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

...

Page 1

GE Fanuc Automation

Computer Numerical Control Products

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

For Machining Center System

User’s Manual

GFZ-63944EN-2/02 June 2004

Page 2

Warnings, Cautions, and Notes as Used in this Publication

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

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

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

GFL-001

Warning

Caution

Note

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

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

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

Page 3

B-63944EN-2/02 SAFETY PRECAUTIONS

SAFETY PRECAUTIONS

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

CONTENTS

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

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

1.3 WARNINGS AND CAUTIONS RELATED TO

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

1.4 WARNINGS AND CAUTIONS RELATED TO HANDLINGs-9

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

s-1

Page 4

SAFETY PRECAUTIONS B-63944EN-2/02

1.1 DEFINITION OF WARNING, CAUTION, AND NOTE

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

WARNING

Applied when there is a danger of the user being

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

CAUTION

Applied when there is a danger of the equipment

being damaged, if the approved procedure is not observed.

NOTE

The Note is used to indicate supplementary

information other than Warning and Caution.

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

s-2

Page 5

B-63944EN-2/02 SAFETY PRECAUTIONS

1.2 GENERAL WARNINGS AND CAUTIONS

WARNING

1 Never attempt to machine a workpiece without first

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

2 Before operating the machine, thoroughly check

the entered data.

Operating the machine with incorrectly specified

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

3 Ensure that the specified feedrate is appropriate

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

The appropriate feedrate varies with the intended

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

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

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

4 When using a tool compensation function,

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

s-3

Page 6

SAFETY PRECAUTIONS B-63944EN-2/02

WARNING

5 The parameters for the CNC and PMC are

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

Failure to set a parameter correctly may result in

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

6 Immediately after switching on the power, do not

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

Some of the keys on the MDI panel are dedicated

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

7 The User’s Manual and programming manual

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

8 Some functions may have been implemented at

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

CAUTION

The liquid-crystal display is manufactured with very

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

s-4

Page 7

B-63944EN-2/02 SAFETY PRECAUTIONS

NOTE

Programs, parameters, and macro variables are

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

Such data may be deleted inadvertently, however,

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

To guard against the occurrence of the above, and

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

s-5

Page 8

SAFETY PRECAUTIONS B-63944EN-2/02

1.3 WARNINGS AND CAUTIONS RELATED TO

PROGRAMMING

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

WARNING

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

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

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

interpolation (positioning by nonlinear movement

between the start and end points), the tool path

must be carefully confirmed before performing

programming. Positioning involves rapid traverse. If

the tool collides with the workpiece, it may damage

the tool, the machine itself, the workpiece, or

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

or normal-direction (perpendicular) control, pay

careful attention to the speed of the rotation axis.

Incorrect programming may result in the rotation

axis speed becoming excessively high, such that

centrifugal force causes the chuck to lose its grip

on the workpiece if the latter is not mounted

securely. Such mishap is likely to damage the tool,

the machine itself, the workpiece, or cause injury to

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

convert the measurement units of data such as the

workpiece origin offset, parameter, and current

position. Before starting the machine, therefore,

determine which measurement units are being

used. Attempting to perform an operation with

invalid data specified may damage the tool, the

machine itself, the workpiece, or cause injury to the

user.

s-6

Page 9

B-63944EN-2/02 SAFETY PRECAUTIONS

WARNING

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

control approaches the origin of the workpiece

coordinate system, the spindle speed may become

excessively high. Therefore, it is necessary to

specify a maximum allowable speed. Specifying

the maximum allowable speed incorrectly may

damage the tool, the machine itself, the workpiece,

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

reference position return as required. Stroke check

is not possible before manual reference position

return is performed. Note that when stroke check is

disabled, an alarm is not issued even if a stroke

limit is exceeded, possibly damaging the tool, the

machine itself, the workpiece, or causing injury to

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

on the tool data specified during automatic

operation. If the tool specification does not match

the tool actually being used, the interference check

cannot be made correctly, possibly damaging the

tool or the machine itself, or causing injury to the

user. After switching on the power, or after

selecting a tool post manually, always start

automatic operation and specify the tool number of

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

incremental mode, or vice versa, the machine may

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

interpolation, helical interpolation, or a canned

cycle, the machine may behave unexpectedly.

Refer to the descriptions of the respective

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

torque limit. If a torque limit skip is specified

without the torque limit actually being applied, a

move command will be executed without

performing a skip.

s-7

Page 10

SAFETY PRECAUTIONS B-63944EN-2/02

WARNING

11 Programmable mirror image Note that programmed operations vary

considerably when a programmable mirror image is

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

system or a reference position return command is

issued in compensation function mode,

compensation is temporarily canceled, resulting in

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

therefore, always cancel compensation function

mode.

s-8

Page 11

B-63944EN-2/02 SAFETY PRECAUTIONS

1.4 WARNINGS AND CAUTIONS RELATED TO

HANDLING

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

WARNING

1 Manual operation When operating the machine manually, determine

the current position of the tool and workpiece, and

ensure that the movement axis, direction, and

feedrate have been specified correctly. Incorrect

operation of the machine may damage the tool, the

machine itself, the workpiece, or cause injury to the

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

reference position return as required.

If the machine is operated without first performing

manual reference position return, it may behave

unexpectedly. Stroke check is not possible before

manual reference position return is performed.

An unexpected operation of the machine may

damage the tool, the machine itself, the workpiece,

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

determine the current position of the tool and

workpiece, and ensure that the movement axis,

direction, and command have been specified

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

command specified may damage the tool, the

machine itself, the workpiece, or cause injury to the

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

large scale factor, such as 100, applied causes the

tool and table to move rapidly. Careless handling

may damage the tool and/or machine, or cause

injury to the user.

s-9

Page 12

SAFETY PRECAUTIONS B-63944EN-2/02

WARNING

5 Disabled override If override is disabled (according to the

specification in a macro variable) during threading,

rigid tapping, or other tapping, the speed cannot be

predicted, possibly damaging the tool, the machine

itself, the workpiece, or causing injury to the

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

when the machine is operating under the control of

a program. Otherwise, the machine may behave

unexpectedly, possibly damaging the tool, the

machine itself, the tool, or causing injury to the

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

imaging may shift the workpiece coordinate

system. Before attempting to operate the machine

under the control of a program, confirm the

coordinate system carefully.

If the machine is operated under the control of a

program without making allowances for any shift in

the workpiece coordinate system, the machine

may behave unexpectedly, possibly damaging the

tool, the machine itself, the workpiece, or causing

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

switches, in combination with the MDI panel, it is

possible to specify operations not supported by the

machine operator's panel, such as mode change,

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

operated inadvertently, the machine may behave

unexpectedly, possibly damaging the tool, the

machine itself, the workpiece, or causing injury to

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

running program. As a result, the servo axes are

stopped. However, the RESET key may fail to

function for reasons such as an MDI panel

problem. So, when the motors must be stopped,

use the emergency stop button instead of the

RESET key to ensure security.

s-10

Page 13

B-63944EN-2/02 SAFETY PRECAUTIONS

WARNING

10 Manual intervention If manual intervention is performed during

programmed operation of the machine, the tool

path may vary when the machine is restarted.

Before restarting the machine after manual

intervention, therefore, confirm the settings of the

manual absolute switches, parameters, and

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

functions can be disabled using custom macro

system variable #3004. Be careful when operating

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

of the machine. During a dry run, the machine

operates at dry run speed, which differs from the

corresponding programmed feedrate. Note that the

dry run speed may sometimes be higher than the

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

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

command in MDI mode, because cutter or tool

nose radius compensation is not applied. When a

command is entered from the MDI to interrupt in

automatic operation in cutter or tool nose radius

compensation mode, pay particular attention to the

tool path when automatic operation is subsequently

resumed. Refer to the descriptions of the

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

machining program is edited (modification,

insertion, or deletion), the machine may behave

unexpectedly if machining is resumed under the

control of that program. Basically, do not modify,

insert, or delete commands from a machining

program while it is in use.

s-11

Page 14

SAFETY PRECAUTIONS B-63944EN-2/02

1.5 WARNINGS RELATED TO DAILY MAINTENANCE

WARNING

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

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

and apply an emergency stop to the machine.

Because this work is performed with the power on

and the cabinet open, only those personnel who

have received approved safety and maintenance

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

touch the high-voltage circuits (marked

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

presents an extremely dangerous electric shock

hazard.

NOTE

The CNC uses batteries to preserve the contents

of its memory, because it must retain data such as

programs, offsets, and parameters even while

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

alarm is displayed on the machine operator's panel

or screen.

When a low battery voltage alarm is displayed,

replace the batteries within a week. Otherwise, the

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

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

details of the battery replacement procedure.

and

s-12

Page 15

B-63944EN-2/02 SAFETY PRECAUTIONS

WARNING

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

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

and apply an emergency stop to the machine.

Because this work is performed with the power on

and the cabinet open, only those personnel who

have received approved safety and maintenance

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

touch the high-voltage circuits (marked

and

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

presents an extremely dangerous electric shock

hazard.

NOTE

The absolute pulse coder uses batteries to

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

alarm is displayed on the machine operator's panel

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

replace the batteries within a week. Otherwise, the

absolute position data held by the pulse coder will

be lost. Refer to the FANUC SERVO MOTOR αi series

Maintenance Manual for details of the battery

replacement procedure.

s-13

Page 16

SAFETY PRECAUTIONS B-63944EN-2/02

WARNING

3 Fuse replacement

Before replacing a blown fuse, however, it is

necessary to locate and remove the cause of the

blown fuse.

For this reason, only those personnel who have

received approved safety and maintenance training

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

careful not to touch the high-voltage circuits

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

presents an extremely dangerous electric shock

hazard.

s-14

Page 17

B-63944EN-2/02 TABLE OF CONTENTS

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

I. GENERAL

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

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

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

II. PROGRAMMING

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

1.1 TOOL FIGURE AND TOOL MOTION BY PROGRAM................................. 12

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

3 INTERPOLATION FUNCTION ..............................................................18

3.1 INVOLUTE INTERPOLATION (G02.2, G03.2) ............................................ 19

3.1.1 Automatic Speed Control for Involute Interpolation..............................................24

3.1.2 Helical Involute Interpolation (G02.2, G03.2) .......................................................26

3.1.3 Involute Interpolation on Linear Axis and Rotary Axis (G02.2, G03.2) ...............27

3.2 THREADING (G33) .....................................................................................30

4 COORDINATE VALUE AND DIMENSION ...........................................32

4.1 POLAR COORDINATE COMMAND (G15, G16) ......................................... 33

5 FUNCTIONS TO SIMPLIFY PROGRAMMING ..................................... 37

5.1 CANNED CYCLE FOR DRILLING............................................................... 38

5.1.1 High-Speed Peck Drilling Cycle (G73)..................................................................43

5.1.2 Left-Handed Tapping Cycle (G74) ........................................................................45

5.1.3 Fine Boring Cycle (G76)........................................................................................47

5.1.4 Drilling Cycle, Spot Drilling (G81) .......................................................................49

5.1.5 Drilling Cycle Counter Boring Cycle (G82) ..........................................................51

5.1.6 Peck Drilling Cycle (G83)......................................................................................53

5.1.7 Small-Hole Peck Drilling Cycle.............................................................................55

5.1.8 Tapping Cycle (G84)..............................................................................................60

5.1.9 Boring Cycle (G85) ................................................................................................62

5.1.10 Boring Cycle (G86) ................................................................................................64

5.1.11 Back Boring Cycle (G87).......................................................................................66

5.1.12 Boring Cycle (G88) ................................................................................................69

c-1

Page 18

TABLE OF CONTENTS B-63944EN-2/02

5.1.13 Boring Cycle (G89) ................................................................................................71

5.1.14 Canned Cycle Cancel for Drilling (G80)................................................................73

5.1.15 Example for Using Canned Cycles for Drilling .....................................................74

5.2 RIGID TAPPING .......................................................................................... 76

5.2.1 Rigid Tapping (G84) ..............................................................................................77

5.2.2 Left-Handed Rigid Tapping Cycle (G74)...............................................................81

5.2.3 Peck Rigid Tapping Cycle (G84 or G74)...............................................................85

5.2.4 Canned Cycle Cancel (G80)...................................................................................89

5.2.5 Override during Rigid Tapping ..............................................................................90

5.2.5.1 Extraction override ............................................................................................ 90

5.2.5.2 Override signal .................................................................................................. 92

5.3 OPTIONAL CHAMFERING AND CORNER R .............................................93

5.4 INDEX TABLE INDEXING FUNCTION........................................................ 97

6 COMPENSATION FUNCTION ............................................................100

6.1 TOOL LENGTH COMPENSATION SHIFT TYPES ...................................101

6.2 AUTOMATIC TOOL LENGTH MEASUREMENT (G37) ............................ 106

6.3 TOOL OFFSET (G45 TO G48).................................................................. 110

6.4 OVERVIEW OF CUTTER COMPENSATION (G40-G42).......................... 115

6.5 OVERVIEW OF TOOL NOSE RADIUS COMPENSATION (G40-G42) ..... 122

6.5.1 Imaginary Tool Nose............................................................................................122

6.5.2 Direction of Imaginary Tool Nose .......................................................................124

6.5.3 Offset Number and Offset Value..........................................................................126

6.5.4 Workpiece Position and Move Command............................................................127

6.5.5 Notes on Tool Nose Radius Compensation..........................................................134

6.6 DETAILS OF CUTTER OR TOOL NOSE RADIUS COMPENSATION...... 136

6.6.1 Overview ..............................................................................................................136

6.6.2 Tool Movement in Start-up ..................................................................................140

6.6.3 Tool Movement in Offset Mode...........................................................................146

6.6.4 Tool Movement in Offset Mode Cancel...............................................................167

6.6.5 Prevention of Overcutting Due to Cutter or Tool Nose Radius Compensation ...175

6.6.6 Interference Check ...............................................................................................179

6.6.6.1 Operation to be performed if an interference is judged to occur ..................... 183

6.6.6.2 Interference check alarm function ...................................................................184

6.6.6.3 Interference check avoidance function ............................................................ 186

6.6.7 Cutter or Tool Nose Radius Compensation for Input from MDI .........................193

6.7 VECTOR RETENTION (G38) .................................................................... 195

6.8 CORNER CIRCULAR INTERPOLATION (G39) ........................................ 196

c-2

Page 19

B-63944EN-2/02 TABLE OF CONTENTS

6.9 THREE-DIMENSIONAL CUTTER COMPENSATION (G40, G41) ............198

6.10 TOOL COMPENSATION VALUES, NUMBER OF COMPENSATION

VALUES, AND ENTERING VALUES FROM THE PROGRAM (G10) ....... 203

6.11 COORDINATE SYSTEM ROTATION (G68, G69)..................................... 207

6.12 ACTIVE OFFSET VALUE CHANGE FUNCTION BASED ON MANUAL

FEED .........................................................................................................214

6.13 ROTARY TABLE DYNAMIC FIXTURE OFFSET....................................... 219

6.14 NORMAL DIRECTION CONTROL (G40.1, G41.1, G42.1)........................ 226

7 MEMORY OPERATION USING Series 15 PROGRAM FORMAT .....231

8 AXIS CONTROL FUNCTIONS............................................................232

8.1 TANDEM CONTROL ................................................................................. 233

8.2 CHOPPING FUNCTION ............................................................................ 234

III. OPERATION

1 SETTING AND DISPLAYING DATA................................................... 245

OFFSET

1.1 SCREENS DISPLAYED BY FUNCTION KEY

1.1.1 Setting and Displaying the Tool Compensation Value ........................................247

1.1.2 Tool Length Measurement ...................................................................................250

1.1.3 Tool Length/Workpiece Origin Measurement B..................................................252

1.1.4 Setting and Displaying the Rotary Table Dynamic Fixture Offset ......................271

SETTING

.................................. 246

APPENDIX

A PARAMETERS.................................................................................... 277

A.1 DESCRIPTION OF PARAMETERS........................................................... 278

A.2 DATA TYPE............................................................................................... 314

A.3 STANDARD PARAMETER SETTING TABLES......................................... 315

c-3

Page 20

Page 21

I. GENERAL

Page 22

Page 23

B-63944EN-2/02 GENERAL 1.GENERAL

1 GENERAL

This manual consists of the following parts:

About this manual

I. GENERAL Describes chapter organization, applicable models, related

manuals, and notes for reading this manual.

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

NC language, characteristics, and restrictions.

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

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

APPENDIX Lists parameters.

NOTE

1 This manual describes the functions that can

operate in the machining center system path

control type. For other functions not specific to the

lathe system, refer to the User's Manual (Common

to Lathe System/Machining Center System) (B-

63944EN). 2 Some functions described in this manual may not

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

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

mentioned in the text. For details of those

parameters, refer to the parameter manual (B-

63950EN). Parameters are used to set functions and

operating conditions of a CNC machine tool, and

frequently-used values in advance. Usually, the

machine tool builder factory-sets parameters so

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

also optional functions. Look up the options

incorporated into your system in the manual written

by the machine tool builder.

- 3 -

Page 24

1.GENERAL GENERAL B-63944EN-2/02

Applicable models

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

Model name Abbreviation

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

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

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

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

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

Series 31i

Series 310i

Series 310is

NOTE

1 Unless otherwise noted, the model names

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

2 Some functions described in this manual may not

be applied to some products.

For details, refer to the DESCRIPTIONS (B-

63942EN).

Special symbols

This manual uses the following symbols:

- IP

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

- ;

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

- 4 -

Page 25

B-63944EN-2/02 GENERAL 1.GENERAL

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

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

Table 1 Related manuals

Manual name Specification

number

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

B-63944EN

B-63943EN-2

B-63874EN B-63874EN-1

- 5 -

Page 26

1.GENERAL GENERAL B-63944EN-2/02

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

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

Table 2 Related manuals

Manual name

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

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

Specification

number

B-65262EN

B-65272EN

B-65302EN

B-65312EN

B-65282EN

B-65322EN

B-65285EN

B-65325EN

B-65270EN

B-65280EN

- 6 -

Page 27

B-63944EN-2/02 GENERAL 1.GENERAL

1.1 NOTES ON READING THIS MANUAL

CAUTION

1 The function of an CNC machine tool system

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

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

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

3 This manual describes as many reasonable variations

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

If a particular combination of operations is not

described, it should not be attempted.

1.2 NOTES ON VARIOUS KINDS OF DATA

CAUTION

Machining programs, parameters, offset data, etc.

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

- 7 -

Page 28

Page 29

II. PROGRAMMING

Page 30

Page 31

B-63944EN-2/02 PROGRAMMING 1.GENERAL

1 GENERAL

- 11 -

Page 32

1.GENERAL PROGRAMMING B-63944EN-2/02

1.1 TOOL FIGURE AND TOOL MOTION BY PROGRAM

Explanation

- Machining using the end of cutter - Tool length compensation function

Usually, several tools are used for machining one workpiece. The tools have different tool length. It is very troublesome to change the program in accordance with the tools. Therefore, the length of each tool used should be measured in advance. By setting the difference between the length of the standard tool and the length of each tool in the CNC (See Chapter “Setting and Displaying Data” in User’s Manual (Common to T/M series)), machining can be performed without altering the program even when the tool is changed. This function is called tool length compensation (See Section “Tool Length Compensation” in User’s Manual (Common to T/M series)).

Standard

H1 H2

tool

Workpiece

H3 H4

- Machining using the side of cutter - Cutter compensation function

ath using cutter compensation

Cutter

Workpiece

Machined part figure

Tool

Because a cutter has a radius, the center of the cutter path goes around the workpiece with the cutter radius deviated. If radius of cutters are stored in the CNC (See Chapter “Setting and Displaying Data” in User’s Manual (Common to T/M series)), the tool can be moved by cutter radius apart from the machining part figure. This function is called cutter compensation (See Section II-6 “Tool Compensation Function”).

- 12 -

Page 33

B-63944EN-2/02 PROGRAMMING 2.PREPARATORY FUNCTION (G FUNCTION)

2 PREPARATORY FUNCTION (G

FUNCTION)

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

Type Meaning

One-shot G code

Modal G code

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

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

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

- 13 -

Page 34

2.PREPARATORY FUNCTION (G FUNCTION) PROGRAMMING B-63944EN-2/02

Explanation

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

as indicated in Table.

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

at power-up or reset.

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

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

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

(No. 3402#0).

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

(No. 3402#3).

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

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

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

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

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

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

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

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

6. G codes are indicated by group.

7. The group of G60 is switched according to the setting of the parameter MDL (No. 5431#0). (When the MDL bit is set to 0, the 00 group is selected. When the MDL bit is set to 1, the 01 group is selected.)

- 14 -

Page 35

B-63944EN-2/02 PROGRAMMING 2.PREPARATORY FUNCTION (G FUNCTION)

Table 2(a) G code list

G code Group Function

G00 Positioning (rapid traverse) G01 Linear interpolation (cutting feed) G02 Circular interpolation CW or helical interpolation CW G03 Circular interpolation CCW or helical interpolation CCW G02.2, G03.2 Involute interpolation CW/CCW G02.3, G03.3 Exponential interpolation CW/CCW G02.4, G03.4 G04 Dwell G05 AI contour control (high-precision contour control compatible command) G05.1 AI contour control / Nano smoothing / Smooth interpolation G05.4 G06.2 01 NURBS interpolation G07 Hypothetical axis interpolation G07.1 (G107) Cylindrical interpolation G08 AI contour control (advanced preview control compatible command) G09 Exact stop G10 Programmable data input G10.6 Tool retract and recover G10.9 Programmable switching of diameter/radius specification G11 G12.1 Polar coordinate interpolation mode G13.1 G15 Polar coordinates command cancel G16 G17 XpYp plane selection G18 ZpXp plane selection G19 G20 (G70) Input in inch G21 (G71) G22 Stored stroke check function on G23 G25 Spindle speed fluctuation detection off G26 G27 Reference position return check G28 Automatic return to reference position G29 Movement from reference position G30 2nd, 3rd and 4th reference position return G30.1 Floating reference position return G31 Skip function G31.8 G33 Threading G34 Variable lead threading G35 Circular threading CW G36 G37 Automatic tool length measurement G38 Cutter or tool nose radius compensation : preserve vector G39

Three-dimensional coordinate conversion CW/CCW

HRV3,4 on/off

Programmable data input mode cancel

Polar coordinate interpolation cancel mode

Polar coordinates command

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

YpZp plane selection

Input in mm

Stored stroke check function off

Spindle speed fluctuation detection on

EGB-axis skip

Circular threading CCW

Cutter or tool nose radius compensation : corner circular interpolation

Zp: Z axis or its parallel axis

- 15 -

Page 36

2.PREPARATORY FUNCTION (G FUNCTION) PROGRAMMING B-63944EN-2/02

Table 2(a) G code list

G code Group Function

G40 Cutter or tool nose radius compensation : cancel

Three-dimensional cutter compensation : cancel

G41

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

G42

G42.2 Cutter compensation for 5-axis machining : right (type 1) G42.4 Cutter compensation for 5-axis machining : right (type 1) (FS16i-compatible command) G42.5 Cutter compensation for 5-axis machining : right (type 1) (FS16i-compatible command) G42.6 G40.1 Normal direction control cancel mode G41.1 Normal direction control on : right G42.1 G43 Tool length compensation + G44 G43.1 Tool length compensation in tool axis direction G43.4 Tool center point control (type 1) G43.5 G45 Tool offset increase G46 Tool offset decrease G47 Tool offset double increase G48 G49 (G49.1) 08 Tool length compensation cancel G50 Scaling cancel G51 G50.1 Programmable mirror image cancel G51.1 G50.2 Polygon turning cancel G51.2 G52 Local coordinate system setting G53 Machine coordinate system setting G53.1 G54 (G54.1) Workpiece coordinate system 1 selection G55 Workpiece coordinate system 2 selection G56 Workpiece coordinate system 3 selection G57 Workpiece coordinate system 4 selection G58 Workpiece coordinate system 5 selection G59 G60 00 Single direction positioning G61 Exact stop mode G62 Automatic corner override G63 Tapping mode G64 G65 00 Macro call

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

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

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

Normal direction control on : left

Tool length compensation -

Tool center point control (type 2)

Tool offset double decrease

Scaling

Programmable mirror image

Polygon turning

Tool axis direction control

Workpiece coordinate system 6 selection

Cutting mode

- 16 -

Page 37

B-63944EN-2/02 PROGRAMMING 2.PREPARATORY FUNCTION (G FUNCTION)

Table 2(a) G code list

G code Group Function

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

Macro modal call A/B cancel

Feature coordinate system selection

Figure copy (linear copy)

Canned cycle cancel

Boring cycle

Incremental programming

Workpiece coordinate system preset

Feed per revolution

Constant surface speed control cancel

Canned cycle : return to R point level

Polar coordinate interpolation mode cancel

- 17 -

Page 38

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/02

3 INTERPOLATION FUNCTION

- 18 -

Page 39

B-63944EN-2/02 PROGRAMMING 3.INTERPOLATION FUNCTION

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

Overview

Involute curve machining can be performed by using involute interpolation. Cutter compensation can be performed. Involute interpolation eliminates the need for approximating an involute curve with minute segments or arcs, and continuous pulse distribution is ensured even in high-speed operation of small blocks. Accordingly, high-speed operation can be performed smoothly. Moreover, machining programs can be created more easily, and the size of machining programs can be reduced. In involute interpolation, the following two types of feedrate override functions are automatically executed, and a favorable cutting surface can be formed with high precision. (Automatic speed control function for involute interpolation)

• Override in cutter compensation mode

• Override in the vicinity of basic circle

Format

Involute interpolation on the Xp-Yp plane

G17 G02.2 Xp_ Yp_ I_ J_ R_ F_ ; G17 G03.2 Xp_ Yp_ I_ J_ R_ F_ ;

Involute interpolation on the Zp-Xp plane

G18 G02.2 Zp_ Xp_ K_ I_ R_ F_ ; G18 G03.2 Zp_ Xp_ K_ I_ R_ F_ ;

Involute interpolation on the Yp-Zp plane

G19 G02.2 Yp_ Zp_ J_ K_ R_ F_ ; G19 G03.2 Yp_ Zp_ J_ K_ R_ F_ ;

Where, G02.2 : Involute interpolation (clockwise) G03.2 : Involute interpolation (counterclockwise) G17/G18/G19 : Xp-Yp/Zp-Xp/Yp-Zp plane selection Xp_ : X-axis or an axis parallel to the X-axis

(specified in a parameter)

Yp_ : Y-axis or an axis parallel to the Y-axis

(specified in a parameter)

Zp_ : Z-axis or an axis parallel to the Z-axis

(specified in a parameter)

I_, J_, K_ : Center of the base circle for an involute curve

viewed from the start point R_ : Base circle radius F_ : Cutting feedrate

- 19 -

Page 40

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/02

Explanation

Involute curve machining can be performed by using involute interpolation. Involute interpolation ensures continuous pulse distribution even in high-speed operation in small blocks, thus enabling smooth and high-speed machining. Moreover, machining programs can be created more easily, and the size of machining programs can be reduced.

- Involute curve

End point

Start point

End point

Start point

End point

Base circle

Clockwise involute interpolation (G02.2)

Counterclockwise involute interpolation (G03.2)

Fig. 3.1 (a) Actual movement

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

X (θ) = R [cos θ + (θ - θ

) sin θ] + X

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

where,

, YO : Coordinates of the center of a base circle

R : Base circle radius

: Angle of the start point of an involute curve

θ : Angle of the point where a tangent from the current

position to the base circle contacts the base circle

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

- 20 -

Page 41

B-63944EN-2/02 PROGRAMMING 3.INTERPOLATION FUNCTION

Start point

Involute curve

(X, Y)

- Start point and end point

- Base circle specification

(Xo, Yo)

Base circle

Fig. 3.1 (b) Involute curve

End point

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

The end point of an involute curve is specified using address Xp, Yp, or Zp. An absolute value or incremental value is used to specify an Xp, Yp, or Zp value. When using an incremental value, specify the coordinates of the end point viewed from the start point of the involute curve. When no end point is specified, alarm PS0241 is issued. If the specified start point or end point lies within the base circle, alarm PS0242 is issued. The same alarm is issued if cutter compensation C causes the offset vector to enter the base circle. Be particularly careful when applying an offset to the inside of an involute curve.

The center of a base circle is specified with I, J, and K, corresponding to X, Y, and Z. The value following I, J, or K is a vector component defined when the center of the base circle is viewed from the start point of the involute curve; this value must always be specified as an incremental value, regardless of the G90/G91 setting. Assign a sign to I, J, and K according to the direction. If I, J, and K are all left unspecified, or I0, J0, K0 is specified, alarm PS0241 or PS0242 is issued. If R is not specified, or R ≤ 0, alarm PS0241 or PS0242 is issued.

- 21 -

Page 42

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/02

- Choosing from two types of involute curves

When only a start point and I, J, and K data are given, two types of involute curves can be created. One type of involute curve extends towards the base circle, and the other extends away from the base circle. When the specified end point is closer to the center of the base circle than the start point, the involute curve extends toward the base circle. In the opposite case, the involute curve extends away from the base circle.

- Feedrate

The cutting feedrate specified in an F code is used as the feedrate for involute interpolation. The feedrate along the involute curve (feedrate along the tangent to the involute curve) is controlled to satisfy the specified feedrate.

- Plane selection

As with circular interpolation, the plane to which to apply involute interpolation can be selected using G17, G18, and G19.

- Cutter compensation

Cutter compensation can be applied to involute curve machining. As with linear and circular interpolation, G40, G41, and G42 are used to specify cutter compensation.

G40: Cutter compensation cancel G41: Cutter compensation left

G42: Cutter compensation right First, a point of intersection with a segment or an arc is approximated both at the start point and at the end point of the involute curve. An involute curve passing the two approximated points of intersection with the start point and end pint becomes the tool center path. Before selecting the involute interpolation mode, specify G41 or G42, cancel involute interpolation, and then specify G40. G41, G42, and G40 for cutter compensation cannot be specified in the involute interpolation mode.

- Automatic speed control

Cutting precision can be improved by automatically overriding the programmed feedrate during involute interpolation. See a subsequent subsection, "Automatic Speed Control for Involute Interpolation."

- 22 -

Page 43

B-63944EN-2/02 PROGRAMMING 3.INTERPOLATION FUNCTION

- Specifiable G codes

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

G04: Dwell

G10: Programmable data input

G17: X-Y plane selection

G18: Z-X plane selection

G19: Y-Z plane selection

G65: Macro call

G66: Macro modal call

G67: Macro modal call cancel

G90: Absolute programming

G91: Incremental programming

- Modes that allow involute interpolation specification

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

G41 : Cutter compensation left

G42 : Cutter compensation right

G51 : Scaling

G51.1 : Programmable mirror image

G68 : Coordinate rotation

- End point error

As shown below the end point may not be located on an involute curve that passes through the start point. When an involute curve that passes through the start point deviates from the involute curve that passes through the end point by more than the value set in parameter No. 5610, alarm PS0243 is issued. If there is an end point error, the programmed feedrate changes by the amount of error.

End point

Path after correction

Deviation

Start point

Correct involute curve

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

(G03.2)

- 23 -

Page 44

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/02

3.1.1 Automatic Speed Control for Involute Interpolation

This function automatically overrides the programmed feedrate in two different ways during involute interpolation. With this function, a favorable cutting surface can be formed with high precision.

• Override in cutter compensation mode

• Override in the vicinity of basic circle

- Override in cutter compensation mode

When cutter compensation is applied to involute interpolation, control is exercised in ordinary involute interpolation so that the tangential feedrate on the tool-center path always keeps the specified feedrate. Under the control, the actual cutting feedrate (feedrate around the perimeter of the tool (cutting point) on the path specified in the program) changes because the curvature of the involute curve changes every moment. If the tool is offset in the inward direction of the involute curve in particular, the actual cutting feedrate becomes higher than the specified feedrate as the tool gets nearer to the base circle. For smooth machining, it is desirable to control the actual cutting feedrate so that the feedrate keeps the specified feedrate. This function calculates an appropriate override value for the ever-changing curvature of the involute curve in the involute interpolation mode after cutter compensation. The function also controls the actual cutting feedrate (tangential feedrate at the cutting point) so that it always keeps the specified feedrate.

Cutting point

Rofs

Rcp

Base circle

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

Path specified in the program

- 24 -

Page 45

B-63944EN-2/02 PROGRAMMING 3.INTERPOLATION FUNCTION

Inward offset OVR = Rcp/(Rcp + Rofs) × 100 Outward offset OVR = Rcp/(Rcp - Rofs) × 100 where,

Rcp : Radius of curvature at the center of the tool of the

involute curve passing through the center of the tool

Rofs : Radius of the cutter

- Clamping the override

The lower limit of override is specified in parameter No. 5620 so that the override for inward offset by cutter compensation or the override in the vicinity of the basic circle will not bring the speed of the tool center to zero in the vicinity of the basic circle. The lower limit of override (OVR1o) is specified in parameter No. 5620 so that the inward offset will not reduce the speed of the tool center to a very low level in the vicinity of the basic circle. Accordingly, the feedrate is clamped but does not fall below the level determined by the programmed feedrate and the lower limit of override (OVR1o). The outward offset may increase the override to a very high level, but the feedrate will not exceed the maximum cutting feedrate.

- Clamping the acceleration in the vicinity of basic circle

If the acceleration calculated from the radius of curvature of the involute curve exceeds a value specified in the corresponding parameter, the tangential velocity is controlled so that the actual acceleration will not exceed the value specified in the parameter. Because the acceleration is always limited to a constant level, efficient velocity control can be performed for each machine. Because smooth velocity control can be performed continuously, impacts in machining in the vicinity of the basic circle can be reduced. To calculate the acceleration, the radius of curvature of the involute curve and the tangential velocity are substituted into the following formula of circular acceleration: Acceleration = F × F/R F: Tangential velocity R: Radius of curvature The maximum permissible acceleration is specified in parameter No.

1735. If the calculated acceleration exceeds the maximum permissible acceleration, the feedrate is clamped to the level calculated by the following expression:

If the calculated clamp level falls below the lower limit of feedrate, the lower limit of feedrate becomes the clamp level. The lower limit of feedrate is specified in parameter No. 1732.

onaccelerati epermissibl Maximum curvature of Radius level Clamp ×=

- 25 -

Page 46

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/02

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

As with arc helical involute interpolation, this function performs helical involute interpolation on the two axes involute interpolation and on up to four other axes simultaneously.

Format

Helical involute interpolation in Xp-Yp plane

G17

Helical involute interpolation in Zp-Xp plane

G18

Helical involute interpolation in Yp-Zp plane

G19

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

G02.2

G03.2

G02.2

G03.2

G02.2

G03.2

Up to four axes can be specified.

Xp Yp

Zp Xp

Yp Zp

I J R

K I R α β γ δ F ;

J K R α β γ δ F ;

β γ δ F ;

- 26 -

Page 47

B-63944EN-2/02 PROGRAMMING 3.INTERPOLATION FUNCTION

3.1.3 Involute Interpolation on Linear Axis and Rotary Axis

(G02.2, G03.2)

By performing involute interpolation in the polar coordinate interpolation mode, involute cutting can be carried out. Cutting is performed along an involute curve drawn in the plane formed by a linear axis and a rotary axis.

Format

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

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

G02.2

G03.2

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

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

G02.2

G03.2

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

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

G02.2

G03.2

G02.2: Clockwise involute interpolation G03.2: Counterclockwise involute interpolation

Example) If the linear axis is the X-axis X, C : End point of the involute curve I, J : Center of the basic circle of the involute curve, viewed from the

R : Radius of basic circle F : Cutting feedrate

X C

Y C

Z C

start point

I J R F ;

J K R F ;

K I R F ;

- 27 -

Page 48

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/02

Example

C (Imaginary axis) Path after tool compensation

Programmed path

N202

N204

N205

N201

C-axis

Tool

X-axis

N200

N203

Fig. 3.1 (e) Involute interpolation in the polar coordinate interpolation mode

Z-axis

O0001 ; . . N010 T0101 ; . . N100 G90 G00 X15.0 C0 Z0 ; N200 G12.1 ; N201 G41 G00 X-1.0 ;

Positioning to the start point Polar coordinate interpolation started

N202 G01 Z-2.0 F__ ; N203 G02.2 X1.0 C9.425 I1.0 J0 R1.0 ; N204 G01 Z0 ;

Involute interpolation during polar coordinate interpolation

N205 G40 G00 X15.0 C0 ; N206 G13.1 ; N300 Z__ ;

Polar coordinate interpolation cancelled

N400 X__ C__ ; . . M30 ;

- 28 -

Page 49

B-63944EN-2/02 PROGRAMMING 3.INTERPOLATION FUNCTION

Limitation

- Number of involute curve turns

Both the start point and end point must be within 100 turns from the point where the involute curve starts. An involute curve can be specified to make one or more turns in a single block. If the specified start point or end point is beyond 100 turns from the point where the involute curve starts, alarm PS0242 is issued.

- Unspecifiable functions

In involute interpolation mode, optional chamfering and corner R cannot be specified.

- Mode that does not allow involute interpolation specification

Involute interpolation cannot be used in the following mode:

G07.1: Cylindrical interpolation

- 29 -

Page 50

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/02

3.2 THREADING (G33)

Straight threads with a constant lead can be cut. The position coder mounted on the spindle reads the spindle speed in real-time. The read spindle speed is converted to the feedrate per minute to feed the tool.

Format

G33IP_ F_ ;

F :Long axis direction lead

Workpiece

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 1-turn 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. 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 3.2 (a) lists the ranges for specifying the thread lead.

Table 3.2 (a) Ranges of lead sizes that can be specified

Least

Metric input

Inch input

command increment

0.001 mm F1 to F50000 (0.01 to 500.00mm)

0.0001 mm F1 to F50000 (0.01 to 500.00mm)

0.0001 inch F1 to F99999 (0.0001 to 9.9999inch)

0.00001 inch F1 to F99999 (0.0001 to 9.9999inch)

Command value range of the lead

- 30 -

Page 51

B-63944EN-2/02 PROGRAMMING 3.INTERPOLATION FUNCTION

NOTE

1 The spindle speed is limited as follows :

1 ≤ spindle speed ≤ (Maximum feedrate) / (Thread lead) Spindle speed : min-1 Thread lead : mm or inch

Maximum feedrate : mm/min or inch/min ; maximum

command-specified feedrate for feed-per-minute mode or maximum feedrate that is determined based on mechanical restrictions including those related to motors, whichever is smaller

2 Cutting feedrate override is not applied to the

converted feedrate in all machining process from rough cutting to finish cutting. The feedrate is fixed at 100%

3 The converted feedrate is limited by the upper

feedrate specified.

4 Feed hold is disabled during threading. Pressing the

feed hold key during threading causes the machine to stop at the end point of the next block after threading (that is, after the G33 mode is terminated)

Example

Threading at a pitch of 1.5mm G33 Z10. F1.5;

- 31 -

Page 52

4.COORDINATE VALUE AND DIMENSION PROGRAMMING B-63944EN-2/02

4 COORDINATE VALUE AND DIMENSION

This chapter contains the following topics.

4.1 POLAR COORDINATE COMMAND (G15, G16)

- 32 -

Page 53

B-63944EN-2/02 PROGRAMMING 4.COORDINATE VALUE AND DIMENSION

4.1 POLAR COORDINATE COMMAND (G15, G16)

The end point coordinate value can be input in polar coordinates (radius and angle). The plus direction of the angle is counterclockwise of the selected plane first axis + direction, and the minus direction is clockwise. Both radius and angle can be commanded in either absolute or incremental programming (G90, G91).

Format

Gxx Gyy G16; Starting the polar coordinate

command (polar coordinate mode) G00 IP_ ; : Polar coordinate command : G15; Canceling the polar coordinate

command (polar coordinate mode)

G16 : Polar coordinate command G15 : Polar coordinate command cancel Gxx : Plane selection of the polar coordinate command

(G17, G18 or G19)

Gyy : Center selection of the polar coordinate command

(G90 or G91)

G90 specifies the origin of the workpiece

coordinate system as the origin of the polar coordinate system, from which a radius is measured.

G91 specifies the current position as the origin of

the polar coordinate system, from which a radius is measured.

IP_ : Specifying the addresses of axes constituting the

plane selected for the polar coordinate system,

and their values First axis : radius of polar coordinate Second axis : angle of polar coordinate

- 33 -

Page 54

4.COORDINATE VALUE AND DIMENSION PROGRAMMING B-63944EN-2/02

- Setting the origin of the workpiece coordinate system as the origin of the polar coordinate system

Specify the radius (the distance between the origin and the point) to be programmed with an absolute programming. The origin of the workpiece coordinate system is set as the origin of the polar coordinate system. When a local coordinate system (G52) is used, the origin of the local coordinate system becomes the center of the polar coordinates.

Command position

Radius

ngle

ctual position

Radius

Command position

ngle

ctual position

When the angle is specified with an absolute command

When the angle is specified with an incremental command

- Setting the current position as the origin of the polar coordinate system

Specify the radius (the distance between the current position and the point) to be programmed with an incremental programming. The current position is set as the origin of the polar coordinate system.

Command position

Radius

When the angle is specified with an absolute command

ngle

ctual position

Command position

ngle

Radius

ctual position

When the angle is specified with an incremental command

Example

Bolt hole circle

- The origin of the workpiece coordinate system is set as the origin of the polar coordinate system.

- The XY plane is selected.

150

270

100mm

- 34 -

Page 55

B-63944EN-2/02 PROGRAMMING 4.COORDINATE VALUE AND DIMENSION

- Specifying angles and a radius with absolute programmings

N1 G17 G90 G16 ; Specifying the polar coordinate command and

selecting the XY plane

Setting the origin of the workpiece coordinate

system as the origin of the polar coordinate system

N2 G81 X100.0 Y30.0 Z-20.0 R-5.0 F200.0 ; Specifying a distance of 100 mm and an angle

of 30 degrees

N3 Y150.0 ; Specifying a distance of 100 mm and an angle

of 150 degrees

N4 Y270.0 ; Specifying a distance of 100 mm and an angle

of 270 degrees

N5 G15 G80 ; Canceling the polar coordinate command

- Specifying angles with incremental programmings and a radius with absolute programmings

N1 G17 G90 G16; Specifying the polar coordinate command and

selecting the XY plane

Setting the origin of the workpiece coordinate

system as the origin of the polar coordinate system

N2 G81 X100.0 Y30.0 Z-20.0 R-5.0 F200.0 ; Specifying a distance of 100 mm and an angle

of 30 degrees

N3 G91 Y120.0 ; Specifying a distance of 100 mm and an angle

of +120 degrees

N4 Y120.0 ; Specifying a distance of 100 mm and an angle

of +120 degrees

N5 G15 G80 ; Canceling the polar coordinate command

Limitation

- Specifying a radius in the polar coordinate mode

In the polar coordinate mode, specify a radius for circular interpolation or helical interpolation (G02, G03) with R.

- Axes that are not considered part of a polar coordinate command in the polar coordinate mode

Axes specified for the following commands are not considered part of the polar coordinate command:

• Dwell (G04)

• Programmable data input (G10)

• Local coordinate system setting (G52)

• Workpiece coordinate system setting (G92)

• Machine coordinate system setting (G53)

• Stored stroke check (G22)

• Coordinate system rotation (G68)

• Scaling (G51)

- 35 -

Page 56

4.COORDINATE VALUE AND DIMENSION PROGRAMMING B-63944EN-2/02

- Optional chamfering and corner R

Optional chamfering and corner R cannot be specified in polar coordinate mode.

- 36 -

Page 57

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

5 FUNCTIONS TO SIMPLIFY

PROGRAMMING

This chapter explains the following items:

5.1 CANNED CYCLE FOR DRILLING

5.2 RIGID TAPPING

5.3 OPTIONAL CHAMFERING AND CORNER R

5.4 INDEX TABLE INDEXING FUNCTION

- 37 -

Page 58

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

5.1 CANNED CYCLE FOR DRILLING

Overview

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, normally more than one block is required. In addition, the use of canned cycles can shorten the program to save memory. Table 5.1 (a) lists canned cycles for drilling.

Table 5.1 (a) Canned cycles for drilling

Explanation

G code

G73

G74 Feed

G76 Feed

G80 - - - Cancel

G81 Feed - Rapid traverse

G82 Feed Dwell Rapid traverse

G83

G84 Feed

G85 Feed - Feed Boring cycle G86 Feed Spindle stop Rapid traverse Boring cycle

G87 Feed Spindle CW Rapid traverse

G88 Feed

G89 Feed Dwell Feed Boring cycle

Drilling

(-Z direction)

Intermittent

feed

Intermittent

feed

A canned cycle for drilling consists of a sequence of six operations.

Operation 1 .........Positioning of axes X and Y (including also

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 point

Operation at the bottom of a hole

- Rapid traverse

Dwell → Spindle CW Oriented spindle stop

- Rapid traverse

Dwell → Spindle CCW

Dwell → Spindle stop

another axis)

Retraction

(+Z direction)

Feed

Rapid traverse

Feed Tapping cycle

Manual Boring cycle

Application

High-speed peck drilling cycle Left-hand tapping cycle Fine boring cycle

Drilling cycle, spot drilling cycle Drilling cycle, counter boring cycle Peck drilling cycle

Back boring cycle

- 38 -

Page 59

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

- Positioning plane

- Drilling axis

Operation 1

Operation 2

Point R level

Operation 3

Operation 4

Fig. 5.1 (a) Operation sequence of canned cycle for drilling

Initial level

Operation 6

Operation 5

Rapid traverse

Feed

The positioning plane is determined by plane selection code G17, G18, or G19. The positioning axis is an axis other than the drilling axis.

Although canned cycles for drilling 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. The drilling axis is a basic axis (X, Y, or Z) not used to define the positioning plane, or any axis parallel to that basic axis. The axis (basic axis or parallel axis) used as the drilling axis is determined according to the axis address for the drilling axis specified in the same block as G codes G73 to G89. If no axis address is specified for the drilling axis, the basic axis is assumed to be the drilling axis.

Table 5.1 (b) Positioning plane and drilling axis

G code Positioning plane Drilling axis

G17 Xp-Yp plane Zp G18 Zp-Xp plane Yp G19 Yp-Zp plane Xp

Xp: X axis or an axis parallel to the X axis Yp: Y axis or an axis parallel to the Y axis Zp: Z axis or an axis parallel to the Z axis

- 39 -

Page 60

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

Example

Assume that the U, V and W axes be parallel to the X, Y, and Z axes respectively. This condition is specified by parameter No. 1022. G17 G81 Z _ _: The Z axis is used for drilling. G17 G81 W _ _: The W axis is used for drilling. G18 G81 Y _ _: The Y axis is used for drilling. G18 G81 V _ _: The V axis is used for drilling. G19 G81 X _ _: The X axis is used for drilling. G19 G81 U _ _: The U axis is used for drilling. G17 to G19 may be specified in a block in which any of G73 to G89 is not specified.

CAUTION

Switch the drilling axis after canceling a canned

cycle for drilling.

NOTE

A parameter FXY (No. 5101 #0) can be set to the Z

axis always used as the drilling axis. When FXY=0, the Z axis is always the drilling axis.

- Travel distance along the drilling axis G90/G91

The travel distance along the drilling axis varies for G90 and G91 as follows:

G90 (Absolute programming) G91 (Incremental programming)

- Drilling mode

Point R

Point Z

Fig. 5.1 (b) Absolute programming and incremental programming

Z = 0

Point R

Point Z

G73, G74, G76, and G81 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.

- 40 -

Page 61

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

- Return point level G98/G99

When the tool reaches the bottom of a hole, the tool may be returned to point R or to the initial level. These operations are specified with G98 and G99. The following illustrates how the tool moves when G98 or G99 is specified. 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

Point R level

- Repeat

- Cancel

Fig. 5.1 (c) Initial level and point R level

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 (G91). If it is specified in absolute programming (G90), drilling is repeated at the same position.

Number of repeats K The maximum command value = 9999

If K0 is specified, drilling data is stored, but drilling is not performed.

NOTE

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

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

Group 01 G codes

G00 : Positioning (rapid traverse) G01 : Linear interpolation G02 : Circular interpolation or helical interpolation (CW) G03 : Circular interpolation or helical interpolation (CCW)

- 41 -

Page 62

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

- Symbols in figures

Subsequent sections explain the individual canned cycles. Figures in these Explanation use the following symbols:

Positioning (rapid traverse G00) Cutting feed (linear interpolation G01) Manual feed Oriented spindle stop

OSS

Shift (rapid traverse G00)

P Dwell

(The spindle stops at a fixed rotation position)

- 42 -

Page 63

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

5.1.1 High-Speed Peck Drilling Cycle (G73)

This cycle performs high-speed peck drilling. It performs intermittent cutting feed to the bottom of a hole while removing chips from the hole.

Format

G73 X_ Y_ Z_ R_ Q_ F_ K_ ;

X_ Y_ : Hole position data Z_ : The distance from point R to the bottom of the hole R_ : The distance from the initial level to point R level Q_ : Depth of cut for each cutting feed F_ : Cutting feedrate K_ : Number of repeats (if required)

G73 (G98) G73 (G99)

Initial level

Explanation

- Operations

- Spindle rotation

Point R

Point Z

Point R

Point R level

Point Z

The high-speed peck drilling cycle performs intermittent feeding along the Z-axis. When this cycle is used, chips can be removed from the hole easily, and a smaller value can be set for retraction. This allows, drilling to be performed efficiently. Set the clearance, d, in parameter 5114. The tool is retracted in rapid traverse.

Before specifying G73, rotate the spindle using an auxiliary function (M code).

- 43 -

Page 64

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

- Auxiliary function

When the G73 code and an M code are specified in the same block, the M code is executed at the time of the first positioning operation. When K is used to specify the number of repeats, the M code is executed for the first hole only; for the second and subsequent holes, the M code is not executed.

- Tool length compensation

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the offset is applied after the time of positioning to point R.

Limitation

- Axis switching

Before the drilling axis can be changed, the canned cycle for drilling must be canceled.

- Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling is not performed.

- Q

Specify Q in blocks that perform drilling. If they are specified in a block that does not perform drilling, they cannot be stored as modal data.

- Cancel

Do not specify a G code of the 01 group (G00 to G03) and G73 in a single block. Otherwise, G73 will be canceled.

- Tool offset

In the canned cycle mode for drilling, tool offsets are ignored.

Example

M3 S2000 ; Cause the spindle to start rotating. G90 G99 G73 X300. Y-250. Z-150. R-100. Q15. F120. ; Position, drill hole 1, then return to point R. Y-550. ; Position, drill hole 2, then return to point R. Y-750. ; Position, drill hole 3, then return to point R. X1000. ; Position, drill hole 4, then return to point R. Y-550. ; Position, drill hole 5, then return to point R. G98 Y-750. ; Position, drill hole 6, then return to the initial level. G80 G28 G91 X0 Y0 Z0 ; Return to the reference position M5 ; Cause the spindle to stop rotating.

- 44 -

Page 65

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

5.1.2 Left-Handed Tapping Cycle (G74)

This cycle performs left-handed tapping. In the left-handed tapping cycle, when the bottom of the hole has been reached, the spindle rotates clockwise.

Format

G74 X_ Y_ Z_ R_P_ F_ K_ ;

X_ Y_ : Hole position data Z_ : 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 F_ : Cutting feedrate K_ : Number of repeats (if required)

G74 (G98) G74 (G99)

Initial level

Explanation

- Operations

- Spindle rotation

Spindle CCW

Point R level

Point Z

Spindle CW

Point R

Spindle CCW

Point Z

Spindle CW

Point R

Tapping is performed by turning the spindle counterclockwise. When the bottom of the hole has been reached, the spindle is rotated clockwise for retraction. This creates a reverse thread.

CAUTION

Feedrate overrides are ignored during left-handed

tapping. A feed hold does not stop the machine until the return operation is completed.

Before specifying G74, use an auxiliary function (M code) to rotate the spindle counterclockwise. If drilling is continuously performed with a small value specified for the distance between the hole position and point R level or between the initial level and point R level, the normal spindle speed may not be reached at the start of hole cutting operation. In this case, insert a dwell before each drilling operation with G04 to delay the operation, without specifying the number of repeats for K. For some machines,

- 45 -

Page 66

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

the above note may not be considered. Refer to the manual provided by the machine tool builder.

- Auxiliary function

When the G74 command and an M code are specified in the same block, the M code is executed at the time of the first positioning operation. When K is used to specify the number of repeats, the M code is executed for the first hole only; for the second and subsequent holes, the M code is not executed.

- Tool length compensation

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the offset is applied after the time of positioning to point R.

Limitation

- Axis switching

Before the drilling axis can be changed, the canned cycle for drilling must be canceled.

- Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling is not performed.

- P

Specify P in blocks that perform drilling. If it is specified in a block that does not perform drilling, it cannot be stored as modal data.

- Cancel

Do not specify a G code of the 01 group (G00 to G03) and G74 in a single block. Otherwise, G74 will be canceled.

- Tool offset

In the canned cycle mode for drilling, tool offsets are ignored.

Example

M4 S100 ; Cause the spindle to start rotating. G90 G99 G74 X300. Y-250. Z-150. R-120. F120. ; Position, tapping hole 1, then return to point R. Y-550. ; Position, tapping hole 2, then return to point R. Y-750. ; Position, tapping hole 3, then return to point R. X1000. ; Position, tapping hole 4, then return to point R. Y-550. ; Position, tapping hole 5, then return to point R. G98 Y-750. ; Position, tapping hole 6, then return to the initial

level. G80 G28 G91 X0 Y0 Z0 ; Return to the reference position M5 ; Cause the spindle to stop rotating.

- 46 -

Page 67

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

5.1.3 Fine Boring Cycle (G76)

The fine boring cycle bores a hole precisely. When the bottom of the hole has been reached, the spindle stops, and the tool is moved away from the machined surface of the workpiece and retracted.

Format

G76 X_ Y_ Z_ R_ Q_ P_ F_ K_ ;

X_ Y_ : Hole position data Z_ : The distance from point R to the bottom of the hole R_ : The distance from the initial level to point R level Q_ : Shift amount at the bottom of a hole P_ : Dwell time at the bottom of a hole F_ : Cutting feedrate K_ : Number of repeats (if required)

G76 (G98) G76 (G99)

Spindle orientation

Shift amount q

Explanation

- Operations

- Spindle rotation

- Auxiliary function

Tool

Spindle CW

Point R

OSS

Initial level

Point Z

Point R

OSS

Spindle CW

Point R level

Point Z

When the bottom of the hole has been reached, the spindle is stopped at the fixed rotation position, and the tool is moved in the direction opposite to the tool nose and retracted. This ensures that the machined surface is not damaged and enables precise and efficient boring to be performed.

Before specifying G76, use a Auxiliary function (M code) to rotate the spindle.

When the G76 command and an M code are specified in the same block, the M code is executed at the time of the first positioning operation. When K is used to specify the number of repeats, the M code is executed for the first hole only; for the second and subsequent holes, the M code is not executed.

- 47 -

Page 68

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

- Tool length compensation

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the offset is applied after the time of positioning to point R.

Limitation

- Axis switching

Before the drilling axis can be changed, the canned cycle for drilling must be canceled.

- Drilling

In a block that does not contain X, Y, Z, R, or any additional axes, drilling is not performed.

- P/Q

Be sure to specify a positive value in Q. If Q is specified with a negative value, the sign is ignored. Set the direction of shift in the parameter (No.5148). Specify P and Q in a block that performs drilling. If they are specified in a block that does not perform drilling, they are not stored as modal data.

CAUTION

Q (shift at the bottom of a hole) is a modal value

retained within canned cycles for drilling. It must be specified carefully because it is also used as the depth of cut for G73 and G83.

- Cancel

Do not specify a G code of the 01 group (G00 to G03) and G76 in a single block. Otherwise, G76 will be canceled.

- Tool offset

In the canned cycle mode for drilling, tool offsets are ignored.

Example

M3 S500 ; Cause the spindle to start rotating. G90 G99 G76 X300. Y-250. Position, bore hole 1, then return to point R. Z-150. R-120. Q5. Orient at the bottom of the hole, then shift by 5

mm. P1000 F120. ; Stop at the bottom of the hole for 1 s. Y-550. ; Position, drill hole 2, then return to point R. Y-750. ; Position, drill hole 3, then return to point R. X1000. ; Position, drill hole 4, then return to point R. Y-550. ; Position, drill hole 5, then return to point R. G98 Y-750. ; Position, drill hole 6, then return to the initial level. G80 G28 G91 X0 Y0 Z0 ; Return to the reference position M5 ; Cause the spindle to stop rotating.

- 48 -

Page 69

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

5.1.4 Drilling Cycle, Spot Drilling (G81)

This cycle is used for normal drilling. Cutting feed is performed to the bottom of the hole. The tool is then retracted from the bottom of the hole in rapid traverse.

Format

G81 X_ Y_ Z_ R_ F_ K_ ;

X_ Y_ : Hole position data Z_ : The distance from point R to the bottom of the hole R_ : The distance from the initial level to point R level F_ : Cutting feedrate K_ : Number of repeats (if required)

G81 (G98) G81 (G99)

Initial level

Explanation

- Operations

- Spindle rotation

- Auxiliary function

- Tool length compensation

Point R

Point Z

Point R level

Point Z

After positioning along the X- and Y-axes, rapid traverse is performed to point R. Drilling is performed from point R to point Z. The tool is then retracted in rapid traverse.

Before specifying G81, use an auxiliary function (M code) to rotate the spindle.

When the G81 command and an M code are specified in the same block, the M code is executed at the time of the first positioning operation. When K is used to specify the number of repeats, the M code is performed for the first hole only; for the second and subsequent holes, the M code is not executed.

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the offset is applied after the time of positioning to point R.

- 49 -

Page 70

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

Limitation

- Axis switching

Before the drilling axis can be changed, the canned cycle for drilling must be canceled.

- Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling is not performed.

- Cancel

Do not specify a G code of the 01 group (G00 to G03) and G81 in a single block. Otherwise, G81 will be canceled.

- Tool offset

In the canned cycle mode for drilling, tool offsets are ignored.

Example

M3 S2000 ; Cause the spindle to start rotating. G90 G99 G81 X300. Y-250. Z-150. R-100. F120. ; Position, drill hole 1, then return to point R. Y-550. ; Position, drill hole 2, then return to point R. Y-750. ; Position, drill hole 3, then return to point R. X1000. ; Position, drill hole 4, then return to point R. Y-550. ; Position, drill hole 5, then return to point R. G98 Y-750. ; Position, drill hole 6, then return to the initial level. G80 G28 G91 X0 Y0 Z0 ; Return to the reference position M5 ; Cause the spindle to stop rotating.

- 50 -

Page 71

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

5.1.5 Drilling Cycle Counter Boring Cycle (G82)

This cycle is used for normal drilling. Cutting feed is performed to the bottom of the hole. At the bottom, a dwell is performed, then the tool is retracted in rapid traverse. This cycle is used to drill holes more accurately with respect to depth.

Format

G82 X_ Y_ Z_ R_ P_ F_ K_ ;

X_ Y_ : Hole position data Z_ : 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 feed rate K_ : Number of repeats (if required)

G82 (G98) G82 (G99)

Initial level

Explanation

- Operations

- Spindle rotation

- Auxiliary function

Point R

Point Z

Point R level

Point Z

After positioning along the X- and Y-axes, rapid traverse is performed to point R. Drilling is then performed from point R to point Z. When the bottom of the hole has been reached, a dwell is performed. The tool is then retracted in rapid traverse.

Before specifying G82, use an auxiliary function (M code) to rotate the spindle.

When the G82 command and an M code are specified in the same block, the M code is executed at the time of the first positioning operation. When K is used to specify the number of repeats, the M code is executed for the first hole only; for the second and subsequent holes, the M code is not executed.

- 51 -

Page 72

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

- Tool length compensation

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the offset is applied after the time of positioning to point R.

Limitation

- Axis switching

Before the drilling axis can be changed, the canned cycle for drilling must be canceled.

- Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling is not performed.

- P

Specify P in blocks that perform drilling. If it is specified in a block that does not perform drilling, it cannot be stored as modal data.

- Cancel

Do not specify a G code of the 01 group (G00 to G03) and G82 in a single block. Otherwise, G82 will be canceled.

- Tool offset

In the canned cycle mode for drilling, tool offsets are ignored.

Example

M3 S2000 ; Cause the spindle to start rotating. G90 G99 G82 X300. Y-250. Z-150. R-100. P1000 F120. ; Position, drill hole 1, and dwell for 1 s at the

bottom of the hole, then return to point R. Y-550. ; Position, drill hole 2, then return to point R. Y-750. ; Position, drill hole 3, then return to point R. X1000. ; Position, drill hole 4, then return to point R. Y-550. ; Position, drill hole 5, then return to point R. G98 Y-750. ; Position, drill hole 6, then return to the initial level. G80 G28 G91 X0 Y0 Z0 ; Return to the reference position M5 ; Cause the spindle to stop rotating.

- 52 -

Page 73

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

5.1.6 Peck Drilling Cycle (G83)

This cycle performs peck drilling. It performs intermittent cutting feed to the bottom of a hole while removing shavings from the hole.

Format

G83 X_ Y_ Z_ R_ Q_ F_ K_ ;

G83 (G98) G83 (G99)

Initial level

Explanation

- Operations

- Spindle rotation

- Auxiliary function

Point R

Point Z

Point R

Point R level

Point Z

Q represents the depth of cut for each cutting feed. It must always be specified as an incremental value. In the second and subsequent cutting feeds, rapid traverse is performed up to a d point just before where the last drilling ended, and cutting feed is performed again. d is set in parameter (No.5115). Be sure to specify a positive value in Q. Negative values are ignored.

Before specifying G83, use an auxiliary function (M code) to rotate the spindle.

When the G83 command and an M code are specified in the same block, the M code is executed at the time of the first positioning operation. When K is used to specify the number of repeats, the M code is executed for the first hole only; for the second and subsequent holes, the M code is not executed.

- 53 -

Page 74

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

- Tool length compensation

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the offset is applied after the time of positioning to point R.

Limitation

- Axis switching

Before the drilling axis can be changed, the canned cycle for drilling must be canceled.

- Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling is not performed.

- Q

Specify Q in blocks that perform drilling. If they are specified in a block that does not perform drilling, they cannot be stored as modal data.

- Cancel

Do not specify a G code of the 01 group (G00 to G03) and G83 in a single block. Otherwise, G83 will be canceled.

- Tool offset

In the canned cycle mode for drilling, tool offsets are ignored.

Example

M3 S2000 ; Cause the spindle to start rotating. G90 G99 G83 X300. Y-250. Z-150. R-100. Q15. F120. ; Position, drill hole 1, then return to point R. Y-550. ; Position, drill hole 2, then return to point R. Y-750. ; Position, drill hole 3, then return to point R. X1000. ; Position, drill hole 4, then return to point R. Y-550. ; Position, drill hole 5, then return to point R. G98 Y-750. ; Position, drill hole 6, then return to the initial level. G80 G28 G91 X0 Y0 Z0 ; Return to the reference position M5 ; Cause the spindle to stop rotating.

- 54 -

Page 75

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

5.1.7 Small-Hole Peck Drilling Cycle

An arbor with the overload torque detection function is used to retract the tool when the overload torque detection signal (skip signal) is detected during drilling. Drilling is resumed after the spindle speed and cutting feedrate are changed. These steps are repeated in this peck drilling cycle. The mode for the small–hole peck drilling cycle is selected when the M code in parameter 5163 is specified. The cycle can be started by specifying G83 in this mode. This mode is canceled when G80 is specified or when a reset occurs.

Format

G83 X_ Y_ Z_ R_ Q_ F_I_ K_P ;

X_ Y_ : Hole position data

Z_ : Distance from point R to the bottom of the hole

R_ : Distance from the initial level to point R

Q_ : Depth of each cut

F_ : Cutting feedrate

I_ : Forward or backward traveling speed (same format as F above)

(If this is omitted, the values in parameters No.5172 and No.5173 are

assumed as defaults.)

K_ : Number of times the operation is repeated (if required)

P_ : Dwell time at the bottom of the hole

Point R level

∆

Point Z

Dwell

(If this is omitted, P0 is assumed as the default.)

G83 (G98) G83 (G99)

Overload torque

∆: Initial clearance when the tool is retracted to point R and the clearance from the

bottom of the hole in the second or subsequent drilling (parameter 5174)

q: Depth of each cut

()

∆

Path along which the tool travels at the rapid traverse rate

Path along which the tool travels at the programmed cutting

feedrate

Path along which the tool travels at the forward or backward rate during the

cycle specified with parameters

Initial level

∆

Point Z

Dwell

Point R Point R

Overload tor

- 55 -

Page 76

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

Explanations

- Componet operations of the cycle

* X- and Y-axis positioning * Positioning at point R along the Z–axis * Cutting along the Z-axis (first time, depth of cut Q, incremental)

Retracting (bottom of hole → minimum clearance ∆, incremental) Retraction

Repeated until point Z is reached

( bottom of hole+∆→ to point R, absolute) Forwarding (point R → to point with hole bottom + clearance ∆, absolute) Cutting

(second and subsequent times, cut of depth Q + ∆, incremental) * Dwell * Return to point R along the Z-axis (or initial point) = end of cycle

Acceleration/deceleration during advancing and retraction is controlled according to the cutting feed acceleration/deceleration time constant. When retraction is performed, the position is checked at point R.

- Specifying an M code

When the M code in parameter 5163 is specified, the system enters the mode for the small–hole peck drilling cycle. This M code does not wait for FIN. Care must be taken when this M code is specified with another M code in the same block.

(Example) M03 M ; → Waits for FIN. M M03 ; → Does not wait for FIN.

- Specifying a G code

When G83 is specified in the mode for the small-hole peck drilling cycle, the cycle is started. This continuous–state G code remains unchanged until another canned cycle is specified or until the G code for canceling the canned cycle is specified. This eliminates the need for specifying drilling data in each block when identical drilling is repeated.

- Signal indicating that the cycle is in progress

In this cycle, the signal indicating that the small–hole peck drilling cycleis in progress is output after the tool is positioned at the hole position along the axes not used for drilling. Signal output continues during positioning to point R along the drilling axis and terminates upon a return to point R or the initial level. For details, refer to the manual of the machine tool builder.

- Overload torque detection signal

A skip signal is used as the overload torque detection signal. The skip signal is effective while the tool is advancing or drilling and the tool

- 56 -

Page 77

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

tip is between points R and Z. (The signal causes a retraction). For details, refer to the manual of the machine tool builder.

NOTE

When receiving overload torque detect signal while the

tool is advancing, the tool will be retracted (clearance ∆

and to the point R), then advanced to the same target

point as previous advancing.

- Changing the drilling conditions

In a single G83 cycle, drilling conditions are changed for each drilling operation (advance → drilling → retraction). Bits 1 and 2 of parameter OLS, NOL No. 5160 can be specified to suppress the change in drilling conditions.

1 Changing the cutting feedrate The cutting feedrate programmed with the F code is changed for

each of the second and subsequent drilling operations. In

parameters No.5166 and No.5167, specify the respective rates of

change applied when the skip signal is detected and when it is

not detected in the previous drilling operation.

Cutting feedrate = F × α

<First drilling> α=1.0

<Second or subseqent drilling> α=α×β÷100, where β is the rate

of change for each drilling operation When the skip signal is detected during the previous

drillingoperation: β=b1% (parameter No.5166) When the skip signal is not detected during the previous

drillingoperation: β=b2% (parameter No.5167)

If the rate of change in cutting feedrate becomes smaller than the

rate specified in parameter 5168, the cutting feedrate is not

changed. The cutting feedrate can be increased up to the maximum cutting

feedrate.

2 Changing the spindle speed The spindle speed programmed with the S code is changed for

each of the second and subsequent advances. In parameters 5164

and 5165, specify the rates of change applied when the skip

signal is detected and when it is not detected in the previous

drilling operation.

Spindle speed = S × γ

<First drilling> γ=1.0 <Second or subseqent drilling> γ=γ×δ÷100, where δ is the rate of

change for each drilling operation

- 57 -

Page 78

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

When the skip signal is detected during the previous drilling

operation: δ=d1% (parameter No.5164) When the skip signal is not detected during the previous drilling

operation: δ=d2% (parameter No.5165)

When the cutting feedrate reaches the minimum rate, the spindle

speed is not changed. The spindle speed can be increased up to a

value corresponding to the maximum value of S analog data.

- Advance and retraction

Advancing and retraction of the tool are not executed in the same manner as rapid-traverse positioning. Like cutting feed, the two operations are carried out as interpolated operations. Note that the tool life management function excludes advancing and retraction from the calculation of the tool life.

- Specifying addess I

The forward or backward traveling speed can be specified with address I in the same format as address F, as shown below: G83 I1000 ; (without decimal point) G83 I1000. ; (with decimal point) Both commands indicate a speed of 1000 mm/min.

Address I specified with G83 in the continuous-state mode continues to be valid until G80 is specified or until a reset occurs.

NOTE

If address I is not specified and parqmeter No.5172 (for

backword) or No.5173 (for forword) is set to 0, the

forword or backword travel speed is same as the cutting

feedrate specified by F.

- Fuctions that can be specified

In this canned cycle mode, the following functions can be specified:

- Hole position on the X-axis, Y-axis, and additional axis

- Operation and branch by custom macro

- Subprogram (hole position group, etc.) calling

- Switching between absolute and incremental modes

- Coordinate system rotation

- Scaling (This command will not affect depth of cut Q or small

clearance ∆.)

- Dry run

- Feed hold

- Single block

When single-block operation is enabled, drilling is stopped after each retraction. Also, a single block stop is performed by setting parameter SBC (No.5105 bit 0)

- 58 -

Page 79

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

- Feedrate override

The feedrate override function works during cutting, retraction, and advancing in the cycle.

- Custom macro interface

The number of retractions made during cutting and the number of retractions made in response to the overload signal received during cutting can be output to custom macro common variables (#100 to #149) specified in parameters No.5170 and No.5171. Parameters No.5170 and No.5171 can specify variable numbers within the range of #100 to #149. Parameter No.5170: Specifies the number of the common variable to

which the number of retractions made during cutting is output.

Parameter No.5171: Specifies the number of the common variable to

which the number of retractions made in response to the overload signal received during cutting is output.

NOTE

The numbers of retruction output to common

valiables are cleared by G83 while small-hole peck driling cycle mode.

Limitation

- Subprogram call

In the canned cycle mode, specify the subprogram call command M98P_ in an independent block.

Example

M03 S_ ; Cause the spindle to start rotating. M ; Specifies the small-hole peck drilling cycle mode. G83 X_ Y_ Z_ R_ Q_ F_ I_ K_ P_ ;

Specifies the small-hole peck drilling cycle. X_ Y_ ; Drills at another position. : : G80 ; Cancels the small-hole peck drilling cycle mode.

- 59 -

Page 80

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

5.1.8 Tapping Cycle (G84)

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_ Y_ Z_ R_P_ F_ K_ ;

G84 (G98) G84 (G99)

Initial level

Explanation

- Operations

- Spindle rotation

Spindle CW P

Point R level

Point ZP

Spindle CCW

Point R

Spindle CW

Point ZP

Spindle CCW

Point R

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.

CAUTION

Feedrate overrides are ignored during tapping. A

feed hold does not stop the machine until the return operation is completed.

Before specifying G84, use an auxiliary function (M code) to rotate the spindle. If drilling is continuously performed with a small value specified for the distance between the hole position and point R level or between the initial level and point R level, the normal spindle speed may not be reached at the start of hole cutting operation. In this case, insert a dwell before each drilling operation with G04 to delay the operation,

- 60 -

Page 81

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

without specifying the number of repeats for K. For some machines, the above note may not be considered. Refer to the manual provided by the machine tool builder.

- Auxiliary function

When the G84 command and an M code are specified in the same block, the M code is executed at the time of the first positioning operation. When the K is used to specify number of repeats, the M code is executed for the first hole only; for the second and subsequent holes, the M code is not executed.

- Tool length compensation

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the offset is applied after the time of positioning to point R.

Limitation

- Axis switching

Before the drilling axis can be changed, the canned cycle for drilling must be canceled.

- Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling is not performed.

- P

Specify P in blocks that perform drilling. If it is specified in a block that does not perform drilling, it cannot be stored as modal data.

- Cancel

Do not specify a G code of the 01 group (G00 to G03) and G84 in a single block. Otherwise, G84 will be canceled.

Example

M3 S100 ; Cause the spindle to start rotating. G90 G99 G84 X300. Y-250. Z-150. R-120. P300 F120. ; Position, drill hole 1, then return to point R. Y-550. ; Position, drill hole 2, then return to point R. Y-750. ; Position, drill hole 3, then return to point R. X1000. ; Position, drill hole 4, then return to point R. Y-550. ; Position, drill hole 5, then return to point R. G98 Y-750. ; Position, drill hole 6, then return to the initial

level. G80 G28 G91 X0 Y0 Z0 ; Return to the reference position M5 ; Cause the spindle to stop rotating.

- 61 -

Page 82

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

5.1.9 Boring Cycle (G85)

This cycle is used to bore a hole.

Format

G85 X_ Y_ Z_ R_ F_ K_ ;

G85 (G98) G85 (G99)

Initial level

Explanation

- Operations

- Spindle rotation

- Auxiliary function

- Tool length compensation

Point R

Point Z

Point R

Point R level

Point Z

After positioning along the X- and Y- axes, rapid traverse is performed to point R. Drilling is performed from point R to point Z. When point Z has been reached, cutting feed is performed to return to point R.

Before specifying G85, use an auxiliary function (M code) to rotate the spindle.

When the G85 command and an M code are specified in the same block, the M code is executed at the time of the first positioning operation. When K is used to specify the number of repeats, the M code is executed for the first hole only; for the second and subsequent holes, the M code is not executed.

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the offset is applied after the time of positioning to point R.

- 62 -

Page 83

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

Limitation

- Axis switching

Before the drilling axis can be changed, the canned cycle for drilling must be canceled.

- Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling is not performed.

- Cancel

Do not specify a G code of the 01 group (G00 to G03) and G85 in a single block. Otherwise, G85 will be canceled.

- Tool offset

In the canned cycle mode for drilling, tool offsets are ignored.

Example

M3 S100 ; Cause the spindle to start rotating. G90 G99 G85 X300. Y-250. Z-150. R-120. F120. ; Position, drill hole 1, then return to point R. Y-550. ; Position, drill hole 2, then return to point R. Y-750. ; Position, drill hole 3, then return to point R. X1000. ; Position, drill hole 4, then return to point R. Y-550. ; Position, drill hole 5, then return to point R. G98 Y-750. ; Position, drill hole 6, then return to the

initial level. G80 G28 G91 X0 Y0 Z0 ; Return to the reference position M5 ; Cause the spindle to stop rotating.

- 63 -

Page 84

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

5.1.10 Boring Cycle (G86)

This cycle is used to bore a hole.

Format

G86 X_ Y_ Z_ R_ F_ K_ ;

G86 (G98) G86 (G99)

Spindle CW

Initial level

Spindle CW

Explanation

- Operations

- Spindle rotation

Point R

Point Z

Spindle stop

Point R level

Point Z

Spindle stop

After positioning along the X- and Y-axes, rapid traverse is performed to point R. Drilling is performed from point R to point Z. When the spindle is stopped at the bottom of the hole, the tool is retracted in rapid traverse.

Before specifying G86, use an auxiliary function (M code) to rotate the spindle. If drilling is continuously performed with a small value specified for the distance between the hole position and point R level or between the initial level and point R level, the normal spindle speed may not be reached at the start of hole cutting operation. In this case, insert a dwell before each drilling operation with G04 to delay the operation, without specifying the number of repeats for K. For some machines, the above note may not be considered. Refer to the manual provided by the machine tool builder.

- 64 -

Page 85

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

- Auxiliary function

When the G86 command and an M code are specified in the same block, the M code is executed at the time of the first positioning operation. When K is used to specify the number of repeats, the M code is executed for the first hole only; for the second and subsequent holes, the M code is not executed.

- Tool length compensation

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the offset is applied after the time of positioning to point R.

Limitation

- Axis switching

Before the drilling axis can be changed, the canned cycle for drilling must be canceled.

- Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling is not performed.

- Cancel

Do not specify a G code of the 01 group (G00 to G03) and G86 in a single block. Otherwise, G86 will be canceled.

- Tool offset

In the canned cycle mode for drilling, tool offsets are ignored.

Example

M3 S2000 ; Cause the spindle to start rotating. G90 G99 G86 X300. Y-250. Z-150. R-100. F120. ; Position, drill hole 1, then return to point R. Y-550. ; Position, drill hole 2, then return to point R. Y-750. ; Position, drill hole 3, then return to point R. X1000. ; Position, drill hole 4, then return to point R. Y-550. ; Position, drill hole 5, then return to point R. G98 Y-750. ; Position, drill hole 6, then return to the initial

level. G80 G28 G91 X0 Y0 Z0 ; Return to the reference position M5 ; Cause the spindle to stop rotating.

- 65 -

Page 86

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

5.1.11 Back Boring Cycle (G87)

This cycle performs accurate boring.

Format

G87 X_ Y_ Z_ R_ Q_ P_ F_ K_ ;

X_ Y_ : Hole position data Z_ : The distance from point R to the bottom of the hole R_ : The distance from the initial level to point R Q_ : Shift amount at the bottom of a hole P_ : Dwell time at the bottom of a hole F_ : Cutting feed rate K_ : Number of repeats (if required)

G87 (G98) G87 (G99)

Spindle orientation

Shift amount q

Explanation

- Spindle rotation

Tool

OSS

Spindle CW

OSS

Spindle CW

Initial level

Not used

Point Z

Point R

After positioning along the X- and Y-axes, the spindle is stopped at the fixed rotation position. The tool is moved in the direction opposite to the tool nose, positioning (rapid traverse) is performed to the bottom of the hole (point R). The tool is then shifted in the direction of the tool nose and the spindle is rotated clockwise. Boring is performed in the positive direction along the Z-axis until point Z is reached. At point Z, the spindle is stopped at the fixed rotation position again, the tool is shifted in the direction opposite to the tool nose, then the tool is returned to the initial level. The tool is then shifted in the direction of the tool nose and the spindle is rotated clockwise to proceed to the next block operation.

Before specifying G87, use an auxiliary function (M code) to rotate the spindle. If drilling is continuously performed with a small value specified for the distance between the hole position and point R level or between the initial level and point R level, the normal spindle speed may not be reached at the start of hole cutting operation. In this case, insert a dwell before each drilling operation with G04 to delay the operation, without specifying the number of repeats for K. For some machines, the above note may not be considered. Refer to the manual provided by the machine tool builder.

- 66 -

Page 87

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

- Auxiliary function

When the G87 command and an M code are specified in the same block, the M code is executed at the time of the first positioning operation. When K is used to specify the number of repeats, the M code is executed for the first hole only; for the second and subsequent holes, the M code is not executed.

- Tool length compensation

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the offset is applied after the time of positioning to point R.

Limitation

- Axis switching

Before the drilling axis can be changed, the canned cycle for drilling must be canceled.

- Drilling

In a block that does not contain X, Y, Z, R, or any additional axes, drilling is not performed.

- P/Q

Be sure to specify a positive value in Q. If Q is specified with a negative value, the sign is ignored. Set the direction of shift in the parameter (No. 5148). Specify P and Q in a block that performs drilling. If they are specified in a block that does not perform drilling, they are not stored as modal data.

CAUTION

Q (shift at the bottom of a hole) is a modal value

retained in canned cycles for drilling. It must be specified carefully because it is also used as the depth of cut for G73 and G83.

- Cancel

Do not specify a G code of the 01 group (G00 to G03) and G87 in a single block. Otherwise, G87 will be canceled.

- Tool offset

In the canned cycle mode for drilling, tool offsets are ignored.

- 67 -

Page 88

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

Example

M3 S500 ; Cause the spindle to start rotating. G90 G87 X300. Y-250. Position, bore hole 1. Z-150. R-120. Q5. Orient at the initial level, then shift by 5 mm. P1000 F120. ; Stop at point Z for 1 s. Y-550. ; Position, drill hole 2. Y-750. ; Position, drill hole 3. X1000. ; Position, drill hole 4. Y-550. ; Position, drill hole 5. Y-750. ; Position, drill hole 6 G80 G28 G91 X0 Y0 Z0 ; Return to the reference position M5 ; Cause the spindle to stop rotating.

- 68 -

Page 89

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

5.1.12 Boring Cycle (G88)

This cycle is used to bore a hole.

Format

G88 X_ Y_ Z_ R_ P_ F_ K_ ;

G88 (G98) G88 (G99)

Spindle CW

Initial level

Spindle CW

Explanation

- Operations

- Spindle rotation

Point R

Point Z

Spindle stop after dwell

Point R

Point Z

Point R level

Spindle stop after dwell

After positioning along the X- and Y-axes, rapid traverse is performed to point R. Boring is performed from point R to point Z. When boring is completed, a dwell is performed at the bottom of the hole, then the spindle is stopped and enters the hold state. At this time, you can switch to the manual mode and move the tool manually. Any manual operations are available; it is desirable to finally retract the tool from the hole for safety, though. At the restart of machining in the DNC operation or memory mode, the tool returns to the initial level or point R level according to G98 or G99 and the spindle rotates clockwise. Then, operation is restarted according to the programmed commands in the next block.

Before specifying G88, use an auxiliary function (M code) to rotate the spindle.

- 69 -

Page 90

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

- Auxiliary function

When the G88 command and an M code are specified in the same block, the M code is executed at the time of the first positioning operation. When K is used to specify the number of repeats, the M code is executed for the first hole only; for the second and subsequent holes, the M code is not executed.

- Tool length compensation

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the offset is applied after the time of positioning to point R.

Limitation

- Axis switching

Before the drilling axis can be changed, the canned cycle for drilling must be canceled.

- Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling is not performed.

- P

Specify P in blocks that perform drilling. If it is specified in a block that does not perform drilling, it cannot be stored as modal data.

- Cancel

Do not specify a G code of the 01 group (G00 to G03) and G88 in a single block. Otherwise, G88 will be canceled.

- Tool offset

In the canned cycle mode for drilling, tool offsets are ignored.

Example

M3 S2000 ; Cause the spindle to start rotating. G90 G99 G88 X300. Y-250. Z-150. R-100. P1000 F120. ; Position, drill hole 1, return to point R then stop

at the bottom of the hole for 1 s. Y-550. ; Position, drill hole 2, then return to point R. Y-750. ; Position, drill hole 3, then return to point R. X1000. ; Position, drill hole 4, then return to point R. Y-550. ; Position, drill hole 5, then return to point R. G98 Y-750. ; Position, drill hole 6, then return to the initial

level. G80 G28 G91 X0 Y0 Z0 ; Return to the reference position M5 ; Cause the spindle to stop rotating.

- 70 -

Page 91

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

5.1.13 Boring Cycle (G89)

This cycle is used to bore a hole.

Format

G89 X_ Y_ Z_ R_ P_ F_ K_ ;

G89 (G98) G89 (G99)

Initial level

Explanation

- Operations

- Spindle rotation

- Auxiliary function

- Tool length compensation

Point R

Point Z

Point R

Point R level

Point Z

This cycle is almost the same as G85. The difference is that this cycle performs a dwell at the bottom of the hole.

Before specifying G89, use an auxiliary function (M code) to rotate the spindle.

When the G89 command and an M code are specified in the same block, the M code is executed at the time of the first positioning operation. When K is used to specify the number of repeats, the M code is executed for the first hole only; for the second and subsequent holes, the M code is not executed.

When a tool length compensation (G43, G44, or G49) is specified in the canned cycle for drilling, the offset is applied after the time of positioning to point R.

- 71 -

Page 92

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

Limitation

- Axis switching

Before the drilling axis can be changed, the canned cycle for drilling must be canceled.

- Drilling

In a block that does not contain X, Y, Z, R, or any other axes, drilling is not performed.

- P

Specify P in blocks that perform drilling. If it is specified in a block that does not perform drilling, it cannot be stored as modal data.

- Cancel

Do not specify a G code of the 01 group (G00 to G03) and G89 in a single block. Otherwise, G89 will be canceled.

- Tool offset

In the canned cycle mode for drilling, tool offsets are ignored.

Example

M3 S100 ; Cause the spindle to start rotating. G90 G99 G89 X300. Y-250. Z-150. R-120. P1000 F120. ; Position, drill hole 1, return to point R then stop

level. G80 G28 G91 X0 Y0 Z0 ; Return to the reference position M5 ; Cause the spindle to stop rotating.

- 72 -

Page 93

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

5.1.14 Canned Cycle Cancel for Drilling (G80)

G80 cancels canned cycles for drilling.

Format

G80 ;

Explanation

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

Example

M3 S100 ; Cause the spindle to start rotating. G90 G99 G88 X300. Y-250. Z-150. R-120. F120. ; Position, drill hole 1, then return to point R. Y-550. ; Position, drill hole 2, then return to point R. Y-750. ; Position, drill hole 3, then return to point R. X1000. ; Position, drill hole 4, then return to point R. Y-550. ; Position, drill hole 5, then return to point R. G98 Y-750. ; Position, drill hole 6, then return to the initial

level. G80 G28 G91 X0 Y0 Z0 ; Return to the reference position, canned cycle

cancel M5 ; Cause the spindle to stop rotating.

- 73 -

Page 94

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

5.1.15 Example for Using Canned Cycles for Drilling

Offset value +200.0 is set in offset No.11, +190.0 is set in offset No.15, and +150.0 is set in offset No.31

Program example ;

N001 G92 X0 Y0 Z0; Coordinate setting at reference position N002 G90 G00 Z250.0 T11 M6; Tool change N003 G43 Z0 H11; Initial level, tool length compensation N004 S30 M3; Spindle start N005 G99 G81 X400.0 Y-350.0 Z-153.0 R-97.0 F120; Positioning, then #1 drilling N006 Y-550.0; Positioning, then #2 drilling and point R level return N007 G98 Y-750.0; Positioning, then #3 drilling and initial level return N008 G99 X1200.0; Positioning, then #4 drilling and point R level return N009 Y-550.0; Positioning, then #5 drilling and point R level return N010 G98 Y-350.0; Positioning, then #6 drilling and initial level return N011 G00 X0 Y0 M5; Reference position return, spindle stop N012 G49 Z250.0 T15 M6; Tool length compensation cancel, tool change N013 G43 Z0 H15; Initial level, tool length compensation N014 S20 M3; Spindle start N015 G99 G82 X550.0 Y-450.0 Z-130.0 R-97.0 P300 F70; Positioning, then #7 drilling, point R level return N016 G98 Y-650.0; Positioning, then #8 drilling, initial level return N017 G99 X1050.0; Positioning, then #9 drilling, point R level return N018 G98 Y-450.0; Positioning, then #10 drilling, initial level return N019 G00 X0 Y0 M5; Reference position return, spindle stop N020 G49 Z250.0 T31 M6; Tool length compensation cancel, tool change N021 G43 Z0 H31; Initial level, tool length compensation N022 S10 M3; Spindle start N023 G85 G99 X800.0 Y-350.0 Z-153.0 R47.0 F50; Positioning, then #11 drilling, point R level return N024 G91 Y-200.0 K2; Positioning, then #12, 13 drilling, point R level return N025 G28 X0 Y0 M5; Reference position return, spindle stop N026 G49 Z0; Tool length compensation cancel N027 M0; Program stop

- 74 -

Page 95

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

Program using tool length offset and canned cycles

Reference position

350

#1 #11

100

400 150 250 250 150

#1 to 6 Drilling of a 10 mm diameter hole #7 to 10 Drilling of a 20 mm diameter hole #11 to 13 Boring of a 95 mm diameter hole (depth 50 mm)

Retract position

250

50 50

30 20

T 11 T 15 T 31

200

#12

200

#13

#10

Initial level

190200 150

Fig. 5.1.15 (a) Example for using canned cycles for drilling

- 75 -

Page 96

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

5.2 RIGID TAPPING

The tapping cycle (G84) and left-handed tapping cycle (G74) may be performed in standard mode or rigid tapping mode. In standard mode, the spindle is rotated and stopped along with a movement along the tapping axis using auxiliary functions M03 (rotating the spindle clockwise), M04 (rotating the spindle counterclockwise), and M05 (stopping the spindle) to perform tapping. In rigid mode, tapping is performed by controlling the spindle motor as if it were a servo motor and by interpolating between the tapping axis and spindle. When tapping is performed in rigid mode, the spindle rotates one turn every time a certain feed (thread lead) which takes place along the tapping axis. This operation does not vary even during acceleration or deceleration. Rigid mode eliminates the need to use a floating tap required in the standard tapping mode, thus allowing faster and more precise tapping.

- 76 -

Page 97

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

5.2.1 Rigid Tapping (G84)

When the spindle motor is controlled in rigid mode as if it were a servo motor, a tapping cycle can be sped up.

Format

G84 X_ Y_ Z_ R_ P_ F_ K_ ;

X_ Y_ : Hole position data Z_ : The distance from point R to the bottom of the hole and the

position of the bottom of the hole R_ : The distance from the initial level to point R level P_ : Dwell time at the bottom of the hole and at point R when a return

is made F_ : Cutting feedrate K_ : Number of repeats (Only for necessity of repeat)

G84.2 X_ Y_ Z_ R_ P_ F_ L_ ; (Series 15 format)

L_ : Number of repeats (only for necessity of repeat)

G84 (G98) G84 (G99)

Explanation

Spindle stop

Initial level

Operation 1

Operation 2

Spindle CW

Point R

Operation 3

Spindle stop Spindle CCW

Operation 4

Operation 6

Spindle stop

Point R level

Operation 5

Point Z

After positioning along the X- and Y-axes, rapid traverse is performed to point R. Tapping is performed from point R to point Z. When tapping is completed, the spindle is stopped and a dwell is performed. The spindle is then rotated in the reverse direction, the tool is retracted to point R, then the spindle is stopped. Rapid traverse to initial level is then performed. While tapping is being performed, the feedrate override and spindle override are assumed to be 100%. Feedrate override can be enabled by setting, however.

Spindle stop

Spindle CW

Point R

Spindle stop Spindle CCW

Point R level

Point Z

- 77 -

Page 98

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

- Rigid mode

Rigid mode can be specified using any of the following methods:

• Specify M29 S***** before a tapping command.

• Specify M29 S***** in a block which contains a tapping command.

• Specify G84 for rigid tapping (parameter G84 No. 5200 #0 set to 1).

- Thread lead

In feed-per-minute mode, the thread lead is obtained from the expression, feedrate ÷ spindle speed. In feed-per-revolution mode, the thread lead equals the feedrate speed.

- Tool length compensation

If a tool length compensation (G43, G44, or G49) is specified in the canned cycle, the offset is applied at the time of positioning to point R.

- Series 15 format command

Rigid tapping can be performed using Series 15 format commands. The rigid tapping sequence (including data transfer to and from the PMC), Limitation, and the like are the same as described in this chapter.

- Acceleration/deceleration after interpolation

Linear or bell-shaped acceleration/deceleration can be applied.

- Look-ahead acceleration/deceleration before interpolation

Look-ahead acceleration/deceleration before interpolation is invalid.

- Override

Various types of override functions are invalid. The following override functions can be enabled by setting corresponding parameters:

• Extraction override

• Override signal

Details are given later.

- Dry run

Dry run can be executed also in G84 (G74). When dry run is executed at the feedrate for the drilling axis in G84 (G74), tapping is performed according to the feedrate. Note that the spindle speed becomes faster at a higher dry run feedrate.

- Machine lock

Machine lock can be executed also in G84 (G74). When G84 (G74) is executed in the machine lock state, the tool does not move along the drilling axis. Therefore, the spindle does not also rotate.

- 78 -

Page 99

B-63944EN-2/02 PROGRAMMING 5.FUNCTIONS TO SIMPLIFY PROGRAMMING

- Reset

When a reset is performed during rigid tapping, the rigid tapping mode is canceled and the spindle motor enters the normal mode. Note that the G84 (G74) mode is not canceled in this case when bit 6 (CLR) of parameter No. 3402 is set.

- Interlock

Interlock can also be applied in G84 (G74).

- Feed hold and single block

When bit 6 (FHD) of parameter No. 5200 is set to 0, feed hold and single block are invalid in the G84 (G74) mode. When this bit is set to 1, they are valid.

- Manual feed

For rigid tapping by manual handle feed, see the section "Rigid Tapping by Manual Handle." With other manual operations, rigid tapping cannot be performed.

- Backlash compensation

In the rigid tapping mode, backlash compensation is applied to compensate the lost motion when the spindle rotates clockwise or counterclockwise. Set the amount of backlash in parameters Nos. 5321 to 5324. Along the drilling axis, backlash compensation has been applied.

Limitation

- Axis switching

Before the drilling axis can be changed, the canned cycle must be canceled. If the drilling axis is changed in rigid mode, alarm PS0206 is issued.

- S command

• If a speed higher than the maximum speed for the gear being used is specified, alarm PS0200 is issued.

• When the rigid tapping canned cycle is cancelled, the S command used for rigid tapping is cleared to S0.

- Distribution amount for the spindle

The maximum distribution amount is as follows (displayed on diagnostic screen No. 451):

• For a serial spindle: 32,767 pulses per 8 ms

This amount is changed according to the gear ratio setting for the position coder or rigid tapping command. If a setting is made to exceed the upper limit, alarm PS0202 is issued.

- F command

If a value exceeding the upper limit of cutting feedrate is specified, alarm PS0011 is issued.

- 79 -

Page 100

5.FUNCTIONS TO SIMPLIFY PROGRAMMING PROGRAMMING B-63944EN-2/02

- Unit of F command

Metric input Inch input Remarks

G94 1 mm/min 0.01 inch/min

G95 0.01 mm/rev 0.0001 inch/rev

Decimal point programming allowed Decimal point programming allowed

- M29

If an S command and axis movement are specified between M29 and G84, alarm PS0203 is issued. If M29 is specified in a tapping cycle, alarm PS0204 is issued.

- P

Specify P in a block that performs drilling. If P is specified in a non-drilling block, it is not stored as modal data.

- Cancel

Do not specify a G code of the 01 group (G00 to G03 or G60 (when the MDL bit (bit 0 of parameter 5431) is set to 1)) and G74 in a single block. Otherwise, G74 will be canceled.

- Tool offset

In the canned cycle mode, tool offsets are ignored.

- Program restart

A program cannot be restarted during rigid tapping.

- Subprogram call

In the canned cycle mode, specify the subprogram call command M98P_ in an independent block.

Example

Z-axis feedrate 1000 mm/min Spindle speed 1000 min Thread lead 1.0 mm <Programming of feed per minute>

G94; Specify a feed-per-minute command. G00 X120.0 Y100.0 ; Positioning M29 S1000 ; Rigid mode specification G84 Z-100.0 R-20.0 F1000 ; Rigid tapping

G95 ; Specify a feed-per-revolution command. G00 X120.0 Y100.0 ; Positioning M29 S1000 ; Rigid mode specification G84 Z-100.0 R-20.0 F1.0 ; Rigid tapping

-1

- 80 -

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

Specifications and Main Features

Frequently Asked Questions

User Manual

SAFETY PRECAUTIONS

1.1 DEFINITION OF WARNING, CAUTION, AND NOTE

1.2 GENERAL WARNINGS AND CAUTIONS

1.5 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 TOOL FIGURE AND TOOL MOTION BY PROGRAM

3 INTERPOLATION FUNCTION

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

3.1.1 Automatic Speed Control for Involute Interpolation

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

3.2 THREADING (G33)

4 COORDINATE VALUE AND DIMENSION

4.1 POLAR COORDINATE COMMAND (G15, G16)

5.1 CANNED CYCLE FOR DRILLING

5.1.1 High-Speed Peck Drilling Cycle (G73)

5.1.2 Left-Handed Tapping Cycle (G74)

5.1.3 Fine Boring Cycle (G76)

5.1.4 Drilling Cycle, Spot Drilling (G81)

5.1.5 Drilling Cycle Counter Boring Cycle (G82)

5.1.6 Peck Drilling Cycle (G83)

5.1.7 Small-Hole Peck Drilling Cycle

5.1.8 Tapping Cycle (G84)

5.1.9 Boring Cycle (G85)

5.1.10 Boring Cycle (G86)

5.1.11 Back Boring Cycle (G87)

5.1.12 Boring Cycle (G88)

5.1.13 Boring Cycle (G89)

5.1.14 Canned Cycle Cancel for Drilling (G80)

5.1.15 Example for Using Canned Cycles for Drilling

5.2 RIGID TAPPING

5.2.1 Rigid Tapping (G84)