FANUC 30i, 31i, 32i Operators Manual

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

For Machining Center System

OPERATOR'S MANUAL

B-64484EN-2/03

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

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

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

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

The products in this manual are manufactured under strict quality control. However, when a serious accident or loss is predicted due to a failure of the product, pay careful attention to safety.

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

B-64484EN-2/03 SAFETY PRECAUTIONS

SAFETY PRECAUTIONS

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

CONTENTS

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

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

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

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

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

DEFINITION OF WARNING, CAUTION, AND NOTE

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

WARNING

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

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

CAUTION

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

approved procedure is not observed.

NOTE

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

Caution.

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

s-1

SAFETY PRECAUTIONS B-64484EN-2/03

GENERAL WARNINGS AND CAUTIONS

WARNING

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

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

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

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

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

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

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

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

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

amount of compensation.

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

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

s-2

B-64484EN-2/03 SAFETY PRECAUTIONS

CAUTION

The liquid-crystal display is manufactured with very precise fabrication

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

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

NOTE

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

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

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

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

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

limited.

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

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

machining programs are automatically downloaded from a personal computer at

each machining.

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

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

WARNINGS AND CAUTIONS RELATED TO PROGRAMMING

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

WARNING

Coordinate system setting

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

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

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

itself, the workpiece, or cause injury to the user. 2

Positioning by nonlinear interpolation

When performing positioning by nonlinear interpolation (positioning by nonlinear

movement between the start and end points), the tool path must be carefully

confirmed before performing programming. Positioning involves rapid traverse. If

the tool collides with the workpiece, it may damage the tool, the machine itself,

the workpiece, or cause injury to the user. 3

Function involving a rotation axis

When programming polar coordinate interpolation or normal-direction

(perpendicular) control, pay careful attention to the speed of the rotation axis.

Incorrect programming may result in the rotation axis speed becoming

excessively high, such that centrifugal force causes the chuck to lose its grip on

the workpiece if the latter is not mounted securely. Such mishap is likely to

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

s-3

SAFETY PRECAUTIONS B-64484EN-2/03

WARNING

Inch/metric conversion

Switching between inch and metric inputs does not convert the measurement

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

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

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

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

to the user. 5

Constant surface speed control

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

the workpiece coordinate system, the spindle speed may become excessively

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

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

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

Stroke check

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

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

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

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

workpiece, or causing injury to the user. 7

Tool post interference check

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

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

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

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

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

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

Absolute/incremental mode

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

versa, the machine may behave unexpectedly. 9

Plane selection

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

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

descriptions of the respective functions for details. 10

Torque limit skip

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

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

be executed without performing a skip. 11

Programmable mirror image

Note that programmed operations vary considerably when a programmable

mirror image is enabled. 12

Compensation function

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

return command is issued in compensation function mode, compensation is

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

compensation function mode.

s-4

B-64484EN-2/03 SAFETY PRECAUTIONS

WARNINGS AND CAUTIONS RELATED TO HANDLING

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

WARNING

Manual operation

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

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

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

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

Manual reference position return

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

required.

If the machine is operated without first performing manual reference position

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

reference position return is performed.

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

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

Manual numeric command

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

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

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

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

operator. 4

Manual handle feed

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

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

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

Disabled override

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

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

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

to the operator. 6

Origin/preset operation

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

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

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

injury to the user. 7

Workpiece coordinate system shift

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

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

of a program, confirm the coordinate system carefully.

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

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

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

workpiece, or causing injury to the operator.

s-5

SAFETY PRECAUTIONS B-64484EN-2/03

WARNING

Software operator's panel and menu switches

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

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

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

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

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

workpiece, or causing injury to the user. 9

RESET key

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

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

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

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

Manual intervention

If manual intervention is performed during programmed operation of the

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

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

manual absolute switches, parameters, and absolute/incremental command

mode. 11

Feed hold, override, and single block

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

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

machine in this case. 12

Dry run

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

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

corresponding programmed feedrate. Note that the dry run speed may

sometimes be higher than the programmed feed rate. 13

Cutter and tool nose radius compensation in MDI mode

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

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

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

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

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

the corresponding functions for details. 14

Program editing

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

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

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

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

s-6

B-64484EN-2/03 SAFETY PRECAUTIONS

WARNINGS RELATED TO DAILY MAINTENANCE

WARNING

Memory backup battery replacement

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

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

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

who have received approved safety and maintenance training may perform this

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

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

electric shock hazard.

NOTE

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

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

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

machine operator's panel or screen.

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

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

MANUAL (Common to Lathe System/Machining Center System) for details of

the battery replacement procedure.

WARNING

Absolute pulse coder battery replacement

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

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

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

who have received approved safety and maintenance training may perform this

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

(marked

and fitted with an insulating cover).

Touching the uncovered high-voltage circuits presents an extremely dangerous

electric shock hazard.

NOTE

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

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

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

of the battery replacement procedure.

series Maintenance Manual for details

s-7

SAFETY PRECAUTIONS B-64484EN-2/03

WARNING

3 Fuse replacement

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

cause of the blown fuse.

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

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

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

electric shock hazard.

s-8

B-64484EN-2/03 TABLE OF CONTENTS

SAFETY PRECAUTIONS........................................................................... S-1

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

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

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

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

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

I. GENERAL

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

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

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

II. PROGRAMMING

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

1.1 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) .......................................................20

3.1.3 Involute Interpolation on Linear Axis and Rotary Axis

(G02.2, G03.2) .......................................................................................................21

3.2 THREADING (G33) .....................................................................................23

3.3 CONTINUOUS THREADING....................................................................... 24

3.4 MULTIPLE THREADING ............................................................................. 24

3.5 CIRCULAR THREAD CUTTING B (G2.1,G3.1)........................................... 26

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

4 COORDINATE VALUE AND DIMENSION ...........................................41

4.1 POLAR COORDINATE COMMAND (G15, G16) ......................................... 41

5 FUNCTIONS TO SIMPLIFY PROGRAMMING .....................................44

5.1 CANNED CYCLE FOR DRILLING............................................................... 44

5.1.1 High-Speed Peck Drilling Cycle (G73)..................................................................48

5.1.2 Left-Handed Tapping Cycle (G74) ........................................................................50

5.1.3 Fine Boring Cycle (G76) ........................................................................................51

5.1.4 Drilling Cycle, Spot Drilling (G81) .......................................................................53

5.1.5 Drilling Cycle Counter Boring Cycle (G82) ..........................................................54

5.1.6 Peck Drilling Cycle (G83)......................................................................................56

5.1.7 Small-Hole Peck Drilling Cycle (G83) ..................................................................58

5.1.8 Tapping Cycle (G84) ..............................................................................................62

5.1.9 Boring Cycle (G85) ................................................................................................64

5.1.10 Boring Cycle (G86) ................................................................................................65

5.1.11 Back Boring Cycle (G87).......................................................................................67

c-1

TABLE OF CONTENTS B-64484EN-2/03

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

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

5.1.14 Canned Cycle Cancel for Drilling (G80)................................................................72

5.1.15 Example for Using Canned Cycles for Drilling .....................................................73

5.2 IN-POSITION CHECK SWITCHING FOR DRILLING CANNED CYCLE..... 74

5.3 RIGID TAPPING .......................................................................................... 88

5.3.1 Rigid Tapping (G84) ..............................................................................................88

5.3.2 Left-Handed Rigid Tapping Cycle (G74)...............................................................92

5.3.3 Peck Rigid Tapping Cycle (G84 or G74) ...............................................................96

5.3.4 Canned Cycle Cancel (G80) ...................................................................................99

5.3.5 Override during Rigid Tapping ..............................................................................99

5.3.5.1 Extraction override ............................................................................................ 99

5.3.5.2 Override signal ................................................................................................ 100

5.4 OPTIONAL CHAMFERING AND CORNER R........................................... 102

5.5 INDEX TABLE INDEXING FUNCTION...................................................... 105

5.6 IN-FEED CONTROL (FOR GRINDING MACHINE)................................... 107

5.7 CANNED GRINDING CYCLE (FOR GRINDING MACHINE)..................... 109

5.7.1 Plunge Grinding Cycle (G75)...............................................................................111

5.7.2 Direct Constant-Dimension Plunge Grinding Cycle (G77)..................................114

5.7.3 Continuous-feed Surface Grinding Cycle (G78) ..................................................117

5.7.4 Intermittent-feed Surface Grinding Cycle (G79)..................................................120

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

G75.7,G76.7)............................................................................................. 123

5.8.1 Stock Removal in Turning (G71.7) ......................................................................124

5.8.2 Stock Removal in Facing (G72.7) ........................................................................135

5.8.3 Pattern Repeating (G73.7) ....................................................................................139

5.8.4 Finishing Cycle (G70.7) .......................................................................................142

5.8.5 End Face Peck Drilling Cycle (G74.7) .................................................................146

5.8.6 Outer Diameter / Internal Diameter Drilling Cycle (G75.7) ................................148

5.8.7 Multiple Threading Cycle (G76.7) .......................................................................150

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

G75.7, and G76.7) ................................................................................................155

6 COMPENSATION FUNCTION ............................................................157

6.1 TOOL LENGTH COMPENSATION SHIFT TYPES ...................................157

6.2 AUTOMATIC TOOL LENGTH MEASUREMENT (G37) ............................ 164

6.3 TOOL OFFSET (G45 TO G48).................................................................. 167

6.4 OVERVIEW OF CUTTER COMPENSATION (G40-G42).......................... 172

6.5 OVERVIEW OF TOOL NOSE RADIUS COMPENSATION (G40-G42) ..... 177

6.5.1 Imaginary Tool Nose ............................................................................................177

6.5.2 Direction of Imaginary Tool Nose .......................................................................179

6.5.3 Offset Number and Offset Value..........................................................................180

6.5.4 Workpiece Position and Move Command............................................................180

6.5.5 Notes on Tool Nose Radius Compensation ..........................................................185

6.6 DETAILS OF CUTTER OR TOOL NOSE RADIUS COMPENSATION...... 187

6.6.1 Overview ..............................................................................................................187

6.6.2 Tool Movement in Start-up ..................................................................................191

6.6.3 Tool Movement in Offset Mode...........................................................................197

6.6.4 Tool Movement in Offset Mode Cancel...............................................................215

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

Compensation.......................................................................................................221

6.6.6 Interference Check ...............................................................................................224

c-2

B-64484EN-2/03 TABLE OF CONTENTS

6.6.6.1 Operation to be performed if an interference is judged to occur ..................... 227

6.6.6.2 Interference check alarm function ...................................................................228

6.6.6.3 Interference check avoidance function ............................................................229

6.6.7 Tool Radius / Tool Nose Radius Compensation for Input from MDI ..................235

6.7 VECTOR RETENTION (G38) .................................................................... 237

6.8 CORNER CIRCULAR INTERPOLATION (G39) ........................................ 238

6.9 3-DIMENSIONAL TOOL COMPENSATION (G40, G41) ........................... 240

6.10 TOOL COMPENSATION VALUES, NUMBER OF COMPENSATION

VALUES, AND ENTERING VALUES FROM THE PROGRAM (G10) ....... 243

6.11 COORDINATE SYSTEM ROTATION (G68, G69)..................................... 246

6.12 GRINDING WHEEL WEAR COMPENSATION .........................................253

6.13 ACTIVE OFFSET VALUE CHANGE FUNCTION BASED ON MANUAL

FEED .........................................................................................................258

6.14 ROTARY TABLE DYNAMIC FIXTURE OFFSET....................................... 261

6.15 TOOL AXIS DIRECTION TOOL LENGTH COMPENSATION................... 267

6.15.1 Control Point Compensation of Tool Length Compensation Along Tool Axis...271

6.16 SPINDLE UNIT COMPENSATION, NUTATING ROTARY HEAD TOOL

LENGTH COMPENSATION ...................................................................... 275

7 MEMORY OPERATION USING Series 15 PROGRAM FORMAT ..... 279

7.1 MULTIPLE REPETITIVE CYCLE ..............................................................280

7.1.1 Stock Removal in Turning (G71.7) ......................................................................281

7.1.2 Stock Removal in Facing (G72.7) ........................................................................293

7.1.3 Pattern Repeating (G73.7) ....................................................................................297

7.1.4 Finishing Cycle (G70.7) .......................................................................................300

7.1.5 End Face Peck Drilling Cycle (G74.7) .................................................................304

7.1.6 Outer Diameter / Internal Diameter Drilling Cycle (G75.7) ................................305

7.1.7 Multiple Threading Cycle (G76.7) .......................................................................307

7.1.8 Restrictions on Multiple Repetitive Cycle ...........................................................312

8 AXIS CONTROL FUNCTIONS............................................................314

8.1 PARALLEL AXIS CONTROL ..................................................................... 314

9 GAS CUTTING MACHINE .................................................................. 319

9.1 TOOL OFFSET B ......................................................................................319

9.2 CONER CONTROL BY FEED RATE ........................................................ 322

9.3 AUTOMATIC EXACT STOP CHECK ........................................................ 324

9.4 AXIS SWITCHING ..................................................................................... 327

9.5 GENTLE CURVE CUTTING ...................................................................... 330

9.6 GENTLE NORMAL DIRECTION CONTROL............................................. 332

9.6.1 Linear Distance Setting ........................................................................................333

III. OPERATION

1 SETTING AND DISPLAYING DATA...................................................337

1.1 SCREENS DISPLAYED BY FUNCTION KEY ................................... 337

1.1.1 Setting and Displaying the Tool Compensation Value ........................................337

1.1.2 Tool Length Measurement ...................................................................................342

1.1.3 Tool Length/Workpiece Origin Measurement .....................................................345

1.1.4 Setting and Displaying the Rotary Table Dynamic Fixture Offset ......................364

c-3

TABLE OF CONTENTS B-64484EN-2/03

1.1.5 Input of Tool Offset Value Measured B ...............................................................367

1.1.6 Spindle Unit Compensation, Nutating Rotary Head Tool Length Compensation367

APPENDIX

A PARAMETERS.................................................................................... 373

A.1 DESCRIPTION OF PARAMETERS........................................................... 373

A.2 DATA TYPE............................................................................................... 420

A.3 STANDARD PARAMETER SETTING TABLES......................................... 421

c-4

I. GENERAL

B-64484EN-2/03 GENERAL 1.GENERAL

1 GENERAL

This manual consists of the following parts:

About this manual

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

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

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

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

NOTE

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

system path control type. For other functions not specific to the lathe system, refer to the Operator's Manual (Common to Lathe System/Machining Center System) (B-64484EN).

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

For detail, refer to the DESCRIPTIONS manual (B-64482EN).

3 This manual does not detail the parameters not mentioned in the text. For

details of those parameters, refer to the Parameter Manual (B-64490EN).

Parameters are used to set functions and operating conditions of a CNC

machine tool, and frequently-used values in advance. Usually, the machine tool builder factory-sets parameters so that the user can use the machine tool easily.

4 This manual describes not only basic functions but also optional functions. Look

up the options incorporated into your system in the manual written by the machine tool builder.

Applicable models

This manual describes the models indicated in the table below. In the text, the abbreviations indicated below may be used.

Model name Abbreviation

FANUC Series 30i-B 30i –B Series 30i FANUC Series 31i-B 31i –B FANUC Series 31i-B5 31i –B5 FANUC Series 32i-B 32i –B Series 32i

NOTE

1 Unless otherwise noted, the model names 31i-B, 31i-B5, and 32i-B are

collectively referred to as 30i. However, this convention is not necessarily

observed when item 3 below is applicable. 2 Some functions described in this manual may not be applied to some products. For details, refer to the Descriptions (B-64482EN).

Series 31i

- 3 -

1.GENERAL GENERAL B-64484EN-2/03

Special symbols

This manual uses the following symbols:

- IP

Indicates a combination of axes such as X_ Y_ Z_ In the underlined position following each address, a numeric value such as a coordinate value is

placed (used in PROGRAMMING.).

- ;

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

Related manuals of Series 30i- MODEL B Series 31i- MODEL B Series 32i- MODEL B

The following table lists the manuals related to Series 30i-B, Series 31i-B, Series 32i-B. This manual is indicated by an asterisk(*).

Table 1 Related manuals

Manual name Specification number

DESCRIPTIONS B-64482EN CONNECTION MANUAL (HARDWARE) B-64483EN CONNECTION MANUAL (FUNCTION) B-64483EN-1 OPERATOR’S MANUAL (Common to Lathe System/Machining Center System) B-64484EN OPERATOR’S MANUAL (For Lathe System) B-64484EN-1 OPERATOR’S MANUAL (For Machining Center System) B-64484EN-2 * MAINTENANCE MANUAL B-64485EN PARAMETER MANUAL B-64490EN

Programming

Macro Executor PROGRAMMING MANUAL B-63943EN-2 Macro Compiler PROGRAMMING MANUAL B-66263EN C Language Executor PROGRAMMING MANUAL B-63943EN-3

PMC

PMC PROGRAMMING MANUAL B-64513EN

Network

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

Operation guidance function

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

Dual Check Safety

Dual Check Safety CONNECTION MANUAL B-64483EN-2

B-63874EN

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

- 4 -

B-64484EN-2/03 GENERAL 1.GENERAL

Related manuals of SERVO MOTOR αi/βi series

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

Table 2 Related manuals

Manual name Specification number

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

The above servo motors and the corresponding spindles can be connected to the CNC covered in this manual. In the αi SV, αi SP, αi PS, and βi SV series, however, they can be connected only to 30 i-B-compatible versions. In the βi SVSP series, they cannot be connected. This manual mainly assumes that the FANUC SERVO MOTOR αi series of servo motor is used. For servo motor and spindle information, refer to the manuals for the servo motor and spindle that are actually connected.

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

B-65285EN

B-65325EN

B-65270EN

B-65280EN

- 5 -

1.GENERAL GENERAL B-64484EN-2/03

1.1 NOTES ON READING THIS MANUAL

CAUTION

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

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

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

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

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

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

should take precedence over this manual. 2 In the header field of each page of this manual, a chapter title is indicated so that

the reader can reference necessary information easily.

By finding a desired title first, the reader can reference necessary parts only. 3 This manual describes as many reasonable variations in equipment usage as

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

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

attempted.

1.2 NOTES ON VARIOUS KINDS OF DATA

CAUTION

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

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

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

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

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

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

create a copy of the various kinds of data beforehand.

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

limited.

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

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

machining programs are automatically downloaded from a personal computer at

each machining.

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

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

- 6 -

II. PROGRAMMING

B-64484EN-2/03 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 Chapter, “Compensation Function”).

- 9 -

2. PREPARATORY FUNCTION (G FUNCTION)

PROGRAMMING B-64484EN-2/03

2 PREPARATORY FUNCTION

(G FUNCTION)

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

Type Meaning

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

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

Z_ ; G01 is effective in this range. X_ ;

G00 Z_ ; G00 is effective in this range.

X_ ;

G01 X_ ;

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-64484EN-2/03 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 G17.1 Plane conversion function G18 ZpXp plane selection G19 G20 (G70) Input in inch G21 (G71) G22 Stored stroke check function on G23 G25 Spindle speed fluctuation detection off G26 G27 Reference position return check G28 Automatic return to reference position G28.2 In-position check disable reference position return G29 Movement from reference position G30 2nd, 3rd and 4th reference position return G30.1 Floating reference position return G30.2 In-position check disable 2nd, 3rd, or 4th reference position return G31 Skip function G31.8 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 Zp: Z 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

(G FUNCTION)

- 11 -

2. PREPARATORY FUNCTION (G FUNCTION)

PROGRAMMING B-64484EN-2/03

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 Tool center point control (type 2) G43.7 Tool offset G44.1 G45 Tool offset : increase G46 Tool offset : decrease G47 Tool offset : double increase G48 G49 (G49.1) 08 Tool length compensation cancel G44.9 Spindle unit compensation G49.9 G50 Scaling cancel G51 G50.1 Programmable mirror image cancel G51.1 G50.2 Polygon turning cancel G51.2 G50.4 Cancel synchronous control G50.5 Cancel composite control G50.6 Cancel superimposed control G51.4 Start synchronous control G51.5 Start composite control G51.6 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 offset conversion

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-64484EN-2/03 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 indexing G68.3 Tilted working plane indexing by tool axis direction G68.4 G70.7 Finishing cycle G71.7 Outer surface rough machining cycle G72.7 End rough machining cycle G73.7 Closed loop cutting cycle G74.7 End cutting off cycle G75.7 Outer or inner cutting off cycle G76.7 Multiple threading cycle G72.1 Figure copying (rotary copy) G72.2 G73 Peck drilling cycle G74 G75 01 Plunge grinding cycle G76 09 Fine boring cycle G77 Plunge direct sizing/grinding cycle G78 Continuous-feed surface grinding cycle G79

G80 09

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

G81 09

G81.1 00 Chopping function/High precision oscillation function

Workpiece coordinate system 6 selection

Cutting mode

Macro modal call A/B cancel

Tilted working plane indexing (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-64484EN-2/03

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-64484EN-2/03 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)...........................................................................................................................23

3.3 CONTINUOUS THREADING...........................................................................................................24

3.4 MULTIPLE THREADING.................................................................................................................24

3.5 CIRCULAR THREAD CUTTING B (G2.1,G3.1).............................................................................26

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

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-64484EN-2/03

Explanation

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

End point

Start point

Base circle

Clockwise involute interpolation (G02.2)

End point

Start point

End point

Counterclockwise involute interpolation (G03.2)

Start point

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 -

+ 410 hidden pages