FANUC Series 30i-MODEL B, 31i-MODEL B, 32i-MODEL B. For Machining Center System. OPERATOR'S MANUAL

B-64484EN-2/02

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-2/02

GENERAL WARNINGS AND CAUTIONS

WARNING

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.

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.

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.

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.

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.

Immediately after switching on the power, do not touch any of the keys on the

MDI unit until the position display or alarm screen appears on the CNC unit.

Some of the keys on the MDI unit 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.

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.

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-2/02

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 nonvolatile memory in

the CNC unit. Usually, they are retained even if the power is turned off.

Such data may be deleted inadvertently, however, or it may prove necessary to

delete all data from nonvolatile memory as part of error recovery.

To guard against the occurrence of the above, and assure quick restoration of

deleted data, backup all vital data, and keep the backup copy in a safe place.

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

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.

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.

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.

Inch/metric conversion

Switching between inch and metric inputs does not convert the measurement

units of data such as the workpiece origin offset, parameter, and current

position. Before starting the machine, therefore, determine which measurement

units are being used. Attempting to perform an operation with invalid data

specified may damage the tool, the machine itself, the workpiece, or cause injury

to the user.

s-3

SAFETY PRECAUTIONS

B-64484EN-2/02

WARNING

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.

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.

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.

Absolute/incremental mode

If a program created with absolute values is run in incremental mode, or vice

versa, the machine may behave unexpectedly.

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-2/02

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

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.

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.

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.

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.

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.

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.

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-2/02

WARNING

8 Software operator's panel and menu switches

Using the software operator's panel and menu switches, in combination with the

MDI unit, 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 unit 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 unit 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-2/02

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 Lathe System/Machining Center System) 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 αi series Maintenance Manual for details

of the battery replacement procedure.

s-7

B-64484EN-2/02

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

1.1

NOTES ON READING THIS MANUAL

1.2

NOTES ON VARIOUS KINDS OF DATA

II. PROGRAMMING

GENERAL

1.1

TOOL FIGURE AND TOOL MOTION BY PROGRAM

PREPARATORY FUNCTION (G FUNCTION)

INTERPOLATION FUNCTION

3.1

INVOLUTE INTERPOLATION (G02.2, G03.2)

3.1.1

Automatic Speed Control for Involute Interpolation

3.1.2

Helical Involute Interpolation (G02.2, G03.2)

3.1.3

Involute Interpolation on Linear Axis and Rotary Axis

(G02.2, G03.2)

3.2

THREADING (G33)

3.3

CONTINUOUS THREADING

3.4

MULTIPLE THREADING

3.5

CIRCULAR THREAD CUTTING B (G2.1,G3.1)

3.6

GROOVE CUTTING BY CONTINUOUS CIRCLE MOTION (G12.4, G13.4)30

COORDINATE VALUE AND DIMENSION

4.1

POLAR COORDINATE COMMAND (G15, G16)

FUNCTIONS TO SIMPLIFY PROGRAMMING

5.1

CANNED CYCLE FOR DRILLING

5.1.1

High-Speed Peck Drilling Cycle (G73)

5.1.2

Left-Handed Tapping Cycle (G74)

5.1.3

Fine Boring Cycle (G76)

5.1.4

Drilling Cycle, Spot Drilling (G81)

5.1.5

Drilling Cycle Counter Boring Cycle (G82)

5.1.6

Peck Drilling Cycle (G83)

5.1.7

Small-Hole Peck Drilling Cycle (G83)

5.1.8

Tapping Cycle (G84)

5.1.9

Boring Cycle (G85)

5.1.10

Boring Cycle (G86)

5.1.11

Back Boring Cycle (G87)

c-1

TABLE OF CONTENTS

B-64484EN-2/02

5.1.12 Boring Cycle (G88)

5.1.13 Boring Cycle (G89)

5.1.14 Canned Cycle Cancel for Drilling (G80)

5.1.15 Example for Using Canned Cycles for Drilling

5.2

IN-POSITION CHECK SWITCHING FOR DRILLING CANNED CYCLE

5.3

RIGID TAPPING

5.3.1

Rigid Tapping (G84)

5.3.2

Left-Handed Rigid Tapping Cycle (G74)

5.3.3

Peck Rigid Tapping Cycle (G84 or G74)

5.3.4

Canned Cycle Cancel (G80)

100

5.3.5

Override during Rigid Tapping

100

5.3.5.1

Extraction override

100

5.3.5.2

Override signal

101

5.4

OPTIONAL CHAMFERING AND CORNER R

103

5.5

INDEX TABLE INDEXING FUNCTION

106

5.6

IN-FEED CONTROL (FOR GRINDING MACHINE)

108

5.7

CANNED GRINDING CYCLE (FOR GRINDING MACHINE)

110

5.7.1

Plunge Grinding Cycle (G75)

112

5.7.2

Direct Constant-Dimension Plunge Grinding Cycle (G77)

115

5.7.3

Continuous-feed Surface Grinding Cycle (G78)

118

5.7.4

Intermittent-feed Surface Grinding Cycle (G79)

121

5.8

MULTIPLE REPETITIVE CYCLE (G70.7, G71.7, G72.7, G73.7, G74.7,

G75.7,G76.7)

124

5.8.1

Stock Removal in Turning (G71.7)

125

5.8.2

Stock Removal in Facing (G72.7)

136

5.8.3

Pattern Repeating (G73.7)

140

5.8.4

Finishing Cycle (G70.7)

143

5.8.5

End Face Peck Drilling Cycle (G74.7)

147

5.8.6

Outer Diameter / Internal Diameter Drilling Cycle (G75.7)

149

5.8.7

Multiple Threading Cycle (G76.7)

151

5.8.8

Restrictions on Multiple Repetitive Cycle (G70.7, G71.7, G72.7, G73.7, G74.7,

G75.7, and G76.7)

156

COMPENSATION FUNCTION

158

6.1

TOOL LENGTH COMPENSATION SHIFT TYPES

158

6.2

AUTOMATIC TOOL LENGTH MEASUREMENT (G37)

165

6.3

TOOL OFFSET (G45 TO G48)

168

6.4

OVERVIEW OF CUTTER COMPENSATION (G40-G42)

173

6.5

OVERVIEW OF TOOL NOSE RADIUS COMPENSATION (G40-G42)

178

6.5.1

Imaginary Tool Nose

178

6.5.2

Direction of Imaginary Tool Nose

180

6.5.3

Offset Number and Offset Value

181

6.5.4

Workpiece Position and Move Command

181

6.5.5

Notes on Tool Nose Radius Compensation

186

6.6

DETAILS OF CUTTER OR TOOL NOSE RADIUS COMPENSATION

188

6.6.1

Overview

188

6.6.2

Tool Movement in Start-up

192

6.6.3

Tool Movement in Offset Mode

198

6.6.4

Tool Movement in Offset Mode Cancel

216

6.6.5

Prevention of Overcutting Due to Tool Radius / Tool Nose Radius

Compensation

222

6.6.6

Interference Check

225

c-2

B-64484EN-2/02

TABLE OF CONTENTS

6.6.6.1

Operation to be performed if an interference is judged to occur

228

6.6.6.2

Interference check alarm function

229

6.6.6.3

Interference check avoidance function

230

6.6.7

Tool Radius / Tool Nose Radius Compensation for Input from MDI

236

6.7

VECTOR RETENTION (G38)

238

6.8

CORNER CIRCULAR INTERPOLATION (G39)

239

6.9

3-DIMENSIONAL TOOL COMPENSATION (G40, G41)

241

6.10

TOOL COMPENSATION VALUES, NUMBER OF COMPENSATION

VALUES, AND ENTERING VALUES FROM THE PROGRAM (G10)

244

6.11

COORDINATE SYSTEM ROTATION (G68, G69)

247

6.12

GRINDING WHEEL WEAR COMPENSATION

254

6.13

ACTIVE OFFSET VALUE CHANGE FUNCTION BASED ON MANUAL

FEED

259

6.14

ROTARY TABLE DYNAMIC FIXTURE OFFSET

262

6.15

TOOL AXIS DIRECTION TOOL LENGTH COMPENSATION

268

6.15.1 Control Point Compensation of Tool Length Compensation Along Tool Axis...272

6.16

SPINDLE UNIT COMPENSATION, NUTATING ROTARY HEAD TOOL

LENGTH COMPENSATION

276

MEMORY OPERATION USING Series 15 PROGRAM FORMAT

280

7.1

MULTIPLE REPETITIVE CYCLE

281

7.1.1

Stock Removal in Turning (G71.7)

282

7.1.2

Stock Removal in Facing (G72.7)

294

7.1.3

Pattern Repeating (G73.7)

298

7.1.4

Finishing Cycle (G70.7)

301

7.1.5

End Face Peck Drilling Cycle (G74.7)

305

7.1.6

Outer Diameter / Internal Diameter Drilling Cycle (G75.7)

306

7.1.7

Multiple Threading Cycle (G76.7)

308

7.1.8

Restrictions on Multiple Repetitive Cycle

313

AXIS CONTROL FUNCTIONS

315

8.1

CHOPPING FUNCTION

315

8.2

CHOPPING FUNCTION BY FLEXIBLE SYNCHRONOUS CONTROL

321

8.3

PARALLEL AXIS CONTROL

323

GAS CUTTING MACHINE

328

9.1

TOOL OFFSET B

328

9.2

CONER CONTROL BY FEED RATE

331

9.3

AUTOMATIC EXACT STOP CHECK

333

9.4

AXIS SWITCHING

336

9.5

GENTLE CURVE CUTTING

339

9.6

GENTLE NORMAL DIRECTION CONTROL

341

9.6.1

Linear Distance Setting

342

III. OPERATION

1 SETTING AND DISPLAYING DATA

347

1.1

SCREENS DISPLAYED BY FUNCTION KEY

...................................347

1.1.1

Setting and Displaying the Tool Compensation Value

347

1.1.2

Tool Length Measurement

352

c-3

B-64484EN-2/02

GENERAL

1.GENERAL

1 GENERAL

This manual consists of the following parts:

About this manual

GENERAL

Describes chapter organization, applicable models, related manuals, and notes for reading this

manual.

II.

PROGRAMMING

Describes each function: Format used to program functions in the NC language, characteristics, and

restrictions.

III. OPERATION

Describes the manual operation and automatic operation of a machine, procedures for inputting and

outputting data, and procedures for editing a program.

APPENDIX

Lists parameters.

NOTE

1 This manual describes the functions that can operate in the machining center

system path control type. For other functions not specific to the lathe system,

refer to the Operator's Manual (Common to Lathe System/Machining Center

System) (B-64484EN).

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

Series 31i

FANUC Series 31i-B5

31i -B5

FANUC Series 32i-B

32i -B

Series 32i

NOTE

1 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.

2 Some functions described in this manual may not be applied to some products.

For details, refer to the Descriptions (B-64482EN).

- 3 -

1.GENERAL

GENERAL

B-64484EN-2/02

Special symbols

This manual uses the following symbols:

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

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)

B-63874EN

OPERATOR’S MANUAL

MANUAL GUIDE i (For Machining Center System) OPERATOR’S MANUAL

B-63874EN-2

MANUAL GUIDE i (Set-up Guidance Functions) OPERATOR’S MANUAL

B-63874EN-1

Dual Check Safety

Dual Check Safety CONNECTION MANUAL

B-64483EN-2

- 4 -

B-64484EN-2/02

GENERAL

1.GENERAL

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

B-65262EN

FANUC AC SPINDLE MOTOR αi series DESCRIPTIONS

B-65272EN

FANUC AC SERVO MOTOR βi series DESCRIPTIONS

B-65302EN

FANUC AC SPINDLE MOTOR βi series DESCRIPTIONS

B-65312EN

FANUC SERVO AMPLIFIER αi series DESCRIPTIONS

B-65282EN

FANUC SERVO AMPLIFIER βi series DESCRIPTIONS

B-65322EN

FANUC SERVO MOTOR αis series

FANUC SERVO MOTOR αi series

FANUC AC SPINDLE MOTOR αi series

B-65285EN

FANUC SERVO AMPLIFIER αi series

MAINTENANCE MANUAL

FANUC SERVO MOTOR βis series

FANUC AC SPINDLE MOTOR βi series

B-65325EN

FANUC SERVO AMPLIFIER βi series

MAINTENANCE MANUAL

FANUC AC SERVO MOTOR αi series

FANUC AC SERVO MOTOR βi series

FANUC LINEAR MOTOR LiS series

B-65270EN

FANUC SYNCHRONOUS BUILT-IN SERVO MOTOR DiS series

PARAMETER MANUAL

FANUC AC SPINDLE MOTOR αi/βi series,

BUILT-IN SPINDLE MOTOR Bi series

B-65280EN

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.

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.

- 5 -

1.GENERAL

GENERAL

B-64484EN-2/02

1.1

NOTES ON READING THIS MANUAL

CAUTION

1 The function of an CNC machine tool system depends not only on the CNC, but on

the combination of the machine tool, its magnetic cabinet, the servo system, the

CNC, the operator's panels, etc. It is too difficult to describe the function,

programming, and operation relating to all combinations. This manual generally

describes these from the stand-point of the CNC. So, for details on a particular

CNC machine tool, refer to the manual issued by the machine tool builder, which

should take precedence over this manual.

2 In the header field of each page of this manual, a chapter title is indicated so that

the reader can reference necessary information easily.

By finding a desired title first, the reader can reference necessary parts only.

3 This manual describes as many reasonable variations in equipment usage as

possible. It cannot address every combination of features, options and commands

that should not be attempted.

If a particular combination of operations is not described, it should not be

attempted.

1.2

NOTES ON VARIOUS KINDS OF DATA

CAUTION

Machining programs, parameters, offset data, etc. are stored in the CNC unit

internal non-volatile memory. In general, these contents are not lost by the

switching ON/OFF of the power. However, it is possible that a state can occur

where precious data stored in the non-volatile memory has to be deleted,

because of deletions from a maloperation, or by a failure restoration. In order to

restore rapidly when this kind of mishap occurs, it is recommended that you

create a copy of the various kinds of data beforehand.

- 6 -

B-64484EN-2/02

PROGRAMMING

1.GENERAL

1 GENERAL

Chapter 1, "GENERAL", consists of the following sections:

1.1 TOOL FIGURE AND TOOL MOTION BY PROGRAM

1.1

TOOL FIGURE AND TOOL MOTION BY PROGRAM

Explanation

Machining using the end of cutter - Tool length compensation function

Usually, several tools are used for machining one workpiece. The tools have different tool length. It is

very troublesome to change the program in accordance with the tools.

Therefore, the length of each tool used should be measured in advance. By setting the difference between

the length of the standard tool and the length of each tool in the CNC (See Chapter, “Setting and

Displaying Data” in OPERATOR’S MANUAL (Common to Lathe System / Machining Center System)),

machining can be performed without altering the program even when the tool is changed. This function is

called tool length compensation (See Section, “Tool Length Compensation” in OPERATOR’S MANUAL

(Common to Lathe System / Machining Center System)).

Standard

tool

Workpiece

Machining using the side of cutter - Cutter compensation function

Cutter path using cutter compensation

Machined part figure

Workpiece

Tool

Because a cutter has a radius, the center of the cutter path goes around the workpiece with the cutter

radius deviated.

If radius of cutters are stored in the CNC (See Chapter, “Setting and Displaying Data” in OPERATOR’S

MANUAL (Common to Lathe System / Machining Center System)), the tool can be moved by cutter

radius apart from the machining part figure. This function is called cutter compensation (See Chapter,

“Compensation Function”).

- 9 -

2. PREPARATORY FUNCTION

(G FUNCTION)

PROGRAMMING

B-64484EN-2/02

2 PREPARATORY FUNCTION

(G FUNCTION)

A number following address G determines the meaning of the command for the concerned block.

G codes are divided into the following two types.

Type

Meaning

One-shot G code

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_ ;

Explanation

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

as indicated in Table 2 (a).

(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. 3402.

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

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.

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.

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.

G codes are indicated by group.

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

- 10 -

2.PREPARATORY FUNCTION

B-64484EN-2/02

PROGRAMMING

(G FUNCTION)

Table 2 (a) G code list

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

3-dimensional coordinate system conversion CW/CCW

G04

Dwell

AI contour control (high-precision contour control compatible command),

G05

High-speed cycle machining, High-speed binary program operation

G05.1

AI contour control / Nano smoothing / Smooth interpolation

G05.4

HRV3, 4 on/off

G06.2

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

Programmable data input mode cancel

G12.1

Polar coordinate interpolation mode

G13.1

Polar coordinate interpolation cancel mode

G12.4

Groove cutting by continuous circle motion (CW)

G13.4

Groove cutting by continuous circle motion (CCW)

G15

Polar coordinates command cancel

G16

Polar coordinates command

G17

XpYp plane selection

Xp: X axis or its parallel axis

G17.1

Plane conversion function

Yp: Y axis or its parallel axis

G18

ZpXp plane selection

Zp: Z axis or its parallel axis

G19

YpZp plane selection

G20 (G70)

Input in inch

G21 (G71)

Input in mm

G22

Stored stroke check function on

G23

Stored stroke check function off

G25

Spindle speed fluctuation detection off

G26

Spindle speed fluctuation detection on

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

EGB-axis skip

G33

Threading

G34

Variable lead threading

G35

Circular threading CW

G36

Circular threading CCW

- 11 -

2. PREPARATORY FUNCTION

(G FUNCTION)

PROGRAMMING

B-64484EN-2/02

Table 2 (a) G code list

G code

Group

Function

G37

Automatic tool length measurement

G38

Tool radius/tool nose radius compensation : preserve vector

G39

Tool radius/tool nose radius compensation : corner circular interpolation

G40

Tool radius/tool nose radius compensation : cancel

3-dimensional cutter compensation : cancel

Tool radius/tool nose radius compensation : left

G41

3-dimensional cutter compensation : left

Tool radius/tool nose radius compensation : right

G42

3-dimensional cutter compensation : right

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)

G42.2

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

3-dimensional cutter compensation : right (type 2)

G40.1

Normal direction control cancel mode

G41.1

Normal direction control on : left

G42.1

Normal direction control on : right

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)

G45

Tool offset : increase

G46

Tool offset : decrease

G47

Tool offset : double increase

G48

Tool offset : double decrease

G49 (G49.1)

Tool length compensation cancel

G44.9

Spindle unit compensation

G49.9

Spindle unit compensation cancel

G50

Scaling cancel

G51

Scaling

G50.1

Programmable mirror image cancel

G51.1

Programmable mirror image

G50.2

Polygon turning cancel

G51.2

Polygon turning

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

Start superimposed control

G52

Local coordinate system setting

G53

Machine coordinate system setting

G53.1

Tool axis direction control

G53.6

Tool center point retention type tool axis direction control

- 12 -

2.PREPARATORY FUNCTION

B-64484EN-2/02

PROGRAMMING

(G FUNCTION)

Table 2 (a) G code list

G code

Group

Function

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

Workpiece coordinate system 6 selection

G54.2

Rotary table dynamic fixture offset

G54.4

Workpiece setting error compensation

G60

Single direction positioning

G61

Exact stop mode

G62

Automatic corner override

G63

Tapping mode

G64

Cutting mode

G65

Macro call

G66

Macro modal call A

G66.1

Macro modal call B

G67

Macro modal call A/B cancel

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

Tilted working plane command (incremental multi-command)

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

Figure copying (linear copy)

G73

Peck drilling cycle

G74

Left-handed tapping cycle

G75

Plunge grinding cycle

G76

Fine boring cycle

G77

Plunge direct sizing/grinding cycle

G78

Continuous-feed surface grinding cycle

G79

Intermittent-feed surface grinding cycle

Canned cycle cancel

G80

Electronic gear box : synchronization cancellation

G80.4

Electronic gear box: synchronization cancellation

G81.4

Electronic gear box: synchronization start

G80.5

Electronic gear box 2 pair: synchronization cancellation

G81.5

Electronic gear box 2 pair: synchronization start

Drilling cycle or spot boring cycle

G81

Electronic gear box : synchronization start

G81.1

Chopping

- 13 -

2. PREPARATORY FUNCTION

(G FUNCTION)

PROGRAMMING

B-64484EN-2/02

Table 2 (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

Boring cycle

G90

Absolute programming

G91

Incremental programming

G91.1

Checking the maximum incremental amount specified

G92

Setting for workpiece coordinate system or clamp at maximum spindle speed

G92.1

Workpiece coordinate system preset

G93

Inverse time feed

G94

Feed per minute

G95

Feed per revolution

G96

Constant surface speed control

G97

Constant surface speed control cancel

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

SV speed control mode ON

G98

Canned cycle : return to initial level

G99

Canned cycle : return to R point level

G107

Cylindrical interpolation

G112

Polar coordinate interpolation mode

G113

Polar coordinate interpolation mode cancel

G160

In-feed control cancel

G161

In-feed control

- 14 -

B-64484EN-2/02

PROGRAMMING

3.INTERPOLATION FUNCTION

3 INTERPOLATION FUNCTION

Chapter 3, "INTERPOLATION FUNCTION", consists of the following sections:

3.1 INVOLUTE INTERPOLATION (G02.2, G03.2)

3.2 THREADING (G33)

3.3 CONTINUOUS THREADING

3.4 MULTIPLE THREADING

3.5 CIRCULAR THREAD CUTTING B (G2.1,G3.1)

3.6 GROOVE CUTTING BY CONTINUOUS CIRCLE MOTION (G12.4, G13.4)

3.1

INVOLUTE INTERPOLATION (G02.2, G03.2)

Overview

Involute curve machining can be performed by using involute interpolation. Cutter compensation can be

performed. Involute interpolation eliminates the need for approximating an involute curve with minute

segments or arcs, and continuous pulse distribution is ensured even in high-speed operation of small

blocks. Accordingly, high-speed operation can be performed smoothly. Moreover, machining programs

can be created more easily, and the size of machining programs can be reduced.

In involute interpolation, the following two types of feedrate override functions are automatically

executed, and a favorable cutting surface can be formed with high precision. (Automatic speed control

function for involute interpolation)

• Override in cutter compensation mode

• Override in the vicinity of basic circle

Format

Involute interpolation on the Xp-Yp plane

G17 G02.2 Xp_ Yp_ I_ J_ R_ F_ ;

G17 G03.2 Xp_ Yp_ I_ J_ R_ F_ ;

Involute interpolation on the Zp-Xp plane

G18 G02.2 Zp_ Xp_ K_ I_ R_ F_ ;

G18 G03.2 Zp_ Xp_ K_ I_ R_ F_ ;

Involute interpolation on the Yp-Zp plane

G19 G02.2 Yp_ Zp_ J_ K_ R_ F_ ;

G19 G03.2 Yp_ Zp_ J_ K_ R_ F_ ;

Where,

G02.2

: Involute interpolation (clockwise)

G03.2

: Involute interpolation (counterclockwise)

G17/G18/G19 : Xp-Yp/Zp-Xp/Yp-Zp plane selection

Xp_

: X-axis or an axis parallel to the X-axis (specified in a parameter)

Yp_

: Y-axis or an axis parallel to the Y-axis (specified in a parameter)

Zp_

: Z-axis or an axis parallel to the Z-axis (specified in a parameter)

I_, J_, K_

: Center of the base circle for an involute curve viewed from the start point

: Base circle radius

: Cutting feedrate

- 15 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64484EN-2/02

Explanation

Involute curve machining can be performed by using involute interpolation. Involute interpolation

ensures continuous pulse distribution even in high-speed operation in small blocks, thus enabling smooth

and high-speed machining. Moreover, machining programs can be created more easily, and the size of

machining programs can be reduced.

End point

Start

point

Base circle

Pe End point

Clockwise involute interpolation (G02.2)

End point

Start point

End

point

Start point

Counterclockwise involute interpolation (G03.2)

Fig. 3.1 (a) Actual movement

Involute curve

An involute curve on the X-Y plane is defined as follows ;

X (θ) = R [cos θ + (θ - θO) sin θ] + XO

Y (θ) = R [sin θ - (θ - θO) cos θ] + YO

where,

XO, YO

: Coordinates of the center of a base circle

: Base circle radius

θO

: Angle of the start point of an involute curve

: Angle of the point where a tangent from the current position to the base circle contacts the

base circle

X (θ), Y (θ) : Current position on the X-axis and Y-axis

- 16 -

B-64484EN-2/02

PROGRAMMING

3.INTERPOLATION FUNCTION

Involute curve

Start point

(X, Y)

R θo

(Xo, Yo)

End point

Base circle

Fig. 3.1 (b) Involute curve

Involute curves on the Z-X plane and Y-Z plane are defined in the same way as an involute curve on the

X-Y plane.

Start point and end point

The end point of an involute curve is specified using address Xp, Yp, or Zp. An absolute value or

incremental value is used to specify an Xp, Yp, or Zp value. When using an incremental value, specify

the coordinates of the end point viewed from the start point of the involute curve.

When no end point is specified, alarm PS0241 is issued.

If the specified start point or end point lies within the base circle, alarm PS0242 is issued. The same alarm

is issued if cutter compensation C causes the offset vector to enter the base circle. Be particularly careful

when applying an offset to the inside of an involute curve.

Base circle specification

The center of a base circle is specified with I, J, and K, corresponding to X, Y, and Z. The value

following I, J, or K is a vector component defined when the center of the base circle is viewed from the

start point of the involute curve; this value must always be specified as an incremental value, regardless

of the G90/G91 setting. Assign a sign to I, J, and K according to the direction.

If I, J, and K are all left unspecified, or I0, J0, K0 is specified, alarm PS0241 or PS0242 is issued.

If R is not specified, or R ≤ 0, alarm PS0241 or PS0242 is issued.

Choosing from two types of involute curves

When only a start point and I, J, and K data are given, two types of involute curves can be created. One

type of involute curve extends towards the base circle, and the other extends away from the base circle.

When the specified end point is closer to the center of the base circle than the start point, the involute

curve extends toward the base circle. In the opposite case, the involute curve extends away from the base

circle.

Feedrate

The cutting feedrate specified in an F code is used as the feedrate for involute interpolation. The feedrate

along the involute curve (feedrate along the tangent to the involute curve) is controlled to satisfy the

specified feedrate.

Plane selection

As with circular interpolation, the plane to which to apply involute interpolation can be selected using

G17, G18, and G19.

Cutter compensation

Cutter compensation can be applied to involute curve machining. As with linear and circular interpolation,

G40, G41, and G42 are used to specify cutter compensation.

G40: Cutter compensation cancel

- 17 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64484EN-2/02

G41: Cutter compensation left

G42: Cutter compensation right

First, a point of intersection with a segment or an arc is approximated both at the start point and at the end

point of the involute curve. An involute curve passing the two approximated points of intersection with

the start point and end pint becomes the tool center path.

Before selecting the involute interpolation mode, specify G41 or G42, cancel involute interpolation, and

then specify G40. G41, G42, and G40 for cutter compensation cannot be specified in the involute

interpolation mode.

Automatic speed control

Cutting precision can be improved by automatically overriding the programmed feedrate during involute

interpolation. See a subsequent subsection, "Automatic Speed Control for Involute Interpolation."

Specifiable G codes

The following G codes can be specified in involute interpolation mode:

G04

: Dwell

G10

: Programmable data input

G17

: X-Y plane selection

G18

: Z-X plane selection

G19

: Y-Z plane selection

G65

: Macro call

G66

: Macro modal call

G67

: Macro modal call cancel

G90

: Absolute programming

G91

: Incremental programming

Modes that allow involute interpolation specification

Involute interpolation can be specified in the following G code modes:

G41

: Cutter compensation left

G42

: Cutter compensation right

G51

: Scaling

G51.1

: Programmable mirror image

G68

: Coordinate rotation

End point error

As shown below the end point may not be located on an involute curve that passes through the start point

(Fig. 3.1 (c)).

When an involute curve that passes through the start point deviates from the involute curve that passes

through the end point by more than the value set in parameter No. 5610, alarm PS0243 is issued.

If there is an end point error, the programmed feedrate changes by the amount of error.

End point

Path after correction

Deviation

Start point

Correct involute curve

Fig. 3.1 (c) End point error in counterclockwise involute interpolation (G03.2)

- 18 -

B-64484EN-2/02

PROGRAMMING

3.INTERPOLATION FUNCTION

3.1.1

Automatic Speed Control for Involute Interpolation

This function automatically overrides the programmed feedrate in two different ways during involute

interpolation. With this function, a favorable cutting surface can be formed with high precision.

• Override in cutter compensation mode

• Override in the vicinity of basic circle

Override in cutter compensation mode

When cutter compensation is applied to involute interpolation, control is exercised in ordinary involute

interpolation so that the tangential feedrate on the tool-center path always keeps the specified feedrate.

Under the control, the actual cutting feedrate (feedrate around the perimeter of the tool (cutting point) on

the path specified in the program) changes because the curvature of the involute curve changes every

moment.

If the tool is offset in the inward direction of the involute curve in particular, the actual cutting feedrate

becomes higher than the specified feedrate as the tool gets nearer to the base circle.

For smooth machining, it is desirable to control the actual cutting feedrate so that the feedrate keeps the

specified feedrate. This function calculates an appropriate override value for the ever-changing curvature

of the involute curve in the involute interpolation mode after cutter compensation. The function also

controls the actual cutting feedrate (tangential feedrate at the cutting point) so that it always keeps the

specified feedrate.

Cutting point

Rofs

Path specified in

the program

Rcp

Base

circle

Fig. 3.1 (d) Override for inward offset by cutter compensation

Inward offset

OVR = Rcp/(Rcp + Rofs) × 100

Outward offset

OVR = Rcp/(Rcp - Rofs) × 100

where,

Rcp :

Radius of curvature at the center of the tool of the involute curve passing through the center of

the tool

Rofs :

Radius of the cutter

Clamping the override

The lower limit of override is specified in parameter No. 5620 so that the override for inward offset by

cutter compensation or the override in the vicinity of the basic circle will not bring the speed of the tool

center to zero in the vicinity of the basic circle.

The lower limit of override (OVR1o) is specified in parameter No. 5620 so that the inward offset will not

reduce the speed of the tool center to a very low level in the vicinity of the basic circle.

- 19 -

3.INTERPOLATION FUNCTION

PROGRAMMING

B-64484EN-2/02

Accordingly, the feedrate is clamped but does not fall below the level determined by the programmed

feedrate and the lower limit of override (OVR1o).

The outward offset may increase the override to a very high level, but the feedrate will not exceed the

maximum cutting feedrate.

Clamping the acceleration in the vicinity of basic circle

If the acceleration calculated from the radius of curvature of the involute curve exceeds a value specified

in the corresponding parameter, the tangential velocity is controlled so that the actual acceleration will not

exceed the value specified in the parameter. Because the acceleration is always limited to a constant level,

efficient velocity control can be performed for each machine. Because smooth velocity control can be

performed continuously, impacts in machining in the vicinity of the basic circle can be reduced.

To calculate the acceleration, the radius of curvature of the involute curve and the tangential velocity are

substituted into the following formula of circular acceleration:

Acceleration = F × F/R

F: Tangential velocity

R: Radius of curvature

The maximum permissible acceleration is specified in parameter No. 1735.

If the calculated acceleration exceeds the maximum permissible acceleration, the feedrate is clamped to

the level calculated by the following expression:

Clamp level=

Radius of curvature ×Maximum permissible acceleration

If the calculated clamp level falls below the lower limit of feedrate, the lower limit of feedrate becomes

the clamp level. The lower limit of feedrate is specified in parameter No. 1732.

3.1.2

Helical Involute Interpolation (G02.2, G03.2)

As with arc helical involute interpolation, this function performs helical involute interpolation on the two

axes involute interpolation and on up to four other axes simultaneously.

Format

Helical involute interpolation in Xp-Yp plane

G02.2

G17

Xp Yp I J R α β γ δ F

;

G03.2

Helical involute interpolation in Zp-Xp plane

G02.2

G18

Zp Xp K I R α β γ δ F

;

G03.2

Helical involute interpolation in Yp-Zp plane

G02.2

G19

Yp Zp J K R α β γ δ F

;

G03.2

α, β, γ, δ : Optional axis other than the axes of involute interpolation. Up to four axes can

be specified.

- 20 -

B-64484EN-2/02

PROGRAMMING

3.INTERPOLATION FUNCTION

3.1.3

Involute Interpolation on Linear Axis and Rotary Axis

(G02.2, G03.2)

By performing involute interpolation in the polar coordinate interpolation mode, involute cutting can be

carried out. Cutting is performed along an involute curve drawn in the plane formed by a linear axis and a

rotary axis.

Format

If the linear axis is the X-axis or an axis parallel to the X-axis, the plane is considered to

be the Xp-Yp plane, and I and J are used.

G02.2

X C I J R F

;

G03.2

If the linear axis is the Y-axis or an axis parallel to the Y-axis, the plane is considered to

be the Yp-Zp plane, and J and K are used.

G02.2

Y C J K R F

;

G03.2

If the linear axis is the Z-axis or an axis parallel to the Z-axis, the plane is considered to

be the Zp-Xp plane, and K and I are used.

G02.2

Z C K I R F

;

G03.2

G02.2 :

Clockwise involute interpolation

G03.2 :

Counterclockwise involute interpolation

Example) If the linear axis is the X-axis

X, C

End point of the involute curve

I, J

Center of the basic circle of the involute curve, viewed from the start point

Radius of basic circle

Cutting feedrate

- 21 -

FANUC Series 30i-MODEL B, 31i-MODEL B, 32i-MODEL B. For Machining Center System. OPERATOR'S MANUAL - page 1