fanuc 30iA, 300iA, 300is A, 31iA5, 310iA5 User Manual

GE Fanuc Automation

Computer Numerical Control Products

Series 30i/300i/300is-MODEL A
Series 31i/310i/310is-MODEL A5
Series 31i/310i/310is-MODEL A
Series 32i/320i/320is-MODEL A

For Lathe System

User’s Manual

GFZ-63944EN-1/02 June 2004

Warnings, Cautions, and Notes
as Used in this Publication

Warning notices are used in this publication to emphasize that hazardous voltages, currents,
temperatures, or other conditions that could cause personal injury exist in this equipment or
may be associated with its use.

In situations where inattention could cause either personal injury or damage to equipment, a
Warning notice is used.

Caution notices are used where equipment might be damaged if care is not taken.

GFL-001

Warning

Caution

Note

Notes merely call attention to information that is especially significant to understanding and
operating the equipment.

This document is based on information available at the time of its publication. While efforts
have been made to be accurate, the information contained herein does not purport to cover all
details or variations in hardware or software, nor to provide for every possible contingency in
connection with installation, operation, or maintenance. Features may be described herein
which are not present in all hardware and software systems. GE Fanuc Automation assumes
no obligation of notice to holders of this document with respect to changes subsequently made.

GE Fanuc Automation makes no representation or warranty, expressed, implied, or statutory
with respect to, and assumes no responsibility for the accuracy, completeness, sufficiency, or
usefulness of the information contained herein. No warranties of merchantability or fitness for
purpose shall apply.

©Copyright 2004 GE Fanuc Automation North America, Inc.

All Rights Reserved.

B-63944EN-1/02 SAFETY PRECAUTIONS

SAFETY PRECAUTIONS

This section describes the safety precautions related to the use of CNC
units.
It is essential that these precautions be observed by users to ensure the
safe operation of machines equipped with a CNC unit (all descriptions
in this section assume this configuration). Note that some precautions
are related only to specific functions, and thus may not be applicable
to certain CNC units.
Users must also observe the safety precautions related to the machine,
as described in the relevant manual supplied by the machine tool
builder. Before attempting to operate the machine or create a program
to control the operation of the machine, the operator must become
fully familiar with the contents of this manual and relevant manual
supplied by the machine tool builder.

CONTENTS

1.1 DEFINITION OF WARNING, CAUTION, AND NOTE ........s-2

1.2 GENERAL WARNINGS AND CAUTIONS ...........................s-3

1.3 WARNINGS AND CAUTIONS RELATED TO

PROGRAMMING.....................................................................s-6

1.4 WARNINGS AND CAUTIONS RELATED TO HANDLINGs-9

1.5 WARNINGS RELATED TO DAILY MAINTENANCE....... s-12

s-1

SAFETY PRECAUTIONS B-63944EN-2/02

1.1 DEFINITION OF WARNING, CAUTION, AND NOTE

This manual includes safety precautions for protecting the user and
preventing damage to the machine. Precautions are classified into
Warning and Caution according to their bearing on safety. Also,
supplementary information is described as a Note. Read the
Warning, Caution, and Note thoroughly before attempting to use
the machine.

WARNING

Applied when there is a danger of the user being

injured or when there is a danger of both the user
being injured and the equipment being damaged if
the approved procedure is not observed.

CAUTION

Applied when there is a danger of the equipment

being damaged, if the approved procedure is not
observed.

NOTE

The Note is used to indicate supplementary

information other than Warning and Caution.

• Read this manual carefully, and store it in a safe place.

s-2

B-63944EN-2/02 SAFETY PRECAUTIONS

1.2 GENERAL WARNINGS AND CAUTIONS

WARNING

1 Never attempt to machine a workpiece without first

checking the operation of the machine. Before
starting a production run, ensure that the machine
is operating correctly by performing a trial run
using, for example, the single block, feedrate
override, or machine lock function or by operating
the machine with neither a tool nor workpiece
mounted. Failure to confirm the correct operation
of the machine may result in the machine behaving
unexpectedly, possibly causing damage to the
workpiece and/or machine itself, or injury to the
user.

2 Before operating the machine, thoroughly check

the entered data.

Operating the machine with incorrectly specified

data may result in the machine behaving
unexpectedly, possibly causing damage to the
workpiece and/or machine itself, or injury to the
user.

3 Ensure that the specified feedrate is appropriate

for the intended operation. Generally, for each
machine, there is a maximum allowable feedrate.

The appropriate feedrate varies with the intended

operation. Refer to the manual provided with the
machine to determine the maximum allowable
feedrate.

If a machine is run at other than the correct speed,

it may behave unexpectedly, possibly causing
damage to the workpiece and/or machine itself, or
injury to the user.

4 When using a tool compensation function,

thoroughly check the direction and amount of
compensation.
Operating the machine with incorrectly specified
data may result in the machine behaving
unexpectedly, possibly causing damage to the
workpiece and/or machine itself, or injury to the
user.

s-3

SAFETY PRECAUTIONS B-63944EN-2/02

WARNING

5 The parameters for the CNC and PMC are

factory-set. Usually, there is not need to change
them. When, however, there is not alternative other
than to change a parameter, ensure that you fully
understand the function of the parameter before
making any change.

Failure to set a parameter correctly may result in

the machine behaving unexpectedly, possibly
causing damage to the workpiece and/or machine
itself, or injury to the user.

6 Immediately after switching on the power, do not

touch any of the keys on the MDI panel until the
position display or alarm screen appears on the
CNC unit.

Some of the keys on the MDI panel are dedicated

to maintenance or other special operations.
Pressing any of these keys may place the CNC
unit in other than its normal state. Starting the
machine in this state may cause it to behave
unexpectedly.

7 The User’s Manual and programming manual

supplied with a CNC unit provide an overall
description of the machine's functions, including
any optional functions. Note that the optional
functions will vary from one machine model to
another. Therefore, some functions described in
the manuals may not actually be available for a
particular model. Check the specification of the
machine if in doubt.

8 Some functions may have been implemented at

the request of the machine-tool builder. When
using such functions, refer to the manual supplied
by the machine-tool builder for details of their use
and any related cautions.

CAUTION

The liquid-crystal display is manufactured with very

precise fabrication technology. Some pixels may
not be turned on or may remain on. This
phenomenon is a common attribute of LCDs and is
not a defect.

s-4

B-63944EN-2/02 SAFETY PRECAUTIONS

NOTE

Programs, parameters, and macro variables are

stored in nonvolatile memory in the CNC unit.
Usually, they are retained even if the power is
turned off.

Such data may be deleted inadvertently, however,

or it may prove necessary to delete all data from
nonvolatile memory as part of error recovery.

To guard against the occurrence of the above, and

assure quick restoration of deleted data, backup all
vital data, and keep the backup copy in a safe
place.

s-5

SAFETY PRECAUTIONS B-63944EN-2/02

1.3 WARNINGS AND CAUTIONS RELATED TO

PROGRAMMING

This section covers the major safety precautions related to
programming. Before attempting to perform programming, read the
supplied User’s Manual carefully such that you are fully familiar with
their contents.

WARNING

1 Coordinate system setting
If a coordinate system is established incorrectly,

the machine may behave unexpectedly as a result
of the program issuing an otherwise valid move
command. Such an unexpected operation may
damage the tool, the machine itself, the workpiece,

or cause injury to the user.
2 Positioning by nonlinear interpolation
When performing positioning by nonlinear

interpolation (positioning by nonlinear movement

between the start and end points), the tool path

must be carefully confirmed before performing

programming. Positioning involves rapid traverse. If

the tool collides with the workpiece, it may damage

the tool, the machine itself, the workpiece, or

cause injury to the user.
3 Function involving a rotation axis
When programming polar coordinate interpolation

or normal-direction (perpendicular) control, pay

careful attention to the speed of the rotation axis.

Incorrect programming may result in the rotation

axis speed becoming excessively high, such that

centrifugal force causes the chuck to lose its grip

on the workpiece if the latter is not mounted

securely. Such mishap is likely to damage the tool,

the machine itself, the workpiece, or cause injury to

the user.
4 Inch/metric conversion
Switching between inch and metric inputs does not

convert the measurement units of data such as the

workpiece origin offset, parameter, and current

position. Before starting the machine, therefore,

determine which measurement units are being

used. Attempting to perform an operation with

invalid data specified may damage the tool, the

machine itself, the workpiece, or cause injury to the

user.

s-6

B-63944EN-2/02 SAFETY PRECAUTIONS

WARNING

5 Constant surface speed control
When an axis subject to constant surface speed

control approaches the origin of the workpiece

coordinate system, the spindle speed may become

excessively high. Therefore, it is necessary to

specify a maximum allowable speed. Specifying

the maximum allowable speed incorrectly may

damage the tool, the machine itself, the workpiece,

or cause injury to the user.
6 Stroke check
After switching on the power, perform a manual

reference position return as required. Stroke check

is not possible before manual reference position

return is performed. Note that when stroke check is

disabled, an alarm is not issued even if a stroke

limit is exceeded, possibly damaging the tool, the

machine itself, the workpiece, or causing injury to

the user.
7 Tool post interference check
A tool post interference check is performed based

on the tool data specified during automatic

operation. If the tool specification does not match

the tool actually being used, the interference check

cannot be made correctly, possibly damaging the

tool or the machine itself, or causing injury to the

user. After switching on the power, or after

selecting a tool post manually, always start

automatic operation and specify the tool number of

the tool to be used.
8 Absolute/incremental mode
If a program created with absolute values is run in

incremental mode, or vice versa, the machine may

behave unexpectedly.
9 Plane selection
If an incorrect plane is specified for circular

interpolation, helical interpolation, or a canned

cycle, the machine may behave unexpectedly.

Refer to the descriptions of the respective

functions for details.
10 Torque limit skip
Before attempting a torque limit skip, apply the

torque limit. If a torque limit skip is specified

without the torque limit actually being applied, a

move command will be executed without

performing a skip.

s-7

SAFETY PRECAUTIONS B-63944EN-2/02

WARNING

11 Programmable mirror image
Note that programmed operations vary

considerably when a programmable mirror image is

enabled.
12 Compensation function
If a command based on the machine coordinate

system or a reference position return command is

issued in compensation function mode,

compensation is temporarily canceled, resulting in

the unexpected behavior of the machine.
Before issuing any of the above commands,

therefore, always cancel compensation function

mode.

s-8

B-63944EN-2/02 SAFETY PRECAUTIONS

1.4 WARNINGS AND CAUTIONS RELATED TO

HANDLING

This section presents safety precautions related to the handling of
machine tools. Before attempting to operate your machine, read the
supplied User’s Manual carefully, such that you are fully familiar with
their contents.

WARNING

1 Manual operation
When operating the machine manually, determine

the current position of the tool and workpiece, and

ensure that the movement axis, direction, and

feedrate have been specified correctly. Incorrect

operation of the machine may damage the tool, the

machine itself, the workpiece, or cause injury to the

operator.
2 Manual reference position return
After switching on the power, perform manual

reference position return as required.

If the machine is operated without first performing

manual reference position return, it may behave

unexpectedly. Stroke check is not possible before

manual reference position return is performed.

An unexpected operation of the machine may

damage the tool, the machine itself, the workpiece,

or cause injury to the user.
3 Manual numeric command
When issuing a manual numeric command,

determine the current position of the tool and

workpiece, and ensure that the movement axis,

direction, and command have been specified

correctly, and that the entered values are valid.
Attempting to operate the machine with an invalid

command specified may damage the tool, the

machine itself, the workpiece, or cause injury to the

operator.
4 Manual handle feed
In manual handle feed, rotating the handle with a

large scale factor, such as 100, applied causes the

tool and table to move rapidly. Careless handling

may damage the tool and/or machine, or cause

injury to the user.

s-9

SAFETY PRECAUTIONS B-63944EN-2/02

WARNING

5 Disabled override
If override is disabled (according to the

specification in a macro variable) during threading,

rigid tapping, or other tapping, the speed cannot be

predicted, possibly damaging the tool, the machine

itself, the workpiece, or causing injury to the

operator.
6 Origin/preset operation
Basically, never attempt an origin/preset operation

when the machine is operating under the control of

a program. Otherwise, the machine may behave

unexpectedly, possibly damaging the tool, the

machine itself, the tool, or causing injury to the

user.
7 Workpiece coordinate system shift
Manual intervention, machine lock, or mirror

imaging may shift the workpiece coordinate

system. Before attempting to operate the machine

under the control of a program, confirm the

coordinate system carefully.

If the machine is operated under the control of a

program without making allowances for any shift in

the workpiece coordinate system, the machine

may behave unexpectedly, possibly damaging the

tool, the machine itself, the workpiece, or causing

injury to the operator.
8 Software operator's panel and menu switches
Using the software operator's panel and menu

switches, in combination with the MDI panel, it is

possible to specify operations not supported by the

machine operator's panel, such as mode change,

override value change, and jog feed commands.
Note, however, that if the MDI panel keys are

operated inadvertently, the machine may behave

unexpectedly, possibly damaging the tool, the

machine itself, the workpiece, or causing injury to

the user.
9 RESET key
Pressing the RESET key stops the currently

running program. As a result, the servo axes are

stopped. However, the RESET key may fail to

function for reasons such as an MDI panel

problem. So, when the motors must be stopped,

use the emergency stop button instead of the

RESET key to ensure security.

s-10

B-63944EN-2/02 SAFETY PRECAUTIONS

WARNING

10 Manual intervention
If manual intervention is performed during

programmed operation of the machine, the tool

path may vary when the machine is restarted.

Before restarting the machine after manual

intervention, therefore, confirm the settings of the

manual absolute switches, parameters, and

absolute/incremental command mode.
11 Feed hold, override, and single block
The feed hold, feedrate override, and single block

functions can be disabled using custom macro

system variable #3004. Be careful when operating

the machine in this case.
12 Dry run
Usually, a dry run is used to confirm the operation

of the machine. During a dry run, the machine

operates at dry run speed, which differs from the

corresponding programmed feedrate. Note that the

dry run speed may sometimes be higher than the

programmed feed rate.
13 Cutter and tool nose radius compensation in

MDI mode
Pay careful attention to a tool path specified by a

command in MDI mode, because cutter or tool

nose radius compensation is not applied. When a

command is entered from the MDI to interrupt in

automatic operation in cutter or tool nose radius

compensation mode, pay particular attention to the

tool path when automatic operation is subsequently

resumed. Refer to the descriptions of the

corresponding functions for details.
14 Program editing
If the machine is stopped, after which the

machining program is edited (modification,

insertion, or deletion), the machine may behave

unexpectedly if machining is resumed under the

control of that program. Basically, do not modify,

insert, or delete commands from a machining

program while it is in use.

s-11

SAFETY PRECAUTIONS B-63944EN-2/02

1.5 WARNINGS RELATED TO DAILY MAINTENANCE

WARNING

1 Memory backup battery replacement
When replacing the memory backup batteries,

keep the power to the machine (CNC) turned on,

and apply an emergency stop to the machine.

Because this work is performed with the power on

and the cabinet open, only those personnel who

have received approved safety and maintenance

training may perform this work.
When replacing the batteries, be careful not to

touch the high-voltage circuits (marked

fitted with an insulating cover).
Touching the uncovered high-voltage circuits

presents an extremely dangerous electric shock

hazard.

NOTE

The CNC uses batteries to preserve the contents

of its memory, because it must retain data such as

programs, offsets, and parameters even while

external power is not applied.
If the battery voltage drops, a low battery voltage

alarm is displayed on the machine operator's panel

or screen.

When a low battery voltage alarm is displayed,

replace the batteries within a week. Otherwise, the

contents of the CNC's memory will be lost.
Refer to the Section “Method of replacing battery”

in the User’s Manual (Common to T/M series) for

details of the battery replacement procedure.

and

s-12

B-63944EN-2/02 SAFETY PRECAUTIONS

WARNING

2 Absolute pulse coder battery replacement
When replacing the memory backup batteries,

keep the power to the machine (CNC) turned on,

and apply an emergency stop to the machine.

Because this work is performed with the power on

and the cabinet open, only those personnel who

have received approved safety and maintenance

training may perform this work.
When replacing the batteries, be careful not to

touch the high-voltage circuits (marked

and

fitted with an insulating cover).
Touching the uncovered high-voltage circuits

presents an extremely dangerous electric shock

hazard.

NOTE

The absolute pulse coder uses batteries to

preserve its absolute position.
If the battery voltage drops, a low battery voltage

alarm is displayed on the machine operator's panel

or screen.
When a low battery voltage alarm is displayed,

replace the batteries within a week. Otherwise, the

absolute position data held by the pulse coder will

be lost.
Refer to the FANUC SERVO MOTOR αi series

Maintenance Manual for details of the battery

replacement procedure.

s-13

SAFETY PRECAUTIONS B-63944EN-2/02

WARNING

3 Fuse replacement

Before replacing a blown fuse, however, it is

necessary to locate and remove the cause of the

blown fuse.

For this reason, only those personnel who have

received approved safety and maintenance training

may perform this work.
When replacing a fuse with the cabinet open, be

careful not to touch the high-voltage circuits

(marked and fitted with an insulating cover).
Touching an uncovered high-voltage circuit

presents an extremely dangerous electric shock

hazard.

s-14

B-63944EN-1/02 TABLE OF CONTENTS

TABLE OF CONTENTS

SAFETY PRECAUTIONS............................................................................s-1

I. GENERAL

1 GENERAL ...............................................................................................3

1.1 NOTES ON READING THIS MANUAL.......................................................... 7

1.2 NOTES ON VARIOUS KINDS OF DATA ...................................................... 7

II. PROGRAMMING

1 GENERAL .............................................................................................11

1.1 OFFSET ......................................................................................................12

2 PREPARATORY FUNCTION (G FUNCTION) ...................................... 13

3 INTERPOLATION FUNCTION ..............................................................19

3.1 CONSTANT LEAD THREADING (G32) ...................................................... 20

3.2 CONTINUOUS THREADING....................................................................... 24

3.3 MULTIPLE THREADING ............................................................................. 25

3.4 TORQUE LIMIT SKIP (G31 P99)................................................................. 27

4 FUNCTIONS TO SIMPLIFY PROGRAMMING .....................................29

4.1 CANNED CYCLE (G90, G92, G94) ............................................................. 30

4.1.1 Outer Diameter/Internal Diameter Cutting Cycle (G90) ........................................31

4.1.1.1 Straight cutting cycle ......................................................................................... 31

4.1.1.2 Taper cutting cycle ............................................................................................ 33

4.1.2 Threading Cycle (G92)...........................................................................................35

4.1.2.1 Straight threading cycle ..................................................................................... 35

4.1.2.2 Taper threading cycle ........................................................................................ 39

4.1.3 End Face Turning Cycle (G94) ..............................................................................42

4.1.3.1 Face cutting cycle .............................................................................................. 42

4.1.3.2 Taper cutting cycle ............................................................................................ 43

4.1.4 How to Use Canned Cycles (G90, G92, G94)........................................................45

4.1.5 Canned Cycle and Tool Nose Radius Compensation.............................................47

4.1.6 Restrictions on Canned Cycles...............................................................................49

4.2 MULTIPLE REPETITIVE CYCLE (G70-G76) ..............................................51

4.2.1 Stock Removal in Turning (G71) ...........................................................................52

4.2.2 Stock Removal in Facing (G72) .............................................................................65

4.2.3 Pattern Repeating (G73) .........................................................................................70

c-1

TABLE OF CONTENTS B-63944EN-1/02

4.2.4 Finishing Cycle (G70)............................................................................................73

4.2.5 End Face Peck Drilling Cycle (G74)......................................................................77

4.2.6 Outer Diameter / Internal Diameter Drilling Cycle (G75) .....................................79

4.2.7 Multiple Threading Cycle (G76)............................................................................81

4.2.8 Restrictions on Multiple Repetitive Cycle (G70-G76)...........................................88

4.3 CANNED CYCLE FOR DRILLING............................................................... 90

4.3.1 Front Drilling Cycle (G83)/Side Drilling Cycle (G87) ..........................................94

4.3.2 Front Tapping Cycle (G84) / Side Tapping Cycle (G88).......................................97

4.3.3 Front Boring Cycle (G85) / Side Boring Cycle (G89) ...........................................99

4.3.4 Canned Cycle for Drilling Cancel (G80)..............................................................100

4.3.5 Precautions to Be Taken by Operator...................................................................101

4.4 RIGID TAPPING ........................................................................................ 102

4.4.1 FRONT FACE RIGID TAPPING CYCLE (G84) /

SIDE FACE RIGID TAPPING CYCLE (G88) ...................................................103

4.4.2 Peck Rigid Tapping Cycle (G84 or G88).............................................................109

4.4.3 Canned Cycle Cancel (G80).................................................................................114

4.4.4 Override during Rigid Tapping ............................................................................115

4.4.4.1 Extraction override .......................................................................................... 115

4.4.4.2 Override signal ................................................................................................ 117

4.5 CHAMFERING AND CORNER R .............................................................. 118

4.6 MIRROR IMAGE FOR DOUBLE TURRET (G68, G69) ............................. 126

4.7 DIRECT DRAWING DIMENSION PROGRAMMING ................................. 128

5 COMPENSATION FUNCTION ............................................................134

5.1 TOOL OFFSET..........................................................................................135

5.1.1 Tool Geometry Offset and Tool Wear Offset.......................................................136

5.1.2 T Code for Tool Offset .........................................................................................137

5.1.3 Tool Selection ......................................................................................................137

5.1.4 Offset Number......................................................................................................137

5.1.5 Offset ....................................................................................................................138

5.1.6 Y Axis Offset........................................................................................................142

5.1.7 Second Geometry Tool Offset..............................................................................143

5.2 OVERVIEW OF TOOL NOSE RADIUS COMPENSATION (G40-G42) ..... 146

5.2.1 Imaginary Tool Nose ............................................................................................147

5.2.2 Direction of Imaginary Tool Nose .......................................................................149

5.2.3 Offset Number and Offset Value..........................................................................151

5.2.4 Workpiece Position and Move Command............................................................154

5.2.5 Notes on Tool Nose Radius Compensation ..........................................................161

c-2

B-63944EN-1/02 TABLE OF CONTENTS

5.3 OVERVIEW OF CUTTER COMPENSATION (G40-G42).......................... 164

5.4 DETAILS OF CUTTER OR TOOL NOSE RADIUS COMPENSATION...... 171

5.4.1 Overview ..............................................................................................................171

5.4.2 Tool Movement in Start-up ..................................................................................175

5.4.3 Tool Movement in Offset Mode...........................................................................181

5.4.4 Tool Movement in Offset Mode Cancel...............................................................202

5.4.5 Prevention of Overcutting Due to Cutter or Tool Nose Radius Compensation ...209

5.4.6 Interference Check ...............................................................................................213

5.4.6.1 Operation to be performed if an interference is judged to occur ..................... 217

5.4.6.2 Interference check alarm function ...................................................................217

5.4.6.3 Interference check avoidance function ............................................................ 219

5.4.7 Cutter or Tool Nose Radius Compensation for Input from MDI .........................225

5.5 VECTOR RETENTION (G38) .................................................................... 227

5.6 CORNER CIRCULAR INTERPOLATION (G39) ........................................ 228

5.7 EXTENDED TOOL SELECTION ............................................................... 231

5.8 AUTOMATIC TOOL OFFSET (G36, G37)................................................. 235

5.9 COORDINATE SYSTEM ROTATION (G68.1, G69.1)............................... 239

5.10 ACTIVE OFFSET VALUE CHANGE FUNCTION BASED ON MANUAL

FEED .........................................................................................................243

6 MEMORY OPERATION BY SERIES 15 FORMAT............................. 247

6.1 ADDRESSES AND SPECIFIABLE VALUE RANGE FOR SERIES 15

PROGRAM FORMAT ................................................................................ 248

6.2 SUBPROGRAM CALLING ........................................................................ 249

6.3 CANNED CYCLE....................................................................................... 250

6.3.1 Outer Diameter/Internal Diameter Cutting Cycle (G90) ......................................251

6.3.1.1 Straight cutting cycle ....................................................................................... 251

6.3.1.2 Taper cutting cycle .......................................................................................... 253

6.3.2 Threading Cycle (G92).........................................................................................255

6.3.2.1 Straight threading cycle ................................................................................... 255

6.3.2.2 Taper threading cycle ...................................................................................... 259

6.3.3 End Face Turning Cycle (G94) ............................................................................262

6.3.3.1 Face cutting cycle ............................................................................................ 262

6.3.3.2 Taper cutting cycle .......................................................................................... 264

6.3.4 How to Use Canned Cycles..................................................................................266

6.3.5 Canned Cycle and Tool Nose Radius Compensation...........................................268

6.3.6 Restrictions on Canned Cycles.............................................................................270

6.4 MULTIPLE REPETITIVE CYCLE ..............................................................272

6.4.1 Stock Removal in Turning (G71) .........................................................................273

c-3

TABLE OF CONTENTS B-63944EN-1/02

6.4.2 Stock Removal in Facing (G72) ...........................................................................288

6.4.3 Pattern Repeating (G73) .......................................................................................294

6.4.4 Finishing Cycle (G70)..........................................................................................297

6.4.5 End Face Peck Drilling Cycle (G74)....................................................................301

6.4.6 Outer Diameter / Internal Diameter Drilling Cycle (G75) ...................................303

6.4.7 Multiple Threading Cycle (G76 <G code system A/B>)

(G78 <G code system C>)....................................................................................305

6.4.8 Restrictions on Multiple Repetitive Cycle ...........................................................313

6.5 CANNED CYCLE FOR DRILLING............................................................. 315

6.5.1 High-speed Peck Drilling Cycle (G83.1) .............................................................321

6.5.2 Drilling Cycle, Spot Drilling Cycle (G81) ...........................................................323

6.5.3 Drilling Cycle, Counter Boring (G82) .................................................................325

6.5.4 Peck Drilling Cycle (G83)....................................................................................327

6.5.5 Tapping Cycle (G84)............................................................................................329

6.5.6 Boring Cycle (G85)..............................................................................................331

6.5.7 Boring Cycle (G85)..............................................................................................333

6.5.8 Canned Cycle for Drilling Cancel (G80)..............................................................335

6.5.9 Precautions to be Taken by Operator ...................................................................335

7 MUITI-PATH CONTROL FUNCTION.................................................. 336

7.1 BALANCE CUT (G68, G69)....................................................................... 337

III. OPERATION

1 DATA INPUT/OUTPUT ....................................................................... 347

1.1 INPUT/OUTPUT ON EACH SCREEN ....................................................... 348

1.1.1 Inputting and Outputting Y-axis Offset Data .......................................................349

1.1.1.1 Inputting Y-axis offset data ............................................................................. 349

1.1.1.2 Outputting Y-axis Offset Data......................................................................... 350

1.1.2 Inputting and Outputting Tool Offset / 2nd Geometry Data ................................351

1.1.2.1 Inputting tool offset / 2nd geometry data......................................................... 351

1.1.2.2 Outputting tool offset / 2nd geometry data...................................................... 352

1.2 INPUT/OUTPUT ON THE ALL IO SCREEN.............................................. 353

1.2.1 Inputting and Outputting Y-axis Offset Data .......................................................354

1.2.2 Inputting and Outputting Tool Offset / 2nd Geometry Data ................................355

2 SETTING AND DISPLAYING DATA...................................................356

OFFSET

2.1 SCREENS DISPLAYED BY FUNCTION KEY

2.1.1 Setting and Displaying the Tool Offset Value .....................................................358

2.1.2 Direct Input of Tool Offset Value ........................................................................362

c-4

SETTING

.................................. 357

B-63944EN-1/02 TABLE OF CONTENTS

2.1.3 Input of Tool Offset Value Measured B ...............................................................364

2.1.4 Counter Input of Offset value...............................................................................367

2.1.5 Setting the Workpiece Coordinate System Shift Value........................................368

2.1.6 Setting Tool Compensation/Second Geometry Offset Values .............................371

2.1.7 Setting the Y-Axis Offset .....................................................................................374

2.1.8 Chuck and Tail Stock Barriers .............................................................................377

APPENDIX

A PARAMETERS.................................................................................... 387

A.1 DESCRIPTION OF PARAMETERS........................................................... 388

A.2 DATA TYPE............................................................................................... 431

A.3 STANDARD PARAMETER SETTING TABLES......................................... 432

c-5

I. GENERAL

B-63944EN-1/02 GENERAL 1.GENERAL

1 GENERAL

This manual consists of the following parts:

About this manual

I. GENERAL
Describes chapter organization, applicable models, related

manuals, and notes for reading this manual.

II. PROGRAMMING
Describes each function: Format used to program functions in the

NC language, characteristics, and restrictions.

III. OPERATION
Describes the manual operation and automatic operation of a

machine, procedures for inputting and outputting data, and
procedures for editing a program.

APPENDIX
Lists parameters.

NOTE

1 This manual describes the functions that can

operate in the lathe system path control type. For

other functions not specific to the lathe system,

refer to the User's Manual (Common to Lathe

System/Machining Center System) (B-63944EN).
2 Some functions described in this manual may not

be applied to some products. For detail, refer to the

DESCRIPTIONS manual (B-63942EN).
3 This manual does not detail the parameters not

mentioned in the text. For details of those

parameters, refer to the parameter manual (B-

63950EN).
Parameters are used to set functions and

operating conditions of a CNC machine tool, and

frequently-used values in advance. Usually, the

machine tool builder factory-sets parameters so

that the user can use the machine tool easily.
4 This manual describes not only basic functions but

also optional functions. Look up the options

incorporated into your system in the manual written

by the machine tool builder.

- 3 -

1.GENERAL GENERAL B-63944EN-1/02

Applicable models

The models covered by this manual, and their abbreviations are :

Model name Abbreviation

FANUC Series 30i-MODEL A 30i –A Series 30i
FANUC Series 300i-MODEL A 300i–A Series 300i
FANUC Series 300is-MODEL A 300is–A Series 300is

FANUC Series 31i-MODEL A 31i –A
FANUC Series 31i-MODEL A5 31i –A5

FANUC Series 310i-MODEL A 310i–A
FANUC Series 310i-MODEL A5 310i–A5

FANUC Series 310is-MODEL A 310is–A
FANUC Series 310is-MODEL A5 310is–A5

FANUC Series 32i-MODEL A 32i –A Series 32i
FANUC Series 320i-MODEL A 320i–A Series 320i
FANUC Series 320is-MODEL A 320is–A Series 320is

Series 31i

Series 310i

Series 310is

NOTE

1 Unless otherwise noted, the model names

31i/310i/310is-A, 31i/310i/310is-A5, and
32i/320i/320is-A are collectively referred to as
30i/300i/300is. However, this convention is not
necessarily observed when item 3 below is
applicable.

2 Some functions described in this manual may not

be applied to some products.

For details, refer to the DESCRIPTIONS (B-

63942EN).

Special symbols

This manual uses the following symbols:

- IP

Indicates a combination of axes such as X_ Y_ Z_
In the underlined position following each address, a numeric value
such as a coordinate value is placed (used in PROGRAMMING.).

- ;

Indicates the end of a block. It actually corresponds to the ISO code
LF or EIA code CR.

- 4 -

B-63944EN-1/02 GENERAL 1.GENERAL

Related manuals of
Series 30i/300i/300is- MODEL A
Series 31i/310i/310is- MODEL A
Series 31i/310i/310is- MODEL A5
Series 32i/320i/320is- MODEL A

The following table lists the manuals related to Series 30i/300i /300is-
A, Series 31i/310i /310is-A, Series 31i/310i /310is-A5, Series
32i/320i /320is-A. This manual is indicated by an asterisk(*).

Table 1 Related manuals

Manual name Specification

number

DESCRIPTIONS B-63942EN
CONNECTION MANUAL (HARDWARE) B-63943EN
CONNECTION MANUAL (FUNCTION) B-63943EN-1
USER’S MANUAL
(Common to Lathe System/Machining Center System)
USER’S MANUAL (For Lathe System) B-63944EN-1 *
USER’S MANUAL (For Lathe Machining Center System) B-63944EN-2
MAINTENANCE MANUAL B-63945EN
PARAMETER MANUAL B-65950EN
Programming
Macro Compiler / Macro Executor PROGRAMMING
MANUAL
Macro Compiler OPERATOR’S MANUAL B-66264EN
C Language Executor OPERATOR’S MANUAL B-63944EN-3
PMC
PMC PROGRAMMING MANUAL B-63983EN
Network
PROFIBUS-DP Board OPERATOR’S MANUAL B-63994EN
Fast Ethernet / Fast Data Server OPERATOR’S MANUAL B-64014EN
DeviceNet Board OPERATOR’S MANUAL B-64044EN
Operation guidance function
MANUAL GUIDE i OPERATOR’S MANUAL
MANUAL GUIDE i Set-up Guidance
OPERATOR’S MANUAL

B-63944EN

B-63943EN-2

B-63874EN
B-63874EN-1

- 5 -

1.GENERAL GENERAL B-63944EN-1/02

Related manuals of SERVO MOTOR αis/αi/βis/βi series

The following table lists the manuals related to SERVO MOTOR
αis/αi/βis/βi series

Table 2 Related manuals

Manual name

FANUC AC SERVO MOTOR αis series
FANUC AC SERVO MOTOR αi series
DESCRIPTIONS
FANUC AC SPINDLE MOTOR αi series
DESCRIPTIONS
FANUC AC SERVO MOTOR βis series
DESCRIPTIONS
FANUC AC SPINDLE MOTOR βi series
DESCRIPTIONS
FANUC SERVO AMPLIFIER αi series
DESCRIPTIONS
FANUC SERVO AMPLIFIER βi series
DESCRIPTIONS
FANUC SERVO MOTOR αis series
FANUC SERVO MOTOR αi series
FANUC AC SPINDLE MOTOR αi series
FANUC SERVO AMPLIFIER αi series
MAINTENANCE MANUAL
FANUC SERVO MOTOR βis series
FANUC AC SPINDLE MOTOR βi series
FANUC SERVO AMPLIFIER βi series
MAINTENANCE MANUAL
FANUC AC SERVO MOTOR αis series
FANUC AC SERVO MOTOR αi series
FANUC AC SERVO MOTOR βis series
PARAMETER MANUAL
FANUC AC SPINDLE MOTOR αi series
FANUC AC SPINDLE MOTOR βi series
PARAMETER MANUAL

Any of the servo motors and spindles listed above can be connected to
the CNC described in this manual. However, αi series servo amplifiers
can only be connected to αi series SVMs (for 30i/31i/32i).
This manual mainly assumes that the FANUC SERVO MOTOR αi
series of servo motor is used. For servo motor and spindle information,
refer to the manuals for the servo motor and spindle that are actually
connected.

Specification

number

B-65262EN

B-65272EN

B-65302EN

B-65312EN

B-65282EN

B-65322EN

B-65285EN

B-65325EN

B-65270EN

B-65280EN

- 6 -

B-63944EN-1/02 GENERAL 1.GENERAL

1.1 NOTES ON READING THIS MANUAL

CAUTION

1 The function of an CNC machine tool system

depends not only on the CNC, but on the
combination of the machine tool, its magnetic
cabinet, the servo system, the CNC, the operator's
panels, etc. It is too difficult to describe the function,
programming, and operation relating to all
combinations. This manual generally describes these
from the stand-point of the CNC. So, for details on a
particular CNC machine tool, refer to the manual
issued by the machine tool builder, which should take
precedence over this manual.

2 In the header field of each page of this manual, a

chapter title is indicated so that the reader can
reference necessary information easily.
By finding a desired title first, the reader can
reference necessary parts only.

3 This manual describes as many reasonable variations

in equipment usage as possible. It cannot address
every combination of features, options and commands
that should not be attempted.

If a particular combination of operations is not

described, it should not be attempted.

1.2 NOTES ON VARIOUS KINDS OF DATA

CAUTION

Machining programs, parameters, offset data, etc.

are stored in the CNC unit internal non-volatile
memory. In general, these contents are not lost by
the switching ON/OFF of the power. However, it is
possible that a state can occur where precious data
stored in the non-volatile memory has to be deleted,
because of deletions from a maloperation, or by a
failure restoration. In order to restore rapidly when
this kind of mishap occurs, it is recommended that
you create a copy of the various kinds of data
beforehand.

- 7 -

II. PROGRAMMING

B-63944EN-1/02 PROGRAMMING 1.GENERAL

1 GENERAL

- 11 -

1.GENERAL PROGRAMMING B-63944EN-1/02

1.1 OFFSET

Explanation

- Tool offset

Usually, several tools are used for machining one workpiece. The
tools have different tool length. It is very troublesome to change the
program in accordance with the tools.

Therefore, the length of each tool used should be measured in advance.
By setting the difference between the length of the standard tool and
the length of each tool in the CNC (see “Setting and Displaying Data”
in the User’s Manual (Common to T/M series)), machining can be
performed without altering the program even when the tool is changed.
This function is called tool offset.

Standard
tool

Rough
cutting
tool

Finishing
tool

Grooving
tool

Threading
tool

Workpiece

Fig. 1.1 (a) Tool offset

- 12 -

B-63944EN-1/01 PROGRAMMING 2.PREPARATORY FUNCTION (G FUNCTION)

2 PREPARATORY FUNCTION (G

FUNCTION)

A number following address G determines the meaning of the
command for the concerned block.
G codes are divided into the following two types.

Type Meaning

One-shot G code

Modal G code

(Example)
G01 and G00 are modal G codes in group 01.

G01 X_ ;
Z_ ; G01 is effective in this range.
X_ ;
G00 Z_ ; G00 is effective in this range.
X_ ;
G01 X_ ;
:

There are three G code systems in the lathe system : A,B, and C
(Table 2(a)). Select a G code system using the parameters GSB and
GSC (No. 3401#6 and #7). To use G code system B or C, the
corresponding option is needed. Generally, User’s Manual describes
the use of G code system A, except when the described item can use
only G code system B or C. In such cases, the use of G code system B
or C is described.

The G code is effective only in the block in which it
is specified.
The G code is effective until another G code of the
same group is specified.

- 13 -

2.PREPARATORY FUNCTION (G FUNCTION) PROGRAMMING B-63944EN-1/01

Explanation

1. When the clear state (parameter CLR (No. 3402#6)) is set at
power-up or reset, the modal G codes are placed in the states
described below.
(1) The modal G codes are placed in the states marked with

as indicated in Table.

(2) G20 and G21 remain unchanged when the clear state is set

at power-up or reset.

(3) Which status G22 or G23 at power on is set by parameter

G23 (No. 3402#7). However, G22 and G23 remain
unchanged when the clear state is set at reset.

(4) The user can select G00 or G01 by setting parameter G01

(No. 3402#0).

(5) The user can select G90 or G91 by setting parameter G91

(No. 3402#3).

When G code system B or C is used in the lathe system,

setting parameter G91 (No. 3402#3) determines which code,
either G90 or G91, is effective.

2. G codes other than G10 and G11 are one-shot G codes.

3. When a G code not listed in the G code list is specified, or a G
code that has no corresponding option is specified, alarm PS0010
occurs.

4. Multiple G codes can be specified in the same block if each G
code belongs to a different group. If multiple G codes that belong
to the same group are specified in the same block, only the last G
code specified is valid.

5. If a G code belonging to group 01 is specified in a for drilling,
the canned cycle for drilling is cancelled. This means that the
same state set by specifying G80 is set. Note that the G codes in
group 01 are not affected by a G code specifying a canned cycle.

6. When G code system A is used, absolute or incremental
programming is specified not by a G code (G90/G91) but by an
address word (X/U, Z/W, C/H, Y/V). Only the initial level is
provided at the return point of the canned cycle for drilling..

7. G codes are indicated by group.

- 14 -

B-63944EN-1/01 PROGRAMMING 2.PREPARATORY FUNCTION (G FUNCTION)

Table 2(a) G code list

G code system

A B C

G00 G00 G00 Positioning (Rapid traverse)
G01 G01 G01 Linear interpolation (Cutting feed)
G02 G02 G02 Circular interpolation CW or helical interpolation CW

G03 G03 G03 Circular interpolation CCW or helical interpolation CCW
G02.2 G02.2 G02.2 Involute interpolation CW
G02.3 G02.3 G02.3 Exponential interpolation CW
G02.4 G02.4 G02.4 Three-dimensional coordinate conversion CW
G03.2 G03.2 G03.2 Involute interpolation CCW
G03.3 G03.3 G03.3 Exponential interpolation CCW
G03.4 G03.4 G03.4

G04 G04 G04 Dwell

G05 G05 G05

G05.1 G05.1 G05.1 AI contour control / Nano smoothing / Smooth interpolation

G05.4 G05.4 G05.4
G06.2 G06.2 G06.2 01 NURBS interpolation

G07 G07 G07 Hypothetical axis interpolation
G07.1

(G107)

G08 G08 G08 Advanced preview control

G09 G09 G09 Exact stop

G10 G10 G10 Programmable data input

G10.6 G10.6 G10.6

G10.9 G10.9 G10.9

G11 G11 G11
G12.1

(G112)

G13.1

(G113)

G15 G15 G15 Polar coordinate command cancel

G16 G16 G16

G17 G17 G17 XpYp plane selection

G18 G18 G18 ZpXp plane selection

G19 G19 G19

G20 G20 G70 Input in inch

G21 G21 G71

G22 G22 G22 Stored stroke check function on

G23 G23 G23

G25 G25 G25

G26 G26 G26

G07.1

(G107)

G12.1

(G112)

G13.1

(G113)

G07.1

(G107)

G12.1

(G112)

G13.1

(G113)

Group Function

01

Three-dimensional coordinate conversion CCW

AI contour control (command compatible with high precision

00

00

21

24

16

06

09

08

contour control)

HRV3,4 on/off

Cylindrical interpolation

Tool retract and recover

Programmable switching of diameter/radius specification

Programmable data input mode cancel

Polar coordinate interpolation mode

Polar coordinate interpolation cancel mode

Polar coordinate command

YpZp plane selection

Input in mm

Stored stroke check function off

Spindle speed fluctuation detection off

Spindle speed fluctuation detection on

- 15 -

2.PREPARATORY FUNCTION (G FUNCTION) PROGRAMMING B-63944EN-1/01

Table 2(a) G code list

G code system

A B C

G27 G27 G27 Reference position return check

G28 G28 G28 Return to reference position

G29 G29 G29 Movement from reference position

G30 G30 G30 2nd, 3rd and 4th reference position return
G30.1 G30.1 G30.1 Floating reference point return

G31 G31 G31 Skip function
G31.8 G31.8 G31.8

G32 G33 G33 Threading

G34 G34 G34 Variable lead threading

G35 G35 G35 Circular threading CW

G36 G36 G36

G37 G37 G37

G37.1 G37.1 G37.1

G37.2 G37.2 G37.2

G38 G38 G38

G39 G39 G39

G40 G40 G40 Cutter compensation of tool nose radius compensation : cancel

G41 G41 G41 Cutter compensation of tool nose radius compensation : left

G42 G42 G42 Cutter compensation of tool nose radius compensation : right
G41.2 G41.2 G41.2 Cutter compensation for 5-axis machining : left (type 1)

G41.3 G41.3 G41.3

G41.4 G41.4 G41.4

G41.5 G41.5 G41.5

G41.6 G41.6 G41.6 Cutter compensation for 5-axis machining : left (type 2)
G42.2 G42.2 G42.2 Cutter compensation for 5-axis machining : right (type 1)

G42.4 G42.4 G42.4

G42.5 G42.5 G42.5

G42.6 G42.6 G42.6

G43 G43 G43 Tool length compensation +

G44 G44 G44 Tool length compensation ­G43.1 G43.1 G43.1 Tool length compensation in tool axis direction
G43.4 G43.4 G43.4 Tool center point control (type 1)
G43.5 G43.5 G43.5 Tool center point control (type 2)
G43.7

(G44.7)

G49

(G49.1)

G43.7

(G44.7)

G49

(G49.1)

G43.7

(G44.7)

G49

(G49.1)

Group Function

00

EGB-axis skip

Circular threading CCW (When the parameter G36 (No. 3405#3)
is set to 1) or Automatic tool offset (X axis) (When the parameter
G36 (No. 3405#3) is set to 0)
Automatic tool offset (Z axis) (When the parameter G36 (No.

01

07

23

3405#3) is set to 0)
Automatic tool offset (X axis) (When the parameter G36 (No.
3405#3) is set to 1)
Automatic tool offset (Z axis) (When the parameter G36 (No.
3405#3) is set to 1)
Cutter compensation of tool nose radius compensation: with
vector held
Cutter compensation of tool nose radius compensation: corner
rounding interpolation

Cutter compensation for 5-axis machining :
(leading edge offset)
Cutter compensation for 5-axis machining : left (type 1)
(FS16i-compatible command)
Cutter compensation for 5-axis machining : left (type 1)
(FS16i-compatible command)

Cutter compensation for 5-axis machining : right (type 1)
(FS16i-compatible command)
Cutter compensation for 5-axis machining : right (type 1)
(FS16i-compatible command)
Cutter compensation for 5-axis machining : right (type 2)

Tool offset (lathe system ATC type)

Tool length compensation cancel

- 16 -

B-63944EN-1/01 PROGRAMMING 2.PREPARATORY FUNCTION (G FUNCTION)

Table 2(a) G code list

G code system

A B C

G50 G92 G92 Coordinate system setting or max. spindle speed clamp
G50.3 G92.1 G92.1

- G50 G50 Scaling cancel

- G51 G51
G50.1 G50.1 G50.1 Programmable mirror image cancel
G51.1 G51.1 G51.1
G50.2

(G250)

G51.2

(G251)

G52 G52 G52 Local coordinate system setting
G53 G53 G53 Machine coordinate system setting

G53.1 G53.1 G53.1

G54

(G54.1)

G55 G55 G55 Workpiece coordinate system 2 selection
G56 G56 G56 Workpiece coordinate system 3 selection
G57 G57 G57 Workpiece coordinate system 4 selection
G58 G58 G58 Workpiece coordinate system 5 selection
G59 G59 G59
G60 G60 G60 00 Single direction positioning
G61 G61 G61 Exact stop mode
G62 G62 G62 Automatic corner override mode
G63 G63 G63 Tapping mode
G64 G64 G64
G65 G65 G65 00 Macro call
G66 G66 G66 Macro modal call A

G66.1 G66.1 G66.1 Macro modal call B

G67 G67 G67
G68 G68 G68 04 Mirror image on for double turret or balance cutting mode

G68.1 G68.1 G68.1

G68.2 G68.2 G68.2

G69 G69 G69 04 Mirror image off for double turret or balance cutting mode cancel

G69.1 G69.1 G69.1 17

G70 G70 G72 Finishing cycle
G71 G71 G73 Stock removal in turning
G72 G72 G74 Stock removal in facing
G73 G73 G75 Pattern repeating cycle
G74 G74 G76 End face peck drilling cycle
G75 G75 G77 Outer diameter/internal diameter drilling cycle

G76 G76 G78 Multiple-thread cutting cycle
G72.1 G72.1 G72.1 Figure copy (rotation copy)
G72.2 G72.2 G72.2

G50.2

(G250)

G51.2

(G251)

G54

(G54.1)

G50.2

(G250)

G51.2

(G251)

G54

(G54.1)

Group Function

00

18

22

20

00

14

15

12

17

00

Workpiece coordinate system preset

Scaling

Programmable mirror image

Polygon turning cancel

Polygon turning

Tool axis direction control

Workpiece coordinate system 1 selection

Workpiece coordinate system 6 selection

Cutting mode

Macro modal call A/B cancel

Coordinate system rotation start or 3-dimensional coordinate
conversion mode on
Feature coordinate system selection

Coordinate system rotation cancel or 3-dimensional coordinate
conversion mode off

Figure copy (parallel copy)

- 17 -

2.PREPARATORY FUNCTION (G FUNCTION) PROGRAMMING B-63944EN-1/01

Table 2(a) G code list

G code system

A B C

G80 G80 G80 10 Canned cycle cancel for drilling
G80.5 G80.5 G80.5 27 Electronic gear box 2 pair: synchronization cancellation
G80.8 G80.8 G80.8 28 Electronic gear box: synchronization cancellation

G81 G81 G81 10 Spot drilling (FS15-T format)
G81.5 G81.5 G81.5 27 Electronic gear box 2 pair: synchronization start
G81.8 G81.81 G81.8 28 Electronic gear box: synchronization start

G82 G82 G82 Counter boring (FS15-T format)

G83 G83 G83 Cycle for face drilling
G83.1 G83.1 G83.1 High-speed peck drilling cycle (FS15-T format)
G83.5 G83.5 G83.5 High-speed peck drilling cycle
G83.6 G83.6 G83.6 Peck drilling cycle

G84 G84 G84 Cycle for face tapping
G84.2 G84.2 G84.2 Rigid tapping cycle (FS15-T format)

G85 G85 G85 Cycle for face boring

G87 G87 G87 Cycle for side drilling
G87.5 G87.5 G87.5 High-speed peck drilling cycle
G87.6 G87.6 G87.6 Peck drilling cycle

G88 G88 G88 Cycle for side tapping

G89 G89 G89

G90 G77 G20 Outer diameter/internal diameter cutting cycle

G92 G78 G21 Threading cycle

G94 G79 G24
G91.1 G91.1 G91.1 00 Maximum specified incremental amount check

G96 G96 G96 Constant surface speed control

G97 G97 G97

G93 G93 G93 Inverse time feed

G98 G94 G94 Feed per minute

G99 G95 G95

- G90 G90 Absolute programming

- G91 G91

- G98 G98 Canned cycle : return to initial level

- G99 G99

Group Function

10

Cycle for side boring

01

End face turning cycle

02

05

03

11

Constant surface speed control cancel

Feed per revolution

Incremental programming

Canned cycle : return to R point level

- 18 -

B-63944EN-1/02 PROGRAMMING 3.INTERPOLATION FUNCTION

3 INTERPOLATION FUNCTION

- 19 -

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-1/02

δ

α

δ

3.1 CONSTANT LEAD THREADING (G32)

Tapered screws and scroll threads in addition to equal lead straight
threads can be cut by using a G32 command.

The spindle speed is read from the position coder on the spindle in
real time and converted to a cutting feedrate for feed-per minute mode,
which is used to move the tool.

L

Straight thread

Format

G32IP_F_;

IP_: End point

F _: Lead of the long axis
(always radius programming)

L

Tapered screw

L

Scroll thread

Fig. 3.1 (a) Thread types

X axis

End point_

X

0

2

Z

1

Start point

Z axis

L

Fig. 3.1 (b) Example of threading

Explanation

In general, threading is repeated along the same tool path in rough
cutting through finish cutting for a screw. Since threading starts when
the position coder mounted on the spindle outputs a
one-spindle-rotation signal, threading is started at a fixed point and the
tool path on the workpiece is unchanged for repeated threading. Note
that the spindle speed must remain constant from rough cutting
through finish cutting. If not, incorrect thread lead will occur.

- 20 -

B-63944EN-1/02 PROGRAMMING 3.INTERPOLATION FUNCTION

X

X

α

α

≤

Tapered thread

L

Z

LZ

45° lead is LZ

lead is LX

α≥45°

Fig. 3.1 (c) LZ and LX of a tapered thread

In general, the lag of the servo system, etc. will produce somewhat
incorrect leads at the starting and ending points of a thread cut. To
compensate for this, a threading length somewhat longer than required
should be specified.
Table 3.1 (a) lists the ranges for specifying the thread lead.

Table 3.1 (a) Ranges of lead sizes that can be specified

Least command increment

Metric input 0.0001 to 500.0000 mm

Inch input 0.000001 to 9.999999 inch

- 21 -

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-1/02

φ

Example

1. Straight threading

The following values are used in programming :

X axis

δ

2

2.Tapered threading

X axis

50

φ

δ

43

φ

0

30

30mm

δ

1

Zaxis

70

2

δ

1

Zaxis

14

40

Thread lead :4mm

=3mm

δ

1

=1.5mm

δ

Depth of cut :1mm (cut twice)

2

(Metric input, diameter programming)

G00 U-62.0 ;
G32 W-74.5 F4.0 ;
G00 U62.0 ;
W74.5 ;
U-64.0 ;
(For the second cut, cut 1mm more)
G32 W-74.5 ;
G00 U64.0 ;
W74.5 ;

The following values are used in programming :
Thread lead : 3.5mm in the direction of the Z axis

=2mm

δ

1

=1mm

δ

Cutting depth in the X axis direction is 1mm (cut twice)

2

(Metric input, diameter programming)
G00 X 12.0 Z72.0 ;
G32 X 41.0 Z29.0 F3.5 ;
G00 X 50.0 ;
Z 72.0 ;
X 10.0 ;
(Cut 1mm more for the second cut)
G32 X 39.0 Z29.0 ;
G00 X 50.0 ;
Z 72.0 ;

- 22 -

B-63944EN-1/02 PROGRAMMING 3.INTERPOLATION FUNCTION

WARNING

1 Feedrate override is effective (fixed at 100%) during threading.
2 It is very dangerous to stop feeding the thread cutter without stopping the spindle.

This will suddenly increase the cutting depth. Thus, the feed hold function is
ineffective while threading. If the feed hold button is pressed during threading, the
tool will stop after a block not specifying threading is executed as if the SINGLE
BLOCK button were pushed. However, the feed hold lamp (SPL lamp) lights when
the FEED HOLD button on the machine control panel is pushed. Then, when the
tool stops, the lamp is turned off (Single Block stop status).

3 When the FEED HOLD button is pressed again in the first block after threading

mode that does not specify threading (or the button has been held down), the tool
stops immediately at the block that does not specify threading.

4 When threading is executed in the single block status, the tool stops after execution

of the first block not specifying threading.

5 When the mode was changed from automatic operation to manual operation during

threading, the tool stops at the first block not specifying threading as when the feed
hold button is pushed as mentioned in Warning 3.

However, when the mode is changed from one automatic operation mode to

another, the tool stops after execution of the block not specifying threading as for
the single block mode in Note 4.

6 When the previous block was a threading block, cutting will start immediately

without waiting for detection of the one-spindle-rotation signal even if the present

block is a threading block.
G32Z _ F_ ;
Z _; (A 1-turn signal is not detected before this block.)
G32 ; (Regarded as threading block.)
Z_ F_ ; (One turn signal is also not detected.)
7 Because the constant surface speed control is effective during scroll thread or

tapered screw cutting and the spindle speed changes, the correct thread lead may

not be cut. Therefore, do not use the constant surface speed control during

threading. Instead, use G97.
8 A movement block preceding the threading block must not specify chamfering or

corner R.
9 A threading block must not specifying chamfering or corner R.
10 The spindle speed override function is disabled during threading. The spindle

speed is fixed at 100%.
11 Thread cycle retract function is ineffective to G32.

- 23 -

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-1/02

3.2 CONTINUOUS THREADING

Threading blocks can be programmed successively to eliminate a
discontinuity due to a discontinuous movement in machining by
adjacent blocks.

Explanation

Since the system is controlled in such a manner that the synchronism
with the spindle does not deviate in the joint between blocks wherever
possible, it is possible to performed special threading operation in
which the lead and shape change midway.

G32

G32

Fig. 3.2 (a) Continuous threading (Example of G32 in G code system A)

G32

Even when the same section is repeated for threading while changing
the depth of cut, this system allows a correct machining without
impairing the threads.

- 24 -

B-63944EN-1/02 PROGRAMMING 3.INTERPOLATION FUNCTION

3.3 MULTIPLE THREADING

Using the Q address to specify an angle between the
one-spindle-rotation signal and the start of threading shifts the
threading start angle, making it possible to produce multiple-thread
screws with ease.

L

L : Lead

Format

(Constant lead threading)
G32 IP _ F_ Q_ ;

IP : End point
F_ : Lead in longitudinal direction

G32 IP _ Q_ ;

Q_ : Threading start angle

Explanation

- Available threading commands

G32: Constant lead threading
G34: Variable lead threading
G76: Combined threading cycle
G92: Threading cycle

Limitation

- Start angle

The start angle is not a continuous state (modal) value. It must be
specified each time it is used. If a value is not specified, 0 is assumed.

- Start angle increment

The start angle (Q) increment is 0.001 degrees. Note that no decimal
point can be specified.
Example:
For a shift angle of 180 degrees, specify Q180000.
Q180.000 cannot be specified, because it contains a decimal

Fig. 3.3 (a) Multiple thread screws.

point.

- 25 -

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-1/02

- Specifiable start angle range

A start angle (Q) of between 0 and 360000 (in 0.001-degree units) can
be specified. If a value greater than 360000 (360 degrees) is specified,
it is rounded down to 360000 (360 degrees).

- Combined threading cycle (G76)

For the G76 combined threading cycle command, always use the FS15
tape format.

Example

Program for producing double-threaded screws
(with start angles of 0 and 180 degrees)

G00 X40.0 ;
G32 W-38.0 F4.0 Q0 ;
G00 X72.0 ;
W38.0 ;
X40.0 ;
G32 W-38.0 F4.0Q180000 ;
G00 X72.0 ;
W38.0 ;

- 26 -

B-63944EN-1/02 PROGRAMMING 3.INTERPOLATION FUNCTION

3.4 TORQUE LIMIT SKIP (G31 P99)

With the motor torque limited (for example, by a torque limit
command, issued through the PMC window), a move command
following G31 P99 (or G31 P98) can cause the same type of cutting
feed as with G01 (linear interpolation).
With the issue of a signal indicating a torque limit has been reached
(because of pressure being applied or for some other reason), a skip
occurs.
For details of how to use this function, refer to the manuals supplied
by the machine tool builder.

Format

G31 P99 IP _ F_ ;
G31 P98 IP _ F_ ;

G31 : One-shot G code (G code effective only in the block in

which it is issued)

Explanation

- G31 P99

If the motor torque limit is reached, or a SKIP signal is received
during execution of G31 P99, the current move command is aborted,
and the next block is executed.

- G31 P98

If the motor torque limit is reached during execution of G31 P98, the
current move command is aborted, and the next block is executed. The
SKIP signal <X0004#7/Path 2 X0013#7> does not affect G31 P98.
Entering a SKIP signal during the execution of G31 P98 does not
cause a skip.

- Torque limit command

If a torque limit is not specified before the execution of G31 P99/98,
the move command continues; no skip occurs even if a torque limit is
reached.

- Custom macro system variable

When G31 P99/98 is specified, the custom macro variables hold the
coordinates at the end of a skip.
If a SKIP signal causes a skip with G31 P99, the custom macro system
variables hold the coordinates based on the machine coordinate system
when it stops, rather than those when the SKIP signal is entered.

- 27 -

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-1/02

Limitation

- Axis command

Only one axis can be controlled in each block with G31 P98/99.
If two or more axes are specified to be controlled in such blocks, or no
axis command is issued, alarm PS0369 is generated.

- Simple synchronous control and angular axis control

G31 P99/98 cannot be used for axes subject to simple synchronous
control or the X-axis or Z-axis when under angular axis control.

- Speed control

Parameter SKF (No. 6200#7) must be set to disable dry run, override,
and automatic acceleration/deceleration for G31 skip commands.

- Consecutive commands

Do not use G31 P99/98 in consecutive blocks.

WARNING

Always specify a torque limit before a G31 P99/98

command. Otherwise, G31 P99/98 allows move
commands to be executed without causing a skip.

NOTE

If G31 is issued with cutter or tool nose radius

compensation specified, alarm PS035 is generated.
Therefore, before issuing G31, execute G40 to
cancel cutter or tool nose radius compensation.

Example

O0001 ;
:
:
Mxx ;
:
:
G31 P99 X200. F100 ;
:
G01 X100. F500 ;
:
:
Myy ;
:
:
M30 ;
:
%

The PMC specifies the torque limit
through the window.

Torque limit skip command

Move command for which a torque
limit is applied

Torque limit canceled by the PMC

- 28 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

4 FUNCTIONS TO SIMPLIFY

PROGRAMMING

This chapter explains the following items:

4.1 CANNED CYCLE (G90, G92, G94)

4.2 MULTIPLE REPETITIVE CYCLE (G70-G76)

4.3 CANNED CYCLE FOR DRILLING

4.4 RIGID TAPPING

4.5 CHAMFERING AND CORNER R

4.6 MIRROR IMAGE FOR DOUBLE TURRET (G68, G69)

4.7 DIRECT DRAWING DIMENSION PROGRAMMING

- 29 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

4.1 CANNED CYCLE (G90, G92, G94)

There are three canned cycles : the outer diameter/internal diameter
cutting canned cycle (G90), the threading canned cycle (G92), and the
end face turning canned cycle (G94).

NOTE

1 Explanatory figures in this section use the ZX plane

as the selected plane, diameter programming for
the X-axis, and radius programming for the Z-axis.
When radius programming is used for the X-axis,
change U/2 to U and X/2 to X.

2 A canned cycle can be performed on any plane

(including parallel axes for plane definition). When
G-code system A is used, however, U, V, and W
cannot be set as a parallel axis.

3 The direction of the length means the direction of

the first axis on the plane as follows:
ZX plane: Z-axis direction
YZ plane: Y-axis direction
XY plane: X-axis direction
4 The direction of the end face means the direction of

the second axis on the plane as follows:
ZX plane: X-axis direction
YZ plane: Z-axis direction
XY plane: Y-axis direction

- 30 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

A’A

4.1.1 Outer Diameter/Internal Diameter Cutting Cycle (G90)

This cycle performs straight or taper cutting in the direction of the
length.

4.1.1.1 Straight cutting cycle

Format

G90X(U)_Z(W)_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the

figure below) in the direction of the length

U_,W_ : Travel distance to the cutting end point (point A' in

the figure below) in the direction of the length

F_ : Cutting feedrate

Explanation

- Operations

X axis

Z

W

4(R)

3(F)

2(F)

Fig. 4.1.1 (a) Straight cutting cycle

1(R)

(R)....Rapid traverse

(F) ....Cutting feed

U/2

X/2

Z axis

A straight cutting cycle performs four operations:
(1) Operation 1 moves the tool from the start point (A) to the

specified coordinate of the second axis on the plane (specified
X-coordinate for the ZX plane) in rapid traverse.

(2) Operation 2 moves the tool to the specified coordinate of the first

axis on the plane (specified Z-coordinate for the ZX plane) in
cutting feed. (The tool is moved to the cutting end point (A') in
the direction of the length.)

(3) Operation 3 moves the tool to the start coordinate of the second

axis on the plane (start X-coordinate for the ZX plane) in cutting
feed.

(4) Operation 4 moves the tool to the start coordinate of the first axis

on the plane (start Z-coordinate for the ZX plane) in rapid
traverse. (The tool returns to the start point (A).)

- 31 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

NOTE

In single block mode, operations 1, 2, 3 and 4 are

performed by pressing the cycle start button once.

- Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other
than G90, G92, or G94.

- 32 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

A

A

4.1.1.2 Taper cutting cycle

Format

G90 X(U)_Z(W)_R_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the

figure below) in the direction of the length

U_,W_ : Travel distance to the cutting end point (point A' in

the figure below) in the direction of the length
R_ : Taper amount (R in the figure below)
F_ : Cutting feedrate

X axis

(R)....Rapid traverse

4(R)

(F) ....Cutting feed

Explanation

- Operations

3(F)

U/2

X/2

Z

’

W

Fig. 4.1.1 (b) Taper cutting cycle

2(F)

1(R)

R

Z axis

The figure of a taper is determined by the coordinates of the cutting
end point (A') in the direction of the length and the sign of the taper
amount (address R). For the cycle in the figure above, a minus sign
is added to the taper amount.

NOTE

The increment system of address R for specifying a

taper depends on the increment system for the
reference axis. Specify a radius value at R.

A taper cutting cycle performs the same four operations as a straight
cutting cycle.
However, operation 1 moves the tool from the start point (A) to the
position obtained by adding the taper amount to the specified
coordinate of the second axis on the plane (specified X-coordinate for
the ZX plane) in rapid traverse.
Operations 2, 3, and 4 after operation 1 are the same as for a straight
cutting cycle.

- 33 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

X

NOTE

In single block mode, operations 1, 2, 3, and 4 are

performed by pressing the cycle start button once.

- Relationship between the sign of the taper amount and tool path

The tool path is determined according to the relationship between the
sign of the taper amount (address R) and the cutting end point in the
direction of the length in the absolute or incremental programming as
follows.

Outer diameter machining Internal diameter machining

1. U < 0, W < 0, R < 0 2. U > 0, W < 0, R > 0

X

U/2

X

U/2

X

- Canceling the mode

X

Z

3(F)

2(F)

4(R)

1(R)

X

R

W

Z

U/2 3(F)

W

2(F)

4(R)

3. U < 0, W < 0, R > 0

at |R|≤|U/2|

Z

3(F)

4(R)

2(F)

W

1(R)

X

R

4. U > 0, W < 0, R < 0

at |R|≤|U/2|

X

Z

U/2

3(F)

W

2(F)

4(R)

To cancel the canned cycle mode, specify a group 01 G code other
than G90, G92, or G94.

R

1(R)

R

1(R)

- 34 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

(R)

)

)

A

4.1.2 Threading Cycle (G92)

4.1.2.1 Straight threading cycle

Format

G92 X(U)_Z(W)_F_Q_;

X_,Z_ : Coordinates of the cutting end point (point A' in the

figure below) in the direction of the length
U_,W_ : Travel distance to the cutting end point (point A' in

the figure below) in the direction of the length
Q_ : Angle for shifting the threading start angle
(Increment: 0.001 degrees,

Valid setting range: 0 to 360 degrees)
F_ : Thread lead (L in the figure below)

X axis

Z

W

Explanation

- Operations

3(R

’

Approx.

45°

r

Detailed chamfered thread

Fig. 4.1.2 (c) Straight threading

4(R)

2(F

L

(The chamfered angle in the left figure is 45

degrees or less because of the delay in the

servo system.)

1

(R) ... Rapid traverse

(F).... Cutting feed

U/2

X/2

Z axis

The ranges of thread leads and restrictions related to the spindle speed
are the same as for threading with G32.

A straight threading cycle performs four operations:

(1) Operation 1 moves the tool from the start point (A) to the

specified coordinate of the second axis on the plane (specified
X-coordinate for the ZX plane) in rapid traverse.

(2) Operation 2 moves the tool to the specified coordinate of the first

axis on the plane (specified Z-coordinate for the ZX plane) in
cutting feed. At this time, thread chamfering is performed.

- 35 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

(3) Operation 3 moves the tool to the start coordinate of the second

axis on the plane (start X-coordinate for the ZX plane) in rapid
traverse. (Retraction after chamfering)

(4) Operation 4 moves the tool to the start coordinate of the first axis

on the plane (start Z-coordinate for the ZX plane) in rapid
traverse. (The tool returns to the start point (A).)

CAUTION

Notes on this threading are the same as in

threading in G32. However, a stop by feed hold is
as follows; Stop after completion of path 3 of
threading cycle.

NOTE

In the single block mode, operations 1, 2, 3, and 4

are performed by pressing cycle start button once.

- Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other
than G90, G92, or G94.

- Time constant and FL feedrate for threading

The time constant for acceleration/deceleration after interpolation for
threading specified in parameter No. 1626 and the FL feedrate
specified in parameter No. 1627 are used.

- Thread chamfering

Thread chamfering can be performed. A signal from the machine
tool, initiates thread chamfering. The chamfering distance r is
specified in a range from 0.1L to 12.7L in 0.1L increments by
parameter No. 5130. (In the above expression, L is the thread lead.)
A thread chamfering angle between 1 to 89 degrees can be specified in
parameter No. 5131. When a value of 0 is specified in the parameter,
an angle of 45 degrees is assumed.
For thread chamfering, the same type of acceleration/deceleration after
interpolation, time constant for acceleration/deceleration after
interpolation, and FL feedrate as for threading are used.

NOTE

Common parameters for specifying the amount and

angle of thread chamfering are used for this cycle
and threading cycle with G76.

- 36 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

- Retraction after chamfering

The following table lists the feedrate, type of acceleration/deceleration
after interpolation, and time constant of retraction after chamfering.

Parameter

CFR

(No. 1611#0)

0 Other than

0 0 Uses the type of acceleration/deceleration after

1 Performs an in-position check before retraction

Parameter

No. 1466

0

Description

Uses the type of acceleration/deceleration after
interpolation for threading, time constant for
threading (parameter No. 1626), FL feedrate
(parameter No. 1627), and retraction feedrate
specified in parameter No. 1466.

interpolation for threading, time constant for
threading (parameter No. 1626), FL feedrate
(parameter No. 1627), and rapid traverse rate
specified in parameter No. 1420.

and uses the type of acceleration/deceleration
after interpolation in rapid traverse, time
constant for rapid traverse, FL feedrate, and
rapid traverse rate specified in parameter No.

1420.

By setting bit 4 (ROC) of parameter No. 1403 to 1, rapid traverse
override can be disabled for the feedrate of retraction after
chamfering.

NOTE

During retraction, the machine does not stop with

an override of 0% for the cutting feedrate
regardless of the setting of bit 4 (RF0) of parameter
No. 1401.

- Shifting the start angle

Address Q can be used to shift the threading start angle.
The start angle (Q) increment is 0.001 degrees and the valid setting
range is between 0 and 360 degrees. No decimal point can be
specified.

- Feed hold in a threading cycle

When the threading cycle retract function is not used, the machine
stops at the end point of retraction after chamfering (end point of
operation 3) by feed hold applied during threading.

- 37 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

- Threading cycle retract

When the "threading cycle retract" option function is used, feed hold
may be applied during threading (operation 2). In this case, the tool
immediately retracts with chamfering and returns to the start point on
the second axis (X-axis), then the first axis (Z-axis) on the plane.

X axis

Z axis

Rapid traverse

Cutting feed

Ordinary cycle

Motion at feed hold

Start point

- Inch threading

Feed hold is effected here.

The chamfered angle is the same as that at the end point.

CAUTION

Another feed hold cannot be made during retreat.

Inch threading specified with address E is not allowed.

- 38 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

A

A

A

4.1.2.2 Taper threading cycle

Format

G92 X(U)_Z(W)_R_F_Q_;

X_,Z_ : Coordinates of the cutting end point (point A' in the

figure below) in the direction of the length
U_,W_ : Travel distance to the cutting end point (point A' in

the figure below) in the direction of the length
Q_ : Angle for shifting the threading start angle
(Increment: 0.001 degrees,

Valid setting range: 0 to 360 degrees)
R_ : Taper amount (R in the figure below)
F_ : Thread lead (L in the figure below)

X axis

U/2

X/2

Z

R

’

pprox. 45

r

3(R)

°

W

4(R)

1(R)

2(F)

L

(The chamfered angle in the left figure

is 45 degrees or less because of the

delay in the servo system.)

(R) ....Rapid traverse

(F) ....Cutting feed

Z axis

Detailed chamfered thread

Fig. 4.1.2 (d) Taper threading cycle

- 39 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

Explanation

The ranges of thread leads and restrictions related to the spindle speed
are the same as for threading with G32.
The figure of a taper is determined by the coordinates of the cutting
end point (A') in the direction of the length and the sign of the taper
amount (address R). For the cycle in the figure above, a minus sign
is added to the taper amount.

NOTE

The increment system of address R for specifying a

taper depends on the increment system for the
reference axis. Specify a radius value at R.

- Operations

A taper threading cycle performs the same four operations as a straight
threading cycle.
However, operation 1 moves the tool from the start point (A) to the
position obtained by adding the taper amount to the specified
coordinate of the second axis on the plane (specified X-coordinate for
the ZX plane) in rapid traverse.
Operations 2, 3, and 4 after operation 1 are the same as for a straight
threading cycle.

CAUTION

Notes on this threading are the same as in

threading in G32. However, a stop by feed hold is
as follows; Stop after completion of path 3 of
threading cycle.

NOTE

In the single block mode, operations 1, 2, 3, and 4

are performed by pressing cycle start button once.

- 40 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

X

- Relationship between the sign of the taper amount and tool path

The tool path is determined according to the relationship between the
sign of the taper amount (address R) and the cutting end point in the
direction of the length in the absolute or incremental programming as
follows.

Outer diameter machining Internal diameter machining

1. U < 0, W < 0, R < 0 2. U > 0, W < 0, R > 0

X

U/2

U/2

X

Z

3(F)

X

3. U < 0, W < 0, R > 0

Z

3(F)

4(R)

1(R)

2(F)

W

at |R|≤|U/2|

4(R)

1(R)

2(F)

W

- Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other
than G90, G92, or G94.

- Time constant and FL feedrate for threading

- Thread chamfering

- Retraction after chamfering

- Shifting the start angle

- Threading cycle retract

- Inch threading

See the pages on which a straight threading cycle is explained.

X

Z

X

U/2 3(F)

R

W

2(F)

4(R)

R

1(R)

4. U > 0, W < 0, R < 0

at |R|≤|U/2|

X

Z

X

U/2

R

3(F)

W

2(F)

4(R)

R

1(R)

- 41 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

A

A

4.1.3 End Face Turning Cycle (G94)

4.1.3.1 Face cutting cycle

Format

G92 X(U)_Z(W)_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the

figure below) in the direction of the end face
U_,W_ : Travel distance to the cutting end point (point A' in

the figure below) in the direction of the end face
F_ : Cutting feedrate

X axis

1(R)

(R) .... Rap id traverse

(F) ....Cutting fe ed

Explanation

- Operations

2(F)

U/2

3(F)

’

X/2

Z

Fig. 4.1.3 (e) Face cutting cycle

W

4(R)

Z axis

A face cutting cycle performs four operations:
(1) Operation 1 moves the tool from the start point (A) to the

specified coordinate of the first axis on the plane (specified
Z-coordinate for the ZX plane) in rapid traverse.

(2) Operation 2 moves the tool to the specified coordinate of the

second axis on the plane (specified X-coordinate for the ZX
plane) in cutting feed. (The tool is moved to the cutting end
point (A') in the direction of the end face.)

(3) Operation 3 moves the tool to the start coordinate of the first axis

on the plane (start Z-coordinate for the ZX plane) in cutting feed.

(4) Operation 4 moves the tool to the start coordinate of the second

axis on the plane (start X-coordinate for the ZX plane) in rapid
traverse. (The tool returns to the start point (A).)

NOTE

In single block mode, operations 1, 2, 3, and 4 are

performed by pressing the cycle start button once.

- 42 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

A

A

- Canceling the mode

To cancel the canned cycle mode, specify a group 01 G code other
than G90, G92, or G94.

4.1.3.2 Taper cutting cycle

Format

G94 X(U)_Z(W)_R_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the

figure below) in the direction of the end face
U_,W_ : Travel distance to the cutting end point (point A' in

the figure below) in the direction of the end face
R_ : Taper amount (R in the figure below)
F_ : Cutting feedrate

X axis

Explanation

1(R)

U/2

X/2

Z

Fig. 4.1.3 (f) Taper cutting cycle

2(F)

R

’

4(R)

3(F)

W

(R) ... Rapid traverse
(F) ... Cutting feed

Z axis

The figure of a taper is determined by the coordinates of the cutting
end point (A') in the direction of the end face and the sign of the taper
amount (address R). For the cycle in the figure above, a minus sign
is added to the taper amount.

NOTE

The increment system of address R for specifying a

taper depends on the increment system for the
reference axis. Specify a radius value at R.

- 43 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

X

- Operations

A taper cutting cycle performs the same four operations as a face
cutting cycle.
However, operation 1 moves the tool from the start point (A) to the
position obtained by adding the taper amount to the specified
coordinate of the first axis on the plane (specified Z-coordinate for the
ZX plane) in rapid traverse.
Operations 2, 3, and 4 after operation 1 are the same as for a face
cutting cycle.

NOTE

In single block mode, operations 1, 2, 3, and 4 are

performed by pressing the cycle start button once.

- Relationship between the sign of the taper amount and tool path

The tool path is determined according to the relationship between the
sign of the taper amount (address R) and the cutting end point in the
direction of the end face in the absolute or incremental programming
as follows.

Outer diameter machining Internal diameter machining

1. U < 0, W < 0, R < 0 2. U > 0, W < 0, R > 0

1(R)

X

Z

Z

Z

R

W

X

- Canceling the mode

U/2

Z

3. U < 0, W < 0, R > 0

Z

U/2

Z

2(F)

R

at |R|≤|W|

R

2(F)

To cancel the canned cycle mode, specify a group 01 G code other
than G90, G92, or G94.

3(F)

1(R)

3(F)

W

2(F)

2(F)

3(F)

4(R)

1(R)

W

3(F)

4(R)

1(R)

4(R)

U/2

W

4. U > 0, W < 0, R < 0

at |R|≤|W|

X

Z

4(R)

U/2

Z

R

- 44 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

4.1.4 How to Use Canned Cycles (G90, G92, G94)

An appropriate canned cycle is selected according to the shape of the
material and the shape of the product.

- Straight cutting cycle (G90)

Shape of material

Shape of
product

- Taper cutting cycle (G90)

Shape of material

Shape of product

- 45 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

- Face cutting cycle (G94)

Shape of material

Shape of product

- Face taper cutting cycle (G94)

Shape of material

Shape of product

- 46 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

4.1.5 Canned Cycle and Tool Nose Radius Compensation

When tool nose radius compensation is applied, the tool nose center
path and offset direction are as shown below. At the start point of a
cycle, the offset vector is canceled. Offset start-up is performed for
the movement from the start point of the cycle. The offset vector is
temporarily canceled again at the return to the cycle start point and
offset is applied again according to the next move command. The
offset direction is determined depending of the cutting pattern
regardless of the G41 or G42 mode.

Outer diameter/internal diameter cutting cycle (G90)

Tool nose radius center path Offset direction

0

Tool nose radius center path

Whole tool nose

8

4

57

3

End face cutting cycle (G94)

1

Whole tool nose

Programmed path

6

Whole
tool nose

2

Tool nose radius center path Offset direction

Tool nose radius center path

Whole tool nose

Whole tool nose

Programmed path

4

5

1

8

6

0

3

2

Whole
tool nose

7

- 47 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

Threading cycle (G92)

Tool nose radius compensation cannot be applied.

Differences between this CNC and the FANUC Series 16i/18i/21i

NOTE

This CNC is the same as the FANUC Series

16i/18i/21i in the offset direction, but differs from
the series in the tool nose radius center path.

- For this CNC
Cycle operations of a canned cycle are replaced

with G00 or G01. In the first block to move the
tool from the start point, start-up is performed.
In the last block to return the tool to the start
point, offset is canceled.

- For the FANUC Series 16i/18i/21i
This series differs from this CNC in operations in

the block to move the tool from the start point
and the last block to return it to the start point.
For details, refer to "FANUC Series 16i/18i/21i
Operator's Manual."

How compensation is applied for the FANUC Series 16i/18i/21i

G90 G94

Tool nose radius center path

4,8,3

5,0,7

4

5

0

8

3

7

Tool nose radius center path

4,8,3

5,0,7

4

5

0

8

3

7

1,6,2

Whole

4,5,1

tool nose

Programmed path

- 48 -

1

2

6

8,0,6

3,7,2

1,6,2

Whole
tool nose

Programmed path

1

4,5,1

2

6

8,0,6

3,7,2

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

4.1.6 Restrictions on Canned Cycles

Limitation

- Modal

Since data items X (U), Z (W), and R in a canned cycle are modal
values common to G90, G92, and G94. For this reason, if a new X
(U), Z (W), or R value is not specified, the previously specified value
is effective.
Thus, when the travel distance along the Z-axis does not vary as
shown in the program example below, a canned cycle can be repeated
only by specifying the travel distance along the X-axis.

Example

X axis

0

The cycle in the above figure is executed by the following

program:

N030 G90 U-8.0 W-66.0 F0.4;

N031 U-16.0;

N032 U-24.0;

N033 U-32.0;

66

4

8

12

Workpiece

16

The modal values common to canned cycles are cleared when a
one-shot G code other than G04 is specified.
Since the canned cycle mode is not canceled by specifying a one-shot
G code, a canned cycle can be performed again by specifying modal
values. If no modal values are specified, no cycle operations are
performed.
When G04 is specified, G04 is executed and no canned cycle is
performed.

- 49 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

- Block in which no move command is specified

In a block in which no move command is specified in the canned cycle
mode, a canned cycle is also performed. For example, a block
containing only EOB or a block in which none of the M, S, and T
codes, and move commands are specified is of this type of block.
When an M, S, or T code is specified in the canned cycle mode, the
corresponding M, S, or T function is executed together with the
canned cycle. If this is inconvenient, specify a group 01 G code
(G00 or G01) other than G90, G92, or G94 to cancel the canned cycle
mode, and specify an M, S, or T code, as in the program example
below. After the corresponding M, S, or T function has been
executed, specify the canned cycle again.

Example

N003 T0101;
:
:
N010 G90 X20.0 Z10.0 F0.2;
N011 G00 T0202; ← Cancels the canned cycle

mode.

N012 G90 X20.5 Z10.0;

- Plane selection command

Specify a plane selection command (G17, G18, or G19) before setting
a canned cycle or specify it in the block in which the first canned
cycle is specified.
If a plane selection command is specified in the canned cycle mode,
the command is executed, but the modal values common to canned
cycles are cleared.
If an axis which is not on the selected plane is specified, alarm
PS0330 is issued.

- Parallel axis

When G code system A is used, U, V, and W cannot be specified as a
parallel axis.

- 50 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

4.2 MULTIPLE REPETITIVE CYCLE (G70-G76)

The multiple repetitive cycle is canned cycles to make CNC
programming easy. For instance, the data of the finish work shape
describes the tool path for rough machining. And also, a canned
cycles for the threading is available.

NOTE

1 Explanatory figures in this section use the ZX plane

as the selected plane, diameter programming for
the X-axis, and radius programming for the Z-axis.
When radius programming is used for the X-axis,
change U/2 to U and X/2 to X.

2 A multiple repetitive cycle can be performed on any

plane (including parallel axes for plane definition).
When G-code system A is used, however, U, V,
and W cannot be set as a parallel axis.

- 51 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

4.2.1 Stock Removal in Turning (G71)

There are two types of stock removals in turning : Type I and II.
To use type II, the "multiple repetitive canned cycle 2" option function
is required.

Format

ZpXp plane

G71 U(∆d) R(e) ;
G71 P(ns) Q(nf) U(∆u) W(∆w) F(f ) S(s ) T(t ) ;
N (ns) ;
...
N (nf) ;

YpZp plane

G71 W(∆d) R(e) ;
G71 P(ns) Q(nf) V(∆w) W(∆u) F(f ) S(s ) T(t ) ;
N (ns) ;
...
N (nf) ;

XpYp plane

G71 V(∆d) R(e) ;
G71 P(ns) Q(nf) U(∆w) V(∆u) F(f ) S(s ) T(t ) ;
N (ns) ;
...
N (nf) ;

∆d : Depth of cut
The cutting direction depends on the direction AA'.

e : Escaping amount
This designation is modal and is not changed until the

ns : Sequence number of the first block for the program of

nf : Sequence number of the last block for the program of

∆u : Distance of the finishing allowance in the direction of

∆w : Distance of the finishing allowance in the direction of

f,s,t : Any F , S, or T function contained in blocks ns to nf in

The move command between A and B is specified in the
blocks from sequence number ns to nf.

This designation is modal and is not changed until the
other value is designated. Also this value can be
specified by the parameter (No. 5132), and the
parameter is changed by the program command.

other value is designated. Also this value can be
specified by the parameter (No. 5133), and the
parameter is changed by the program command.

finishing shape.

finishing shape.

the second axis on the plane (X-axis for the ZX plane)

the first axis on the plane (Z-axis for the ZX plane)

the cycle is ignored, and the F, S, or T function in this
G71 block is effective.

- 52 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

A

Unit

Depends on the increment

∆d

system for the reference
axis.
Depends on the increment

e

system for the reference
axis.

Depends on the increment

∆u

system for the reference
axis.

Depends on the increment

∆w

system for the reference
axis.

Diameter/radius

programming

Radius programming

Radius programming

Depends on
diameter/radius
programming for the
second axis on the plane.
Depends on
diameter/radius
programming for the first
axis on the plane.

Sign

Not

required

Not

required

Required

Required

(R)

B

(F)

45°

(R)

e

(F)

C

A

∆d

Explanation

- Operations

Target figure

’

+X

(F): Cutting feed
(R): Rapid traverse

+Z

Fig. 4.2.1 (a) Cutting path in stock removal in turning (type I)

e: Escaping amount

∆W

∆u/2

When a target figure passing through A, A', and B in this order is
given by a program, the specified area is removed by ∆d (depth of cut),
with the finishing allowance specified by ∆u/2 and ∆w left. After the
last cutting is performed in the direction of the second axis on the
plane (X-axis for the ZX plane), rough cutting is performed as
finishing along the target figure. After rough cutting as finishing, the
block next to the sequence block specified at Q is executed.

- 53 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

A

A

A

A

A

A

A

A

NOTE

1 While both ∆d and ∆u are specified by the same

address, the meanings of them are determined by
the presence of addresses P and Q.

2 The cycle machining is performed by G71

command with P and Q specification.

3 F, S, and T functions which are specified in the

move command between points A and B are
ineffective and those specified in G71 block or the
previous block are effective. M and second
auxiliary functions are treated in the same way as
F, S, and T functions.

4 When an option of constant surface speed control

is selected, G96 or G97 command specified in the
move command between points A and B are
ineffective, and that specified in G71 block or the
previous block is effective.

- Target figure
Patterns

The following four cutting patterns are considered. All of these
cutting cycles cut the workpiece with moving the tool in parallel to the
first axis on the plane (Z-axis for the ZX plane). The signs of ∆u and
∆w are as follows:

B

U(+)…W(+)

U(+)…W(-)

B

'

B

+X

U(-)…W (+)

+Z

'

'

'

U(-)…W (-)

Both linear and
circular interpolation
are possible

B

Fig. 4.2.1 (b) Four target figure patterns

- 54 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

Limitation

(1) For U(+), a figure for which a position higher than the cycle start

point is specified cannot be machined.

For U(-), a figure for which a position lower than the cycle start

point is specified cannot be machined.

(2) For type I, the figure must show monotone increase or decrease

along the first and second axes on the plane.

(3) For type II, the figure must show monotone increase or decrease

along the first axis on the plane.

- Start block

In the start block in the program for a target figure (block with
sequence number ns in which the path between A and A' is specified),
G00 or G01 must be specified. If it is not specified, alarm PS0065 is
issued.
When G00 is specified, cutting along path A-A' is performed in the
positioning mode. When G01 is specified, cutting along path A-A' is
performed in the linear interpolation mode.
In this start block, also select type I or II.

- Check functions

During cycle operation, whether the target figure shows monotone
increase or decrease is always checked.

NOTE

When tool nose radius compensation is applied,

the target figure to which compensation is applied
is checked.

The following checks can also be made.

Check Related parameter

Checks that a block with the sequence
number specified at address Q is contained
in the program before cycle operation.
Checks the target figure before cycle
operation.
(Also checks that a block with the sequence
number specified at address Q is contained.)

Enabled when bit 2 (QSR) of
parameter No. 5102 is set to

1.
Enabled when bit 2 (FCK) of
parameter No. 5104 is set to

1.

- 55 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

- Types I and II
Selection of type I or II

For G71, there are types I and II.
When the target figure has pockets, be sure to use type II.
Escaping operation after rough cutting in the direction of the first axis
on the plane (Z-axis for the ZX plane) differs between types I and II.
With type I, the tool escapes to the direction of 45 degrees. With
type II, the tool cuts the workpiece along the target figure. When the
target figure has no pockets, determine the desired escaping operation
and select type I or II.

NOTE

To use type II, the multiple repetitive canned cycle

II option is required.

Selecting type I or II

In the start block for the target figure (sequence number ns), select
type I or II.

(1) When type I is selected
Specify the second axis on the plane (X-axis for the ZX plane).

Do not specify the first axis on the plane (Z-axis for the ZX
plane).

(2) When type II is selected
Specify the second axis on the plane (X-axis for the ZX plane)

and first axis on the plane (Z-axis for the ZX plane).

When you want to use type II without moving the tool along the

first axis on the plane (Z-axis for the ZX plane), specify the
incremental programming with travel distance 0 (W0 for the ZX
plane).

- Type I

(1) In the block with sequence number ns, only the second axis on

the plane (X-axis (U-axis) for the ZX plane) must be specified.

Example

ZX plane
G71 V10.0 R5.0 ;

G71 P100 Q200....;

N100 X(U)_ ; (Specifies only the second axis on the plane.)
: ;
: ;
N200…………;

- 56 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

A

A

(2) The figure along path A'-B must show monotone increase or

decrease in the directions of both axes forming the plane (Z- and
X-axes for the ZX plane). It must not have any pocket as
shown in the figure below.

’

X

Z

Fig. 4.2.1 (c) Figure which does not show monotone increase or

No pockets are allowed.

decrease (type I)

CAUTION

If a figure does not show monotone change along

the first or second axis on the plane, alarm PS0064
or PS0329 is issued. If the movement does not
show monotone change, but is very small, and it
can be determined that the movement is not
dangerous, however, the permissible amount can
be specified in parameters Nos. 5145 and 5146 to
specify that the alarm is not issued in this case.

(3) The tool escapes to the direction of 45 degrees in cutting feed

after rough cutting.

45°

Escaping amount e (specified in the
command or parameter No. 5133)

Fig. 4.2.1 (d) Cutting in the direction of 45 degrees (type I)

(4) Immediately after the last cutting, rough cutting is performed as

finishing along the target figure. Bit 1 (RF1) of parameter No.
5105 can be set to 1 so that rough cutting as finishing is not
performed.

- 57 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

A

A

- Type II

(F)

B

(R)

(F)

(R)

(R)

(F)

C

d

∆

d

∆

Target figure

+X

(F): Cutting feed
(R): Rapid traverse

+Z

Fig. 4.2.1 (e) Cutting path in stock removal in turning (type II)

’

W

∆

u/2

∆

When a target figure passing through A, A', and B in this order is
given by the program for a target figure as shown in the figure, the
specified area is removed by ∆d (depth of cut), with the finishing
allowance specified by ∆u/2 and ∆w left. Type II differs from type I
in cutting the workpiece along the figure after rough cutting in the
direction of the first axis on the plane (Z-axis for the ZX plane).
After the last cutting, the tool returns to the start point specified in
G71 and rough cutting is performed as finishing along the target
figure, with the finishing allowance specified by ∆u/2 and ∆w left.

Type II differs from type I in the following points:
(1) In the block with sequence number ns, the two axes forming the

plane (X-axis (U-axis) and Z-axis (W-axis) for the ZX plane)
must be specified. When you want to use type II without
moving the tool along the Z-axis on the ZX plane in the first
block, specify W0.

Example

ZX plane
G71 V10.0 R5.0;

G71 P100 Q200.......;

N100 X(U)_ Z(W)_ ; (Specifies the two axes

forming the plane.)
: ;
: ;
N200…………;

- 58 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

(2) The figure need not show monotone increase or decrease in the

direction of the second axis on the plane (X-axis for the ZX
plane) and it may have concaves (pockets).

+X

10

+Z

. . .

Fig. 4.2.1 (f) Figure having pockets (type II)

3

2

1

The figure must show monotone change in the direction of the

first axis on the plane (Z-axis for the ZX plane), however. The
following figure cannot be machined.

Monotone change is not
observed along the Z-

+X

+Z

Fig. 4.2.1 (g) Figure which cannot be machined (type II)

axis.

CAUTION

For a figure along which the tool moves backward

along the first axis on the plane during cutting
operation (including a vertex in an arc command),
the cutting tool may contact the workpiece. For this
reason, for a figure which does not show monotone
change, alarm PS0064 or PS0329 is issued. If the
movement does not show monotone change, but is
very small, and it can be determined that the
movement is not dangerous, however, the
permissible amount can be specified in parameter
No. 5145 to specify that the alarm is not issued in
this case.

The first cut portion need not be vertical. Any figure is

permitted if monotone change is shown in the direction of the
first axis on the plane (Z-axis for the ZX plane).

- 59 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

r

+X

+Z

Fig. 4.2.1 (h) Figure which can be machined (type II)

(3) After turning, the tool cuts the workpiece along its figure and

escapes in cutting feed.

Escaping amount e (specified in the command o
parameter No. 5133)

Escaping after cutting

Depth of cut ∆d (specified in the
command or parameter No. 5132)

Fig. 4.2.1 (i) Cutting along the workpiece figure (type II)

The escaping amount after cutting (e) can be specified at address

R or set in parameter No. 5133.

When moving from the bottom, however, the tool escapes to the

direction of 45 degrees.

45°

e (specified in the command or

parameter No. 5133)

Bottom

Fig. 4.2.1 (j) Escaping from the bottom to the direction of 45 degrees

(4) When a position parallel to the first axis on the plane (Z-axis for

the ZX plane) is specified in a block in the program for the target
figure, it is assumed to be at the bottom of a pocket.

- 60 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

(5) After all rough cutting terminates along the first axis on the plane

(Z-axis for the ZX plane), the tool temporarily returns to the
cycle start point. At this time, when there is a position whose
height equals to that at the start point, the tool passes through the
point in the position obtained by adding depth of cut ∆d to the
position of the figure and returns to the start point.

Then, rough cutting is performed as finishing along the target

figure. At this time, the tool passes through the point in the
obtained position (to which depth of cut ∆d is added) when
returning to the start point.

Bit 2 (RF2) of parameter No. 5105 can be set to 1 so that rough

cutting as finishing is not performed.

Escaping operation after rough cutting
as finishing

Escaping operation after
rough cutting

{

Fig. 4.2.1 (k) Escaping operation when the tool returns to the start point

(type II)

Start point

{

Depth of cut ∆d

(6) Order and path for rough cutting of pockets
Rough cutting is performed in the following order.

(a) When the figure shows monotone decrease along the first

axis on the plane (Z-axis for the ZX plane)

Rough cutting is performed in the order <1>, <2>, and <3>
from the rightmost pocket.

<3>

+X

+Z

Fig. 4.2.1 (l) Rough cutting order in the case of monotone decrease

<2>

(type II)

<1>

- 61 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

•

(b) When the figure shows monotone increase along the first

axis on the plane (Z-axis for the ZX plane)

Rough cutting is performed in the order <1>, <2>, and <3> from
the leftmost pocket.

<1>

<2>

<3>

+X

+Z

Fig. 4.2.1 (m) Rough cutting order in the case of monotone increase

(type II)

The path in rough cutting is as shown below.

35

3

34

24

23

29

28

33

30

26

27

31

32

4

5

25

22

910

2

21

8

14

6

11

15

7

12

16

20

13

17

19

18

1

Fig. 4.2.1 (n) Cutting path for multiple pockets (type II)

The following figure shows how the tool moves after rough cutting for
a pocket in detail.

22

D

Cutting feed

g

21

20

19

Rapid traverse

Escaping from
the bottom

Fig. 4.2.1 (o) Details of motion after cutting for a pocket (type II)

- 62 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

Cuts the workpiece at the cutting feedrate and escapes to the direction
of 45 degrees. (Operation 19)
Then, moves to the height of point D in rapid traverse. (Operation

20)
Then, moves to the position the amount of g before point D.
(Operation 21)
Finally, moves to point D in cutting feed.
The clearance g to the cutting feed start position is set in parameter No.

5134.
For the last pocket, after cutting the bottom, the tool escapes to the
direction of 45 degrees and returns to the start point in rapid traverse.
(Operations 34 and 35)

CAUTION

1 This CNC differs from the FANUC Series

16i/18i/21i in cutting of a pocket.

The tool first cuts the nearest pocket to the start

point. After cutting of the pocket terminates, the
tool moves to the nearest but one pocket and starts
cutting.

2 When the figure has a pocket, generally specify a

value of 0 for ∆w (finishing allowance). Otherwise,
the tool may dig into the wall on one side.

- Tool nose radius compensation

When this cycle is specified in the tool nose radius compensation
mode, offset is temporarily canceled during movement to the start
point. Start-up is performed in the first block. Offset is temporarily
canceled again at the return to the cycle start point after termination of
cycle operation. Start-up is performed again according to the next
move command. This operation is shown in the figure below.

Start-up

Offset cancel

Cycle start point

z

Offset cancel

Start-up

- 63 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

A

A

A

A

A

A

This cycle operation is performed according to the figure determined
by the tool nose radius compensation path when the offset vector is 0
at start point A and start-up is performed in a block between path
A-A'.

B

Position between A-

Target figure program for
which tool nose radius
compensation is not applied

' in which start-up is

performed

+X

+Z

Fig. 4.2.1 (p) Path when tool nose radius compensation is applied

Tool nose center path when tool nose radius
compensation is applied with G42

’

B

’

Position between

+X

Target figure program for
which tool nose radius

+Z

compensation is not applied

Tool nose center path when tool
nose radius compensation is
applied with G42

-A' in which start-

up is performed

NOTE

To perform pocketing in the tool nose radius

compensation mode, specify the linear block A-A'
outside the workpiece and specify the figure of an
actual pocket. This prevents a pocket from being
dug.

- 64 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

4.2.2 Stock Removal in Facing (G72)

This cycle is the same as G71 except that cutting is performed by an
operation parallel to the second axis on the plane (X-axis for the ZX
plane).

Format

ZpXp plane

G72 W(∆d) R(e) ;
G72 P(ns) Q(nf) U(∆u) W(∆w) F(f ) S(s ) T(t ) ;
N (ns) ;
...
N (nf) ;

YpZp plane

G72 V(∆d) R(e) ;
G72 P(ns) Q(nf) V(∆w) W(∆u) F(f ) S(s ) T(t ) ;
N (ns) ;
...
N (nf) ;

XpYp plane

G72 U(∆d) R(e) ;
G72 P(ns) Q(nf) U(∆w) W(∆u) F(f ) S(s ) T(t ) ;
N (ns) ;
...
N (nf) ;

∆d : Depth of cut
The cutting direction depends on the direction AA'. This

designation is modal and is not changed until the other
value is designated. Also this value can be specified by
the parameter (No. 5132), and the parameter is changed

by the program command.
e : Escaping amount
This designation is modal and is not changed until the

other value is designated. Also this value can be

specified by the parameter (No. 5133), and the

parameter is changed by the program command.
ns : Sequence number of the first block for the program of

finishing shape.
nf : Sequence number of the last block for the program of

finishing shape.
∆u : Distance of the finishing allowance in the direction of the

second axis on the plane (X-axis for the ZX plane)
∆w : Distance of the finishing allowance in the direction of the

first axis on the plane (Z-axis for the ZX plane)
f,s,t : Any F , S, or T function contained in blocks ns to nf in

the cycle is ignored, and the F, S, or T function in this

G72 block is effective.

The move command between A and B is specified in the
blocks from sequence number ns to nf.

- 65 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

A

∆

A

Unit

Depends on the increment

∆d

∆u

∆w

system for the reference
axis.
Depends on the increment

e

system for the reference
axis.

Depends on the increment
system for the reference
axis.

Depends on the increment
system for the reference
axis.

'

Diameter/radius

programming

Radius programming

Radius programming

Depends on
diameter/radius
programming for the
second axis on the plane.
Depends on
diameter/radius
programming for the first
axis on the plane.

d

(F): Cutting feed
(R): Rapid traverse

C

Sign

Not

required

Not

required

Required

Required

(F)

e

(R)

Target figure

(F)

+X

B

+Z

Fig. 4.2.2 (q) Cutting path in stock removal in facing (type I)

Tool path

(R)

45°

∆u/2

∆w

- 66 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

A

A

A

A

A

A

A

A

Explanation

- Operations

When a target figure passing through A, A', and B in this order is
given by a program, the specified area is removed by ∆d (depth of cut),
with the finishing allowance specified by ∆u/2 and ∆w left.

NOTE

1 While both ∆d and ∆u are specified by the same

address, the meanings of them are determined by
the presence of addresses P and Q.

2 The cycle machining is performed by G72

command with P and Q specification.

3 F, S, and T functions which are specified in the

move command between points A and B are
ineffective and those specified in G72 block or the
previous block are effective. M and second
auxiliary functions are treated in the same way as
F, S, and T functions.

4 When an option of constant surface speed control

is selected, G96 or G97 command specified in the
move command between points A and B are
ineffective, and that specified in G72 block or the
previous block is effective.

- Target figure
Patterns

The following four cutting patterns are considered. All of these
cutting cycles cut the workpiece with moving the tool in parallel to the
second axis on the plane (X-axis for the ZX plane). The signs of ∆u
and ∆w are as follows:

+X

B

B

U(-)...W(+)...

'

'

U(+)...W(+)...

B

B

U(-)...W(-)...

'

'

U(+)...W (-)...

+Z

Both linear and circular

interpolation are possible

Fig. 4.2.2 (r) Signs of the values specified at U and W in stock removal

in facing

- 67 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

Limitation

(1) For W(+), a figure for which a position higher than the cycle start

point is specified cannot be machined.

For W(-), a figure for which a position lower than the cycle start

point is specified cannot be machined.

(2) For type I, the figure must show monotone increase or decrease

along the first and second axes on the plane.

(3) For type II, the figure must show monotone increase or decrease

along the second axis on the plane.

- Start block

In the start block in the program for a target figure (block with
sequence number ns in which the path between A and A' is specified),
G00 or G01 must be specified. If it is not specified, alarm PS0065 is
issued.
When G00 is specified, cutting along path A-A' is performed in the
positioning mode. When G01 is specified, cutting along path A-A' is
performed in the linear interpolation mode.
In this start block, also select type I or II.

- Check functions

During cycle operation, whether the target figure shows monotone
increase or decrease is always checked.

NOTE

When tool nose radius compensation is applied,

the target figure to which compensation is applied
is checked.

The following checks can also be made.

Check Related parameter

Checks that a block with the sequence
number specified at address Q is contained
in the program before cycle operation.
Checks the target figure before cycle
operation.
(Also checks that a block with the sequence
number specified at address Q is contained.)

Enabled when bit 2 (QSR)
of parameter No. 5102 is
set to 1.
Enabled when bit 2 (FCK)
of parameter No. 5104 is
set to 1.

- Types I and II
Selection of type I or II

For G72, there are types I and II.
When the target figure has pockets, be sure to use type II.
Escaping operation after rough cutting in the direction of the second
axis on the plane (X-axis for the ZX plane) differs between types I and
II. With type I, the tool escapes to the direction of 45 degrees.
With type II, the tool cuts the workpiece along the target figure.
When the target figure has no pockets, determine the desired escaping
operation and select type I or II.

- 68 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

Selecting type I or II

In the start block for the target figure (sequence number ns), select
type I or II.

(1) When type I is selected
Specify the first axis on the plane (Z-axis for the ZX plane). Do

not specify the second axis on the plane (X-axis for the ZX
plane).

(2) When type II is selected
Specify the second axis on the plane (X-axis for the ZX plane)

and first axis on the plane (Z-axis for the ZX plane).

When you want to use type II without moving the tool along the

second axis on the plane (X-axis for the ZX plane), specify the
incremental programming with travel distance 0 (U0 for the ZX
plane).

- Type I

G72 differs from G71 in the following points:

(1) G72 cuts the workpiece with moving the tool in parallel with the

second axis on the plane (X-axis on the ZX plane).

(2) In the start block in the program for a target figure (block with

sequence number ns), only the first axis on the plane (Z-axis
(W-axis) for the ZX plane) must be specified.

- Type II

G72 differs from G71 in the following points:

(1) G72 cuts the workpiece with moving the tool in parallel with the

second axis on the plane (X-axis on the ZX plane).

(2) The figure need not show monotone increase or decrease in the

direction of the first axis on the plane (Z-axis for the ZX plane)
and it may have concaves (pockets). The figure must show
monotone change in the direction of the second axis on the plane
(X-axis for the ZX plane), however.

(3) When a position parallel to the second axis on the plane (X-axis

for the ZX plane) is specified in a block in the program for the
target figure, it is assumed to be at the bottom of a pocket.

(4) After all rough cutting terminates along the second axis on the

plane (X-axis for the ZX plane), the tool temporarily returns to
the start point. Then, rough cutting as finishing is performed.

- Tool nose radius compensation

See the pages on which G71 is explained.

- 69 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

4.2.3 Pattern Repeating (G73)

This function permits cutting a fixed pattern repeatedly, with a pattern
being displaced bit by bit. By this cutting cycle, it is possible to
efficiently cut work whose rough shape has already been made by a
rough machining, forging or casting method, etc.

Format

ZpXp plane

G73 W(∆k) U(∆i) R(d) ;
G73 P(ns) Q(nf) U(∆u) W(∆w) F(f ) S(s ) T(t ) ;
N (ns) ;
...
N (nf) ;

YpZp plane

G73 V(∆k) W(∆i) R(d) ;
G73 P(ns) Q(nf) V(∆w) W(∆u) F(f ) S(s ) T(t ) ;
N (ns) ;
...
N (nf) ;

XpYp plane

G73 U(∆k) V(∆i) R(d) ;
G73 P(ns) Q(nf) U(∆w) V(∆u) F(f ) S(s ) T(t ) ;
N (ns) ;
...
N (nf) ;

∆i : Distance of escape in the direction of the second axis

This designation is modal and is not changed until the

∆k : Distance of escape in the direction of the first axis on

This designation is modal and is not changed until the

d : The number of division
This value is the same as the repetitive count for rough

ns : Sequence number of the first block for the program of

nf : Sequence number of the last block for the program of

The move command between A and B is specified in the
blocks from sequence number ns to nf.

on the plane (X-axis for the ZX plane)

other value is designated. Also this value can be
specified by the parameter No. 5135, and the
parameter is changed by the program command.

the plane (Z-axis for the ZX plane)

other value is designated. Also this value can be
specified by the parameter No. 5136, and the
parameter is changed by the program command.

cutting. This designation is modal and is not changed
until the other value is designated. Also, this value can
be specified by the parameter No. 5137, and the
parameter is changed by the program command.

finishing shape.

finishing shape.

- 70 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

A

∆

A

∆u : Distance of the finishing allowance in the direction of

the second axis on the plane (X-axis for the ZX plane)

∆w : Distance of the finishing allowance in the direction of

the first axis on the plane (Z-axis for the ZX plane)

f, s, t : Any F, S, and T function contained in the blocks

between sequence number "ns" and "nf" are ignored,
and the F, S, and T functions in this G73 block are
effective.

Unit

Depends on the increment

∆i

∆k

∆u

∆w

system for the reference
axis.
Depends on the increment
system for the reference
axis.

Depends on the increment
system for the reference
axis.

Depends on the increment
system for the reference
axis.

Radius programming Required

Radius programming Required

Depends on
diameter/radius
programming for the
second axis on the plane.
Depends on
diameter/radius
programming for the first
axis on the plane.

Diameter/radius

programming

Sign

Required

Required

w

∆k+∆

D

∆u/2

C

(R)

u/2

∆

(F): Cutting feed
(R): Rapid traverse

∆i+∆

u/2

+X

B

Target figure

+Z

(R)

(F)

∆w

'

w

Fig. 4.2.3 (s) Cutting path in pattern repeating

- 71 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

Explanation

- Operations

When a target figure passing through A, A', and B in this order is
given by a program, rough cutting is performed the specified number
of times, with the finishing allowance specified by ∆u/2 and ∆w left.

NOTE

1 While the values ∆i and ∆k, or ∆u and ∆w are

specified by the same address respectively, the
meanings of them are determined by the presence
of addresses P and Q.

2 The cycle machining is performed by G73

command with P and Q specification.

3 After cycle operation terminates, the tool returns to

point A.

4 F, S, and T functions which are specified in the

move command between points A and B are
ineffective and those specified in G73 block or the
previous block are effective. M and second
auxiliary functions are treated in the same way as
F, S, and T functions.

- Target figure
Patterns

As in the case of G71, there are four target figure patterns. Be
careful about signs of ∆u, ∆w, ∆i, and ∆k when programming this
cycle.

- Start block

In the start block in the program for the target figure (block with
sequence number ns in which the path between A and A' is specified),
G00 or G01 must be specified. If it is not specified, alarm PS0065 is
issued.
When G00 is specified, cutting along path A-A' is performed in the
positioning mode. When G01 is specified, cutting along path A-A' is
performed in the linear interpolation mode.

- Check function

The following check can be made.

Check Related parameter

Checks that a block with the sequence
number specified at address Q is contained
in the program before cycle operation.

Enabled when bit 2 (QSR)
of parameter No. 5102 is
set to 1.

- Tool nose radius compensation

Like G71, this cycle operation is performed according to the figure
determined by the tool nose radius compensation path when the offset
vector is 0 at start point A and start-up is performed in a block
between path A-A'.

- 72 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

4.2.4 Finishing Cycle (G70)

After rough cutting by G71, G72 or G73, the following command
permits finishing.

Format

G70 P(ns) Q(nf) ;

ns : Sequence number of the first block for the

program of finishing shape.

nf : Sequence number of the last block for the

program of finishing shape.

Explanation

- Operations

The blocks with sequence numbers ns to nf in the program for a target
figure are executed for finishing. The F, S, T, M, and second
auxiliary functions specified in the G71, G72, or G73 block are
ignored and the F, S, T, M, and second auxiliary functions specified in
the blocks with sequence numbers ns to nf are effective.
When cycle operation terminates, the tool is returned to the start point
in rapid traverse and the next G70 cycle block is read.

- Target figure
Check function

The following check can be made.

Check Related parameter

Checks that a block with the sequence
number specified at address Q is contained
in the program before cycle operation.

- Storing P and Q blocks

When rough cutting is executed by G71, G72, or G73, up to three
memory addresses of P and Q blocks are stored. By this, the blocks
indicated by P and Q are immediately found at execution of G70
without searching memory from the beginning for them. After some
G71, G72, and G73 rough cutting cycles are executed, finishing cycles
can be performed by G70 at a time. At this time, for the fourth and
subsequent rough cutting cycles, the cycle time is longer because
memory is searched for P and Q blocks.

Enabled when bit 2 (QSR)
of parameter No. 5102 is
set to 1.

- 73 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

Example

G71 P100 Q200 ...;
N100 ...;
...;
...;
N200 ...;
G71 P300 Q400 ...;
N300 ...;
...;
...;
N400 ...;
...;
...;
G70 P100 Q200 ; (Executed without a search for

the first to third cycles)

G70 P300 Q400 ; (Executed after a search for the

fourth and subsequent cycles)

NOTE

The memory addresses of P and Q blocks stored

during rough cutting cycles by G71, G72, and G73
are erased after execution of G70.

All stored memory addresses of P and Q blocks

are also erased by a reset.

- Return to the cycle start point

In a finishing cycle, after the tool cuts the workpiece to the end point
of the target figure, it returns to the cycle start point in rapid traverse.

NOTE

The tool returns to the cycle start point always in

the nonlinear positioning mode regardless of the
setting of bit 1 (LRP) of parameter No. 1401.

Before executing a finishing cycle for a target figure

with a pocket cut by G71 or G72, check that the
tool does not interfere with the workpiece when
returning from the end point of the target figure to
the cycle start point.

- Tool nose radius compensation

Like G71, this cycle operation is performed according to the figure
determined by the tool nose radius compensation path when the offset
vector is 0 at start point A and start-up is performed in a block
between path A-A'.

- 74 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

Example

Stock removal in facing (G72)

X axis

160

60

10

10

120

φ

10

80

20

190

2

7

40

φ

20

(Diameter designation for X axis, metric input)

Start point

2

88

110

Z axis

2

N010 G50 X220.0 Z190.0 ;
N011 G00 X176.0 Z132.0 ;
N012 G72 W7.0 R1.0 ;
N013 G72 P014 Q019 U4.0 W2.0 F0.3 S550 ;
N014 G00 Z56.0 S700 ;
N015 G01 X120.0 W14.0 F0.15 ;
N016 W10.0 ;
N017 X80.0 W10.0 ;
N018 W20.0 ;
N019 X36.0 W22.0 ;
N020 G70 P014 Q019 ;

Escaping amount: 1.0
Finishing allowance (4.0 in diameter in the X direction, 2.0 in the Z direction)

- 75 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

Pattern repeating (G73)

16

B

16

X axis

180

160

φ

φ

0

40

10

40

20

120

φ

220

10

80

φ

20

2

(Diameter designation, metric input)

N010 G50 X260.0 Z220.0 ;
N011 G00 X220.0 Z160.0 ;
N012 G73 U14.0 W14.0 R3 ;
N013 G73 P014 Q019 U4.0 W2.0 F0.3 S0180 ;
N014 G00 X80.0 W-40.0 ;
N015 G01 W-20.0 F0.15 S0600 ;
N016 X120.0 W-10.0;
N017 W-20.0 S0400 ;
N018 G02 X160.0 W-20.0 R20.0 ;
N019 G01 X180.0 W-10.0 S0280 ;
N020 G70 P014 Q019 ;

14

40

110

14

2

130

Z axis

- 76 -

B-63944EN-1/02 PROGRAMMING 4.FUNCTIONS TO SIMPLIFY PROGRAMMING

4.2.5 End Face Peck Drilling Cycle (G74)

This cycle enables chip breaking in outer diameter cutting. If the
second axis on the plane (X-axis (U-axis) for the ZX plane) and
address P are omitted, operation is performed only along the first axis
on the plane (Z-axis for the ZX plane), that is, a peck drilling cycle is
performed.

Format

G74R (e) ;
G74X(U)_ Z(W)_ P(∆i) Q(∆k) R(∆d) F (f ) ;

e : Return amount
This designation is modal and is not changed until

the other value is designated. Also this value can be
specified by the parameter No. 5139, and the
parameter is changed by the program command.

X_,Z_ : Coordinate of the second axis on the plane (X-axis

for the ZX plane) at point B and

Coordinate of the first axis on the plane (Z-axis for

the ZX plane) at point C

U_,W_ : Travel distance along the second axis on the plane

(U for the ZX plane) from point A to B

Travel distance along the first axis on the plane (W

for the ZX plane) from point A to C

∆i : Travel distance in the direction of the second axis on

the plane (X-axis for the ZX plane)

∆k : Depth of cut in the direction of the first axis on the

plane (Z-axis for the ZX plane)

∆d : Relief amount of the tool at the cutting bottom
f : Feedrate

Unit

Depends on the increment

e

system for the reference axis.
Depends on the increment

∆i

system for the reference axis.
Depends on the increment

∆k

system for the reference axis.
Depends on the increment

∆d

system for the reference axis.

NOTE

1 Normally, specify a positive value for ∆d. When X

(U) and ∆i are omitted, specify a value with the sign
indicating the direction in which the tool is to
escape.

2 No decimal point can be input for P(∆i) and Q(∆k).

Diameter/radius

programming

Radius programming

Radius programming

Radius programming

Radius programming NOTE 1

Sign

Not

required

Not

required

Not

required

- 77 -

4.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-1/02

∆k' ∆k

∆k

∆k

∆k

[0 < ∆k’ ≤ ∆k]

d

∆

C

(R)

Z

+X

Explanation

- Operations

A cycle operation of cutting by ∆k and return by e is repeated.
When cutting reaches point C, the tool escapes by ∆d. Then, the tool
returns in rapid traverse, moves to the direction of point B by ∆i, and
performs cutting again.

NOTE

1 While both e and ∆d are specified by the same

2 The cycle machining is performed by G74

- Tool nose radius compensation

Tool nose radius compensation cannot be applied.

A

∆i

(R)

(F)

∆i

∆i’

B

(R) ... Rapid traverse
(F) ... Cutting feed

U/2

[0 < ∆i’ ≤ ∆i]

X

(R)

(F)

W

(R)

(F)

(R)

e

(F)

(F)

(R)

+Z

Fig. 4.2.5 (a) Cutting path in end face peek drilling cycle

address, the meanings of them are determined by
specifying the X, Y, or Z axis. When the axis is
specified, ∆d is used.

command with specifying the axis.

- 78 -