Fanuc 30i, 31i, 32i Operators Manual

Download

FANUC Series 30*-MODEL A FANUC Series 31*-MODEL A FANUC Series 32*-MODEL A

For Machining Center System

OPERATOR'S MANUAL

B-63944EN-2/04

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

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

The products in this manual are controlled based on Japan’s “Foreign Exchange and Foreign Trade Law”. The export of Series 30i/300i/300is-MODEL A, Series 31i/310i/310is-MODEL A5 from Japan is subject to an export license by the government of

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

In this manual we have tried as much as possible to describe all the various matters. However, we cannot describe all the matters which must not be done, or which cannot be done, because there are so many possibilities. Therefore, matters which are not especially described as possible in this manual should be regarded as ”impossible”.

CHANGE IN CNC MODEL NAMES

The model names of the following CNCs described in this manual have been changed from those shown in lower lines to those shown in upper lines in fields of the following table. The model names were changed, but their specifications remain unchanged. Keep the following in mind when using these models.

• Replace the old model names in this manual with the corresponding new model names.

• Replace the old model names indicated by the machines with the corresponding new model names.

Table 1 CNC Model Names

Model name Abbreviation

FANUC Series 30i-MODEL A (Old model name : FANUC Series 300i-MODEL A) FANUC Series 30i-MODEL A (Old model name : FANUC Series 300is-MODEL A)

FANUC Series 31i-MODEL A (Old model name : FANUC Series 310i-MODEL A) FANUC Series 31i-MODEL A5 (Old model name : FANUC Series 310i-MODEL A5)

FANUC Series 31i-MODEL A (Old model name : FANUC Series 310is-MODEL A) FANUC Series 31i-MODEL A5 (Old model name : FANUC Series 310is-MODEL A5)

FANUC Series 32i-MODEL A (Old model name : FANUC Series 320i-MODEL A) FANUC Series 32i-MODEL A (Old model name : FANUC Series 320is-MODEL A)

30i –A (300i–A) 30i –A (300is–A)

31i –A (310i–A) 31i –A5 (310i–A5)

31i –A (310is–A) 31i –A5 (310is–A5)

32i –A (320i–A) 32i –A (320is–A)

Series 30i (Series 300i) Series 30i (Series 300is)

Series 31i (Series 310i)

Series 31i (Series 310is)

Series 32i (Series 320i) Series 32i (Series 320is)

B-63944EN-2/04 SAFETY PRECAUTIONS

SAFETY PRECAUTIONS

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

CONTENTS

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

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

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

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

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

DEFINITION OF WARNING, CAUTION, AND NOTE

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

WARNING

Applied when there is a danger of the user being injured or when there is a

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

CAUTION

Applied when there is a danger of the equipment being damaged, if the

approved procedure is not observed.

NOTE

The Note is used to indicate supplementary information other than Warning and

Caution.

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

s-1

SAFETY PRECAUTIONS B-63944EN-2/04

GENERAL WARNINGS AND CAUTIONS

WARNING

1 Never attempt to machine a workpiece without first checking the operation of the

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

the workpiece and/or machine itself, or injury to the user. 2 Before operating the machine, thoroughly check the entered data. Operating the machine with incorrectly specified data may result in the machine

behaving unexpectedly, possibly causing damage to the workpiece and/or

machine itself, or injury to the user. 3 Ensure that the specified feedrate is appropriate for the intended operation.

Generally, for each machine, there is a maximum allowable feedrate. The appropriate feedrate varies with the intended operation. Refer to the manual

provided with the machine to determine the maximum allowable feedrate. If a machine is run at other than the correct speed, it may behave unexpectedly,

possibly causing damage to the workpiece and/or machine itself, or injury to the

user. 4 When using a tool compensation function, thoroughly check the direction and

amount of compensation.

Operating the machine with incorrectly specified data may result in the machine

behaving unexpectedly, possibly causing damage to the workpiece and/or

machine itself, or injury to the user. 5 The parameters for the CNC and PMC are factory-set. Usually, there is not need

to change them. When, however, there is not alternative other than to change a

parameter, ensure that you fully understand the function of the parameter before

making any change. Failure to set a parameter correctly may result in the machine behaving

unexpectedly, possibly causing damage to the workpiece and/or machine itself,

or injury to the user. 6 Immediately after switching on the power, do not touch any of the keys on the

MDI panel until the position display or alarm screen appears on the CNC unit. Some of the keys on the MDI panel are dedicated to maintenance or other

special operations. Pressing any of these keys may place the CNC unit in other

than its normal state. Starting the machine in this state may cause it to behave

unexpectedly. 7 The OPERATOR’S MANUAL and programming manual supplied with a CNC

unit provide an overall description of the machine's functions, including any

optional functions. Note that the optional functions will vary from one machine

model to another. Therefore, some functions described in the manuals may not

actually be available for a particular model. Check the specification of the

machine if in doubt. 8 Some functions may have been implemented at the request of the machine-tool

builder. When using such functions, refer to the manual supplied by the

machine-tool builder for details of their use and any related cautions.

s-2

B-63944EN-2/04 SAFETY PRECAUTIONS

CAUTION

The liquid-crystal display is manufactured with very precise fabrication

technology. Some pixels may not be turned on or may remain on. This

phenomenon is a common attribute of LCDs and is not a defect.

NOTE

Programs, parameters, and macro variables are stored in nonvolatile memory in

the CNC unit. Usually, they are retained even if the power is turned off. Such data may be deleted inadvertently, however, or it may prove necessary to

delete all data from nonvolatile memory as part of error recovery. To guard against the occurrence of the above, and assure quick restoration of

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

WARNINGS AND CAUTIONS RELATED TO PROGRAMMING

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

WARNING

Coordinate system setting

If a coordinate system is established incorrectly, the machine may behave

unexpectedly as a result of the program issuing an otherwise valid move

command. Such an unexpected operation may damage the tool, the machine

itself, the workpiece, or cause injury to the user. 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-3

SAFETY PRECAUTIONS B-63944EN-2/04

WARNING

Constant surface speed control

When an axis subject to constant surface speed control approaches the origin of

the workpiece coordinate system, the spindle speed may become excessively

high. Therefore, it is necessary to specify a maximum allowable speed.

Specifying the maximum allowable speed incorrectly may damage the tool, the

machine itself, the workpiece, or cause injury to the user. 6

Stroke check

After switching on the power, perform a manual reference position return as

required. Stroke check is not possible before manual reference position return is

performed. Note that when stroke check is disabled, an alarm is not issued even

if a stroke limit is exceeded, possibly damaging the tool, the machine itself, the

workpiece, or causing injury to the user. 7

Tool post interference check

A tool post interference check is performed based on the tool data specified

during automatic operation. If the tool specification does not match the tool

actually being used, the interference check cannot be made correctly, possibly

damaging the tool or the machine itself, or causing injury to the user. After

switching on the power, or after selecting a tool post manually, always start

automatic operation and specify the tool number of the tool to be used. 8

Absolute/incremental mode

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

versa, the machine may behave unexpectedly. 9

Plane selection

If an incorrect plane is specified for circular interpolation, helical interpolation, or

a canned cycle, the machine may behave unexpectedly. Refer to the

descriptions of the respective functions for details. 10

Torque limit skip

Before attempting a torque limit skip, apply the torque limit. If a torque limit skip

is specified without the torque limit actually being applied, a move command will

be executed without performing a skip. 11

Programmable mirror image

Note that programmed operations vary considerably when a programmable

mirror image is enabled. 12

Compensation function

If a command based on the machine coordinate system or a reference position

return command is issued in compensation function mode, compensation is

temporarily canceled, resulting in the unexpected behavior of the machine. Before issuing any of the above commands, therefore, always cancel

compensation function mode.

s-4

B-63944EN-2/04 SAFETY PRECAUTIONS

WARNINGS AND CAUTIONS RELATED TO HANDLING

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

WARNING

Manual operation

When operating the machine manually, determine the current position of the tool

and workpiece, and ensure that the movement axis, direction, and feedrate have

been specified correctly. Incorrect operation of the machine may damage the

tool, the machine itself, the workpiece, or cause injury to the operator. 2

Manual reference position return

After switching on the power, perform manual reference position return as

required.

If the machine is operated without first performing manual reference position

return, it may behave unexpectedly. Stroke check is not possible before manual

reference position return is performed.

An unexpected operation of the machine may damage the tool, the machine

itself, the workpiece, or cause injury to the user. 3

Manual numeric command

When issuing a manual numeric command, determine the current position of the

tool and workpiece, and ensure that the movement axis, direction, and command

have been specified correctly, and that the entered values are valid. Attempting to operate the machine with an invalid command specified may

damage the tool, the machine itself, the workpiece, or cause injury to the

operator. 4

Manual handle feed

In manual handle feed, rotating the handle with a large scale factor, such as 100,

applied causes the tool and table to move rapidly. Careless handling may

damage the tool and/or machine, or cause injury to the user. 5

Disabled override

If override is disabled (according to the specification in a macro variable) during

threading, rigid tapping, or other tapping, the speed cannot be predicted,

possibly damaging the tool, the machine itself, the workpiece, or causing injury

to the operator. 6

Origin/preset operation

Basically, never attempt an origin/preset operation when the machine is

operating under the control of a program. Otherwise, the machine may behave

unexpectedly, possibly damaging the tool, the machine itself, the tool, or causing

injury to the user. 7

Workpiece coordinate system shift

Manual intervention, machine lock, or mirror imaging may shift the workpiece

coordinate system. Before attempting to operate the machine under the control

of a program, confirm the coordinate system carefully.

If the machine is operated under the control of a program without making

allowances for any shift in the workpiece coordinate system, the machine may

behave unexpectedly, possibly damaging the tool, the machine itself, the

workpiece, or causing injury to the operator.

s-5

SAFETY PRECAUTIONS B-63944EN-2/04

WARNING

Software operator's panel and menu switches

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

MDI panel, it is possible to specify operations not supported by the machine

operator's panel, such as mode change, override value change, and jog feed

commands. Note, however, that if the MDI panel keys are operated inadvertently, the

machine may behave unexpectedly, possibly damaging the tool, the machine

itself, the workpiece, or causing injury to the user. 9

RESET key

Pressing the RESET key stops the currently running program. As a result, the

servo axes are stopped. However, the RESET key may fail to function for

reasons such as an MDI panel problem. So, when the motors must be stopped,

use the emergency stop button instead of the RESET key to ensure security. 10

Manual intervention

If manual intervention is performed during programmed operation of the

machine, the tool path may vary when the machine is restarted. Before restarting

the machine after manual intervention, therefore, confirm the settings of the

manual absolute switches, parameters, and absolute/incremental command

mode. 11

Feed hold, override, and single block

The feed hold, feedrate override, and single block functions can be disabled

using custom macro system variable #3004. Be careful when operating the

machine in this case. 12

Dry run

Usually, a dry run is used to confirm the operation of the machine. During a dry

run, the machine operates at dry run speed, which differs from the

corresponding programmed feedrate. Note that the dry run speed may

sometimes be higher than the programmed feed rate. 13

Cutter and tool nose radius compensation in MDI mode

Pay careful attention to a tool path specified by a command in MDI mode,

because cutter or tool nose radius compensation is not applied. When a

command is entered from the MDI to interrupt in automatic operation in cutter or

tool nose radius compensation mode, pay particular attention to the tool path

when automatic operation is subsequently resumed. Refer to the descriptions of

the corresponding functions for details. 14

Program editing

If the machine is stopped, after which the machining program is edited

(modification, insertion, or deletion), the machine may behave unexpectedly if

machining is resumed under the control of that program. Basically, do not

modify, insert, or delete commands from a machining program while it is in use.

s-6

B-63944EN-2/04 SAFETY PRECAUTIONS

WARNINGS RELATED TO DAILY MAINTENANCE

WARNING

Memory backup battery replacement

When replacing the memory backup batteries, keep the power to the machine

(CNC) turned on, and apply an emergency stop to the machine. Because this

work is performed with the power on and the cabinet open, only those personnel

who have received approved safety and maintenance training may perform this

work. When replacing the batteries, be careful not to touch the high-voltage circuits

(marked and fitted with an insulating cover). Touching the uncovered high-voltage circuits presents an extremely dangerous

electric shock hazard.

NOTE

The CNC uses batteries to preserve the contents of its memory, because it must

retain data such as programs, offsets, and parameters even while external

power is not applied. If the battery voltage drops, a low battery voltage alarm is displayed on the

machine operator's panel or screen.

When a low battery voltage alarm is displayed, replace the batteries within a

week. Otherwise, the contents of the CNC's memory will be lost. Refer to the Section “Method of replacing battery” in the OPERATOR’S

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

procedure.

WARNING

Absolute pulse coder battery replacement

When replacing the memory backup batteries, keep the power to the machine

(CNC) turned on, and apply an emergency stop to the machine. Because this

work is performed with the power on and the cabinet open, only those personnel

who have received approved safety and maintenance training may perform this

work. When replacing the batteries, be careful not to touch the high-voltage circuits

(marked

and fitted with an insulating cover).

Touching the uncovered high-voltage circuits presents an extremely dangerous

electric shock hazard.

NOTE

The absolute pulse coder uses batteries to preserve its absolute position. If the battery voltage drops, a low battery voltage alarm is displayed on the

machine operator's panel or screen. When a low battery voltage alarm is displayed, replace the batteries within a

week. Otherwise, the absolute position data held by the pulse coder will be lost. Refer to the FANUC SERVO MOTOR

of the battery replacement procedure.

series Maintenance Manual for details

s-7

SAFETY PRECAUTIONS B-63944EN-2/04

WARNING

3 Fuse replacement

Before replacing a blown fuse, however, it is necessary to locate and remove the

cause of the blown fuse.

For this reason, only those personnel who have received approved safety and

maintenance training may perform this work. When replacing a fuse with the cabinet open, be careful not to touch the

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

electric shock hazard.

s-8

B-63944EN-2/04 TABLE OF CONTENTS

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

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

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

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

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

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

I. GENERAL

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

1.1 NOTES ON READING THIS MANUAL..........................................................5

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

II. PROGRAMMING

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

1.1 TOOL FIGURE AND TOOL MOTION BY PROGRAM...................................9

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

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

3.1 INVOLUTE INTERPOLATION (G02.2, G03.2)............................................15

3.1.1 Automatic Speed Control for Involute Interpolation ..............................................19

3.1.2 Helical Involute Interpolation (G02.2, G03.2) .......................................................21

3.1.3 Involute Interpolation on Linear Axis and Rotary Axis

(G02.2, G03.2) .......................................................................................................22

3.2 THREADING (G33) .....................................................................................24

3.3 CIRCULAR THREAD CUTTING B (G2.1,G3.1)...........................................25

3.4 GROOVE CUTTING BY CONTINUOUS CIRCLE MOTION (G12.4, G13.4)28

4 COORDINATE VALUE AND DIMENSION ...........................................39

4.1 POLAR COORDINATE COMMAND (G15, G16).........................................39

5 FUNCTIONS TO SIMPLIFY PROGRAMMING.....................................42

5.1 CANNED CYCLE FOR DRILLING...............................................................42

5.1.1 High-Speed Peck Drilling Cycle (G73)..................................................................46

5.1.2 Left-Handed Tapping Cycle (G74) ........................................................................48

5.1.3 Fine Boring Cycle (G76)........................................................................................50

5.1.4 Drilling Cycle, Spot Drilling (G81) .......................................................................52

5.1.5 Drilling Cycle Counter Boring Cycle (G82)..........................................................53

5.1.6 Peck Drilling Cycle (G83)......................................................................................55

5.1.7 Small-Hole Peck Drilling Cycle (G83) ..................................................................57

5.1.8 Tapping Cycle (G84)..............................................................................................61

5.1.9 Boring Cycle (G85)................................................................................................63

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

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

5.1.12 Boring Cycle (G88)................................................................................................68

5.1.13 Boring Cycle (G89)................................................................................................70

c-1

TABLE OF CONTENTS B-63944EN-2/04

5.1.14 Canned Cycle Cancel for Drilling (G80)................................................................71

5.1.15 Example for Using Canned Cycles for Drilling .....................................................72

5.2 RIGID TAPPING..........................................................................................74

5.2.1 Rigid Tapping (G84) ..............................................................................................74

5.2.2 Left-Handed Rigid Tapping Cycle (G74)...............................................................78

5.2.3 Peck Rigid Tapping Cycle (G84 or G74)...............................................................82

5.2.4 Canned Cycle Cancel (G80)...................................................................................85

5.2.5 Override during Rigid Tapping ..............................................................................85

5.2.5.1 Extraction override ............................................................................................85

5.2.5.2 Override signal .................................................................................................. 86

5.3 OPTIONAL CHAMFERING AND CORNER R.............................................88

5.4 INDEX TABLE INDEXING FUNCTION........................................................91

5.5 IN-FEED CONTROL (FOR GRINDING MACHINE).....................................93

5.6 CANNED GRINDING CYCLE (FOR GRINDING MACHINE).......................95

5.6.1 Plunge Grinding Cycle (G75).................................................................................97

5.6.2 Direct Constant-Dimension Plunge Grinding Cycle (G77)..................................100

5.6.3 Continuous-feed Surface Grinding Cycle (G78)..................................................103

5.6.4 Intermittent-feed Surface Grinding Cycle (G79)..................................................106

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

G75.7,G76.7).............................................................................................109

5.7.1 Stock Removal in Turning (G71.7)......................................................................110

5.7.2 Stock Removal in Facing (G72.7)........................................................................121

5.7.3 Pattern Repeating (G73.7)....................................................................................125

5.7.4 Finishing Cycle (G70.7).......................................................................................128

5.7.5 End Face Peck Drilling Cycle (G74.7).................................................................132

5.7.6 Outer Diameter / Internal Diameter Drilling Cycle (G75.7) ................................134

5.7.7 Multiple Threading Cycle (G76.7).......................................................................136

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

G75.7, and G76.7)................................................................................................141

6 COMPENSATION FUNCTION............................................................143

6.1 TOOL LENGTH COMPENSATION SHIFT TYPES ...................................143

6.2 AUTOMATIC TOOL LENGTH MEASUREMENT (G37) ............................150

6.3 TOOL OFFSET (G45 TO G48)..................................................................153

6.4 OVERVIEW OF CUTTER COMPENSATION (G40-G42)..........................158

6.5 OVERVIEW OF TOOL NOSE RADIUS COMPENSATION (G40-G42).....163

6.5.1 Imaginary Tool Nose............................................................................................163

6.5.2 Direction of Imaginary Tool Nose .......................................................................165

6.5.3 Offset Number and Offset Value..........................................................................166

6.5.4 Workpiece Position and Move Command............................................................166

6.5.5 Notes on Tool Nose Radius Compensation..........................................................171

6.6 DETAILS OF CUTTER OR TOOL NOSE RADIUS COMPENSATION......173

6.6.1 Overview..............................................................................................................173

6.6.2 Tool Movement in Start-up ..................................................................................177

6.6.3 Tool Movement in Offset Mode...........................................................................183

6.6.4 Tool Movement in Offset Mode Cancel...............................................................201

6.6.5 Prevention of Overcutting Due to Tool Radius / Tool Nose Radius

Compensation.......................................................................................................207

6.6.6 Interference Check ...............................................................................................210

6.6.6.1 Operation to be performed if an interference is judged to occur..................... 213

6.6.6.2 Interference check alarm function ...................................................................214

6.6.6.3 Interference check avoidance function ............................................................215

6.6.7 Tool Radius / Tool Nose Radius Compensation for Input from MDI..................221

c-2

B-63944EN-2/04 TABLE OF CONTENTS

6.7 VECTOR RETENTION (G38)....................................................................223

6.8 CORNER CIRCULAR INTERPOLATION (G39)........................................224

6.9 3-DIMENSIONAL TOOL COMPENSATION (G40, G41)...........................226

6.10 TOOL COMPENSATION VALUES, NUMBER OF COMPENSATION

VALUES, AND ENTERING VALUES FROM THE PROGRAM (G10).......229

6.11 COORDINATE SYSTEM ROTATION (G68, G69).....................................232

6.12 GRINDING WHEEL WEAR COMPENSATION .........................................239

6.13 ACTIVE OFFSET VALUE CHANGE FUNCTION BASED ON MANUAL

FEED.........................................................................................................243

6.14 ROTARY TABLE DYNAMIC FIXTURE OFFSET.......................................247

6.15 TOOL AXIS DIRECTION TOOL LENGTH COMPENSATION...................253

6.15.1 Control Point Compensation of Tool Length Compensation Along Tool Axis...257

6.16 SPINDLE UNIT COMPENSATION, NUTATING ROTARY HEAD TOOL

LENGTH COMPENSATION......................................................................261

7 MEMORY OPERATION USING Series 15 PROGRAM FORMAT.....265

7.1 MULTIPLE REPETITIVE CYCLE ..............................................................266

7.1.1 Stock Removal in Turning (G71.7)......................................................................267

7.1.2 Stock Removal in Facing (G72.7)........................................................................279

7.1.3 Pattern Repeating (G73.7)....................................................................................283

7.1.4 Finishing Cycle (G70.7).......................................................................................286

7.1.5 End Face Peck Drilling Cycle (G74.7).................................................................290

7.1.6 Outer Diameter / Internal Diameter Drilling Cycle (G75.7) ................................291

7.1.7 Multiple Threading Cycle (G76.7).......................................................................293

7.1.8 Restrictions on Multiple Repetitive Cycle ...........................................................298

8 AXIS CONTROL FUNCTIONS............................................................300

8.1 CHOPPING FUNCTION............................................................................300

8.2 CHOPPING FUNCTION BY FLEXIBLE SYNCHRONOUS CONTROL.....306

8.3 PARALLEL AXIS CONTROL.....................................................................307

9 GAS CUTTING MACHINE ..................................................................313

9.1 TOOL OFFSET B ......................................................................................313

9.2 CONER CONTROL BY FEED RATE ........................................................316

9.3 AUTOMATIC EXACT STOP CHECK ........................................................318

9.4 AXIS SWITCHING.....................................................................................321

9.5 GENTLE CURVE CUTTING......................................................................324

9.6 GENTLE NORMAL DIRECTION CONTROL.............................................326

9.6.1 Linear Distance Setting ........................................................................................327

III. OPERATION

1 SETTING AND DISPLAYING DATA...................................................331

1.1 SCREENS DISPLAYED BY FUNCTION KEY ...................................331

1.1.1 1. Tool compensation value

2. Tool length measurement

3. Tool length/workpiece origin measurement

4. Rotary table dynamic fixture offset

Setting and Displaying the Tool Compensation Value ........................................331

1.1.2 Tool Length Measurement ...................................................................................336

c-3

TABLE OF CONTENTS B-63944EN-2/04

1.1.3 Tool Length/Workpiece Origin Measurement .....................................................339

1.1.4 Setting and Displaying the Rotary Table Dynamic Fixture Offset ......................358

1.1.5 Input of Tool Offset Value Measured B...............................................................361

1.1.6 Spindle Unit Compensation, Nutating Rotary Head Tool Length Compensation361

APPENDIX

A PARAMETERS....................................................................................367

A.1 DESCRIPTION OF PARAMETERS...........................................................367

A.2 DATA TYPE...............................................................................................415

A.3 STANDARD PARAMETER SETTING TABLES.........................................416

c-4

I. GENERAL

B-63944EN-2/04 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 Operator'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.

Applicable models

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

Model name Abbreviation

FANUC Series 30i-A 30i –A Series 30i FANUC Series 300i-A 300i–A Series 300i FANUC Series 300is-A 300is–A Series 300is FANUC Series 31i-A 31i –A FANUC Series 31i-A5 31i –A5 FANUC Series 310i-A 310i–A FANUC Series 310i-A5 310i–A5 FANUC Series 310is-A 310is–A FANUC Series 310is-A5 310is–A5 FANUC Series 32i-A 32i –A Series 32i FANUC Series 320i-A 320i–A Series 320i FANUC Series 320is-A 320is–A Series 320is

Series 31i

Series 310i

Series 310is

- 3 -

1.GENERAL GENERAL B-63944EN-2/04

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 2 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.

Related manuals of Series 30i/300i/300is- MODEL A Series 31i/310i/310is- MODEL A 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 OPERATOR’S MANUAL (Common to Lathe System/Machining Center System) B-63944EN OPERATOR’S MANUAL (For Lathe System) B-63944EN-1 OPERATOR’S MANUAL (For Machining Center System) B-63944EN-2 * MAINTENANCE MANUAL B-63945EN PARAMETER MANUAL B-63950EN

Programming

Macro Compiler / Macro Executor PROGRAMMING MANUAL B-63943EN-2 Macro Compiler OPERATOR’S MANUAL B-66264EN C Language Executor PROGRAMMING MANUAL B-63943EN-3

PMC

PMC PROGRAMMING MANUAL B-63983EN

Network

PROFIBUS-DP Board CONNECTION MANUAL B-63993EN Fast Ethernet / Fast Data Server OPERATOR’S MANUAL B-64014EN DeviceNet Board CONNECTION MANUAL B-64043EN FL-net Board CONNECTION MANUAL B-64163EN CC-Link Board CONNECTION MANUAL B-64463EN

Operation guidance function

MANUAL GUIDE i (Common to Lathe System/Machining Center System) OPERATOR’S MANUAL MANUAL GUIDE i (For Machining Center System) OPERATOR’S MANUAL MANUAL GUIDE i (Set-up Guidance Functions) OPERATOR’S MANUAL

B-63874EN

B-63874EN-2 B-63874EN-1

- 4 -

B-63944EN-2/04 GENERAL 1.GENERAL

Related manuals of SERVO MOTOR αi/βi series

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

Table 2 Related manuals

Manual name Specification number

FANUC AC SERVO MOTOR αi series DESCRIPTIONS FANUC AC SPINDLE MOTOR αi series DESCRIPTIONS FANUC AC SERVO MOTOR βi series DESCRIPTIONS FANUC AC SPINDLE MOTOR βi series DESCRIPTIONS FANUC SERVO AMPLIFIER αi series DESCRIPTIONS FANUC SERVO AMPLIFIER βi series DESCRIPTIONS FANUC SERVO MOTOR αis series FANUC SERVO MOTOR αi series FANUC AC SPINDLE MOTOR αi series FANUC SERVO AMPLIFIER αi series MAINTENANCE MANUAL FANUC SERVO MOTOR βis series FANUC AC SPINDLE MOTOR βi series FANUC SERVO AMPLIFIER βi series MAINTENANCE MANUAL FANUC AC SERVO MOTOR αi series FANUC AC SERVO MOTOR βi series FANUC LINEAR MOTOR LiS series FANUC SYNCHRONOUS BUILT-IN SERVO MOTOR DiS series PARAMETER MANUAL FANUC AC SPINDLE MOTOR αi/βi series, BUILT-IN SPINDLE MOTOR Bi series PARAMETER MANUAL

The above servo motors and the corresponding spindles can be connected to the CNC covered in this manual. In the αi SV series, they can be connected only to upgrade versions. In the βi SVSP series, they cannot be connected. This manual mainly assumes that the FANUC SERVO MOTOR αi series of servo motor is used. For servo motor and spindle information, refer to the manuals for the servo motor and spindle that are actually connected.

B-65262EN B-65272EN B-65302EN B-65312EN B-65282EN B-65322EN

B-65285EN

B-65325EN

B-65270EN

B-65280EN

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.

- 5 -

1.GENERAL GENERAL B-63944EN-2/04

1.2 NOTES ON VARIOUS KINDS OF DATA

CAUTION

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

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

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

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

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

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

create a copy of the various kinds of data beforehand.

- 6 -

II. PROGRAMMING

B-63944EN-2/04 PROGRAMMING 1.GENERAL

1 GENERAL

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

1.1 TOOL FIGURE AND TOOL MOTION BY PROGRAM ...................................................................9

1.1 TOOL FIGURE AND TOOL MOTION BY PROGRAM

Explanation

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

Usually, several tools are used for machining one workpiece. The tools have different tool length. It is very troublesome to change the program in accordance with the tools. Therefore, the length of each tool used should be measured in advance. By setting the difference between the length of the standard tool and the length of each tool in the CNC (See Chapter “Setting and Displaying Data” in OPERATOR’S MANUAL (Common to Lathe System / Machining Center System)), machining can be performed without altering the program even when the tool is changed. This function is called tool length compensation (See Section “Tool Length Compensation” in OPERATOR’S MANUAL (Common to Lathe System / Machining Center System)).

Standard

H1 H2

tool

Workpiece

H3 H4

- Machining using the side of cutter - Cutter compensation function

ath using cutter compensation

Cutter

Machined part figure

Workpiece

Tool

Because a cutter has a radius, the center of the cutter path goes around the workpiece with the cutter radius deviated. If radius of cutters are stored in the CNC (See Chapter “Setting and Displaying Data” in OPERATOR’S MANUAL (Common to Lathe System / Machining Center System)), the tool can be moved by cutter radius apart from the machining part figure. This function is called cutter compensation (See Section II-6 “Compensation Function”).

- 9 -

2. PREPARATORY FUNCTION (G FUNCTION)

PROGRAMMING B-63944EN-2/04

2 PREPARATORY FUNCTION

(G FUNCTION)

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

Type Meaning

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

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

Z_ ; G01 is effective in this range. X_ ;

G00 Z_ ; G00 is effective in this range.

X_ ;

G01 X_ ;

Explanation

1. When the clear state (bit 6 (CLR) of parameter No. 3402) is set at power-up or reset, the modal G

codes are placed in the states described below. (1) The modal G codes are placed in the states marked with (2) G20 and G21 remain unchanged when the clear state is set at power-up or reset. (3) Which status G22 or G23 at power on is set by bit 7 (G23) of parameter No. 3402. However,

G22 and G23 remain unchanged when the clear state is set at reset. (4) The user can select G00 or G01 by setting bit 0 (G01) of parameter No. 3402. (5) The user can select G90 or G91 by setting bit 3 (G91) of parameter No. 3402. When G code system B or C is used in the lathe system, setting bit 3 (G91) of parameter No.

3402 determines which code, either G90 or G91, is effective. (6) In the machining center system, the user can select G17, G18, or G19 by setting bits 1 (G18)

and 2 (G19) of parameter No. 3402.

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

as indicated in Table 2 (a).

- 10 -

2.PREPARATORY FUNCTION

B-63944EN-2/04 PROGRAMMING

Table 2 (a) G code list

G code Group Function

G00 Positioning (rapid traverse) G01 Linear interpolation (cutting feed) G02 Circular interpolation CW or helical interpolation CW G03 Circular interpolation CCW or helical interpolation CCW G02.1, G03.1 Circular thread cutting B CW/CCW G02.2, G03.2 Involute interpolation CW/CCW G02.3, G03.3 Exponential interpolation CW/CCW G02.4, G03.4 G04 Dwell

G05 G05.1 AI contour control / Nano smoothing / Smooth interpolation

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

3-dimensional coordinate system conversion CW/CCW

AI contour control (high-precision contour control compatible command), High-speed cycle machining, High-speed binary program operation

HRV3, 4 on/off

Programmable data input mode cancel

Polar coordinate interpolation cancel mode

Groove cutting by continuous circle motion (CCW)

Polar coordinates command

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

Zp: Z axis or its parallel axis

(G FUNCTION)

- 11 -

2. PREPARATORY FUNCTION (G FUNCTION)

PROGRAMMING B-63944EN-2/04

Table 2 (a) G code list

G code Group Function

G37 Automatic tool length measurement G38 Tool radius/tool nose radius compensation : preserve vector G39 G40 Tool radius/tool nose radius compensation : cancel

G41

G42 G41.2 3-dimensional cutter compensation : left (type 1)

G41.3 3-dimensional cutter compensation : leading edge offset G41.4 3-dimensional cutter compensation : left (type 1) (FS16i-compatible command) G41.5 3-dimensional cutter compensation : left (type 1) (FS16i-compatible command) G41.6 3-dimensional cutter compensation : left (type 2) G42.2 3-dimensional cutter compensation : right (type 1) G42.4 3-dimensional cutter compensation : right (type 1) (FS16i-compatible command) G42.5 3-dimensional cutter compensation : right (type 1) (FS16i-compatible command) G42.6 G40.1 Normal direction control cancel mode G41.1 Normal direction control on : left G42.1 G43 Tool length compensation + G44 Tool length compensation G43.1 Tool length compensation in tool axis direction G43.3 Nutating rotary head tool length compensation G43.4 Tool center point control (type 1) G43.5 G45 Tool offset : increase G46 Tool offset : decrease G47 Tool offset : double increase G48 G49 (G49.1) 08 Tool length compensation cancel G44.9 Spindle unit compensation G49.9 G50 Scaling cancel G51 G50.1 Programmable mirror image cancel G51.1 G50.2 Polygon turning cancel G51.2 G50.4 Cancel synchronous control G50.5 Cancel composite control G50.6 Cancel superimposed control G51.4 Start synchronous control G51.5 Start composite control G51.6 Start superimposed control G52 Local coordinate system setting G53 Machine coordinate system setting G53.1 Tool axis direction control G53.6

Tool radius/tool nose radius compensation : corner circular interpolation

3-dimensional cutter compensation : cancel Tool radius/tool nose radius compensation : left 3-dimensional cutter compensation : left Tool radius/tool nose radius compensation : right 3-dimensional cutter compensation : right

3-dimensional cutter compensation : right (type 2)

Normal direction control on : right

Tool center point control (type 2)

Tool offset : double decrease

Spindle unit compensation cancel

Scaling

Programmable mirror image

Polygon turning

Tool center point retention type tool axis direction control

- 12 -

2.PREPARATORY FUNCTION

B-63944EN-2/04 PROGRAMMING

Table 2 (a) G code list

G code Group Function

G54 (G54.1) Workpiece coordinate system 1 selection G55 Workpiece coordinate system 2 selection G56 Workpiece coordinate system 3 selection G57 Workpiece coordinate system 4 selection G58 Workpiece coordinate system 5 selection G59 G54.2 23 Rotary table dynamic fixture offset G54.4 33 Workpiece setting error compensation G60 00 Single direction positioning G61 Exact stop mode G62 Automatic corner override G63 Tapping mode G64 G65 00 Macro call G66 Macro modal call A G66.1 Macro modal call B G67 G68 Coordinate system rotation start or 3-dimensional coordinate conversion mode on G69 Coordinate system rotation cancel or 3-dimensional coordinate conversion mode off G68.2 Tilted working plane command G68.3 Tilted working plane command by tool axis direction G68.4 G70.7 Finishing cycle G71.7 Outer surface rough machining cycle G72.7 End rough machining cycle G73.7 Closed loop cutting cycle G74.7 End cutting off cycle G75.7 Outer or inner cutting off cycle G76.7 Multiple threading cycle G72.1 Figure copying (rotary copy) G72.2 G73 Peck drilling cycle G74 G75 01 Plunge grinding cycle G76 09 Fine boring cycle G77 Plunge direct sizing/grinding cycle G78 Continuous-feed surface grinding cycle G79

G80 09 G80.4 Electronic gear box: synchronization cancellation

G81.4 G80.5 Electronic gear box 2 pair: synchronization cancellation G81.5

G81 09 G81.1 00 Chopping

Workpiece coordinate system 6 selection

Cutting mode

Macro modal call A/B cancel

Tilted working plane command (incremental multi-command)

Figure copying (linear copy)

Left-handed tapping cycle

Intermittent-feed surface grinding cycle Canned cycle cancel Electronic gear box : synchronization cancellation

Electronic gear box: synchronization start

Electronic gear box 2 pair: synchronization start Drilling cycle or spot boring cycle Electronic gear box : synchronization start

(G FUNCTION)

- 13 -

2. PREPARATORY FUNCTION (G FUNCTION)

PROGRAMMING B-63944EN-2/04

Table 2 (a) G code list

G code Group Function

G82 Drilling cycle or counter boring cycle G83 Peck drilling cycle G84 Tapping cycle G84.2 Rigid tapping cycle (FS15 format) G84.3 Left-handed rigid tapping cycle (FS15 format) G85 Boring cycle G86 Boring cycle G87 Back boring cycle G88 Boring cycle G89 G90 Absolute programming G91 G91.1 Checking the maximum incremental amount specified G92 Setting for workpiece coordinate system or clamp at maximum spindle speed G92.1 G93 Inverse time feed G94 Feed per minute G95 G96 Constant surface speed control G97 G96.1 Spindle indexing execution (waiting for completion) G96.2 Spindle indexing execution (not waiting for completion) G96.3 Spindle indexing completion check G96.4 G98 Canned cycle : return to initial level G99 G107 00 Cylindrical interpolation G112 Polar coordinate interpolation mode G113 G160 In-feed control cancel G161

Boring cycle

Incremental programming

Workpiece coordinate system preset

Feed per revolution

Constant surface speed control cancel

SV speed control mode ON

Canned cycle : return to R point level

Polar coordinate interpolation mode cancel

In-feed control

- 14 -

B-63944EN-2/04 PROGRAMMING 3.INTERPOLATION FUNCTION

3 INTERPOLATION FUNCTION

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

3.1 INVOLUTE INTERPOLATION (G02.2, G03.2)...............................................................................15

3.2 THREADING (G33)...........................................................................................................................24

3.3 CIRCULAR THREAD CUTTING B (G2.1,G3.1).............................................................................25

3.4 GROOVE CUTTING BY CONTINUOUS CIRCLE MOTION (G12.4, G13.4)...............................28

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

- 15 -

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/04

Explanation

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

End point

Pe Po

Start point

Base circle

Clockwise involute interpolation (G02.2)

End point

Start point

End point

Counterclockwise involute interpolation (G03.2)

Start point

Ps Po

Fig. 3.1 (a) Actual movement

- Involute curve

An involute curve on the X-Y plane is defined as follows ; X (θ) = R [cos θ + (θ - θO) sin θ] + XO Y (θ) = R [sin θ - (θ - θO) cos θ] + YO where, XO, YO : Coordinates of the center of a base circle R : Base circle radius

θO : 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

- 16 -

B-63944EN-2/04 PROGRAMMING 3.INTERPOLATION FUNCTION

Start point

(Xo, Yo)

Involute curve

(X, Y)

End point

Base circle

Fig. 3.1 (b) Involute curve

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

- Start point and end point

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

- Base circle specification

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

- Choosing from two types of involute curves

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

- Feedrate

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

- Plane selection

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

- Cutter compensation

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

- 17 -

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/04

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

- Automatic speed control

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

- Specifiable G codes

The following G codes can be specified in involute interpolation mode: G04 : Dwell G10 : Programmable data input G17 : X-Y plane selection G18 : Z-X plane selection G19 : Y-Z plane selection G65 : Macro call G66 : Macro modal call G67 : Macro modal call cancel G90 : Absolute programming G91 : Incremental programming

- Modes that allow involute interpolation specification

Involute interpolation can be specified in the following G code modes: G41 : Cutter compensation left G42 : Cutter compensation right G51 : Scaling G51.1 : Programmable mirror image G68 : Coordinate rotation

- End point error

As shown below the end point may not be located on an involute curve that passes through the start point (Fig. 3.1 (c)). When an involute curve that passes through the start point deviates from the involute curve that passes through the end point by more than the value set in parameter No. 5610, alarm PS0243 is issued. If there is an end point error, the programmed feedrate changes by the amount of error.

End point

Path after correction

Deviation

Start point

Correct involute curve

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

- 18 -

B-63944EN-2/04 PROGRAMMING 3.INTERPOLATION FUNCTION

3.1.1 Automatic Speed Control for Involute Interpolation

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

• Override in cutter compensation mode

• Override in the vicinity of basic circle

- Override in cutter compensation mode

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

Cutting point

Rofs

Rcp

Base circle

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

Path specified in the program

Inward offset OVR = Rcp/(Rcp + Rofs) × 100 Outward offset OVR = Rcp/(Rcp - Rofs) × 100 where, Rcp : Radius of curvature at the center of the tool of the involute curve passing through the center of the tool Rofs : Radius of the cutter

- Clamping the override

The lower limit of override is specified in parameter No. 5620 so that the override for inward offset by cutter compensation or the override in the vicinity of the basic circle will not bring the speed of the tool center to zero in the vicinity of the basic circle. The lower limit of override (OVR1o) is specified in parameter No. 5620 so that the inward offset will not reduce the speed of the tool center to a very low level in the vicinity of the basic circle.

- 19 -

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/04

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:

onaccelerati epermissibl Maximum curvature of Radius level Clamp ×=

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.

- 20 -

B-63944EN-2/04 PROGRAMMING 3.INTERPOLATION FUNCTION

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

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

Format

Helical involute interpolation in Xp-Yp plane

G02.2 G17 Xp Yp I J R α β γ δ F ; G03.2

Helical involute interpolation in Zp-Xp plane

G02.2 G18 Zp Xp K I R α β γ δ F ; G03.2

Helical involute interpolation in Yp-Zp plane

G02.2 G19 Yp Zp J K R α β γ δ F ; G03.2

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

be specified.

- 21 -

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/04

3.1.3 Involute Interpolation on Linear Axis and Rotary Axis

(G02.2, G03.2)

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

Format

If the linear axis is the X-axis or an axis parallel to the X-axis, the plane is considered to be the Xp-Yp plane, and I and J are used.

G02.2 X

C I J R F ;

G03.2

If the linear axis is the Y-axis or an axis parallel to the Y-axis, the plane is considered to be the Yp-Zp plane, and J and K are used.

G02.2 Y

C J K R F ;

G03.2

If the linear axis is the Z-axis or an axis parallel to the Z-axis, the plane is considered to be the Zp-Xp plane, and K and I are used.

G02.2 Z C K I R F ; G03.2

G02.2 : Clockwise involute interpolation G03.2 : Counterclockwise involute interpolation Example) If the linear axis is the X-axis X, C : End point of the involute curve I, J : Center of the basic circle of the involute curve, viewed from the start point R : Radius of basic circle F : Cutting feedrate

- 22 -

B-63944EN-2/04 PROGRAMMING 3.INTERPOLATION FUNCTION

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 ; Positioning to the start point N200 G12.1 ; Polar coordinate interpolation started N201 G41 G00 X-1.0 ; N202 G01 Z-2.0 F

; N203 G02.2 X1.0 C9.425 I1.0 J0 R1.0 ; Involute interpolation during polar coordinate interpolation N204 G01 Z0 ; N205 G40 G00 X15.0 C0 ; N206 G13.1 ; Polar coordinate interpolation cancelled N300 Z ; N400 X

C ;

: :

M30 ;

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.

- 23 -

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/04

- Mode that does not allow involute interpolation specification

Involute interpolation cannot be used in the following mode: G07.1: Cylindrical interpolation

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 command increment Command value range of the lead

Metric input

Inch input

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

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)

- 24 -

B-63944EN-2/04 PROGRAMMING 3.INTERPOLATION FUNCTION

NOTE

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;

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

Overview

Circular thread cutting B can perform circular interpolation on two axes and, at the same time, can perform linear interpolation between the major axis of the two axes subject to circular interpolation, which has a longer traveling distance, and up to two other, arbitrary axes. This circular thread cutting function does not move the tool in synchronization with the rotation of the spindle (workpiece) using the spindle motor, but controls the rotation of the workpiece using a servo motor (rotation axis) to perform threading at equal pitches along cylindrical material, grooving, tool grinding, and other machining.

Application example

For example, the grooving shown in Fig. 3.3 (a) can be performed by executing circular interpolation on the ZpXp plane in synchronization with linear interpolation on the Z-axis and the C-axis.

X axis

Z axis

C axis

Fig. 3.3 (a) Example of grooving

- 25 -

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/04

Format

Xp-Yp plane

G17

G02.1 G03.1

α β

;

Zp-Xp plane

G18

G02.1 G03.1

α β

K R

;

Yp-Zp plane

G19

G02.1 G03.1

α β

G02.1: Clockwise circular thread cutting B command

G03.1: Counterclockwise circular thread cutting B command

X,Y,Z: Coordinates of the end point for circular interpolation

α,β: Coordinates of the end point for linear interpolation

I,J,K: Signed distance from the start point to the center of an arc

R: Arc radius

F: Feedrate in the major axis direction

α and β are arbitrary axes other than the circular interpolation axis. Up to two such axes

can be specified.

X, Y, Z, I, J, K, and R are the same as those for G02 and G03.

In the case of the ZpXp plane, the major axis being the Z-axis, the minor axis being the X-axis, the arbitrary axis being the C-axis, and clockwise direction G91 G18 G02.1 Z_ C_ I_ K_ F_ R_

J R

;

X axis

Start point

Fig. 3.3 (b)

rc cente

End point (X,Z)

C axis

Z axis

Explanation

- 26 -

B-63944EN-2/04 PROGRAMMING 3.INTERPOLATION FUNCTION

- Relationship between major axis and minor axis

The relationship between the major axis and minor axis is as shown in Fig. 3.3 (c).

End point

ΔX

45° 45°

Center

Start

oint

If |ΔX| > |ΔY|,

ΔY

the major axis is the X-axis, and the minor axis is the Y-axis.

If |ΔX| < |ΔY|, the major axis is the Y-axis, and the minor axis is the X-axis.

Fig. 3.3 (c)

When diameter programming is used, the relationship between the major axis and minor axis is judged with the radius value.

- Permissible arc range

If the arc goes beyond the range shown in Fig. 3.3 (d) or Fig. 3.3 (e), alarm PS2070 is issued.

Minor axis

Major axis

90°

45° 45°

45°45°

Fig. 3.3 (d)

90°

45°

45° to 135°

225° to 315°

0°

Rotation axis

Range in which interpolation is enabled

0°

Minor axis

45°45°

Fig. 3.3 (e)

Rotation axis

315° to 45° 135° to 225°

Range in which interpolation is enabled

- Feedrate

If the specified feedrate for the major axis is F, the feedrate for the minor axis Fs and feedrate for the α axis Fα are expressed as follows.

Length of α axis

Fα = F × (The maximum value is the maximum cutting feedrate for each axis.)

Length of major axis

Fs = F × TAN θ

θ: Angle of a tangent to the major axis

- 27 -

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/04

End

Minor axis

Start point

Major axis

Fig. 3.3 (f)

point

Center

- Tool radius compensation

Tool radius compensation applies only to two axes of the plane on which circular interpolation is performed.

Limitation

- Tool offset and tool length compensation

In a block in which circular thread cutting B is specified, tool offset or tool length compensation cannot be specified.

- I,J,K and the R command

Either I,J,K or the R command cannot be omitted.

- Unavailable functions

Circular thread cutting B cannot be used together with the following functions:

• 3-dimensional cutter compensation

• Tool center point control

3.4 GROOVE CUTTING BY CONTINUOUS CIRCLE MOTION

(G12.4, G13.4)

Overview

Groove cutting with a width greater than the tool diameter can be performed by causing the tool to make continuous circle motion independently of axis movement by the groove cutting path program and superposing the continuous circle motion on the axis movement by the groove cutting path program.

Continuous circle motion

Groove cutting path specification route

Fig. 3.4 (a)

- 28 -

B-63944EN-2/04 PROGRAMMING 3.INTERPOLATION FUNCTION

Format

G12.4 P1Ii Kk Qq Ff; (Mode on) G13.4 : : (Groove cutting path program) : G12.4 P0; (Mode cancel) G13.4

G12.4 : Clockwise continuous circle motion G13.4 : Counterclockwise continuous circle motion i : Groove width k : Tool diameter q : Travel distance in the groove cutting direction per continuous circle motion (pitch) f : Feedrate (speed of the center of a tool that performs continuous circle motion)

Groove cutting path program

i (Groove width)

k (Tool diameter)

q (pitch)

Fig. 3.4 (b)

NOTE

1 In the G12.4/G13.4 blocks, addresses other than the commands mentioned

above cannot be used. 2 If bit 4 (GCC) of parameter No. 3452 is 0, continuous circle motion stops due to

the stoppage of axis movement by the groove cutting path program, but because

axis movement by the groove cutting path program is independent of continuous

circle motion, the stoppage will not exactly be at the position of continuous circle

motion converted from the groove cutting path program and the pitch.

Explanation

- Mode on

The continuous circle motion-based groove cutting mode sets continuous circle motion-based groove cutting mode to the on state. The continuous circle motion-based groove cutting enable signal must be "1".

- 29 -

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/04

If the mode on command is specified with the continuous circle motion-based groove cutting enable signal being "0", alarm PS0010 is issued. No axis movement is performed with the continuous circle motion-based groove cutting mode on command.

- Mode cancel

The continuous circle motion-based groove cutting mode cancel command causes the tool to move with cutting feed (continuous circle motion speed) from the present position on the continuous circle to the end-specified position (groove center) of the groove cutting path program. After the end of movement, the command sets continuous circle motion-based groove cutting mode to the cancel state.

- Startup

In the first move command block of the groove cutting path program, the tool moves to a point on the continuous circle with cutting feed (continuous circle motion speed). After the end of the movement to a point on the continuous circle, continuous circle motion is started in synchronization with the move command of the groove cutting path program.

Depending on the first move command block of the groove cutting path program, the direction of startup varies.

• In the case of an axis command perpendicular to a plane or if there is no movement along an axis used to form the currently selected plane Assuming that R = (I-K)/2, the following holds true: (X,Y) = (-R,0)

Startup

Groove cutting path command

Ｚ

• If there is movement along an axis used to form the selected plane Direction opposite to the direction of movement projected onto the currently selected plane

Groove cutting path command

End

Startup

Start point

point

- Increments systems for horizontal w i dth, tool diameter, and pitch

The increment systems for i (horizontal width), K (tool diameter), and q (pitch) follow the incremental system of the reference axis (parameter No. 1031).

- Feedrate

For the feedrate F, specify the central speed of the tool that performs continuous circle motion. The speed on the groove cutting path is:

Speed on the groove cutting path = F × Q / π (I-K)

- Pitch

If the pitch is large, there may be portions left uncut. The tool diameter must be greater than the pitch.

- 30 -

B-63944EN-2/04 PROGRAMMING 3.INTERPOLATION FUNCTION

- Groove cutting path program

The groove cutting path program specifies the path of the center of continuous circle motion.

(1) Effective commands The groove cutting path program can execute only the G01, G02, G03, G04, G90, G91, and

auxiliary functions. The G00 command causes alarm PS5256. By setting bit 0 (GG0) of parameter No. 3452, however, the G00 command can be moved as G01 movement. The modal code changes from G00 to G01.

(2) Specifying a controlled axis The groove cutting path program can specify the control axes below.

• Commands for the axes forming a plane

• Commands for axes perpendicular to a plane (independent command for the Z-axis)

• Commands for linear axes other than the axes forming a plane

• Commands for rotation axes

(3) Specification of a pitch in a move command block In addition to the specification of a pitch with the continuous circle motion-based groove cutting

mode on command, a pitch can be specified in each move command block. The pitch specification is modal; the pitch last specified is effective from the time the mode is entered with G12.4P1/G13.4P1 until the mode is exited.

(4) Command example

(Example 1) Example of a command for an axis perpendicular to a plane

(independent command for the Z-axis) : G12.4 P1 Ii Kk Ff ; G01 Z--- Q--- ; Specify the pitch for the Z-axis (pitch of this block). X--- Y--- Q--- ; Specify the pitch for the X- and Y-axes (pitch of the

subsequent blocks)

For a command for the Z-axis only, the pitch is regarded as the travel distance in the Z-axis direction.

(Example 2) If a move command for other than a plane is included : G12.4P1 Ii Kk Ff ; G01 X--- Y--- Z--- Q--- ; This is a pitch on a slanted path. : The pitch is the travel distance in the synthetic direction of the X-, Y-, and

Z-axes.

(Example 3) Pitch switching : G12.4P1 Ii Kk Ff ; G01 X--- Y--- Q--- ; X--- Y--- Q--- ; Specify Q in the block in which the pitch is to be changed. :

The pitch is the travel distance in the synthetic direction of the specified axes.

- 31 -

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/04

(Example 4) Command containing a rotation axis : G12.4P1 Ii Kk Ff ; G01 Ａ--- Q--- ;

X--- Y--- ; Specify Q in the block in which the pitch is to be changed. : The increment system for Q follows that of the reference axis. Thus, if the

increment system for the reference axis is IS-B, the pitch Q100 will be 0.1°.

So that a cut along the Z-axis will start after the stabilization of the radius of continuous circle motion, the continuous circle motion-based groove cutting mode on command must be specified in the air, apart from the cut position by at least the pitch per rotation. Cutting with a constant groove width is possible by letting the tool escape in the Z-axis direction at the end of cutting while keeping continuous circle motion and then after the tool comes out into the air, executing the continuous circle motion-based groove cutting mode cancel command to stop continuous circle motion.

NOTE

The radius of continuous circle motion is smaller than that specified at the start

of continuous circle motion, and is larger when continuous circle motion comes to a deceleration stop. In the steady state, the radius is smaller than that specified. This is an error that occurs due to acceleration/deceleration after information and the delay of the servo system.

Error that occurs due to acceleration/deceleration after interpolation and the delay of the servo system

Specified

ctual path

- Mode in progress signal

This signal notifies the PMC that continuous circle motion-based groove cutting mode is in progress. The signal is set to "1" if continuous circle motion-based groove cutting mode is turned on. The signal is set to "0" if continuous circle motion-based groove cutting mode is canceled.

- Clamping the feedrate with the acceleration of continuous circle motion

Using the I and K commands in G12.4/13.4 and the acceleration clamp value for continuous circle motion (parameter No. 3490), the feedrate command F for continuous circle motion can be clamped.

Clamp feedrate F = SQR (parameter No.3490 × (I-K) / 2)× 60

Example If parameter No. 3490 = 100 If G13.4 P1 I10.0 K5.0 Q1.0 F1000 ;, clamp feedrate = 948. Thus, execution with

an F value of 948

If G13.4 P1 I10.0 K8.0 Q1.0 F1000 ;, clamp feedrate = 600. Thus, execution with

an F value of 600

If G13.4 P1 I10.0 K9.0 Q1.0 F1000 ;, clamp feedrate = 424. Thus, execution with

an F value of 424

A continuous circle motion feedrate override is applied to the clamped feedrate.

- 32 -

B-63944EN-2/04 PROGRAMMING 3.INTERPOLATION FUNCTION

- Acceleration deceleration after interpolation

In continuous circle motion-based groove cutting mode, acceleration/deceleration after interpolation is enabled.

- Selecting stoppage conditions

(1) Stoppage of continuous circle motion due to a feed hold, single block, etc. It can be selected whether to continue or stop continuous circle motion when a specified operation is

stopped due to one of the various stoppage conditions such as a feed hold and a single block, using a parameter:

Bit 4 (GCC) of parameter No. 3452 = 0 : Stops continuous circle motion. Bit 4 (GCC) of parameter No. 3452 = 1 : Continues continuous circle motion.

(2) Stoppage condition/mode switching The conditions for groove cutting path operation, continuous circle motion stoppage/continuation,

and switching to operation mode in connection with stoppage conditions are as given in Table 3.4 (a).

Table 3.4 (a)

Continuous circle motion

Stoppage condition

Feed hold Deceleration stop Deceleration stop Continuation Possible after the stoppage

Single block Deceleration stop Deceleration stop Continuation Possible after the stoppage

Switching to manual mode Switching between auto modes MDI operation Deceleration stop Deceleration stop Continuation Possible after the stoppage

Pitch override of 0% Deceleration stop Deceleration stop Continuation Possible after the stoppage

M/S/T code FIN awaiting Programming error Deceleration stop Decelerati on stop Continuation Possible after the stoppage

Overheat alarm Deceleration stop Deceleration stop Continuation Possible after the stoppage

BG edit alarm Continuation Continuation Continuation Automatic operation does

Mode end Deceleration stop Withdrawal by the

Reset Deceleration stop Deceleration stop Deceleration stop Possible after the end of all

Machine lock *1 Deceleration stop Deceleration stop Deceleration stop Servo off *1 Deceleration stop Deceleration stop Deceleration stop Interlock *2 Deceleration stop Deceleration stop Deceleration stop OT alarm Deceleration stop Deceleration stop Deceleration stop Possible after the end of all

DS alarm Deceleration stop Deceleration stop Deceleration stop Possible after the end of all

Groove cutting

path operation

Deceleration stop Deceleration stop Continuation To be performed after the

Deceleration stop Deceleration stop Continuation Possible after the stoppage

stoppage/continuation Stoppage (GCC = 0)

radius/ deceleration stop

Continuation

(GCC = 1)

Withdrawal by the radius/ deceleration stop

Switching to operation

mode

of path operation

stoppage of path operation

of path operation

not stop. Follows other stoppage conditions.

operations

――― ――― ―――

operations

- 33 -

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/04

Continuous circle motion

Stoppage condition

Emergency stop Immediate stop Immediate stop Immediate stop Possible after an

PC-related alarm Immediate stop Immediate stop Immediate stop Possible after an alarm is

Servo alarm Immediate stop Immediate stop Immediate stop Possible after an alarm is

Spindle alarm Immediate stop Immediate stop Immediate stop Possible after an alarm is

System alarm Immediate stop Immediate stop Immediate stop The power must be turned

Groove cutting

path operation

stoppage/continuation Stoppage (GCC = 0)

Continuation

(GCC = 1)

Switching to operation

mode

emergency stop is canceled

canceled

off and then back on.

*1: Stoppage occurs only on the axis on which the function is enabled. *2: Stoppage occurs on all axes if the function is enabled on at least one axis.

• If bit 4 (GCC) of parameter No. 3452 is 0, continuous circle motion stops due to the stoppage of axis movement by the groove cutting path program, but because axis movement by the groove cutting path program is independent of continuous circle motion, the stoppage will not exactly be at the position of continuous circle motion converted from the groove cutting path program and the pitch.

• After the mode is switched to manual mode, the axes on which manual movement is possible do not include the axes on which to perform continuous circle motion.

• If continuous circle motion is to continue (bit 4 (GCC) of parameter No. 3452 = 1), there will be no fluctuations in radius because continuous circle motion continues.

• Movement to the continuous circle motion start position and movement to the groove cutting path program end position after the end of continuous circle motion will stop under the stoppage conditions below.

Reset Deceleration stop Machine lock Deceleration stop Servo off Deceleration stop Interlock Deceleration stop OT alarm Deceleration stop DS alarm Deceleration stop Emergency stop Immediate stop PC-related alarm Immediate stop Servo alarm Immediate stop Spindle alarm Immediate stop System alarm Immediate stop

- Feedrate specification and pitch override

(1) Feedrate specification For the feedrate during cutting, specify the feedrate for continuous circle motion.

This feedrate is displayed as a specified feedrate.

(2) Continuous circle motion feedrate override The feedrate override signals (*FV0 to *FV7) are not effective to the specified feedrate for

continuous circle motion. Use the continuous circle motion feedrate override signals (*CGROV7 to *CBROV0). If the continuous circle motion feedrate override is at 0%, continuous circle motion can be stopped independently of the movement on the groove cutting path.

- 34 -

B-63944EN-2/04 PROGRAMMING 3.INTERPOLATION FUNCTION

(3) Feedrate override The feedrate on the groove cutting path is determined with the pitch command. The feedrate

override signals (*FV0 to *FV7) are effective to the feedrate on the groove cutting path. This makes it possible to change the feedrate for continuous circle motion independently of the feedrate on the groove cutting path. Also, the override cancel signal (OVC) and the second feedrate override signal (optional function) are effective to the feedrate on the groove cutting path.

(4) Dry run The feedrate during a dry run is as given in Table 3.4 (b).

A dry run is not effective to the feedrate on the groove cutting path.

Table 3.4 (c)

Feedrate Override

Feedrate on the groove

cutting path

Feedrate for continuous

circle motion

Feedrate F for continuous circle motion ×

pitch / 2πR

Dry run rate

(Parameter No.1410)

Feedrate override

Manual rapid traverse selection signal (RT)

0 1

JV JVmax

JV : Manual feedrate override Jvmax : Maximum manual feedrate override

(5) Feedrate display

• Specified feedrate display shows the specified speed for continuous circle motion.

• Actual cutting feedrate display show the sy nthetic one from the feedrate for continuous circle

motion and the feedrate on the groove cutting path.

(6) Clamping with the maximum cutting feedrate If the specification of the feedrate for continuous circle motion exceeds the maximum cutting

feedrate (parameter No. 1430), the specification of the feedrate for continuous circle motion is clamped to calculate the feedrate on the groove cutting path. In addition, the feedrate for continuous circle motion and the feedrate on the groove cutting path, to which their respective overrides have been applied, are clamped with the maximum cutting feedrate.

Limitation

- Mirror image

A mirror image is effective to groove cutting path commands only. No mirror image is applied to continuous circle motion, movement to the continuous circle motion start position, and movement to the groove cutting path program end position after the end of continuous circle motion.

- Distance to go

- Workpiece coordinate system and machine coordinate system

Movement to the continuous circle motion start position, movement of continuous circle motion, and movement to the groove cutting path program end position after the end of continuous circle motion are not reflected in the workpiece coordinate system. The workpiece coordinate system is the coordinate system of the groove cutting path program. Note, however, that these movements are reflected in the machine coordinate system.

- 35 -

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/04

- Axis moving signal

The axis moving signal does not change due to axis moving due to continuous circle motion. Use the continuous circle motion-based groove cutting mode in progress signal.

- Graphic display

The tool path of the program during cutting is in the workpiece coordinate system and, therefore, the groove cutting command path is drawn.

- Restart functions

The restart functions, such as program restart and tool retract and recover, cannot be used to start continuous circle motion-based groove cutting in the middle of the groove cutting path program.

- Retrace

Retrace cannot be used in continuous circle motion-based groove cutting mode.

- AI contour control

In continuous circle motion-based groove cutting mode, AI contour control is disabled. If continuous circle motion-based groove cutting is specified during AI contour control, AI contour control is temporarily canceled. If continuous circle motion-based groove cutting mode is canceled, AI contour control returns to on. Note that if AI contour control is disabled, acceleration/deceleration before look-ahead interpolation, acceleration control, and optimum torque acceleration/deceleration are also disabled.

- One-digit F code

The one-digit F code cannot be used in continuous circle motion-based groove cutting mode.

- Interruption type custom macro

The interruption type custom macro cannot be used in continuous circle motion-based groove cutting mode.

- Commands that can be executed in continuous circle motion-based groove cutting mode

The groove cutting path program can executed the following commands only:

• G01

• G02, G03 (except helical interpolation and helical interpolation B)

• G04

• G90, G91

• M/S/T (auxiliary function), Second auxiliary function

• G00 (An operation can be selected with bit 0 (GG0) of parameter No. 3452.

GG0 = 0: Alarm PS5256 is issued. GG0 = 1: The G00 command is moved as G01 operation.)

• G94 (Feed per minute)

- Modes in which the continuous circle motion-based groove cutting mode command cannot be specified

The continuous circle motion-based groove cutting command cannot be executed in the function modes below. Interpolation function

• Helical interpolation

• Helical interpolation B

• Conical interpolation / spiral interpolation

• Polar coordinate interpolation

• Cylindrical interpolation / Cutting point interpolation for cylindrical interpolation

- 36 -

B-63944EN-2/04 PROGRAMMING 3.INTERPOLATION FUNCTION

• Exponential interpolation

• Smooth interpolation

• Nano smoothing

• NURBS interpolation

• Hypothetical axis interpolation

• Variable lead thread cutting

• Circular thread cutting

• 3-dimensional circular interpolation

• Involute interpolation

• Thread cutting

Feed function

• One-digit F code feed / feed per revolution / inverse time feed

• Exact stop / Tapping mode / automatic corner override

Coordinate value and dimension

• Polar coordinate command

Function to simplify programming

• Figure copying

• 3-dimensional coordinate system conversion

• Canned cycle for drilling

• Rigid tapping

• Index table indexing

Compensation function

• Scaling

• Programmable mirror image

• Tool offset

• Tool radius compensation

• Tool nose radius compensation／vector retention／corner circular interpolation

• 3-dimensional tool compensation

• Coordinate system rotation

Axis control function

• Polygon turning

• Arbitrary angular axis control

5-axis machining function

• Tool center point control for 5-axis machining

• Tilted working plane command

• Inclined Rotary Axis Control

• 3-dimensional cutter compensation

Multi-path control function

• Inter-path waiting / Path spindle control

• Synchronous/Composite/Superimposed control

Example

If the following program is executed, the center of the tool moves as shown in

the figure below.

(This program is merely a sample. The Q and F commands must be determined

according to the cutting conditions.)

O0002 ; N01 G90 G0 X0 Y0 Z0 ; N02 G91 G00 X20.0 Y20.0 ; N03 G01 Z-25.0 F5000 ; N04 G13.4 P1 I20.0 K10.0 Q5.0 F3000 ;

- 37 -

3.INTERPOLATION FUNCTION PROGRAMMING B-63944EN-2/04 N05 Y40.0 ;

N06 X40.0 Y20.0 ; N07 G02 X40.0 Y-40.0 R40.0 ; N08 X-20.0 Y-20.0 R20.0 ; N09 G01 X-60. ; N10 G13.4 P0 ; N11 G00 Z25.0 ; N12 X-20.0 Y-20.0 M02 ; %

- 38 -

4.COORDINATE VALUE AND

)

B-63944EN-2/04 PROGRAMMING

DIMENSION

4 COORDINATE VALUE AND DIMENSION

Chapter 4, "COORDINATE VALUE AND DIMENSION", consists of the following sections:

4.1 POLAR COORDINATE COMMAND (G15, G16)...........................................................................39

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

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

- 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.

olar coordinate mode

Command position

Radius

ngle

ctual position

Command position

Radius

ngle

ctual position

When the angle is specified with an absolute command

When the angle is specified with an incremental command

- 39 -

4. COORDINATE VALUE AND

DIMENSION

PROGRAMMING B-63944EN-2/04

- 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

ngle

Radius

Command position

ngle

ctual position

When the angle is specified with an absolute command

When the angle is specified with an incremental command

ctual position

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

- Specifying angles and a radius w i th 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 w i th 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.

- 40 -

4.COORDINATE VALUE AND

B-63944EN-2/04 PROGRAMMING

DIMENSION

- 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)

- Optional chamfering and corner R

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

- 41 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

5 FUNCTIONS TO SIMPLIFY PROGRAMMING

Chapter 5, "FUNCTIONS TO SIMPLIFY PROGRAMMING", consists of the following sections:

5.1 CANNED CYCLE FOR DRILLING .................................................................................................42

5.2 RIGID TAPPING................................................................................................................................74

5.3 OPTIONAL CHAMFERING AND CORNER R ...............................................................................88

5.4 INDEX TABLE INDEXING FUNCTION.........................................................................................91

5.5 IN-FEED CONTROL (FOR GRINDING MACHINE)......................................................................93

5.6 CANNED GRINDING CYCLE (FOR GRINDING MACHINE)......................................................95

5.7 MULTIPLE REPETITIVE CYCLE (G70.7, G71.7, G72.7, G73.7, G74.7, G75.7,G76.7)..............109

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

G code

G73 Intermittent feed - Rapid traverse High-speed peck drilling cycle G74 Feed Dwell → Spindle CW Feed Left-hand tapping cycle G76 Feed Spindle orientation Rapid traverse F ine boring cycle G80 - - - Cancel

G81 Feed - Rapid traverse

G82 Feed Dwell Rapid traverse G83 Intermittent feed - Rapid traverse Peck drilling cycle

G84 Feed Dwell → Spindle CCW Feed Tapping cycle G85 Feed - Feed Boring cycle G86 Feed Spindle stop Rapid traverse Boring cycle G87 Feed Spindle CW Rapid traverse Back boring cycle G88 Feed Dwell → Spindle stop Manual Boring cycle G89 Feed Dwell Feed Boring cycle

Drilling

(-Z direction)

Explanation

A canned cycle for drilling consists of a sequence of six operations. Operation 1 Positioning of axes X and Y (including also another axis) Operation 2 Rapid traverse up to point R level Operation 3 Hole machining Operation 4 Operation at the bottom of a hole Operation 5 Retraction to point R level Operation 6 Rapid traverse up to the initial point

Operation at the bottom of a hole

Retraction

(+Z direction)

Application

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

- 42 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

PROGRAMMING

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

- Positioning plane

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

- 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

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.

- 43 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

CAUTION

Switch the drilling axis after canceling a canned cycle for drilling.

NOTE

A bit 0 (FXY) of parameter No. 5101 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 Fig. 5.1 (b):

G90 (Absolute programming) G91 (Incremental programming)

Point R

Point Z

Fig. 5.1 (b) Absolute programming and incremental programming

Z = 0

Point R

Point Z

- Drilling mode

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.

- 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 operations performed when G98 and G99 are specified are shown in Fig. 5.1 (c). 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

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

- 44 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

PROGRAMMING

- Repeat

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.

- Single block

If a drilling cycle is performed in a single block, the control unit stops at each of the end points of operations 1, 2, and 6 in Fig. 5.1 (a). This means that three starts are made to make a single hole. At the end points of operations 1 and 2, the feed hold lamp turns on and the control unit stops. If the repetitive count is not exhausted at the end point of operation 6, the control unit stops in the feed hold mode, and otherwise, stops in the single block stop mode. Note that G87 does not cause a stop at point R in G87. G88 causes a stop at point Z after a dwell.

- Cancel

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)

- 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

OSS

P Dwell

Oriented spindle stop (The spindle stops at a fixed rotation position) Shift (rapid traverse G00)

- 45 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

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

Point R

Point Z

Point R

Point R level

Point Z

Explanation

- Operations

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.

- Spindle rotation

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

- 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.

- 46 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

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.

- 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.

- 47 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

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

Spindle CCW

Point R level

Point R

Spindle CCW

Point R

Point Z

Spindle CW

Point Z

Spindle CW

Explanation

- Operations

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.

- Spindle rotation

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, 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.

- 48 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

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.

- 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.

- 49 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

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

Tool

Shift amount q

Spindle CW

Point R

OSS

Initial level

Point Z

Point R

OSS

Spindle CW

Point R level

Point Z

Explanation

- Operations

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.

- Spindle rotation

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

- Auxiliary function

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.

- 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.

- 50 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

PROGRAMMING

- 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.

- 51 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

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

Point R

Point Z

Point R

Point R level

Point Z

Explanation

- Operations

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.

- Spindle rotation

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

- Auxiliary function

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.

- 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.

- 52 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

PROGRAMMING

- 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.

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

Point R

Point R level

Point Z

Explanation

- Operations

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.

- 53 -

Point Z

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

When the bottom of the hole has been reached, a dwell is performed. The tool is then retracted in rapid traverse.

- Spindle rotation

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

- Auxiliary function

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.

- 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.

- 54 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

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

Point R

Point Z

Point R

Point R level

Point Z

Explanation

- Operations

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.

- Spindle rotation

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

- Auxiliary function

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.

- 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.

- 55 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

- 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. Q1000000000000005. 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.

- 56 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

PROGRAMMING

5.1.7 Small-Hole Peck Drilling Cycle (G83)

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 Nos. 5172 and 5173 are assumed as

defaults.) K_ : Number of times the operation is repeated (if required) P_ : Dwell time at the bottom of the hole (If this is omitted, P0 is assumed as the default.)

G83 (G98) G83 (G99)

Initial level

Point R

Overload torque

Dwell

Δ: 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

()

Point Z

Overload tor

Point R level

Point Z

Dwell

Explanations

- Component operations of the cycle

* X- and Y-axis positioning * Positioning at point R along the Z-axis

- 57 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

* Cutting along the Z-axis (first time, depth of cut Q, incremental)

Retracting (bottom of hole → minimum clearance ∆, incremental) Retraction (bottom of hole +Δ → 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 mode, the small-diameter peck drilling cycle in progress signal is set to "1" at the start of point R positioning on the axis in the drilling direction after G83 is specified and positioning is performed to the specified hold position. This signal is set to "0" if another canned cycle is specified or if this mode is canceled with G80, a reset, or an emergency stop. 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 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 Δ 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 Nos.5166 and 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.

- 58 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

Cutting feedrate = F × α

<First drilling> α=1.0

α=α×β÷100, where β is the rate of change for each drilling operation When the skip signal is detected during the previous drilling operation: β=b1% (parameter No.5166) When the skip signal is not detected during the previous drilling operation: 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

γ=γ×δ÷100, where δ is the rate of change for each drilling operation 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.

PROGRAMMING

- 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 address 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 parameter 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.

- Functions 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

- 59 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

• 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 Δ.)

• 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)

- 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 Nos.5170 and 5171. Parameters Nos.5170 and 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 retraction output to common variables are cleared by G83 while

small-hole peck drilling 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.

- 60 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

PROGRAMMING

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

Spindle CW P

Point R level

Point ZP

Spindle CCW

Point R

Spindle CW

Point ZP

Spindle CCW

Point R

Explanation

- Operations

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.

- Spindle rotation

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, 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.

- 61 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

- 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.

- 62 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

PROGRAMMING

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

Point R

Point Z

Point R

Point R level

Point Z

Explanation

- Operations

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.

- Spindle rotation

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

- Auxiliary function

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.

- 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 G85 in a single block. Otherwise, G85 will be canceled.

- 63 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

- 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.

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

Point R

Point Z

Spindle stop

Point R

Point R level

Point Z

Spindle stop

Explanation

- Operations

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.

- Spindle rotation

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.

- 64 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

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.

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 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

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

Tool

Shift amount q

OSS

Spindle CW

OSS

Spindle CW

Initial level

Not used

Point Z

Point R

Explanation

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.

- Spindle rotation

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.

- 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.

- 66 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

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 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.

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.

- 67 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

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

Point R

Point Z

Spindle stop after dwell

Point R

Point Z

Point R level

Spindle stop after dwell

Explanation

- Operations

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.

- Spindle rotation

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

- 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.

- 68 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

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.

- 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.

- 69 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

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

Point R

Point Z

Point R

Point R level

Point Z

Explanation

- Operations

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

- Spindle rotation

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

- Auxiliary function

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.

- 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.

- 70 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

PROGRAMMING

- 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 at the bottom of the hole

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.

- 71 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

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

- 72 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

Program using tool length offset and canned cycles

Reference position

350

PROGRAMMING

#1 #11

100

100 100

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

- 73 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

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.

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 (if required)

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

L_ : Number of repeats (if required)

G84 (G98) G84 (G99)

Spindle stop

Initial level

Operation 1

Operation 2

Spindle CW

Point R

Operation 3

Spindle stop Spindle CCW

Operation 4

Operation 6 P

Spindle stop

Point R level

Operation 5

Point Z

Spindle CW

Spindle stop Spindle CCW

Spindle stop

Point R

Spindle stop

Point R level

Point Z

- 74 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

PROGRAMMING

Explanation

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.

- 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 (bit 0 (G84) of parameter No. 5200 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.

- 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.

- 75 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

- 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 diagnosis data 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.

- Unit of F command

Metric input Inch input Remarks

G94 1 mm/min 0.01 inch/min Decimal point programming allowed G95 0.01 mm/rev 0.0001 inch/rev 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.

- 76 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

PROGRAMMING

- Cancel

Do not specify a G code of the 01 group (G00 to G03 or G60 (when the bit 0 (MDL) of parameter No. 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 <Programming of feed per revolution> 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

- 77 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

5.2.2 Left-Handed Rigid Tapping Cycle (G74)

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

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 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 return is made. F_ : Cutting feedrate K_ : Number of repeats (if required)

G84.3 X_ Y_ Z_ R_ P_ F_ L_ ;

(Series 15 format)

L_ : Number of repeats (if required)

G74 (G98) G74 (G99)

Spindle stop

Initial level

Operation 1

Operation 2

Spindle CCW

Point R

Operation 3

Spindle stop Spindle CW

Operation 4

Operation 6

Point R level

Operation 5

Point Z

Spindle stop

Spindle CCW

Spindle stop

Point R

Spindle stop

Point R level

Point Z

Spindle CW

Explanation

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 normal 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.

- 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 G74 for rigid tapping. (bit 0 (G84) of parameter No. 5200 set to1).

- 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.

- 78 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

PROGRAMMING

- 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

- 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

- 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.

- Reset

- 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.

- 79 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

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

• Specifying a rotation speed exceeding the maximum speed for the gear used causes alarm PS0200.

• 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 diagnosis data No. 451):

- F command

Specifying a value that exceeds the upper limit of cutting feedrate causes alarm PS0011.

- Unit of F command

Metric input Inch input Remarks

G94 1 mm/min 0.01 inch/min Decimal point programming allowed G95 0.01 mm/rev 0.0001 inch/rev Decimal point programming allowed

- M29

Specifying an S command or axis movement between M29 and G84 causes alarm PS0203. Then, specifying M29 in the tapping cycle causes alarm PS0204.

- 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 bit 0 (MDL) of parameter No. 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.

- 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 for feed per minute> G94 ; Specify a feed-per-minute command. G00 X120.0 Y100.0 ; Positioning M29 S1000 ; Rigid mode specification G74 Z-100.0 R-20.0 F1000 ; Rigid tapping <Programming for feed per revolution> G95 ; Specify a feed-per-revolution command.

-1

- 80 -

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

G00 X120.0 Y100.0 ; Positioning M29 S1000 ; Rigid mode specification G74 Z-100.0 R-20.0 F1.0 ; Rigid tapping

PROGRAMMING

- 81 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

5.2.3 Peck Rigid Tapping Cycle (G84 or G74)

Tapping a deep hole in rigid tapping mode may be difficult due to chips sticking to the tool or increased cutting resistance. In such cases, the peck rigid tapping cycle is useful. In this cycle, cutting is performed several times until the bottom of the hole is reached. Two peck tapping cycles are available: High-speed peck tapping cycle and standard peck tapping cycle. These cycles are selected using the PCP bit (bit 5) of parameter 5200.

Format

G84 (or G74) X_ Y_ Z_ R_ P_ Q_ 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 Q_ : Depth of cut for each cutting feed F_ : The cutting feedrate K_ : Number of repeats (if required)

G84.2 (or G84.3) X_ Y_ Z_ R_ P_ Q_ F_ L_ ;

(Series 15 format)

L_ : Number of repeats (if required)

G84, G74 (G98) G84, G74 (G99)

• High-speed peck tapping cycle (Bit 5 (PCP) of parameter No. 5200=0) <1> The tool operates at a normal

cutting feedrate. The normal

time constant is used. <2> Retraction can be overridden. The retraction time constant is used.

Point R

d = retraction distance

Point R le v e l

<1>

<2>

Initial lev e l

Point R

<1>

Point R le ve l

<2>

• Peck tapping cycle (Bit 5 (PCP) of parameter No.

5200=1) <1> The tool operates at a normal

cutting feedrate. The normal

time constant is used. <2> Retraction can be overridden. The retraction time constant is

used. <3> Retraction can be overridden. The normal time constant is

used.

Point R

Point Z

d = cutting start distance

Initial level

Point R level

<2>

<3>

Point Z

<1>

- 82 -

<3>

<2>

Point Z

Point R level

Point Z

Point R

<1>

5.FUNCTIONS TO SIMPLIFY

B-63944EN-2/04 PROGRAMMING

PROGRAMMING

Explanation

- High-speed peck tapping cycle

After positioning along the X- and Y-axes, rapid traverse is performed to point R. From point R, cutting is performed with depth Q (depth of cut for each cutting feed), then the tool is retracted by distance d. The bit 4 (DOV) of parameter No. 5200 specifies whether retraction can be overridden or not. When point Z has been reached, the spindle is stopped, then rotated in the reverse direction for retraction. Set the retraction distance, d, in parameter 5213.

- Peck tapping cycle

After positioning along the X- and Y-axes, rapid traverse is performed to point R level. From point R, cutting is performed with depth Q (depth of cut for each cutting feed), then a return is performed to point R. The bit 4 (DOV) of parameter No. 5200 specifies whether the retraction can be overridden or not. The moving of cutting feedrate F is performed from point R to a position distance d from the end point of the last cutting, which is where cutting is restarted. For this moving of cutting feedrate F, the specification of the bit 4 (DOV) of parameter No. 5200 is also valid. When point Z has been reached, the spindle is stopped, then rotated in the reverse direction for retraction. Set d (distance to the point at which cutting is started) in parameter No. 5213.

- 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

- 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.

- Reset

- 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.

- 83 -

5. FUNCTIONS TO SIMPLIFY PROGRAMMING

PROGRAMMING B-63944EN-2/04

- 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

• Specifying a rotation speed exceeding the maximum speed for the gear used causes alarm PS0200.

• 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 diagnosis data 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

Specifying a value that exceeds the upper limit of cutting feedrate causes alarm PS0011.

- Unit of F command

Metric input Inch input Remarks

G94 1 mm/min 0.01 inch/min Decimal point programming allowed G95 0.01 mm/rev 0.0001 inch/rev Decimal point programming allowed

- M29

Specifying an S command or axis movement between M29 and G84 causes alarm PS0203. Then, specifying M29 in the tapping cycle causes alarm PS0204.

- P/Q

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. When Q0 is specified, the peck rigid tapping cycle is not performed.

- Cancel

Do not specify a group 01 G code (G00 to G03 or G60 (when the bit 0 (MDL) of parameter No. 5431 is set to 1)) and G84 in the same block. If they are specified together, G84 is canceled.

- Tool offset

In the canned cycle mode, tool offsets are ignored.

- Subprogram call

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

- 84 -

Fanuc 30i, 31i, 32i Operators Manual

Specifications and Main Features

Frequently Asked Questions

User Manual

CHANGE IN CNC MODEL NAMES

SAFETY PRECAUTIONS

DEFINITION OF WARNING, CAUTION, AND NOTE

GENERAL WARNINGS AND CAUTIONS

WARNINGS AND CAUTIONS RELATED TO PROGRAMMING

WARNINGS AND CAUTIONS RELATED TO HANDLING

WARNINGS RELATED TO DAILY MAINTENANCE

TABLE OF CONTENTS

I. GENERAL

1 GENERAL

1.1 NOTES ON READING THIS MANUAL

1.2 NOTES ON VARIOUS KINDS OF DATA

II. PROGRAMMING

1 GENERAL

1.1 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)

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

4 COORDINATE VALUE AND DIMENSION

4.1 POLAR COORDINATE COMMAND (G15, G16)

5 FUNCTIONS TO SIMPLIFY PROGRAMMING

5.1 CANNED CYCLE FOR DRILLING

5.1.1 High-Speed Peck Drilling Cycle (G73)

5.1.2 Left-Handed Tapping Cycle (G74)

5.1.3 Fine Boring Cycle (G76)

5.1.4 Drilling Cycle, Spot Drilling (G81)

5.1.5 Drilling Cycle Counter Boring Cycle (G82)

5.1.6 Peck Drilling Cycle (G83)

5.1.7 Small-Hole Peck Drilling Cycle (G83)

5.1.8 Tapping Cycle (G84)

5.1.9 Boring Cycle (G85)

5.1.10 Boring Cycle (G86)

5.1.11 Back Boring Cycle (G87)

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)

5.2.2 Left-Handed Rigid Tapping Cycle (G74)

5.2.3 Peck Rigid Tapping Cycle (G84 or G74)