two complete clockwise revolutions plus 45 degrees (360 + 360 + 45 = 765).

2-26 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

Pseudo Axes

A pseudo axis is an auxiliary function that may be addressed as an axis and is handled by the
machine logic. The pseudo axis name can be any allowed axis name (X,Y,Z,A,B,C,U,V,W,P,Q,D).
In a part program block it is possible to program up to 3 pseudo axes but in the AMP it is possible
to configure up to 6 pseudo axes.

Diameter Axes

A reaming/facing head can be mounted on the spindle and controlled simultaneously with other
axes. By programming such an axis (typically a U axis) as a diameter, the following can be
obtained:

• Boring operations on cylindrical or conical holes

• Circular radiuses (concave or convex)

• Chamfers

• Grooves

• Facing operations

• Threads

Programming a U (diameter) axis is similar to programming other linear axes; however, its
coordinates must be expressed in diameters. The measuring units can be inches or millimetres
according to the current mode ( G70/G71).

When the U axis is programmed in the same block as an X, Y or Z move, it is simultaneous with
and coordinated to the other axes. U axis moves can be performed at rapid rate (G00) or feedrate
(G01) with F in ipm or mmpm.

Before executing a profile with the U axis, the interpolation plane must be defined with the following
command:

G16 Z U

IMPORTANT

The order of Z and U in this command is critical, i.e. G16 UZ and G16 ZU define
two different interpolation planes.

Cutter diameter compensation (G41 or G42) and a machining allowance (MSA)
can be applied to profiles programmed with U.

10 Series CNC Programming Manual (17) 2-27

Chapter 2

Programming the Axes

Example

:

This is an example reaming/facing head used in a finishing operation.

N116 (DIS, "FINISHING WITH R/F HEAD")
N117 F60 S630 T9 .9 M6
N118 G16 Z U ;Defines interpolation plane
N119 (UAO, 2) ;Calls absolute origin for the head
N120 (UTO, 1, Z-200) ;Temporary origin for Z (skimming the part)
N121 X Y160 M3 ;Position to hole 1
N122 G41 Z2 U51
N123 G1 Z-1 U44 .98 ;Executes the chamfer
N124 Z-44 ;Executes hole diameter 45
N125 G G40 U40
N126 Z2 F40 S380
N127 G41 Y U106 ;Positions to hole 2
N128 G1 Z-1 U99 .975 ;Executes the chamfer
N129 Z-15 ;Executes hole diameter 100
N130 r5 ;Executes radius R = 5
N131 U60 ;Executes counter boring
N132 r-3 ;Executes radius R = 3
N133 Z-40 U40 ;Executes taper
N134 G40 Z-44 ;Continues Z axis travel
N135 G U35
N136 Z100 M5
N137 G16 X Y
N138 (UAO,1)

2-28 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

The direction of the arcs programmed with G02/G03 or with the r address and the direction for
cutter diameter compensation (G41/G42) can be determined by looking at the profile on the Z-U
plane. Since negative diameters are usually not programmed, you must consider only the first two
quadrants of the plane.

10 Series CNC Programming Manual (17) 2-29

Chapter 2

Programming the Axes

UDA - Dual Axes

It is possible to treat one or more axes as slaves or subordinate to another defined as the master.
In this way only the movements of the Master need be programmed as the movement of the slaves
is determined by those of the Master to which they are associated and by whether or not reverse
mirror movement has been applied.

Syntax

(UDA,master1/slave1
(UDA)

where:

master1. . . master4 Are the master axis names (one ASCII character per axis). You can

slave1. . . slave8 Are the slave axes names (one ASCII character per axis). You can

no parameters (UDA) without parameters disables the dual axes mode (UDA)

Characteristics:

Dual axes management does not require any special setting in the system with AMP.
After an (UDA...) command, the positive operating limit is the minimum between the positive limit of the
master axis and the current position of the master plus the distance that may be covered by the slave
axis. In short:

PositiveLim = min(Master PositiveLim, MasterPosition + Slave PositiveLim - SlavePosition)

In the case of a "mirror", the distance that may be covered by the slave refers to its negative limit, so it
will be:

[,master2/slave2,master3/slave3,master4/slave4])

program up to 4 master axes.

program a maximum of 8 slave axes per master.

PositiveLim = min(Master PositiveLim, MasterPosition - Slave NegativeLim + SlavePosition)

The considerations made for the positive limit also apply to the negative limit:

NegativeLim = max(Master NegativeLim, MasterPosition + Slave NegativeLim - SlavePosition)

In the case of a mirror, it will be:

NegativeLim = max(Master NegativeLim, MasterPosition - Slave PositiveLim + SlavePosition)

2-30 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

When the (UDA...) command is executed, reference must be made both to the master axis and the
slave axes.

The RESET command does not cancel the association between the master and slave axes.

Dual axes may be used on rotated planes or in polar or cylindrical coordinates (UVP, UVC).

Dual axes, whether master or slave, must be defined on real axes and not virtual axes.

NOTE:

The names of masters and slaves must be separated by a / (slash).

IMPORTANT

axis name. This rule does not apply to master axes.

Example:

(UDA,X/-U) U is slaved and mirrored to X
(UDA, A/B - CD) B, C, D are slaved to A and C is mirrored to A

To mirror the slave axis movement, you must program the - operator before the

10 Series CNC Programming Manual (17) 2-31

Chapter 2

Programming the Axes

SDA - Special Dual Axes

It is possible to treat one or more axes as slaves or subordinate to another defined as the master.
In this way only the movements of the Master need be programmed as the movement of the slaves
is determined by those of the Master to which they are associated and by whether or not reverse
mirror movement has been applied. The movement of the master and slave axes can occur even if
the axes are not referenced.

Syntax

(SDA,master1/slave1
(SDA)

where:

master1. . . master4 Are the master axis names (one ASCII character per axis). You can

slave1. . . slave8 Are the slave axes names (one ASCII character per axis). You can

no parameters (SDA) without parameters disables the special dual axes mode (SDA)

Characteristics:

After an (SDA...) command, the positive operating limit is the minimum between the positive limit of the
master axis and the current position of the master plus the distance that may be covered by the slave
axis. In short:

PositiveLim = min(Master PositiveLim, MasterPosition + Slave PositiveLim - SlavePosition)

In the case of a "mirror", the distance that may be covered by the slave refers to its negative limit, so it
will be:

[,master2/slave2,master3/slave3,master4/slave4])

program up to 4 master axes.

programa maximum of 8 slave axes per master.

PositiveLim = min(Master PositiveLim, MasterPosition - Slave NegativeLim + SlavePosition)

The considerations made for the positive limit also apply to the negative limit:

NegativeLim = max(Master NegativeLim, MasterPosition + Slave NegativeLim - SlavePosition)

In the case of a mirror, it will be:

NegativeLim = max(Master NegativeLim, MasterPosition - Slave PositiveLim + SlavePosition)

2-32 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

Upon activating the (SDA,...) command the master and the slaves need not be referenced.
The RESET command does not remove the master/slave association.

This allows one to perform the zero point micro-search cycle with dual movement active. In this
case performing the zero point micro-search cycle, the system simultaneously moves the
associated slaves. At the end of the search the master axis is referenced where as the slave axes
are not. In order to reference the slave axes they should be exchanged, one by one, with the
master axis by new SDA programming and the zero point micro-search cycle repeated for each
one of them, redefined as the master. The initialisation of the slaves is not however necessary if
one intends to program only the master with SDA active.

The use of the SDA function is recommended in cases where a zero point micro-search cycle is to
be performed following a shutdown of the system with the work still on the work-bench.

NOTE:

The names of masters and slaves must be separated by a / (slash).

IMPORTANT

the axis name. This rule does not apply to master axes.

Example:

(SDA,X/-U) U is slaved and mirrored to X
(SDA, A/B - CD) B, C, D are slaved to A and C is mirrored to A

To mirror the slave axis movement, you must program the - operator before

10 Series CNC Programming Manual (17) 2-33

Chapter 2

Programming the Axes

XDA - Master/Slave axes

One or more axes can be used as “slave” axes, i.e. subordinate to another axis, defined as
“master”. In this manner, you only need to program the movements of the master, since the
movements of the slaves are determined by the master they are associated with and by a following
factor, which is defined specifically for each individual slave. Commands of different types can be
imparted with this feature, each of them having a specific syntax.

Master/Slave Association

This instruction defines the association between a master axis and its slaves (up to 8 axes). It

does NOT activate the following function, whose activation is by means of a specific command.

This means that after this instruction a movement of the master does not bring about a movement
of the slave(s).

movements cannot be programmed.

After this instruction and until the slave is released from the master, slave

Syntax

(XDA, 1, master/slave1[slave2[..]], mode, ratio, space)

where:

master Is the name of the master axis and is denoted by a single ASCII character.

slave1…slave8 Are the names of the slave axes (each of them denoted by a single ASCII

character). You can program up to 8 slaves.

mode Defines the master axis following mode used by the slave(s). It can be:

0
1
2
3

ratio This is the master following ratio specified for the slave(s). It must be

viewed as a multiplication factor for the feedrate of the master or the
distance covered by it. If the value of this ratio is 1.0, the motion of the
master is reproduced exactly by the slave; if it is smaller than 1.0,
feedrate/distance are reduced, if it is greater than 1.0 they are increased.
This value can be preceded by a sign.

The slave follows the master point by point
The slave follows the master in terms of speed
The slave follows the master in terms of position
The slave follows the master in terms of position, and the
synchronisation distance is taken up

distance This is the distance to be covered by the slave to synchronise with the

motion of the master.

2-34 10 Series CNC Programming Manual (17)

Chapter 2

r

A

Programming the Axes

Characteristics:

The master axis can identify either an axis present in the process in which the XDA command is
activated or an axis which is not present; in the latter case, a “virtual” axis, having the name
specified, will be created; this axis will have the dynamic characteristics inherited from the slave
axes (the lowest values of feedrate, accelerations and jerk). This axis may be part of a
virtualisation (UPR, UDA,…) and also of a TCP. The operation of master axis Homing cannot be
performed.

At least one slave axis must be present in the process in which the XDA command is activated; it
can be a SHARED axis, i.e. an axis shared with the machine logic environment. In this connection,
the axis may continue to be moved by the machine logic even after the association with the master,
however it cannot be moved while it is following the master. It cannot be part of any virtualisation or
TCP.

Let us now examine the various following modalities available:

Mode 0

In this mode, the slave axis follows the master proportionately to the value of the ratio (if the ratio =
1, the slave reproduces the movement of the master axis exactly), synchronisation is
instantaneous and the variation in the feedrate of the slave is “

in steps”. Slave position and

feedrate values are calculated, instant by instant, according to the following formulas:

Vslave = Vmaster * FollowRate

PosSlave = PosSlave

V

V maste

t 0

+ (PosMaster – PosMaster

t0

V slave

ctivation =

Synchronisation

) * FollowRate

t0

t

If the speed specified for the slave axis as a result of the following command exceeds the
maximum admissible value for this axis, the system will reduce the feedrate requested accordingly
and will give out an emergency (servo error) message, in that the slave is unable to follow the
required position.

10 Series CNC Programming Manual (17) 2-35

Chapter 2

r

A

r

A

Programming the Axes

Mode 1

In this mode, the slave follows the feedrate of the master proportionately to the value of the ratio (if
the ratio = 1, the slave copies the movement of the master axis exactly); the synchronisation
depends on the dynamic characteristics of the slave axis and/or the distance parameter which
defines the synchronisation distance.

If the distance value = 0, the slave will synchronise with the master based on its maximum
acceleration and using linear ramps

only.

V

V maste

Synchronisation

t 0

V slave

ctivation

t 1

t

If the value is not 0, the slave will synchronise with the master based on an acceleration calculated
as a function of the synchronisation distance and using linear ramps

only. The acceleration will be

calculated again with each sampling process based on the following formula

Aslave = ((Vmaster * FollowRate)2 + Vslave 2 ) / 2 * Distance

where the value of the distance is gradually reduced based on the distance covered during the
synchronisation stage. No check is made on the ensuing acceleration value, and therefore servo
errors may arise if the acceleration exceeds the maximum value that can be withstood by the axis.

V maste

Synchronisation

V slave

ctivation

t 0

t 1

Distance

t

2-36 10 Series CNC Programming Manual (17)

Chapter 2

r

A

Programming the Axes

Once the synchronisation with the master has taken place, the slave will move according to this
formula:

Vslave = Vmaster * FollowRate

The feedrate (Vslave) determined in this manner is “theoretical”, since it is necessary to determine
whether this request is compatible with the dynamic characteristics of the axis (maximum feedrate
and maximum acceleration). The moment the feedrate of the master varies, the slave will follow
this variation based on its acceleration value. If the feedrate requested of the slave exceeds its
maximum admissible feedrate, the system will reduce the feedrate requested accordingly. Hence,
the feedrate and acceleration values with which the slave has to be moved,

Vslave

and Aslave i,

i

will be determined instant by instant. The position of the slave will therefore be calculated on the
basis of these values:

PosSlave

= PosSlave

tn+1

+ Vslave i + Aslave

tn

i

Mode 2

In this mode, the slave follows the position of the master proportionately to the value of the ratio (if
the ratio = 1 the slave reproduces exactly the movement of the master); synchronisation depends
on the dynamic characteristics of the slave axis and/or the distance parameter which defines the
synchronisation distance.

If the distance value is 0, the slave will synchronise with the master based on its maximum
acceleration and using linear ramps

V

V maste

only.

Synchronisation

V slave

ctivation

t 0

t 1

t

10 Series CNC Programming Manual (17) 2-37

Chapter 2

r

A

Programming the Axes

If the value of distance is not 0, the slave axis will synchronise with the master axis based on an
acceleration calculated as a function of the synchronisation distance and using linear ramps

only.

The acceleration value will be calculated again with each sampling step according to this formula

Aslave = ((Vmaster * FollowRate)2 + Vslave 2 ) / 2 * Distance

where the value of the distance is gradually reduced based on the distance covered during the
synchronisation stage. No check is made on the ensuing acceleration value and therefore servo
error messages may be generated the moment the acceleration exceeds the maximum value that
the axis can withstand.

V maste

Synchronisation

ctivation

t 0

t 1

V slave

Distance

t

Once the synchronisation with the master axis has occurred, the slave will move according to the
following formulas:

PosSlave = PosSlavet1 + (PosMaster – PosMaster

) * FollowRate

t1

Vslave = Vmaster * FollowRate

The position, PosSlave, and the feedrate, Vslave, determined in this manner should be rated as
“theoretical” values, since it is necessary to determine whether the values requested are
compatible with the dynamic characteristics of the axis (Maximum feedrate and maximum
acceleration). The moment the feedrate of the master varies, the slave will follow this variation
according to its own acceleration value. If the feedrate requested for the slave exceeds the
maximum value admissible for this axis, the system will reduce the feedrate accordingly. To this
end, the two values with which to move the slave,

Vslave

and Aslave i will be calculated instant

i

by instant. The actual position of the slave axis will therefore be calculated on the basis of these
values:

PosSlave

= PosSlave

tn+1

+ Vslave i + Aslave

tn

i

The difference between the actual and the theoretical position of the axis is taken up by the slave
during its motion (even when the master has stopped moving) by moving, to the extent feasible, at
a rate higher than the theoretical value (

Vslave).

2-38 10 Series CNC Programming Manual (17)

Chapter 2

r

A

r

Programming the Axes

Mode 3

In this mode, the slave follows the position and feedrate of the master proportionately to the value
of the ratio (if the ratio = 1, the slave reproduces exactly the movement of the master);
synchronisation depends on the dynamic characteristics of the slave.

V maste

V slave

ctivation =

Synchronisation

Distance lost
during acceleration
stage

t 0

Distance recovered
after synchronisation
with Maste

t

During the entire movement of the slave (i.e. both during and after the synchronisation stage), the
motion of the axis is according to the following formulas (always using linear ramps):

PosSlave = PosSlaveto + (PosMaster – PosMaster

) * FollowRate

t0

Vslave = Vmaster * FollowRate

The position (PosSlave) and the feedrate (Vslave) determined in this manner should be rated as
“theoretical” values, in that it is necessary to determine whether these requests are compatible with
the dynamic characteristics of the axis (max admissible feedrate and max admissible acceleration).
The moment the feedrate of the master varies, the slave follows the variation according to its own
acceleration value. If the feedrate requested of the slave is higher than its maximum admissible
feedrate, the system reduces the feedrate requested accordingly. To this end, the two values with
which the axis is to be moved (

Vslave

and Aslave i) will be calculated instant by instant. The

i

actual position of the slave will therefore be calculated on the basis of these values:

PosSlave

= PosSlave

tn+1

+ Vslave i + Aslave

tn

i

The difference between the actual and the theoretical position of the axis is taken up by the slave
during its motion (even when the master has stopped moving) by moving, to the extent feasible, at
a rate higher than the theoretical value (

Vslave).

10 Series CNC Programming Manual (17) 2-39

Chapter 2

Programming the Axes

Releasing the Slave(s) from the Master

This instruction removes the association between the master and the slave(s). Following this

instruction it will be possible to program any movement of the slave axis.

Syntax

(XDA)

2-40 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

Defining/Changing the following ratio

This instruction defines/changes the parameter that determines the ratio according to which the
master is followed by the slave(s) concerned.

Syntax

(XDA, 2, slave1[slave2[..]], ratio)
(xda

, 2, slave1[slave2[..]], ratio)

where:

slave1…slave8 are the names of the slave axes (each of which is denoted by a single

ASCII character). You can program up to 8 slaves.

ratio This is the master following ratio specified for the slave(s). It must be

viewed as a multiplication factor for the feedrate of the master or the
distance covered by it. If the value of this ratio is 1.0, the motion of the
master is reproduced exactly by the slave; if it is smaller than 1.0,
feedrate/distance are reduced, if it is greater than 1.0 they are increased.
This value can be preceded by a sign.

Characteristics:

The command can be used both when a slave is already following the master axis (it then brings
about the release of the slave from the master and activates a new synchronisation stage using the
new following parameter) and when the following function is not active (the command activates the
following value to be used in the next movement stage).

If the uppercase syntax is used, the movement is stopped and the continuous command underway,
if any, is terminated. If the lowercase syntax is used, instead, a continuous mode command is
given out; at any rate, the axes are stopped at zero speed and after that are restarted immediately.
If you do not want the movement to stop, this can be accomplished by having the machine logic
execute a similar command.

10 Series CNC Programming Manual (17) 2-41

Chapter 2

Programming the Axes

Activating the following function

The following of the Master axis by the slave(s) is immediately activated. The following modality is
defined by the “mode” parameter contained in the master/slave association command.

Syntax

(XDA, 3, slave1[slave2[..]])
(xda

, 3, slave1[slave2[..]])

where:

slave1…slave8 are the names of the slave axes (each of which is denoted by a single

ASCII character). You can program up to 8 slaves.

Characteristics:

If the uppercase syntax is used, the movement is stopped and the continuous command underway,
if any, is terminated. If the lowercase syntax is used, instead, a continuous mode command is
given out; at any rate, the axes are stopped at zero speed and are restarted immediately. If you do
not want the movement to stop, this can be accomplished by having the machine logic execute a
similar command.

2-42 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

Deactivating the following function

The following of the Master axis by the slave(s) is immediately deactivated. The release modality is
defined by the “mode” parameter contained in the master/slave association command.

Syntax

(XDA, 4, slave1[slave2[..]])
(xda

, 4, slave1[slave2[..]])

where:

slave1…slave8 are the names of the slave axes (each of which is denoted by a single

ASCII character). You can program up to 8 slaves.

Characteristics:

The slave axis remains associated with the master, it just does not follow it any longer. Depending
on the “
will occur:

If uppercase syntax is used, the movement is stopped and the continuous command underway, if
any, is terminated. If lowercase syntax is used, instead, a continuous mode command is given out;
at any rate, the axes are stopped at zero speed and are then restarted immediately. If you do not
want the movement to stop, this can be accomplished by having the machine logic execute a
similar command.

Example:

N10 (XDA,1,X/ZA,3,0.8,0.0) Activates master X and slaves Z and A
N20 (XDA,3,ZA) Activates following function by A and Z
N30 G1X100F2000
N40 X300
N50 (xda,4,Z) Deactivates following function by Z in continuous mode
N60 X400
N70 X500
N80 (xda,4,A) Deactivates following function by A in continuous mode
N90 X660
N100 X700
N110 (xda,3,ZA) Reactivates following function by A and Z in continuous mode
N120 GX0
N130 (XDA) Removes association of slaves Z and A with master X
N140 GX

mode” parameter defined in the master/slave association command, either of the following

0 The slave changes abruptly from the current feedrate to zero.

others The slave comes to a halt according to its deceleration ramp.

10 Series CNC Programming Manual (17) 2-43

Chapter 2

Programming the Axes

AXF – Definition of axes with dynamic following function

With this command it is possible to define the axes to be managed separately from the others from
the dynamic standpoint. The axes defined in the following triliteral describe the programmed
geometry, but move independently of the other process axes.

Syntax

(AXF, axle names)

(AXF)

where:

axle names Is a nominal list of the axes to which you want the following algorithm to be applied.

The triliteral without parameters disables the algorithm on all process axes.

Characteristics

The axes to which the dynamic following algorithm is applied are interpolated separately from the
others, since with this triliteral two different interpolators are created: one for normal axes and one
for the axes that follow.

The effect obtained is to prevent speed on the profile dropping to zero at the points where such
axes start or end their movement, thereby making the entire process smoother, as shown in the
example.

The axes that follow still have to be programmed.

This command is activated only if there is at least one axis to which the algorithm is not applied.

Each time the triliteral is programmed, any earlier following axis configuration is disabled.

Rotary axes move according to the dynamic parameters configured for them.
If the speed programmed for the profile exceeds maximum admissible

WARNING

speed, the axes cannot work properly (Servo Error).
In this case, reduce the set speed.

2-44 10 Series CNC Programming Manual (17)

Chapter 2

p

Programming the Axes

Example:

Given a process with 3 linear axes (XYZ) and 1 rotary axis (B), let us assume that the process is
programmed as described below:

(AXF,B) After this command, the B axis is enabled to follow

dynamically all the other axes of the process

G16XY
G1 X100 YZAB F5000
G3 X150 Y50 I100 J50 B90
G1 Y150

(AXF) After this command, rotary axis B is interpolated again

The chart shows the evolution of speed on the profile and the B axis, respectively, for the two
cases described above.

V

A rounded corner is programmed, which becomes part of the
movement of the rotary axis:

• without the AXF command, the linear axes, at the start

and end of the radius, come to a halt, as axis B is added
in the interpolation

• with the AXF command, the movement of B starts and

ends on the radius but does not limit the dynamics of the
linear axes: the speed on the profile does not drop to 0

together with the other process axes

on profile

on B axis

t

on

rofile

V

on B axis

t

radius

10 Series CNC Programming Manual (17) 2-45

Chapter 2

Programming the Axes

ORIGINS AND COORDINATE CONTROL CODES

The functions in this class perform the following operations:

G CODE FUNCTION

G04 Dwell at end of step

G09 Deceleration at end of step

G16 Define interpolation plane

G17 Circular interpolation and cutter diameter compensation on XY plane

G18 Circular interpolation and cutter diameter compensation on ZX plane

G19 Circular interpolation and cutter diameter compensation on YZ plane

G27 Continuous movement with automatic velocity reduction on bevel

G28 Continuous movement without automatic velocity reduction on bevel

G29 Point-to-point movements

G70 Programming in inches

G71 Programming in millimetres

G79 Programming referred to axes home switch

G90 Absolute programming

G91 Incremental programming

G92 Axis presetting

G93 Inverse time (V/D) feedrate programming mode

G94 Feedrate programming in ipm or mmpm

G95 Feedrate programming in ipr or mmpr

NOTE:

The planes specified in G17, G18, G19 are valid if they have been configured in the following
sequence: X, Y and Z.

2-46 10 Series CNC Programming Manual (17)

Programming the Axes

G17 G18 G19 - Selecting the Interpolation Plane

These G codes are used for defining the interpolation plane as described below:

G17 Active interpolation plane formed by axes 1 and 2 (XY).

G18 Active interpolation plane formed by axes 3 and 1 (ZX).

G19 Active interpolation plane formed by axes 2 and 3 (YZ).

Axes 1 (X), 2 (Y), and 3 (Z) are the first three axes declared in the AMP environment.

Syntax

G17

G18

Chapter 2

G19

The syntax for each function is simply the G code by itself in one block without parameters or other
pieces of information.

10 Series CNC Programming Manual (17) 2-47

Chapter 2

Programming the Axes

G16 - Defining the Interpolation Plane

Like G17, G18, and G19, G16 defines the abscissa and the ordinate of the interpolation plane but
is not linked to the first and second configured axes.

Syntax

G16

axis1 axis2

where:

axis1 Is the name of the abscissa of the interpolation plane (typically X). It must be one of

the configured axes in the system.

axis2 Is the name of the ordinate of the interpolation plane (typically Y). It must be one of

the configured axes in the system.

Characteristics:

G16, G17, G18, G19 cannot be used if the following G codes are active:

• Cutter diameter compensation (G41-G42)

• Standard canned cycles (G81-G89)

Example:

G16 X A specifies the interpolation plane formed by axes X and A .

2-48 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

G27 G28 G29 - Defining the Dynamic Mode

The G functions in this class define how the axis moves on the profile and positions at profile end.
These codes are always accepted by the control.

G27 Specifies a continuous move with automatic velocity reduction on bevels. At the

end of each element velocity is automatically calculated by the control and
optimised according to the profile shape. This calculation is based on DLA,
MDA and VEF values.

G28 Specifies a continuous move without automatic velocity reduction on bevels. At

the end of each element the velocity on the profile is equal to the programmed
feedrate.

G29 Specifies a point-to-point move that is independent from the programmed path

function (G01-G02-G03). At the end of each element the velocity on the profile
is 0.

Syntax

G27

[G-codes] [operands]

G28 [G-codes] [operands]

G29 [G-codes] [operands]

where:

G-codes Other G codes that are compatible with G27, G28 and G29 (See "Compatible G

codes" table in Chapter 1).

operands Any operand or code that can be used in a G function block.

10 Series CNC Programming Manual (17) 2-49

Chapter 2

Programming the Axes

Characteristics

:

The following diagram shows how G27, G28 and G29 operate when the programmed feedrate is
constant throughout the profile.

FEED

G27

G28

1

1

2

2

3

BLOCKS

3

BLOCKS

G29

1

2

BLOCKS

3

2-50 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

The following diagram shows how G27, G28 and G29 operate when the programmed feedrate
varies through the profile.

G27

12 3

G28

12 3

G29

12 3

In each block the move is divided into three steps:

1) Acceleration

2) Uniform move at programmed feedrate

BLOCKS

BLOCKS

BLOCKS

3) Decelerated motion

G27 and G28 differ only in the step with decelerated motion.
Positioning at the machining rate (G1, G2, G3) is available in continuous mode (G27, G28 and
G29) whereas rapid positioning (G0) is always point to point, i.e. with deceleration down to null
velocity and accurate positioning regardless of the system status.

With G27-G28 (continuous mode) the control explores and executes the profile as if it were a
single block. For this reason, auxiliary functions M, S and T are not allowed within the profile
executed in G27-G28.

Continuous mode can be temporarily closed by a G00 move that is still part of the profile. The
allowed M, S and T functions may therefore be programmed in a block following G00.

NOTE:

The G code that has been configured in AMP (typically G27) is automatically selected at power-up
or after a reset.

10 Series CNC Programming Manual (17) 2-51

Chapter 2

Programming the Axes

Example:

This is a contouring example in continuous and point-to-point mode.

Y

25.65

230

295

0

1

5

187

235

4

0

70.477

3

X

2

75

Program 1 (continuous mode):

(UGS,X,-400,100,Y,-400,100)
N9 (DIS,"MILL DIA. 16")
N10 T4.4 M6 S800
1 N11 G X-235 Y-230 M13
N12 Z-10
2 N13 G27 G1 X75 F500 ;Continuous mode starts (G27)
3 N14 Y .
4 N15 G3 X-70.477 Y25.651 I J
5 N16 G1 X-187 Y-295
N17 G Z5 M5 ;Temporary shift to point to point mode
N18 (DIS,"MILL DIA. 28") ;for spindle stop, tool change and S functions

N19 T5.5 M6 S1200
N20 X.. Y.. M13
N21 Z-..
N22 G1 X.. Y.. ;Continuous mode restarts

IMPORTANT

If G29 were programmed in block N17, continuous mode would stop and
subsequent moves in G1-G2-G3 would be performed in point-to-point mode.

2-52 10 Series CNC Programming Manual (17)

Program 2 (point-to-point mode):

(UGS,X,-400,100,Y,-400,100)
N9 (DIS, "MILL DIA. 16")

N10 T4.4 M6 S800
1 N11 G29 G X-235 Y-230 M13 ;Point-to-point operation starts
N12 Z-10
2 N13 G1 X75 F500 M5 ;Spindle stop
3 N14 Y S1200 M13 ;Spindle CW with coolant
4 N15 G3 X-70.477 Y25.651 I J
N16 DWT=2
5 N17 G1 G4 X-187 Y-295 ;Dwell at the end of the element
N18 G Z5 M5
N19 (DIS,"MILL DIA. 28")
N20 T5.5 M6 S1200
N21 G X.. Y.. M13
N22 Z-..
N23 G1 X.. Y..

Chapter 2

Programming the Axes

IMPORTANT

By programming point-to-point with G29 in block N11, M and S functions have
been included in the profile (blocks N13 and N14). The dwell at the end of the
element (block N17), however, can also be programmed in continuous mode.

10 Series CNC Programming Manual (17) 2-53

Chapter 2

Programming the Axes

AUTOMATIC DECELERATION ON BEVELS IN G27 MODE

When G27 mode is active, the control automatically calculates the vector velocity on the bevels
(i.e. between two subsequent moves) using a two-step algorithm.

During the first step the vector velocity is calculated with a formula based on profile variations. The
variation of the profile is associated to the angle formed by two subsequent moves.

The control compares the actual angle with the MDA value; if the angle is greater, the vector
velocity is put to zero as in G29 mode; otherwise, the control calculates for this bevel a velocity that
is based on the angle, MDA and VEF values.

The second step of the algorithm, called "
according to the value of the DLA variable.

The "

look ahead" step is an optimisation of the first step. In fact, in order to provide a correct stop

at the profile end, the calculated vector velocity is re-processed taking into account the total
distance to be covered in G27 mode and the acceleration configured for each axis.

IMPORTANT

The look ahead feature (G1 G27) does not handle feedrate override. In fact, at
this stage a 100% feedrate is assumed. Higher feedrates may generate SERVO
ERRORS.

look ahead", is optional. It can be enabled or disabled

2-54 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

DLA - Deceleration Look Ahead

The DLA code enables/disables look ahead calculation in G27 dynamic mode. The control reads
the motion blocks that make up the profile and those that follow the block in execution in order to
recalculate the exit feedrate for the various blocks. It also calculates the deceleration on the bevels
according to the profile. If the profile includes sudden trajectory variations and there are not
enough block lengths to ensure appropriate deceleration, it is critical for the system to anticipate
these events so that velocities can be adjusted. The number of motion blocks the system can look
ahead after the current block can be specified in the characterisation. It ranges from 2 to 64 blocks.

Syntax

DLA=value

where:

value can be: 0 disables look ahead

1 enables look ahead

NOTE:

If DLA=1 system block time increases because the control must execute a greater number of
calculations for each instruction. This results in greater accuracy.

It is advisable to set DLA=0 when it is clear that the programmed feedrate and the total distance to
be covered in continuous mode are such as to provide a good stop at the end of the profile.

With DLA=0 the control will consider only the deviations from the theoretical profile on bevels.

Characteristics:

The default value of this variable is configurable in AMP.

10 Series CNC Programming Manual (17) 2-55

Chapter 2

Programming the Axes

DYM - Dynamic Mode

The DYM defines the type of algorithm to use for calculating the velocity between one element and
the next with G27 active.

Syntax

DYM=value

where:

value It is a numeric value which can be:

0 to use the standard 10 Series formula
1 to use the standard 8600 Series formula
2 to use the 1° alternative 10 Series formula
3 to use the 2° alternative 10 Series formula

The standard Series 10 algorithm is based on precise mathematical formulas which assume a
linear response from the machine and that the dynamic parameters configured are always
applicable under any condition.

The algorithm already present in the 8600 series uses approximate formulas, therefore applying
greater restrictions on movement.

The alternative algorithms keep into consideration the dynamic components (acceleration) that the
axes can bear when passing from one block to the other. In this way it recalculates the final speed
at of the first block in order to pass to the next one without excessive stress on the machine.

It is recommended that you verify the behaviour of both algorithms on the machine and then decide
which default algorithm best suits that particular machinery and that particular type of work.

Characteristics

The default value of this variable can be set in AMP.

2-56 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

MDA - Maximum Deceleration Angle

The MDA code defines the maximum angular axis departure in which G27 is active. The selected
value (from 0 to 180 degrees) defines an angle that is the limit of G27 operation.

Syntax

MDA=value

where:

value is a numeric value with the following characteristics:

• angle between 0° and 180° if DYM = 0

• number between 0 and 2 if DYM = 1

In both cases, it represents the maximum deviation between two consecutive
elements beyond which, in G27, the stop is forced on the final point.

If DYM = 1, the value is to be calculated as:

Characteristics:

sine of the maximum angle for deviations

1 +

[sine (angle - 90°)] for deviations > 90° and ≤ 180°.

• Not significative if DYM = 2 or DYM=3

≤ 90°

In order to alter the default value (MDA = 90 degrees) you may assign MDA in the configuration or
enter it through a specific data entry or a part program block.

The system forces the axis to decelerate to zero velocity when the direction is greater

IMPORTANT

than the angle defined by the MDA value. The system calculates a deceleration ramp
for the programmed axis if the direction is less than or equal to the angle defined by
the MDA value.

Since the system calculates deceleration on bevels from the actual angle and the
MDA and VEF values, it is possible to alter velocity reduction by changing the MDA
value. Small values of MDA generate dramatic deceleration on bevels.

The system RESET restores the configured MDA value.

Examples:

DYM=0
MDA=90°
MDA=180°

DYM=1
MDA=1
MDA=2

10 Series CNC Programming Manual (17) 2-57

Chapter 2

α

Programming the Axes

VEF - Velocity Factor

The VEF code defines a velocity determining factor on bevels in the G27 mode. The velocity
calculated from the MDA value can be increased or decreased by changing the VEF value. Small
VEF values dramatically reduce velocity on bevels.

Syntax

VEF=value

where:

value is a number with the following characteristics:

• number from 0.1 to 8 if DYM = 0 The default value is 0.8.

• number from 0 to 99999 if DYM = 1 The default value is 0.8.

• number from -1 to 99999 if DYM = 2 The default value is 0.8

• number from 0 to 99999 if DYM = 3 The default value is 0.8

Characteristics:

The characteristics of the velocity calculation vary according to the value of the DYM variable.

DYM = 0

The following diagram shows different decelerations calculated by the system by varying the VEF
value and keeping the MDA value constant.

V

V

prog

VEF > 1

VEF = 1

VEF < 1

MDA

angle

2-58 10 Series CNC Programming Manual (17)

Chapter 2

Programming the Axes

where:

V is the velocity on the bevel

α is the angle between two subsequent movements

Vprog is the programmed feedrate

DYM = 1

The VEF code defines the maximum form error admissable on the bevel. If the value is 0, at the
end of each block the system deccelerates the axes to zero.

DYM = 2

The VEF value defines the maximum speed “step” for the axis in the passage from one block to the
next: for example if VEF=0.8 the axis will have a speed “step” of 1+0.8 of the acceleration of set
working acceleration; if VEF=-0,3 the axis will have a speed “step” of +1-0.3 or +0,7.
The system will calculate the speed on the edges according to all the axes that are part of the
movement; each axis will have a different speed and the system will choose the minimum among
these.

DYM = 3

VEF is a value that defines the time, in ms, it takes to reach the speed to be applied to the corner
as a function of the accelerations configured on the various axes. The formula to be applied is:

Vcorner = Acceleration * VEF

Hence, having determined Vcorner, the VEF to be programmed will be:

Vcorner

VEF=

Acceleration

The system will calculate the speed on the edges according to all the axes that are part of the
movement; each axis will have a different speed and the system will choose the minimum among
these.

IMPORTANT

A system RESET restores the VEF value configured in AMP

10 Series CNC Programming Manual (17) 2-59

Chapter 2

Programming the Axes

Jerk Limitation

The speed diagrams shown in the previous sections show the continuity of the speed function V(t),
while the acceleration function
machine and the type of machining process, this may cause defects in the finish of the part.

a(t) has a step pattern. Depending on the characteristics of the

This problem may be solved using an acceleration function

The purpose of the "Jerk Limitation" function is to limit variations in acceleration, so as to control its
maximum value, resulting in smoother movement and, consequently, a better surface finish.

V(t)

a(t) with a continuous pattern.

t

2-60 10 Series CNC Programming Manual (17)

Programming the Axes

MOV - Enable Jerk Limitation

The MOV code is used to define some characteristic of the movements management.

Syntax:

MOV = value

where:

value movements behaviour to be enabled.

The value to be specified is obtained from the sum of the decimal weights
corresponding to each of the features desired.

0 1 2 3 4 5 6 7

Chapter 2

Movements change optimization
during profiling with G27/G28

Enable non linear-ramp

Enable ramps with Jerk Limitation

Speed management of rotating axes
with UPR 2 or 6

Enabling of Trapezoidal Ramps

Recalculation of machining speed
The programmed feed rate only refers
to linear axes.

Enabling of VFF for manual
movements.

The default value of this variable is 0. The MOV value can be configured in AMP. The RESET
restores the default value.

Example:

if you want to use Jerk Limitation with non-linear ramps and at the same time have VFF enabled
for normal movements, the MOV variable must be set to the value 128+8=136

10 Series CNC Programming Manual (17) 2-61

Chapter 2

A

p

Programming the Axes

Meaning of bits 1, 3 and 5:

(value 2): Enables the non linear ramps (S ramps) where the execution mode is

Bit 1

characterised by the value of the JRK variable. The system modulates
continuously the acceleration value between 0 and a maximum whose
value is given by A/JRK, so that, with JRK=1 the nominal acceleration
value is reached, with JRK=2 half the nominal acceleration value is
reached, with JRK=0.5 twice the nominal acceleration value is reached.
The ensuing jerk values on the movement will NOT be controlled and will
range from 0 to an undetermined value.

Jerk

ccel

T

ram

In the example above, a movement at a speed of 20000 mm/min with an
acceleration of 1500 mm/sec

2

has been programmed. The maximum

Speed

acceleration value is reached only at a time halfway between the
acceleration stage or the deceleration stage. For JRK=1 the acceleration
value reached corresponds to the value requested.

The execution time of the acceleration stage corresponds to the time it
would have taken using a linear acceleration ramp, multiplied by the value
of JRK and constant 1.485.

T

ramp

= T

linear ramp

* JRK * 1.485.

2-62 10 Series CNC Programming Manual (17)

Chapter 2

A

Programming the Axes

Ramp time is also affected by the “minimum ramp time” parameter configured in AMP for each
axis. If the time calculated for the ramp does not meet the minimum ramp time limit, the ramp will
be recalculated to comply with this requirement.

N.B. The minimum ramp time is time it takes to reach the maximum acceleration value (Jerk

application time) so that, as can be seen from the chart below, the total ramp time corresponds to
twice the minimum time.

Speed

ccel

Jerk application

time

Jerk

10 Series CNC Programming Manual (17) 2-63

Chapter 2

A

Programming the Axes

(value 8): Enables the non linear ramps (ramps with jerk limitation). Acceleration

Bit 3

ramps are calculated on the basis of the jerk parameters configured in
AMP. The jerk value used within a movement is calculated by the system
so as to ensure that the movement complies with the jerk characteristics
specified for each axis. The jerk value configured for each axis must be
construed as the maximum value that can be reached during the
acceleration stage. The system modulates the jerk value continuously
between 0 and its maximum value, and it will modulate in the same
manner the acceleration value, which will not necessarily reach the
maximum value configured.

Speed

Jerk

ccel

In the example above, a movement at a speed of 20000 mm/min with an
acceleration of 1500 mm/sec

2

and with jerk of 15000 mm/sec3 has been
programmed. The maximum acceleration value is reached only at a time
halfway between the acceleration stage or the deceleration stage and it is
below the maximum value that is requested. Only with a higher jerk it will
be possible to reach the maximum acceleration.

Ramp time is affected by the jerk parameter and by the “minimum ramp
time” parameter configured in AMP for each axis. If the time calculated for
the ramp does not meet the minimum ramp time limit, the ramp will be
recalculated to comply with this requirement.

N.B. The minimum ramp time is time it takes to reach the maximum

acceleration value (Jerk application time) so that, as can be seen from the
chart below, the total ramp time corresponds to twice the minimum time.

2-64 10 Series CNC Programming Manual (17)

A

Jerk application

time

Chapter 2

Programming the Axes

Speed

ccel

Jerk

10 Series CNC Programming Manual (17) 2-65

Chapter 2

A

Programming the Axes

Bit 5 (value 32) :

Enables the non linear ramps (trapezoidal ramps). Acceleration ramps are
calculated on the basis of the jerk parameters configured in AMP. The jerk
value used within a movement is calculated by the system so as to ensure
that the movement complies with the jerk characteristics specified for each
axis. The jerk value configured for each axis must be construed as the
value that can be used during the acceleration stage. The system keeps
the jerk value continuously during the acceleration stage.

Speed

Jerk

ccel

In the example above, a movement at a speed of 20000 mm/min with an
acceleration of 1500 mm/sec

2

and with jerk of 15000 mm/sec3 has been
programmed. The maximum acceleration value is reached and maintained
for a certain time in the central part of the acceleration or deceleration
stage; it may or may not reach the maximum value requested as a function
of speed leap to be made.

Ramp time is affected by the jerk parameter and also by the “minimum
ramp time” parameter configured in AMP for each axis. If the time
calculated for the ramp does not meet the minimum ramp time limit, the
ramp will be recalculated to comply with this requirement.

N.B. The minimum ramp time is time it takes to reach the maximum

acceleration value (Jerk application time).

2-66 10 Series CNC Programming Manual (17)