FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. For Machining Center System USER’S MANUAL - page 1
B-64304EN-2/01
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-2
GENERAL WARNINGS AND CAUTIONS
s-3
WARNINGS AND CAUTIONS RELATED TO
PROGRAMMING
s-6
WARNINGS AND CAUTIONS RELATED TO HANDLING
s-8
WARNINGS RELATED TO DAILY MAINTENANCE
s-11
s-1
SAFETY PRECAUTIONS
B-64304EN-2/01
DEFINITION OF WARNING, CAUTION, AND NOTE
This manual includes safety precautions for protecting the user and
preventing damage to the machine. Precautions are classified into
Warning and Caution according to their bearing on safety. Also,
supplementary information is described as a Note. Read the
Warning, Caution, and Note thoroughly before attempting to use
the machine.
WARNING
Applied when there is a danger of the user being
injured or when there is a danger of both the user
being injured and the equipment being damaged if
the approved procedure is not observed.
CAUTION
Applied when there is a danger of the equipment
being damaged, if the approved procedure is not
observed.
NOTE
The Note is used to indicate supplementary
information other than Warning and Caution.
•
Read this manual carefully, and store it in a safe place.
s-2
B-64304EN-2/01
SAFETY PRECAUTIONS
GENERAL WARNINGS AND CAUTIONS
WARNING
1
Never attempt to machine a workpiece without first
checking the operation of the machine. Before
starting a production run, ensure that the machine
is operating correctly by performing a trial run
using, for example, the single block, feedrate
override, or machine lock function or by operating
the machine with neither a tool nor workpiece
mounted. Failure to confirm the correct operation
of the machine may result in the machine behaving
unexpectedly, possibly causing damage to the
workpiece and/or machine itself, or injury to the
user.
2
Before operating the machine, thoroughly check
the entered data.
Operating the machine with incorrectly specified
data may result in the machine behaving
unexpectedly, possibly causing damage to the
workpiece and/or machine itself, or injury to the
user.
3
Ensure that the specified feedrate is appropriate
for the intended operation. Generally, for each
machine, there is a maximum allowable feedrate.
The appropriate feedrate varies with the intended
operation. Refer to the manual provided with the
machine to determine the maximum allowable
feedrate.
If a machine is run at other than the correct speed,
it may behave unexpectedly, possibly causing
damage to the workpiece and/or machine itself, or
injury to the user.
4
When using a tool compensation function,
thoroughly check the direction and amount of
compensation.
Operating the machine with incorrectly specified
data may result in the machine behaving
unexpectedly, possibly causing damage to the
workpiece and/or machine itself, or injury to the
user.
s-3
SAFETY PRECAUTIONS
B-64304EN-2/01
WARNING
5
The parameters for the CNC and PMC are
factory-set. Usually, there is not need to change
them. When, however, there is not alternative other
than to change a parameter, ensure that you fully
understand the function of the parameter before
making any change.
Failure to set a parameter correctly may result in
the machine behaving unexpectedly, possibly
causing damage to the workpiece and/or machine
itself, or injury to the user.
6
Immediately after switching on the power, do not
touch any of the keys on the MDI panel until the
position display or alarm screen appears on the
CNC unit.
Some of the keys on the MDI panel are dedicated
to maintenance or other special operations.
Pressing any of these keys may place the CNC
unit in other than its normal state. Starting the
machine in this state may cause it to behave
unexpectedly.
7
The User’s Manual and programming manual
supplied with a CNC unit provide an overall
description of the machine's functions, including
any optional functions. Note that the optional
functions will vary from one machine model to
another. Therefore, some functions described in
the manuals may not actually be available for a
particular model. Check the specification of the
machine if in doubt.
8
Some functions may have been implemented at
the request of the machine-tool builder. When
using such functions, refer to the manual supplied
by the machine-tool builder for details of their use
and any related cautions.
CAUTION
The liquid-crystal display is manufactured with very
precise fabrication technology. Some pixels may
not be turned on or may remain on. This
phenomenon is a common attribute of LCDs and is
not a defect.
s-4
B-64304EN-2/01
SAFETY PRECAUTIONS
NOTE
Programs, parameters, and macro variables are
stored in nonvolatile memory in the CNC unit.
Usually, they are retained even if the power is
turned off.
Such data may be deleted inadvertently, however,
or it may prove necessary to delete all data from
nonvolatile memory as part of error recovery.
To guard against the occurrence of the above, and
assure quick restoration of deleted data, backup all
vital data, and keep the backup copy in a safe
place.
s-5
SAFETY PRECAUTIONS
B-64304EN-2/01
WARNINGS AND CAUTIONS RELATED TO PROGRAMMING
This section covers the major safety precautions related to
programming. Before attempting to perform programming, read the
supplied User’s Manual carefully such that you are fully familiar with
their contents.
WARNING
1
Coordinate system setting
If a coordinate system is established incorrectly,
the machine may behave unexpectedly as a result
of the program issuing an otherwise valid move
command. Such an unexpected operation may
damage the tool, the machine itself, the workpiece,
or cause injury to the user.
2
Positioning by nonlinear interpolation
When performing positioning by nonlinear
interpolation (positioning by nonlinear movement
between the start and end points), the tool path
must be carefully confirmed before performing
programming. Positioning involves rapid traverse. If
the tool collides with the workpiece, it may damage
the tool, the machine itself, the workpiece, or
cause injury to the user.
3
Function involving a rotation axis
When programming normal-direction
(perpendicular) control, pay careful attention to the
speed of the rotation axis. Incorrect programming
may result in the rotation axis speed becoming
excessively high, such that centrifugal force causes
the chuck to lose its grip on the workpiece if the
latter is not mounted securely. Such mishap is
likely to damage the tool, the machine itself, the
workpiece, or cause injury to the user.
4
Inch/metric conversion
Switching between inch and metric inputs does not
convert the measurement units of data such as the
workpiece origin offset, parameter, and current
position. Before starting the machine, therefore,
determine which measurement units are being
used. Attempting to perform an operation with
invalid data specified may damage the tool, the
machine itself, the workpiece, or cause injury to the
user.
s-6
B-64304EN-2/01
SAFETY PRECAUTIONS
WARNING
5
Constant surface speed control
When an axis subject to constant surface speed
control approaches the origin of the workpiece
coordinate system, the spindle speed may become
excessively high. Therefore, it is necessary to
specify a maximum allowable speed. Specifying
the maximum allowable speed incorrectly may
damage the tool, the machine itself, the workpiece,
or cause injury to the user.
6
Stroke check
After switching on the power, perform a manual
reference position return as required. Stroke check
is not possible before manual reference position
return is performed. Note that when stroke check is
disabled, an alarm is not issued even if a stroke
limit is exceeded, possibly damaging the tool, the
machine itself, the workpiece, or causing injury to
the user.
7
Absolute/incremental mode
If a program created with absolute values is run in
incremental mode, or vice versa, the machine may
behave unexpectedly.
8
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.
9
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.
10 Programmable mirror image
Note that programmed operations vary
considerably when a programmable mirror image is
enabled.
11 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-7
SAFETY PRECAUTIONS
B-64304EN-2/01
WARNINGS AND CAUTIONS RELATED TO HANDLING
This section presents safety precautions related to the handling of
machine tools. Before attempting to operate your machine, read the
supplied User’s Manual carefully, such that you are fully familiar with
their contents.
WARNING
1
Manual operation
When operating the machine manually, determine
the current position of the tool and workpiece, and
ensure that the movement axis, direction, and
feedrate have been specified correctly. Incorrect
operation of the machine may damage the tool, the
machine itself, the workpiece, or cause injury to the
operator.
2
Manual reference position return
After switching on the power, perform manual
reference position return as required.
If the machine is operated without first performing
manual reference position return, it may behave
unexpectedly. Stroke check is not possible before
manual reference position return is performed.
An unexpected operation of the machine may
damage the tool, the machine itself, the workpiece,
or cause injury to the user.
3
Manual 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.
4
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.
5
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.
s-8
B-64304EN-2/01
SAFETY PRECAUTIONS
WARNING
6
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.
7
Software operator's panel and menu switches
Using the software operator's panel and menu
switches, in combination with the MDI panel, it is
possible to specify operations not supported by the
machine operator's panel, such as mode change,
override value change, and jog feed commands.
Note, however, that if the MDI panel keys are
operated inadvertently, the machine may behave
unexpectedly, possibly damaging the tool, the
machine itself, the workpiece, or causing injury to
the user.
8
RESET key
Pressing the RESET key stops the currently
running program. As a result, the servo axes are
stopped. However, the RESET key may fail to
function for reasons such as an MDI panel
problem. So, when the motors must be stopped,
use the emergency stop button instead of the
RESET key to ensure security.
9
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.
10 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.
s-9
SAFETY PRECAUTIONS
B-64304EN-2/01
WARNING
11 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.
12 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.
13 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-10
B-64304EN-2/01
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 User’s Manual (Common to T/M series) for
details of the battery replacement procedure.
s-11
SAFETY PRECAUTIONS
B-64304EN-2/01
WARNING
2 Absolute pulse coder battery replacement
When replacing the memory backup batteries,
keep the power to the machine (CNC) turned on,
and apply an emergency stop to the machine.
Because this work is performed with the power on
and the cabinet open, only those personnel who
have received approved safety and maintenance
training may perform this work.
When replacing the batteries, be careful not to
touch the high-voltage circuits (marked
and
fitted with an insulating cover).
Touching the uncovered high-voltage circuits
presents an extremely dangerous electric shock
hazard.
NOTE
The absolute pulse coder uses batteries to
preserve its absolute position.
If the battery voltage drops, a low battery voltage
alarm is displayed on the machine operator's panel
or screen.
When a low battery voltage alarm is displayed,
replace the batteries within a week. Otherwise, the
absolute position data held by the pulse coder will
be lost.
Refer to the FANUC SERVO MOTOR αi series
Maintenance Manual for details of the battery
replacement procedure.
s-12
B-64304EN-2/01
SAFETY PRECAUTIONS
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-13
B-64304EN-2/01
TABLE OF CONTENTS
TABLE OF CONTENTS
SAFETY PRECAUTIONS
s-1
DEFINITION OF WARNING, CAUTION, AND NOTE
s-2
GENERAL WARNINGS AND CAUTIONS
s-3
WARNINGS AND CAUTIONS RELATED TO PROGRAMMING
s-6
WARNINGS AND CAUTIONS RELATED TO HANDLING
s-8
WARNINGS RELATED TO DAILY MAINTENANCE
s-11
I. GENERAL
1 GENERAL
3
1.1
GENERAL FLOW OF OPERATION OF CNC MACHINE TOOL
7
1.2
NOTES ON READING THIS MANUAL
8
1.3
NOTES ON VARIOUS KINDS OF DATA
8
II. PROGRAMMING
1
GENERAL
11
1.1
TOOL FIGURE AND TOOL MOTION BY PROGRAM
12
2
PREPARATORY FUNCTION (G FUNCTION)
13
3
INTERPOLATION FUNCTION
18
3.1
SINGLE DIRECTION POSITIONING (G60)
19
3.2
THREADING (G33)
22
4
COORDINATE VALUE AND DIMENSION
24
4.1
POLAR COORDINATE COMMAND (G15, G16)
25
5
FUNCTIONS TO SIMPLIFY PROGRAMMING
28
5.1
CANNED CYCLE FOR DRILLING
29
5.1.1
High-Speed Peck Drilling Cycle (G73)
34
5.1.2
Left-Handed Tapping Cycle (G74)
36
5.1.3
Fine Boring Cycle (G76)
43
5.1.4
Drilling Cycle, Spot Drilling (G81)
45
5.1.5
Drilling Cycle Counter Boring Cycle (G82)
47
5.1.6
Peck Drilling Cycle (G83)
49
5.1.7
Small-Hole Peck Drilling Cycle (G83)
51
5.1.8
Tapping Cycle (G84)
57
5.1.9
Boring Cycle (G85)
60
5.1.10
Boring Cycle (G86)
62
5.1.11
Back Boring Cycle (G87)
64
5.1.12
Boring Cycle (G88)
67
5.1.13
Boring Cycle (G89)
69
5.1.14
Canned Cycle Cancel for Drilling (G80)
71
5.1.15
Example for Using Canned Cycles for Drilling
72
5.2
RIGID TAPPING
74
5.2.1
Rigid Tapping (G84)
75
c-1
TABLE OF CONTENTS
B-64304EN-2/01
5.2.2
Left-Handed Rigid Tapping Cycle (G74)
79
5.2.3
Peck Rigid Tapping Cycle (G84 or G74)
83
5.2.4
Canned Cycle Cancel (G80)
86
5.2.5
Override during Rigid Tapping
87
5.2.5.1
Extraction override
87
5.2.5.2
Override signal
89
5.3
OPTIONAL CHAMFERING AND CORNER R
90
5.4
INDEX TABLE INDEXING FUNCTION
94
5.5
IN-FEED CONTROL (FOR GRINDING MACHINE)
97
5.6
CANNED GRINDING CYCLE (FOR GRINDING MACHINE)
101
5.6.1
Plunge Grinding Cycle (G75)
103
5.6.2
Direct Constant-Dimension Plunge Grinding Cycle (G77)
107
5.6.3
Continuous-feed Surface Grinding Cycle (G78)
111
5.6.4
Intermittent-feed Surface Grinding Cycle (G79)
115
6
COMPENSATION FUNCTION
118
6.1
TOOL LENGTH COMPENSATION (G43, G44, G49)
119
6.1.1
Overview
119
6.1.2
G53, G28, and G30 Commands in Tool Length Compensation Mode
125
6.2
TOOL LENGTH COMPENSATION SHIFT TYPES
127
6.3
AUTOMATIC TOOL LENGTH MEASUREMENT (G37)
137
6.4
TOOL OFFSET (G45 - G48)
141
6.5
OVERVIEW OF CUTTER COMPENSATION (G40-G42)
146
6.6
DETAILS OF CUTTER COMPENSATION
153
6.6.1
Overview
153
6.6.2
Tool Movement in Start-up
157
6.6.3
Tool Movement in Offset Mode
163
6.6.4
Tool Movement in Offset Mode Cancel
184
6.6.5
Prevention of Overcutting Due to Cutter Compensation
192
6.6.6
Interference Check
196
6.6.6.1
Operation to be performed if an interference is judged to occur
200
6.6.6.2
Interference check alarm function
200
6.6.6.3
Interference check avoidance function
202
6.6.7
Cutter Compensation for Input from MDI
208
6.7
CORNER CIRCULAR INTERPOLATION (G39)
210
6.8
TOOL COMPENSATION VALUES, NUMBER OF COMPENSATION
VALUES, AND ENTERING VALUES FROM THE PROGRAM (G10)
212
6.9
SCALING (G50, G51)
215
6.10
COORDINATE SYSTEM ROTATION (G68, G69)
224
6.11
NORMAL DIRECTION CONTROL (G40.1,G41.1,G42.1)
231
6.12
PROGRAMMABLE MIRROR IMAGE (G50.1, G51.1)
236
7
MEMORY OPERATION USING Series 10/11 PROGRAM FORMAT 238
8
AXIS CONTROL FUNCTIONS
239
8.1
ELECTRONIC GEAR BOX (G80, G81 (G80.4, G81.4))
240
8.1.1
Electronic Gear Box
240
c-2
B-64304EN-2/01
TABLE OF CONTENTS
III. OPERATION
1 SETTING AND DISPLAYING DATA
253
1.1
SCREENS DISPLAYED BY FUNCTION KEY
...................................254
1.1.1
Setting and Displaying the Tool Compensation Value
255
1.1.2
Tool Length Measurement
258
APPENDIX
A
PARAMETERS
263
A.1
DESCRIPTION OF PARAMETERS
264
A.2
DATA TYPE
311
A.3
STANDARD PARAMETER SETTING TABLES
312
B
DIFFERENCES FROM SERIES 0i-C
314
B.1
SETTING UNIT
315
B.1.1
Differences in Specifications
315
B.1.2
Differences in Diagnosis Display
315
B.2
AUTOMATIC TOOL OFFSET
316
B.2.1
Differences in Specifications
316
B.2.2
Differences in Diagnosis Display
317
B.3
CIRCULAR INTERPOLATION
318
B.3.1
Differences in Specifications
318
B.3.2
Differences in Diagnosis Display
318
B.4
HELICAL INTERPOLATION
319
B.4.1
Differences in Specifications
319
B.4.2
Differences in Diagnosis Display
319
B.5
SKIP FUNCTION
320
B.5.1
Differences in Specifications
320
B.5.2
Differences in Diagnosis Display
321
B.6
MANUAL REFERENCE POSITION RETURN
322
B.6.1
Differences in Specifications
322
B.6.2
Differences in Diagnosis Display
324
B.7
WORKPIECE COORDINATE SYSTEM
325
B.7.1
Differences in Specifications
325
B.7.2
Differences in Diagnosis Display
325
B.8
LOCAL COORDINATE SYSTEM
326
B.8.1
Differences in Specifications
326
B.8.2
Differences in Diagnosis Display
327
B.9
Cs CONTOUR CONTROL
328
B.9.1
Differences in Specifications
328
B.9.2
Differences in Diagnosis Display
328
B.10
SERIAL/ANALOG SPINDLE CONTROL
329
B.10.1 Differences in Specifications
329
B.10.2 Differences in Diagnosis Display
329
B.11
CONSTANT SURFACE SPEED CONTROL
330
B.11.1 Differences in Specifications
330
B.11.2 Differences in Diagnosis Display
330
c-3
TABLE OF CONTENTS
B-64304EN-2/01
B.12
TOOL FUNCTIONS
331
B.12.1 Differences in Specifications
331
B.12.2 Differences in Diagnosis Display
331
B.13
TOOL COMPENSATION MEMORY
332
B.13.1 Differences in Specifications
332
B.13.2 Differences in Diagnosis Display
332
B.14
CUSTOM MACRO
333
B.14.1 Differences in Specifications
333
B.14.2 Differences in Diagnosis Display
334
B.14.3 Miscellaneous
335
B.15
INTERRUPTION TYPE CUSTOM MACRO
336
B.15.1 Differences in Specifications
336
B.15.2 Differences in Diagnosis Display
336
B.16
PROGRAMMABLE PARAMETER INPUT (G10)
337
B.16.1 Differences in Specifications
337
B.16.2 Differences in Diagnosis Display
337
B.17
AI ADVANCED PREVIEW CONTROL /AI CONTOUR CONTROL
338
B.17.1 Differences in Specifications
338
B.17.2 Differences in Diagnosis Display
340
B.18
MACHINING CONDITION SELECTION FUNCTION
341
B.18.1 Differences in Specifications
341
B.18.2 Differences in Diagnosis Display
341
B.19
AXIS SYNCHRONOUS CONTROL
342
B.19.1 Differences in Specifications
342
B.19.2 Differences in Diagnosis Display
346
B.20
ARBITRARY ANGULAR AXIS CONTROL
347
B.20.1 Differences in Specifications
347
B.20.2 Differences in Diagnosis Display
347
B.21
RUN HOUR AND PARTS COUNT DISPLAY
348
B.21.1 Differences in Specifications
348
B.21.2 Differences in Diagnosis Display
348
B.22
MANUAL HANDLE FEED
349
B.22.1 Differences in Specifications
349
B.22.2 Differences in Diagnosis Display
349
B.23
PMC AXIS CONTROL
350
B.23.1 Differences in Specifications
350
B.23.2 Differences in Diagnosis Display
354
B.24
EXTERNAL SUBPROGRAM CALL (M198)
355
B.24.1 Differences in Specifications
355
B.24.2 Differences in Diagnosis Display
355
B.25
SEQUENCE NUMBER SEARCH
356
B.25.1 Differences in Specifications
356
B.25.2 Differences in Diagnosis Display
356
B.26
STORED STROKE CHECK
357
B.26.1 Differences in Specifications
357
B.26.2 Differences in Diagnosis Display
358
B.27
STORED PITCH ERROR COMPENSATION
359
B.27.1 Differences in Specifications
359
B.27.2 Differences in Diagnosis Display
359
c-4
B-64304EN-2/01
TABLE OF CONTENTS
B.28
SCREEN ERASURE FUNCTION AND AUTOMATIC SCREEN
ERASURE FUNCTION
360
B.28.1 Differences in Specifications
360
B.28.2 Differences in Diagnosis Display
360
B.29
RESET AND REWIND
361
B.29.1 Differences in Specifications
361
B.29.2 Differences in Diagnosis Display
361
B.30
MANUAL ABSOLUTE ON AND OFF
362
B.30.1 Differences in Specifications
362
B.30.2 Differences in Diagnosis Display
362
B.31
EXTERNAL DATA INPUT
363
B.31.1 Differences in Specifications
363
B.31.2 Differences in Diagnosis Display
364
B.32
DATA SERVER FUNCTION
365
B.32.1 Differences in Specifications
365
B.32.2 Differences in Diagnosis Display
365
B.33
POWER MATE CNC MANAGER
366
B.33.1 Differences in Specifications
366
B.33.2 Differences in Diagnosis Display
366
B.34
CUTTER COMPENSATION/TOOL NOSE RADIUS COMPENSATION
367
B.34.1 Differences in Specifications
367
B.34.2 Differences in Diagnosis Display
372
B.35
CANNED CYCLE FOR DRILLING
373
B.35.1 Differences in Specifications
373
B.35.2 Differences in Diagnosis Display
374
B.36
CANNED GRINDING CYCLE
375
B.36.1 Differences in Specifications
375
B.36.2 Differences in Diagnosis Display
375
B.37
SINGLE DIRECTION POSITIONING
376
B.37.1 Differences in Specifications
376
B.37.2 Differences in Diagnosis Display
376
B.38
OPTIONAL ANGLE CHAMFERING AND CORNER ROUNDING
377
B.38.1 Differences in Specifications
377
B.38.2 Differences in Diagnosis Display
377
c-5
B-64304EN-2/01
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, valid data ranges, and alarms.
NOTE
1 This manual describes the functions that can
operate in the M series path control type. For
other functions not specific to the M series , refer to
the User's Manual (Common to Lathe
System/Machining Center System) (B-64304EN).
2 Some functions described in this manual may not
be applied to some products. For detail, refer to the
DESCRIPTIONS manual (B-64302EN).
3 This manual does not detail the parameters not
mentioned in the text. For details of those
parameters, refer to the parameter manual
(B-64310EN).
Parameters are used to set functions and
operating conditions of a CNC machine tool, and
frequently-used values in advance. Usually, the
machine tool builder factory-sets parameters so
that the user can use the machine tool easily.
4 This manual describes not only basic functions but
also optional functions. Look up the options
incorporated into your system in the manual written
by the machine tool builder.
- 3 -
1.GENERAL
GENERAL
B-64304EN-2/01
Applicable models
The models covered by this manual, and their abbreviations are :
Model name
Abbreviation
FANUC Series 0i -MD
0i-MD
Series 0i-MD
FANUC Series 0i Mate -MD
0i Mate-MD
Series 0i Mate-MD
Special symbols
This manual uses the following symbols:
- IP
Indicates a combination of axes such as X_ Y_ Z_
In the underlined position following each address, a numeric value
such as a coordinate value is placed (used in PROGRAMMING.).
- ;
Indicates the end of a block. It actually corresponds to the ISO code
LF or EIA code CR.
- 4 -
B-64304EN-2/01
GENERAL
1.GENERAL
Related manuals of Series 0i -D,Series 0i Mate -D
The following table lists the manuals related to Series 0i -D,Series 0i
Mate -D. This manual is indicated by an asterisk(*).
Table 1 Related manuals
Specification
Manual name
number
DESCRIPTIONS
B-64302EN
CONNECTION MANUAL (HARDWARE)
B-64303EN
CONNECTION MANUAL (FUNCTION)
B-64303EN-1
USER’S MANUAL
B-64304EN
(Common to Lathe System/Machining Center System)
USER’S MANUAL (For Lathe System)
B-64304EN-1
USER’S MANUAL (For Machining Center System)
B-64304EN-2
*
MAINTENANCE MANUAL
B-64305EN
PARAMETER MANUAL
B-64310EN
START-UP MANUAL
B-64304EN-3
Programming
Macro Compiler / Macro Executor
B-64303EN-2
PROGRAMMING MANUAL
Macro Compiler OPERATOR’S MANUAL
B-64304EN-5
C Language PROGRAMMING MANUAL
B-64303EN-3
PMC
PMCPROGRAMMING MANUAL
B-64393EN
Network
PROFIBUS-DP Board OPERATOR’S MANUAL
B-64404EN
Fast Ethernet / Fast Data Server OPERATOR’S MANUAL
B-64414EN
Operation guidance function
MANUAL GUIDE i
B-63874EN
(Common to Lathe System/Machining Center System)
OPERATOR’S MANUAL
MANUAL GUIDE i (For Machining Center System)
B-63874EN-2
OPERATOR’S MANUAL
MANUAL GUIDE i (Set-up Guidance Functions)
B-63874EN-1
OPERATOR’S MANUAL
MANUAL GUIDE 0i OPERATOR’S MANUAL
B-64434EN
TURN MATE i OPERATOR’S MANUAL
B-64254EN
- 5 -
1.GENERAL
GENERAL
B-64304EN-2/01
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
Specification
Manual name
number
FANUC AC SERVO MOTOR αi series
B-65262EN
DESCRIPTIONS
FANUC AC SPINDLE MOTOR αi series
B-65272EN
DESCRIPTIONS
FANUC AC SERVO MOTOR βi series
B-65302EN
DESCRIPTIONS
FANUC AC SPINDLE MOTOR βi series
B-65312EN
DESCRIPTIONS
FANUC SERVO AMPLIFIER αi series
B-65282EN
DESCRIPTIONS
FANUC SERVO AMPLIFIER βi series
B-65322EN
DESCRIPTIONS
FANUC SERVO MOTOR αis series
FANUC SERVO MOTOR αi series
FANUC AC SPINDLE MOTOR αi series
B-65285EN
FANUC SERVO AMPLIFIER αi series
MAINTENANCE MANUAL
FANUC SERVO MOTOR βis series
FANUC AC SPINDLE MOTOR βi series
B-65325EN
FANUC SERVO AMPLIFIER βi series
MAINTENANCE MANUAL
FANUC AC SERVO MOTOR αi/βi series,
FANUC LINEAR MOTOR LiS series
B-65270EN
FANUC SYNCHRONOUS BUILT-IN SERVO MOTOR DiS
series PARAMETER MANUAL
FANUC AC SPINDLE MOTOR αi/βi series,
BUILT-IN SPINDLE MOTOR Bi series
B-65280EN
PARAMETER MANUAL
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.
- 6 -
B-64304EN-2/01
GENERAL
1.GENERAL
1.1
GENERAL FLOW OF OPERATION OF CNC MACHINE
TOOL
When machining the part using the CNC machine tool, first prepare
the program, then operate the CNC machine by using the program.
(1) First, prepare the program from a part drawing to operate the
CNC machine tool.
How to prepare the program is described in the Part II,
“Programming.”
(2) The program is to be read into the CNC system. Then, mount the
workpieces and tools on the machine, and operate the tools
according to the programming. Finally, execute the machining
actually.
How to operate the CNC system is described in the Part III,
“Operation.”
Part
Part
drawing
program
CNC
Machine Tool
PART II, "PROGRAMMING"
PART III, "OPERATION"
Before the actual programming, make the machining plan for how to
machine the part.
Machining plan
1.
Determination of workpieces machining range
2.
Method of mounting workpieces on the machine tool
3.
Machining sequence in every cutting process
4.
Cutting tools and cutting conditions
Decide the cutting method in every cutting process.
Cutting process
1
2
3
Cutting procedure
End face
Outer
Grooving
cutting
diameter
cutting
1. Cutting method :
Rough
Semi
Finish
2. Cutting tools
3. Cutting conditions :
Feedrate
Cutting depth
4. Tool path
- 7 -
1.GENERAL
GENERAL
B-64304EN-2/01
1.2
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.
1.3
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.
- 8 -
B-64304EN-2/01
PROGRAMMING
1.GENERAL
1
GENERAL
Chapter 1, "GENERAL", consists of the following sections:
1.1 TOOL FIGURE AND TOOL MOTION BY PROGRAM
12
- 11 -
1.GENERAL
PROGRAMMING
B-64304EN-2/01
1.1
TOOL FIGURE AND TOOL MOTION BY PROGRAM
Explanation
- Machining using the end of cutter - Tool length compensation function
Usually, several tools are used for machining one workpiece. The
tools have different tool length. It is very troublesome to change the
program in accordance with the tools.
Therefore, the length of each tool used should be measured in advance.
By setting the difference between the length of the standard tool and
the length of each tool in the CNC
(See Chapter
“Setting and
Displaying Data” in User’s Manual (Common to 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 Chapter,
“Compensation
Function” in this manual).
H1
H2
H3
H4
Standard
tool
Workpiece
- Machining using the side of cutter - Cutter compensation function
Cutter path using cutter compensation
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 User’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” in this
manual).
- 12 -
2.PREPARATORY FUNCTION
B-64304EN-2/01
PROGRAMMING
(G FUNCTION)
2
PREPARATORY FUNCTION
(G FUNCTION)
A number following address G determines the meaning of the
command for the concerned block.
G codes are divided into the following two types.
Type
Meaning
The G code is effective only in the block in which it
One-shot G code
is specified.
The G code is effective until another G code of the
Modal G code
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_ ;
:
- 13 -
2. PREPARATORY FUNCTION
(G FUNCTION)
PROGRAMMING
B-64304EN-2/01
Explanation
1.
When the clear state (parameter CLR (No. 3402#6)) is set at
power-up or reset, the modal G codes are placed in the states
described below.
(1) The modal G codes are placed in the states marked with
as indicated in Table 2.
(2) G20 and G21 remain unchanged when the clear state is set
at power-up or reset.
(3) Which status G22 or G23 at power on is set by parameter
G23
(No.
3402#7). However, G22 and G23 remain
unchanged when the clear state is set at reset.
(4) The user can select G00 or G01 by setting parameter G01
(No. 3402#0).
(5) The user can select G90 or G91 by setting parameter G91
(No. 3402#3).
When G code system B or C is used in the lathe system,
setting parameter G91 (No. 3402#3) determines which code,
either G90 or G91, is effective.
(6) In the machining center system, the user can select G17,
G18, or G19 by setting parameters G18 and G19 (No.
3402#1 and #2).
2.
G codes in group 00 other than G10 and G11 are one-shot G
codes.
3.
When a G code not listed in the G code list is specified, or a G
code that has no corresponding option is specified, alarm PS0010
occurs.
4.
Multiple G codes can be specified in the same block if each G
code belongs to a different group. If multiple G codes that belong
to the same group are specified in the same block, only the last G
code specified is valid.
5.
If a G code belonging to group 01 is specified in a canned cycle
for drilling, the canned cycle for drilling is cancelled. This means
that the same state set by specifying G80 is set. Note that the G
codes in group 01 are not affected by a G code specifying a
canned cycle for drilling.
6.
G codes are indicated by group.
7.
The group of G60 is switched according to the setting of the
parameter MDL (No. 5431#0). (When the MDL bit is set to 0,
the 00 group is selected. When the MDL bit is set to 1, the 01
group is selected.)
- 14 -
2.PREPARATORY FUNCTION
B-64304EN-2/01
PROGRAMMING
(G FUNCTION)
Table 2 G code list
G code
Group
Function
G00
Positioning (rapid traverse)
G01
Linear interpolation (cutting feed)
01
G02
Circular interpolation CW or helical interpolation CW
G03
Circular interpolation CCW or helical interpolation CCW
G04
Dwell, Exact stop
G05.1
AI advanced preview control / AI contour control
G05.4
HRV3 on/off
G07.1 (G107)
00
Cylindrical interpolation
G09
Exact stop
G10
Programmable data input
G11
Programmable data input mode cancel
G15
Polar coordinates command cancel
17
G16
Polar coordinates command
G17
XpYp plane selection
Xp: X axis or its parallel axis
G18
02
ZpXp plane selection
Yp: Y axis or its parallel axis
G19
YpZp plane selection
Zp: Z axis or its parallel axis
G20
Input in inch
06
G21
Input in mm
G22
Stored stroke check function on
04
G23
Stored stroke check function off
G27
Reference position return check
G28
Automatic return to reference position
G29
00
Movement from reference position
G30
2nd, 3rd and 4th reference position return
G31
Skip function
G33
01
Threading
G37
Automatic tool length measurement
00
G39
Cutter compensation : corner circular interpolation
G40
Cutter compensation : cancel
G41
07
Cutter compensation : left
G42
Cutter compensation : right
G40.1
Normal direction control cancel mode
G41.1
19
Normal direction control on : left
G42.1
Normal direction control on : right
G43
Tool length compensation +
08
G44
Tool length compensation -
G45
Tool offset : increase
G46
Tool offset : decrease
00
G47
Tool offset : double increase
G48
Tool offset : double decrease
G49
08
Tool length compensation cancel
G50
Scaling cancel
11
G51
Scaling
G50.1
Programmable mirror image cancel
22
G51.1
Programmable mirror image
G52
Local coordinate system setting
00
G53
Machine coordinate system setting
- 15 -