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
1
Coordinate system setting
If a coordinate system is established incorrectly, the machine may behave
unexpectedly as a result of the program issuing an otherwise valid move
command. Such an unexpected operation may damage the tool, the machine
itself, the workpiece, or cause injury to the user.
2
Positioning by nonlinear interpolation
When performing positioning by nonlinear interpolation (positioning by nonlinear
movement between the start and end points), the tool path must be carefully
confirmed before performing programming. Positioning involves rapid traverse. If
the tool collides with the workpiece, it may damage the tool, the machine itself,
the workpiece, or cause injury to the user.
3
Function involving a rotation axis
When programming polar coordinate interpolation or normal-direction
(perpendicular) control, pay careful attention to the speed of the rotation axis.
Incorrect programming may result in the rotation axis speed becoming
excessively high, such that centrifugal force causes the chuck to lose its grip on
the workpiece if the latter is not mounted securely. Such mishap is likely to
damage the tool, the machine itself, the workpiece, or cause injury to the user.
s-3
SAFETY PRECAUTIONS B-64484EN-2/03
WARNING
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.
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
1
Manual operation
When operating the machine manually, determine the current position of the tool
and workpiece, and ensure that the movement axis, direction, and feedrate have
been specified correctly. Incorrect operation of the machine may damage the
tool, the machine itself, the workpiece, or cause injury to the operator.
2
Manual reference position return
After switching on the power, perform manual reference position return as
required.
If the machine is operated without first performing manual reference position
return, it may behave unexpectedly. Stroke check is not possible before manual
reference position return is performed.
An unexpected operation of the machine may damage the tool, the machine
itself, the workpiece, or cause injury to the user.
3
Manual numeric command
When issuing a manual numeric command, determine the current position of the
tool and workpiece, and ensure that the movement axis, direction, and command
have been specified correctly, and that the entered values are valid.
Attempting to operate the machine with an invalid command specified may
damage the tool, the machine itself, the workpiece, or cause injury to the
operator.
4
Manual handle feed
In manual handle feed, rotating the handle with a large scale factor, such as 100,
applied causes the tool and table to move rapidly. Careless handling may
damage the tool and/or machine, or cause injury to the user.
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
8
Software operator's panel and menu switches
Using the software operator's panel and menu switches, in combination with the
MDI unit, it is possible to specify operations not supported by the machine
operator's panel, such as mode change, override value change, and jog feed
commands.
Note, however, that if the MDI unit keys are operated inadvertently, the machine
may behave unexpectedly, possibly damaging the tool, the machine itself, the
workpiece, or causing injury to the user.
9
RESET key
Pressing the RESET key stops the currently running program. As a result, the
servo axes are stopped. However, the RESET key may fail to function for
reasons such as an MDI unit problem. So, when the motors must be stopped,
use the emergency stop button instead of the RESET key to ensure security.
10
Manual intervention
If manual intervention is performed during programmed operation of the
machine, the tool path may vary when the machine is restarted. Before restarting
the machine after manual intervention, therefore, confirm the settings of the
manual absolute switches, parameters, and absolute/incremental command
mode.
11
Feed hold, override, and single block
The feed hold, feedrate override, and single block functions can be disabled
using custom macro system variable #3004. Be careful when operating the
machine in this case.
12
Dry run
Usually, a dry run is used to confirm the operation of the machine. During a dry
run, the machine operates at dry run speed, which differs from the
corresponding programmed feedrate. Note that the dry run speed may
sometimes be higher than the programmed feed rate.
13
Cutter and tool nose radius compensation in MDI mode
Pay careful attention to a tool path specified by a command in MDI mode,
because cutter or tool nose radius compensation is not applied. When a
command is entered from the MDI to interrupt in automatic operation in cutter or
tool nose radius compensation mode, pay particular attention to the tool path
when automatic operation is subsequently resumed. Refer to the descriptions of
the corresponding functions for details.
14
Program editing
If the machine is stopped, after which the machining program is edited
(modification, insertion, or deletion), the machine may behave unexpectedly if
machining is resumed under the control of that program. Basically, do not
modify, insert, or delete commands from a machining program while it is in use.
s-6
B-64484EN-2/03 SAFETY PRECAUTIONS
WARNINGS RELATED TO DAILY MAINTENANCE
WARNING
1
Memory backup battery replacement
When replacing the memory backup batteries, keep the power to the machine
(CNC) turned on, and apply an emergency stop to the machine. Because this
work is performed with the power on and the cabinet open, only those personnel
who have received approved safety and maintenance training may perform this
work.
When replacing the batteries, be careful not to touch the high-voltage circuits
(marked and fitted with an insulating cover).
Touching the uncovered high-voltage circuits presents an extremely dangerous
electric shock hazard.
NOTE
The CNC uses batteries to preserve the contents of its memory, because it must
retain data such as programs, offsets, and parameters even while external
power is not applied.
If the battery voltage drops, a low battery voltage alarm is displayed on the
machine operator's panel or screen.
When a low battery voltage alarm is displayed, replace the batteries within a
week. Otherwise, the contents of the CNC's memory will be lost.
Refer to the Section “Method of replacing battery” in the OPERATOR’S
MANUAL (Common to Lathe System/Machining Center System) for details of
the battery replacement procedure.
WARNING
2
Absolute pulse coder battery replacement
When replacing the memory backup batteries, keep the power to the machine
(CNC) turned on, and apply an emergency stop to the machine. Because this
work is performed with the power on and the cabinet open, only those personnel
who have received approved safety and maintenance training may perform this
work.
When replacing the batteries, be careful not to touch the high-voltage circuits
(marked
and fitted with an insulating cover).
Touching the uncovered high-voltage circuits presents an extremely dangerous
electric shock hazard.
NOTE
The absolute pulse coder uses batteries to preserve its absolute position.
If the battery voltage drops, a low battery voltage alarm is displayed on the
machine operator's panel or screen.
When a low battery voltage alarm is displayed, replace the batteries within a
week. Otherwise, the absolute position data held by the pulse coder will be lost.
Refer to the FANUC SERVO MOTOR
of the battery replacement procedure.
i
series Maintenance Manual for details
α
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
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
p
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
01
00
00
21
00
17
02
06
04
19
00
01
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
00
07
18
08
00
27
11
22
31
00
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
14
15
12
16
00
09
01
34
24
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
09
03
00
05
13
00
10
21
20
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.
Yp
0
End point
Pe
Po
R
Start
point
Yp
Ps
J
I
Base circle
Clockwise involute interpolation (G02.2)
Xp
Yp
Yp
Po
Ps
I
R
Pe
J
End point
Xp
0
End point
Ro
J
Start point
Ps
Pe
Xp
End
point
Pe
Counterclockwise involute interpolation (G03.2)
I
J
0
R
Start point
Ps
Po
Xp
R
0
I
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 -
Loading...