fanuc 30iB, 31i B, 32i- B Operators Manual

FANUC Series 30+-MODEL B
FANUC Series 31+-MODEL B
FANUC Series 32+-MODEL B

Common to Lathe System / Machining Center System

OPERATOR'S MANUAL

B-64484EN/03

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

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

The products in this manual are controlled based on Japan’s “Foreign Exchange and
Foreign Trade Law”. The export of Series 30i-B, Series 31i-B5 from Japan is subject to an

export license by the government of Japan. Other models in this manual may also be
subject to export controls.
Further, re-export to another country may be subject to the license of the government of
the country from where the product is re-exported. Furthermore, the product may also be
controlled by re-export regulations of the United States government.
Should you wish to export or re-export these products, please contact FANUC for advice.

The products in this manual are manufactured under strict quality control. However, when
some serious accidents or losses are predicted due to a failure of the product, make
adequate consideration for safety.

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”.

B-64484EN/03 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

DEFINITION OF WARNING, CAUTION, AND NOTE.........................................................................s-1

GENERAL WARNINGS AND CAUTIONS ............................................................................................ s-2

WARNINGS AND CAUTIONS RELATED TO PROGRAMMING.......................................................s-3

WARNINGS AND CAUTIONS RELATED TO HANDLING ................................................................s-5

WARNINGS RELATED TO DAILY MAINTENANCE .........................................................................s-7

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-1

SAFETY PRECAUTIONS B-64484EN/03

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.
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 OPERATOR’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.

s-2

B-64484EN/03 SAFETY PRECAUTIONS

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.

NOTE

Programs, parameters, and macro variables are stored in non-volatile 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 non-volatile 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.

The number of times to write machining programs to the non-volatile memory is

limited.

You must use "High-speed program management" when registration and the

deletion of the machining programs are frequently repeated in such case that the

machining programs are automatically downloaded from a personal computer at

each machining.

In "High-speed program management", the program is not saved to the

non-volatile memory at registration, modification, or deletion of programs.

WARNINGS AND CAUTIONS RELATED TO PROGRAMMING

This section covers the major safety precautions related to programming. Before attempting to perform
programming, read the supplied OPERATOR’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.

s-3

SAFETY PRECAUTIONS B-64484EN/03

WARNING

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.
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.
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-4

B-64484EN/03 SAFETY PRECAUTIONS

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 OPERATOR’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.
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.

s-5

SAFETY PRECAUTIONS B-64484EN/03

WARNING

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.
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-6

B-64484EN/03 SAFETY PRECAUTIONS

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 and 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 OPERATOR’S

MANUAL (Common to T/M series) for details of the battery replacement

procedure.

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

of the battery replacement procedure.

i

series Maintenance Manual for details

α

s-7

SAFETY PRECAUTIONS B-64484EN/03

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-8

B-64484EN/03 TABLE OF CONTENTS

TABLE OF CONTENTS

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

DEFINITION OF WARNING, CAUTION, AND NOTE .............................................s-1

GENERAL WARNINGS AND CAUTIONS............................................................... s-2

WARNINGS AND CAUTIONS RELATED TO PROGRAMMING ............................s-3

WARNINGS AND CAUTIONS RELATED TO HANDLING...................................... s-5

WARNINGS RELATED TO DAILY MAINTENANCE............................................... s-7

I. GENERAL

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

1.1 NOTES ON READING THIS MANUAL.......................................................... 6

1.2 NOTES ON VARIOUS KINDS OF DATA ......................................................6

II. PROGRAMMING

1 GENERAL ...............................................................................................9

1.1 TOOL MOVEMENT ALONG WORKPIECE PARTS

FIGURE-INTERPOLATION ........................................................................... 9

1.2 FEED-FEED FUNCTION............................................................................. 11

1.3 PART DRAWING AND TOOL MOVEMENT................................................ 12

1.3.1 Reference Position (Machine-specific Position) ....................................................12

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

Coordinate System .................................................................................................13

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

Incremental Programming).....................................................................................18

1.4 CUTTING SPEED - SPINDLE FUNCTION.................................................. 21

1.5 SELECTION OF TOOL USED FOR VARIOUS MACHINING - TOOL

FUNCTION .................................................................................................. 22

1.6 COMMAND FOR MACHINE OPERATIONS - AUXILIARY FUNCTION ...... 23

1.7 PROGRAM CONFIGURATION ................................................................... 24

1.8 TOOL MOVEMENT RANGE - STROKE...................................................... 26

2 CONTROLLED AXES ........................................................................... 27

2.1 NUMBER OF CONTROLLED AXES ........................................................... 27

2.2 NAMES OF AXES .......................................................................................27

2.3 INCREMENT SYSTEM................................................................................ 28

2.4 MAXIMUM STROKE.................................................................................... 29

3 PREPARATORY FUNCTION (G FUNCTION) ...................................... 30

3.1 G CODE LIST IN THE MACHINING CENTER SYSTEM ............................32

3.2 G CODE LIST IN THE LATHE SYSTEM .....................................................36

4 INTERPOLATION FUNCTIONS............................................................ 40

4.1 POSITIONING (G00)................................................................................... 40

4.2 SINGLE DIRECTION POSITIONING (G60) ................................................ 41

4.3 LINEAR INTERPOLATION (G01)................................................................44

c-1

TABLE OF CONTENTS B-64484EN/03

4.4 CIRCULAR INTERPOLATION (G02, G03).................................................. 46

4.5 HELICAL INTERPOLATION (G02, G03) .....................................................50

4.6 HELICAL INTERPOLATION B (G02, G03).................................................. 51

4.7 SPIRAL INTERPOLATION, CONICAL INTERPOLATION (G02, G03)........ 52

4.8 POLAR COORDINATE INTERPOLATION (G12.1, G13.1) .........................58

4.9 CYLINDRICAL INTERPOLATION (G07.1) .................................................. 66

4.9.1 Cylindrical Interpolation ........................................................................................66

4.9.2 Cylindrical Interpolation by Plane Distance Command.........................................69

4.10 CUTTING POINT INTERPOLATION FOR CYLINDRICAL

INTERPOLATION (G07.1)........................................................................... 71

4.11 EXPONENTIAL INTERPOLATION (G02.3, G03.3)..................................... 81

4.12 SMOOTH INTERPOLATION (G05.1).......................................................... 87

4.13 NANO SMOOTHING ................................................................................... 92

4.14 NURBS INTERPOLATION (G06.2) ........................................................... 100

4.14.1 NURBS Interpolation Additional Functions ........................................................104

4.15 HYPOTHETICAL AXIS INTERPOLATION (G07) ...................................... 108

4.16 VARIABLE LEAD THREADING (G34)....................................................... 110

4.17 CIRCULAR THREADING (G35, G36) .......................................................111

4.18 SKIP FUNCTION (G31)............................................................................. 115

4.19 MULTI-STEP SKIP (G31) .......................................................................... 117

4.20 HIGH-SPEED SKIP SIGNAL (G31)........................................................... 117

4.21 SKIP POSITION MACRO VARIABLE IMPROVEMENT ............................ 118

4.22 CONTINUOUS HIGH-SPEED SKIP FUNCTION.......................................118

4.23 TORQUE LIMIT SKIP................................................................................ 119

4.24 3-DIMENSIONAL CIRCULAR INTERPOLATION......................................122

5 FEED FUNCTIONS ............................................................................. 127

5.1 OVERVIEW ............................................................................................... 127

5.2 RAPID TRAVERSE ...................................................................................128

5.3 CUTTING FEED ........................................................................................ 129

5.4 CUTTING FEEDRATE CONTROL ............................................................ 136

5.4.1 Exact Stop (G09, G61), Cutting Mode (G64), Tapping Mode (G63) ..................137

5.4.2 Automatic Corner Override ..................................................................................137

5.4.2.1 Automatic override for inner corners (G62) ................................................. 137

5.4.2.2 Internal circular cutting feedrate change....................................................... 139

5.5 FEEDRATE INSTRUCTION ON IMAGINARY CIRCLE FOR A ROTARY

AXIS ..........................................................................................................140

5.6 DWELL ...................................................................................................... 144

6 REFERENCE POSITION.....................................................................146

6.1 REFERENCE POSITION RETURN........................................................... 146

6.2 FLOATING REFERENCE POSITION RETURN (G30.1)........................... 152

7 COORDINATE SYSTEM..................................................................... 154

7.1 MACHINE COORDINATE SYSTEM.......................................................... 154

7.2 WORKPIECE COORDINATE SYSTEM ....................................................158

7.2.1 Setting a Workpiece Coordinate System ..............................................................158

7.2.2 Selecting a Workpiece Coordinate System ..........................................................160

7.2.3 Changing Workpiece Coordinate System ............................................................161

c-2

B-64484EN/03 TABLE OF CONTENTS

7.2.4 Workpiece Coordinate System Preset (G92.1).....................................................163

7.2.5 Addition of Workpiece Coordinate System Pair (G54.1 or G54) ........................165

7.2.6 Automatic Coordinate System Setting .................................................................167

7.2.7 Workpiece Coordinate System Shift ....................................................................167

7.3 LOCAL COORDINATE SYSTEM ..............................................................169

7.4 PLANE SELECTION.................................................................................. 170

7.5 PLANE CONVERSION FUNCTION ..........................................................171

8 COORDINATE VALUE AND DIMENSION .........................................177

8.1 ABSOLUTE AND INCREMENTAL PROGRAMMING................................ 177

8.2 INCH/METRIC CONVERSION (G20, G21) ............................................... 179

8.3 DECIMAL POINT PROGRAMMING.......................................................... 182

8.4 DIAMETER AND RADIUS PROGRAMMING ............................................183

8.5 DIAMETER AND RADIUS SETTING SWITCHING FUNCTION................ 184

9 SPINDLE SPEED FUNCTION (S FUNCTION) ...................................187

9.1 SPECIFYING THE SPINDLE SPEED WITH A CODE............................... 187

9.2 SPECIFYING THE SPINDLE SPEED VALUE DIRECTLY (S5-DIGIT

COMMAND) .............................................................................................. 187

9.3 CONSTANT SURFACE SPEED CONTROL (G96, G97) ..........................187

9.4 SPINDLE POSITIONING FUNCTION .......................................................191

9.4.1 Spindle Orientation...............................................................................................192

9.4.2 Spindle Positioning ..............................................................................................193

9.4.3 Canceling Spindle Positioning .............................................................................194

9.5 SPINDLE SPEED FLUCTUATION DETECTION....................................... 196

9.6 SPINDLE CONTROL WITH SERVO MOTOR........................................... 199

9.6.1 Spindle Control with Servo Motor .......................................................................199

9.6.2 Spindle Indexing Function ...................................................................................200

10 TOOL FUNCTION (T FUNCTION) ......................................................202

10.1 TOOL SELECTION FUNCTION ................................................................ 202

10.2 TOOL MANAGEMENT FUNCTION...........................................................203

10.3 TOOL MANAGEMENT EXTENSION FUNCTION ..................................... 217

10.3.1 Customization of Tool Management Data Display ..............................................217

10.3.2 Setting of Spindle Position / Standby Position Display .......................................221

10.3.3 Input of Customize Data with the Decimal Point.................................................223

10.3.4 Protection of Various Tool Information Items with the KEY Signal...................225

10.3.5 Selection of a Tool Life Count Period..................................................................225

10.3.6 Each tool Data Screen ..........................................................................................226

10.3.7 Total Life Time Display for Tools of The Same Type.........................................226

10.4 TOOL MANAGEMENT FUNCTION FOR OVERSIZE TOOLS .................. 226

10.5 TOOL LIFE MANAGEMENT...................................................................... 228

10.5.1 Tool Life Management Data ................................................................................229

10.5.2 Registering, Changing, and Deleting Tool Life Management Data.....................231

10.5.3 Tool Life Management Commands in Machining Program.................................236

10.5.4 Tool Life Counting and Tool Selection................................................................242

10.5.5 Tool Life Count Restart M Code..........................................................................244

10.5.6 Disabling Life Count ............................................................................................246

10.5.7 Remaining Tool Number Check Function ...........................................................246

11 AUXILIARY FUNCTION...................................................................... 248

c-3

TABLE OF CONTENTS B-64484EN/03

11.1 AUXILIARY FUNCTION (M FUNCTION)................................................... 248

11.2 MULTIPLE M COMMANDS IN A SINGLE BLOCK....................................249

11.3 M CODE GROUPING FUNCTION ............................................................250

11.3.1 Setting an M Code Group Number Using the Setting Screen ..............................250

11.3.2 Setting an M Code Group Number Using a Program...........................................251

11.3.3 M Code Group Check Function ...........................................................................252

11.4 SECOND AUXILIARY FUNCTIONS (B CODES) ......................................252

12 PROGRAM MANAGEMENT ...............................................................255

12.1 FOLDERS.................................................................................................. 255

12.1.1 Folder Configuration ............................................................................................255

12.1.2 Folder Attributes...................................................................................................257

12.1.3 Default Folders .....................................................................................................257

12.2 PROGRAMS.............................................................................................. 258

12.2.1 Program Name......................................................................................................258

12.2.2 Program Attributes ...............................................................................................260

12.3 RELATION WITH CONVENTIONAL FUNCTIONS.................................... 260

12.3.1 Relation with Folders ...........................................................................................260

12.3.2 Relation with Program Names..............................................................................261

12.3.3 Related Parameters ...............................................................................................263

12.3.4 Part Program Storage Size / Number of Registerable Programs ..........................263

13 PROGRAM CONFIGURATION...........................................................265

13.1 PROGRAM COMPONENTS OTHER THAN PROGRAM SECTIONS....... 266

13.2 PROGRAM SECTION CONFIGURATION ................................................ 268

13.3 SUBPROGRAM (M98, M99) .....................................................................274

14 FUNCTIONS TO SIMPLIFY PROGRAMMING ................................... 279

14.1 FIGURE COPYING (G72.1, G72.2)........................................................... 279

14.2 3-DIMENSIONAL COORDINATE SYSTEM CONVERSION ..................... 284

15 COMPENSATION FUNCTION ............................................................295

15.1 TOOL LENGTH COMPENSATION (G43, G44, G49)................................295

15.1.1 Overview ..............................................................................................................295

15.1.2 G53, G28, G30, and G30.1 Commands in Tool Length Compensation Mode ....300

15.2 SCALING (G50, G51)................................................................................ 302

15.3 PROGRAMMABLE MIRROR IMAGE (G50.1, G51.1) ............................... 309

15.4 NORMAL DIRECTION CONTROL (G40.1,G41.1,G42.1).......................... 311

15.5 WORKPIECE SETTING ERROR COMPENSATION ................................315

15.6 TOOL OFFSET FOR MILLING AND TURNING FUNCTION (G43.7)........ 361

15.7 TOOL OFFSET CONVERSION FUNCTION (G44.1) ................................ 367

16 CUSTOM MACRO............................................................................... 380

16.1 VARIABLES...............................................................................................380

16.2 SYSTEM VARIABLES ............................................................................... 385

16.3 READING AND WRITING VARIABLES FOR ANOTHER PATH...............436

16.4 ARITHMETIC AND LOGIC OPERATION ..................................................440

16.5 INDIRECT AXIS ADDRESS SPECIFICATION.......................................... 447

16.6 READING PARAMETERS.........................................................................448

16.7 MACRO STATEMENTS AND NC STATEMENTS..................................... 449

c-4

B-64484EN/03 TABLE OF CONTENTS

16.8 BRANCH AND REPETITION..................................................................... 450

16.8.1 Unconditional Branch (GOTO Statement)...........................................................450

16.8.2 GOTO Statement Using Stored Sequence Numbers ............................................450

16.8.3 Conditional Branch (IF Statement) ......................................................................451

16.8.4 Repetition (WHILE Statement)............................................................................452

16.8.5 Precision Specification for Macro Relational Operators......................................454

16.9 MACRO CALL ...........................................................................................456

16.9.1 Simple Call (G65) ................................................................................................457

16.9.2 Modal Call: Call After the Move Command (G66) .............................................464

16.9.3 Modal Call: Each Block Call (G66.1) ..................................................................467

16.9.4 Macro Call Using a G Code .................................................................................469

16.9.5 Macro Call Using a G Code (Specification of Multiple Definitions)...................470

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

Definitions)...........................................................................................................471

16.9.7 Macro Call Using an M Code...............................................................................471

16.9.8 Macro Call Using an M Code (Specification of Multiple Definitions)................473

16.9.9 Special Macro Call using M code ........................................................................474

16.9.10 Subprogram Call Using an M Code .....................................................................476

16.9.11 Subprogram Call Using an M Code (Specification of Multiple Definitions).......477

16.9.12 Subprogram Calls Using a T Code.......................................................................477

16.9.13 Subprogram Calls Using an S Code.....................................................................478

16.9.14 Subprogram Calls Using a Secondary Auxiliary Function ..................................478

16.9.15 Subprogram Call Using a Specific Address .........................................................479

16.10 MACRO CALL ARGUMENT FOR AXIS NAME EXPANSION ................... 482

16.11 PROCESSING MACRO STATEMENTS ...................................................483

16.12 REGISTERING CUSTOM MACRO PROGRAMS .....................................486

16.13 CODES AND RESERVED WORDS USED IN CUSTOM MACROS ......... 486

16.14 EXTERNAL OUTPUT COMMANDS..........................................................486

16.15 RESTRICTIONS........................................................................................ 490

16.16 INTERRUPTION TYPE CUSTOM MACRO............................................... 492

16.16.1 Specification Method ...........................................................................................493

16.16.2 Details of Functions..............................................................................................494

17 REAL-TIME CUSTOM MACRO ..........................................................501

17.1 TYPES OF REAL TIME MACRO COMMANDS......................................... 503

17.1.1 Modal Real Time Macro Command / One-shot Real Time Macro Command.....503

17.2 VARIABLES...............................................................................................508

17.2.1 Variables Dedicated to Real Time Custom Macros .............................................509

17.2.1.1 System variables ........................................................................................... 509

17.2.1.2 Real time macro variables (RTM variables) ................................................. 511

17.2.2 Custom Macro Variables......................................................................................512

17.2.2.1 System variables ........................................................................................... 513

17.2.2.2 Local variables .............................................................................................. 514

17.3 ARITHMETIC AND LOGICAL OPERATION.............................................. 514

17.4 CONTROL ON REAL TIME MACRO COMMANDS ..................................515

17.4.1 Conditional Branch (ZONCE Statement).............................................................516

17.4.2 Condition Transition (ZEDGE Statement)...........................................................517

17.4.3 Repetition (ZWHILE Statement) .........................................................................518

17.4.4 Multi-statement (ZDO...ZEND Statement) ..........................................................519

17.5 MACRO CALL ...........................................................................................521

17.6 OTHERS.................................................................................................... 522

17.7 AXIS CONTROL COMMAND .................................................................... 523

c-5

TABLE OF CONTENTS B-64484EN/03

17.8 NOTES ...................................................................................................... 534

17.9 LIMITATION ..............................................................................................535

18 PROGRAMMABLE PARAMETER INPUT (G10)................................538

19 PATTERN DATA INPUT ..................................................................... 542

19.1 OVERVIEW ............................................................................................... 542

19.2 EXPLANATION.......................................................................................... 542

19.3 EXPLANATION OF OPERATION.............................................................. 546

19.4 DEFINITION OF THE SCREEN ................................................................550

19.4.1 Definition of the Pattern Menu Screen.................................................................551

19.4.2 Definition of the Custom Macro Screen...............................................................553

19.4.3 Setting the Character-codes..................................................................................556

20 HIGH-SPEED CUTTING FUNCTIONS................................................ 561

20.1 AI CONTOUR CONTROL FUNCTION I AND AI CONTOUR CONTROL

FUNCTION II (G05.1)................................................................................ 561

20.2 MACHINING CONDITION SELECTING FUNCTION ................................575

20.3 MACHINING QUALITY LEVEL ADJUSTMENT.........................................575

20.4 HIGH-SPEED CYCLE MACHINING .......................................................... 577

20.5 HIGH-SPEED BINARY PROGRAM OPERATION..................................... 578

20.6 OPTIMUM ACCELERATION/DECELERATION FOR RIGID TAPPING .... 579

20.7 PATH TABLE OPERATION.......................................................................581

21 AXIS CONTROL FUNCTIONS............................................................607

21.1 AXIS SYNCHRONOUS CONTROL........................................................... 607

21.2 POLYGON TURNING (G50.2, G51.2).......................................................609

21.3 SYNCHRONOUS, COMPOSITE AND SUPERIMPOSED CONTROL BY
PROGRAM COMMAND (G50.4, G51.4, G50.5, G51.5, G50.6, AND

G51.6)........................................................................................................ 614

21.4 ROTARY AXIS ROLL-OVER..................................................................... 617

21.4.1 Rotary Axis Roll-over ..........................................................................................617

21.4.2 Rotary Axis Control .............................................................................................618

21.5 TOOL RETRACT AND RECOVER............................................................ 619

21.5.1 Improvement of Tool compensation for Tool Retract and Recover.....................622

21.6 ELECTRONIC GEAR BOX........................................................................ 626

21.6.1 Electronic Gear Box .............................................................................................626

21.6.2 Spindle Electronic Gear Box................................................................................632

21.6.3 Electronic Gear Box Automatic Phase Synchronization......................................639

21.6.4 Skip Function for EGB Axis ................................................................................643

21.6.5 Electronic Gear Box 2 Pair...................................................................................645

21.6.5.1 Specification method (G80.5, G81.5) ........................................................... 645

21.6.5.2 Description of commands compatible with those for a hobbing machine

(G80, G81) .................................................................................................... 648

21.6.5.3 Controlled axis configuration example......................................................... 651

21.6.5.4 Sample programs........................................................................................... 652

21.6.5.5 Synchronization ratio specification range..................................................... 655

21.6.5.6 Retract function............................................................................................. 658

21.6.6 U-axis Control ......................................................................................................658

21.6.7 U-axis Control 2 Pairs ..........................................................................................660

21.7 TANDEM CONTROL .................................................................................661

c-6

B-64484EN/03 TABLE OF CONTENTS

21.8 PIVOT AXIS CONTROL ............................................................................ 661

21.9 CHOPPING FUNCTION ............................................................................ 664

21.10 SKIP FUNCTION FOR FLEXIBLE SYNCHRONOUS CONTROL .............671

21.11 CHOPPING FUNCTION BY FLEXIBLE SYNCHRONOUS CONTROL ..... 673

21.12 HIGH PRECISION OSCILLATION FUNCTION......................................... 674

22 5-AXIS MACHINING FUNCTION ........................................................682

22.1 TOOL CENTER POINT CONTROL........................................................... 682

22.2 HIGH-SPEED SMOOTH TCP.................................................................... 739

22.2.1 High-speed Smooth TCP......................................................................................739

22.2.1.1 Rotation axes compensation (G43.4L1, G43.5L1) ....................................... 744

22.2.1.2 Smooth control (G43.4P3, G43.5P3)............................................................ 749

22.2.2 Tolerance change in High-speed Smooth TCP mode...........................................755

22.2.2.1 Tolerance change in rotation axes compensation (G43.4L1, G43.5L1) ....... 755

22.2.2.2 Tolerance change in smooth control (G43.4P3, G43.5P3) ........................... 758

22.2.3 Information Display in High-speed Smooth TCP ................................................758

22.3 EXPANSION OF AXIS MOVE COMMAND IN TOOL CENTER POINT

CONTROL ................................................................................................. 764

22.4 TOOL POSTURE CONTROL .................................................................... 766

22.5 CUTTING POINT COMMAND................................................................... 776

22.6 TILTED WORKING PLANE INDEXING..................................................... 786

22.6.1 Tilted Working Plane Indexing ............................................................................786

22.6.1.1 Tilted working plane indexing based on Eulerian angle............................... 789

22.6.1.2 General specifications of the tilted working plane indexing......................... 790

22.6.1.3 Tilted working plane indexing based on roll-pitch-yaw ............................... 793

22.6.1.4 Tilted working plane indexing based on three points ................................... 795

22.6.1.5 Tilted working plane indexing based on two vectors.................................... 799

22.6.1.6 Tilted working plane indexing based on projection angles........................... 802

22.6.1.7 Tilted working plane indexing by tool axis direction ...................................805

22.6.2 Multiple command of tilted working plane indexing ...........................................815

22.6.2.1 Absolute multiple command ......................................................................... 815

22.6.2.2 Incremental multiple command..................................................................... 817

22.6.3 Tool Axis Direction Control.................................................................................819

22.6.3.1 Tool axis direction control............................................................................ 819

22.6.3.2 Tool center point retention type tool axis direction control.......................... 836

22.6.4 Tilted Working Plane Indexing in Tool Length Compensation ...........................840

22.7 INCLINED ROTARY AXIS CONTROL ......................................................847

22.8 3-DIMENSIONAL CUTTER COMPENSATION .........................................850

22.8.1 Cutter Compensation in Tool Rotation Type Machine ........................................852

22.8.1.1 Tool side offset ............................................................................................. 853

22.8.1.2 Leading edge offset....................................................................................... 869

22.8.1.3 Tool tip position (cutting point) command ................................................... 873

22.8.2 Cutter Compensation in Table Rotation Type Machine.......................................876

22.8.3 Cutter Compensation in Composite Type Machine .............................................881

22.8.4 Interference Check and Interference Avoidance ..................................................886

22.8.5 Restrictions...........................................................................................................889

22.8.5.1 Restrictions common to machine configurations.......................................... 889

22.8.5.2 Restriction on tool rotation type.................................................................... 891

22.8.5.3 Restriction on machine configurations having table rotation axes (table

rotation type and composite type)................................................................. 892

22.8.6 Examples ..............................................................................................................895

22.9 EXPANSION OF THE WAY TO SET 5-AXIS MACHINING FUNCTION

PARAMETERS.......................................................................................... 900

c-7

TABLE OF CONTENTS B-64484EN/03

22.10 MACHINE CONFIGURATION SELECTING FUNCTION ..........................903

22.10.1 Machine Configuration Selecting Screen.............................................................903

22.10.2 Switching Machine Configuration .......................................................................904

22.10.3 Setting Machine Configuration Data....................................................................906

22.10.4 Inputting and Outputting Machine Configuration Data .......................................909

23 MUITI-PATH CONTROL FUNCTION.................................................. 911

23.1 OVERVIEW ............................................................................................... 911

23.2 WAITING FUNCTION FOR PATHS ..........................................................912

23.3 COMMON MEMORY BETWEEN EACH PATH.........................................917

23.4 SPINDLE CONTROL BETWEEN EACH PATH......................................... 918

23.5 SYNCHRONOUS/COMPOSITE/SUPERIMPOSED CONTROL................ 919

III. OPERATION

1 GENERAL ...........................................................................................925

1.1 MANUAL OPERATION.............................................................................. 925

1.2 TOOL MOVEMENT BY PROGRAMING - AUTOMATIC OPERATION .....926

1.3 AUTOMATIC OPERATION ....................................................................... 927

1.4 TESTING A PROGRAM ............................................................................ 928

1.4.1 Check by Running the Machine ...........................................................................928

1.4.2 How to View the Position Display Change without Running the Machine .........930

1.5 EDITING A PROGRAM ............................................................................. 930

1.6 DISPLAYING AND SETTING DATA.......................................................... 930

1.7 DISPLAY ...................................................................................................933

1.7.1 Program Display...................................................................................................933

1.7.2 Current Position Display ......................................................................................934

1.7.3 Alarm Display ......................................................................................................935

1.7.4 Parts Count Display, Run Time Display ..............................................................936

2 OPERATIONAL DEVICES.................................................................. 937

2.1 POWER ON/OFF....................................................................................... 937

2.1.1 Turning on the Power ...........................................................................................937

2.1.2 Power Disconnection............................................................................................938

2.2 SETTING AND DISPLAY UNITS............................................................... 939

2.2.1 8.4" LCD CNC Display Panel ..............................................................................939

2.2.2 10.4" LCD CNC Display Panel (12.1"/15"/19" LCD CNC Display Panel).........940

2.2.3 Standard MDI Unit (ONG Key) ...........................................................................941

2.2.4 Standard MDI Unit (QWERTY Key)...................................................................942

2.2.5 Small MDI Unit (ONG Key) ................................................................................943

2.3 EXPLANATION OF THE MDI UNIT........................................................... 944

2.4 FUNCTION KEYS AND SOFT KEYS ........................................................ 947

2.4.1 General Screen Operations ...................................................................................947

2.4.2 Function Keys ......................................................................................................948

2.4.3 Soft Keys ..............................................................................................................949

2.5 EXTERNAL I/O DEVICES ......................................................................... 957

3 MANUAL OPERATION....................................................................... 959

3.1 MANUAL REFERENCE POSITION RETURN...........................................959

3.2 JOG FEED (JOG)...................................................................................... 960

3.3 INCREMENTAL FEED ..............................................................................962

c-8

B-64484EN/03 TABLE OF CONTENTS

3.4 MANUAL HANDLE FEED..........................................................................963

3.5 MANUAL ABSOLUTE ON AND OFF......................................................... 966

3.6 MANUAL LINEAR/CIRCULAR INTERPOLATION..................................... 970

3.7 RIGID TAPPING BY MANUAL HANDLE................................................... 974

3.8 MANUAL NUMERICAL COMMAND.......................................................... 976

3.9 3-DIMENSIONAL MANUAL FEED ............................................................984

3.9.1 Tool Axis Direction Handle Feed / Tool Axis Direction JOG Feed / Tool Axis

Direction Incremental Feed ..................................................................................985

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

Direction JOG Feed / Tool Axis Right-Angle Direction Incremental Feed.........987

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

Tool Tip Center Rotation Incremental Feed.........................................................990

3.9.4 Table Vertical Direction Handle Feed / Table Vertical Direction JOG Feed /

Table Vertical Direction Incremental Feed ..........................................................992

3.9.5 Table Horizontal Direction Handle Feed / Table Horizontal Direction JOG

Feed / Table Horizontal Direction Incremental Feed ...........................................994

3.10 DISTANCE CODED LINEAR SCALE INTERFACE................................... 997

3.10.1 Procedure for Reference Position Establishment .................................................998

3.10.2 Reference Position Return....................................................................................999

3.10.3 Distance Coded Rotary Encoder ..........................................................................999

3.10.4 Axis Synchronization Control ..............................................................................999

3.10.5 Axis Control by PMC.........................................................................................1001

3.10.6 Angular Axis Control .........................................................................................1001

3.10.7 Note ....................................................................................................................1001

3.11 LINEAR SCALE WITH DISTANCE-CODED REFERENCE MARKS

(SERIAL) ................................................................................................. 1002

4 AUTOMATIC OPERATION ...............................................................1007

4.1 MEMORY OPERATION ..........................................................................1007

4.2 MDI OPERATION.................................................................................... 1009

4.3 DNC OPERATION...................................................................................1012

4.4 SCHEDULE OPERATION ....................................................................... 1015

4.5 EXTERNAL SUBPROGRAM CALL (M198).............................................1018

4.6 EXTERNAL SUBPROGRAM CALLS USING THE DATA SERVER

AVAILABLE IN MULTI-PATH SYSTEMS ................................................ 1022

4.7 MANUAL HANDLE INTERRUPTION ......................................................1023

4.7.1 Manual Interruption of 3-dimensional Coordinate System Conversion.............1029

4.8 MIRROR IMAGE...................................................................................... 1030

4.9 PROGRAM RESTART ............................................................................ 1031

4.9.1 Auxiliary Function Output in Program Restart Function ...................................1047

4.10 QUICK PROGRAM RESTART ................................................................ 1051

4.10.1 Suppress Motion of Quick Program Restart.......................................................1068

4.10.2 Quick Program Restart for a Machining Cycle ..................................................1072

4.11 TOOL RETRACT AND RECOVER.......................................................... 1080

4.11.1 Retract ................................................................................................................1082

4.11.2 Withdrawal .........................................................................................................1083

4.11.3 Return .................................................................................................................1083

4.11.4 Repositioning .....................................................................................................1084

4.11.5 Tool Retract and Recover for Threading............................................................1084

4.11.6 Operation Procedure for a Canned Cycle for Drilling........................................1087

4.12 MANUAL INTERVENTION AND RETURN..............................................1089

c-9

TABLE OF CONTENTS B-64484EN/03

4.13 RETRACE................................................................................................ 1092

4.14 ACTIVE BLOCK CANCEL FUNCTION.................................................... 1101

5 TEST OPERATION ........................................................................... 1105

5.1 MACHINE LOCK AND AUXILIARY FUNCTION LOCK ........................... 1105

5.2 FEEDRATE OVERRIDE.......................................................................... 1106

5.3 RAPID TRAVERSE OVERRIDE.............................................................. 1107

5.4 DWELL/AUXILIARY FUNCTION TIME OVERRIDE ................................ 1107

5.5 DRY RUN ................................................................................................1109

5.6 SINGLE BLOCK ......................................................................................1110

5.7 HIGH SPEED PROGRAM CHECK FUNCTION ...................................... 1111

5.8 MANUAL HANDLE RETRACE ................................................................ 1113

5.8.1 Displaying Program Being Executed in Backward Movement ..........................1124

5.9 AUXILIARY FUNCTION OUTPUT BLOCK REVERSE MOVEMENT FOR

MANUAL HANDLE RETRACE ................................................................ 1126

5.10 MANUAL HANDLE RETRACE FUNCTION FOR MULTI-PATH.............. 1126

5.11 EXTENSION OF THE MANUAL HANDLE RETRACE FUNCTION ......... 1130

6 SAFETY FUNCTIONS.......................................................................1134

6.1 EMERGENCY STOP............................................................................... 1134

6.2 OVERTRAVEL......................................................................................... 1134

6.3 STORED STROKE CHECK..................................................................... 1135

6.4 STROKE LIMIT CHECK BEFORE MOVE ............................................... 1139

6.5 STROKE LIMIT AREA CHANGING FUNCTION .....................................1141

6.6 WRONG OPERATION PREVENTION FUNCTIONS ..............................1142

6.6.1 Functions that are Used When Data is Set .........................................................1142

6.6.1.1 Input data range check ................................................................................ 1143

6.6.1.2 Confirmation of incremental input.............................................................. 1144

6.6.1.3 Prohibition of the absolute input by the soft key ........................................1145

6.6.1.4 Confirmation of the deletion of the program .............................................. 1145

6.6.1.5 Confirmation of the deletion of all data ...................................................... 1146

6.6.1.6 Confirmation of a data update during the data setting process ................... 1146

6.6.2 Functions that are Used when the Program is Executed ....................................1147

6.6.2.1 Display of updated modal information .......................................................1147

6.6.2.2 Start check signal ........................................................................................ 1147

6.6.2.3 Axis status display ......................................................................................1148

6.6.2.4 Confirmation of the start from a middle block............................................ 1149

6.6.2.5 Data range check......................................................................................... 1150

6.6.2.6 Maximum incremental value check ............................................................ 1151

6.6.3 Setting Screen.....................................................................................................1151

6.6.3.1 Operation confirmation function setting screen .......................................... 1151

6.6.3.2 Tool offset range setting screen ..................................................................1153

6.6.3.3 Workpiece origin offset range setting screen.............................................. 1156

6.6.3.4 Y-axis tool offset range setting screen........................................................ 1158

6.6.3.5 Workpiece shift range setting screen ..........................................................1159

7 ALARM AND SELF-DIAGNOSIS FUNCTIONS................................ 1161

7.1 ALARM DISPLAY .................................................................................... 1161

7.2 ALARM HISTORY DISPLAY ...................................................................1163

7.3 CHECKING BY DIAGNOSTIC DISPLAY................................................. 1164

7.4 RETURN FROM THE ALARM SCREEN................................................. 1166

7.4.1 Return from the Alarm Screen ...........................................................................1166

c-10

B-64484EN/03 TABLE OF CONTENTS

7.4.2 Relationship with Other Functions .....................................................................1167

8 DATA INPUT/OUTPUT ..................................................................... 1169

8.1 OVERWRITING FILES ON A MEMORY CARD/USB MEMORY.............1171

8.2 INPUT/OUTPUT ON EACH SCREEN .....................................................1173

8.2.1 Inputting and Outputting a Program...................................................................1174

8.2.1.1 Inputting a program..................................................................................... 1174

8.2.1.2 Outputting a program.................................................................................. 1176

8.2.1.3 Inputting and outputting of O8-digit........................................................... 1177

8.2.2 Inputting and Outputting Parameters..................................................................1178

8.2.2.1 Inputting parameters ................................................................................... 1178

8.2.2.2 Outputting parameters................................................................................. 1179

8.2.3 Inputting and Outputting Offset Data.................................................................1180

8.2.3.1 Inputting offset data .................................................................................... 1180

8.2.3.2 Outputting offset data ................................................................................. 1181

8.2.4 Inputting and Outputting Pitch Error Compensation Data .................................1185

8.2.4.1 Inputting pitch error compensation data .....................................................1185

8.2.4.2 Outputting pitch error compensation data................................................... 1186

8.2.4.3 Input/output format of pitch error compensation data ................................1187

8.2.5 Inputting and Outputting 3-dimensional Error Compensation Data ..................1188

8.2.5.1 Inputting 3-dimensional error compensation data....................................... 1188

8.2.5.2 Outputting 3-dimensional error compensation data .................................... 1190

8.2.5.3 Input/output format of 3-dimensional error compensation data.................. 1190

8.2.6 Inputting and Outputting Three-dimensional Rotary Error Compensation Data1192

8.2.6.1 Inputting three-dimensional rotary error compensation data ...................... 1192

8.2.6.2 Outputting three-dimensional rotary error compensation data.................... 1193

8.2.6.3 Input/output format of three-dimensional rotary error compensation data. 1194

8.2.7 Inputting and Outputting Custom Macro Common Variables ...........................1196

8.2.7.1 Inputting custom macro common variables ................................................ 1196

8.2.7.2 Outputting custom macro common variables..............................................1197

8.2.8 Inputting and Outputting Workpiece Coordinates System Data ........................1199

8.2.8.1 Inputting workpiece coordinate system data............................................... 1199

8.2.8.2 Outputting workpiece coordinate system data ............................................ 1200

8.2.9 Inputting and Outputting Operation History Data..............................................1200

8.2.9.1 Outputting operation history data ............................................................... 1201

8.2.9.2 Inputting operation history signal selection data ........................................ 1201

8.2.9.3 Outputting operation history signal section data......................................... 1202

8.2.9.4 Input/output format of operation history signal selection data ...................1203

8.2.10 Inputting and Outputting Tool Management Data .............................................1204

8.2.10.1 Inputting tool management data.................................................................. 1204

8.2.10.2 Outputting tool management data ............................................................... 1205

8.2.10.3 Inputting magazine data.............................................................................. 1206

8.2.10.4 Outputting magazine data ........................................................................... 1208

8.2.10.5 Inputting tool life status name data............................................................. 1208

8.2.10.6 Outputting tool life status name data ..........................................................1209

8.2.10.7 Inputting name data of customize data........................................................ 1210

8.2.10.8 Outputting name data of customize data..................................................... 1211

8.2.10.9 Inputting customize data displayed as tool management data.....................1211

8.2.10.10 Outputting customize data displayed as tool management data.................. 1212

8.2.10.11 Inputting spindle waiting position name data ............................................. 1213

8.2.10.12 Outputting spindle waiting position name data........................................... 1214

8.2.10.13 Inputting decimal point position data of customize data............................. 1215

8.2.10.14 Outputting decimal point position data of customize data.......................... 1216

8.2.10.15 Inputting tool geometry data....................................................................... 1217

8.2.10.16 Outputting tool geometry data ....................................................................1218

8.2.11 Inputting and Outputting Workpiece Setting Error Compensation Value .........1219

8.2.11.1 Inputting values on the workpiece setting error compensation screen........ 1219

c-11

TABLE OF CONTENTS B-64484EN/03

8.2.11.2 Outputting values on the workpiece setting error compensation screen..... 1220

8.2.11.3 Input/output format of workpiece setting error values................................ 1221

8.2.12 Inputting and Outputting Tool Life Management Data......................................1222

8.2.12.1 Inputting tool life management data ...........................................................1222

8.2.12.2 Outputting tool life management data......................................................... 1223

8.3 INPUT/OUTPUT ON THE ALL IO SCREEN............................................ 1224

8.3.1 Inputting/Outputting a Program .........................................................................1227

8.3.2 Inputting/Outputting all Programs and Folders ..................................................1229

8.3.3 Inputting and Outputting Parameters..................................................................1231

8.3.4 Inputting and Outputting Offset Data.................................................................1232

8.3.5 Inputting/Outputting Pitch Error Compensation Data........................................1234

8.3.6 Inputting/Outputting Custom Macro Common Variables ..................................1235

8.3.7 Inputting and Outputting Workpiece Coordinates System Data ........................1237

8.3.8 Inputting and Outputting Operation History Data..............................................1238

8.3.9 Inputting and Outputting Tool Management Data .............................................1239

8.3.10 Inputting and Outputting All Tool Management Data at a Time .......................1244

8.3.11 Inputting and Outputting Workpiece Setting Error Compensation Value .........1247

8.3.12 File Format and Error Messages.........................................................................1248

8.4 EMBEDDED ETHERNET OPERATIONS................................................1249

8.4.1 FTP File Transfer Function ................................................................................1249

8.5 SCREEN HARD COPY FUNCTION ........................................................ 1255

8.6 USB FUNCTION......................................................................................1256

9 CREATING PROGRAMS.................................................................. 1258

9.1 CREATING PROGRAMS USING THE MDI PANEL................................ 1258

9.2 AUTOMATIC INSERTION OF SEQUENCE NUMBERS ......................... 1259

9.3 CREATING PROGRAMS IN TEACH IN MODE (PLAYBACK) ................ 1260

10 EDITING PROGRAMS ...................................................................... 1263

10.1 EDIT DISABLE ATTRIBUTE AND DISPLAY DISABLE ATTRIBUTE ...... 1263

10.2 INSERTING, ALTERING AND DELETING A WORD .............................. 1264

10.2.1 Word Search.......................................................................................................1265

10.2.2 Heading a Program.............................................................................................1267

10.2.3 Inserting a Word.................................................................................................1267

10.2.4 Altering a Word..................................................................................................1268

10.2.5 Deleting a Word .................................................................................................1268

10.3 REPLACING A WORD OR ADDRESS.................................................... 1269

10.4 DELETING BLOCKS ............................................................................... 1271

10.4.1 Deleting a Block.................................................................................................1271

10.4.2 Deleting Multiple Blocks ...................................................................................1271

10.5 PROGRAM SEARCH .............................................................................. 1272

10.6 SEQUENCE NUMBER SEARCH ............................................................ 1273

10.7 DELETING PROGRAMS......................................................................... 1275

10.7.1 Deleting One Program........................................................................................1275

10.7.2 Deleting All Programs........................................................................................1275

10.8 EDITING OF CUSTOM MACROS........................................................... 1275

10.9 CURSOR MOVEMENT LIMITATIONS ON PROGRAM EDITING...........1276

10.10 PASSWORD FUNCTION ........................................................................ 1277

10.11 EDITING PROGRAM CHARACTERS..................................................... 1279

10.11.1 Available Keys ...................................................................................................1281

10.11.2 Input Mode .........................................................................................................1282

10.11.3 Line Number Display .........................................................................................1282

c-12

B-64484EN/03 TABLE OF CONTENTS

10.11.4 Search .................................................................................................................1282

10.11.5 Replacement .......................................................................................................1283

10.11.6 Reversing Edit Operations (Undo Function)......................................................1284

10.11.7 Copy ...................................................................................................................1284

10.11.8 Cut ......................................................................................................................1284

10.11.9 Paste ...................................................................................................................1284

10.11.10 Saving.................................................................................................................1285

10.11.11 Creation ..............................................................................................................1285

10.11.12 Line Search.........................................................................................................1285

10.12 PROGRAM COPY FUNCTION................................................................1286

10.12.1 Copying and Moving Files between Devices.....................................................1287

10.13 KEYS AND PROGRAM ENCRYPTION................................................... 1290

10.14 SIMULTANEOUS EDITING OF MULTIPATH PROGRAMS.................... 1293

10.15 MULTI-PATH EDITING FUNCTION ........................................................ 1296

10.15.1 Overview ............................................................................................................1296

10.15.2 Details.................................................................................................................1296

11 PROGRAM MANAGEMENT .............................................................1301

11.1 SELECTING A DEVICE........................................................................... 1302

11.1.1 Selecting a Memory Card Program as a Device.................................................1302

11.1.2 Selecting a From Cassette as a Device ...............................................................1306

11.1.3 Selecting a USB Memory as a Device................................................................1307

11.2 CREATING A FOLDER ........................................................................... 1308

11.3 RENAMING A FOLDER ..........................................................................1309

11.4 CHANGING CURRENT FOLDER ...........................................................1309

11.5 CHANGING FOLDER ATTRIBUTES....................................................... 1311

11.6 DELETING A FOLDER............................................................................ 1311

11.7 SELECTING A DEFAULT FOLDER ........................................................ 1312

11.8 RENAMING A FILE .................................................................................1313

11.9 DELETING A FILE................................................................................... 1313

11.10 CHANGING FILE ATTRIBUTES..............................................................1314

11.11 SELECTING A MAIN PROGRAM............................................................ 1315

11.12 PROGRAM AND FOLDER COPY/MOVE FUNCTION ............................ 1315

11.12.1 Copy and movement between different devices.................................................1318

11.13 FOLDER MANAGEMENT .......................................................................1319

11.13.1 Program Management under the Path Folder.....................................................1321

11.13.2 Program Management only in the Path Folder...................................................1322

11.13.3 Folder for Subprogram/Macro Calls ..................................................................1324

11.14 PROGRAM VERIFICATION.................................................................... 1324

12 SETTING AND DISPLAYING DATA................................................. 1326

12.1 SCREENS DISPLAYED BY FUNCTION KEY ................................. 1344

12.1.1 Position Display in the Workpiece Coordinate System .....................................1344

12.1.2 Position Display in the Relative Coordinate System..........................................1346

12.1.3 Overall Position Display ....................................................................................1349

12.1.4 Workpiece Coordinate System Preset ................................................................1350

12.1.5 Actual Feedrate Display .....................................................................................1351

12.1.6 Display of Run Time and Parts Count................................................................1353

12.1.7 Setting the Floating Reference Position .............................................................1355

12.1.8 Operating Monitor Display ................................................................................1355

c-13

TABLE OF CONTENTS B-64484EN/03

12.1.9 Display of 3-dimensional Manual Feed (Tool Tip Coordinates, Number of

Pulses, Machine Axis Move Amount)................................................................1357

12.1.10 Overall Position Display (15/19-inch Display Unit)..........................................1360

12.1.11 Workpiece Coordinate System Preset (15/19-inch Display Unit)......................1363

12.1.12 Actual Feedrate Display (15/19-inch Display Unit)...........................................1363

12.1.13 Display of Run Time and Parts Count (15/19-inch Display Unit) .....................1365

12.1.14 Setting the Floating Reference Position (15/19-inch Display Unit)...................1367

12.1.15 Operating Monitor Display (15/19-inch Display Unit)......................................1367

12.1.16 Display of 3-dimensional Manual Feed (Tool Tip Coordinates, Number of

Pulses, Machine Axis Move Amount) (15/19-inch Display Unit) .....................1369

12.2 SCREENS DISPLAYED BY FUNCTION KEY ................................. 1372

12.2.1 Program Contents Display..................................................................................1372

12.2.1.1 Displaying the executed block .................................................................... 1373

12.2.1.2 Text display................................................................................................. 1375

12.2.2 Editing a Program...............................................................................................1376

12.2.3 Program Screen for MDI Operation ...................................................................1377

12.2.4 Program Folder Screen.......................................................................................1378

12.2.4.1 Split display on the program folder screen .................................................1379

12.2.4.2 Folder tree display....................................................................................... 1383

12.2.5 Next Block Display Screen ................................................................................1385

12.2.6 Program Check Screen .......................................................................................1386

12.2.7 Background Editing............................................................................................1386

12.2.8 Stamping the Machining Time ...........................................................................1392

12.2.9 Screen for Assistance in Entering Tilted Working Plane Indexing....................1399

12.2.9.1 Command type selection screen.................................................................. 1405

12.2.9.2 Tilted working plane data setting screen..................................................... 1406

12.2.9.3 Details of the tilted working plane data setting screen................................ 1409

12.2.9.4 Limitation.................................................................................................... 1416

12.2.10 Program Contents Display (15/19-inch Display Unit) .......................................1416

12.2.10.1 Displaying the executed block .................................................................... 1417

12.2.11 Editing a Program (15/19-inch Display Unit) ....................................................1417

12.2.12 Program Screen for MDI Operation (15/19-inch Display Unit).........................1419

12.2.13 Program Folder Screen (15/19-inch Display Unit) ............................................1419

12.2.13.1 Split display on the program folder screen .................................................1420

12.2.13.2 Folder tree display (15/19-inch display unit).............................................. 1424

12.2.14 Next Block Display Screen (15/19-inch Display Unit)......................................1424

12.2.15 Program Check Screen (15/19-inch Display Unit).............................................1425

12.2.16 Background Editing (15/19-inch Display Unit) .................................................1426

12.2.17 Stamping the Machining Time (15/19-inch Display Unit).................................1431

12.2.18 Screen for Assistance in Entering Tilted Working Plane Indexing (15/19-inch

Display Unit) ......................................................................................................1439

12.2.18.1 Command type selection screen.................................................................. 1445

12.2.18.2 Tilted working plane data setting screen..................................................... 1446

12.2.18.3 Details of the tilted working plane data setting screen................................ 1449

12.2.18.4 Limitation.................................................................................................... 1456

12.3 SCREENS DISPLAYED BY FUNCTION KEY ................................. 1457

12.3.1 Displaying and Entering Setting Data ................................................................1458

12.3.2 Sequence Number Comparison and Stop ...........................................................1461

12.3.3 Displaying and Setting Run Time, Parts Count, and Time ................................1462

12.3.4 Displaying and Setting the Workpiece Origin Offset Value ..............................1464

12.3.5 Direct Input of Workpiece Origin Offset Value Measured ................................1465

12.3.6 Displaying and Setting Custom Macro Common Variables...............................1466

12.3.7 Displaying and Setting Real Time Custom Macro Data ....................................1468

12.3.8 Displaying and Setting the Software Operator’s Panel ......................................1469

c-14

B-64484EN/03 TABLE OF CONTENTS

12.3.9 Setting and Displaying Tool Management Data ................................................1472

12.3.9.1 Displaying and setting magazine screen ..................................................... 1472

12.3.9.2 Displaying and setting tool management screen......................................... 1473

12.3.9.3 Each tool data screen .................................................................................. 1478

12.3.9.4 Displaying the total life of tools of the same type....................................... 1481

12.3.9.5 Tool geometry data screen .......................................................................... 1484

12.3.10 Displaying and Switching the Display Language ..............................................1488

12.3.11 Protection of Data at Eight Levels......................................................................1490

12.3.11.1 Operation level setting ................................................................................ 1490

12.3.11.2 Password modification................................................................................ 1491

12.3.11.3 Protection level setting................................................................................ 1493

12.3.11.4 Setting the change protection level and output protection level of

a program .................................................................................................... 1495

12.3.12 Precision Level Selection ...................................................................................1496

12.3.13 Machining Level Selection.................................................................................1498

12.3.13.1 Smoothing level selection ........................................................................... 1498

12.3.13.2 Precision level selection.............................................................................. 1499

12.3.14 Machining Quality Level Selection....................................................................1499

12.3.15 Displaying and Setting Tool Life Management Data.........................................1500

12.3.15.1 Tool life management (list screen).............................................................. 1502

12.3.15.2 Tool life management (group editing screen) ............................................. 1505

12.3.16 Displaying and Setting Workpiece Setting Error Compensation Data...............1511

12.3.17 Displaying and Setting Pattern Data Inputs........................................................1512

12.3.18 Setting and Displaying Data When the Tool Offset for Milling and Turning

Function Is Enabled............................................................................................1514

12.3.19 Displaying and Entering Setting Data (15/19-inch Display Unit)......................1517

12.3.20 Sequence Number Comparison and Stop (15/19-inch Display Unit).................1519

12.3.21 Displaying and Setting Run Time, Parts Count, and Time (15/19-inch Display

Unit) ...................................................................................................................1521

12.3.22 Displaying and Setting the Workpiece Origin Offset Value (15/19-inch Display

Unit) ...................................................................................................................1523

12.3.23 Direct Input of Workpiece Origin Offset Value Measured (15/19-inch Display

Unit) ...................................................................................................................1524

12.3.24 Displaying and Setting Custom Macro Common Variables (15/19-inch Display

Unit) ...................................................................................................................1525

12.3.25 Displaying and Setting Real Time Custom Macro Data (15/19-inch Display

Unit) ...................................................................................................................1527

12.3.26 Displaying and Setting the Software Operator’s Panel (15/19-inch Display

Unit) ...................................................................................................................1528

12.3.27 Setting and Displaying Tool Management Data (15/19-inch Display Unit)......1531

12.3.27.1 Displaying and setting magazine screen (15-inch display unit).................. 1531

12.3.27.2 Displaying and setting tool management screen (15-inch display unit) .....1532

12.3.27.3 Each tool data screen (15-inch display unit)............................................... 1538

12.3.27.4 Displaying the total life of tools of the same type (15-inch display unit)... 1540

12.3.27.5 Tool geometry data screen (15-inch display unit)....................................... 1544

12.3.28 Displaying and Switching the Display Language (15/19-inch Display Unit)....1549

12.3.29 Protection of Data at Eight Levels (15/19-inch Display Unit)...........................1550

12.3.29.1 Operation level setting (15-inch display unit)............................................. 1550

12.3.29.2 Password modification (15-inch display unit) ............................................1552

12.3.29.3 Protection level setting (15-inch display unit) ............................................ 1553

12.3.29.4 Setting the change protection level and output protection level of

a program (15-inch display unit)................................................................. 1555

12.3.30 Precision Level Selection (15/19-inch Display Unit).........................................1556

12.3.31 Machining Level Selection (15/19-inch Display Unit) ......................................1558

12.3.31.1 Smoothing level selection ........................................................................... 1558

12.3.31.2 Precision level selection.............................................................................. 1559

c-15

TABLE OF CONTENTS B-64484EN/03

12.3.32 Machining Quality Level Selection (15/19-inch Display Unit) .........................1559

12.3.33 Displaying and Setting Tool Life Management Data (15/19-inch Display Unit)1561

12.3.33.1 Tool life management (list screen) (15-inch display unit) .......................... 1562

12.3.33.2 Tool life management (group editing screen) (15-inch display unit).......... 1565

12.3.34 Displaying and Setting Workpiece Setting Error Compensation Data

(15/19-inch Display Unit) ..................................................................................1572

12.3.35 Displaying and Setting Pattern Data Inputs (15/19-inch Display Unit).............1573

12.3.36 Built-in 3D Interference Check ..........................................................................1576

12.3.36.1 Monitor menu screen ..................................................................................1576

12.3.36.2 Tool monitor screen .................................................................................... 1579

12.3.36.3 Tool holder and object monitor screen ....................................................... 1580

12.3.36.4 Figure setting menu screen ......................................................................... 1581

12.3.36.5 Object figure setting screen......................................................................... 1582

12.3.36.6 Tool holder figure setting screen ................................................................ 1585

12.3.36.7 Rectangular parallelepiped setting screen................................................... 1601

12.3.36.8 Cylinder setting screen................................................................................ 1602

12.3.36.9 Plane setting screen..................................................................................... 1603

12.3.36.10 Shape number list screen............................................................................. 1605

12.3.36.11 Interference check valid figure selection screen......................................... 1607

12.3.36.12 Moving axis setting menu screen and moving axis setting screen.............. 1609

12.3.36.13 Setting screens ............................................................................................ 1612

12.3.36.14 Name setting screen .................................................................................... 1612

12.3.36.15 Display setting screen ................................................................................. 1614

12.3.36.16 Drawing coordinate system setting screen.................................................. 1615

12.3.36.17 Input and output setting data for 3D interference check ............................. 1617

12.3.37 Setting and Displaying Data When the Tool Offset for Milling and Turning

Function Is Enabled (15/19-inch Display Unit) .................................................1624

12.4 SCREENS DISPLAYED BY FUNCTION KEY ................................. 1627

12.4.1 Displaying and Setting Parameters.....................................................................1627

12.4.2 Servo Parameters................................................................................................1630

12.4.3 Servo Tuning ......................................................................................................1631

12.4.4 Spindle Setting ...................................................................................................1632

12.4.5 Spindle Tuning ...................................................................................................1633

12.4.6 Spindle Monitor..................................................................................................1634

12.4.7 Color Setting Screen...........................................................................................1635

12.4.8 Machining Parameter Tuning.............................................................................1636

12.4.8.1 Machining parameter tuning (AI contour) .................................................. 1636

12.4.8.2 Machining parameter tuning (nano smoothing).......................................... 1642

12.4.9 Displaying Memory Data ...................................................................................1644

12.4.10 Parameter Tuning Screen ...................................................................................1646

12.4.10.1 Displaying the menu screen and selecting a menu item.............................. 1646

12.4.10.2 Parameter tuning screen (system setting).................................................... 1649

12.4.10.3 Parameter tuning screen (axis setting) ........................................................1650

12.4.10.4 Displaying and setting the FSSB servo amplifier setting screen................. 1651

12.4.10.5 Displaying and setting the FSSB spindle amplifier setting screen.............. 1651

12.4.10.6 Displaying and setting the FSSB axis setting screen ..................................1652

12.4.10.7 Displaying and setting the servo setting screen ..........................................1652

12.4.10.8 Parameter tuning screen (spindle setting) ................................................... 1653

12.4.10.9 Parameter tuning screen (miscellaneous settings)....................................... 1653

12.4.10.10 Displaying and setting the servo tuning screen........................................... 1654

12.4.10.11 Displaying and setting the spindle tuning screen........................................ 1654

12.4.10.12 Displaying and setting the machining parameter tuning screen.................. 1655

12.4.11 Periodic Maintenance Screen .............................................................................1658

12.4.12 System Configuration Screen.............................................................................1667

12.4.13 Power Consumption Monitoring Screen ............................................................1669

12.4.14 Displaying and Setting Parameters (15/19-inch Display Unit) ..........................1672

c-16

B-64484EN/03 TABLE OF CONTENTS

12.4.15 Servo Parameters (15/19-inch Display Unit) .....................................................1674

12.4.16 Servo Tuning (15/19-inch Display Unit)............................................................1675

12.4.17 Spindle Setting (15/19-inch Display Unit).........................................................1676

12.4.18 Spindle Tuning (15/19-inch Display Unit).........................................................1677

12.4.19 Spindle Monitor (15/19-inch Display Unit) .......................................................1678

12.4.20 Color Setting Screen (15/19-inch Display Unit) ................................................1679

12.4.21 Machining Parameter Tuning (15/19-inch Display Unit)...................................1680

12.4.21.1 Machining parameter tuning (AI contour) .................................................. 1680

12.4.21.2 Machining parameter tuning (nano smoothing).......................................... 1685

12.4.22 Displaying Memory Data (15/19-inch Display Unit).........................................1687

12.4.23 Parameter Tuning Screen (15/19-inch Display Unit).........................................1690

12.4.23.1 Displaying the menu screen and selecting a menu item (15/19-inch display

unit)............................................................................................................. 1690

12.4.23.2 Parameter tuning screen (system setting) (15/19-inch display unit)........... 1693

12.4.23.3 Parameter tuning screen (axis setting) (15/19-inch display unit)................ 1694

12.4.23.4 Displaying and setting the FSSB servo amplifier setting screen

(15/19-inch display unit)............................................................................. 1695

12.4.23.5 Displaying and setting the FSSB spindle amplifier setting screen

(15/19-inch display unit)............................................................................. 1695

12.4.23.6 Displaying and setting the FSSB axis setting screen (15/19-inch display

unit)............................................................................................................. 1696

12.4.23.7 Displaying and setting the servo setting screen (15/19-inch display unit).. 1696

12.4.23.8 Parameter tuning screen (spindle setting) (15/19-inch display unit)........... 1697

12.4.23.9 Parameter tuning screen (miscellaneous settings) (15/19-inch display unit)1697

12.4.23.10 Displaying and setting the servo tuning screen (15/19-inch display unit) .. 1698

12.4.23.11 Displaying and setting the spindle tuning screen (15/19-inch display unit)1698

12.4.23.12 Displaying and setting the machining parameter tuning screen (15/19-inch

display unit) ................................................................................................ 1699

12.4.24 Periodic Maintenance Screen (15/19-inch Display Unit)...................................1703

12.4.25 System Configuration Screen (15/19-inch Display Unit) ..................................1710

12.4.26 Power Consumption Monitoring Screen (15/19-inch Display Unit)..................1713

12.5 SCREENS DISPLAYED BY FUNCTION KEY ................................. 1715

12.5.1 External Operator Message History ...................................................................1715

12.6 SWITCHING BETWEEN MULTI-PATH DISPLAY AND SINGLE-PATH

DISPLAY FUNCTION .............................................................................. 1718

12.7 FIVE AXES DISPLAY IN ONE SCREEN FOR THE 8.4-INCH DISPLAY

UNIT ........................................................................................................ 1722

12.8 PATH NAME EXPANSION DISPLAY FUNCTION ..................................1725

12.9 SCREEN ERASURE FUNCTION AND AUTOMATIC SCREEN

ERASURE FUNCTION............................................................................ 1727

12.10 LOAD METER SCREEN .........................................................................1729

12.10.1 Single-path Display ............................................................................................1729

12.10.2 Two-path Display and Three-path Display ........................................................1730

12.11 DISPLAYING THE PROGRAM NUMBER/NAME, SEQUENCE NUMBER,
AND STATUS, AND WARNING MESSAGES FOR DATA SETTING OR

INPUT/OUTPUT OPERATION ................................................................ 1734

12.11.1 Displaying the Program Number, Program Name, and Sequence Number........1734

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

Operation............................................................................................................1735

12.11.3 Displaying the Program Number, Program Name, and Sequence Number

(15/19-inch Display Unit) ..................................................................................1738

12.11.4 Displaying the Program Name ...........................................................................1739

c-17

TABLE OF CONTENTS B-64484EN/03

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

(15/19-inch Display Unit) ..................................................................................1740

13 GRAPHIC FUNCTION.......................................................................1743

13.1 GRAPHIC DISPLAY ................................................................................ 1743

13.2 DYNAMIC GRAPHIC DISPLAY...............................................................1754

13.2.1 Path Drawing......................................................................................................1754

13.2.1.1 GRAPHIC PARAMETER (DYNAMIC GRAPHIC) screen...................... 1754

13.2.1.2 PATH GRAPHIC screen ............................................................................1759

13.2.1.3 PATH GRAPHIC (TOOL POSITION) screen........................................... 1765

13.2.2 Animation...........................................................................................................1767

13.2.2.1 GRAPHIC PARAMETER (DYNAMIC GRAPHIC) screen...................... 1767

13.2.2.2 ANIMATION GRAPHIC screen................................................................ 1770

13.2.3 Programmable Data Input (G10) for Blank Figure Drawing Parameters...........1776

13.2.4 Warning Messages .............................................................................................1777

13.2.5 Note ....................................................................................................................1778

13.2.6 Restrictions.........................................................................................................1778

14 VIRTUAL MDI KEY FUNCTION........................................................1786

14.1 VIRTUAL MDI KEY.................................................................................. 1786

14.1.1 Limitations..........................................................................................................1789

15 TEMPLATE PROGRAM FUNCTION ................................................1790

15.1 Template Program Function .................................................................... 1790

15.1.1 Details.................................................................................................................1790

15.1.2 Operation............................................................................................................1794

15.1.3 Protection Function ............................................................................................1798

15.1.4 Limitations..........................................................................................................1800

16 MULTI-PATH PROGRAM MANAGEMENT FUNCTION................... 1801

16.1 MULTI-PATH PROGRAM MANAGEMENT FUNCTION.......................... 1801

16.1.1 Details.................................................................................................................1801

16.1.1.1 Multi-path program folder ..........................................................................1802

16.1.1.2 Making of machining programs.................................................................. 1802

16.1.1.3 Edit of multi-path program .........................................................................1804

16.1.1.4 Selection of machining program................................................................. 1804

16.1.1.5 Input/output of Multi-path program............................................................ 1805

16.1.1.6 Name change of the multi-path program folder.......................................... 1808

16.1.2 Operation of inputting and editing for each program.........................................1808

16.1.3 Limitations..........................................................................................................1810

IV. MAINTENANCE

1 ROUTINE MAINTENANCE ............................................................... 1813

1.1 ACTION TO BE TAKEN WHEN A PROBLEM OCCURRED ................... 1814

1.2 BACKING UP VARIOUS DATA ITEMS...................................................1815

1.3 METHOD OF REPLACING BATTERY ....................................................1817

1.3.1 Replacing Battery for Control Unit ....................................................................1818

1.3.2 Battery in the PANEL i (3 VDC) .......................................................................1821

1.3.3 Replacing Battery for Absolute Pulsecoders ......................................................1822

1.3.3.1 Overview..................................................................................................... 1822

1.3.3.2 Replacing batteries ...................................................................................... 1822

1.3.3.3 Replacing the batteries in a separate battery case ....................................... 1823

1.3.3.4 Replacing the battery built into the servo amplifier.................................... 1823

c-18

B-64484EN/03 TABLE OF CONTENTS

APPENDIX

A PARAMETERS.................................................................................. 1827

A.1 DESCRIPTION OF PARAMETERS......................................................... 1827

A.2 DATA TYPE............................................................................................. 2146

A.3 STANDARD PARAMETER SETTING TABLES....................................... 2147

B PROGRAM CODE LIST.................................................................... 2149

C LIST OF FUNCTIONS AND PROGRAM FORMAT ..........................2152

D RANGE OF COMMAND VALUE.......................................................2164

E NOMOGRAPHS ................................................................................ 2167

E.1 INCORRECT THREADED LENGTH .......................................................2167

E.2 SIMPLE CALCULATION OF INCORRECT THREAD LENGTH .............. 2168

E.3 TOOL PATH AT CORNER ...................................................................... 2170

E.4 RADIUS DIRECTION ERROR AT CIRCLE CUTTING ............................ 2173

F SETTINGS AT POWER-ON, IN THE CLEAR STATE, OR IN

THE RESET STATE.......................................................................... 2174

G CHARACTER-TO-CODES CORRESPONDENCE TABLE ..............2177

G.1 CHARACTER-TO-CODES CORRESPONDENCE TABLE...................... 2177

G.2 FANUC DOUBLE-BYTE CHARACTER CODE TABLE ...........................2178

H ALARM LIST .....................................................................................2184

I PC TOOL FOR MEMORY CARD PROGRAM

OPERATION/EDITING...................................................................... 2266

I.1 PC TOOL FOR MEMORY CARD PROGRAM OPERATION/EDITING ... 2266

I.1.1 Usage Notes........................................................................................................2266

I.1.2 List of Functions of PC Tool..............................................................................2266

I.1.3 Explanation of Operations..................................................................................2267

I.2 NAMING RULES .....................................................................................2275

I.2.1 Naming Rules of Program File...........................................................................2275

I.2.2 Naming Rules of Folder .....................................................................................2275

I.3 RULES OF CHARACTERS IN PROGRAM FILE..................................... 2276

I.3.1 Usable Characters in Program File.....................................................................2276

I.4 ERROR MESSAGE AND NOTE.............................................................. 2277

I.4.1 List of Error Message.........................................................................................2277

I.4.2 Note ....................................................................................................................2278

J ISO/ASCII CODE CONVERSION TOOL...........................................2279

c-19

I. GENERAL

B-64484EN/03 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 OPERATOR’S MANUAL (Lathe System) (B-64484EN-1) or
the OPERATOR’S MANUAL (Machining Center System) (B-64484EN-2).

2 Some functions described in this manual may not be applied to some products.

For detail, refer to the Descriptions manual (B-64482EN).

3 This manual does not detail the parameters not mentioned in the text. For details

of those parameters, refer to the Parameter Manual (B-64490EN).

Parameters are used to set functions and operating conditions of a CNC

machine tool, and frequently-used values in advance. Usually, the machine tool
builder factory-sets parameters so that the user can use the machine tool easily.

4 This manual describes not only basic functions but also optional functions. Look

up the options incorporated into your system in the manual written by the
machine tool builder.

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-B 30i –B Series 30i
FANUC Series 31i-B 31i –B
FANUC Series 31i-B5 31i –B5
FANUC Series 32i-B 32i –B Series 32i

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

Series 31i

- 3 -

1.GENERAL GENERAL B-64484EN/03

NOTE

2 Unless otherwise noted, the model names 31i-B, 31i-B5, and 32i-B are

collectively referred to as 30i. 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-64482EN).

Special symbols

This manual uses the following symbols:

M

-

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".

-

T

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.

- IP

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

- ;

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

Related manuals of
Series 30i- MODEL B
Series 31i- MODEL B
Series 32i- MODEL B

The following table lists the manuals related to Series 30i-B, Series 31i-B, Series 32i-B. This manual is
indicated by an asterisk(*).

Table 1 Related manuals

Manual name Specification number

DESCRIPTIONS B-64482EN
CONNECTION MANUAL (HARDWARE) B-64483EN
CONNECTION MANUAL (FUNCTION) B-64483EN-1
OPERATOR’S MANUAL (Common to Lathe System/Machining Center System) B-64484EN *
OPERATOR’S MANUAL (For Lathe System) B-64484EN-1
OPERATOR’S MANUAL (For Machining Center System) B-64484EN-2

- 4 -

B-64484EN/03 GENERAL 1.GENERAL

Manual name Specification number

MAINTENANCE MANUAL B-64485EN
PARAMETER MANUAL B-64490EN

Programming

Macro Executor PROGRAMMING MANUAL B-63943EN-2
Macro Compiler PROGRAMMING MANUAL B-66263EN
C Language Executor PROGRAMMING MANUAL B-63943EN-3

PMC

PMC PROGRAMMING MANUAL B-64513EN

Network

PROFIBUS-DP Board CONNECTION MANUAL B-63993EN
Fast Ethernet / Fast Data Server OPERATOR’S MANUAL B-64014EN
DeviceNet Board CONNECTION MANUAL B-64043EN
FL-net Board CONNECTION MANUAL B-64163EN
CC-Link Board CONNECTION MANUAL B-64463EN

Operation guidance function

MANUAL GUIDE i (Common to Lathe System/Machining Center System)
OPERATOR’S MANUAL
MANUAL GUIDE i (For Machining Center System) OPERATOR’S MANUAL
MANUAL GUIDE i (Set-up Guidance Functions) OPERATOR’S MANUAL

Dual Check Safety

Dual Check Safety CONNECTION MANUAL B-64483EN-2

B-63874EN

B-63874EN-2
B-63874EN-1

Related manuals of SERVO MOTOR αi/βi series

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

Table 2 Related manuals

Manual name Specification number

FANUC AC SERVO MOTOR αi series DESCRIPTIONS
FANUC AC SPINDLE MOTOR αi series DESCRIPTIONS
FANUC AC SERVO MOTOR βi 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 αi series
FANUC AC SERVO MOTOR βi series
FANUC LINEAR MOTOR LiS series
FANUC SYNCHRONOUS BUILT-IN SERVO MOTOR DiS series PARAMETER
MANUAL
FANUC AC SPINDLE MOTOR αi/βi series,
BUILT-IN SPINDLE MOTOR Bi series
PARAMETER MANUAL

The above servo motors and the corresponding spindles can be connected to the CNC covered in this
manual. In the αi SV, αi SP, αi PS, and βi SV series, however, they can be connected only to 30 i-B-
compatible versions. In the βi SVSP series, they cannot be connected.

B-65262EN
B-65272EN
B-65302EN
B-65312EN
B-65282EN
B-65322EN

B-65285EN

B-65325EN

B-65270EN

B-65280EN

- 5 -

1.GENERAL GENERAL B-64484EN/03

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.

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.

The number of times to write machining programs to the non-volatile memory is

limited.

You must use "High-speed program management" when registration and the

deletion of the machining programs are frequently repeated in such case that the

machining programs are automatically downloaded from a personal computer at

each machining.

In "High-speed program management", the program is not saved to the non-

volatile memory at registration, modification, or deletion of programs.

- 6 -

II. PROGRAMMING

B-64484EN/03 PROGRAMMING 1.GENERAL

X

1 GENERAL

Chapter 1, "GENERAL", consists of the following sections:

1.1 TOOL MOVEMENT ALONG WORKPIECE PARTS FIGURE-INTERPOLATION .......................9

1.2 FEED-FEED FUNCTION ..................................................................................................................11

1.3 PART DRAWING AND TOOL MOVEMENT.................................................................................12

1.4 CUTTING SPEED - SPINDLE FUNCTION .....................................................................................21

1.5 SELECTION OF TOOL USED FOR VARIOUS MACHINING - TOOL FUNCTION ...................22

1.6 COMMAND FOR MACHINE OPERATIONS - AUXILIARY FUNCTION...................................23

1.7 PROGRAM CONFIGURATION .......................................................................................................24

1.8 TOOL MOVEMENT RANGE - STROKE ........................................................................................26

1.1 TOOL MOVEMENT ALONG WORKPIECE PARTS FIGURE-

INTERPOLATION

The tool moves along straight lines and arcs constituting the workpiece parts figure (See Chapter,
“INTERPOLATION FUNCTIONS”).

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

Tool

Workpiece

Tool

Program
G01X_Y_ ;
X_ ;

Program
G01Z_ ;
G01X_Z_ ;

Workpiece

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

- 9 -

Z

1.GENERAL PROGRAMMING B-64484EN/03

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.

- 10 -

B-64484EN/03 PROGRAMMING 1.GENERAL

1.2 FEED-FEED FUNCTION

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

• For milling machining (feed per minute)

mm/min

F

Workpiece

Table

Tool

• For lathe cutting (feed per revolution)

F

Fig. 1.2 (a) Feed function

Feed amount per minute

(mm/rev)

For example, to feed the tool at a rate of 150 mm/min (feed per minute) or 150 mm/rev (feed per
revolution), specify the following in the program:
F150.0
The function of deciding the feed rate is called the feed function (See Chapter, “FEED FUNCTIONS”).

- 11 -

1.GENERAL PROGRAMMING B-64484EN/03

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

Table

• For lathe cutting

Tool post

Chuck

Fig. 1.3.1 (a) Reference position

Reference
position

Explanation

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

1. Manual reference position return (See Section, “MANUAL REFERENCE POSITION RETURN”)
Reference position return is performed by manual button operation.

2. Automatic reference position return (See Section, “REFERENCE POSITION RETURN”)
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.

- 12 -

B-64484EN/03 PROGRAMMING 1.GENERAL

1.3.2 Coordinate System on Part Drawing and Coordinate System

Specified by CNC - Coordinate System

• For milling machining

Z

Z

• For lathe cutting

X

Y

Part drawing

Program

X

Tool

Z

Workpiece

Machine tool

Y

X

Coordinate system

CNC

Command

Tool

Y

X

X

Part drawing

Program

Z

Z

Coordinate system

CNC

Command

X

Workpiece

Z

Machine tool

Fig. 1.3.2 (a) Coordinate system

- 13 -

1.GENERAL PROGRAMMING B-64484EN/03

Explanation

- Coordinate system

The following two coordinate systems are specified at different locations:
(See Chapter, “ COORDINATE SYSTEM”)
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
Chapter, “ COORDINATE SYSTEM”
The positional relation between these two coordinate systems is determined when a workpiece is set on
the table.

- 14 -

B-64484EN/03 PROGRAMMING 1.GENERAL

• For milling machining

Coordinate system on
part drawing estab

Coordinate system
specified by the CNC
established on the table

Table

Y

Y

Workpiece

lished on the workpiece

X

X

• For lathe cutting

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.

- 15 -

1.GENERAL PROGRAMMING B-64484EN/03

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.

2. Mounting a workpiece directly against the jig

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

Workpiece's
standard point

Fixed distance

X

Program origin

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)).

- 16 -

B-64484EN/03 PROGRAMMING 1.GENERAL

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

Chuck

X

40

X

Program origin

Workpiece

60 40

150

Workpiece

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.

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

- Coordinates and
dimensions on part drawing

- Coordinate system on
lathe as specified by CNC

Chuck

60

Workpiece

100

Workpiece

80

X

30

Z

30

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.

- 17 -

1.GENERAL PROGRAMMING B-64484EN/03

A

X

A

1.3.3 How to Indicate Command Dimensions for Moving the Tool

(Absolute and Incremental Programming)

Explanation

Command for moving the tool can be indicated by absolute command or incremental command (See
Section, “ABSOLUTE AND INCREMENTAL PROGRAMMING”).

- 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

• For lathe cutting

Z

X

Command specifying movement from
point A to point B

X

Tool

Y

B(10.0,30.0,5.0)

G90 X10.0 Y30.0 Z5.0 ;

Coordinates of point B

Tool

Workpiece

φ

30

70

Command specifying movement from point A to
point B

B

Z

110

30.0Z70.0;

Coordinates of point B

- 18 -

B-64484EN/03 PROGRAMMING 1.GENERAL

A

A

φ

A

- Incremental command

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

• For milling machining

Z

Tool

• For lathe cutting

Z=-10.0

X

B

Y- 30 .0

Command specifying movement from
point A to point B

X

Workpiece

φ

30

B

X=40.0

Y

G91 X40.0 Y-30.0 Z-10.0 ;

Distance and direction for
movement along each axis

Tool

-30.0 (diameter value)

60

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

- 19 -

1.GENERAL PROGRAMMING B-64484EN/03

A

φ30ABφ

A

A

- Diameter programming / radius programming

Dimensions of the X-axis can be set in diameter or in radius. Which programming is used is determined
according to the setting of bit 3 (DIA) of parameter No. 1006.

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

Coordinate values of points A and B

Z

(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

80

Workpiece

Coordinate values of points A and B

Z

(15.0, 80.0), B(20.0, 60.0)

- 20 -

B-64484EN/03 PROGRAMMING 1.GENERAL

φ

φ

1

1.4 CUTTING SPEED - SPINDLE FUNCTION

Explanation

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

Tool

Spindle speed N

min

-1

Workpiece

Tool diameter

D mm

V: Cutting speed

m/min

<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

-1

, which is obtained from N=1000v/πD. Hence the following

command is required:
S250;
Commands related to the spindle speed are called the spindle speed function (See Chapter, “SPINDLE
SPEED FUNCTION (S FUNCTION)”).

• For lathe cutting

To ol

-1

unit.

Cutting speed

v m/min

Workpiece

Spindle speed

D

N min

-

<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 Chapter, “SPINDLE
SPEED FUNCTION (S FUNCTION)”).
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 Section, “CONSTANT
SURFACE SPEED CONTROL (G96, G97)”).

- 21 -

1.GENERAL PROGRAMMING B-64484EN/03

A

1.5 SELECTION OF TOOL USED FOR VARIOUS MACHINING -

TOOL FUNCTION

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 Chapter, “TOOL FUNCTION (T FUNCTION)”).

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 Chapter, “TOOL FUNCTION (T FUNCTION)”).

- 22 -

B-64484EN/03 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 Chapter, “AUXILIARY FUNCTION”).
For example, when M03 is specified, the spindle is rotated clockwise at the specified spindle speed.

- 23 -

1.GENERAL PROGRAMMING B-64484EN/03

A

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 Chapter,
“PROGRAM CONFIGURATION”).

Explanation

The block and the program have the following configurations.

- Block

1 block

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

Sequence
number

Preparatory
function

Dimension word

Fig. 1.7 (b) Block configuration

uxiliary

function

Spindle
function

Tool
function

End of block

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_.

- 24 -

B-64484EN/03 PROGRAMMING 1.GENERAL

- Program

;
Oxxxxx ;

Program number

Block

Block

Block

:

:

:

M30 ;

:

:

:

End of program

Fig. 1.7 (c) Program configuration

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.

- 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

- 25 -

1.GENERAL PROGRAMMING B-64484EN/03

y

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 area

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 Section, “STORED
STROKE CHECK”).

Motor

Limit
switch

Machine zero point

these distances.

Specif

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

- 26 -

B-64484EN/03 PROGRAMMING 2.CONTROLLED AXES

2 CONTROLLED AXES

Chapter 2, "CONTROLLED AXES", consists of the following sections:

2.1 NUMBER OF CONTROLLED AXES...............................................................................................27

2.2 NAMES OF AXES .............................................................................................................................27

2.3 INCREMENT SYSTEM.....................................................................................................................28

2.4 MAXIMUM STROKE........................................................................................................................29

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 (each axis)

(including Cs axes and PMC axes)
Controlled axes expansion (total)
(including Cs axes and PMC axes)
Basic simultaneously controlled axes
(each path)
Simultaneously controlled axes expansion
(total / each path)
Axis control by PMC (not available on Cs axis) Max. 32 axes Max. 16 axes Max. 16 axes Max. 8 axes
Designation of Spindle axes (each path ) Max. 4 axes Max. 4 axes Max. 4 axes Max. 2 axes
Designation of Spindle axes (total) Max. 8 axes Max. 6 axes Max. 6 axes Max. 2 axes
Cs contouring control (each path) Max. 4 axes Max. 4 axes Max. 4 axes Max. 2 axes
Cs contouring control (total) Max. 8 axes Max. 6 axes Max. 6 axes Max. 2 axes

Machining center system 3 axes 3 axes 3 axes 3 axes

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 bit
0 (JAX) of parameter No. 1002 is set to 0 and 3 when it is set to 1).

Series 30i-B Series 31i-B5 Series 31i-B Series 32i-B

Max. 24 axes Max. 12 axes Max. 12 axes Max. 5 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. 5 axes Max. 4 axes Max. 4 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)

- 27 -

2.CONTROLLED AXES PROGRAMMING B-64484EN/03

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.

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.
IS-C, IS-D, and IS-E are optional functions.

Table 2.3 (a) Increment system

Name of increment system Least input increment Least command increment

0.01 mm 0.01 mm

IS-A

IS-B

IS-C

IS-D

IS-E

The least command increment is either metric or inch depending on the machine tool. Set metric or inch
to the bit 0 (INM) of parameter No. 0100.
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.

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

- 28 -

B-64484EN/03 PROGRAMMING 2.CONTROLLED AXES

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” (B-64482EN).

2.4 MAXIMUM STROKE

Explanation

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

Table 2.4 (a) Maximum strokes

Name of increment system Least input increment Maximum stroke

0.01 mm ±999999.99 mm

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-64482EN).

0.001 inch ±99999.999 inch

0.01 deg ±999999.99 deg

0.001 mm ±999999.999 mm

0.0001 inch ±99999.9999 inch

0.001 deg ±999999.999 deg

0.0001 mm ±99999.9999 mm

0.00001 inch ±9999.99999 inch

0.0001 deg ±99999.9999 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

- 29 -

3. PREPARATORY FUNCTION
(G FUNCTION)

PROGRAMMING B-64484EN/03

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

(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 bits 6 (GSB) and 7 (GSC) of parameter No. 3401. To use G code system B or C, the corresponding
option is needed. Generally, OPERATOR’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.

Explanation

1. When the clear state (bit 6 (CLR) of parameter No. 3402) 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
(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 bit 7 (G23) of parameter No. 3402. However,

G22 and G23 remain unchanged when the clear state is set at reset.
(4) The user can select G00 or G01 by setting bit 0 (G01) of parameter No. 3402.
(5) The user can select G90 or G91 by setting bit 3 (G91) of parameter No. 3402.
When G code system B or C is used in the lathe system, setting bit 3 (G91) of parameter No.

3402 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 bits 1 (G18)

and 2 (G19) of parameter No. 3401.

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 bit 0 (MDL) of parameter No. 5431. (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.)

as indicated in Table.

- 30 -

3.PREPARATORY FUNCTION

B-64484EN/03 PROGRAMMING

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..

(G FUNCTION)

- 31 -

3. PREPARATORY FUNCTION
(G FUNCTION)

PROGRAMMING B-64484EN/03

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
G02.1, G03.1 Circular thread cutting B CW/CCW
G02.2, G03.2 Involute interpolation CW/CCW
G02.3, G03.3 Exponential interpolation CW/CCW
G02.4, G03.4
G04 Dwell

G05

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
G12.4 Groove cutting by continuous circle motion (CW)
G13.4
G15 Polar coordinates command cancel
G16
G17 XpYp plane selection
G17.1 Plane conversion function
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
G28.2 In-position check disable reference position return
G29 Movement from reference position
G30 2nd, 3rd and 4th reference position return
G30.1 Floating reference position return
G30.2 In-position check disable 2nd, 3rd, or 4th reference position return
G31 Skip function
G31.8

01

00

00

21

00

17

02

06

04

19

00

3-dimensional coordinate system conversion CW/CCW

AI contour control (high-precision contour control compatible command),
High-speed cycle machining, High-speed binary program operation

HRV3, 4 on/off

Programmable data input mode cancel

Polar coordinate interpolation cancel mode

Groove cutting by continuous circle motion (CCW)

Polar coordinates command

YpZp plane selection

Input in mm

Stored stroke check function off

Spindle speed fluctuation detection on

EGB-axis skip

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

- 32 -

3.PREPARATORY FUNCTION

B-64484EN/03 PROGRAMMING

Table 3.1 (a) G code list

G code Group Function

G33 Threading
G34 Variable lead threading
G35 Circular threading CW
G36
G37 Automatic tool length measurement
G38 Tool radius/tool nose radius compensation : preserve vector
G39

G40

G41

G41.2 3-dimensional cutter compensation : left (type 1)
G41.3 3-dimensional cutter compensation : leading edge offset
G41.4 3-dimensional cutter compensation : left (type 1) (FS16i-compatible command)
G41.5 3-dimensional cutter compensation : left (type 1) (FS16i-compatible command)
G41.6 3-dimensional cutter compensation : left (type 2)

G42

G42.2 3-dimensional cutter compensation : right (type 1)
G42.4 3-dimensional cutter compensation : right (type 1) (FS16i-compatible command)
G42.5 3-dimensional cutter compensation : 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 Tool length compensation ­G43.1 Tool length compensation in tool axis direction
G43.3 Nutating rotary head tool length compensation
G43.4 Tool center point control (type 1)
G43.5 Tool center point control (type 2)
G43.7 Tool offset
G44.1
G45 Tool offset : increase
G46 Tool offset : decrease
G47 Tool offset : double increase
G48
G49 (G49.1) 08 Tool length compensation cancel
G44.9 Spindle unit compensation
G49.9
G50 Scaling cancel
G51
G50.1 Programmable mirror image cancel
G51.1
G50.2 Polygon turning cancel
G51.2
G50.4 Cancel synchronous control
G50.5 Cancel composite control
G50.6 Cancel superimposed control
G51.4 Start synchronous control
G51.5 Start composite control
G51.6

01

00

07

18

08

00

27

11

22

31

00

Circular threading CCW

Tool radius/tool nose radius compensation : corner circular interpolation
Tool radius/tool nose radius compensation : cancel
3-dimensional cutter compensation : cancel
Tool radius/tool nose radius compensation : left
3-dimensional cutter compensation : left

Tool radius/tool nose radius compensation : right
3-dimensional cutter compensation : right

3-dimensional cutter compensation : right (type 2)

Normal direction control on : right

Tool offse conversion

Tool offset : double decrease

Spindle unit compensation cancel

Scaling

Programmable mirror image

Polygon turning

Start superimposed control

(G FUNCTION)

- 33 -

3. PREPARATORY FUNCTION
(G FUNCTION)

PROGRAMMING B-64484EN/03

Table 3.1 (a) G code list

G code Group Function

G52 Local coordinate system setting
G53 Machine coordinate system setting
G53.1 Tool axis direction control
G53.6
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
G54.4 33 Workpiece setting error compensation
G60 00 Single direction positioning
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 Tilted working plane command
G68.3 Tilted working plane command by tool axis direction
G68.4
G70.7 Finishing cycle
G71.7 Outer surface rough machining cycle
G72.7 End rough machining cycle
G73.7 Closed loop cutting cycle
G74.7 End cutting off cycle
G75.7 Outer or inner cutting off cycle
G76.7 Multiple threading cycle
G72.1 Figure copying (rotary copy)
G72.2
G73 Peck drilling cycle
G74
G75 01 Plunge grinding cycle
G76 09 Fine boring cycle
G77 Plunge direct sizing/grinding cycle
G78 Continuous-feed surface grinding cycle
G79

G80 09

G80.4 Electronic gear box: synchronization cancellation
G81.4
G80.5 Electronic gear box 2 pair: synchronization cancellation
G81.5

G81 09

G81.1 00 Chopping function/High precision oscillation function

00

14

15

12

16

00

09

01

34

24

Tool center point retention type tool axis direction control

Workpiece coordinate system 6 selection

Cutting mode

Macro modal call A/B cancel

Tilted working plane command (incremental multi-command)

Figure copying (linear copy)

Left-handed tapping cycle

Intermittent-feed surface grinding cycle
Canned cycle cancel
Electronic gear box : synchronization cancellation

Electronic gear box: synchronization start

Electronic gear box 2 pair: synchronization start
Drilling cycle or spot boring cycle
Electronic gear box : synchronization start

- 34 -

3.PREPARATORY FUNCTION

B-64484EN/03 PROGRAMMING

Table 3.1 (a) G code list

G code Group Function

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
G96.1 Spindle indexing execution (waiting for completion)
G96.2 Spindle indexing execution (not waiting for completion)
G96.3 Spindle indexing completion check
G96.4
G98 Canned cycle : return to initial level
G99
G107 00 Cylindrical interpolation
G112 Polar coordinate interpolation mode
G113
G160 In-feed control cancel
G161

09

03

00

05

13

00

10

21

20

Boring cycle

Incremental programming

Workpiece coordinate system preset

Feed per revolution

Constant surface speed control cancel

SV speed control mode ON

Canned cycle : return to R point level

Polar coordinate interpolation mode cancel

In-feed control

(G FUNCTION)

- 35 -

3. PREPARATORY FUNCTION
(G FUNCTION)

PROGRAMMING B-64484EN/03

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 3-dimensional coordinate system 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 Tool retract and recover
G10.9 G10.9 G10.9 Programmable switching of diameter/radius specification

G11 G11 G11
G12.1

(G112)

G13.1

(G113)

G17 G17 G17 XpYp plane selection
G17.1 G17.1 G17.1 Plane conversion function

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 Spindle speed fluctuation detection off

G26 G26 G26

G27 G27 G27 Reference position return check

G28 G28 G28 Return to reference position
G28.2 G28.2 G28.2 In-position check disable reference position return

G29 G29 G29 Movement from reference position

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

G07.1

(G107)

G12.1

(G112)

G13.1

(G113)

G07.1

(G107)

G12.1

(G112)

G13.1

(G113)

Table 3.2 (b) G code list

Group Function

01

3-dimensional coordinate system conversion CCW

AI contour control (command compatible with high precision

00

00

21

16

06

09

08

00

contour control), High-speed cycle machining, High-speed
binary program operation

HRV3, 4 on/off

Cylindrical interpolation

Programmable data input mode cancel

Polar coordinate interpolation mode

Polar coordinate interpolation cancel mode

YpZp plane selection

Input in mm

Stored stroke check function off

Spindle speed fluctuation detection on

Floating reference point return

- 36 -

3.PREPARATORY FUNCTION

B-64484EN/03 PROGRAMMING

Table 3.2 (b) G code list

G code system

A B C

G30.2 G30.2 G30.2

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 Tool radius/tool nose radius compensation: with vector held

G39 G39 G39

G40 G40 G40 Tool radius/tool nose radius compensation : cancel

G41 G41 G41 Tool radius/tool nose radius compensation : left

G42 G42 G42 Tool radius/tool nose radius compensation : right
G41.2 G41.2 G41.2 3-dimensional cutter compensation : 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 3-dimensional cutter compensation : left (type 2)
G42.2 G42.2 G42.2 3-dimensional cutter compensation : right (type 1)

G42.4 G42.4 G42.4

G42.5 G42.5 G42.5

G42.6 G42.6 G42.6
G40.1 G40.1 G40.1 Normal direction control cancel mode
G41.1 G41.1 G41.1 Normal direction control left on

G42 .1 G42 .1 G42 .1

G43 G43 G43

G44 G44 G44

G43.1 G43.1 G43.1

G43.4 G43.4 G43.4

G43.5 G43.5 G43.5

G43.7

(G44.7)

G44.1 G44.1 G44.1

G43.7

(G44.7)

G43.7

(G44.7)

Group Function

In-position check disable 2nd, 3rd, or 4th reference position

00

01

07

19

23

return

EGB-axis skip

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

Tool radius/tool nose radius compensation: corner rounding
interpolation

3-dimensional cutter compensation :
(leading edge offset)
3-dimensional cutter compensation : left (type 1) (FS16i­compatible command)
3-dimensional cutter compensation : left (type 1) (FS16i­compatible command)

3-dimensional cutter compensation : right (type 1) (FS16i­compatible command)
3-dimensional cutter compensation : right (type 1) (FS16i­compatible command)
3-dimensional cutter compensation : right (type 2)

Normal direction control right on
Tool length compensation +
(Bit 3 (TCT) of parameter No. 5040 must be "1".)
Tool length compensation -
(Bit 3 (TCT) of parameter No. 5040 must be "1".)
Tool length compensation in tool axis direction
(Bit 3 (TCT) of parameter No. 5040 must be "1".)
Tool center point control (type 1)
(Bit 3 (TCT) of parameter No. 5040 must be "1".)
Tool center point control (type 2)
(Bit 3 (TCT) of parameter No. 5040 must be "1".)
Tool offset
(Bit 3 (TCT) of parameter No. 5040 must be "1".)
Tool offset conversion
(Bit 3 (TCT) of parameter No. 5040 must be "1".)

- 37 -

(G FUNCTION)

3. PREPARATORY FUNCTION
(G FUNCTION)

PROGRAMMING B-64484EN/03

Table 3.2 (b) G code list

G code system

A B C

G49

(G49.1)

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)

G50.4 G50.4 G50.4 Cancel synchronous control
G50.5 G50.5 G50.5 Cancel composite control
G50.6 G50.6 G50.6 Cancel superimposed control
G51.4 G51.4 G51.4 Start synchronous control
G51.5 G51.5 G51.5 Start composite control
G51.6 G51.6 G51.6 Start superimposed control

G52 G52 G52 Local coordinate system setting

G53 G53 G53 Machine coordinate system setting
G53.1 G53.1 G53.1 Tool axis direction control
G53.6 G53.6 G53.6

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
G54.4 G54.4 G54.4 26 Workpiece setting error compensation

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 Tilted working plane command
G68.3 G68.3 G68.3 Tilted working plane command by tool axis direction
G68.4 G68.4 G68.4

G69 G69 G69 04

G69.1 G69.1 G69.1 17

G70 G70 G72 Finishing cycle

G71 G71 G73 Stock removal in turning

G72 G72 G74

G49

(G49.1)

G50.2

(G250)

G51.2

(G251)

G54

(G54.1)

G49

(G49.1)

G50.2

(G250)

G51.2

(G251)

G54

(G54.1)

Group Function

23

00

18

22

20

00

14

15

12

17

00

Tool length compensation cancel
(Bit 3 (TCT) of parameter No. 5040 must be "1".)

Workpiece coordinate system preset

Scaling

Programmable mirror image

Polygon turning cancel

Polygon turning

Tool center point retention type 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
system conversion mode on

Tilted working plane command (incremental multi-command)
Mirror image off for double turret or balance cutting mode
cancel
Coordinate system rotation cancel or 3-dimensional
coordinate system conversion mode off

Stock removal in facing

- 38 -

3.PREPARATORY FUNCTION

B-64484EN/03 PROGRAMMING

Table 3.2 (b) G code list

G code system

A B C

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 copying (rotational copying)
G72.2 G72.2 G72.2

G71 G71 G72 Traverse grinding cycle

G72 G72 G73 Traverse direct sizing/grinding cycle

G73 G73 G74 Oscillation grinding cycle

G74 G74 G75

G80 G80 G80 10

G81.1 G81.1 G81.1 00 Chopping function/High precision oscillation function
G80.4 G80.4 G80.4 Electronic gear box: synchronization cancellation
G81.4 G81.4 G81.4
G80.5 G80.5 G80.5 Electronic gear box 2 pair: synchronization cancellation
G81.5 G81.5 G81.5

G81 G81 G81

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
G96.1 G96.1 G96.1 Spindle indexing execution (waiting for completion)
G96.2 G96.2 G96.2 Spindle indexing execution (not waiting for completion)
G96.3 G96.3 G96.3 Spindle indexing completion check
G96.4 G96.4 G96.4

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

00

Figure copying (linear copying)

01

Oscillation direct sizing/grinding cycle
Canned cycle cancel for drilling
Electronic gear box : synchronization cancellation

28

27

10

01

02

00

05

03

11

Electronic gear box: synchronization start

Electronic gear box 2 pair: synchronization start
Spot drilling (FS15-T format)
Electronic gear box : synchronization start

Cycle for side boring

End face turning cycle

Constant surface speed control cancel

SV speed control mode ON

Feed per revolution

Incremental programming

Canned cycle : return to R point level

(G FUNCTION)

- 39 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-64484EN/03

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).

Chapter 4, "INTERPOLATION FUNCTIONS", consists of the following sections:

4.1 POSITIONING (G00).........................................................................................................................40

4.2 SINGLE DIRECTION POSITIONING (G60) ...................................................................................41

4.3 LINEAR INTERPOLATION (G01)...................................................................................................44

4.4 CIRCULAR INTERPOLATION (G02, G03).....................................................................................46

4.5 HELICAL INTERPOLATION (G02, G03)........................................................................................50

4.6 HELICAL INTERPOLATION B (G02, G03)....................................................................................51

4.7 SPIRAL INTERPOLATION, CONICAL INTERPOLATION (G02, G03).......................................52

4.8 POLAR COORDINATE INTERPOLATION (G12.1, G13.1)...........................................................58

4.9 CYLINDRICAL INTERPOLATION (G07.1)....................................................................................66

4.10 CUTTING POINT INTERPOLATION FOR CYLINDRICAL INTERPOLATION (G07.1) ...........71

4.11 EXPONENTIAL INTERPOLATION (G02.3, G03.3) .......................................................................81

4.12 SMOOTH INTERPOLATION (G05.1)..............................................................................................87

4.13 NANO SMOOTHING ........................................................................................................................92

4.14 NURBS INTERPOLATION (G06.2) ...............................................................................................100

4.15 HYPOTHETICAL AXIS INTERPOLATION (G07).......................................................................108

4.16 VARIABLE LEAD THREADING (G34) ........................................................................................110

4.17 CIRCULAR THREADING (G35, G36) ...........................................................................................111

4.18 SKIP FUNCTION (G31) ..................................................................................................................115

4.19 MULTI-STEP SKIP (G31) ...............................................................................................................117

4.20 HIGH-SPEED SKIP SIGNAL (G31) ...............................................................................................117

4.21 SKIP POSITION MACRO VARIABLE IMPROVEMENT ............................................................118

4.22 CONTINUOUS HIGH-SPEED SKIP FUNCTION..........................................................................118

4.23 TORQUE LIMIT SKIP .....................................................................................................................119

4.24 3-DIMENSIONAL CIRCULAR INTERPOLATION......................................................................122

4.1 POSITIONING (G00)

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

Format

G00 IP_ ;

IP_ : For an absolute programming, the coordinates of an end point, and for an

incremental programming, 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.

- 40 -

B-64484EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS

• 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

Start position

End position

Non linear interpolation type positioning

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.

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

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

End point

Temporary stop

Format

G60 IP_ ;

IP_ : For an absolute programming, the coordinates of an end point, and for an

incremental programming, the distance the tool moves.

Explanation

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.

- 41 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-64484EN/03

G60, which is a one-shot G-code, can be used as a modal G-code in group 01 by setting 1 to the bit 0
(MDL) of parameter No. 5431.
This setting can eliminate specifying a G60 command for every block. Other specifications are the same
as those for a one-shot G60 command. When a 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 mode start

Single direction positioning

Single direction positioning mode cancel

- Overview of operation

• In the case of positioning of non-linear interpolation type (bit 1 (LRP) of parameter No. 1401 =

0)

As shown below (Fig. 4.2 (a)), 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

Fig. 4.2 (a)

• 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.

- 42 -

B-64484EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS

X

Programmed start point

Fig. 4.2 (b)

Overrun distance in the Z-axis direction

Overrun distance in the
X-axis direction

Programmed end point

Z

Limitation

• 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 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 arbitrary 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

• 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.

T

• 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.

- 43 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-64484EN/03

4.3 LINEAR INTERPOLATION (G01)

Tools can move along a line.

Format

G01 IP_ F_ ;

IP_ : For an absolute programming, the coordinates of an end point, and for an incremental

programming, 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.

α

β

γ

G01

α

β

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 :

ζ

Ff ;

γ

ζ

α

α

2222

ζγβα

+++=L

F ×=

β

F ×=

γ

γ

f

F ×=

ζ

f

F ×=

L

β

f

L

L

ζ

L

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 β (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.

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

+

300

4020

)(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.

- 44 -

B-64484EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS

Example

- Linear interpolation

• For milling machining

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

Y axis

100.0

0 (Start point)

• For lathe cutting

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

- Feedrate for the rotary axis

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

(End point)

200.0

X axis

X

46.0

20.1

End

φ40.0

point

Start
point

φ20.0

Z

90

(End point)

(Start point)

°

Feedrate is 300 deg/min

- 45 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-64484EN/03

Y

4.4 CIRCULAR INTERPOLATION (G02, G03)

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

Format

Arc in the XpYp plane

G17

G03

Xp_ Yp_

R_

F_ ;

Arc in the ZpXp plane

G02 I_ K_

G02 I_ J_

G18

G03

Zp_ Xp_

R_

F_ ;

Arc in the YpZp plane

G02 J_ K_

G19

G03

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_ Command values of X axis or its parallel axis (set by parameter No. 1022)
Yp

_

Zp

_

I_ Xp axis distance from the start point to the center of an arc with sign

J_ Yp axis distance from the start point to the center of an arc with sign
K_ Zp axis distance from the start point to the center of an arc with sign
R_ Arc radius (with sign, radius value for lathe cutting)
F_ Feedrate along the arc

T

Yp_ Zp_

F_ ;

R_

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)

NOTE

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

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 (Fig. 4.4 (a)).

G03

G02

G17

X

X

G03

G02

G18

Fig. 4.4 (a)

- 46 -

Z

G02

G19

G03

YZ

B-64484EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS

j j

- 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 (Fig. 4.4 (b)).

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

End point (x,y)

y

x

End point (z,x)

x

Start

i

point

z

k

Start
point

End point (y,z)

z

y

Start
point

Center

Center

Fig. 4.4 (b)

i

Center

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.

- Command for a circle

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

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

F300.0 ;

F300.0 ;

<2>

r=50mm

End point

<1>

Start point

r=50mm

Y

X

- 47 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-64484EN/03

- Feedrate

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 tool radius compensation is applied

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 PS0021 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.
When an end point does not lie on the arc, a spiral results, as shown below.

End point

e

γ

(t)

Start point

s

γ

e

γ

Radius

Start point

γ

θ

(t)

θ

s

γ

Center

s(t)

+=

End point

θ

Center

θ

ts)e(

)(θγγγγ−

θ

The arc radius changes linearly with the center angle θ(t). Spiral interpolation is performed using a
circular command that specifies one arc radius for the start point and another arc radius for the end point.
To use spiral interpolation, set a large value in parameter No. 3410, used to specify the limit on the arc
radius error.

- 48 -

B-64484EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS

Example

M

Y axis

100

60

40

0

90 120 140

The above tool path can be programmed as follows;
(1) In absolute programming
G92X200.0 Y40.0 Z0 ;
G90 G03 X140.0 Y100.0 R60.0 F300. ;
G02 X120.0 Y60.0 R50.0 ;
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 ;

T

- Command of circular interpolation X, Z

G02X_Z_I_K_F_; G03X_Z_I_K_F_;

X-axis

End point

X

Z

Center of arc

(Diameter programming)

Start point

K

Z-axis

X-axis

End point

X

Z

K

50

(Diameter
programming)

Start point

I

60

Z-axis

X axis

200

G02X_Z_R_F_;

End point

X-axis

X

Z

Center of arc

R

(Diameter
programming)

Start point

Z-axis

(Absolute programming)

(Absolute programming)

X

15.0

R25.0

10.0

50.0

30.0

50.0

(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

(Absolute programming)

- 49 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-64484EN/03

T

s

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 in the XpYp plane

G17

G03

Xp_ Yp_

R_

α_ (β_) F_ ;

Arc in the ZpXp plane

G02 K_ I_

G02 I_ J_

G18

G03

Zp_ Xp_

R_

α_ (β_) F_ ;

Arc in the YpZp plane

G02 J_ K_

G19

G03

α, β : Any one axis where circular interpolation is not applied.
Up to two other axes can be specified.

Yp_ Zp_

R_

α_ (β_) F_ ;

Explanation

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.

Z

Tool path

X

he feedrate along the circumference of two circular interpolated axes is the

pecified 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:

F ×

(Length of arc)

Length of arc

2

+ (Length of linear axis)2

The velocity along the linear axis is expressed as follows:

F ×

(Length of arc)

Length of linear axis

2

+ (Length of linear axis)2

- 50 -

B-64484EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS

X

The feedrate along the tool path is specified.

Z

Tool path

Y

Limitation

• Tool radius/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.

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

G17

Arc in the ZpXp plane

G18

Arc in the YpZp plane

G19

α, β, γ, δ : Any axis to which circular interpolation is not applied.
Up to four axes can be specified.

G02 I_ J_

G03

Xp_ Yp_

R_

α_ β_ γ_ δ_ F_ ;

G02 K_ I_

G03

Zp_ Xp_

R_

α_ β_ γ_ δ_ F_ ;

G02 J_ K_

G03

Yp_ Zp_

R_

α_ β_ γ_ δ_ F_ ;

- 51 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-64484EN/03

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

X_Y_I_J_Q_L_F_;

G03

ZpXp plane

G02

G02

G18

Z_X_K_I_Q_L_F_;

G03

YpZp plane

G02

G19

Y_Z_J_K_Q_L_F_;

G03

X, Y, Z : Coordinates of the end point
L : Number of revolutions (positive value without a decimal point) (*1)
Q : Radius increment or decrement per spiral revolution (*1, *2)
I, J, K : Signed distance from the start point to the center (same as the distance specified

for circular interpolation)

F : Feedrate

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

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

- 52 -

B-64484EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS

- Conical interpolation
XpYp plane

G02 G17

X_ Y_ I_ J_ Z_ Q_ L_ F_ ;

G03

ZpXp plane

G02

G18

Z_ X_ K_ I_ Y_ Q_ L_ F_ ;

G03

YpZp plane

G02

G19

Y_ Z_ J_ K_ X_ Q_ L_ F_ ;

G03

X, Y, Z : Coordinates of the end point
L : Number of revolutions (positive value without a decimal point) (*1)
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 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.

F : Feedrate (The tangential velocity about the linear axis is specified.)
(*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 K_

X_ Y_ I_ J_ Z_

Q_ G18

F_ ;

G03

L_

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.

Explanation

- Function of spiral interpolation

Spiral interpolation in the XY plane is defined as follows:

2

0

0

X0 : X coordinate of the center

: Y coordinate of the center

Y

0

R : Radius at the beginning of spiral interpolation
Q' : Variation in radius

)Q'(R)Y(Y)X(X +=−+−

22

- 53 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-64484EN/03

When the programmed command is assigned to this function, the following expression is obtained:

θ

222

)Q)

++=−−+−−

SS

(L'(RJ)Y(YI)X(X

360

where

: X coordinate of the start point

X

S

: Y coordinate of the start point

Y

S

I : X coordinate of the vector from the start point to the center
J : Y coordinate of the vector from the start point to the center
R : Radius at the beginning of spiral interpolation
Q : Radius increment or decrement per spiral revolution
L' : (Current number of revolutions) - 1
θ : Angle between the start point and the current position (degrees)

- Controlled axes

For conical interpolation, two axes of a plane and two additional axes, that is, four axes in total, can be
specified. A rotary axis can be specified as the additional axis.

- Difference between end points

If the difference between the programmed end point and the calculated end point of a spiral exceeds a
value specified in parameter No. 3471 about any axis of a selected plane, an alarm PS5123 will be issued.
If the difference between the programmed height and calculated height of the end point a cone exceeds a
value specified in parameter No. 3471, an alarm PS5123 will be issued. The figure below (Fig. 4.7 (a))
illustrates details.

Y

100.0

X

-30.0

α

G90 G02 X0 Y-33.5 I0 J-100. F300;

The coordinates of the programmed end point are (0, -33.5) while the coordinates of
the calculated end point are (0, -30.0). A value greater than the difference (α:
Tolerance) is specified in parameter No. 3471. If the end point is exceeded, an alarm
PS5123 will be issued. The same is specified for the height of conical interpolation.

-33.5

Q-20.
L4

Fig. 4.7 (a)

20.0

20.0

20.0

- 54 -

B-64484EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS

- Tool radius compensation

M

The spiral or conical interpolation command can be programmed in tool radius compensation mode. This
compensation is performed in the same way as described in "When it is exceptional" in "Tool Movement
in Offset Mode" section. A virtual circle centered on the center of spiral interpolation is thought at the end
of a block. The tool path is obtained by performing tool radius compensation along the virtual circle and
the blocks before and after the spiral interpolation. When the end point of the block is at the center of the
spiral interpolation, no virtual circle can be drawn. If drawing is attempted, an alarm PS5124 is issued.

Tool center path

Virtual circle

Programmed spiral
interpolation

r

Center

r

After cutter

compensation

- Actual cutting feedrate

A constant speed is maintained in spiral interpolation or conical interpolation. The angular velocity near
the center, however, may increase because of the small radius of the spiral. This can be avoided by
maintaining the angular velocity after the radius of the spiral reaches a value specified in parameter No.

3472. Consequently, the actual cutting feedrate decreases.
An example is illustrated below (Fig. 4.7 (b)).

1.5

r

-0.5

Specified feedrate: F100.
Parameter 3472 (r) = 1.000
IS-B

While the radius of the spiral shown
at the left is greater than the value
specified in parameter No. 3472, the
actual cutting feedrate is F100. As
the radius decreases, the actual
feedrate also decreases, the actual
feedrate near the end point being
about F65.

Fig. 4.7 (b)

- Deceleration by acceleration

During spiral interpolation, the function of deceleration by acceleration is enabled. The feedrate may
decrease as the tool approaches the center of the spiral.

- Dry run

When the dry run signal is inverted from 0 to 1 or from 1 to 0 during movement along an axis, the
movement is accelerated or decelerated to the desired speed without first reducing the speed to zero.

- 55 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-64484EN/03

Limitation

- Radius

During spiral interpolation and conical interpolation, the addresses "C", "R", ",C", or ",R" cannot be
specified.

- Feed functions

The functions of feed per rotation, inverse time feed, F command with one digit, and automatic corner
override cannot be used.

- Retrace

A program including spiral or conical interpolation cannot be retraced.

- Polar coordinate interpolation, scaling, and normal direction control

Spiral interpolation and conical interpolation cannot be specified in these modes.

- Optional function

To use the conical interpolation function, the optional function for helical interpolation is also necessary.

Example

- Spiral interpolation

The path indicated below is programmed with absolute and incremental values as follows:

20. 20.

120

100

80

Y axis

60

40

20

-120 -100 -80 -60 -40 –20 20 40 60 80 100 120

-20

-40

-60

-80

-100

-120

This sample path has the following values:

• Start point : (0, 100.0)

• End point (X, Y) : (0, -30.0)

• Distance to the center (I, J) : (0, -100.0)

• Radius increment or decrement (Q) : -20.0

• Number of revolutions (L) : 4

(1) With absolute values, the path is programmed as follows:

X axis

G90 G02 X0 Y-30.0 I0 J-100.0

Q-20.0

L4

F300.0 ;

- 56 -

B-64484EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS

(2) With incremental values, the path is programmed as follows:

G91 G02 X0 Y-130.0 I0 J-100.0

Q-20.0

L4

F300.0 ;

(Either the Q or L setting can be omitted.)

- Conical interpolation

The sample path shown below is programmed with absolute and incremental values as follows:

(0,-37.5,62.5)

+X

This sample path has the following values:

• Start point : (0, 100.0, 0)

• End point (X, Y, Z) : (0, -37.5, 62.5)

• Distance to the center (I, J) : (0, -100.0)

• Radius increment or decrement (Q) : -25.0

• Height increment or decrement (K) : 25.0

• Number of revolutions (L) : 3

(1) With absolute values, the path is programmed as follows:

+Z

25.0 25.0

25.0

25.0

+Y

100.0

-100.0

K25.0

G90 G02 X0 Y-37.5 Z62.5 I0 J-100.0

Q-25.0

L3

F300.0 ;

(2) With incremental values, the path is programmed as follows:

K25.0

G91 G02 X0 Y-137.5 Z62.5 I0 J-100.0

Q-25.0

L3

F300.0 ;

(Either the Q or L setting can be omitted.)

- 57 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-64484EN/03

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

Overview

Polar coordinate interpolation is a function that exercises contour control in converting a command
programmed in a Cartesian coordinate system to the movement of a linear axis (movement of a tool) and
the movement of a rotary axis (rotation of a workpiece). This function is useful for grinding a cam shaft.

Format

G12.1; Starts polar coordinate interpolation mode (enables polar coordinate

interpolation).

Specify linear or circular interpolation using coordinates in a Cartesian

coordinate system consisting of a linear axis and rotary axis (hypothetical
axis).

G13.1; Polar coordinate interpolation mode is cancelled (for not performing polar

coordinate interpolation).

Specify G12.1 and G13.1 in Separate Blocks.

Explanation

- Polar coordinate interpolation mode (G12.1)

The axes of polar coordinate interpolation (linear axis and rotary axis) should be specified in advance,
with corresponding parameters. Specifying G12.1 places the system in the polar coordinate interpolation
mode, and selects a plane (called the polar coordinate interpolation plane) formed by one linear axis and a
hypothetical axis intersecting the linear axis at right angles. The linear axis is called the first axis of the
plane, and the hypothetical axis is called the second axis of the plane. Polar coordinate interpolation is
performed in this plane.
In the polar coordinate interpolation mode, both linear interpolation and circular interpolation can be
specified by absolute or incremental programming.
Tool radius compensation can also be performed. The polar coordinate interpolation is performed for a
path obtained after tool radius compensation.
The tangential velocity in the polar coordinate interpolation plane (Cartesian coordinate system) is
specified as the feedrate, using F.

- Polar coordinate interpolation cancel mode (G13.1)

Specifying G13.1 cancels the polar coordinate interpolation mode.

- Polar coordinate interpolation plane

G12.1 starts the polar coordinate interpolation mode and selects a polar coordinate interpolation plane
(Fig. 4.8 (a)). Polar coordinate interpolation is performed on this plane.

- 58 -

B-64484EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS

Rotary axis (hypothetical axis)

(unit: mm or inch)

Linear axis
(unit: mm or inch)

Origin of the local coordinate system (G52 command)
(Or origin of the workpiece coordinate system)

Fig. 4.8 (a) Polar coordinate interpolation plane

When the power is turned on or the system is reset, polar coordinate interpolation is canceled (G13.1).
The linear and rotation axes for polar coordinate interpolation must be set in parameters Nos. 5460 and
5461 beforehand.

CAUTION

The plane used before G12.1 is specified (plane selected by G17, G18, or G19)

is canceled. It is restored when G13.1 (canceling polar coordinate interpolation)
is specified.

When the system is reset, polar coordinate interpolation is canceled and the

plane specified by G17, G18, or G19 is used.

- Distance moved and feedrate for polar coordinate interpolation

• The unit for coordinates on the hypothetical axis is the same as the unit for the linear axis (mm/inch).
In the polar coordinate interpolation mode, program commands are specified with Cartesian

coordinates on the polar coordinate interpolation plane. The axis address for the rotary axis is used
as the axis address for the second axis (hypothetical axis) in the plane. Whether a diameter or radius
is specified for the first axis in the plane is the same as for the rotary axis regardless of the
specification for the first axis in the plane.

The hypothetical axis is at coordinate 0 immediately after G12.1 is specified. Polar interpolation is

started assuming the rotation angle of 0 for the position of the tool when G12.1 is specified.
Example)
When a value on the X-axis (linear axis) is input in millimeters
G12.1;

G01 X10. F1000. ; ........A 10-mm movement is made on the Cartesian coordinate system.

C20. ;............................. A 20-mm movement is made on the Cartesian coordinate system.

G13.1;

When a value on the X-axis (linear axis) is input in inches
G12.1;

G01 X10. F1000. ; ......A 10-inch movement is made on the Cartesian coordinate system.

C20. ;............................. A 20-inch movement is made on the Cartesian coordinate system.

G13.1;

• The unit for the feedrate is mm/min or inch/min.
Specify the feedrate as a speed (relative speed between the workpiece and tool) tangential to the

polar coordinate interpolation plane (Cartesian coordinate system) using F.

- 59 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-64484EN/03

- G codes which can be specified in the polar coordinate interpolation mode

G01.......................Linear interpolation

G02, G03..............Circular interpolation

G02.2, G03.2........Involute interpolation

G04.......................Dwell, Exact stop

G40, G41, G42 .....Tool radius compensation (Polar coordinate interpolation is applied to the path

after tool radius compensation.)

G65, G66, G67 .....Custom macro command

G90, G91..............Absolute programming, incremental programming

G94, G95..............Feed per minute, feed per revolution

- Circular interpolation in the polar coordinate plane

The addresses for specifying the radius of an arc for circular interpolation (G02 or G03) in the polar
coordinate interpolation plane depend on the first axis in the plane (linear axis).

• I and J in the Xp-Yp plane when the linear axis is the X-axis or an axis parallel to the X-axis.

• J and K in the Yp-Zp plane when the linear axis is the Y-axis or an axis parallel to the Y-axis.

• K and I in the Zp-Xp plane when the linear axis is the Z-axis or an axis parallel to the Z-axis.

The radius of an arc can be specified also with an R command.

NOTE

In a lathe system, the parallel axes U, V, and W can be used in the G code

system B or C.

- Movement along axes not in the polar coordinate interpolation plane in the
polar coordinate interpolation mode

The tool moves along such axes normally, independent of polar coordinate interpolation.

- Current position display in the polar coordinate interpolation mode

Actual coordinates are displayed. However, the remaining distance to move in a block is displayed based
on the coordinates in the polar coordinate interpolation plane (Cartesian coordinates).

- Coordinate system for the polar coordinate interpolation

Basically, before G12.1 is specified, a local coordinate system (or workpiece coordinate system) where
the center of the rotary axis is the origin of the coordinate system must be set.

- Compensation in the direction of the hypothetical axis in polar coordinate
interpolation

If the first axis of the plane has an error from the center of the rotary axis in the hypothetical axis
direction, in other words, if the rotary axis center is not on the X-axis, the hypothetical axis direction
compensation function in the polar coordinate interpolation mode is used. With the function, the error is
considered in polar coordinate interpolation. The amount of error is specified in parameter No. 5464.

- 60 -

B-64484EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS

Hypothetical axis (C-axis)

Rotary axis

(X, C)

Error in the direction of
hypothetical axis (P)

Center of rotary axis

(X, C) : Point in the X-C plane (The center of the rotary axis is considered to be the origin of

the X-C plane.)
X : X coordinate in the X-C plane
C : Hypothetical axis coordinate in the X-C plane
P : Error in the direction of the hypothetical axis (specified in parameter No. 5464)

X-axis

- Shifting the coordinate system in polar coordinate interpolation

In the polar coordinate interpolation mode, the workpiece coordinate system can be shifted. The current
position display function shows the position viewed from the workpiece coordinate system before the
shift. The function to shift the coordinate system is enabled when bit 2 (PLS) of parameter No. 5450 is
specified accordingly.
The shift can be specified in the polar coordinate interpolation mode, by specifying the position of the
center of the rotary axis C (A, B) in the X-C (Y-A, Z-B) interpolation plane with reference to the origin of
the workpiece coordinate system, in the following format.

G12.1 X_ C_ ; (Polar coordinate interpolation for the X-axis and C-axis)
G12.1 Y_ A_ ; (Polar coordinate interpolation for the Y-axis and A-axis)
G12.1 Z_ B_ ; (Polar coordinate interpolation for the Z-axis and B-axis)

C

G12.1 Xx Cc ;

Center of C-axis

c

Origin of workpiece
coordinate system

x

X

Limitation

- Changing the coordinate system during polar coordinate interpolation

In the G12.1 mode, the coordinate system must not be changed (G92, G52, G53, relative coordinate reset,
G54 through G59, etc.).

- 61 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-64484EN/03

- Tool radius/tool nose radius compensation

The polar coordinate interpolation mode (G12.1 or G13.1) cannot be started or terminated in the tool
radius/tool nose radius compensation mode (G41 or G42). G12.1 or G13.1 must be specified in the tool
radius/tool nose radius compensation canceled mode (G40).
For the tool radius/tool nose radius compensation canceled mode (G40) command, be sure to specify the
polar coordinate axis to cancel the offset vector.

- Tool length offset command

Tool length offset must be specified in the polar coordinate interpolation cancel mode before G12.1 is
specified. It cannot be specified in the polar coordinate interpolation mode. Furthermore, no offset values
can be changed in the polar coordinate interpolation mode.

- Tool offset command

A tool offset must be specified before the G12.1 mode is set. No offset can be changed in the G12.1
mode.

- Program restart

For a block in the G12.1 mode, the program and the block cannot be restarted.

- Cutting feedrate for the rotary axis

Polar coordinate interpolation converts the tool movement for a figure programmed in a Cartesian
coordinate system to the tool movement in the rotary axis (C-axis) and the linear axis (X-axis). When the
tool comes close to the center of the workpiece, the C-axis velocity component increases. If the maximum
cutting feedrate for the C-axis (parameter No. 1430) is exceeded, the automatic feedrate override function
and automatic speed clamp function are enabled.
If the maximum cutting feedrate for the X-axis is exceeded, the automatic feedrate override function and
automatic speed clamp function are enabled.

- 62 -

B-64484EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS

θ

θ

θ

WARNING

1 Consider lines L1, L2, and L3. ΔX is the distance the tool moves per time unit at

the feedrate specified with address F in the Cartesian coordinate system. As the
tool moves from L1 to L2 to L3, the angle at which the tool moves per time unit
corresponding to ΔX in the Cartesian coordinate system increases from θ1 to θ2
to θ3. In other words, the C-axis component of the feedrate becomes larger as
the tool moves closer to the center of the workpiece. The C component of the
feedrate may exceed the maximum cutting feedrate for the C-axis because the
tool movement in the Cartesian coordinate system has been converted to the
tool movement for the C-axis and the X-axis.

ΔX

1

2

3

L1

L2

L3

L: Distance (in mm) between the tool center and workpiece center when the

tool center is the nearest to the workpiece center

R: Maximum cutting feedrate (deg/min) of the C axis

Then, a speed specifiable with address F in polar coordinate interpolation can be

given by the formula below. If the maximum cutting feedrate for the C-axis is
exceeded, the automatic speed control function for polar coordinate interpolation
automatically controls the feedrate.

F < L × R ×

π

(mm/min)

180

2 The following function cannot be used for the rotary axis of polar coordinate

interpolation.

• Index table indexing function

- Automatic speed control for polar coordinate interpolation

If the velocity component of the rotary axis exceeds the maximum cutting feedrate in the polar coordinate
interpolation mode, the speed is automatically controlled.

- Automatic override

If the velocity component of the rotary axis exceeds the permissible velocity (maximum cutting feedrate
multiplied by the permission factor specified in parameter No. 5463), the feedrate is automatically
overridden as indicated below.
Override = (Permissible velocity) ÷ (Velocity component of rotary axis) × 100(%)

- Automatic speed clamp

If the velocity component of the rotary axis after automatic override still exceeds the maximum cutting
feedrate, the speed of the rotary axis is automatically clamped. As a result, the velocity component of the
rotary axis will not exceed the maximum cutting feedrate.
The automatic speed clamp function works only when the center of the tool is very close to the center of
the rotary axis.

- 63 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-64484EN/03

A

C-axis

[Example]

G90 G00 X10.0 C0. ;
G12.1 ;
G01 C0.1 F1000 ;
X-10.0 :
G13.1 ;

-10.

BCD

+10.

X-axis

Automatic speed control for polar coordinate interpolation

Suppose that the maximum cutting feedrate of the rotary axis is 360 (3600 deg/min) and that the
permission factor of automatic override for polar coordinate interpolation (parameter No. 5463) is 0
(90%). If the program indicated above is executed, the automatic override function starts working when
the X coordinate becomes 2.273 (point A). The automatic speed clamp function starts working when the
X coordinate becomes 0.524 (point B).
The minimum value of automatic override for this example is 3%. The automatic speed clamp function
continues working until the X coordinate becomes -0.524 (point C). Then, the automatic override
function works until the X coordinate becomes -2.273 (point D).
(The coordinates indicated above are the values in the Cartesian coordinate system.)

NOTE

1 While the automatic speed clamp function is working, the machine lock or

interlock function may not be enabled immediately.

2 If a feed hold stop is made while the automatic speed clamp function is working,

the automatic operation halt signal is output. However, the operation may not
stop immediately.

3 The clamped speed may exceed the clamp value by a few percent.

- 64 -

B-64484EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS

Example

Sample program for polar coordinate interpolation in a Cartesian coordinate system consisting of the
X-axis (a linear axis) and a hypothetical axis

Hypothetical axis

N204

N205

N206

C axis

N203

N202

N208

N207

Path after cutter compensation

Path before cutter compensation

N201

N200

Tool

Z axis

X axis

O001;
.
No10 T0101
.
N0100 G90 G00 X60.0 C0 Z

; Positioning to start point
N0200 G12.1; Start of polar coordinate interpolation
N0201 G42 G01 X20.0F

;
N0202 C10.0;
N0203 G03 X10.0 C20.0 R10.0;
N0204 G01 X-20.0; Geometry program
N0205 C-10.0; (program based on cartesian coordinates on
N0206 G03 X-10.0 C-20.0 I10.0 J0; X axis-hypothetical axis plane)
N0207 G01 X20.0;
N0208 C0;
N0209 G40 X60.0;
N0210 G13.1; Cancellation of polar coordinate interpolation
N0300 Z
N0400 X

;

C ;
.
N0900M30;

- 65 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-64484EN/03

4.9 CYLINDRICAL INTERPOLATION (G07.1)

4.9.1 Cylindrical Interpolation

In cylindrical interpolation function, the amount of movement of a rotary axis specified by angle is
converted to the amount of movement on the circumference to allow linear interpolation and circular
interpolation with another axis.
Since programming is enabled with the cylinder side face expanded, programs such as a program for
grooving cylindrical cams can be created very easily.

Format

G07.1

IP

(enables cylindrical interpolation).

G07.1 IP 0;

IP : An address for the rotary axis
r : The radius of the workpiece
Specify G07.1 IPr; and G07.1 IP0; in separate blocks.
G107 can be used instead of G07.1.

NOTE

Only a positive value is effective as the radius of the workpiece. If a negative

value is specified, alarm PS0175 is issued.

Explanation

- Plane selection (G17, G18, G19)

To specify a G code for plane selection, set the rotary axis in parameter No. 1022 as a linear axis that is
one of the basic three axes of the basic coordinate system or an axis parallel to one of the basic axes. For
example, when rotary axis C-axis is assumed to be parallel to the X-axis, specifying G17, axis address C,
and Y at the same time can select a plane formed by the C-axis and Y-axis (the Xp-Yp plane).

T

NOTE

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

- Feedrate

A feedrate specified in the cylindrical interpolation mode is the feedrate on the circumference.

- Circular interpolation (G02, G03)

Circular interpolation can be performed between the rotary axis set for cylindrical interpolation and
another linear axis. Radius R is used in commands in the same way as described.
The unit for a radius is not degrees but millimeters (for metric input) or inches (for inch input).

<Example Circular interpolation between the Z axis and C axis>
For the C axis of parameter No.1022, 5 (axis parallel with the X axis) is to be set. In this case, the

command for circular interpolation is
G18 Z_C_;
G02 (G03) Z_C_R_;

Starts the cylindrical interpolation mode

r;

:
:
:

The cylindrical interpolation mode is cancelled.

- 66 -

B-64484EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS

For the C axis of parameter No.1022, 6 (axis parallel with the Y axis) may be specified instead. In

this case, however, the command for circular interpolation is
G19 C_Z_;
G02 (G03) Z_C_R_;

- Tool radius/tool nose radius compensation

To perform tool radius/tool nose radius compensation in the cylindrical interpolation mode, cancel any
ongoing tool radius/tool nose radius compensation mode before entering the cylindrical interpolation
mode. Then, start and terminate tool radius/tool nose radius compensation within the cylindrical
interpolation mode.

- Cylindrical interpolation accuracy

In the cylindrical interpolation mode, the amount of travel of a rotary axis specified by an angle is once
internally converted to a distance of a linear axis on the outer surface so that linear interpolation or
circular interpolation can be performed with another axis. After interpolation, such a distance is converted
back to an angle. For this conversion, the amount of travel is rounded to a least input increment.
So when the radius of a cylinder is small, the actual amount of travel can differ from a specified amount
of travel. Note, however, that such an error is not accumulative.
If manual operation is performed in the cylindrical interpolation mode with manual absolute on, an error
can occur for the reason described above.

= travelofamount actual The

⎡
⎢

⎣

REV MOTION

⎡

π

× REV MOTION

R22

⎢
⎣

valueSpecified

π

×

××

⎤

R22

⎤

⎥

⎥
⎦

⎦

MOTION REV : The amount of travel per rotation of the rotary axis (360°)
R : Workpiece radius

[]

: Rounded to the least input increment

Limitation

- Arc radius specification in the circular interpolation

In the cylindrical interpolation mode, an arc radius cannot be specified with word address I, J, or K.

- Positioning

In the cylindrical interpolation mode, positioning operations (including those that produce rapid traverse
cycles such as G28, G53, G73, G74, G76, G80 to G89) cannot be specified. Before positioning can be
specified, the cylindrical interpolation mode must be cancelled. Cylindrical interpolation (G07.1) cannot
be performed in the positioning mode (G00).

- Cylindrical interpolation mode setting

In the cylindrical interpolation mode, the cylindrical interpolation mode cannot be reset. The cylindrical
interpolation mode must be cancelled before the cylindrical interpolation mode can be reset.

- Rotary axis

Only one rotary axis can be set for cylindrical interpolation. Therefore, it is impossible to specify more
than one rotary axis in the G07.1 command.

- Rotary axis roll-over

If a rotary axis using the roll-over function is specified at the start of the cylindrical interpolation mode,
the roll-over function is automatically disabled in the cylindrical interpolation mode. After the cylindrical
interpolation mode is canceled, the roll-over function is enabled automatically.

- 67 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-64484EN/03

- Rotary axis control function

If a rotary axis using the multiple rotary axis control function is specified at the start of the cylindrical
interpolation mode, the rotary axis control function is automatically disabled in the cylindrical
interpolation mode. After the cylindrical interpolation mode is canceled, the rotary axis control function is
enabled automatically.

- Tool radius/tool nose radius compensation

If the cylindrical interpolation mode is specified when tool radius/tool nose radius compensation is
already being applied, correct compensation is not performed. Specify compensation in the cylindrical
interpolation mode.

- Canned cycle for drilling

Canned cycles (G73, G74, and G81 to G89 for M series / G80 to G89 for T series) for drilling, cannot be
specified during cylindrical interpolation mode.

M

- Coordinate system setting

In the cylindrical interpolation mode, a workpiece coordinate system (G92, G54 to G59) or local
coordinate system (G52) cannot be specified.

- Tool offset

A tool offset must be specified before the cylindrical interpolation mode is set. No offset can be changed
in the cylindrical interpolation mode.

- Index table indexing function

Cylindrical interpolation cannot be specified when the index table indexing function is being used.

- Parallel axis

The rotary axis specified for cylindrical interpolation must not be a parallel axis.

T

- Coordinate system setting

In the cylindrical interpolation mode, a workpiece coordinate system G50 cannot be specified.

- Mirror image for double turret

Mirror image for double turret, G68 and G69, cannot be specified during cylindrical interpolation mode.

- 68 -

B-64484EN/03 PROGRAMMING 4.INTERPOLATION FUNCTIONS

.

Example

Example of a Cylindrical Interpolation
O0001 (CYLINDRICAL INTERPOLATION );
N01 G00 G90 Z100.0 C0 ;
N02 G01 G91 G18 Z0 C0 ;
N03 G07.1 C57299 ;*
N04 G90 G01 G42 Z120.0 D01 F250. ;
N05 C30.0 ;
N06 G03 Z90.0 C60.0 R30.0 ;
N07 G01 Z70.0 ;
N08 G02 Z60.0 C70.0 R10.0 ;
N09 G01 C150.0 ;
N10 G02 Z70.0 C190.0 R75.0 ;
N11 G01 Z110.0 C230.0 ;
N12 G03 Z120.0 C270.0 R75.0 ;
N13 G01 C360.0 ;
N14 G40 Z100.0 ;
N15 G07.1 C0 ;
N16 M30 ;

(* A command with a decimal point can also be used.)

Z

Z

C

R

mm

120
110

90

70

60

N05

N06

N11

N07

N08

0

30

60 70

N09

N10

150

N12

230190

270

N13

360

4.9.2 Cylindrical Interpolation by Plane Distance Command

Overview

In the conventional rotary axis command in cylindrical interpolation, the angle of the rotary axis is
specified.
This function enables the rotary axis command in cylindrical interpolation to be specified by distance on
the developed plane by setting parameters.

Format

G07.1

IP

:
G07.1 IP 0;

IP : An address for the rotary axis
r : The radius of the workpiece
Specify G07.1 IPr; and G07.1 IP0; in separate blocks.
G107 can be used instead of G07.1.

Starts the cylindrical interpolation mode (enables cylindrical interpolation)

r;

The cylindrical interpolation mode is cancelled.

C

deg

- 69 -

4.INTERPOLATION FUNCTIONS PROGRAMMING B-64484EN/03

NOTE

Only a positive value is effective as the radius of the workpiece. If a negative

value is specified, alarm PS0175 is issued.

Explanation

By using bit 2 (DTO) of parameter No. 3454, it is possible to switch the rotation axis command during
cylindrical interpolation between the angle of the rotation axis and the distance on the developed plane.

• In the case of the angle of the rotation axis (When bit 2 (DTO) of parameter No. 3454 is set to 0)
The rotation axis command in cylindrical interpolation mode is executed with the angle of the

rotation axis. From the program, specify the angle of the rotation axis that corresponds to the
specified point on the developed plane.

The rotation axis command uses the angle of the rotation axis [deg].

Specify with the
angle of the
rotation axis.

• In the case of the distance on the developed plane (When bit 2 (DTO) of parameter No. 3454 is set to

1)

The rotation axis command in cylindrical interpolation is executed with the distance on the

developed plane. The rotation axis command uses the distance on the developed plane and, therefore,
the command unit varies depending on which of inch or metric input to use.

Specify with the
distance on the
developed plane.

Rotation axis command

Note

NOTE

1 For details of the operation of cylindrical interpolation, as well as limitations, see

Subsection, "Cylindrical Interpolation".

2 This function is an optional function.

- 70 -