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

s

-

FANUC Series 30*/300*/300*
FANUC Series 31*/310*/310*s-MODEL A5
FANUC Series 31*/310*/310*s-MODEL A
FANUC Series 32*/320*/320*s-MODEL A

MODEL A

Common to Lathe System/Machining Center System

USER’S MANUAL

(Volume 1 of 2)

B-63944EN/02

• No part of this manual may be reproduced in any form.

• All specifications and designs are subject to change without notice.

The export of this product is subject to the authorization of the government of the country

from where the product is exported.

In this manual we have tried as much as possible to describe all the various matters.

However, we cannot describe all the matters which must not be done, or which cannot be

done, because there are so many possibilities.

Therefore, matters which are not especially described as possible in this manual should be

regarded as ”impossible”.

This manual contains the program names or device names of other companies, some of

which are registered trademarks of respective owners. However, these names are not

followed by  or  in the main body.

B-63944EN/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/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/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/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/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/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/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/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/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/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/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/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/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/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/02 TABLE OF CONTENTS

TABLE OF CONTENTS

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

I. GENERAL

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

1.1 NOTES ON READING THIS MANUAL.......................................................... 8

1.2 NOTES ON VARIOUS KINDS OF DATA ...................................................... 8

II. PROGRAMMING

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

1.1 TOOL MOVEMENT ALONG WORKPIECE PARTS

FIGURE-INTERPOLATION ......................................................................... 12

1.2 FEED-FEED FUNCTION............................................................................. 14

1.3 PART DRAWING AND TOOL MOVEMENT................................................ 15

1.3.1 Reference Position (Machine-specific Position) ....................................................15

1.3.2 Coordinate System on Part Drawing and Coordinate System Specified by CNC -

Coordinate System .................................................................................................16

1.3.3 How to Indicate Command Dimensions for Moving the Tool (Absolute,

Incremental Commands) ........................................................................................22

1.4 CUTTING SPEED - SPINDLE FUNCTION.................................................. 25

1.5 SELECTION OF TOOL USED FOR VARIOUS MACHINING - TOOL

FUNCTION .................................................................................................. 26

1.6 COMMAND FOR MACHINE OPERATIONS - AUXILIARY FUNCTION ...... 27

1.7 PROGRAM CONFIGURATION ................................................................... 28

1.8 TOOL MOVEMENT RANGE - STROKE...................................................... 31

2 CONTROLLED AXES ........................................................................... 33

2.1 NUMBER OF CONTROLLED AXES ........................................................... 34

2.2 NAMES OF AXES .......................................................................................35

2.3 INCREMENT SYSTEM................................................................................ 36

2.4 MAXIMUM STROKE.................................................................................... 37

3 PREPARATORY FUNCTION (G FUNCTION) ...................................... 38

3.1 G CODE LIST IN THE MACHINING CENTER SYSTEM ............................ 40

3.2 G CODE LIST IN THE LATHE SYSTEM .................................................... 43

4 INTERPOLATION FUNCTIONS............................................................ 47

4.1 POSITIONING (G00) ................................................................................... 48

c-1

TABLE OF CONTENTS B-63944EN/02

4.2 SINGLE DIRECTION POSITIONING (G60) ................................................ 50

4.3 LINEAR INTERPOLATION (G01)................................................................ 53

4.4 CIRCULAR INTERPOLATION (G02, G03).................................................. 56

4.5 HELICAL INTERPOLATION (G02, G03) ..................................................... 62

4.6 HELICAL INTERPOLATION B (G02, G03).................................................. 64

4.7 SPIRAL INTERPOLATION, CONICAL INTERPOLATION (G02, G03)........ 65

4.8 POLAR COORDINATE INTERPOLATION (G12.1, G13.1) ......................... 73

4.9 CYLINDRICAL INTERPOLATION (G07.1) .................................................. 82

4.10 CUTTING POINT INTERPOLATION FOR CYLINDRICAL

INTERPOLATION (G07.1)........................................................................... 87

4.11 EXPONENTIAL INTERPOLATION (G02.3, G03.3) ..................................... 99

4.12 SMOOTH INTERPOLATION (G05.1) ........................................................ 107

4.13 NANO SMOOTHING ................................................................................. 111

4.14 NURBS INTERPOLATION (G06.2) ........................................................... 118

4.15 HYPOTHETICAL AXIS INTERPOLATION (G07) ...................................... 123

4.16 VARIABLE LEAD THREADING (G34)....................................................... 125

4.17 CIRCULAR THREADING (G35, G36) .......................................................126

4.18 SKIP FUNCTION (G31)............................................................................. 131

4.19 MULTI-STEP SKIP (G31) .......................................................................... 133

4.20 HIGH-SPEED SKIP SIGNAL (G31) ...........................................................134

4.21 THREE-DIMENSIONAL CIRCULAR INTERPOLATION............................ 135

5 FEED FUNCTIONS ............................................................................. 140

5.1 OVERVIEW ............................................................................................... 141

5.2 RAPID TRAVERSE ................................................................................... 143

5.3 CUTTING FEED ........................................................................................ 144

5.4 CUTTING FEEDRATE CONTROL ............................................................ 150

5.4.1 Exact Stop (G09, G61), Cutting Mode (G64), Tapping Mode (G63) ..................151

5.4.2 Automatic Corner Override ..................................................................................152

5.4.2.1 Automatic override for inner corners (G62).................................................... 152

5.4.2.2 Internal circular cutting feedrate change ......................................................... 154

5.5 DWELL ...................................................................................................... 155

6 REFERENCE POSITION.....................................................................157

6.1 REFERENCE POSITION RETURN........................................................... 158

6.2 FLOATING REFERENCE POSITION RETURN (G30.1)........................... 165

7 COORDINATE SYSTEM.....................................................................167

7.1 MACHINE COORDINATE SYSTEM.......................................................... 168

c-2

B-63944EN/02 TABLE OF CONTENTS

7.2 WORKPIECE COORDINATE SYSTEM .................................................... 170

7.2.1 Setting a Workpiece Coordinate System..............................................................170

7.2.2 Selecting a Workpiece Coordinate System ..........................................................173

7.2.3 Changing Workpiece Coordinate System ............................................................174

7.2.4 Workpiece Coordinate System Preset (G92.1).....................................................178

7.2.5 Addition of Workpiece Coordinate System Pair (G54.1 or G54) ........................181

7.2.6 Automatic Coordinate System Setting .................................................................183

7.2.7 Workpiece Coordinate System Shift ....................................................................184

7.3 LOCAL COORDINATE SYSTEM ..............................................................186

7.4 PLANE SELECTION.................................................................................. 188

8 COORDINATE VALUE AND DIMENSION .........................................189

8.1 ABSOLUTE AND INCREMENTAL PROGRAMMING................................ 190

8.2 INCH/METRIC CONVERSION (G20, G21) ............................................... 192

8.3 DECIMAL POINT PROGRAMMING .......................................................... 193

8.4 DIAMETER AND RADIUS PROGRAMMING ............................................195

8.5 DIAMETER AND RADIUS SETTING SWITCHING FUNCTION................ 196

9 SPINDLE SPEED FUNCTION (S FUNCTION) ...................................200

9.1 SPECIFYING THE SPINDLE SPEED WITH A CODE............................... 201

9.2 SPECIFYING THE SPINDLE SPEED VALUE DIRECTLY (S5-DIGIT

COMMAND) .............................................................................................. 201

9.3 CONSTANT SURFACE SPEED CONTROL (G96, G97) .......................... 202

9.4 SPINDLE POSITIONING FUNCTION .......................................................207

9.4.1 Spindle Orientation...............................................................................................208

9.4.2 Spindle Positioning ..............................................................................................209

9.4.3 Canceling Spindle Positioning .............................................................................211

9.5 SPINDLE SPEED FLUCTUATION DETECTION....................................... 213

10 TOOL FUNCTION (T FUNCTION) ......................................................218

10.1 TOOL SELECTION FUNCTION ................................................................ 219

10.2 TOOL MANAGEMENT FUNCTION........................................................... 221

10.3 TOOL MANAGEMENT EXTENSION FUNCTION ..................................... 240

10.3.1 Customization of Tool Management Data Display ..............................................240

10.3.2 Setting of Spindle Position / Standby Position Display .......................................245

10.3.3 Input of Customize Data with the Decimal Point.................................................247

10.3.4 Protection of Various Tool Information Items with the KEY Signal...................250

10.3.5 Selection of a Tool Life Count Period..................................................................250

10.3.6 Individual Data Screen .........................................................................................251

c-3

TABLE OF CONTENTS B-63944EN/02

10.3.7 Total Life Time Display for Tools of The Same Type.........................................251

10.4 TOOL MANAGEMENT FUNCTION OVERSIZE TOOLS SUPPORT ........252

11 AUXILIARY FUNCTION...................................................................... 254

11.1 AUXILIARY FUNCTION (M FUNCTION)................................................... 255

11.2 MULTIPLE M COMMANDS IN A SINGLE BLOCK.................................... 256

11.3 M CODE GROUPING FUNCTION ............................................................257

11.3.1 Setting an M Code Group Number Using the Setting Screen ..............................257

11.3.2 Setting an M Code Group Number Using a Program...........................................259

11.3.3 M Code Group Check Function ...........................................................................260

11.4 SECOND AUXILIARY FUNCTIONS (B CODES) ......................................261

12 PROGRAM MANAGEMENT ...............................................................264

12.1 FOLDERS.................................................................................................. 265

12.1.1 Folder Configuration ............................................................................................265

12.1.2 Folder Attributes...................................................................................................268

12.1.3 Default Folders .....................................................................................................269

12.2 FILES......................................................................................................... 270

12.2.1 File Name .............................................................................................................270

12.2.2 File Attributes.......................................................................................................272

12.3 RELATION WITH CONVENTIONAL FUNCTIONS.................................... 273

12.3.1 Relation with Folders ...........................................................................................273

12.3.2 Relation with File Names .....................................................................................275

12.3.3 Related Parameters ...............................................................................................277

13 PROGRAM CONFIGURATION...........................................................278

13.1 PROGRAM COMPONENTS OTHER THAN PROGRAM SECTIONS....... 280

13.2 PROGRAM SECTION CONFIGURATION ................................................ 283

13.3 SUBPROGRAM (M98, M99) ..................................................................... 291

14 FUNCTIONS TO SIMPLIFY PROGRAMMING ................................... 296

14.1 FIGURE COPY (G72.1, G72.2) ................................................................. 297

14.2 THREE-DIMENSIONAL COORDINATE CONVERSION........................... 305

15 COMPENSATION FUNCTION ............................................................316

15.1 TOOL LENGTH COMPENSATION (G43, G44, G49)................................ 317

15.1.1 Overview ..............................................................................................................317

15.1.2 G53, G28, G30, and G30.1 Commands in Tool Length Compensation Mode ....323

15.2 SCALING (G50, G51) ................................................................................ 325

15.3 PROGRAMMABLE MIRROR IMAGE (G50.1, G51.1) ............................... 335

c-4

B-63944EN/02 TABLE OF CONTENTS

15.4 TOOL AXIS DIRECTION TOOL LENGTH COMPENSATION................... 337

15.4.1 Control Point Compensation of Tool Length Compensation Along Tool Axis...343

16 CUSTOM MACRO............................................................................... 348

16.1 VARIABLES............................................................................................... 349

16.2 SYSTEM VARIABLES ............................................................................... 356

16.3 ARITHMETIC AND LOGIC OPERATION .................................................. 411

16.4 INDIRECT AXIS ADDRESS SPECIFICATION .......................................... 419

16.5 MACRO STATEMENTS AND NC STATEMENTS..................................... 421

16.6 BRANCH AND REPETITION..................................................................... 422

16.6.1 Unconditional Branch (GOTO Statement)...........................................................422

16.6.2 GOTO Statement Using Stored Sequence Numbers ............................................423

16.6.3 Conditional Branch (IF Statement) ......................................................................425

16.6.4 Repetition (WHILE Statement)............................................................................427

16.7 MACRO CALL ...........................................................................................430

16.7.1 Simple Call (G65) ................................................................................................431

16.7.2 Modal Call: Call After the Move Command (G66) .............................................442

16.7.3 Modal Call: Each Block Call (G66.1) .................................................................447

16.7.4 Macro Call Using a G Code .................................................................................450

16.7.5 Macro Call Using a G Code (Specification of Multiple Definitions)...................452

16.7.6 Macro Call Using a G Code with a Decimal Point (Specification of Multiple

Definitions)...........................................................................................................453

16.7.7 Macro Call Using an M Code...............................................................................454

16.7.8 Macro Call Using an M Code (Specification of Multiple Definitions)................456

16.7.9 Subprogram Call Using an M Code .....................................................................457

16.7.10 Subprogram Call Using an M Code (Specification of Multiple Definitions).......458

16.7.11 Subprogram Calls Using a T Code .......................................................................459

16.7.12 Subprogram Calls Using an S Code .....................................................................460

16.7.13 Subprogram Calls Using a Secondary Auxiliary Function ..................................461

16.7.14 Subprogram Call Using a Specific Address .........................................................462

16.8 PROCESSING MACRO STATEMENTS ................................................... 466

16.9 REGISTERING CUSTOM MACRO PROGRAMS .....................................468

16.10 CODES AND RESERVED WORDS USED IN CUSTOM MACROS ......... 469

16.11 EXTERNAL OUTPUT COMMANDS.......................................................... 471

16.12 RESTRICTIONS ........................................................................................ 475

16.13 INTERRUPTION TYPE CUSTOM MACRO............................................... 477

16.13.1 Specification Method ...........................................................................................478

16.13.2 Details of Functions..............................................................................................479

c-5

TABLE OF CONTENTS B-63944EN/02

17 REAL-TIME CUSTOM MACRO ..........................................................489

17.1 TYPES OF REAL TIME MACRO COMMANDS......................................... 493

17.1.1 Modal Real Time Macro Command / One-shot Real Time Macro Command.....493

17.2 VARIABLES............................................................................................... 500

17.2.1 Variables Dedicated To Real Time Custom Macros ............................................501

17.2.1.1 System variables.............................................................................................. 501

17.2.1.2 Real time macro variables (RTM variables)................................................... 503

17.2.2 Custom Macro Variables......................................................................................505

17.2.2.1 System variables.............................................................................................. 505

17.2.2.2 Local variables................................................................................................. 506

17.3 ARITHMETIC AND LOGICAL OPERATION.............................................. 507

17.4 CONTROL ON REAL TIME MACRO COMMANDS ..................................509

17.4.1 Conditional Branch (ZONCE Statement).............................................................510

17.4.2 Condition Transition (ZEDGE Statement)...........................................................511

17.4.3 Repetition (ZWHILE Statement) .........................................................................512

17.4.4 Multi-statement (ZDO...ZEND Statement) ..........................................................513

17.5 MACRO CALL ...........................................................................................516

17.6 OTHERS.................................................................................................... 518

17.7 AXIS CONTROL COMMAND .................................................................... 519

17.8 NOTES ...................................................................................................... 532

17.9 LIMITATION .............................................................................................. 534

18 PROGRAMMABLE PARAMETER INPUT (G10)................................536

19 HIGH-SPEED CUTTING FUNCTIONS................................................ 539

19.1 AI CONTOUR CONTROL FUNCTION I AND AI CONTOUR CONTROL

FUNCTION II (G05.1) ................................................................................ 540

19.2 JERK CONTROL ....................................................................................... 557

19.2.1 Speed Control with Change of Acceleration on Each Axis..................................557

19.2.2 Look-Ahead Smooth Bell-Shaped Acceleration/Deceleration before

Interpolation .........................................................................................................560

19.3 OPTIMUM TORQUE ACCELERATION/DECELERATION........................ 562

20 AXIS CONTROL FUNCTIONS............................................................574

20.1 AXIS SYNCHRONOUS CONTROL........................................................... 575

20.1.1 Axis Configuration for Axis Synchronous Control..............................................576

20.1.2 Synchronous Error Compensation........................................................................579

20.1.3 Synchronous Establishment .................................................................................581

20.1.4 Automatic Setting for Grid Position Matching ....................................................585

20.1.5 Synchronous Error Check ....................................................................................586

c-6

B-63944EN/02 TABLE OF CONTENTS

20.1.6 Methods of Alarm Recovery by Synchronous Error Check.................................588

20.1.7 Axis Synchronous Control Torque Difference Alarm..........................................590

20.2 POLYGON TURNING (G50.2, G51.2)....................................................... 593

20.3 ROTARY AXIS ROLL-OVER..................................................................... 599

20.3.1 Rotary Axis Roll-over ..........................................................................................599

20.3.2 Rotary Axis Control .............................................................................................600

20.4 ANGULAR AXIS CONTROL...................................................................... 601

20.5 TOOL RETRACT AND RECOVER............................................................ 611

20.6 ELECTRIC GEAR BOX ............................................................................. 616

20.6.1 Electric Gear Box .................................................................................................616

20.6.2 Electronic Gear Box Automatic Phase Synchronization......................................625

20.6.3 Skip Function for EGB Axis ................................................................................630

20.6.4 Electronic Gear Box 2 Pair...................................................................................632

20.6.4.1 Specification method (G80.5, G81.5).............................................................. 632

20.6.4.2 Description of commands compatible with those for a hobbing machine

(G80, G81)....................................................................................................... 635

20.6.4.3 Controlled axis configuration example............................................................ 639

20.6.4.4 Sample programs ............................................................................................. 640

20.6.4.5 Synchronization ratio specification range........................................................ 645

20.6.4.6 Retract function ............................................................................................... 649

21 5-AXIS MACHINING FUNCTION ........................................................650

21.1 TOOL CENTER POINT CONTROL FOR 5-AXIS MACHINING................. 651

21.2 TILTED WORKING PLANE COMMAND ................................................... 705

21.3 INCLINED ROTARY AXIS CONTROL ...................................................... 731

21.4 CUTTER COMPENSATION FOR 5-AXIS MACHINING............................ 735

21.4.1 Cutter Compensation in Tool Rotation Type Machine ........................................738

21.4.1.1 Tool side offset ................................................................................................ 739

21.4.1.2 Leading edge offset ......................................................................................... 759

21.4.1.3 Tool tip position (cutting point) command ...................................................... 765

21.4.2 Cutter Compensation in Table Rotation Type Machine.......................................769

21.4.3 Cutter Compensation in Mixed-Type Machine....................................................777

21.4.4 Interference Check and Interference Avoidance ..................................................784

21.4.5 Restrictions...........................................................................................................788

21.4.5.1 Restrictions common to machine configurations............................................. 788

21.4.5.2 Restriction on tool rotation type ...................................................................... 791

21.4.5.3 Restriction on machine configurations having table rotation axes (table

rotation type and mixed-type).......................................................................... 792

21.4.6 Examples ..............................................................................................................796

c-7

TABLE OF CONTENTS B-63944EN/02

22 MUITI-PATH CONTROL FUNCTION.................................................. 801

22.1 OVERVIEW ............................................................................................... 802

22.2 WAITING FUNCTION FOR PATHS ..........................................................804

22.3 COMMON MEMORY BETWEEN EACH PATH......................................... 810

22.4 SPINDLE CONTROL BETWEEN EACH PATH......................................... 812

22.5 SYNCHRONOUS CONTROL, MIXTURE CONTROL, AND

SUPERPOSITION CONTROL................................................................... 813

III. OPERATION

1 GENERAL ...........................................................................................819

1.1 MANUAL OPERATION.............................................................................. 820

1.2 TOOL MOVEMENT BY PROGRAMING - AUTOMATIC OPERATION .....822

1.3 AUTOMATIC OPERATION ....................................................................... 824

1.4 TESTING A PROGRAM ............................................................................ 826

1.4.1 Check by Running the Machine ...........................................................................826

1.4.2 How to View the Position Display Change without Running the Machine .........828

1.5 EDITING A PROGRAM ............................................................................. 829

1.6 DISPLAYING AND SETTING DATA.......................................................... 830

1.7 DISPLAY ................................................................................................... 833

1.7.1 Program Display...................................................................................................833

1.7.2 Current Position Display ......................................................................................834

1.7.3 Alarm Display ......................................................................................................835

1.7.4 Parts Count Display, Run Time Display ..............................................................835

2 OPERATIONAL DEVICES..................................................................836

2.1 SETTING AND DEISPLAY UNITS ............................................................ 837

2.1.1 7.2" LCD CNC Display Panel..............................................................................838

2.1.2 8.4" LCD CNC Display Panel..............................................................................838

2.1.3 10.4" LCD CNC Display Panel............................................................................839

2.1.4 12.1" LCD CNC Display Panel............................................................................840

2.1.5 15" LCD CNC Display Panel...............................................................................840

2.1.6 Standard MDI Unit (ONG Key)...........................................................................841

2.1.7 Standard MDI Unit (QWERTY Key)...................................................................842

2.1.8 Small MDI Unit (ONG Key) ................................................................................843

2.2 OPERATIONAL DEVICES......................................................................... 844

2.3 FUNCTION KEYS AND SOFT KEYS ........................................................ 847

2.3.1 General Screen Operations ...................................................................................848

2.3.2 Function Keys ......................................................................................................850

c-8

B-63944EN/02 TABLE OF CONTENTS

2.3.3 Soft Keys ..............................................................................................................851

2.3.4 Key Input and Input Buffer ..................................................................................861

2.3.5 Warning Messages ...............................................................................................862

2.4 EXTERNAL I/O DEVICES ......................................................................... 863

2.5 POWER ON/OFF....................................................................................... 865

2.5.1 Turning on the Power ...........................................................................................865

2.5.2 Power Disconnection............................................................................................866

3 MANUAL OPERATION....................................................................... 867

3.1 MANUAL REFERENCE POSITION RETURN........................................... 868

3.2 JOG FEED (JOG)...................................................................................... 870

3.3 INCREMENTAL FEED .............................................................................. 872

3.4 MANUAL HANDLE FEED.......................................................................... 874

3.5 MANUAL ABSOLUTE ON AND OFF......................................................... 877

3.6 RIGID TAPPING BY MANUAL HANDLE................................................... 883

3.7 MANUAL NUMERICAL COMMAND.......................................................... 886

3.8 MANUAL FEED FOR 5-AXIS MACHINING............................................... 895

3.8.1 Tool Axis Direction Handle Feed / Tool Axis Direction JOG Feed / Tool Axis

Direction Incremental Feed ..................................................................................896

3.8.2 Tool Axis Right-Angle Direction Handle Feed / Tool Axis Right-Angle

Direction JOG Feed / Tool Axis Right-Angle Direction Incremental Feed.........898

3.8.3 Tool Tip Center Rotation Handle Feed / Tool Tip Center Rotation JOG Feed /

Tool Tip Center Rotation Incremental Feed.........................................................903

3.8.4 Table Vertical Direction Handle Feed / Table Vertical Direction JOG Feed /

Table Vertical Direction Incremental Feed ..........................................................906

3.8.5 Table Horizontal Direction Handle Feed / Table Horizontal Direction JOG Feed /

Table Horizontal Direction Incremental Feed......................................................908

3.9 DISTANCE CODED LINEAR SCALE INTERFACE................................... 912

3.9.1 Procedure for Reference Position Establishment .................................................912

3.9.2 Reference Position Return ....................................................................................914

3.9.3 Distance Coded Rotary Encoder ..........................................................................914

3.9.4 Axis Synchronization Control..............................................................................915

3.9.5 Axis Control by PMC...........................................................................................916

3.9.6 Angular Axis Control ...........................................................................................917

3.9.7 Note ....................................................................................................................917

3.10 LINEAR SCALE WITH DISTANCE-CODED REFERENCE MARKS

(SERIAL) ................................................................................................... 919

c-9

TABLE OF CONTENTS B-63944EN/02

4 AUTOMATIC OPERATION .................................................................925

4.1 MEMORY OPERATION ............................................................................ 926

4.2 MDI OPERATION ...................................................................................... 929

4.3 DNC OPERATION..................................................................................... 934

4.4 EXTERNAL SUBPROGRAM CALL (M198)............................................... 936

4.5 MANUAL HANDLE INTERRUPTION ........................................................ 939

4.6 MIRROR IMAGE........................................................................................ 946

4.7 PROGRAM RESTART .............................................................................. 948

4.8 TOOL RETRACT AND RECOVER............................................................ 962

4.8.1 Retract ..................................................................................................................966

4.8.2 Withdrawal ...........................................................................................................967

4.8.3 Return ...................................................................................................................967

4.8.4 Repositioning .......................................................................................................968

4.8.5 Tool Retract and Return for Threading ................................................................969

4.8.6 Operation Procedure for a Canned Cycle for Drilling..........................................972

5 TEST OPERATION ............................................................................. 974

5.1 MACHINE LOCK AND AUXILIARY FUNCTION LOCK ............................. 975

5.2 FEEDRATE OVERRIDE............................................................................ 977

5.3 RAPID TRAVERSE OVERRIDE................................................................ 978

5.4 DRY RUN .................................................................................................. 979

5.5 SINGLE BLOCK ........................................................................................980

6 SAFETY FUNCTIONS.........................................................................982

6.1 EMERGENCY STOP................................................................................. 983

6.2 OVERTRAVEL........................................................................................... 984

6.3 STORED STROKE CHECK....................................................................... 986

6.4 STROKE LIMIT CHECK BEFORE MOVE ................................................. 991

6.5 WRONG OPERATION PREVENTION FUNCTIONS ................................994

6.5.1 Functions that are Used When Data is Set ...........................................................995

6.5.1.1 Input data range check..................................................................................... 996

6.5.1.2 Confirmation of incremental input .................................................................. 998

6.5.1.3 Prohibition of the absolute input by the soft key ............................................. 999

6.5.1.4 Confirmation of the deletion of the program................................................. 1000

6.5.1.5 Confirmation of the deletion of all data......................................................... 1001

6.5.1.6 Confirmation of a data update during the data setting process...................... 1002

6.5.2 Functions that are Used when the Program is Executed ....................................1003

6.5.2.1 Display of updated modal information .......................................................... 1004

6.5.2.2 Start check signal........................................................................................... 1005

6.5.2.3 Axis status display ......................................................................................... 1006

c-10

B-63944EN/02 TABLE OF CONTENTS

6.5.2.4 Confirmation of the start from a middle block .............................................. 1007

6.5.2.5 Data range check ........................................................................................... 1008

6.5.2.6 Maximum incremental value check............................................................... 1009

6.5.3 Setting Screen.....................................................................................................1010

6.5.3.1 Operation confirmation function setting screen............................................. 1011

6.5.3.2 Tool offset range setting screen..................................................................... 1013

6.5.3.3 Workpiece origin offset range setting screen ................................................ 1018

6.5.3.4 Y-axis tool offset range setting screen........................................................... 1020

6.5.3.5 Workpiece shift range setting screen ............................................................. 1022

7 ALARM AND SELF-DIAGNOSIS FUNCTIONS................................ 1024

7.1 ALARM DISPLAY .................................................................................... 1025

7.2 ALARM HISTORY DISPLAY ...................................................................1027

7.3 CHECKING BY SELF-DIAGNOSIS SCREEN ......................................... 1028

8 DATA INPUT/OUTPUT ..................................................................... 1029

8.1 INPUT/OUTPUT ON EACH SCREEN ..................................................... 1030

8.1.1 Inputting and Outputting a Program...................................................................1031

8.1.1.1 Inputting a program ....................................................................................... 1031

8.1.1.2 Outputting a program..................................................................................... 1032

8.1.2 Inputting and Outputting Parameters..................................................................1033

8.1.2.1 Inputting parameters ...................................................................................... 1033

8.1.2.2 Outputting parameters ................................................................................... 1034

8.1.3 Inputting and Outputting Offset Data.................................................................1035

8.1.3.1 Inputting offset data....................................................................................... 1035

8.1.3.2 Outputting offset data .................................................................................... 1036

8.1.4 Inputting and Outputting Pitch Error Compensation Data .................................1041

8.1.4.1 Inputting pitch error compensation data ........................................................ 1041

8.1.4.2 Outputting pitch error compensation data ..................................................... 1042

8.1.4.3 Input/output format of pitch error compensation data ................................... 1043

8.1.5 Inputting and Outputting Three-dimensional Error Compensation Data ...........1044

8.1.5.1 Inputting three-dimensional error compensation data ................................... 1044

8.1.5.2 Outputting three-dimensional error compensation data................................. 1045

8.1.5.3 Input/output format of three-dimensional error compensation data .............. 1046

8.1.6 Inputting and Outputting Custom Macro Common Variables ...........................1048

8.1.6.1 Inputting custom macro common variables................................................... 1048

8.1.6.2 Outputting custom macro common variables ................................................ 1049

8.1.7 Inputting and Outputting Workpiece Coordinates System Data ........................1051

8.1.7.1 Inputting workpiece coordinate system data.................................................. 1051

8.1.7.2 Outputting workpiece coordinate system data............................................... 1052

8.1.8 Inputting and Outputting Operation History Data..............................................1053

8.1.8.1 Outputting operation history data .................................................................. 1053

c-11

TABLE OF CONTENTS B-63944EN/02

8.1.9 Inputting and Outputting Tool Management Data .............................................1054

8.1.9.1 Inputting tool management data ....................................................................1054

8.1.9.2 Outputting tool management data.................................................................. 1055

8.1.9.3 Inputting magazine data................................................................................. 1056

8.1.9.4 Outputting magazine data .............................................................................. 1057

8.1.9.5 Inputting tool life status name data................................................................ 1058

8.1.9.6 Outputting tool life status name data ............................................................. 1059

8.1.9.7 Inputting name data of customize data .......................................................... 1060

8.1.9.8 Outputting name data of customize data........................................................ 1061

8.1.9.9 Inputting customize data displayed as tool management data ....................... 1062

8.1.9.10 Outputting customize data displayed as tool management data..................... 1063

8.1.9.11 Inputting spindle waiting position name data ................................................ 1064

8.1.9.12 Outputting spindle waiting position name data ............................................. 1065

8.1.9.13 Inputting decimal point position data of customize data ...............................1066

8.1.9.14 Outputting decimal point position data of customize data............................. 1067

8.1.9.15 Inputting tool geometry data.......................................................................... 1068

8.1.9.16 Outputting tool geometry data....................................................................... 1069

8.2 INPUT/OUTPUT ON THE ALL IO SCREEN............................................ 1070

8.2.1 Inputting/Outputting a Program .........................................................................1071

8.2.2 Inputting and Outputting Parameters..................................................................1072

8.2.3 Inputting and Outputting Offset Data.................................................................1073

8.2.4 Inputting/Outputting Pitch Error Compensation Data........................................1074

8.2.5 Inputting/Outputting Custom Macro Common Variables ..................................1076

8.2.6 Inputting and Outputting Workpiece Coordinates System Data ........................1077

8.2.7 Inputting and Outputting Operation History Data..............................................1078

8.2.8 Inputting and Outputting Tool Management Data .............................................1079

8.2.9 File Format and Error Messages.........................................................................1083

8.3 EMBEDDED ETHERNET OPERATIONS................................................ 1084

8.3.1 FTP File Transfer Function ................................................................................1084

9 CREATING PROGRAMS..................................................................1088

9.1 CREATING PROGRAMS USING THE MDI PANEL................................ 1089

9.2 AUTOMATIC INSERTION OF SEQUENCE NUMBERS ......................... 1090

9.3 CREATING PROGRAMS IN TEACH IN MODE (PLAYBACK) ................ 1092

10 EDITING PROGRAMS ...................................................................... 1095

10.1 EDIT DISABLE ATTRIBUTE.................................................................... 1096

10.2 INSERTING, ALTERING AND DELETING A WORD .............................. 1097

10.2.1 Word Search .......................................................................................................1098

10.2.2 Heading a Program.............................................................................................1100

10.2.3 Inserting a Word.................................................................................................1101

c-12

B-63944EN/02 TABLE OF CONTENTS

10.2.4 Altering a Word..................................................................................................1102

10.2.5 Deleting a Word .................................................................................................1103

10.3 DELETING BLOCKS ............................................................................... 1104

10.3.1 Deleting a Block.................................................................................................1104

10.3.2 Deleting Multiple Blocks ...................................................................................1105

10.4 PROGRAM SEARCH .............................................................................. 1106

10.5 SEQUENCE NUMBER SEARCH ............................................................ 1107

10.6 DELETING PROGRAMS......................................................................... 1109

10.6.1 Deleting One Program........................................................................................1109

10.6.2 Deleting All Programs........................................................................................1109

10.7 EDITING OF CUSTOM MACROS ........................................................... 1110

10.8 PASSWORD FUNCTION ........................................................................ 1111

10.9 EDITING PROGRAM CHARACTERS ..................................................... 1114

10.9.1 Available Keys ...................................................................................................1118

10.9.2 Input Mode .........................................................................................................1119

10.9.3 Line Number Display .........................................................................................1119

10.9.4 Search .................................................................................................................1120

10.9.5 Replacement .......................................................................................................1121

10.9.6 Reversing Edit Operations (Undo Function)......................................................1122

10.9.7 Selection .............................................................................................................1122

10.9.8 Copy ..................................................................................................................1123

10.9.9 Deletion ..............................................................................................................1123

10.9.10 Paste 1123

10.9.11 Saving.................................................................................................................1123

10.9.12 Creation ..............................................................................................................1124

10.9.13 Line Number Search...........................................................................................1124

10.10 PROGRAM COPY FUNCTION................................................................ 1125

10.11 KEYS AND PROGRAM ENCRYPTION................................................... 1127

11 PROGRAM MANAGEMENT .............................................................1131

11.1 SELECTING A DEVICE........................................................................... 1132

11.1.1 Selecting a Memory Card Program as a Device.................................................1133

11.2 CREATING A FOLDER ........................................................................... 1139

11.3 RENAMING A FOLDER .......................................................................... 1140

11.4 CHANGING FOLDER ATTRIBUTES....................................................... 1141

11.5 DELETING A FOLDER............................................................................ 1142

11.6 SELECTING A DEFAULT FOLDER ........................................................ 1143

11.7 RENAMING A FILE .................................................................................1144

c-13

TABLE OF CONTENTS B-63944EN/02

11.8 DELETING A FILE................................................................................... 1145

11.9 CHANGING FILE ATTRIBUTES.............................................................. 1146

11.10 SELECTING A MAIN PROGRAM............................................................ 1147

11.11 MAKING A PROGRAM COMPACT......................................................... 1148

12 SETTING AND DISPLAYING DATA................................................. 1149

12.1 SCREENS DISPLAYED BY FUNCTION KEY ....................................... 1157

12.1.1 Position Display in the Workpiece Coordinate System .....................................1158

12.1.2 Position Display in the Relative Coordinate System..........................................1160

12.1.3 Overall Position Display ....................................................................................1163

12.1.4 Workpiece Coordinate System Preset ................................................................1165

12.1.5 Actual Feedrate Display .....................................................................................1166

12.1.6 Display of Run Time and Parts Count................................................................1168

12.1.7 Setting the Floating Reference Position .............................................................1170

12.1.8 Operating Monitor Display ................................................................................1171

12.1.9 Display of Manual Feed for 5-axis Machining (Tool Tip Coordinates, Number

of Pulses, Machine Axis Move Amount) ...........................................................1174

12.2 SCREENS DISPLAYED BY FUNCTION KEY ....................................... 1178

12.2.1 Program Contents Display..................................................................................1179

12.2.2 Editing a Program...............................................................................................1180

12.2.3 Program Screen for MDI Operation...................................................................1182

12.2.4 Program Folder Screen.......................................................................................1183

12.2.5 Next Block Display Screen ................................................................................1184

12.2.6 Program Check Screen .......................................................................................1185

12.2.7 Background Editing............................................................................................1186

12.2.8 Stamping the Machining Time...........................................................................1192

12.3 SCREENS DISPLAYED BY FUNCTION KEY ....................................... 1202

12.3.1 Displaying and Entering Setting Data ................................................................1203

12.3.2 Sequence Number Comparison and Stop...........................................................1206

12.3.3 Displaying and Setting Run Time, Parts Count, and Time ................................1208

12.3.4 Displaying and Setting the Workpiece Origin Offset Value ..............................1211

12.3.5 Direct Input of Workpiece Origin Offset value measured .................................1212

12.3.6 Displaying and Setting Custom Macro Common Variables ..............................1214

12.3.7 Displaying and Setting Real Time Custom Macro Data ....................................1216

12.3.8 Displaying and Setting the Software Operator's Panel.......................................1218

12.3.9 Setting and Displaying Tool Management Data ................................................1221

12.3.9.1 Displaying and setting magazine screen........................................................ 1221

12.3.9.2 Displaying and setting tool management screen............................................ 1223

c-14

B-63944EN/02 TABLE OF CONTENTS

12.3.9.3 Each tool data screen .....................................................................................1230

12.3.9.4 Displaying the total life of tools of the same type .........................................1233

12.3.9.5 Tool geometry data screen............................................................................. 1238

12.3.10 Displaying and Switching the Display Language ..............................................1243

12.3.11 Protection of Data at Eight Levels......................................................................1245

12.3.11.1 Operation level setting................................................................................... 1245

12.3.11.2 Password modification................................................................................... 1247

12.3.11.3 Protection level setting .................................................................................. 1249

12.3.11.4 Setting the change protection level and output protection level of a

program.......................................................................................................... 1253

12.3.12 Precision Level Selection ...................................................................................1255

12.4 SCREENS DISPLAYED BY FUNCTION KEY ....................................... 1256

12.4.1 Displaying and Setting Parameters.....................................................................1257

12.4.2 Displaying and Setting Pitch Error Compensation Data ....................................1260

12.4.3 Displaying and Setting Three-Dimensional Error Compensation Data .............1263

12.4.4 Servo Parameters................................................................................................1267

12.4.5 Servo Tuning ......................................................................................................1268

12.4.6 Spindle Setting ...................................................................................................1269

12.4.7 Spindle Tuning ...................................................................................................1270

12.4.8 Spindle Monitor..................................................................................................1271

12.4.9 Color Setting Screen...........................................................................................1272

12.4.10 Machining Parameter Tuning .............................................................................1275

12.4.11 Displaying Memory Data ...................................................................................1283

12.4.12 Parameter Tuning Screen ...................................................................................1285

12.4.12.1 Displaying the menu screen and selecting a menu item ................................ 1285

12.4.12.2 Parameter tuning screen (system setting) ...................................................... 1289

12.4.12.3 Parameter tuning screen (axis setting)........................................................... 1291

12.4.12.4 Displaying and setting the FSSB amplifier setting screen............................. 1292

12.4.12.5 Displaying and setting the FSSB axis setting screen..................................... 1293

12.4.12.6 Displaying and setting the servo setting screen............................................. 1294

12.4.12.7 Parameter tuning screen (spindle setting)...................................................... 1295

12.4.12.8 Parameter tuning screen (miscellaneous settings) ......................................... 1296

12.4.12.9 Displaying and setting the servo tuning screen .............................................1297

12.4.12.10 Displaying and setting the spindle tuning screen.............................................1298

12.4.12.11 Displaying and setting the machining parameter tuning screen ......................1299

12.5 SCREENS DISPLAYED BY FUNCTION KEY ....................................... 1304

12.6 DISPLAYING THE PROGRAM NUMBER, SEQUENCE NUMBER, AND

STATUS, AND WARNING MESSAGES FOR DATA SETTING OR

INPUT/OUTPUT OPERATION ................................................................ 1305

12.6.1 Displaying the Program Number and Sequence Number...................................1305

c-15

TABLE OF CONTENTS B-63944EN/02

12.6.2 Displaying the Status and Warning for Data Setting or Input/Output

Operation............................................................................................................1307

13 GRAPHIC FUNCTION.......................................................................1310

13.1 GRAPHIC DISPLAY ................................................................................ 1311

IV. MAINTENANCE

1 ROUTINE MAINTENANCE ............................................................... 1327

1.1 ACTION TO BE TAKEN WHEN A PROBLEM OCCURRED ................... 1328

1.2 BACKING UP VARIOUS DATA ITEMS ................................................... 1329

1.3 METHOD OF REPLACING BATTERY .................................................... 1331

1.3.1 Replacing Battery for LCD-mounted Type CNC Control Unit .........................1332

1.3.2 Replacing the Battery for Stand-alone Type CNC Control Unit........................1335

1.3.3 Battery in the CNC Display Unit with PC Functions (3 VDC)..........................1337

1.3.4 Battery for Absolute Pulsecoders .......................................................................1339

APPENDIX

A PARAMETERS.................................................................................. 1347

A.1 DESCRIPTION OF PARAMETERS......................................................... 1348

A.2 DATA TYPE............................................................................................. 1559

A.3 STANDARD PARAMETER SETTING TABLES....................................... 1560

B PROGRAM CODE LIST.................................................................... 1562

C LIST OF FUNCTIONS AND PROGRAM FORMAT ..........................1565

D RANGE OF COMMAND VALUE.......................................................1576

E NOMOGRAPHS ................................................................................ 1579

E.1 INCORRECT THREADED LENGTH ....................................................... 1580

E.2 SIMPLE CALCULATION OF INCORRECT THREAD LENGTH .............. 1582

E.3 TOOL PATH AT CORNER ...................................................................... 1584

E.4 RADIUS DIRECTION ERROR AT CIRCLE CUTTING ............................ 1587

F CHARACTER-TO-CODES CORRESPONDENCE TABLE ..............1588

G ALARM LIST ..................................................................................... 1589

H PC TOOL FOR MEMORY CARD PROGRAM OPERATION/

EDITING ............................................................................................1646

H.1 PC TOOL FOR MEMORY CARD PROGRAM OPERATION/EDITING ... 1647

H.1.1 Usage Notes........................................................................................................1647

c-16

B-63944EN/02 TABLE OF CONTENTS

H.1.2 List of Functions of PC Tool ..............................................................................1647

H.1.3 Explanation Of Operations .................................................................................1648

H.2 NAMING RULES ..................................................................................... 1658

H.2.1 Naming Rules of Program File...........................................................................1658

H.2.2 Naming Rules Of Folder ....................................................................................1659

H.3 RULES OF CHARACTERS IN PROGRAM FILE..................................... 1660

H.3.1 Usable Characters in Program File.....................................................................1661

H.4 ERROR MESSAGE AND NOTE.............................................................. 1663

H.4.1 List of Error Message .........................................................................................1663

H.4.2 Note ..................................................................................................................1663

c-17

I. GENERAL

B-63944EN/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, explanations, and limitations.
III. OPERATION
Describes the manual operation and automatic operation of a

machine, procedures for inputting and outputting data, and

procedures for editing a program.
IV. MAINTENANCE
Describes procedures for daily maintenance and replacing

batteries.
APPENDIX
Lists parameters, valid data ranges, and alarms.

NOTE

1 This manual describes the functions common to

the lathe system and machining center system.
For the functions specific to the lathe system or
machining center system, refer to the User's
Manual (T series) (B-63944EN-1) or the User's
Manual (M series) (B-63944EN-2).

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 (B­63950EN).

Parameters are used to set functions and operating

conditions of a CNC machine tool, and frequently­used 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/02

Applicable models

This manual describes the models indicated in the table below.
In the text, the abbreviations indicated below may be used.

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

NOTE

1 For an explanatory purpose, the following

descriptions may be used according to the types of
path control used:

- T series: For the lathe system

- M series: For the machining center system

2 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.

3 Some functions described in this manual may not

be applied to some products.

For details, refer to the DESCRIPTIONS (B-

63942EN).

Series 31i

Series 310i

Series 310is

- 4 -

B-63944EN/02 GENERAL 1.GENERAL

Special symbols

This manual uses the following symbols:

M

-

T

-

-

- IP

- ;

Indicates a description that is valid only for the machine center system
set as system control type (in parameter No. 0983).
In a general description of the method of machining, a machining
center system operation is identified by a phase such as "for milling
machining".

Indicates a description that is valid only for the lathe system set as
system control type (in parameter No. 0983).
In a general description of the method of machining, a lathe system
operation is identified by a phrase such as "for lathe cutting".

Indicates the end of a description of a system control type.
When a system control type mark mentioned above is not followed by
this mark, the description of the system control type is assumed to
continue until the next item or paragraph begins. In this case, the next
item or paragraph provides a description common to the control types.

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.

- 5 -

1.GENERAL GENERAL B-63944EN/02

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

- 6 -

B-63944EN/02 GENERAL 1.GENERAL

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

- 7 -

1.GENERAL GENERAL B-63944EN/02

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.

- 8 -

II. PROGRAMMING

B-63944EN/02 PROGRAMMING 1.GENERAL

1 GENERAL

- 11 -

1.GENERAL PROGRAMMING B-63944EN/02

X

1.1 TOOL MOVEMENT ALONG WORKPIECE PARTS FIGURE-

INTERPOLATION

The tool moves along straight lines and arcs constituting the
workpiece parts figure (See II-4).

Explanation

The function of moving the tool along straight lines and arcs is called
the interpolation.

- Tool movement along a straight line

• For milling machining

• For lathe cutting

Workpiece

Fig. 1.1 (a) Tool movement along a straight line

Workpiece

Tool

To ol

Program
G01X_Y_ ;
X_ ;

Program
G01Z_ ;
G01X_Z_ ;

Z

- 12 -

B-63944EN/02 PROGRAMMING 1.GENERAL

X

- Tool movement along an arc

• For milling machining

Program
G03 X_ Y_ R_ ;

Workpiece

Tool

• For lathe cutting

Program
G02 X_ Z_ R_ ;
or
G03 X_ Z_ R_ ;

Workpiece

Fig. 1.1 (b) Tool movement along an arc

Z

The term interpolation refers to an operation in which the tool moves
along a straight line or arc in the way described above.
Symbols of the programmed commands G01, G02, ... are called the
preparatory function and specify the type of interpolation conducted in
the control unit.

(a) Movement along straight line

G01 Y_ ;
X_ Y_ ;

CNC

(b) Movement along arc

G03X_ Y_ R_ ;

X axis

Interpolation

Y axis

a)Movement
along straight

line
b)Movement
along arc

Fig. 1.1 (c) Interpolation function

Tool
movement

NOTE

Some machines move tables instead of tools but

this manual assumes that tools are moved against
workpieces.

- 13 -

1.GENERAL PROGRAMMING B-63944EN/02

1.2 FEED-FEED FUNCTION

Movement of the tool at a specified speed for cutting a workpiece is
called the feed.

• For milling machining

mm/min

F

Workpiece

Table

Tool

• For lathe cutting

mm/min

F

Workpiece

Chuck

Fig. 1.2 (a) Feed function

Tool

Feedrates can be specified by using actual numerics. For example, to
feed the tool at a rate of 150 mm/min, specify the following in the
program:
F150.0
The function of deciding the feed rate is called the feed function (See
II-5).

- 14 -

B-63944EN/02 PROGRAMMING 1.GENERAL

1.3 PART DRAWING AND TOOL MOVEMENT

1.3.1 Reference Position (Machine-specific Position)

A CNC machine tool is provided with a fixed position. Normally, tool
change and programming of absolute zero point as described later are
performed at this position. This position is called the reference
position.

• For milling machining

Reference position

Tool

Workpiece

Explanation

Table

• For lathe cutting

Tool post

Chuck

Fig. 1.3.1 (a) Reference position

Reference
position

The tool can be moved to the reference position in two ways:

1. Manual reference position return (See III-3.1)
Reference position return is performed by manual button

operation.

2. Automatic reference position return (See II-6)
In general, manual reference position return is performed first

after the power is turned on. In order to move the tool to the
reference position for tool change thereafter, the function of
automatic reference position return is used.

- 15 -

1.GENERAL PROGRAMMING B-63944EN/02

X

y

1.3.2 Coordinate System on Part Drawing and Coordinate System

Specified by CNC - Coordinate System

• For milling machining

Z

Y

Part drawing

• For lathe cutting

Program

X

Tool

Z

Workpiece

Machine tool

Z

Y

Coordinate system

CNC

Command

Tool

Y

X

X

Part drawing

X

Program

Z

Coordinate s

Command

X

Workpiece

Z

Machine tool

Fig. 1.3.2 (a) Coordinate system

Z

stem

CNC

- 16 -

B-63944EN/02 PROGRAMMING 1.GENERAL

Explanation

- Coordinate system

The following two coordinate systems are specified at different
locations: (See II-7)
1 Coordinate system on part drawing
The coordinate system is written on the part drawing. As the

program data, the coordinate values on this coordinate system are
used.

2. Coordinate system specified by the CNC
The coordinate system is prepared on the actual machine tool

table. This can be achieved by programming the distance from
the current position of the tool to the zero point of the coordinate
system to be set.

Y

230

300

Program
origin

Fig. 1.3.2 (b) Coordinate system specified by the CNC

Present tool position

Distance to the zero point of a coor­dinate system to be set

X

Concrete programming methods for setting coordinate systems
specified by the CNC are explained in II-7, "COORDINATE
SYSTEM".

- 17 -

1.GENERAL PROGRAMMING B-63944EN/02

The positional relation between these two coordinate systems is
determined when a workpiece is set on the table.

• For milling machining

Coordinate system on
part drawing estab

Coordinate system
specified by the CNC
established on the table

• For lathe cutting

Table

Y

Y

Workpiece

lished on the workpiece

X

X

Coordinate system specified by the
CNC established on the chuck

X

Workpiece

Z

Chuck

Fig. 1.3.2 (c) Coordinate system specified by CNC and coordinate

system on part drawing

Coordinate system on part drawing
established on the workpiece

X

Z

The tool moves on the coordinate system specified by the CNC in
accordance with the command program generated with respect to the
coordinate system on the part drawing, and cuts a workpiece into a
shape on the drawing.
Therefore, in order to correctly cut the workpiece as specified on the
drawing, the two coordinate systems must be set at the same position.

- 18 -

B-63944EN/02 PROGRAMMING 1.GENERAL

A

- Methods of setting the two coordinate systems in the same position

M

To set the two coordinate systems at the same position, simple
methods shall be used according to workpiece shape, the number of
machinings.

1. Using a standard plane and point of the workpiece.

Y

Fixed distance

Program
origin

Bring the tool center to the workpiece standard point.

nd set the coordinate system specified by CNC at this position.

Workpiece's
standard point

Fixed distance

X

2. Mounting a workpiece directly against the jig

Program origin

Jig

Meet the tool center to the reference position. And set the coordinate
specified by CNC at this position. (Jig shall be mounted on the
point from the reference

3. Mounting a workpiece on a pallet, then mounting the workpiece
and pallet on the jig

Pallet

Jig

Workpiece

(Jig and coordinate system shall be specified by the same as (2)).

- 19 -

1.GENERAL PROGRAMMING B-63944EN/02

X

p

T

The following method is usually used to define two coordinate
systems at the same location.

1 When coordinate zero point is set at chuck face

- Coordinates and
dimensions on part drawing

- Coordinate system on
lathe as s

ecified by CNC

Workpiece

60 40

40

150

X

Chuck

Workpiece

Program origin

Z

Z

When the coordinate system on the part drawing and the coordinate
system specified by the CNC are set at the same position, the program
origin can be set on the chuck face.

- 20 -

B-63944EN/02 PROGRAMMING 1.GENERAL

p

2. When coordinate zero point is set at workpiece end face.

- Coordinates and
dimensions on part drawing

60

Workpiece

80

100

X

30

Z

30

- Coordinate system on
lathe as s

ecified by CNC

Chuck

Workpiece

X

Z

Program origin

When the coordinate system on the part drawing and the coordinate
system specified by the CNC are set at the same position, the program
origin can be set on the end face of the workpiece.

- 21 -

1.GENERAL PROGRAMMING B-63944EN/02

A

X

φ30A

1.3.3 How to Indicate Command Dimensions for Moving the Tool

(Absolute, Incremental Commands)

Explanation

Command for moving the tool can be indicated by absolute command
or incremental command (See II-8.1).

- Absolute command

The tool moves to a point at "the distance from zero point of the
coordinate system" that is to the position of the coordinate values.

• For milling machining

Z

X

Command specifying movement from
point A to point B

• For lathe cutting

X

Tool

Y

B(10.0,30.0,5.0)

G90 X10.0 Y30.0 Z5.0 ;

Coordinates of point B

Tool

Workpiece

70

Command specifying movement from point A to
point B

B

Z

110

30.0Z70.0;

Coordinates of point B

- 22 -

B-63944EN/02 PROGRAMMING 1.GENERAL

A

φ30A

A

- Incremental command

Specify the distance from the previous tool position to the next tool
position.

• For milling machining

Z

Tool

X

B

Command specifying movement from
point A to point B

• For lathe cutting

X

Workpiece

Y-30.0

B

X=40.0

Y

Z=-10.0

G91 X40.0 Y-30.0 Z-10.0 ;

Distance and direction for
movement along each axis

Tool

-30.0 (diameter value)

φ60

Z

-40.0

Command specifying movement from point

to point B

U-30.0 W-40.0

Distance and direction for movement
along each axis

- 23 -

1.GENERAL PROGRAMMING B-63944EN/02

φ30ABφ

A

- Diameter programming / radius programming

Dimensions of the X axis can be set in diameter or in radius. Diameter
programming or radius programming is employed independently in
each machine.

1. Diameter programming
In diameter programming, specify the diameter value indicated

on the drawing as the value of the X axis.

X

Workpiece

40

60

80

Z

Coordinate values of points A and B A(30.0, 80.0), B(40.0, 60.0)

2. Radius programming
In radius programming, specify the distance from the center of

the workpiece, i.e. the radius value as the value of the X axis.

X

B

60

20

15

Z

80

Workpiece

Coordinate values of points A and B A(15.0, 80.0), B(20.0, 60.0)

- 24 -

B-63944EN/02 PROGRAMMING 1.GENERAL

φ

1.4 CUTTING SPEED - SPINDLE FUNCTION

The speed of the tool with respect to the workpiece when the
workpiece is cut is called the cutting speed.
As for the CNC, the cutting speed can be specified by the spindle
speed in min

• For milling machining

<When a workpiece should be machined with a tool 100 mm in
diameter at a cutting speed of 80 m/min.>
The spindle speed is approximately 250 min
N=1000v/πD. Hence the following command is required:
S250;
Commands related to the spindle speed are called the spindle speed
function ( See II-9) .

• For lathe cutting

-1

unit.

Spindle speed N

min

-1

Tool

Workpiece

Tool diameter

D mm

V: Cutting speed

m/min

-1

, which is obtained from

To ol

Cutting speed

v m/min

Workpiece

Spindle speed

φD

N min

-1

<When a workpiece 200 mm in diameter should be machined at a
cutting speed of 300 m/min.>
The spindle speed is approximately 478 min

-1

, which is obtained from
N=1000v/πD. Hence the following command is required:
S478 ;
Commands related to the spindle speed are called the spindle speed
function (See II-9).
The cutting speed v (m/min) can also be specified directly by the
speed value. Even when the workpiece diameter is changed, the CNC
changes the spindle speed so that the cutting speed remains constant.
This function is called the constant surface speed control function (See
II-9.3).

- 25 -

1.GENERAL PROGRAMMING B-63944EN/02

A

1.5 SELECTION OF TOOL USED FOR VARIOUS MACHINING -

TOOL FUNCTION

Overview

For each of various types of machining (such as drilling, tapping,
boring, and milling for milling machining, or rough machining,
semifinish machining, finish machining, threading, and grooving for
lathe cutting), a necessary tool is to be selected. When a number is
assigned to each tool and the number is specified in the program, the
corresponding tool is selected.

Examples

M

Tool number

01

02

TC magazine

Fig. 1.5 (a) Tool used for various machining

<When No.01 is assigned to a drilling tool>
When the tool is stored at location 01 in the ATC magazine, the tool
can be selected by specifying T01. This is called the tool function (See
II-10).

T

Tool number

01

06

02

03

Fig. 1.5 (b) Tool used for various machining

05

04

Tool post

<When No.01 is assigned to a roughing tool>

When the tool is stored at location 01 of the tool post, the tool can be
selected by specifying T0101. This is called the tool function (See II-

10).

- 26 -

B-63944EN/02 PROGRAMMING 1.GENERAL

1.6 COMMAND FOR MACHINE OPERATIONS - AUXILIARY

FUNCTION

When a workpiece is actually machined with a tool, the spindle is
rotated, coolant is supplied, and the chuck is opened/closed. So,
control needs to be exercised on the spindle motor of the machine,
coolant valve on/off operation, and chuck open/close operation.

• For milling machining

Tool

Spindle
rotation

Coolant on/off

Workpiece

• For lathe cutting

Coolant on/off

Chuck open/close

Workpiece

Fig. 1.6 (a) Auxiliary function

Spindle rotation

The function of specifying the on-off operations of the components of
the machine is called the auxiliary function. In general, the function is
specified by an M code (See II-11).
For example, when M03 is specified, the spindle is rotated clockwise
at the specified spindle speed.

- 27 -

1.GENERAL PROGRAMMING B-63944EN/02

1.7 PROGRAM CONFIGURATION

A group of commands given to the CNC for operating the machine is
called the program. By specifying the commands, the tool is moved
along a straight line or an arc, or the spindle motor is turned on and off.
In the program, specify the commands in the sequence of actual tool
movements.

Block

Block

Tool movement

Block

sequence

Program

Fig. 1.7 (a) Program configuration

Block

:

:

:

:

Block

A group of commands at each step of the sequence is called the block.
The program consists of a group of blocks for a series of machining.
The number for discriminating each block is called the sequence
number, and the number for discriminating each program is called the
program number (See II-13).

- 28 -

B-63944EN/02 PROGRAMMING 1.GENERAL

A

Explanation

The block and the program have the following configurations.

- Block

1 block

Nxxxxx Gxx Xxxx.x Yxxx.x Mxx Sxx Txx ;

- Program

Sequence
number

Preparatory
function

Dimension word

uxiliary

function

Spindle
function

Tool
function

End of block

Fig. 1.7 (b) Block configuration

A block starts with a sequence number to identify the block and ends
with an end-of-block code.
This manual indicates the end-of-block code by ; (LF in the ISO code
and CR in the EIA code).
The contents of the dimension word depend on the preparatory
function. In this manual, the portion of the dimension word may be
represent as IP_.

;
xxxxx ;

Program number

Block

Block

Block

:

:

:

M30 ;

Fig. 1.7 (c) Program configuration

:

:

:

End of program

Normally, a program number is specified after the end-of-block (;)
code at the beginning of the program, and a program end code (M02
or M30) is specified at the end of the program.

- 29 -

1.GENERAL PROGRAMMING B-63944EN/02

- Main program and subprogram

When machining of the same pattern appears at many portions of a
program, a program for the pattern is created. This is called the
subprogram. On the other hand, the original program is called the
main program. When a subprogram execution command appears
during execution of the main program, commands of the subprogram
are executed. When execution of the subprogram is finished, the
sequence returns to the main program.

Main program

:
:

M98P1001

:
:
:

Subprogram #1

O1001

M98P1002

:
:

M98P1001

:
:
:

M99

Subprogram #2

O1002

M99

Fig. 1.7 (d) Subprogram execution

- 30 -

B-63944EN/02 PROGRAMMING 1.GENERAL

1.8 TOOL MOVEMENT RANGE - STROKE

Limit switches are installed at the ends of each axis on the machine to
prevent tools from moving beyond the ends. The range in which tools
can move is called the stroke.

Machine zero point

Motor

Limit
switch

Stroke a rea

Besides strokes defined with limit switches, the operator can define an
area which the tool cannot enter using a program or data in memory.
This function is called stroke check (see III-6.3).

- 31 -

1.GENERAL PROGRAMMING B-63944EN/02

y

Motor

Limit
switch

Machine zero point

Specif

these distances.

Tools cannot enter this area. The
area is specified by data in memory
or a program.

- 32 -

B-63944EN/02 PROGRAMMING 2.CONTROLLED AXES

2 CONTROLLED AXES

- 33 -

2.CONTROLLED AXES PROGRAMMING B-63944EN/02

2.1 NUMBER OF CONTROLLED AXES

Explanation

The number of controlled axes used with this NC system depends on
the model and system control type as indicated below.

Lathe system 2 axes 2 axes 2 axes 2 axes Number of basic

controlled axes

Controlled axes expansion (total)
(including Cs axes and PMC axes)
Basic simultaneously controlled axes
(each path)
Simultaneously controlled axes
expansion (total / each path)

Machining
center system

Series 30i-A

Series 300i-A

Series 300is-A

3 axes 3 axes 3 axes 3 axes

Max. 32 axes Max. 20 axes Max. 20 axes Max. 9 axes

2 axes 2 axes 2 axes 2 axes

Max. 24 axes Max. 12 axes Max. 12 axes Max. 5 axes

Series 31i-A5

Series 310i-A5

Series 310is-A5

Series 31i-A

Series 310i-A

Series 310is-A

Series 32i-A

Series 320i-A

Series 320is-A

NOTE

1 The maximum number of controlled axes that can

be used is limited depending on the option
configuration. Refer to the manual provided by the
machine tool builder for details.

2 The number of simultaneously controllable axes for

manual operation (jog feed, manual reference
position return, or manual rapid traverse) is 1 or 3
(1 when parameter JAX (No. 1002#0) is set to 0
and 3 when it is set to 1).

- 34 -

B-63944EN/02 PROGRAMMING 2.CONTROLLED AXES

2.2 NAMES OF AXES

Explanation

The move axes of machine tools are assigned names. These names are
referred to as addresses or axis names. Axis names are determined
according to the machine tool. The naming rules comply with
standards such as the ISO standards.
With complex machines, one character would become insufficient for
representing axis names. So, up to three characters can be used for
axis names. A move axis may be named "X", "X1", or "XA1". The
first character of the three characters is called the first axis name
character, the second character is called the second axis name
character, and third character is called the third axis name character.
Example)

X A 1

3rd axis name character

2nd axis name character

1st axis name character

NOTE

1 Axis names are predetermined according to the

machine used. Refer to the manual supplied by the
machine tool builder.

2 Since many ordinary machines use one character

to represent each address, one-character
addresses are used in the description in this
manual.

- 35 -

2.CONTROLLED AXES PROGRAMMING B-63944EN/02

2.3 INCREMENT SYSTEM

Explanation

The increment system consists of the least input increment (for input)
and least command increment (for output). The least input increment
is the least increment for programming the travel distance. The least
command increment is the least increment for moving the tool on the
machine. Both increments are represented in mm, inches, or deg.
Five types of increment systems are available as indicated in Table 2.3
(a). For each axis, an increment system can be set using a bit from bit
0 to bit 3 (ISA, ISC, ISD, or ISE) of parameter No. 1013.
When IS-D or IS-E is to be selected, the corresponding option is
required.

Table 2.3 (a) Increment system

Name of increment

system

IS-A

IS-B

IS-C

IS-D

IS-E

Least input increment

0.01 mm 0.01 mm

0.001 inch 0.001 inch

0.01 deg 0.01 deg

0.001 mm 0.001 mm

0.0001 inch 0.0001 inch

0.001 deg 0.001 deg

0.0001 mm 0.0001 mm

0.00001 inch 0.00001 inch

0.0001 deg 0.0001 deg

0.00001 mm 0.00001 mm

0.000001 inch 0.000001 inch

0.00001 deg 0.00001 deg

0.000001 mm 0.000001 mm

0.0000001 inch 0.0000001 inch

0.000001 deg 0.000001 deg

The least command increment is either metric or inch depending on
the machine tool. Set metric or inch to the parameter INM
(No.0100#0).
For selection between metric and inch for the least input increment, G
code (G20 or G21) or a setting parameter selects it.
Combined use of the inch system and the metric system is not allowed.
There are functions that cannot be used between axes with different
unit systems (circular interpolation, cutter compensation, etc.). For the
increment system, see the machine tool builder's manual.

NOTE

1 The unit (mm or inch) in the table is used for

indicating a diameter value for diameter programming
(when bit 3 (DIA) of parameter No. 1006 is set to 1)
or a radius value for radius programming.

2 Some increment systems are unavailable depending

on the model. For details, refer to “Descriptions” (B­63942EN).

Least command

increment

- 36 -

B-63944EN/02 PROGRAMMING 2.CONTROLLED AXES

2.4 MAXIMUM STROKE

Explanation

The maximum stroke controlled by this CNC is shown in the table
below:
Maximum stroke = Least command increment × 99999999
(999999999 for IS-D and IS-E)
Commands that exceed the maximum stroke are not permitted.

Table 2.4 (a) Maximum strokes

Name of increment

system

IS-A

IS-B

IS-C

IS-D

IS-E

NOTE

1 The actual stroke depends on the machine tool.
2 The unit (mm or inch) in the table is used for

indicating a diameter value for diameter
programming (when bit 3 (DIA) of parameter No.
1006 is set to 1) or a radius value for radius
programming.

3 Some increment systems are unavailable

depending on the model. For details, refer to
“Descriptions” (B-63942EN).

Least input increment Maximum stroke

0.01 mm ±999999.99 mm

0.001 inch ±99999.999 inch

0.01 deg ±999999.99 deg

0.001 mm ±99999.999 mm

0.0001 inch ±9999.9999 inch

0.001 deg ±99999.999 deg

0.0001 mm ±9999.9999 mm

0.00001 inch ±999.99999 inch

0.0001 deg ±9999.9999 deg

0.00001 mm ±9999.99999 mm

0.000001 inch ±999.999999 inch

0.00001 deg ±9999.99999 deg

0.000001 mm ±999.999999 mm

0.0000001 inch ±99.9999999 inch

0.000001 deg ±999.999999 deg

- 37 -

3.PREPARATORY FUNCTION (G FUNCTION) PROGRAMMING B-63944EN/02

3 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_ ;
:

T

There are three G code systems in the lathe system : A, B, and C
(Table 3.1(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.

- 38 -

B-63944EN/02 PROGRAMMING3.PREPARATORY FUNCTION (G FUNCTION)

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.

(6) In the machining center system, the user can select G17,

G18, or G19 by setting parameters G18 and G19 (No.
3402#1 and #2).

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 canned cycle

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 for drilling.

6. G codes are indicated by group.

7. The group of G60 is switched according to the setting of the

parameter MDL (No. 5431#0). (When the MDL bit is set to 0,
the 00 group is selected. When the MDL bit is set to 1, the 01
group is selected.)

T

8. 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..

- 39 -

3.PREPARATORY FUNCTION (G FUNCTION) PROGRAMMING B-63944EN/02

3.1 G CODE LIST IN THE MACHINING CENTER SYSTEM

M

G code Group Function

G00 Positioning (rapid traverse)
G01 Linear interpolation (cutting feed)
G02 Circular interpolation CW or helical interpolation CW
G03 Circular interpolation CCW or helical interpolation CCW
G02.2, G03.2 Involute interpolation CW/CCW
G02.3, G03.3 Exponential interpolation CW/CCW
G02.4, G03.4
G04 Dwell
G05 AI contour control (high-precision contour control compatible command)
G05.1 AI contour control / Nano smoothing / Smooth interpolation
G05.4
G06.2 01 NURBS interpolation
G07 Hypothetical axis interpolation
G07.1 (G107) Cylindrical interpolation
G08 AI contour control (advanced preview control compatible command)
G09 Exact stop
G10 Programmable data input
G10.6 Tool retract and recover
G10.9 Programmable switching of diameter/radius specification
G11
G12.1 Polar coordinate interpolation mode
G13.1
G15 Polar coordinates command cancel
G16
G17 XpYp plane selection
G18 ZpXp plane selection
G19
G20 (G70) Input in inch
G21 (G71)
G22 Stored stroke check function on
G23
G25 Spindle speed fluctuation detection off
G26
G27 Reference position return check
G28 Automatic return to reference position
G29 Movement from reference position
G30 2nd, 3rd and 4th reference position return
G30.1 Floating reference position return
G31 Skip function
G31.8
G33 Threading
G34 Variable lead threading
G35 Circular threading CW
G36

01

00

00

21

17

02

06

04

19

00

01

Three-dimensional coordinate conversion CW/CCW

HRV3,4 on/off

Programmable data input mode cancel

Polar coordinate interpolation cancel mode

Polar coordinates command

YpZp plane selection

Input in mm

Stored stroke check function off

Spindle speed fluctuation detection on

EGB-axis skip

Circular threading CCW

Table 3.1 (a) G code list

Xp: X axis or its parallel axis
Yp: Y axis or its parallel axis
Zp: Z axis or its parallel axis

- 40 -

B-63944EN/02 PROGRAMMING3.PREPARATORY FUNCTION (G FUNCTION)

Table 3.1 (a) G code list

G code Group Function

G37 Automatic tool length measurement
G38 Cutter or tool nose radius compensation : preserve vector
G39

G40

G41

G41.2 Cutter compensation for 5-axis machining : left (type 1)
G41.3 Cutter compensation for 5-axis machining : (leading edge offset)
G41.4 Cutter compensation for 5-axis machining : left (type 1) (FS16i-compatible command)
G41.5 Cutter compensation for 5-axis machining : left (type 1) (FS16i-compatible command)
G41.6 Cutter compensation for 5-axis machining : left (type 2)

G42

G42.2 Cutter compensation for 5-axis machining : right (type 1)
G42.4 Cutter compensation for 5-axis machining : right (type 1) (FS16i-compatible command)
G42.5 Cutter compensation for 5-axis machining : right (type 1) (FS16i-compatible command)
G42.6
G40.1 Normal direction control cancel mode
G41.1 Normal direction control on : left
G42.1
G43 Tool length compensation +
G44
G43.1 Tool length compensation in tool axis direction
G43.4 Tool center point control (type 1)
G43.5
G45 Tool offset increase
G46 Tool offset decrease
G47 Tool offset double increase
G48
G49 (G49.1) 08 Tool length compensation cancel
G50 Scaling cancel
G51
G50.1 Programmable mirror image cancel
G51.1
G50.2 Polygon turning cancel
G51.2
G52 Local coordinate system setting
G53 Machine coordinate system setting
G53.1
G54 (G54.1) Workpiece coordinate system 1 selection
G55 Workpiece coordinate system 2 selection
G56 Workpiece coordinate system 3 selection
G57 Workpiece coordinate system 4 selection
G58 Workpiece coordinate system 5 selection
G59
G60 00 Single direction positioning

00

07

19

08

08

00

11

22

31

00

14

Cutter or tool nose radius compensation : corner circular interpolation
Cutter or tool nose radius compensation : cancel
Three-dimensional cutter compensation : cancel
Cutter or tool nose radius compensation : left
Three-dimensional cutter compensation : left

Cutter or tool nose radius compensation : right
Three-dimensional cutter compensation : right

Cutter compensation for 5-axis machining : right (type 2)

Normal direction control on : right

Tool length compensation -

Tool center point control (type 2)

Tool offset double decrease

Scaling

Programmable mirror image

Polygon turning

Tool axis direction control

Workpiece coordinate system 6 selection

- 41 -

3.PREPARATORY FUNCTION (G FUNCTION) PROGRAMMING B-63944EN/02

Table 3.1 (a) G code list

G code Group Function

G61 Exact stop mode
G62 Automatic corner override
G63 Tapping mode
G64
G65 00 Macro call
G66 Macro modal call A
G66.1 Macro modal call B
G67
G68 Coordinate system rotation start or 3-dimensional coordinate conversion mode on
G69 Coordinate system rotation cancel or 3-dimensional coordinate conversion mode off
G68.2
G72.1 Figure copy (rotation copy)
G72.2
G73 Peck drilling cycle
G74 Left-handed tapping cycle
G76 Fine boring cycle
G80
G80.5 24 Electronic gear box 2 pair: synchronization cancellation
G80.8 34 Electronic gear box: synchronization cancellation
G81 09 Drilling cycle or spot boring cycle
G81.1 00 Chopping
G81.5 24 Electronic gear box 2 pair: synchronization start
G81.8 34 Electronic gear box: synchronization start
G82 Drilling cycle or counter boring cycle
G83 Peck drilling cycle
G84 Tapping cycle
G84.2 Rigid tapping cycle (FS15 format)
G84.3 Left-handed rigid tapping cycle (FS15 format)
G85 Boring cycle
G86 Boring cycle
G87 Back boring cycle
G88 Boring cycle
G89
G90 Absolute programming
G91
G91.1 Checking the maximum incremental amount specified
G92 Setting for workpiece coordinate system or clamp at maximum spindle speed
G92.1
G93 Inverse time feed
G94 Feed per minute
G95
G96 Constant surface speed control
G97
G98 Canned cycle : return to initial level
G99
G107 00 Cylindrical interpolation
G112 Polar coordinate interpolation mode
G113

15

12

16

00

09

09

03

00

05

13

10

21

Cutting mode

Macro modal call A/B cancel

Feature coordinate system selection

Figure copy (linear copy)

Canned cycle cancel

Boring cycle

Incremental programming

Workpiece coordinate system preset

Feed per revolution

Constant surface speed control cancel

Canned cycle : return to R point level

Polar coordinate interpolation mode cancel

- 42 -

B-63944EN/02 PROGRAMMING3.PREPARATORY FUNCTION (G FUNCTION)

3.2 G CODE LIST IN THE LATHE SYSTEM

T

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)

Table 3.2 (a) G code list

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

- 43 -

3.PREPARATORY FUNCTION (G FUNCTION) PROGRAMMING B-63944EN/02

Table 3.2 (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) (FS16i­compatible command)
Cutter compensation for 5-axis machining : left (type 1) (FS16i­compatible command)

Cutter compensation for 5-axis machining : right (type 1) (FS16i­compatible command)
Cutter compensation for 5-axis machining : right (type 1) (FS16i­compatible command)
Cutter compensation for 5-axis machining : right (type 2)

Tool offset (lathe system ATC type)

Tool length compensation cancel

- 44 -

B-63944EN/02 PROGRAMMING3.PREPARATORY FUNCTION (G FUNCTION)

Table 3.2 (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)

- 45 -

3.PREPARATORY FUNCTION (G FUNCTION) PROGRAMMING B-63944EN/02

Table 3.2 (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

- 46 -

B-63944EN/02 PROGRAMMING 4.INTERPOLATION FUNCTIONS

4 INTERPOLATION FUNCTIONS

Interpolation functions specify the way to make an axis movement (in
other words, a movement of the tool with respect to the workpiece or
table).

- 47 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/02

4.1 POSITIONING (G00)

The G00 command moves a tool to the position in the workpiece
system specified with an absolute or an incremental command at a
rapid traverse rate.
In the absolute command, coordinate value of the end point is
programmed.
In the incremental command the distance the tool moves is
programmed.

Format

G00 IP_ ;

IP_ : For an absolute command, the coordinates of an end

point, and for an incremental command, the distance
the tool moves.

Explanation

Either of the following tool paths can be selected according to bit 1
(LRP) of parameter No. 1401.

• Nonlinear interpolation type positioning

The tool is positioned with the rapid traverse rate for each axis
separately. The tool path is normally straight.

• Linear interpolation type positioning. The tool is positioned

within the shortest possible time at a speed that is not more than
the rapid traverse rate for each axis.

Linear interpolation type positioning

End position

The rapid traverse rate in G00 command is set to the parameter No.
1420 for each axis independently by the machine tool builder. In the
positioning mode actuated by G00, the tool is accelerated to a
predetermined speed at the start of a block and is decelerated at the
end of a block. Execution proceeds to the next block after confirming
the in-position.
"In-position " means that the feed motor is within the specified range.
This range is determined by the machine tool builder by setting to
parameter (No. 1826).

Non linear interpolation type positioning

Start position

- 48 -

B-63944EN/02 PROGRAMMING 4.INTERPOLATION FUNCTIONS

Limitation

The rapid traverse rate cannot be specified in the address F.
Even if linear interpolation type positioning is specified, nonlinear
type interpolation positioning is used in the following cases. Therefore,
be careful to ensure that the tool does not foul the workpiece.

• G28 specifying positioning between the reference and

intermediate positions.

• G53

- 49 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/02

4.2 SINGLE DIRECTION POSITIONING (G60)

For accurate positioning without play of the machine (backlash), final
positioning from one direction is available.

Overrun

Start point

Start point

Format

Explanation

End point

Temporary stop

G60 IP_ ;

IP_ : For an absolute command, the coordinates of an end

point, and for an incremental command, the distance
the tool moves.

An overrun and a positioning direction are set by the parameter (No.

5440). Even when a commanded positioning direction coincides with
that set by the parameter, the tool stops once before the end point.
G60, which is an one-shot G-code, can be used as a modal G-code in
group 01 by setting 1 to the parameter MDL (No. 5431#0).
This setting can eliminate specifying a G60 command for every block.
Other specifications are the same as those for an one-shot G60
command. When an one-shot G code is specified in the single
direction positioning mode, the one-shot G command is effective like
G codes in group 01.

(Example)

When one-shot G60 commands are used.

G90;
G60 X0Y0;
G60 X100;
G60 Y100;
G04 X10;
G00 X0Y0;

When modal G60 command is used.

G90G60;
X0Y0;
X100;
Y100;
G04X10;
G00X0 Y0;

Single direction positioning
Single direction positioning
Single direction positioning

Single direction positioning mode start
Single direction positioning
Single direction positioning
Single direction positioning

Single direction positioning mode cancel

- 50 -

B-63944EN/02 PROGRAMMING 4.INTERPOLATION FUNCTIONS

- Overview of operation

• In the case of positioning of non-linear interpolation type (bit

1 (LRP) of parameter No. 1401 = 0)

As shown below, single direction positioning is performed

independently along each axis.

X

Overrun distance in the Z-axis direction

Overrun distance in the
X-axis direction

Programmed end point

Z

Programmed start point

• In the case of positioning of linear interpolation type (bit 1

(LRP) of parameter No. 1401 = 1)

Positioning of interpolation type is performed until the tool once

stops before or after a specified end point. Then, the tool is
positioned independently along each axis until the end point is
reached.

X

Limitation

Overrun distance in the Z-axis direction

Overrun distance in the
X-axis direction

Programmed end point

Z

Programmed start point

• Single direction positioning is not performed along an axis for

which no overrun distance is set in parameter No. 5440.

• Single direction positioning is not performed along an axis for

which travel distance 0 is specified.

• The mirror image function is not applied in a parameter-set

direction. Even in the mirror image mode, the direction of single
direction positioning remains unchanged. If positioning of linear
interpolation type is used, and the state of mirror image when a
single direction positioning block is looked ahead differs from
the state of mirror image when the execution of the block is
started, an alarm is issued. When switching mirror image in the
middle of a program, disable looking ahead by specifying a

- 51 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/02

non-buffering M code. Then, switch mirror image when there is
no look-ahead block.

• In the cylindrical interpolation mode (G07.1), single direction

positioning cannot be used.

• In the polar coordinate interpolation mode (G12.1), single

direction positioning cannot be used.

• When specifying single direction positioning on a machine that

uses angular axis control, first position the angular axis then
specify the positioning of the Cartesian axis. If the reverse
specification order is used, or the angular axis and Cartesian axis
are specified in the same block, an incorrect positioning direction
can result.

• In positioning at a restart position by program restart function,

single direction positioning is not performed.

M

T

• During canned cycle for drilling, no single direction positioning

is effected in drilling axis.

• The single direction positioning does not apply to the shift

motion in the canned cycles of G76 and G87.

• The G-code for single direction positioning is always G60, if

G-code system is A or B or C in all case.

• The single direction positioning can not be commanded during

the multiple repetitive cycle (G70-G76).

• No single direction positioning is effected in the drilling or

patting axis, during canned cycle for drilling (G83-G89) and the
rigid tapping (G84, G88). However, it can be commanded for
positioning.

• The single direction positioning can not be commanded during

the canned cycle (G90, G92, G94).

• During the single direction positioning mode (G60), the

following G-code can not be commanded.

G07.1, G12.1, G70-G76, G90-G94.

- 52 -

B-63944EN/02 PROGRAMMING 4.INTERPOLATION FUNCTIONS

4.3 LINEAR INTERPOLATION (G01)

Tools can move along a line.

Format

G01 IP_ F_ ;

IP_ : For an absolute command, the coordinates of an end

point, and for an incremental command, the distance
the tool moves.

F_ : Speed of tool feed (Feedrate)

Explanation

A tools move along a line to the specified position at the feedrate
specified in F.
The feedrate specified in F is effective until a new value is specified.
It need not be specified for each block.
The feedrate commanded by the F code is measured along the tool
path. If the F code is not commanded, the feedrate is regarded as zero.
The feedrate of each axis direction is as follows.

G01 αα ββ γγ ζζ Ff ;

α

Feed rate of α axis direction : f

Feed rate of β axis direction :

Feed rate of γ axis direction :

Feed rate of ζ axis direction :

2222

ζγβα

+++=L

α

F ×=

L

β

β

F ×=

L

γ

γ

f

F ×=

L

ζ

ζ

f

F ×=

L

f

The feedrate of the rotary axis is commanded in the unit of deg/min
(the unit is decimal point position).
When the straight line axis α (such as X, Y, or Z) and the rotating axis
b (such as A, B, or C) are linearly interpolated, the feedrate is that in
which the tangential feedrate in the α and β cartesian coordinate
system is commanded by F(mm/min).
β-axis feedrate is obtained ; at first, the time required for distribution
is calculated by using the above formula, then the β-axis feedrate unit
is changed to deg/min.

- 53 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/02

X

A calculation example is as follows.
G91 G01 X20.0B40.0 F300.0 ;
This changes the unit of the C axis from 40.0 deg to 40mm
with metric input. The time required for distribution is
calculated as follows:

22

4020

300

+

)(14907.0 mm

The feedrate for the C axis is

40

14907.0

mindeg/3.268

In simultaneous 3 axes control, the feedrate is calculated the same way
as in 2 axes control.

Example

- Linear interpolation

• For milling machining

(G91) G01X200.0Y100.0F200.0;

Y axis

100.0

0 (Start point)

200.0

• For lathe cutting

(Diameter programming)
G01X40.0Z20.1F20; (Absolute command)
or
G01U20.0W-25.9F20; (Incremental command)

20.1

40.0

φ

(End point)

46.0

End

Start

point

point

X axis

20.0

φ

Z

- 54 -

B-63944EN/02 PROGRAMMING 4.INTERPOLATION FUNCTIONS

- Feedrate for the rotary axis

G91G01C-90.0 F300.0 ;Feed rate of 300deg/min

(Start point)

90°

(End point)

Feedrate is 300 deg/min

- 55 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/02

4.4 CIRCULAR INTERPOLATION (G02, G03)

The command below will move a tool along a circular arc.

Format

Arc in the XpYp plane

G

02





G

17



G

03



YpXp




Arc in the ZpXp plane

G

02





G

18



G

03



XpZp




Arc in the YpZp plane

G

02





G

19



G

03



ZpYp




Command Description

G17 Specification of arc on XpYp plane
G18 Specification of arc on ZpXp plane
G19 Specification of arc on YpZp plane
G02 Circular Interpolation Clockwise direction (CW)
G03 Circular Interpolation Counterclockwise direction (CCW)

Xp_

Yp

_

Zp

_

I_

J_

K_

R_ Arc radius (with sign, radius value for lathe cutting)
F_ Feedrate along the arc

Command values of X axis or its parallel axis
(set by parameter No. 1022)
Command values of Y axis or its parallel axis
(set by parameter No. 1022)
Command values of Z axis or its parallel axis
(set by parameter No. 1022)
Xp axis distance from the start point to the center of an arc
with sign
Yp axis distance from the start point to the center of an arc
with sign
Zp axis distance from the start point to the center of an arc
with sign

T

NOTE

The U-, V-, and W-axes can be used with G-codes

B and C.

JI

__



__






__






__






_;

F



R

_



KI

__



_;

F



R

_



KJ

__



_;

F

R



_



- 56 -

B-63944EN/02 PROGRAMMING 4.INTERPOLATION FUNCTIONS

X

j

j

Explanation

- Direction of the circular interpolation

"Clockwise"(G02) and "counterclockwise"(G03) on the XpYp plane
(ZpXp plane or YpZp plane) are defined when the XpYp plane is
viewed in the positive-to-negative direction of the Zp axis (Yp axis or
Xp axis, respectively) in the Cartesian coordinate system. See the
figure below.

Y

G03

G02

G17

- Distance moved on an arc

The end point of an arc is specified by address Xp, Yp or Zp, and is
expressed as an absolute or incremental value according to G90 or
G91. For the incremental value, the distance of the end point which is
viewed from the start point of the arc is specified with sign.

- Distance from the start point to the center of arc

The arc center is specified by addresses I, J, and K for the Xp, Yp, and
Zp axes, respectively. The numerical value following I, J, or K,
however, is a vector component in which the arc center is seen from
the start point, and is always specified as an incremental value
irrespective of G90 and G91, as shown below.

I, J, and K must be signed according to the direction.

X

G02

G18

G03

Z

G02

G19

G03

YZ

- Command for a circle

End point (x,y)

y

x

Center

End point (z,x)

x

Start

i

point

z

Center

k

Start
point

i

End point (y,z)

z

y

Center

Start
point

k

I0,J0, and K0 can be omitted.
If the difference between the radius at the start point and that at the
end point exceeds the permitted value in a parameter (No.3410), an
alarm PS0020 occurs.

When Xp, Yp , and Zp are omitted (the end point is the same as the
start point) and the center is specified with I, J, and K, a 360° arc
(circle) is specified.
G02 I_ ; Command for a circle

- 57 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/02

- Arc radius

The distance between an arc and the center of a circle that contains the
arc can be specified using the radius, R, of the circle instead of I, J,
and K.
In this case, one arc is less than 180°, and the other is more than 180°
are considered. When an arc exceeding 180° is commanded, the radius
must be specified with a negative value. If Xp, Yp, and Zp are all
omitted, if the end point is located at the same position as the start
point and when R is used, an arc of 0° is programmed
G02R_ ; (The cutter does not move.)

For arc <1> (less than 180°)
G91 G02 XP60.0 YP55.0 R50.0 F300.0 ;
For arc <2> (greater than 180°)
G91 G02 XP60.0 YP55.0 R-50.0 F300.0 ;

- Feedrate

<2>

Start point

r=50mm

<1>

Y

End point

r=50mm

X

The feedrate in circular interpolation is equal to the feedrate specified
by the F code, and the feedrate along the arc (the tangential feedrate of
the arc) is controlled to be the specified feedrate.
The error between the specified feedrate and the actual tool feedrate is
±2% or less. However, this feedrate is measured along the arc after the
cutter compensation is applied

- 58 -

B-63944EN/02 PROGRAMMING 4.INTERPOLATION FUNCTIONS

Limitation

- Simultaneously specifying R with I, J, and K

If I, J, K, and R addresses are specified simultaneously, the arc
specified by address R takes precedence and the other are ignored.

- Specifying an axis that is not contained in the specified plane

If an axis not comprising the specified plane is commanded, an alarm
PS0028 occurs.
For example,
For milling machining:
If the X-axis and a U-axis parallel to the X-axis are specified when the
XY plane is specified
For lathe cutting:
If the X-axis and a U-axis parallel to the X-axis are specified when the
ZX plane is specified with G code system B or C

- Specifying a semicircle with R

When an arc having a center angle approaching 180° is specified, the
calculated center coordinates may contain an error. In such a case,
specify the center of the arc with I, J, and K.

- Difference in the radius between the start and end points

If the difference in the radius between the start and end points of the
arc exceeds the value specified in parameter No. 3410, alarm PS0020
is generated.
If the end point is not on the arc, the tool moves in a straight line
along one of the axes after reaching the end point.

- 59 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/02

Example

M

Yaxis

100

50

40

60

0

90 120 140

60

The above tool path can be programmed as follows ;
(1) In absolute programming
G92X200.0 Y40.0 Z0 ;
G90 G03 X140.0 Y100.0R60.0 F300.;
G02 X120.0 Y60.0R50.0 ;
or
G92X200.0 Y40.0Z0 ;
G90 G03 X140.0 Y100.0I-60.0 F300.;
G02 X120.0 Y60.0I-50.0 ;
(2) In incremental programming
G91 G03 X-60.0 Y60.0 R60.0 F300.;
G02 X-20.0 Y-40.0 R50.0 ;
or
G91 G03 X-60.0 Y60.0 I-60.0 F300. ;
G02 X-20.0 Y-40.0 I-50.0 ;

X axis

200

- 60 -

B-63944EN/02 PROGRAMMING 4.INTERPOLATION FUNCTIONS

X

X

X

X

T

- Command of circular interpolation X, Z

G02X_Z_I_K_F_; G03X_Z_I_K_F_;

X-axis

End point

Z

(Absolute programming)

K

Center of arc

(Diameter programming)

Start point

Z-axis

(Absolute programming)

End point

X-axis

Z

15.0

10.0

50.0

φ

30.0

R25.0

50.0

G02X_Z_R_F_;

Center of arc

End point

X-axis

(Diameter
programming)

Start point

I

K

Z-axis

(Absolute programming)

R

Z

(Diameter
programming)

Start point

Z-axis

(Diameter programming)

G02X50.0Z30.0I25.0F0.3; or
G02U20.0W-20.0I25.0F0.3; or
G02X50.0Z30.0R25.0F0.3 or
G02U20.0W-20.0R25.F0.3;

Z

- 61 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/02

4.5 HELICAL INTERPOLATION (G02, G03)

Helical interpolation which moved helically is enabled by specifying
up to two other axes which move synchronously with the circular
interpolation by circular commands.

Format

Arc of XpYp plane

G17

Arc of ZpXp plane

G18

Arc of YpZp plane

G19

G02

G03

G02

G03

G02

G03

Xp_Yp_

Zp_Xp_

Yp_Zp_

I_J_

R_

K_I_

R_

J_K_

R_

α_(β

α_(β

α_(β

_)F_;

_)F_;

_)F_;

Explanation

α, β

: Any one axis where circular interpolation is not applied.

Up to two other axes can be specified.

A tangential velocity of an arc in a specified plane or a tangential
velocity about the linear axis can be specified as the feedrate,
depending on the setting of bit 5 (HTG) of parameter No.1403.
An F command specifies a feedrate along a circular arc, when HTG is
specified to 0. Therefore, the feedrate of the linear axis is as follows:

Length of linear axis

F ×

Length of circular arc

Determine the feedrate so the linear axis feedrate does not exceed any
of the various limit values.

- 62 -

B-63944EN/02 PROGRAMMING 4.INTERPOLATION FUNCTIONS

r

Z

Tool p a t h

X

The feedrate along the circumference of two circula
interpolated axes is the specified feedrate.

Y

If HTG is set to 1, specify a feedrate along the tool path about the
linear axis. Therefore, the tangential velocity of the arc is expressed
as follows:

Length of arc

F ×

(Length of arc)2 + (Length of linear axis)2

The velocity along the linear axis is expressed as follows:

Length of linear axis

F ×

(Length of arc)2 + (Length of linear axis)2

Z

Limitation

Tool path

X

The feedrate along the tool path is specified.

Y

• Cutter compensation or tool nose radius compensation is applied

only for a circular arc.

• Tool offset and tool length compensation cannot be used in a block

in which a helical interpolation is commanded.

- 63 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/02

4.6 HELICAL INTERPOLATION B (G02, G03)

The helical interpolation B function differs from the helical
interpolation function just in that circular interpolation and a
movement on four axes outside the specified plane can be
simultaneously performed.
For the restrictions and parameters, see the description of the helical
interpolation function.

Format

Arc in the XpYp plane

G02

G17

G03

Arc in the ZpXp plane

G02

G18

G03

Arc in the YpZp plane

G02

G19

G03

α, β, γ, δ

: Any axis to which circular interpolation is not applied.

Up to four axes can be specified.

Xp Yp

Zp Xp

Yp Zp

I J

R

K I

R

J K

R

α β γ δ F ;

α β γ δ F ;

α β γ δ F ;

- 64 -

B-63944EN/02 PROGRAMMING 4.INTERPOLATION FUNCTIONS

4.7 SPIRAL INTERPOLATION, CONICAL INTERPOLATION

(G02, G03)

Spiral interpolation is enabled by specifying the circular interpolation
command together with a desired number of revolutions or a desired
increment (decrement) for the radius per revolution.
Conical interpolation is enabled by specifying the spiral
interpolation command together with an additional axis of movement,
as well as a desired increment (decrement) for the position along the
additional axes per spiral revolution.

Format

- Spiral interpolation

XpYp plane

G17

ZpXp plane

G18

YpZp plane

G19

X, Y, Z : Coordinates of the end point
L : Number of revolutions (positive value without a decimal point)

Q : Radius increment or decrement per spiral revolution (*1, *2)
I, J, K : Signed distance from the start point to the center (same as

F : Feedrate

(*1) Either the number of revolutions (L) or the radius increment or

(*2) The increment system for Q depends on the reference axis.

G02

G03

G02

G03

G02

G03

(*1)

the distance specified for circular interpolation)

decrement (Q) can be omitted. When L is omitted, the number of
revolutions is automatically calculated from the distance between
the current position and the center, the position of the end point,
and the radius increment or decrement. When Q is omitted, the
radius increment or decrement is automatically calculated from
the distance between the current position and the center, the
position of the end point, and the number of revolutions. If both L
and Q are specified but their values contradict, Q takes
precedence. Generally, either L or Q should be specified. The L
value must be a positive value without a decimal point. To
specify four revolutions plus 90°, for example, round the number
of revolutions up to five and specify L5.

X Y

I J Q L F ;

Z X

K I Q L F ;

Y Z

J K Q L F ;

- 65 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-63944EN/02

- Conical interpolation

XpYp plane

G17

ZpXp plane

G18

YpZp plane

G19

X, Y, Z : Coordinates of the end point
L : Number of revolutions (positive value without a decimal point)

Q : Radius increment or decrement per spiral revolution (*1, *2)
I, J, K : Two of the three values represent a signed vector from the start

F : Feedrate (The tangential velocity about the linear axis is

(*1) One of the height increment/decrement (I, J, K), radius

increment/decrement (Q), and the number of revolutions (L) must be
specified. The other two items can be omitted.

• Sample command for the XpYp plane

G02
G03

G02
G03

G02
G03

(*1)

point to the center. The remaining value is a height increment or
decrement per spiral revolution in conical interpolation. (*1)
When the XpYp plane is selected:

The I and J values represent a signed vector from the start
point to the center.
The K value represents a height increment or decrement per
spiral revolution.

When the ZpXp plane is selected:

The K and I values represent a signed vector from the start
point to the center.
The J value represents a height increment or decrement per
spiral revolution.

When the YpZp plane is selected:

The J and K values represent a signed vector from the start
point to the center.
The I value represents a height increment or decrement per
spiral revolution.

specified.)

X_Y_I_J_Z_Q_L_F_;

Z_X_K_I_Y_Q_L_F_;

Y_Z_J_K_X_Q_L_F_;

G17

If both L and Q are specified, but their values contradict, Q takes
precedence. If both L and a height increment or decrement are
specified, but their values contradict, the height increment or
decrement takes precedence. If both Q and a height increment or
decrement are specified, but their values contradict, Q takes
precedence. The L value must be a positive value without a decimal
point. To specify four revolutions plus 90°, for example, round the
number of revolutions up to five and specify L5.

(*2) The increment system for Q depends on the reference axis.

G02
G03

X_Y_I_J_Z_ Q_ F_;

K_

L_

- 66 -