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

Download

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

For Lathe System

OPERATOR'S MANUAL

B-64484EN-1/03

• 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 a serious accident or loss is predicted due to a failure of the product, pay careful attention to 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-1/03 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-1/03

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 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. 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-1/03 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

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-1/03

WARNING

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-1/03 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

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-1/03

WARNING

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-1/03 SAFETY PRECAUTIONS

WARNINGS RELATED TO DAILY MAINTENANCE

WARNING

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/Machining Center System) for details of the battery

replacement procedure.

WARNING

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.

series Maintenance Manual for details

s-7

SAFETY PRECAUTIONS B-64484EN-1/03

WARNING

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-1/03 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 OFFSET ........................................................................................................9

2 PREPARATORY FUNCTION (G FUNCTION) ...................................... 10

3 INTERPOLATION FUNCTION ..............................................................15

3.1 CONSTANT LEAD THREADING (G32) ...................................................... 15

3.2 CONTINUOUS THREADING....................................................................... 18

3.3 MULTIPLE THREADING ............................................................................. 19

4 FUNCTIONS TO SIMPLIFY PROGRAMMING .....................................21

4.1 CANNED CYCLE (G90, G92, G94) ............................................................. 21

4.1.1 Outer Diameter/Internal Diameter Cutting Cycle (G90) ........................................22

4.1.1.1 Straight cutting cycle ......................................................................................... 22

4.1.1.2 Taper cutting cycle ............................................................................................ 23

4.1.2 Threading Cycle (G92)...........................................................................................24

4.1.2.1 Straight threading cycle ..................................................................................... 24

4.1.2.2 Taper threading cycle ........................................................................................ 27

4.1.3 End Face Turning Cycle (G94) ..............................................................................30

4.1.3.1 Face cutting cycle .............................................................................................. 30

4.1.3.2 Taper cutting cycle ............................................................................................ 31

4.1.4 How to Use Canned Cycles (G90, G92, G94)........................................................32

4.1.5 Canned Cycle and Tool Nose Radius Compensation .............................................34

4.1.6 Restrictions on Canned Cycles ...............................................................................35

4.2 MULTIPLE REPETITIVE CANNED CYCLE (G70-G76) .............................. 38

4.2.1 Stock Removal in Turning (G71) ...........................................................................39

4.2.2 Stock Removal in Facing (G72) .............................................................................51

4.2.3 Pattern Repeating (G73) .........................................................................................55

4.2.4 Finishing Cycle (G70) ............................................................................................58

4.2.5 End Face Peck Drilling Cycle (G74) ......................................................................62

4.2.6 Outer Diameter / Internal Diameter Drilling Cycle (G75) .....................................64

4.2.7 Multiple Threading Cycle (G76) ............................................................................66

4.2.8 Restrictions on Multiple Repetitive Canned Cycle (G70-G76)..............................71

4.3 CANNED CYCLE FOR DRILLING............................................................... 74

c-1

TABLE OF CONTENTS B-64484EN-1/03

4.3.1 Front Drilling Cycle (G83)/Side Drilling Cycle (G87) ..........................................77

4.3.2 Front Tapping Cycle (G84) / Side Tapping Cycle (G88).......................................80

4.3.3 Front Boring Cycle (G85) / Side Boring Cycle (G89) ...........................................81

4.3.4 Canned Cycle for Drilling Cancel (G80)................................................................82

4.3.5 Canned Cycle for Drilling with M Code Output Improved....................................82

4.3.6 Precautions to be Taken by Operator .....................................................................83

4.4 IN-POSITION CHECK SWITCHING FOR DRILLING CANNED CYCLE..... 83

4.5 RIGID TAPPING .......................................................................................... 90

4.5.1 Front Face Rigid Tapping Cycle (G84) / Side Face Rigid Tapping Cycle (G88)..90

4.5.2 Peck Rigid Tapping Cycle (G84 or G88) ...............................................................96

4.5.3 Canned Cycle Cancel (G80) .................................................................................100

4.5.4 Override during Rigid Tapping ............................................................................100

4.5.4.1 Extraction override .......................................................................................... 100

4.5.4.2 Override signal ................................................................................................ 101

4.6 CANNED GRINDING CYCLE (FOR GRINDING MACHINE)..................... 103

4.6.1 Traverse Grinding Cycle (G71)............................................................................105

4.6.2 Traverse Direct Constant-Size Grinding Cycle (G72) .........................................107

4.6.3 Oscillation Grinding Cycle (G73) ........................................................................109

4.6.4 Oscillation Direct Constant-Size Grinding Cycle (G74) ......................................111

4.7 CHAMFERING AND CORNER R .............................................................. 113

4.8 MIRROR IMAGE FOR DOUBLE TURRET (G68, G69) ............................. 119

4.9 DIRECT DRAWING DIMENSION PROGRAMMING ................................. 120

5 COMPENSATION FUNCTION ............................................................126

5.1 TOOL OFFSET..........................................................................................126

5.1.1 Tool Geometry Offset and Tool Wear Offset.......................................................126

5.1.2 T Code for Tool Offset .........................................................................................127

5.1.3 Tool Selection.......................................................................................................127

5.1.4 Offset Number......................................................................................................128

5.1.5 Offset....................................................................................................................128

5.1.6 Y Axis Offset........................................................................................................131

5.1.6.1 Support of arbitrary axes for Y axis offset ......................................................131

5.1.7 Second Geometry Tool Offset..............................................................................131

5.1.8 4th/5th Axis Offset ...............................................................................................134

5.2 OVERVIEW OF TOOL NOSE RADIUS COMPENSATION (G40-G42) ..... 136

5.2.1 Imaginary Tool Nose ............................................................................................136

5.2.2 Direction of Imaginary Tool Nose .......................................................................138

5.2.3 Offset Number and Offset Value..........................................................................139

5.2.4 Workpiece Position and Move Command............................................................140

5.2.5 Notes on Tool Nose Radius Compensation ..........................................................145

5.3 OVERVIEW OF CUTTER COMPENSATION (G40-G42).......................... 148

5.4 DETAILS OF CUTTER OR TOOL NOSE RADIUS COMPENSATION...... 154

5.4.1 Overview ..............................................................................................................154

5.4.2 Tool Movement in Start-up ..................................................................................158

5.4.3 Tool Movement in Offset Mode...........................................................................164

5.4.4 Tool Movement in Offset Mode Cancel...............................................................183

5.4.5 Prevention of Overcutting Due to Cutter or Tool Nose Radius Compensation ...189

5.4.6 Interference Check ...............................................................................................192

5.4.6.1 Operation to be performed if an interference is judged to occur ..................... 196

5.4.6.2 Interference check alarm function ...................................................................196

5.4.6.3 Interference check avoidance function ............................................................ 198

5.4.7 Cutter or Tool Nose Radius Compensation for Input from MDI .........................203

5.5 VECTOR RETENTION (G38) .................................................................... 205

c-2

B-64484EN-1/03 TABLE OF CONTENTS

5.6 CORNER CIRCULAR INTERPOLATION (G39) ........................................ 206

5.7 EXTENDED TOOL SELECTION ............................................................... 208

5.8 AUTOMATIC TOOL OFFSET (G36, G37)................................................. 211

5.9 COORDINATE SYSTEM ROTATION (G68.1, G69.1)............................... 214

5.10 ACTIVE OFFSET VALUE CHANGE FUNCTION BASED ON MANUAL

FEED .........................................................................................................218

6 MEMORY OPERATION USING Series 15 FORMAT.........................222

6.1 ADDRESSES AND SPECIFIABLE VALUE RANGE FOR Series 15

PROGRAM FORMAT ................................................................................ 222

6.2 SUBPROGRAM CALLING ........................................................................ 222

6.3 CANNED CYCLE....................................................................................... 223

6.3.1 Outer Diameter/Internal Diameter Cutting Cycle (G90) ......................................224

6.3.1.1 Straight cutting cycle ....................................................................................... 224

6.3.1.2 Taper cutting cycle .......................................................................................... 225

6.3.2 Threading Cycle (G92).........................................................................................226

6.3.2.1 Straight threading cycle ................................................................................... 226

6.3.2.2 Taper threading cycle ...................................................................................... 229

6.3.3 End Face Turning Cycle (G94) ............................................................................232

6.3.3.1 Face cutting cycle ............................................................................................ 232

6.3.3.2 Taper cutting cycle .......................................................................................... 233

6.3.4 How to Use Canned Cycles ..................................................................................235

6.3.5 Canned Cycle and Tool Nose Radius Compensation ...........................................236

6.3.6 Restrictions on Canned Cycles .............................................................................237

6.4 MULTIPLE REPETITIVE CANNED CYCLE ..............................................240

6.4.1 Stock Removal in Turning (G71) .........................................................................241

6.4.2 Stock Removal in Facing (G72) ...........................................................................253

6.4.3 Pattern Repeating (G73) .......................................................................................257

6.4.4 Finishing Cycle (G70) ..........................................................................................260

6.4.5 End Face Peck Drilling Cycle (G74) ....................................................................264

6.4.6 Outer Diameter / Internal Diameter Drilling Cycle (G75) ...................................266

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

(G78 <G code system C>)....................................................................................268

6.4.8 Restrictions on Multiple Repetitive Canned Cycle ..............................................274

6.5 CANNED CYCLE FOR DRILLING............................................................. 276

6.5.1 High-speed Peck Drilling Cycle (G83.1) .............................................................280

6.5.2 Drilling Cycle, Spot Drilling Cycle (G81) ...........................................................281

6.5.3 Drilling Cycle, Counter Boring (G82) .................................................................282

6.5.4 Peck Drilling Cycle (G83)....................................................................................283

6.5.5 Tapping Cycle (G84) ............................................................................................285

6.5.6 Boring Cycle (G85) ..............................................................................................286

6.5.7 Boring Cycle (G89) ..............................................................................................287

6.5.8 Canned Cycle for Drilling Cancel (G80)..............................................................288

6.5.9 Precautions to be Taken by Operator ...................................................................288

7 MUITI-PATH CONTROL FUNCTION.................................................. 289

7.1 BALANCE CUT (G68, G69)....................................................................... 289

III. OPERATION

1 DATA INPUT/OUTPUT ....................................................................... 297

1.1 INPUT/OUTPUT ON EACH SCREEN ....................................................... 297

1.1.1 Inputting and Outputting Y-axis Offset Data .......................................................297

c-3

TABLE OF CONTENTS B-64484EN-1/03

1.1.1.1 Inputting Y-axis offset data ............................................................................. 297

1.1.1.2 Outputting Y-axis Offset Data......................................................................... 298

1.1.2 Inputting and Outputting Tool Offset / 2nd Geometry Data ................................299

1.1.2.1 Inputting tool offset / 2nd geometry data......................................................... 299

1.1.2.2 Outputting tool offset / 2nd geometry data...................................................... 300

1.1.3 Inputting and Outputting 4th/5th Axis Offset Data ..............................................300

1.1.3.1 Inputting 4th/5th axis offset data ..................................................................... 300

1.1.3.2 Outputting 4th/5th Axis Offset Data................................................................ 301

1.2 INPUT/OUTPUT ON THE ALL IO SCREEN.............................................. 303

1.2.1 Inputting and Outputting Y-axis Offset Data .......................................................304

1.2.2 Inputting and Outputting Tool Offset / 2nd Geometry Tool Offset .....................305

2 SETTING AND DISPLAYING DATA...................................................307

2.1 SCREENS DISPLAYED BY FUNCTION KEY ................................... 307

2.1.1 Setting and Displaying the Tool Offset Value .....................................................307

2.1.2 Direct Input of Tool Offset Value ........................................................................312

2.1.3 Direct Input of Tool Offset Value Measured B ....................................................315

2.1.4 Counter Input of Offset value...............................................................................317

2.1.5 Setting the Workpiece Coordinate System Shift Value........................................318

2.1.6 Setting Tool Offset/Second Geometry Tool Offset Values ..................................321

2.1.7 Setting the Y-Axis Offset .....................................................................................324

2.1.8 Setting the 4th/5th Axis Offset .............................................................................330

2.1.9 Chuck and Tail Stock Barriers .............................................................................335

APPENDIX

A PARAMETERS.................................................................................... 345

A.1 DESCRIPTION OF PARAMETERS........................................................... 345

A.2 DATA TYPE............................................................................................... 382

A.3 STANDARD PARAMETER SETTING TABLES......................................... 383

c-4

I. GENERAL

B-64484EN-1/03 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, characteristics, and

restrictions. III. OPERATION Describes the manual operation and automatic operation of a machine, procedures for inputting and

outputting data, and procedures for editing a program. APPENDIX Lists parameters.

NOTE

1 This manual describes the functions that can operate in the lathe system path

control type. For other functions not specific to the lathe system, refer to the Operator's Manual (Common to Lathe System/Machining Center System) (B-63484EN).

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 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).

Series 31i

- 3 -

1.GENERAL GENERAL B-64484EN-1/03

Special symbols

This manual uses the following symbols:

- IP

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

- ;

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

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 (a) 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) 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

- 4 -

B-64484EN-1/03 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 1 (b) 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. 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.

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-1/03

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-1/03 PROGRAMMING 1.GENERAL

1 GENERAL

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

1.1 OFFSET................................................................................................................................................9

1.1 OFFSET

Explanation

- Tool offset

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

Therefore, the length of each tool used should be measured in advance. By setting the difference between the length of the standard tool and the length of each tool in the CNC (see Chapter, “Setting and Displaying Data” in the 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 offset.

Standard tool

Rough cutting tool

Finishing tool

Grooving tool

Threading tool

Workpiece

Fig. 1.1 (a) Tool offset

- 9 -

2. PREPARATORY FUNCTION (G FUNCTION)

PROGRAMMING B-64484EN-1/03

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_ ;

There are three G code systems in the lathe system : A,B, and C (Table 2 (a)). Select a G code system using bits 6 (GSB) and 7 (GSC) 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.

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

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

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

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

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

7. G codes are indicated by group.

as indicated in Table.

- 10 -

2.PREPARATORY FUNCTION

B-64484EN-1/03 PROGRAMMING

Table 2 (a) G code list

G code system

A B C

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

G03 G03 G03 Circular interpolation CCW or helical interpolation CCW G02.2 G02.2 G02.2 Involute interpolation CW G02.3 G02.3 G02.3 Exponential interpolation CW G02.4 G02.4 G02.4 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 Floating reference point return

G30.2 G30.2 G30.2

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

G07.1

(G107)

G12.1

(G112)

G13.1

(G113)

G07.1

(G107)

G12.1

(G112)

G13.1

(G113)

Group Function

3-dimensional coordinate system conversion CCW

AI contour control (command compatible with high precision

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

In-position check disable 2nd, 3rd, or 4th reference position return

EGB-axis skip

(G FUNCTION)

- 11 -

2. PREPARATORY FUNCTION (G FUNCTION)

PROGRAMMING B-64484EN-1/03

Table 2 (a) G code list

G code system

A B C

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

G49

(G49.1)

G43.7

(G44.7)

G49

(G49.1)

G43.7

(G44.7)

G49

(G49.1)

Group Function

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) (FS16i-compatible command) 3-dimensional cutter compensation : left (type 1) (FS16i-compatible command)

3-dimensional cutter compensation : right (type 1) (FS16i-compatible command) 3-dimensional cutter compensation : right (type 1) (FS16i-compatible 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".) Tool length compensation cancel (Bit 3 (TCT) of parameter No. 5040 must be "1".)

- 12 -

2.PREPARATORY FUNCTION

B-64484EN-1/03 PROGRAMMING

Table 2 (a) G code list

G code system

A B C

G50 G92 G92 Coordinate system setting or max spindle speed clamp

G50.3 G92.1 G92.1

- G50 G50 Scaling cancel

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

(G250)

G51.2

(G251)

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

G69.1 G69.1 G69.1 17

G50.2

(G250)

G51.2

(G251)

G54

(G54.1)

G50.2

(G250)

G51.2

(G251)

G54

(G54.1)

Group Function

04 Mirror image off for double turret or balance cutting mode

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)

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

(G FUNCTION)

- 13 -

2. PREPARATORY FUNCTION (G FUNCTION)

PROGRAMMING B-64484EN-1/03

Table 2 (a) G code list

G code system

A B C

G70 G70 G72 Finishing cycle G71 G71 G73 Stock removal in turning G72 G72 G74 Stock removal in facing G73 G73 G75 Pattern repeating cycle G74 G74 G76 End face peck drilling cycle G75 G75 G77 Outer diameter/internal diameter drilling cycle G76 G76 G78 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

Multiple-thread cutting cycle

Oscillation direct sizing/grinding cycle Canned cycle cancel for drilling Electronic gear box : synchronization cancellation

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

- 14 -

B-64484EN-1/03 PROGRAMMING 3.INTERPOLATION FUNCTION

3 INTERPOLATION FUNCTION

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

3.1 CONSTANT LEAD THREADING (G32).........................................................................................15

3.2 CONTINUOUS THREADING...........................................................................................................18

3.3 MULTIPLE THREADING.................................................................................................................19

3.1 CONSTANT LEAD THREADING (G32)

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

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

Format

G32IP_F_;

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

Straight thread

_: End point

Tapered screw

Fig. 3.1 (a) Thread types

X axis

End point_

Scroll thread

Start point

Z axis

Fig. 3.1 (b) Example of threading

Explanation

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

- 15 -

3.INTERPOLATION FUNCTION PROGRAMMING B-64484EN-1/03

≤

Tapered thread

45° lead is LZ

lead is LX

α≥45°

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

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

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

Least command increment

Metric input 0.0001 to 500.0000 mm

Inch input 0.000001 to 9.999999 inch

- 16 -

B-64484EN-1/03 PROGRAMMING 3.INTERPOLATION FUNCTION

Example

1. Straight threading

The following values are used in programming :

X axis

2.Tapered threading

X axis

30mm

Zaxis

Thread lead :4mm

Depth of cut :1mm (cut twice) (Metric input, diameter programming)

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

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

Cutting depth in the X axis direction is 1mm (cut twice) (Metric input, diameter programming) G 00 X 12.0 Z72 .0 ; G 32 X 41.0 Z29 .0 F3.5 ; G 00 X 50.0 ; Z 72.0 ; X 10.0 ; (Cut 1mm more for the second cut) G 32 X 39.0 Z29 .0 ; G 00 X 50.0 ; Z 72.0 ;

δ δ

=2mm

=1mm

=3mm

=1.5mm

WARNING

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

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

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

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

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

execution of the first block not specifying threading.

- 17 -

3.INTERPOLATION FUNCTION PROGRAMMING B-64484EN-1/03

WARNING

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

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

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

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

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

without waiting for detection of the one-spindle-rotation signal even if the present block is a threading block.

(Example)

G00 Z0.0 X50.0 ; One-rotation signal is G32 Z10.0 F_ ; : Detected Z20.0 ; : Not detected G32 Z30.0 ; : Not detected

7 Because the constant surface speed control is effective during scroll thread or

tapered screw cutting and the spindle speed changes, the correct thread lead may not be cut. Therefore, do not use the constant surface speed control during threading. Instead, use G97.

8 A movement block preceding the threading block must not specify chamfering or

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

speed is fixed at 100%. 11 Thread cycle retract function is ineffective to G32. 12 If tool offset (with the T code or G43.7) is specified in a block for threading, alarm

PS0509, “TOOL OFFSET COMMAND IS NOT AVAILABLE”, is issued.

3.2 CONTINUOUS THREADING

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

Explanation

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

G32

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

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

G32

- 18 -

B-64484EN-1/03 PROGRAMMING 3.INTERPOLATION FUNCTION

3.3 MULTIPLE THREADING

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

L : Lead

Fig. 3.3 (a) Multiple thread screws.

Format

(Constant lead threading) G32 IP _ F_ Q_ ;

IP : End point F_ : Lead in longitudinal direction

G32 IP _ Q_ ;

Q_ : Threading start angle

Explanation

- Available threading commands

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

Limitation

- Start angle

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

value is not specified, 0 is assumed.

- Start angle increment

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

- Specifiable start angle range

A start angle (Q) of between 0 and 360000 (in 0.001-degree units) can be specified. If a value

greater than 360000 (360 degrees) is specified, it is rounded down to 360000 (360 degrees).

- Multiple threading cycle (G76)

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

- 19 -

3.INTERPOLATION FUNCTION PROGRAMMING B-64484EN-1/03

Example

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

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

- 20 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

4 FUNCTIONS TO SIMPLIFY PROGRAMMING

Chapter 4, "FUNCTIONS TO SIMPLIFY PROGRAMMING", consists of the following sections:

4.1 CANNED CYCLE (G90, G92, G94)..................................................................................................21

4.2 MULTIPLE REPETITIVE CANNED CYCLE (G70-G76)...............................................................38

4.3 CANNED CYCLE FOR DRILLING .................................................................................................74

4.4 IN-POSITION CHECK SWITCHING FOR DRILLING CANNED CYCLE...................................83

4.5 RIGID TAPPING................................................................................................................................90

4.6 CANNED GRINDING CYCLE (FOR GRINDING MACHINE)....................................................103

4.7 CHAMFERING AND CORNER R..................................................................................................113

4.8 MIRROR IMAGE FOR DOUBLE TURRET (G68, G69)...............................................................119

4.9 DIRECT DRAWING DIMENSION PROGRAMMING .................................................................120

4.1 CANNED CYCLE (G90, G92, G94)

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

NOTE

1 Explanatory figures in this section use the ZX plane as the selected plane,

diameter programming for the X-axis, and radius programming for the Z-axis.

When radius programming is used for the X-axis, change U/2 to U and X/2 to X. 2 A canned cycle can be performed on any plane (including parallel axes for plane

definition). When G-code system A is used, however, U, V, and W cannot be set

as a parallel axis. 3 The direction of the length means the direction of the first axis on the plane as

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

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

- 21 -

4. FUNCTIONS TO SIMPLIFY

A’A

PROGRAMMING

PROGRAMMING B-64484EN-1/03

4.1.1 Outer Diameter/Internal Diameter Cutting Cycle (G90)

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

4.1.1.1 Straight cutting cycle

Format

G90X(U)_Z(W)_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.1.1 (a)) in the direction

of the length

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.1.1 (a)) in the

direction of the length

F_ : Cutting feedrate

X axis

4(R)

3(F)

2(F)

Fig. 4.1.1.1 (a) Straight cutting cycle

1(R)

(R)....Rapid traverse

(F)....Cutting fee d

U/2

X/2

Z axis

Explanation

- Operations

A straight cutting cycle performs four operations: (1) Operation 1 moves the tool from the start point (A) to the specified coordinate of the second axis on

the plane (specified X-coordinate for the ZX plane) in rapid traverse.

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

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

(3) Operation 3 moves the tool to the start coordinate of the second axis on the plane (start X-coordinate

for the ZX plane) in cutting feed.

(4) Operation 4 moves the tool to the start coordinate of the first axis on the plane (start Z-coordinate for

the ZX plane) in rapid traverse. (The tool returns to the start point (A).)

NOTE

In single block mode, operations 1, 2, 3 and 4 are performed by pressing the

cycle start button once.

- Canceling the mode

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

- 22 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

4.1.1.2 Taper cutting cycle

Format

G90 X(U)_Z(W)_R_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.1.2 (a)) in the direction

of the length

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.1.2 (a)) in the

direction of the length R_ : Taper amount (R in the Fig. 4.1.1.2 (a)) F_ : Cutting feedrate

X axis

(R) ....Rapid traverse

4(R)

(F)....Cutting feed

3(F)

U/2

X/2

’

Fig. 4.1.1.2 (a) Taper cutting cycle

2(F)

1(R)

Z axis

Explanation

The figure of a taper is determined by the coordinates of the cutting end point (A') in the direction of the length and the sign of the taper amount (address R). For the cycle in the Fig. 4.1.1.2 (a), a minus sign is added to the taper amount.

NOTE

The increment system of address R for specifying a taper depends on the

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

- Operations

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

NOTE

In single block mode, operations 1, 2, 3, and 4 are performed by pressing the

cycle start button once.

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

The tool path is determined according to the relationship between the sign of the taper amount (address R) and the cutting end point in the direction of the length in the absolute or incremental programming as Table 4.1.1.2 (a).

- 23 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING B-64484EN-1/03

Table 4.1.1.2 (a)

Outer diameter machining Internal diameter machining

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

U/2

3(F)

2(F)

4(R)

1(R)

U/2 3(F)

2(F)

4(R)

U/2

3. U < 0, W < 0, R > 0 at |R|≤|U/2|

3(F)

4(R)

2(F)

1(R)

4. U > 0, W < 0, R < 0 at |R|≤|U/2|

U/2

3(F)

2(F)

4(R)

- Canceling the mode

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

1(R)

4.1.2 Threading Cycle (G92)

4.1.2.1 Straight threading cycle

Format

G92 X(U)_Z(W)_F_Q_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.2.1 (a)) in the direction

of the length

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.2.1 (a)) in the

direction of the length Q_ : Angle for shifting the threading start angle (Increment: 0.001 degrees, Valid setting range: 0 to 360 degrees) F_ : Thread lead (L in the Fig. 4.1.2.1 (a))

- 24 -

4.FUNCTIONS TO SIMPLIFY

)

B-64484EN-1/03 PROGRAMMING

X axis

3(R

’

4(R)

2(F

1(R

X/2

(R) ... Rapid traverse

(F).... Cutting feed

PROGRAMMING

U/2

Z axis

Approx.

45°

Detailed chamfered thread

Fig. 4.1.2.1 (a) Straight threading

(The chamfered angle in the left figure is 45 degrees or less because of the delay in the servo system.)

Explanation

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

- Operations

A straight threading cycle performs four operations: (1) Operation 1 moves the tool from the start point (A) to the specified coordinate of the second axis on

the plane (specified X-coordinate for the ZX plane) in rapid traverse.

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

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

(3) Operation 3 moves the tool to the start coordinate of the second axis on the plane (start X-coordinate

for the ZX plane) in rapid traverse. (Retraction after chamfering)

(4) Operation 4 moves the tool to the start coordinate of the first axis on the plane (start Z-coordinate for

the ZX plane) in rapid traverse. (The tool returns to the start point (A).)

CAUTION

Notes on this threading are the same as in threading in G32. However, a stop by

feed hold is as follows; Stop after completion of path 3 of threading cycle.

NOTE

In the single block mode, operations 1, 2, 3, and 4 are performed by pressing

cycle start button once.

- Canceling the mode

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

- Acceleration/deceleration after interpolation for threading

Acceleration/deceleration after interpolation for threading is acceleration/deceleration of exponential interpolation type. By setting bit 5 (THLx) of parameter No. 1610, the same acceleration/deceleration as for cutting feed can be selected. (The settings of bits 1 (CTBx) and 0 (CTLx) of parameter No. 1610 are followed.) However, as a time constant and FL feedrate, the settings of parameter No. 1626 and No. 1627 for the threading cycle are used.

- 25 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

- Time constant and FL feedrate for threading

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

- Thread chamfering

Thread chamfering can be performed. A signal from the machine tool, initiates thread chamfering. The chamfering distance r is specified in a range from 0.1L to 12.7L in 0.1L increments by parameter No.

5130. (In the above expression, L is the thread lead.) A thread chamfering angle between 1 to 89 degrees can be specified in parameter No. 5131. When a value of 0 is specified in the parameter, an angle of 45 degrees is assumed. For thread chamfering, the same type of acceleration/deceleration after interpolation, time constant for acceleration/deceleration after interpolation, and FL feedrate as for threading are used.

NOTE

Common parameters for specifying the amount and angle of thread chamfering

are used for this cycle and threading cycle with G76.

- Retraction after chamfering

The Table 4.1.2.1 (a) lists the feedrate, type of acceleration/deceleration after interpolation, and time constant of retraction after chamfering.

Table 4.1.2.1 (a)

Bit 0 (CFR) of

parameter No. 1611

0 Other than 0

0 0

Parameter No.

1466

Description

Uses the type of acceleration/deceleration after interpolation for threading, time constant for threading (parameter No. 1626), FL feedrate (parameter No. 1627), and retraction feedrate specified in parameter No. 1466. Uses the type of acceleration/deceleration after interpolation for threading, time constant for threading (parameter No. 1626), FL feedrate (parameter No. 1627), and rapid traverse rate specified in parameter No. 1420. Before retraction a check is made to see that the specified feedrate has become 0 (delay in acceleration/deceleration is 0), and the type of acceleration/deceleration after interpolation for rapid traverse is used together with the rapid traverse time constant and the rapid traverse rate (parameter No. 1420).

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

NOTE

During retraction, the machine does not stop with an override of 0% for the

cutting feedrate regardless of the setting of bit 4 (RF0) of parameter No. 1401.

- Shifting the start angle

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

- Feed hold in a threading cycle

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

- 26 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

- Threading cycle retract

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

X axis

Z axis

Rapid traverse

Cutting feed

Ordinary cycle Motion at feed hold

Start point

Feed hold is effected here.

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

CAUTION

Another feed hold cannot be made during retreat.

- Inch threading

Inch threading specified with address E is not allowed.

4.1.2.2 Taper threading cycle

Format

G92 X(U)_Z(W)_R_F_Q_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.2.2 (a)) in the direction

of the length

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.2.2 (a)) in the

direction of the length Q_ : Angle for shifting the threading start angle (Increment: 0.001 degrees, Valid setting range: 0 to 360 degrees) R_ : Taper amount (R in the Fig. 4.1.2.2 (a)) F_ : Thread lead (L in the Fig. 4.1.2.2 (a))

- 27 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING B-64484EN-1/03

X axis

U/2

X/2

’

pprox. 45

3(R)

4(R)

1(R)

2(F)

(The chamfered angle in the left figure is 45 degrees or less because of the delay in the servo system.)

(R)....Rapi d t r averse

(F)....Cutting feed

Z axis

Detailed chamfered thread

Fig. 4.1.2.2 (a) Taper threading cycle

Explanation

The ranges of thread leads and restrictions related to the spindle speed are the same as for threading with G32. The figure of a taper is determined by the coordinates of the cutting end point (A') in the direction of the length and the sign of the taper amount (address R). For the cycle in the Fig. 4.1.2.2 (a), a minus sign is added to the taper amount.

NOTE

The increment system of address R for specifying a taper depends on the

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

- Operations

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

CAUTION

Notes on this threading are the same as in threading in G32. However, a stop by

feed hold is as follows; Stop after completion of path 3 of threading cycle.

- 28 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

NOTE

In the single block mode, operations 1, 2, 3, and 4 are performed by pressing

cycle start button once.

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

Table 4.1.2.2 (a)

Outer diameter machining Internal diameter machining

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

U/2

3(F)

2(F)

4(R)

1(R)

U/2 3(F)

2(F)

4(R)

U/2

3. U < 0, W < 0, R > 0 at |R|≤|U/2|

3(F)

4(R)

2(F)

1(R)

4. U > 0, W < 0, R < 0 at |R|≤|U/2|

U/2

3(F)

2(F)

4(R)

- Canceling the mode

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

- Acceleration/deceleration after interpolation for threading

- Time constant and FL feedrate for threading

- Thread chamfering

- Retraction after chamfering

- Shifting the start angle

- Threading cycle retract

- Inch threading

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

1(R)

- 29 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING B-64484EN-1/03

4.1.3 End Face Turning Cycle (G94)

4.1.3.1 Face cutting cycle

Format

G94 X(U)_Z(W)_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.3.1 (a)) in the direction

of the end face

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.3.1 (a)) in the

direction of the end face

F_ : Cutting feedrate

X axis

1(R)

(R)... R apid traverse

(F) .... Cuttin g fe e d

2(F)

U/2

3(F)

’

X/2

Fig. 4.1.3.1 (a) Face cutting cycle

4(R)

Z axis

Explanation

- Operations

A face cutting cycle performs four operations: (1) Operation 1 moves the tool from the start point (A) to the specified coordinate of the first axis on the

plane (specified Z-coordinate for the ZX plane) in rapid traverse.

(2) Operation 2 moves the tool to the specified coordinate of the second axis on the plane (specified

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

(3) Operation 3 moves the tool to the start coordinate of the first axis on the plane (start Z-coordinate for

the ZX plane) in cutting feed.

(4) Operation 4 moves the tool to the start coordinate of the second axis on the plane (start X-coordinate

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

NOTE

In single block mode, operations 1, 2, 3, and 4 are performed by pressing the

cycle start button once.

- Canceling the mode

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

- 30 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

4.1.3.2 Taper cutting cycle

Format

G94 X(U)_Z(W)_R_F_;

X_,Z_ : Coordinates of the cutting end point (point A' in the Fig. 4.1.3.2 (a)) in the direction

of the end face

U_,W_ : Travel distance to the cutting end point (point A' in the Fig. 4.1.3.2 (a)) in the

direction of the end face R_ : Taper amount (R in the Fig. 4.1.3.2 (a)) F_ : Cutting feedrate

X axis

1(R)

U/2

X/2

Fig. 4.1.3.2 (a) Taper cutting cycle

2(F)

’

4(R)

3(F)

(R)... Rap id tra ve rs e (F) ... Cutting feed

Z axis

Explanation

The figure of a taper is determined by the coordinates of the cutting end point (A') in the direction of the end face and the sign of the taper amount (address R). For the cycle in the Fig. 4.1.3.2 (a), a minus sign is added to the taper amount.

NOTE

The increment system of address R for specifying a taper depends on the

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

- Operations

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

NOTE

In single block mode, operations 1, 2, 3, and 4 are performed by pressing the

cycle start button once.

- 31 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING B-64484EN-1/03

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

The tool path is determined according to the relationship between the sign of the taper amount (address R) and the cutting end point in the direction of the end face in the absolute or incremental programming as Table 4.1.3.2 (a).

Table 4.1.3.2 (a)

Outer diameter machining Internal diameter machining

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

1(R)

U/2

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

U/2

2(F)

at |R|≤|W|

2(F)

3(F)

1(R)

3(F)

4(R)

U/2

2(F)

4. U > 0, W < 0, R > 0 at |R|≤|W|

U/2

2(F)

- Canceling the mode

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

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

3(F)

4(R)

1(R)

3(F)

4(R)

1(R)

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

- Straight cutting cycle (G90)

Shape of material

Shape of product

- 32 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

- Taper cutting cycle (G90)

Shape of material

Shape of product

- Face cutting cycle (G94)

Shape of product

- Face taper cutting cycle (G94)

Shape of material

Shape of product

- 33 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

4.1.5 Canned Cycle and Tool Nose Radius Compensation

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

Outer diameter/internal diameter cutting cycle (G90)

Tool nose radius center path

Offset direction

Tool nose radius center path

Total tool nose

Programmed path

End face cutting cycle (G94)

Tool nose radius center path

Total tool nose

0 3

Total tool nose

Offset direction

Total tool nose

Programmed path

Total tool nose

Threading cycle (G92)

Tool nose radius compensation cannot be applied.

- 34 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

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

NOTE

This CNC is the same as the FANUC Series 16i/18i/21i in the offset direction,

but differs from the series in the tool nose radius center path.

- For this CNC Cycle operations of a canned cycle are replaced with G00 or G01. In the first

block to move the tool from the start point, start-up is performed. In the last block to return the tool to the start point, offset is canceled.

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

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

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

G90 G94

Tool nose radius center path

4,8,3

5,0,7

Tool nose radius center path

4,8,3

5,0,7

1,6,2

Total tool

4,5,1

nose

Programmed path

8,0,6

3,7,2

1,6,2

Total tool nose

Programmed path

4,5,1

8,0,6

3,7,2

4.1.6 Restrictions on Canned Cycles

Limitation

- Modal

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

- 35 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

Example

X axis

The cycle in the above figure is executed by the following program: N030 G90 U-8.0 W-66.0 F0.4; N031 U-16.0; N032 U-24.0; N033 U-32.0;

Workpiece

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

- Block in which no move command is specified

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

Example

N003 T0101; : : N010 G90 X20.0 Z10.0 F0.2; N011 G00 T0202;

Cancels the canned cycle mode.

←

N012 G90 X20.5 Z10.0;

- Plane selection command

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

- Parallel axis

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

- 36 -

4.FUNCTIONS TO SIMPLIFY

)

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

- Reset

If a reset operation is performed during execution of a canned cycle when any of the following states for holding a modal G code of group 01 is set, the modal G code of group 01 is replaced with the G01 mode:

• Reset state (bit 6 (CLR) of parameter No. 3402 = 0)

• Cleared state (bit 6 (CLR) of parameter No. 3402 = 1) and state where the modal G code of group 01

is held at reset time (bit 1 (C01) of parameter No. 3406 = 1) Example of operation) If a reset is made during execution of a canned cycle (X0 block) and the X20.Z1. command is

executed, linear interpolation (G01) is performed instead of the canned cycle.

- Manual intervention

After manual intervention is performed with the manual absolute on command before the execution of a canned cycle or after the stop of the execution, when a cycle operation starts, the manual intervention amount is canceled even with an incremental cycle start command.

Example of G94

Cancellation

2(F

3(F)

1(R)

Manual intervention

4(R

- 37 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

4.2 MULTIPLE REPETITIVE CANNED CYCLE (G70-G76)

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

NOTE

1 Explanatory figures in this section use the ZX plane as the selected plane,

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

2 A multiple repetitive canned cycle can be performed on any plane (including

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

- 38 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

4.2.1 Stock Removal in Turning (G71)

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

Format

ZpXp plane

G71 U(Δd) R(e) ; G71 P(ns) Q(nf) U(Δu) W(Δw) F(f ) S(s ) T(t ) ;

N (ns) ; ... N (nf) ;

YpZp plane

G71 W(Δd) R(e) ; G71 P(ns) Q(nf) V(Δw) W(Δu) F(f ) S(s ) T(t ) ; N (ns) ;

The move commands for the target figure from A to A’ to B are specified in the blocks with sequence numbers ns to nf.

... N (nf) ;

XpYp plane

G71 V(Δd) R(e) ; G71 P(ns) Q(nf) U(Δw) V(Δu) F(f ) S(s ) T(t ) ; N (ns) ; ... N (nf) ;

Δd : Depth of cut The cutting direction depends on the direction AA'. This designation is modal and is

not changed until the other value is designated. Also this value can be specified by

the parameter No. 5132, and the parameter is changed by the program command. e : Escaping amount This designation is modal and is not changed until the other value is designated. Also

this value can be specified by the parameter No. 5133, and the parameter is changed

by the program command. ns : Sequence number of the first block for the program of finishing shape. nf : Sequence number of the last block for the program of finishing shape. Δu : Distance of the finishing allowance in the direction of the second axis on the plane

(X-axis for the ZX plane) Δw : Distance of the finishing allowance in the direction of the first axis on the plane (Z-axis

for the ZX plane) f,s,t : Any F , S, or T function contained in blocks ns to nf in the cycle is ignored, and the F,

S, or T function in this G71 block is effective.

Unit Diameter/radius programming Sign

Depends on the increment

Δd

system for the reference axis.

Radius programming

Not

required

Decimal point

input

Allowed

- 39 -

4. FUNCTIONS TO SIMPLIFY

A’Δ

PROGRAMMING

PROGRAMMING B-64484EN-1/03

Unit Diameter/radius programming Sign

Depends on the increment

system for the reference axis. Depends on the increment

Δu

system for the reference axis. Depends on the increment

Δw

system for the reference axis.

Radius programming Depends on diameter/radius programming

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

Not

required

Required Allowed

Decimal point

(F)

Target figure

45°

(R)

(F)

u/2

input

Allowed

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

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

e: Escaping amount

Explanation

- Operations

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

NOTE

1 While both Δd and Δu are specified by the same address, the meanings of them

are determined by the presence of addresses P and Q. 2 The cycle machining is performed by G71 command with P and Q specification. 3 F, S, and T functions which are specified in the move command between points

A and B are ineffective and those specified in G71 block or the previous block

are effective. M and second auxiliary functions are treated in the same way as F,

S, and T functions. 4 When an option of constant surface speed control is selected, G96 or G97

command specified in the move command between points A and B are

ineffective, and that specified in G71 block or the previous block is effective.

- Target figure Patterns

The following four cutting patterns are considered. All of these cutting cycles cut the workpiece with moving the tool in parallel to the first axis on the plane (Z-axis for the ZX plane). At this time, the signs of the finishing allowances of Δu and Δw are as follows:

- 40 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

Both linear and circular interpolation are possible

B +X

U(+)…W(+)

U(-)…W(+)

Fig. 4.2.1 (b) Four target figure patterns

' '

U(+)… W(-)

' '

U(-)…W(-)

Limitation

(1) For U(+), a figure for which a position higher than the cycle start point is specified cannot be

machined.

For U(-), a figure for which a position lower than the cycle start point is specified cannot be

machined.

(2) For type I, the figure must show monotone increase or decrease along the first and second axes on

the plane.

(3) For type II, the figure must show monotone increase or decrease along the first axis on the plane.

- Start block

In the start block in the program for a target figure (block with sequence number ns in which the path between A and A' is specified), G00 or G01 must be specified. If it is not specified, alarm PS0065, “G00/G01 IS NOT IN THE FIRST BLOCK OF SHAPE PROGRAM” is issued. When G00 is specified, positioning is performed along A-A'. When G01 is specified, linear interpolation is performed with cutting feed along A-A'. In this start block, also select type I or II.

- Check functions

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

NOTE

When tool nose radius compensation is applied, the target figure to which

compensation is applied is checked.

The following checks can also be made.

Check Related parameter

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

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

- 41 -

4. FUNCTIONS TO SIMPLIFY

A A

PROGRAMMING

PROGRAMMING B-64484EN-1/03

- Types I and II Selection of type I or II

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

NOTE

To use type II, the multiple repetitive canned cycle II option is required.

Selecting type I or II

In the start block for the target figure (sequence number ns), select type I or II. (1) When type I is selected Specify the second axis on the plane (X-axis for the ZX plane). Do not specify the first axis on the

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

the ZX plane). When you want to use type II without moving the tool along the first axis on the plane (Z-axis for

the ZX plane), specify the incremental programming with travel distance 0 (W0 for the ZX plane).

- Type I

(1) In the block with sequence number ns, only the second axis on the plane (X-axis (U-axis) for the ZX

plane) must be specified.

Example

ZX plane G71 V10.0 R5.0 ;

G71 P100 Q200....;

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

(2) The figure along path A'-B must show monotone increase or decrease in the directions of both axes

forming the plane (Z- and X-axes for the ZX plane). It must not have any pocket as shown in the Fig.

4.2.1 (c).

’

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

No pockets are allowed.

- 42 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

CAUTION

If a figure does not show monotone change along the first or second axis on the

plane, alarm PS0064, “THE FINISHING SHAPE IS NOT A MONOTONOUS CHANGE(FIRST AXES)” or PS0329, “THE FINISHING SHAPE IS NOT A MONOTONOUS CHANGE(SECOND AXES)” is issued. If the movement does not show monotone change, but is very small, and it can be determined that the movement is not dangerous, however, the permissible amount can be specified in parameters Nos. 5145 and 5146 to specify that the alarm is not issued in this case.

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

45°

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

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

(4) Immediately after the last cutting, rough cutting is performed as finishing along the target figure. Bit

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

- Type II

(F)

(R)

(F)

(R)

(F)

Target figure

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

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

’

u/2

When a target figure passing through A, A', and B in this order is given by the program for a target figure as shown in the Fig. 4.2.1 (e), the specified area is removed by Δd (depth of cut), with the finishing allowance specified by Δu/2 and Δw left. Type II differs from type I in cutting the workpiece along the figure after rough cutting in the direction of the first axis on the plane (Z-axis for the ZX plane). After the last cutting, the tool returns to the start point specified in G71 and rough cutting is performed as finishing along the target figure, with the finishing allowance specified by Δu/2 and Δw left.

Type II differs from type I in the following points:

- 43 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

(1) In the block with sequence number ns, the two axes forming the plane (X-axis (U-axis) and Z-axis

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

Example

ZX plane G71 V10.0 R5.0;

G71 P100 Q200.......;

N100 X(U)_ Z(W)_ ;

(Specifies the two axes forming the plane.) : ; : ; N200…………;

(2) The figure need not show monotone increase or decrease in the direction of the second axis on the

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

. . .

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

The figure must show monotone change in the direction of the first axis on the plane (Z-axis for the

ZX plane), however. The Fig. 4.2.1 (g) cannot be machined.

Monotone change is not observed along the Z-

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

axis.

CAUTION

For a figure along which the tool moves backward along the first axis on the

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

The first cut portion need not be vertical. Any figure is permitted if monotone change is shown in

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

- 44 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

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

(3) After turning, the tool cuts the workpiece along its figure and escapes in cutting feed.

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

Escaping after cutting

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

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

The escaping amount after cutting (e) can be specified at address R or set in parameter No. 5133. When moving from the bottom, however, the tool escapes to the direction of 45 degrees.

45°

e (specified in the command or

parameter No. 5133)

Bottom

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

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

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

(5) After all rough cutting terminates along the first axis on the plane (Z-axis for the ZX plane), the tool

temporarily returns to the cycle start point. At this time, when there is a position whose height equals to that at the start point, the tool passes through the point in the position obtained by adding depth of cut Δd to the position of the figure and returns to the start point.

Then, rough cutting is performed as finishing along the target figure. At this time, the tool passes

through the point in the obtained position (to which depth of cut Δd is added) when returning to the start point.

Bit 2 (RF2) of parameter No. 5105 can be set to 1 so that rough cutting as finishing is not performed.

- 45 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

Escaping operation after rough cutting as finishing

{

Fig. 4.2.1 (k) Escaping operation when the too l returns to the start point (type II)

Escaping operation after rough cutting

Start point

{

Depth of cut Δd

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

(a) When the figure shows monotone decrease along the first axis on the plane (Z-axis for the ZX

plane)

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

<3>

<2>

<1>

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

(b) When the figure shows monotone increase along the first axis on the plane (Z-axis for the ZX

plane)

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

<1>

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

<2>

<3>

The path in rough cutting is as shown Fig. 4.2.1 (n).

- 46 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

15 7

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

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

•

Cutting feed

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

Rapid traverse

Escaping from the bottom

Cuts the workpiece at the cutting feedrate and escapes to the direction of 45 degrees. (Operation 19) Then, moves to the height of point D in rapid traverse. (Operation 20) Then, moves to the position the amount of g before point D. (Operation 21) Finally, moves to point D in cutting feed. The clearance g to the cutting feed start position is set in parameter No. 5134. For the last pocket, after cutting the bottom, the tool escapes to the direction of 45 degrees and returns to the start point in rapid traverse. (Operations 34 and 35)

CAUTION

1 This CNC differs from the FANUC Series 16i/18i/21i in cutting of a pocket. The tool first cuts the nearest pocket to the start point. After cutting of the pocket

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

2 When the figure has a pocket, generally specify a value of 0 for Δw (finishing

allowance). Otherwise, the tool may dig into the wall on one side.

3 This CNC differs from the FANUC Series 16i/18i/21i in the path of cutting after

turning depending on the figure of the workpiece. When the tool becomes moving only along the first axis on the plane (Z-axis for the ZX plane) according to the figure of the workpiece during cutting, it starts retraction along the second axis on the plane (X-axis for the ZX plane).

- Tool nose radius compensation

- 47 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING B-64484EN-1/03

If tool nose radius compensation is specified in the program specifying a target finishing figure, alarm PS0325, “UNAVAILABLE COMMAND IS IN SHAPE PROGRAM”, is issued.

Program example

G42;..............................Specify this command before a multiple repetitive canned cycle command.

G71U1.0R0.5; G71P10Q20; N10G00X0; : N20X50.;

G40;..............................Specify this command after the program specifying a target finishing figure.

When this cycle is specified in the tool nose radius compensation mode, offset is temporarily canceled during movement to the start point. Start-up is performed in the first block. Offset is temporarily canceled again at the return to the cycle start point after termination of cycle operation. Start-up is performed again according to the next move command. This operation is shown in the Fig. 4.2.1 (p).

Start-up

Offset cancel

Cycle start point

Offset cancel

Start-up

Fig. 4.2.1 (p)

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

Position between A-

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

' in which start-up is

performed

Fig. 4.2.1 (q) Path when tool nose radi u s co mp en sation is applied

Tool nose center path when too l nose radius compensation is applied with G42

’

- 48 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

’

Position between

Target figure program for which tool nose radius

compensation is not applied

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

-A' in which start-

up is performed

PROGRAMMING

NOTE

To perform pocketing in the tool nose radius compensation mode, specify the

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

- Reducing the cycle time

In G71 and G72, the tool can be moved to the previous turning start point (operation 1) in rapid traverse by setting bit 0 (ASU) of parameter No. 5107 to 1. Bit 0 (ASU) of parameter No. 5107 is valid for both type I and II commands.

For the type I command

Operation 1

Operation 2

: The mode specified in the start block is followed.

Rapid traverse can be selected.

Previous turning point

Current turning point

For the type I G71 and G72 commands, operations 1 and 2 to the current turning start point that are usually performed in 2 cycles can be performed in 1 cycle by setting bit 1 (ASC) of parameter No. 5107 to 1. The feed mode specified in the start block in the program for a target figure (G00 or G01) is used. Bit 1 (ASC) of parameter No. 5107 is valid only for the type I command.

- 49 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

For the type II command

Operation 1

Operation 2

Previous turning point

Current turning point

- 50 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

4.2.2 Stock Removal in Facing (G72)

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

Format

ZpXp plane

G72 W(Δd) R(e) ; G72 P(ns) Q(nf) U(Δu) W(Δw) F(f ) S(s ) T(t ) ;

N (ns) ; ... N (nf) ;

YpZp plane

G72 V(Δd) R(e) ; G72 P(ns) Q(nf) V(Δw) W(Δu) F(f ) S(s ) T(t ) ; N (ns) ;

The move commands for the target figure from A to A’ to B are specified in the blocks with sequence numbers ns to nf.

... N (nf) ;

XpYp plane

G72 U(Δd) R(e) ; G72 P(ns) Q(nf) U(Δw) W(Δu) F(f ) S(s ) T(t ) ; N (ns) ; ... N (nf) ;

Δd : Depth of cut The cutting direction depends on the direction AA'. This designation is modal and is not

changed until the other value is designated. Also this value can be specified by the

parameter No. 5132, and the parameter is changed by the program command. e : Escaping amount This designation is modal and is not changed until the other value is designated. Also

this value can be specified by the parameter No. 5133, and the parameter is changed

(X-axis for the ZX plane) Δw : Distance of the finishing allowance in the direction of the first axis on the plane (Z-axis

for the ZX plane) f,s,t : Any F , S, or T function contained in blocks ns to nf in the cycle is ignored, and the F, S,

or T function in this G72 block is effective.

Unit Diameter/radius programming Sign

Depends on the increment

Δd

system for the reference axis. Depends on the increment

system for the reference axis.

Radius programming

Not

required

Not

required

Decimal point

input

Allowed

- 51 -

4. FUNCTIONS TO SIMPLIFY

A'Δ

PROGRAMMING

PROGRAMMING B-64484EN-1/03

Unit Diameter/radius programming Sign

Depends on the increment

Δu

system for the reference axis. Depends on the increment

Δw

system for the reference axis.

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

Required Allowed

Decimal point

input

(F)

(R)

Target figure

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

(F)

Δw

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

Tool path

(R)

45°

u/2

Explanation

- Operations

NOTE

1 While both Δd and Δu are specified by the same address, the meanings of them

are determined by the presence of addresses P and Q. 2 The cycle machining is performed by G72 command with P and Q specification. 3 F, S, and T functions which are specified in the move command between points

A and B are ineffective and those specified in G72 block or the previous block

are effective. M and second auxiliary functions are treated in the same way as F,

S, and T functions. 4 When an option of constant surface speed control is selected, G96 or G97

command specified in the move command between points A and B are

ineffective, and that specified in G72 block or the previous block is effective.

- Target figure Patterns

The following four cutting patterns are considered. All of these cutting cycles cut the workpiece with moving the tool in parallel to the second axis on the plane (X-axis for the ZX plane). At this time, the signs of the finishing allowances of Δu and Δw are as follows:

- 52 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

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

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

PROGRAMMING

' '

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

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

' '

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

Both linear and circular interpolation are possible

Limitation

(1) For W(+), a figure for which a position higher than the cycle start point is specified cannot be

machined.

For W(-), a figure for which a position lower than the cycle start point is specified cannot be

machined.

(2) For type I, the figure must show monotone increase or decrease along the first and second axes on

the plane.

(3) For type II, the figure must show monotone increase or decrease along the second axis on the plane.

- Start block

In the start block in the program for a target figure (block with sequence number ns in which the path between A and A' is specified), G00 or G01 must be specified. If it is not specified, alarm PS0065, “G00/G01 IS NOT IN THE FIRST BLOCK OF SHAPE PROGRAM” is issued. When G00 is specified, positioning is performed along A-A’. When G01 is specified, linear interpolation is performed with cutting feed along A-A’. In this start block, also select type I or II.

- Check functions

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

NOTE

When tool nose radius compensation is applied, the target figure to which

compensation is applied is checked.

The following checks can also be made.

Check Related parameter

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

- Types I and II Selection of type I or II

For G72, there are types I and II. When the target figure has pockets, be sure to use type II.

- 53 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

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

Selecting type I or II

In the start block for the target figure (sequence number ns), select type I or II. (1) When type I is selected Specify the first axis on the plane (Z-axis for the ZX plane). Do not specify the second axis on the

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

the ZX plane). When you want to use type II without moving the tool along the second axis on the plane (X-axis for

the ZX plane), specify the incremental programming with travel distance 0 (U0 for the ZX plane).

- Type I

G72 differs from G71 in the following points: (1) G72 cuts the workpiece with moving the tool in parallel with the second axis on the plane (X-axis on

the ZX plane). (2) In the start block in the program for a target figure (block with sequence number ns), only the first

axis on the plane (Z-axis (W-axis) for the ZX plane) must be specified.

- Type II

G72 differs from G71 in the following points: (1) G72 cuts the workpiece with moving the tool in parallel with the second axis on the plane (X-axis on

the ZX plane). (2) The figure need not show monotone increase or decrease in the direction of the first axis on the

plane (Z-axis for the ZX plane) and it may have concaves (pockets). The figure must show

monotone change in the direction of the second axis on the plane (X-axis for the ZX plane),

however. (3) When a position parallel to the second axis on the plane (X-axis for the ZX plane) is specified in a

block in the program for the target figure, it is assumed to be at the bottom of a pocket. (4) After all rough cutting terminates along the second axis on the plane (X-axis for the ZX plane), the

tool temporarily returns to the start point. Then, rough cutting as finishing is performed.

- Tool nose radius compensation

See the pages on which G71 is explained.

- Reducing the cycle time

See the pages on which G71 is explained.

- 54 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

4.2.3 Pattern Repeating (G73)

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

Format

ZpXp plane

G73 W(Δk) U(Δi) R(d) ; G73 P(ns) Q(nf) U(Δu) W(Δw) F(f ) S(s ) T(t ) ;

N (ns) ;

...

N (nf) ;

YpZp plane

G73 V(Δk) W(Δi) R(d) ; G73 P(ns) Q(nf) V(Δw) W(Δu) F(f ) S(s ) T(t ) ; N (ns) ; ... N (nf) ;

XpYp plane

G73 U(Δk) V(Δi) R(d) ; G73 P(ns) Q(nf) U(Δw) V(Δu) F(f ) S(s ) T(t ) ; N (ns) ; ... N (nf) ;

Δi : Distance of escape in the direction of the second axis on the plane (X-axis for the ZX

plane)

This designation is modal and is not changed until the other value is designated. Also

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

Δk : Distance of escape in the direction of the first axis on the plane (Z-axis for the ZX

plane)

This designation is modal and is not changed until the other value is designated. Also

this value can be specified by the parameter No. 5136, and the parameter is changed

by the program command. d : The number of division This value is the same as the repetitive count for rough cutting. This designation is

modal and is not changed until the other value is designated. Also, this value can be

specified by the parameter No. 5137, and the parameter is changed by the program

command. ns : Sequence number of the first block for the program of finishing shape. nf : Sequence number of the last block for the program of finishing shape. Δu : Distance of the finishing allowance in the direction of the second axis on the plane

(X-axis for the ZX plane) Δw : Distance of the finishing allowance in the direction of the first axis on the plane (Z-axis

for the ZX plane) f, s, t : Any F, S, and T function contained in the blocks between sequence number "ns" and

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

The move commands for the target figure from A to A’ to B are specified in the blocks with sequence numbers ns to nf.

- 55 -

4. FUNCTIONS TO SIMPLIFY

Δi+Δ

Δk+Δ

PROGRAMMING

PROGRAMMING B-64484EN-1/03

Unit Diameter/radius programming Sign

Depends on the increment

Δi

system for the reference axis. Depends on the increment

Δk

system for the reference axis. Depends on the increment

Δu

system for the reference axis. Depends on the increment

Δw

system for the reference axis.

Radius programming Required Allowed

Radius programming Required Allowed Depends on diameter/radius programming for

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

Required Allowed

Decimal point

input

NOTE

Decimal point input is allowed with d. However, a value rounded off to an integer

is used as the number of division, regardless of the setting of bit 0 (DPI) of parameter No. 3401. When an integer is input, the input integer is used as the number of division.

Δw

(R)

(F)

u/2

Δu/2

(R)

Δu/2

' Δw

Target figure

Fig. 4.2.3 (t) Cutting path in pattern repeating

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

Explanation

- Operations

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

NOTE

1 While the values Δi and Δk, or Δu and Δw are specified by the same address

respectively, the meanings of them are determined by the presence of

addresses P and Q. 2 The cycle machining is performed by G73 command with P and Q specification. 3 After cycle operation terminates, the tool returns to point A. 4 F, S, and T functions which are specified in the move command between points

A and B are ineffective and those specified in G73 block or the previous block

are effective. M and second auxiliary functions are treated in the same way as F,

S, and T functions.

- 56 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

- Target figure Patterns

As in the case of G71, there are four target figure patterns. Be careful about signs of Δu, Δw, Δi, and Δk when programming this cycle.

- Start block

In the start block in the program for the target figure (block with sequence number ns in which the path between A and A' is specified), G00 or G01 must be specified. If it is not specified, alarm PS0065, “G00/G01 IS NOT IN THE FIRST BLOCK OF SHAPE PROGRAM” is issued. When G00 is specified, positioning is performed along A-A’. When G01 is specified, linear interpolation is performed with cutting feed along A-A’.

- Check function

The following check can be made.

Check Related parameter

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

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

- Tool nose radius compensation

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

- 57 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

4.2.4 Finishing Cycle (G70)

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

Format

G70 P(ns) Q(nf) ;

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

Explanation

- Operations

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

- Target figure Check function

The following check can be made.

Check Related parameter

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

- Storing P and Q blocks

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

Example

G71 P100 Q200 ...; N100 ...; ...; ...; N200 ...; G71 P300 Q400 ...; N300 ...; ...; ...; N400 ...; ...; ...; G70 P100 Q200 ; (Executed without a search for the first to third cycles) G70 P300 Q400 ; (Executed after a search for the fourth and subsequent

cycles)

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

- 58 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

NOTE

The memory addresses of P and Q blocks stored during rough cutting cycles by

G71, G72, and G73 are erased after execution of G70.

All stored memory addresses of P and Q blocks are also erased by a reset.

- Return to the cycle start point

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

NOTE

The tool returns to the cycle start point always in the nonlinear positioning mode

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

Before executing a finishing cycle for a target figure with a pocket cut by G71 or

G72, check that the tool does not interfere with the workpiece when returning from the end point of the target figure to the cycle start point.

- Tool nose radius compensation

When using tool nose radius compensation, specify a tool nose radius compensation command (G41 or G42) before a multiple repetitive canned cycle command (G70) and specify the cancel command (G40) after the multiple repetitive canned cycle command (G70).

Program example

G42;..............................Specify this command before a multiple repetitive canned cycle command.

G70P10Q20;

G40;..............................Specify this command after a multiple repetitive canned cycle command.

- 59 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

Example

Stock removal in facing (G72)

20 2

Start point

Z axis

X axis

160

120

2010

190

(Diameter designation for X axis, metric input)

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

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

- 60 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

Pattern repeating (G73)

X axis

PROGRAMMING

180

160

120

220

(Diameter designation, metric input)

N010 G50 X260.0 Z220.0 ; N011 G00 X220.0 Z160.0 ; N012 G73 U14.0 W14.0 R3 ; N013 G73 P014 Q019 U4.0 W2.0 F0.3 S0180 ; N014 G00 X80.0 W-40.0 ; N015 G01 W-20.0 F0.15 S0600 ; N016 X 120.0 W-10.0; N017 W-20.0 S0400 ; N018 G02 X160.0 W-20.0 R20.0 ; N019 G01 X180.0 W-10.0 S0280 ; N020 G70 P014 Q019 ;

110

130

Z axis

- 61 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

4.2.5 End Face Peck Drilling Cycle (G74)

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

Format

G74R (e) ; G74X(U)_ Z(W)_ P(Δi) Q(Δk) R(Δd) F (f ) ;

e : Return amount This designation is modal and is not changed until the other value is designated.

Also this value can be specified by the parameter No. 5139, and the parameter is

changed by the program command. X_,Z_ : Coordinate of the second axis on the plane (X-axis for the ZX plane) at point B and Coordinate of the first axis on the plane (Z-axis for the ZX plane) at point C U_,W_ : Travel distance along the second axis on the plane (U for the ZX plane) from point A

to B Travel distance along the first axis on the plane (W for the ZX plane) from point A to

C (When G code system A is used. In other cases, X_,Z_ is used for specification.) Δi : Travel distance in the direction of the second axis on the plane (X-axis for the ZX

plane)

Δk : Depth of cut in the direction of the first axis on the plane (Z-axis for the ZX plane) Δd : Relief amount of the tool at the cutting bottom

f : Feedrate

Unit

Depends on the increment system for

the reference axis. Depends on the increment system for

Δi

the reference axis. Depends on the increment system for

Δk

the reference axis. Depends on the increment system for

Δd

the reference axis.

Diameter/radius

programming

Radius programming Not required Allowed

Radius programming Not required Not allowed

Radius programming NOTE Allowed

Sign

NOTE

Normally, specify a positive value for Δd. When X (U) and Δi are omitted, specify

a value with the sign indicating the direction in which the tool is to escape.

Decimal point

input

- 62 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

Δk' Δk

(R)

(F)

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

(F)

(R)

Δk

(F)

(R)

Δk

(F)

Δk

(F)

(R)

[0 < Δk’ ≤ Δk]

Δi

(R)

U/2

Δi

Δi’

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

[0 < Δi’ ≤ Δi]

Explanation

- Operations

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

NOTE

1 While both e and Δd are specified by the same address, the meanings of them

are determined by specifying the X, Y, or Z axis. When the axis is specified, Δd is used.

2 The cycle machining is performed by G74 command with specifying the axis.

- Tool nose radius compensation

Tool nose radius compensation cannot be applied.

- 63 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

4.2.6 Outer Diameter / Internal Diameter Drilling Cycle (G75)

This cycle is equivalent to G74 except that the second axis on the plane (X-axis for the ZX plane) changes places with the first axis on the plane (Z-axis for the ZX plane). This cycle enables chip breaking in end facing. It also enables grooving during outer diameter cutting and cutting off (when the Z-axis (W-axis) and Q are omitted for the first axis on the plane).

Format

G75R (e) ; G75X(U)_ Z(W)_ P(Δi) Q(Δk) R(Δd) F (f ) ;

e : Return amount This designation is modal and is not changed until the other value is designated.

Also this value can be specified by the parameter No. 5139, and the parameter is

changed by the program command. X_, Z_ : Coordinate of the second axis on the plane (X-axis for the ZX plane) at point B and Coordinate of the first axis on the plane (Z-axis for the ZX plane) at point C U_, W_ : Travel distance along the second axis on the plane (U for the ZX plane) from point

A to B Travel distance along the first axis on the plane (W for the ZX plane) from point A

to C (When G code system A is used. In other cases, X_,Z_ is used for specification.) Δi : Depth of cut in the direction of the second axis on the plane (X-axis for the ZX

plane) Δk : Travel distance in the direction of the first axis on the plane (Z-axis for the ZX

plane) Δd : Relief amount of the tool at the cutting bottom f : Feedrate

Unit Diameter/radius programming Sign

Depends on the increment system for

the reference axis. Depends on the increment system for

Δi

the reference axis. Depends on the increment system for

Δk

the reference axis. Depends on the increment system for

Δd

the reference axis.

Radius programming Not required Allowed

Radius programming Not required Not allowed

Radius programming NOTE Allowed

NOTE

Normally, specify a positive value for Δd. When Z (W) and Δk are omitted,

specify a value with the sign indicating the direction in which the tool is to escape.

Decimal point

input

- 64 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

(R)

(F)

Δi

U/2

Δi

Δi’

Δd

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

Fig. 4.2.6 (b) Outer diameter/internal diameter drilling cycle

Explanation

- Operations

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

Both G74 and G75 are used for grooving and drilling, and permit the tool to relief automatically. Four symmetrical patterns are considered, respectively.

- Tool nose radius compensation

Tool nose radius compensation cannot be applied.

- 65 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

4.2.7 Multiple Threading Cycle (G76)

This threading cycle performs one edge cutting by the constant amount of cut.

Format

G76 P(m) (r) (a) Q(Δdmin) R(d ) ; G76 X(U)_ Z(W)_ R(i ) P(k ) Q(Δd) F (L ) ;

m : Repetitive count in finishing (1 to 99) This value can be specified by the parameter No. 5142, and the parameter is changed by

the program command. r : Chamfering amount (0 to 99) When the thread lead is expressed by L, the value of L can be set from 0.0L to 9.9L in

0.1L increment (2-digit number). This value can be specified by the parameter No. 5130,

and the parameter is changed by the program command. a : Angle of tool nose One of six kinds of angle, 80°, 60°, 55°, 30°, 29°, and 0°, can be selected, and specified

by 2-digit number. This value can be specified by the parameter No. 5143, and the

parameter is changed by the program command.

m, r, and a are specified by address P at the same time.

(Example) When m=2, r=1.2L, a=60°, specify as shown below (L is lead of thread).

P 02 12 60

Δdmin : Minimum cutting depth When the cutting depth of one cycle operation becomes smaller than this limit, the

cutting depth is clamped at this value. This value can be specified by parameter

No. 5140, and the parameter is changed by the program command. d : Finishing allowance This value can be specified by parameter No. 5141, and the parameter is changed

by the program command. X_, Z_ : Coordinates of the cutting end point (point D in the Fig. 4.2.7 (a)) in the direction of

the length U_, W_ : Travel distance to the cutting end point (point D in the Fig. 4.2.7 (a)) in the direction

of the length (When G code system A is used. In other cases, X_,Z_ is used for specification.) i : Taper amount If i = 0, ordinary straight threading can be made. k : Height of thread Δd : Depth of cut in 1st cut L : Lead of thread

Unit

Δdmin

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

the reference axis. Depends on the increment system for

the reference axis.

Diameter/radius

programming

Radius programming Not required Not allowed

Radius programming Not required Allowed

Radius programming Required Allowed

Radius programming Not required Not allowed

Sign

Decimal point

input

- 66 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

Unit

Depends on the increment system for

Δd

the reference axis.

U/2

(R)

Fig. 4.2.7 (a) Cutting path in multiple threading cycle

Diameter/radius

programming

Sign

Decimal point

input

Radius programming Not required Not allowed

(R) A

(R)

(F)

Δd

Tool nose

Δd√n

1st

2nd

3rd

nth

Fig. 4.2.7 (b) Detail of cutting

- Repetitive count in finishing

The last finishing cycle (cycle in which the finishing allowance is removed by cutting) is repeated.

- 67 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

Last finishi ng cy c l e

d (finishing allowance)

Explanation

- Operations

This cycle performs threading so that the length of the lead only between C and D is made as specified in the F code. In other sections, the tool moves in rapid traverse. The time constant for acceleration/deceleration after interpolation and FL feedrate for thread chamfering and the feedrate for retraction after chamfering are the same as for thread chamfering with G92 (canned cycle).

NOTE

1 The meanings of the data specified by address P, Q, and R determined by the

presence of X (U) and Z (W).

2 The cycle machining is performed by G76 command with X (U) and Z (W)

specification.

3 The values specified at addresses P, Q, and R are modal and are not changed

until another value is specified.

4 Specify a value smaller than the height of thread as the finishing allowance. (d <

CAUTION

Notes on threading are the same as those on G32 threading. For feed hold in a

threading cycle, however, see "Feed hold in a threading cycle" described below.

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

The signs of incremental dimensions for the cycle shown in Fig. 4.2.7 (a) are as follows: Cutting end point in the direction of the length for U and W: Minus (determined according to the directions of paths A-C and C-D) Taper amount (i): Minus (determined according to the direction of path A-C) Height of thread (k): Plus (always specified with a plus sign) Depth of cut in the first cut (Δd): Plus (always specified with a plus sign) The four patterns shown in the Table 4.2.7 (a) are considered corresponding to the sign of each address. A female thread can also be machined.

- 68 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

Table 4.2.7 (a)

Outer diameter machining Internal diameter machining

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

PROGRAMMING

U/2

3(R)

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

3(R)

4(R)

2(F)

at |i|≤|U/2|

4(R)

2(F)

1(R)

U/2 3(R)

4. U > 0, W < 0, i < 0 at |i|≤|U/2|

U/2

3(R)

2(F)

4(R)

2(F)

4(R)

1(R)

- Acceleration/deceleration after interpolation for threading

- Time constant and FL feedrate for threading

- Thread chamfering

Thread chamfering can be performed in this threading cycle. A signal from the machine tool initiates thread chamfering. The maximum amount of thread chamfering (r) that can be specified in the command is 99 (9.9L). The amount can be specified in a range from 0.1L to 12.7L in 0.1L increments in parameter No. 5130. A thread chamfering angle between 1 to 89 degrees can be specified in parameter No. 5131. When a value of 0 is specified in the parameter, an angle of 45 degrees is assumed. For thread chamfering, the same type of acceleration/deceleration after interpolation, time constant for acceleration/deceleration after interpolation, and FL feedrate as for threading are used.

NOTE

Common parameters for specifying the amount and angle of thread chamfering

are used for this cycle and G92 threading cycle.

- 69 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

- Retraction after chamfering

The Table 4.2.7 (b) lists the feedrate, type of acceleration/deceleration after interpolation, and time constant of retraction after chamfering.

Table 4.2.7 (b)

Bit 0 (CFR) of

parameter No.

1611

0 Other than 0

0 0

Parameter No.

1466

Description

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

NOTE

During retraction, the machine does not stop with an override of 0% for the

cutting feedrate regardless of the setting of bit 4 (RF0) of parameter No. 1401.

- Shifting the start angle

The threading start angle cannot be shifted.

- Feed hold in a threading cycle

When the threading cycle retract function is not used, the machine stops at the end point of retraction after chamfering (point E on the cutting path for a multiple threading cycle) by feed hold applied during threading.

- Feed hold when the threading cycle retract function is used

When the "threading cycle retract" optional function is used, feed hold may be applied during threading in a combined threading cycle (G76). In this case, the tool quickly retracts in the same way as for the last chamfering in a threading cycle and returns to the start point in the current cycle. When cycle start is triggered, the multiple threading cycle resumes.

X-axis

Z-axis

Ordinary cycle Motion at feed hold

Start point in the current cycle

Rapid traverse

Cu ttin g fe ed

Feed hold is applied at this point

The angle of chamfering during retraction is the same as that of chamfering at the end point.

- 70 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

CAUTION

Another feed hold cannot be performed during retraction.

- Inch threading

Inch threading specified with address E is not allowed.

- Tool nose radius compensation

Tool nose radius compensation cannot be applied.

Example

1.8

3.68

X axis

1.8

G80 X80.0 Z130.0; G76 P011060 Q100 R200 ; G76 X60.64 Z25.0 P3 680 Q1800 F6.0 ;

60.64

105

Z axis

4.2.8 Restrictions on Multiple Repetitive Canned Cycle (G70-G76)

Programmed commands

- Program memory

Programs using G70, G71, G72, or G73 must be stored in the program memory. The use of the mode in which programs stored in the program memory are called for operation enables these programs to be executed in other than the MEM mode. Programs using G74, G75, or G76 need not be stored in the program memory.

- Blocks in which data related to a multiple repetitive canned cycle is specified

The addresses P, Q, X, Z, U, W, and R should be specified correctly for each block.

In a block in which G70, G71, G72, or G73 is specified, the following functions cannot be specified:

• Custom macro calls (simple call, modal call, and subprogram call)

- 71 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

- Blocks in which data related to a target figure is specified

In the block which is specified by address P of a G71, G72 or G73, G00 or G01 code in group 01 should be commanded. If it is not commanded, alarm PS0065, “G00/G01 IS NOT IN THE FIRST BLOCK OF SHAPE PROGRAM” is generated.

In blocks with sequence numbers between those specified at P and Q in G70, G71, G72, and G73, the following commands can be specified: (1) Dwell (G04) (2) G00, G01, G02, and G03 When a circular interpolation command (G02, G03) is used, there must be no radius difference between the start point and end point of the arc. If there is a radius difference, the target finishing figure may not be recognized correctly, resulting in a cutting error such as excessive cutting. (3) Custom macro branch and repeat command The branch destination must be between the sequence numbers specified at P and Q, however. High-speed branch specified by bits 1 and 4 of parameter No. 6000 is invalid. No custom macro call (simple, modal, or subprogram call) cannot be specified. (4) Direct drawing dimension programming command and chamfering and corner R command Direct drawing dimension programming and chamfering and corner R require multiple blocks to be

specified. The block with the last sequence number specified at Q must not be an intermediate block

of these specified blocks.

When G70, G71, G72, or G73 is executed, the sequence number specified by address P and Q should not be specified twice or more in the same program.

When #1 = 2500 is executed using a custom macro, 2500.000 is assigned to #1. In such a case, P#1 is equivalent to P2500.

Relation with other functions

- Manual intervention

After manual intervention is performed with the manual absolute on command before the execution of a multiple repetitive canned cycles (G70 to G76) or after the stop of the execution, when a cycle operation starts, the manual intervention amount is canceled even with an incremental cycle start command. When only the first plane axis is specified in G74 or only the second plane axis is specified in G74, however, the manual intervention amount is canceled only along the specified axis.

- Interruption type macro

Any interruption type macro program cannot be executed during execution of a multiple repetitive canned cycle.

- Program restart and tool retract and recover

These functions cannot be executed in a block in a multiple repetitive canned cycle.

Example of G72

Cancellation

Manual intervention

- 72 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

- Axis name and second auxiliary functions

Even if address U, V, or W is used as an axis name or second auxiliary function, data specified at address U, V, or W in a G71 to G73 block is assumed to be that for the multiple repetitive canned cycle.

- Tool nose radius compensation

When using tool nose radius compensation, specify a tool nose radius compensation command (G41, G42) before a multiple repetitive canned cycle command (G70, G71, G72, G73) and specify the cancel command (G40) outside the programs (from the block specified with P to the block specified with Q) specifying a target finishing figure. If tool nose radius compensation is specified in the program specifying a target finishing figure, alarm PS0325, “UNAVAILABLE COMMAND IS IN SHAPE PROGRAM”, is issued.

- Multi-spindle control

When a spindle selection by address P of multi-spindle control is used, S code cannot be specified at the block of multiple repetitive canned cycle command (G71-G73). (The alarm PS5305 “ILLEGAL SPINDLE NUMBER” is issued.) In this case, instead of specifying S code at the block of multiple repetitive canned cycle command (G71-G73) is specified, specify S code before the multiple repetitive canned cycle command (G71-G73) block.

- 73 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

4.3 CANNED CYCLE FOR DRILLING

Canned cycles for drilling make it easier for the programmer to create programs. With a canned cycle, a frequently-used machining operation can be specified in a single block with a G function; without canned cycles, more than one block is required. In addition, the use of canned cycles can shorten the program to save memory. Table 4.3 (a) lists canned cycles for drilling.

Table 4.3 (a) Canned cycles for drilling

G code Drilling axis

G80 - - - - Cancel G83 Z axis

G84 Z axis Cutting feed G85 Z axis Cutting feed Dwell Cutting feed Front boring cycle G87 X axis

G88 X axis Cutting feed G89 X axis Cutting feed Dwell Cutting feed Side boring cycle

Hole machining

operation

Cutting feed /

intermittent

Cutting feed /

intermittent

Explanation

The canned cycle for drilling consists of the following six operation sequences.

Operation 1 Positioning of X (Z) and C axis Operation 2 Rapid traverse up to point R level Operation 3 Hole machining Operation 4 Operation at the bottom of a hole Operation 5 Retraction to point R level Operation 6 Rapid traverse up to the initial level

Operation in the

bottom hole position

Dwell Rapid traverse Front drilling cycle

Dwell →

spindle CCW

Dwell Rapid traverse Side drilling cycle

Dwell →

Spindle CCW

Retraction operation Applications

Cutting feed Front tapping cycle

Cutting feed Side tapping cycle

Operation 1

Operation 2

Point R level

Operation 3

Operation 4

Fig. 4.3 (a) Operation sequence of canned cycle for drilling

Initial level

Operation 6

Operation 5

Rapid traverse Feed

- Positioning axis and drilling axis

The C-axis and X- or Z-axis are used as positioning axes. The X- or Z-axis, which is not used as a positioning axis, is used as a drilling axis. A drilling G code specifies positioning axes and a drilling axis as shown below.

- 74 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

Although canned cycles include tapping and boring cycles as well as drilling cycles, in this chapter, only the term drilling will be used to refer to operations implemented with canned cycles.

Table 4.3 (b) Positioning axis and drilling axis

G code Positioning axis Drilling axis

G83, G84, G85 X axis, C axis Z axis G87, G88, G89 Z axis, C axis X axis

G83 and G87, G84 and G88, and G85 and G89 have the same function respectively except for axes specified as positioning axes and a drilling axis.

PROGRAMMING

- Drilling mode

G83 to G85/G87 to G89 are modal G codes and remain in effect until canceled. When in effect, the current state is the drilling mode. Once drilling data is specified in the drilling mode, the data is retained until modified or canceled. Specify all necessary drilling data at the beginning of canned cycles; when canned cycles are being performed, specify data modifications only. The feedrate specified at F is retained also after the drilling cycle is canceled. When Q data is required, it must be specified in each block. Once specified, the M code used for C-axis clamp/unclamp functions as a modal code. It is canceled by specifying G80.

- Return point level

In G code system A, the tool returns to the initial level from the bottom of a hole. In G code system B or C, specifying G98 returns the tool to the initial level from the bottom of a hole and specifying G99 returns the tool to the point R level from the bottom of a hole. The following illustrates how the tool moves when G98 or G99 is specified (Fig. 4.3 (b)). Generally, G99 is used for the first drilling operation and G98 is used for the last drilling operation. The initial level does not change even when drilling is performed in the G99 mode.

G98 (Return to initial level) G99 (Return to point R level)

Initial level

Fig. 4.3 (b)

- Number of repeats

To repeat drilling for equally-spaced holes, specify the number of repeats in K_. K is effective only within the block where it is specified. Specify the first hole position in incremental programming. If it is specified in absolute programming, drilling is repeated at the same position.

Number of repeats K The maximum command value = 9999

When K0 is specified, drilling data is just stored without drilling being performed.

Point R level

- 75 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

NOTE

For K, specify an integer of 0 or 1 to 9999.

- M code used for C-axis clamp/unclamp

When an M code specified in parameter No. 5110 for C-axis clamp/unclamp is coded in a program, the following operations occur. (1) The CNC issues the M code for C-axis clamp after the tool is positioned and while the tool is being

fed in rapid traverse to the point-R level.

(2) The CNC issues the M code for C-axis unclamp (the M code for C-axis clamp +1) after the tool

retracts to the point-R level.

(3) After the CNC issues the M code for C-axis unclamp, the tool dwells for the time specified in

parameter No. 5111.

- Cancel

To cancel a canned cycle, use G80 or a group 01 G code.

Group 01 G codes (Example) G00 : Positioning (rapid traverse) G01 : Linear interpolation G02 : Circular interpolation (CW) G03 : Circular interpolation (CCW)

- Symbols in figures

Subsequent subsections explain the individual canned cycles. Figures in these explanations use the following symbols:

Positioning (rapid traverse G00)

Cutting feed (linear interpolation G01) P1 Dwell specified in the program P2 Dwell specified in parameter No.5111

Mα Issuing the M code for C-axis clamp

(The value of α is specified with parameter No. 5110.)

M (α + 1) Issuing the M code for C-axis unclamp

CAUTION

1 In each canned cycle, addresses R, Z, and X are handled as follows:

R_ : Always handled as a radius. Z_ or X_ : Depends on diameter/radius programming.

2 For the B or C G-code system, G90 or G91 can be used to select an incremental

or absolute programming for hole position data (X, C or Z, C), the distance from point R to the bottom of the hole (Z or X), and the distance from the initial level to the point R level (R).

3 For canned cycles for drilling specified in the Series 15 format (by setting bit 1

(FCV) of parameter No. 0001 to 1 and bit 3 (F16) of parameter No. 5102 to 0), incremental programming is used for point R data when bit 6 (RAB) of parameter No. 5102 is set to 0.

When bit 6 (RAB) of parameter No. 5102 is set to 1, in G code system A,

absolute programming is used, and in G code system B or C, absolute or incremental programming is used according to G90 or G91.

For canned cycles for drilling in the Series 16 format, incremental programming

is used for point R data.

- 76 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

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

The peck drilling cycle or high-speed peck drilling cycle is used depending on the setting in RTR, bit 2 of parameter No. 5101. If depth of cut for each drilling is not specified, the normal drilling cycle is used. Without using the RTR parameter, the high-speed peck drilling cycle can be specified with G83.5 or G87.5 and the peck drilling cycle can be specified with G83.6 or G87.6.

- High-speed peck drilling cycle (G83, G87) (bit 2 (RTR) of parameter No. 5101 =0)

This cycle performs high-speed peck drilling. The drill repeats the cycle of drilling at the cutting feedrate and retracting the specified retraction distance intermittently to the bottom of a hole. The drill draws cutting chips out of the hole when it retracts.

Format

G83 X(U)_ C(H)_ Z(W)_ R_ P_ Q_ F_ K_ M_ ;

G87 Z(W)_ C(H)_ X(U)_ R_ P_ Q_ F_ K_ M_ ;

X_ C_ or Z_ C_ : Hole position data Z_ or X_ : The distance from point R to the bottom of the hole R_ : The distance from the initial level to point R level P_ : Dwell time at the bottom of a hole Q_ : Depth of cut for each cutting feed F_ : Cutting feedrate K_ : Number of repeats (When it is needed) M_ : M code for C-axis clamp (When it is needed.)

G83 or G87 (G98 mode) G83 or G87 (G99 mode)

Initial level

Point R

M (α + 1), P2

Point Z

Mα : M code for C-axis clamp M (α + 1) : M code for C-axis unclamp P1 : Dwell specified in the program P2 : Dwell specified in parameter No. 5111 d : Retraction distance specified in parameter No. 5114

Point R

M (α + 1), P2

Point R level

Point Z

- 77 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING B-64484EN-1/03

- Peck drilling cycle (G83, G87) (bit 2 (RTR) of parameter No. 5101 =1)

Format

G83 X(U)_ C(H)_ Z(W)_ R_ P_ Q_ F_ K_ M_ ;

G87 Z(W)_ C(H)_ X(U)_ R_ P_ Q_ F_ K_ M_ ;

X_ C_ or Z_ C_ : Hole position data Z_ or X_ : The distance from point R to the bottom of the hole R_ : The distance from the initial level to point R level P_ : Dwell time at the bottom of a hole Q_ : Depth of cut for each cutting feed F_ : Cutting feedrate K_ : Number of repeats (When it is needed.) M_ : M code for C-axis clamp (When it is needed.)

G83 or G87 (G98 mode) G83 or G87 (G99 mode)

Initial level

M (α + 1), P2

Point Z

M (α + 1), P2

Point R

Point R level

Point Z

Point R

Example

M51 ; Setting C-axis index mode ON M3 S2000 ; Rotating the drill G00 X50.0 C0.0 ; Positioning the drill along the X- and C-axes G83 Z-40.0 R-5.0 Q5000 F5.0 M31 ; Drilling hole 1 C90.0 Q5000 M31 ; Drilling hole 2 C180.0 Q5000 M31 ; Drilling hole 3 C270.0 Q5000 M31 ; Drilling hole 4 G80 M05 ; Canceling the drilling cycle and stopping drill rotation M50 ; Setting C-axis index mode off

NOTE

If the depth of cut for each cutting feed (Q) is not commanded, normal drilling is

performed. (See the description of the drilling cycle.)

- 78 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

- Drilling cycle (G83 or G87)

If depth of cut (Q) is not specified for each drilling, the normal drilling cycle is used. The tool is then

retracted from the bottom of the hole in rapid traverse.

Format

G83 X(U)_ C(H)_ Z(W)_ R_ P_ F_ K_ M_ ;

G87 Z(W)_ C(H)_ X(U)_ R_ P_ F_ K_ M_ ;

X_ C_ or Z_ C_ : Hole position data Z_ or X_ : The distance from point R to the bottom of the hole R_ : The distance from the initial level to point R level P_ : Dwell time at the bottom of a hole F_ : Cutting feedrate K_ : Number of repeats (When it is needed.) M_ : M code for C-axis clamp (When it is needed.)

G83 or G87 (G98 mode) G83 or G87 (G99 mode)

Point R

Initial level

Point R level

M (α + 1), P2

Point Z

Point R

M (α + 1), P2

Mα : M code for C-axis clamp M (α + 1) : M code for C-axis unclamp P1 : Dwell specified in the program P2 : Dwell specified in parameter No. 5111

Example

M51 ; Setting C-axis index mode ON M3 S2000 ; Rotating the drill G00 X50.0 C0.0 ; Positioning the drill along the X- and C-axes G83 Z-40.0 R-5.0 P500 F5.0 M31 ; Drilling hole 1 C90.0 M31 ; Drilling hole 2 C180.0 M31 ; Drilling hole 3 C270.0 M31 ; Drilling hole 4 G80 M05 ; Canceling the drilling cycle and stopping drill rotation M50 ; Setting C-axis index mode off

Point R level

Point Z

- 79 -

4. FUNCTIONS TO SIMPLIFY

PROGRAMMING

PROGRAMMING B-64484EN-1/03

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

This cycle performs tapping. In this tapping cycle, when the bottom of the hole has been reached, the spindle is rotated in the reverse direction.

Format

G84 X(U)_ C(H)_ Z(W)_ R_ P_ F_ K_ M_ ;

G88 Z(W)_ C(H)_ X(U)_ R_ P_ F_ K_ M_ ;

X_ C_ or Z_ C_ : Hole position data Z_ or X_ : The distance from point R to the bottom of the hole R_ : The distance from the initial level to point R level P_ : Dwell time at the bottom of a hole F_ : Cutting feedrate K_ : Number of repeats (When it is needed.) M_ : M code for C-axis clamp (when it is needed.)

G84 or G88 (G98 mode) G84 or G88 (G99 mode)

Point R

Initial level

Spindle CW

M (α + 1), P2

Point Z

Spindle CCW

Point R

Spindle CW

M (α + 1), P2

Point R level

Point Z

Spindle CCW

Mα : M code for C-axis clamp M (α + 1) : M code for C-axis unclamp P1 : Dwell specified in the program P2 : Dwell specified in parameter No. 5111

Explanation

Tapping is performed by rotating the spindle clockwise. When the bottom of the hole has been reached, the spindle is rotated in the reverse direction for retraction. This operation creates threads. Feedrate overrides are ignored during tapping. A feed hold does not stop the machine until the return operation is completed.

NOTE

Bit 3 (M5T) of parameter No. 5105 specifies whether the spindle stop command

(M05) is issued before the direction in which the spindle rotates is specified with M03 or M04. For details, refer to the operator's manual created by the machine tool builder.

Example

M51 ; Setting C-axis index mode ON M3 S2000 ; Rotating the drill

- 80 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

G00 X50.0 C0.0 ; Positioning the drill along the X- and C- axes G84 Z-40.0 R-5.0 P500 F5.0 M31 ; Drilling hole 1 C90.0 M31 ; Drilling hole 2 C180.0 M31 ; Drilling hole 3 C270.0 M31 ; Drilling hole 4 G80 M05 ; Canceling the drilling cycle and stopping drill rotation M50 ; Setting C-axis index mode off

PROGRAMMING

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

This cycle is used to bore a hole.

Format

G85 X(U)_ C(H)_ Z(W)_ R_ P_ F_ K_ M_ ;

G89 Z(W)_ C(H)_ X(U)_ R_ P_ F_ K_ M_ ;

X_ C_ or Z_ C_ : Hole position data Z_ or X_ : The distance from point R to the bottom of the hole R_ : The distance from the initial level to point R level P_ : Dwell time at the bottom of a hole F_ : Cutting feedrate K_ : Number of repeats (When it is needed.) M_ : M code for C-axis clamp (When it is needed.)

G85 or G89 (G98 mode) G85 or G89 (G99 mode)

Point R

Initial level

M (α + 1), P2

Point Z

Point R

Mα : M code for C-axis clamp M (α + 1) : M code for C-axis unclamp P1 : Dwell specified in the program P2 : Dwell specified in parameter No. 5111

Explanation

After positioning, rapid traverse is performed to point R. Drilling is performed from point R to point Z. After the tool reaches point Z, it returns to point R at a feedrate twice the cutting feedrate.

Example

M51 ; Setting C-axis index mode ON M3 S2000 ; Rotating the drill G00 X50.0 C0.0 ; Positioning the drill along the X- and C-axes G85 Z-40.0 R-5.0 P500 F5.0 M31 ; Drilling hole 1 C90.0 M31 ; Drilling hole 2 C180.0 M31 ; Drilling hole 3 C270.0 M31 ; Drilling hole 4

- 81 -

Point R level M (α + 1), P2

Point Z

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

G80 M05 ; Canceling the drilling cycle and stopping drill rotation M50 ; Setting C-axis index mode off

4.3.4 Canned Cycle for Drilling Cancel (G80)

G80 cancels canned cycle for drilling.

Format

G80 ;

Explanation

Canned cycle for drilling is canceled to perform normal operation. Point R and point Z are cleared. Other drilling data is also canceled (cleared).

Example

M51 ; Setting C-axis index mode ON M3 S2000 ; Rotating the drill G00 X50.0 C0.0 ; Positioning the drill along the X- and C-axes. G83 Z-40.0 R-5.0 P500 F5.0 M31 ; Drilling hole 1 C90.0 M31 ; Drilling hole 2 C180.0 M31 ; Drilling hole 3 C270.0 M31 ; Drilling hole 4 G80 M05 ; Canceling the drilling cycle and stopping drill rotation M50 ; Setting C-axis index mode off

4.3.5 Canned Cycle for Drilling with M Code Output Improved

Overview

Up to two pairs of M codes used for C-axis clamp/unclamp in canned cycles for drilling can be set for each path.

Details

Set the M codes for C-axis clamp/unclamp in the following parameters.

Bit 4 of parameter No. 5161=1

Pair 1 Pair 2

M code for clamp

M code for unclamp

When the M code for clamp set in parameter No. 5110 or 13544 (valid when bit 4 (CME) of parameter No. 5161 is set to 1) is specified in the block for a canned cycle for drilling, the specified M code is output before the tool is fed in rapid traverse to the point-R level after positioned. The M code for unclamp paired with that specified M code is output after the tool retracts to the point-R level.

Example 1: When bit 4 of parameter No. 5161 is set to 1, and 68, 78, 168, and 178 are specified in parameters

Nos. 5110, 13543, 13544, 13545, respectively, the following M codes are output.

Command Clamp Unclamp

G83X_C_...M68 M68 M78

G83X_C_...M168 M168 M178

No.5110 No.13544 No.5110

No.13543 No.13545 (Setting in parameter No. 5110 + 1)

- 82 -

Bit 4 of parameter No. 5161=0

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

Example 2: When bit 4 of parameter No. 5161 is set to 0, and 68 is specified in parameter No. 5110, respectively,

the following M codes are output.

Command Clamp Unclamp

G83X_C_...M68 M68 M69

PROGRAMMING

NOTE

1 Both the M codes for clamp and unclamp are set to 0, the setting of the pair is

invalid.

2 If the same M code for clamp is set for pairs 1 and 2, the setting for pair 1 that is

specified in parameter No. 13543 is used as the M code for unclamp.

4.3.6 Precautions to be Taken by Operator

- Reset and emergency stop

Even when the controller is stopped by resetting or emergency stop in the course of drilling cycle, the drilling mode and drilling data are saved; with this mind, therefore, restart operation.

- Single block

When drilling cycle is performed with a single block, the operation stops at the end points of operations 1, 2, 6 in Fig. 4.3 (a). Consequently, it follows that operation is started up 3 times to drill one hole. The operation stops at the end points of operations 1, 2 with the feed hold lamp ON. If there is a remaining repetitive count at the end of operation 6, the operation is stopped by feed hold. If there is no remaining repetitive count, the operation is stopped in the single block stop state.

- Feed hold

When "Feed Hold" is applied between operations 3 and 5 by G84/G88, the feed hold lamp lights up immediately if the feed hold is applied again to operation 6.

- Override

During operation with G84 and G88, the feedrate override is 100%.

4.4 IN-POSITION CHECK SWITCHING FOR DRILLING

CANNED CYCLE

Overview

This function enables dedicated in-position widths to be used for drilling canned cycle. Up to four different dedicated in-position widths are available, one for hole bottoms and three for other than hole bottoms. Using a little large in-position width for operations at locations where no nigh precision is required makes drilling canned cycle faster.

Explanation

Setting bit 4 (ICS) of parameter No. 5107 to 1 enables dedicated in-position widths to be used for drilling canned cycle. Up to four different dedicated in-position widths are available, one for hole bottoms and three for other than hole bottoms. In conventional drilling canned cycle, the same operation is performed for both in-position checks between cycles for locations where no very high precision is required (A in Fig. 4.4 (a)) and in-position checks between cycles for hole bottoms where a high precision is required (B in Fig. 4.4 (a)) because the same in-position width is used for all cycles.

- 83 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

Using this function makes it possible to reduce the time needed to get in an in-position state (to reduce the necessary cycle time) by setting a small in-position width for hole bottoms so as to assure a high precision while setting a little large in-position width for other than hole bottoms.

Fig. 4.4 (a) Example of a peck drilling cycle (G83)

- Parameters related to in-position wi dths

This function uses the following in-position widths.

In-position width for other than hole bottoms (regular) (parameter No. 5184) In-position width for other than hole bottoms (for retraction in peck drilling cycle) (parameter No.

5185)

In-position width for other than hole bottoms (for shift in boring cycles (G76 and G87) (parameter

No. 5186)

In-position width for hole bottoms (parameter No. 5187)

- Supported drilling canned cycle

The following table lists the drilling canned cycle for which this function is usable.

Table 4.4 (a) Drilling canned cycle for which this function is usable (lathe system)

G code Use

G83 High-speed peck drilling cycle G83.5 Front high-speed peck drilling cycle G83.6 Front peck drilling cycle

G84 Front tapping cycle

G85 Front boring cycle

G87 Side drilling cycle G87.5 Side high-speed peck drilling cycle G87.6 Side peck drilling cycle

G88 Side tapping cycle

G89 Side boring cycle

- 84 -

4.FUNCTIONS TO SIMPLIFY

B-64484EN-1/03 PROGRAMMING

PROGRAMMING

- Front drilling cycle (G83)/side drilling cycle (G87)

Shown below are the points where a dedicated effective area (for in-position check) is applied in front drilling cycle and side drilling cycle. If no Q (depth of cut for each cutting feed) is specified in a drilling cycle (G83 or G87), an ordinary drilling cycle is assumed.

G83 X(U)_ C(H)_ Z(W)_ R_ P_ F_ K_ M_ ;

G87 Z(W)_ C(H)_ X(U)_ R_ P_ F_ K_ M_ ;

X_ C_ or Z_ C_ : Hole position data Z_ or X_ : The distance from point R to the bottom of the hole R_ : The distance from the initial level to point R level P_ : Dwell time at the bottom of a hole F_ : Cutting feedrate K_ : Number of repeats (When it is needed) M_ : M code for C-axis clamp (When it is needed.)

G83 or G87 (G98 mode) G83 or G87 (G99 mode)

Mα

Initial level

Point R

Point R level

M(α+1),P2

Point Z

Mα : M code for C-axis clamp M(α+1) : M code for C-axis unclamp P1 : Dwell specified in the program P2 : Dwell specified in parameter No. 5111

In-position width for other than hole bottoms (regular) In-position width for hole bottoms

Point R

Point R level

M(α+1),P2

Point Z

- 85 -

4. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-64484EN-1/03

- Front high-speed peck drilling cycle (G83, G83.5) / Side high-speed peck drilling cycle (G87, G87.5)

Shown below are the points where a dedicated effective area (for in-position check) is applied in front high-speed peck drilling cycle and side high-speed peck drilling cycle. In high-speed peck drilling cycles (G83 and G87) (bit 2 (RTR) of parameter No. 5101 = 0), G83.5 and G87.5 can also be used to perform high-speed peck drilling regardless of the setting of the parameter RTR.

G83 X(U)_ C(H)_ Z(W)_ R_ P_ Q_ F_ K_ M_ ;

G87 Z(W)_ C(H)_ X(U)_ R_ P_ Q_ F_ K_ M_ ;

G83 or G87 (G98 mode) G83 or G87 (G99 mode)

Initial level

Point R

Mα

M(α+1),P2

Point Z

Point R

Mα

M(α+1),P2

Point R level

Point Z

Mα : M code for C-axis clamp M(α+1) : M code for C-axis unclamp P1 : Dwell specified in the program P2 : Dwell specified in parameter No. 5111 d : Retraction distance specified in parameter No. 5114

In-position width for other than hole bottoms (regular) In-position width for other than hole bottoms (for retraction in peck drilling cycle) In-position width for hole bottoms

- 86 -

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

Specifications and Main Features

Frequently Asked Questions

User Manual

SAFETY PRECAUTIONS

DEFINITION OF WARNING, CAUTION, AND NOTE

GENERAL WARNINGS AND CAUTIONS

WARNINGS AND CAUTIONS RELATED TO PROGRAMMING

WARNINGS AND CAUTIONS RELATED TO HANDLING

WARNINGS RELATED TO DAILY MAINTENANCE

TABLE OF CONTENTS

I. GENERAL

1 GENERAL

1.1 NOTES ON READING THIS MANUAL

1.2 NOTES ON VARIOUS KINDS OF DATA

II. PROGRAMMING

1 GENERAL

1.1 OFFSET

2 PREPARATORY FUNCTION (G FUNCTION)

3 INTERPOLATION FUNCTION

3.1 CONSTANT LEAD THREADING (G32)

3.2 CONTINUOUS THREADING

3.3 MULTIPLE THREADING

4 FUNCTIONS TO SIMPLIFY PROGRAMMING

4.1 CANNED CYCLE (G90, G92, G94)

4.1.1 Outer Diameter/Internal Diameter Cutting Cycle (G90)

4.1.1.1 Straight cutting cycle

4.1.1.2 Taper cutting cycle

4.1.2 Threading Cycle (G92)

4.1.2.1 Straight threading cycle

4.1.2.2 Taper threading cycle

4.1.3 End Face Turning Cycle (G94)

4.1.3.1 Face cutting cycle

4.1.3.2 Taper cutting cycle

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

4.1.5 Canned Cycle and Tool Nose Radius Compensation

4.1.6 Restrictions on Canned Cycles

4.2 MULTIPLE REPETITIVE CANNED CYCLE (G70-G76)

4.2.1 Stock Removal in Turning (G71)

4.2.2 Stock Removal in Facing (G72)

4.2.3 Pattern Repeating (G73)

4.2.4 Finishing Cycle (G70)

4.2.5 End Face Peck Drilling Cycle (G74)

4.2.6 Outer Diameter / Internal Diameter Drilling Cycle (G75)

4.2.7 Multiple Threading Cycle (G76)

4.2.8 Restrictions on Multiple Repetitive Canned Cycle (G70-G76)

4.3 CANNED CYCLE FOR DRILLING

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

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

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

4.3.4 Canned Cycle for Drilling Cancel (G80)

4.3.5 Canned Cycle for Drilling with M Code Output Improved

4.3.6 Precautions to be Taken by Operator