FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. For Lathe System USER’S MANUAL

B-64304EN-1/01

PROGRAMMING

7.AXIS CONTROL FUNCTIONS

7.2

SYNCHRONOUS, COMPOSITE AND SUPERIMPOSED

CONTROL BY PROGRAM COMMAND (G50.4, G51.4,

G50.5, G51.5, G50.6, AND G51.6)

Synchronous control, composite control, and superimposed control

can be started or canceled using a program command instead of a DI

signal. Synchronous control, composite control, and superimposed

control based on a DI signal is also possible.

For the basic operations of synchronous control, composite control,

and superimposed control, see Sections, "SYNCHRONOUS

CONTROL AND COMPOSITE CONTROL" and Section,

"SUPERIMPOSED CONTROL" in the CONNECTION MANUAL

(FUNCTION) (B-64303EN-1).

Format

G51.4 P_ Q_ (L_) ;

Synchronous control start (L is omissible.)

G50.4 Q_ ;

Synchronous control cancel

P: Synchronous master axis ID number

Q: Synchronous slave axis ID number

L: Parking command

1: Master parking (slave parking cancel)

2: Slave parking (master parking cancel)

0: No parking (parking cancel)

(When L is omitted, the specification of L0 is assumed.)

G51.5 P_ Q_ ;

Composite control start

G50.5 P_ Q_ ;

Composite control cancel

P: Composite axis 1 ID number

Q: Composite axis 2 ID number

G51.6 P_ Q_ ;

Superimposed control start

G50.6 Q_ ;

Superimposed control cancel

P: Superimposed master axis ID number

Q: Superimposed slave axis ID number

As an ID number, set a unique value for identifying each axis in parameter

No. 12600 for both of P and Q.

G51.4/G50.4, G51.5/G50.5, and G51.6/G50.6 are one-shot G codes of

group 00.

- 345 -

7.AXIS CONTROL FUNCTIONS

PROGRAMMING

B-64304EN-1/01

Explanation

Synchronous control

Synchronous control is performed with the G51.4/G50.4 commands,

instead of simultaneously controlled axis selection signals.

Parameter setting examples for a 2-path system

•

Parameter No.12600

Path 1

Path 2

101

201

102

202

•

Parameter No.8180

Path 1

Path 2

102

•

Program example (M100 to M103 are synchronization M codes.)

Path 1

Path 2

Operation

N10 M100 ;

M100 ;

Synchronization between paths 1 and 2

N20 G51.4 P102 Q202 ;

Start of Z1-Z2 synchronous control

N30 M101 ;

M101 ;

Synchronization between paths 1 and 2

N40 G00 Z100.;

Synchronous slave movement

Z1-Z2 synchronous control

N50 M102 ;

M102 ;

Synchronization between paths 1 and 2

N60 G50.4 Q202 ;

Cancellation of Z1-Z2 synchronous control

N70 M103 ;

M103 ;

Synchronization between paths 1 and 2

- Start of synchronous control

N20 G51.4 P102 Q202 : Start of synchronous control with the Z1-axis

being a master axis and the Z2-axis being a slave axis

- Cancellation of synchronous control

N60 G50.4 Q202 : Cancellation of synchronous control with the

Z1-axis being a master axis and the Z2-axis being a slave axis

- Parking

Use the L command to specify the start and cancellation of the parking

of synchronous axes.

If the L command is omitted or if the L0 command is issued, the

parking of both synchronous master axis and synchronous slave axis is

canceled.

- Parameter check

If the axis number corresponding to the P specified with G51.4 is not

set in slave axis parameter No. 8180, alarm PS5339 is issued.

- 346 -

B-64304EN-1/01

PROGRAMMING

7.AXIS CONTROL FUNCTIONS

Composite control

Composite control is performed with the G51.5/G50.5 commands,

instead of composite control axis selection signals.

Parameter setting examples for a 2-path system

•

Parameter No.12600

Path 1

Path 2

101

201

102

202

•

Parameter No.8183

Path 1

Path 2

101

102

•

Program example (M100 to M103 are synchronization M codes.)

Path 1

Path 2

Operation

N10 M100 ;

M100 ;

Synchronization between paths 1 and 2

N20 G51.5 P101 Q201 ;

Start of X1-X2 composite control

N30 G51.5 P102 Q202 ;

Start of Z1-Z2 composite control

N40 M101 ;

M101 ;

Synchronization between paths 1 and 2

N50 G00 X 100. Z100.;

Composite movement

X1-X2 and Z1-Z2 composite control

N60 M102 ;

M102 ;

Synchronization between paths 1 and 2

N70 G50.5 P101 Q201 ;

Cancellation of X1-X2 composite control

N80 G50.5 P102 Q202 ;

Cancellation of Z1-Z2 composite control

N90 M103 ;

M103 ;

Synchronization between paths 1 and 2

- Start of composite control

N20 G51.5 P101 Q201 : Start of composite control on the X1- and

X2-axes

N30 G51.5 P102 Q202 : Start of composite control on the Z1- and

Z2-axes

- Cancellation of composite control

N70 G50.5 P101 Q201 : Cancellation of composite control on the X1-

and X2-axes

N80 G50.5 P102 Q202 : Cancellation of composite control on the Z1-

and Z2-axes

- Parameter check

If the composite control axis corresponding to the P or Q specified

with G51.5/G50.5 is not set in parameter No. 8183, alarm PS5339 is

issued.

- 347 -

7.AXIS CONTROL FUNCTIONS

PROGRAMMING

B-64304EN-1/01

Superimposed control

Superimposed control is performed with the G51.6/G50.6 commands,

instead of superimposed control axis selection signals.

Parameter setting examples for a 2-path system

•

Parameter No.12600

Path 1

Path 2

101

201

102

202

•

Parameter No.8186

Path 1

Path 2

•

Program example (M100 to M103 are synchronization M codes.)

Path 1

Path 2

Operation

N10 M100 ;

M100 ;

Synchronization between paths 1 and 3

N20 G51.6 P102 Q202 ;

Start of Z1-Z2 superimposed control

N30 M101 ;

M101 ;

Synchronization between paths 1 and 3

N40 G00 Z100.;

G00 Z-200.;

Z1-Z2 superimposed control

(Z+100 superimposed on Z2)

N50 M102 ;

M102 ;

Synchronization between paths 1 and 3

N60 G50.6 Q202 ;

Cancellation of Z1-Z2 superimposed control

N70 M103 ;

M103 ;

Synchronization between paths 1 and 3

- Start of superimposed control

N20 G51.6 P102 Q202 : Start of superimposed control with the

Z1-axis being a master axis and the Z2-axis being a slave axis

- Cancellation of superimposed control

N60 G50.6 Q202 : Cancellation of superimposed control with the

Z1-axis being a master axis and the Z2-axis being a slave axis

- Parameter check

If the axis number corresponding to the P specified with G51.6 is not

set in superimposed slave axis parameter No. 8186, alarm PS5339 is

issued.

NOTE

1 If G codes (G50.4/G50.5/G50.6) for canceling synchronous,

composite, and superimposed control with program commands

are issued for axes under synchronous, composite, and

superimposed control with DI signals, synchronous, composite,

and superimposed control is canceled.

2 If the synchronous control axis selection signal, composite

control axis selection signal, and superimposed control axis

selection signal are changed from '1' to '0' for axes under

synchronous, composite, and superimposed control with

program commands, synchronous, composite, and

superimposed control is canceled.

- 348 -

8.2-PATH CONTROL FUNCTION PROGRAMMING

B-64304EN-1/01

8.1

OVERVIEW

The 2-path control function is intended to perform two types of

machining simultaneously and independently. The function applies

to lathes and automatic lathes with which two tool posts operate

simultaneously to machine one workpiece.

To control two paths to machine one workpiece simultaneously, the

machining program for each path is stored in the program memory for

the path. In automatic operation, this function selects the program

for path 1 and that for path 2 from the program memory for the

relevant path. When the paths are activated, the programs selected

for the relevant tool posts are executed simultaneously and

independently.

To make tool posts 1 and 2 synchronous during machining, the

waiting function can be used.

Other functions specific to 2-path control that include the following

functions can also be used: Interference check for each path, balance

cutting, synchronous/composite/superimposed control, spindle control

between each path, and common memory between each path.

Only one LCD/MDI is provided for two paths. The path selection

signal is used to switch LCD/MDI operation or display between paths

1 and 2.

For a system with two paths

CNC

LCD/MDI

Program memory for

Path 1

path 1

program

position

axis

analysis

control

Programs

Program memory for

Path 2

path 2

program

position

axis

analysis

control

Programs

- 350 -

B-64304EN-1/01

PROGRAMMING

8.2-PATH CONTROL FUNCTION

8.2

WAITING FUNCTION FOR PATHS

Overview

Control based on M codes is used to cause one path to wait for the

other during machining. When an M code for waiting is specified in

a block for one path during automatic operation, the another path

waits for the same M code to be specified before staring the execution

of the next block.

A range of M codes used as M codes for waiting is to be set in the

parameters

(Nos.

8110 and

8111) beforehand. Waiting can be

ignored using a signal.

Format

Mm ;

m: Number of an M code for waiting

Explanation

CAUTION

1 An M code for waiting must always be specified in a

single block.

2 Unlike other M codes, the M code for waiting is not

output to the PMC.

3 If the operation of a single path is required, the M

code for waiting need not be deleted. By using the

signal to specify that waiting be ignored (NOWT),

the M code for waiting in a machining program can

be ignored. For details, refer to the manual

supplied by the machine tool builder.

4 If using a waiting M code in 1 block multiple-M code

command, be sure to specify it as the first M code.

- 351 -

8.2-PATH CONTROL FUNCTION PROGRAMMING

B-64304EN-1/01

8.3

COMMON MEMORY BETWEEN EACH PATH

Overview

In a 2-path system, this function enables data within the specified

range to be accessed as data common to both paths. The data

includes tool compensation memory and custom macro common

variables.

Explanation

The path common memory function enables the following operations.

- Tool compensation memory

Part or all of tool compensation memory for individual paths can be

used as common data by setting parameter No. 5029.

Tool offset pairs of

path 1

path 2

Tool

compensation

number 1

No.5029=20

80 tool

120 tool

offset

Tool

pairs

compensation

number 20

NOTE

1 The same unit for tool compensation (bits 0 and 1

of parameter No. 5042) must be set for both paths.

2 Set a value less than the number of tool

compensation values for each path for parameter

No. 5029.

3 When the setting of parameter No. 5029 exceeds

the number of tool compensation values for each

path, the smaller of the numbers of tool

compensation values for both paths is used as a

common number.

4 For details, refer to the relevant manual of the

machine tool builder.

- 352 -

B-64304EN-1/01

PROGRAMMING

8.2-PATH CONTROL FUNCTION

- Custom macro common variables

All or part of custom macro common variables #100 to #199 and #500

to #999 can be used as common data by setting parameters No. 6036

(#100 to #199) and 6037 (#500 to #999).

Macro variables

for path 1

for path 2

Macro variable number

No.6036=20

100

macro

Macro variable number 119

variables

NOTE

If the value of parameter No. 6036 or 6037 exceeds

the maximum number of custom macro common

variables, the maximum number of custom macro

common variables is assumed.

- 353 -

8.2-PATH CONTROL FUNCTION PROGRAMMING

B-64304EN-1/01

8.4

SPINDLE CONTROL BETWEEN EACH PATH

Overview

This function allows a workpiece attached to one spindle to be

machined simultaneously with two tool posts and each of two

workpieces attached to each of two spindles to be machined

simultaneously with each of two tool posts.

Tool post 1

Spindle

Tool post 2

Fig. 8.4 (a) Application to a lathe with one spindle and two tool posts

Tool post 1

Spindle 1

Spindle 2

Tool post 2

Fig. 8.4 (b) Application to a lathe with two spindles and two tool posts

The spindle belonging to each path can generally be controlled by

programmed commands for the path. With path spindle command

selection signals, programmed commands for any path can control the

spindle belonging to any path.

NOTE

For the method of spindle command selection, refer

to the relevant manual of the machine tool builder.

- 354 -

B-64304EN-1/01

PROGRAMMING

8.2-PATH CONTROL FUNCTION

8.5

SYNCHRONOUS/COMPOSITE/SUPERIMPOSED

CONTROL

Overview

In 2-path control, the synchronous control function, composite control

function, and superimposed control function enable synchronous

control, composite control, and superimposed control in a single path

system or between 2-path systems.

Explanation

- Synchronous control

• Synchronizes movement along an axis of one system with that

along an axis of the another path.

Example)

Synchronizing movement along the Z1 (master) and Z2 (slave)

axes

Turret 1

Workpiece

Z2 (Synchronized with

movement along the Z1 axis)

Machining according to a program for path 1

- 355 -

8.2-PATH CONTROL FUNCTION PROGRAMMING

B-64304EN-1/01

• Synchronizes movement along an axis of one path with that along

another axis of the same path.

Example)

Synchronizing movement along the Z1 (master) and B1 (slave)

axes

Turret 1

Tail stock

Workpiece 1

B1 (Synchronized with

movement along the Z1

axis)

- Composite control

• Exchanges the move commands for different axes of different path.

Example)

Exchanging the commands for the X1 and X2 axes

→ Upon the execution of a command programmed for path 1,

movement is performed along the X2 and Z1 axes.

Upon the execution of a command programmed for path 2,

movement is performed along the X1 and Z2 axes.

Machining according to a program

Turret 1

for path 1

Workpiece 1

Workpiece 2

Turret 1

Machining according to

a program for path 2

- 356 -

B-64304EN-1/01

PROGRAMMING

8.2-PATH CONTROL FUNCTION

- Superimposed control

• Provides a move command of an axis for a different axis in another

path.

Example)

Providing the Z2 (slave) axis with a move command specified

for the Z1 (master) axis

Turret 1

Machining according to

a program for path 1

Workpiece 1

Turret 2

Machining according to a program

for path 2

NOTE

The method used to specify synchronous,

composite, or superimposed control varies with the

machine tool builder. For details, refer to the

manual supplied by the machine tool builder.

- 357 -

8.2-PATH CONTROL FUNCTION PROGRAMMING

B-64304EN-1/01

8.6

BALANCE CUT (G68, G69)

Overview

When a thin workpiece is to be machined as shown below, a precision

machining can be achieved by machining each side of the workpiece

with a tool simultaneously; this function can prevent the workpiece

from warpage that can result when only one side is machined at a time

(see the figure below). When both sides are machined at the same

time, the movement of one tool must be in phase with that of the other

tool.

Otherwise, the workpiece can vibrate, resulting in poor

machining. With this function, the movement of one tool post can be

easily synchronized with that of the other tool post.

Tool post 2

Tool post 1

Format

G68 ; Balance cut mode on

G69 ; Balance cut mode cancel

- 358 -

B-64304EN-1/01

PROGRAMMING

8.2-PATH CONTROL FUNCTION

Explanation

When G68 is specified in the programs for tool posts 1 and 2, the

balance cut mode is set to on. When G69 is specified, the balance

cut mode is canceled.

When G68 or G69 is specified for either tool post, the tool post waits

until G68 or G69 is specified for the other tool post.

In the balance cut mode, balance cutting is performed when a move

command in cutting feed is specified for both tool posts.

In balance cutting, the tool posts start moving simultaneously in each

block in which a move command in cutting feed is specified.

Specify G68 or G69 in a single block.

NOTE

1 Balance cutting is not performed in dry run or

machine lock state. G68 or G69 specified for one

tool post is synchronized with G68 or G69 specified

for the other tool post, however.

2 In the balance cut mode, G68 specified for one tool

post is not synchronized with G68 specified for the

other tool post. In the balance cut cancel mode,

G69 specified for one tool post is not synchronized

with G69 specified for the other tool post.

3 Balance cutting is not performed in a block in which

0 is specified for the travel distance.

4 Balance cutting is not performed when rapid

traverse is specified.

- 359 -

8.2-PATH CONTROL FUNCTION PROGRAMMING

B-64304EN-1/01

Caution

CAUTION

1 Balance cut only starts cutting feed on both tool

posts at the same time; it does not maintain

synchronization thereafter. To synchronize all the

movements of both tool posts, the setting for both

tool posts, such as the travel distance and feedrate,

must be the same. Override and interlock can be

applied independently to both tool posts. The

settings for both tool posts that are related to

override and interlock must also be the same to

perform balance cutting.

2 After feed hold is applied during execution of

balance cutting for both tool posts, balance cutting

is not performed at the restart. Balance cutting is

performed when the next move command is

executed for both tool posts.

NOTE

1 Time delay before the pulse distribution of both tool

posts is started is 2 msec or shorter.

2 Overlap is invalid. In the balance cut mode,

synchronization is established at the start of each

move block in which cutting is specified, so

movement can momentarily stop.

3 In the balance cut mode, continuous thread cutting

overlap is also invalid. Perform continuous thread

cutting in the balance cut cancel mode.

4 To establish synchronization of the pulse

distribution in a block in which thread cutting is

specified, the same position coder must be

selected.

5 The cancel mode (G69) is unconditionally set by a

reset.

6 When the option "mirror image for double turret" is

selected, the balance cut function cannot be used.

To use the option “mirror image for double turret”,

set bit 0 (NVC) of parameter No. 8137 to 0 to

disable the balance cut function.

- 360 -

B-64304EN-1/01

OPERATION

1.DATA INPUT/OUTPUT

DATA INPUT/OUTPUT

By using the memory card interface on the left side of the display,

information written in a memory card is read into the CNC and

information is written from the CNC to a memory card.

The following types of data can be input and output:

1. Y-axis offset data

The above data can be input and output on the screens used for

displaying and setting the data and on the ALL IO screen.

Chapter

1, "DATA INPUT/OUTPUT", consists of the following

sections:

1.1 INPUT/OUTPUT ON EACH SCREEN

364

1.1.1 Inputting and Outputting Y-axis Offset Data

364

1.1.1.1 Inputting Y-axis offset data

364

1.1.1.2 Outputting Y-axis Offset Data

365

1.2 INPUT/OUTPUT ON THE ALL IO SCREEN

366

1.2.1 Inputting and Outputting Y-axis Offset Data

367

- 363 -

1.DATA INPUT/OUTPUT

OPERATION

B-64304EN-1/01

1.1

INPUT/OUTPUT ON EACH SCREEN

Data can be input to and output from the Y-axis offset screens.

1.1.1

Inputting and Outputting Y-axis Offset Data

1.1.1.1 Inputting Y-axis offset data

Y-axis offset data is loaded into the memory of the CNC from a

memory card. The input format is the same as the output format.

The Y-axis offset data that is registered in the memory and has a

corresponding data number is replaced with data input by this

operation.

Inputting Y-axis offset data (for 8.4/10.4-inch display unit)

Procedure

Make sure the input device is ready for reading.

Press the EDIT switch on the machine operator’s panel.

Press function key

Press the continuous menu key

several times until soft key

[Y OFFSET] appears.

Press soft key [Y OFFSET] to display the Y-axis offset data.

screen.

Press soft key [(OPRT)].

Press the continuous menu key

several times until soft key

[F INPUT] appears.

Press soft key [F INPUT].

Type the name of the file that you want to input.

If the input file name is omitted, default input file name

"TOOLOFST.TXT" is assumed.

10 Press soft key [EXEC].

This starts reading the Y-axis offset data, and "INPUT" blinks in

the lower right part of the screen. When the read operation ends,

the "INPUT" indication disappears.

To cancel the input, press soft key [CANCEL].

- 364 -

B-64304EN-1/01

OPERATION

1.DATA INPUT/OUTPUT

1.1.1.2 Outputting Y-axis Offset Data

Y-axis offset data is output in a output format from the memory of the

CNC to a memory card.

Outputting Y-axis offset data (for 8.4/10.4-inch display unit)

Procedure

Make sure the output device is ready for outputting.

Press the EDIT switch on the machine operator’s panel.

Press function key

Press the continuous menu key

several times until soft key

[Y OFFSET] appears.

Press soft key [Y OFFSET] to display the Y-axis offset data.

screen.

Press soft key [(OPRT)].

Press the continuous menu key

several times until soft key

[F OUTPUT] appears.

Press soft key [F OUTPUT].

Type the file name that you want to output.

If the file name is omitted, default file name "TOOLOFST.TXT"

is assumed.

10 Press soft key [EXEC].

This starts outputting the Y-axis offset data, and “OUTPUT”

blinks in the lower right part of the screen. When the read

operation ends, the “OUTPUT” indication disappears.

To cancel the output, press soft key [CANCEL].

- 365 -

1.DATA INPUT/OUTPUT

OPERATION

B-64304EN-1/01

1.2

INPUT/OUTPUT ON THE ALL IO SCREEN

Just by using the ALL IO screen, you can input and output Y-axis

offset data and tool offset / 2nd geometry data.

The following explains how to display the ALL IO screen:

Displaying the ALL IO screen (for 8.4/10.4-inch display unit)

Procedure

1 Press function key

2 Press the continuous menu key

several times until soft key

[ALL IO] is displayed..

3 Press soft key [ALL IO] to display the ALL IO screen.

The subsequent steps to select data from the ALL IO screen will be

explained for each type of data.

- 366 -

B-64304EN-1/01

OPERATION

1.DATA INPUT/OUTPUT

1.2.1

Inputting and Outputting Y-axis Offset Data

With the lathe system, Y-axis offset data can be input and output

using the ALL IO screen.

Inputting Y-axis offset data (for 8.4/10.4-inch display unit)

Procedure

On the ALL IO screen, press the continuous menu key

several times until soft key [Y OFFSET] is displayed.

Press soft key [Y OFFSET].

Select EDIT mode.

Press soft key [(OPRT)].

Press soft key [N INPUT].

Set the name of the file that you want to input.

Type a file name, and press soft key [F NAME].

If the input file name is omitted, default file name

"TOOLOFST.TXT" is assumed.

Press soft key [EXEC].

This starts reading the Y-axis offset data, and "INPUT" blinks in

the lower right part of the screen. When the read operation ends,

the "INPUT" indication disappears.

To cancel the input, press soft key [CANCEL].

Outputting Y-axis offset data (for 8.4/10.4-inch display unit)

Procedure

On the ALL IO screen, press the continuous menu key

several times until soft key [Y OFFSET] is displayed.

Press soft key [Y OFFSET].

Select EDIT mode.

Press soft key [(OPRT)].

Press soft key [F OUTPUT].

Set the file name to be output.

Type a file name, and press soft key [F NAME].

If the file name is omitted, default file name "TOOLOFST.TXT"

is assumed.

Press soft key [EXEC].

This starts outputting the Y-axis offset data, and “OUTPUT”

blinks in the lower right part of the screen. When the read

operation ends, the “OUTPUT” indication disappears.

To cancel the output, press soft key [CANCEL].

- 367 -

2.SETTING AND DISPLAYING DATA OPERATION

B-64304EN-1/01

SETTING AND DISPLAYING DATA

Chapter 2, "SETTING AND DISPLAYING DATA", consists of the

following sections:

2.1 SCREENS DISPLAYED BY FUNCTION KEY

..........369

2.1.1 Setting and Displaying the Tool Offset Value

370

2.1.2 Direct Input of Tool Offset Value

374

2.1.3 Direct Input of Tool Offset Value Measured B

376

2.1.4 Counter Input of Offset value

379

2.1.5 Setting the Workpiece Coordinate System Shift Value380

2.1.6 Setting the Y-Axis Offset

382

2.1.7 Chuck and Tail Stock Barriers

385

- 368 -

B-64304EN-1/01

OPERATION

2.SETTING AND DISPLAYING DATA

2.1

SCREENS DISPLAYED BY FUNCTION KEY

Press function key

to display or set tool compensation values

and other data.

This section explains the display and setting of the following data

items:

Tool offset value

Workpiece coordinate system shift value

Y-axis offset value

Chuck and tail stock barriers

For the display and setting of data other than the above, refer to

“USER’S MANUAL (Common to Lathe System/Machining Center

System)” (B-64304EN).

- 369 -

2.SETTING AND DISPLAYING DATA OPERATION

B-64304EN-1/01

2.1.1

Setting and Displaying the Tool Offset Value

Dedicated screens are provided for displaying and setting tool offset

values and tool nose radius compensation values.

Whether to use tool geometry and wear compensation can be selected

using bit 6 (NGW) of parameter No. 8136; whether to use tool nose

radius compensation can be selected using bit 7 (NCR) of parameter

No. 8136.

(0: Use the function./1: Does not use the function.)

Setting and displaying the tool offset value and the tool nose radius compensation

value

Procedure

Press function key

When using a 2-path system, select, in advance, a path for which

a tool offset value is to be set, by using the path selection switch.

Press chapter selection soft key [OFFSET] or press function key

several times until the tool compensation screen is

displayed.

Different screens are displayed depending on whether tool

geometry offset, wear offset, or neither is applied.

Fig. 2.1.1 (a) When tool geometry/wear offset is not used (10.4-inch)

- 370 -

B-64304EN-1/01

OPERATION

2.SETTING AND DISPLAYING DATA

Fig. 2.1.1 (b) With tool geometry offset (10.4-inch)

Fig. 2.1.1 (c) With tool wear offset (10.4-inch)

Move the cursor to the compensation value to be set or changed

using page keys and cursor keys, or enter the compensation

number for the compensation value to be set or changed and

press soft key [NO.SRH].

To set a compensation value, enter a value and press soft key

[INPUT]. To change the compensation value, enter a value to

add to the current value (a negative value to reduce the current

value) and press soft key [+INPUT].

T (TIP) is the number of the imaginary tool nose.

T may be specified on the geometry compensation screen or on

the wear compensation screen.

- 371 -

2.SETTING AND DISPLAYING DATA OPERATION

B-64304EN-1/01

When tool nose radius compensation is not used (bit 7 (NCR) of

parameter No.

8136 is set to

1), neither radius nor T

(TIP) is

displayed.

Explanation

- Decimal point input

A decimal point can be used when entering a compensation value.

- Other method

An external input/output device can be used to input or output a cutter

compensation value. See Chapter III-8 “Data Input/Output” in the

User’s Manual (Common to Lathe System/Machining Center System).

Tool length compensation values can be set using the following

functions described in subsequent subsections: direct input of tool

offset value measured, direct input of tool offset value measured B,

and counter input of offset value.

- Number of tool compensation values

Up to 64 (1-path system) or 200 (2-path system) tool compensation

value sets are available.

When the function for 64 (1-path system) or 200 (2-path system) tool

compensation value sets is not used (bit 5 (NDO) of parameter No.

8136 to 1), up to 32 tool compensation value sets are available.

For each set, tool geometry offset can be distinguished from the tool

wear offset.

(When bit 6 (NGW) of parameter No. 8136 is set to 0)

- Disabling entry of compensation values

In some cases, tool wear compensation or tool geometry compensation

values cannot be input because of the settings in bits 0 (WOF) and 1

(GOF) of parameter No.3290. The number of the first tool offset

amount of which entry is to be disabled can be set for parameter No.

3294 and the number of tool offset amounts following the start

number can be set for parameter No. 3295 to disable entry of tool

offset amounts within the specified range from the MDI.

Consecutive input values are set as follows:

When values are input for offset numbers, starting from one for

which input is not inhibited to one for which input is inhibited, a

warning is issued and values are set only for those offset

numbers for which input is not inhibited.

When values are input for offset numbers, starting from one for

which input is inhibited to one for which input is not inhibited, a

warning is issued and no values are set.

- Displaying radius and T (TIP)

When tool nose radius compensation is not used according to the

setting, neither radius nor T (TIP) is displayed.

(Bit 7 (NCR) of

parameter No. 8136 is set to 1.)

- 372 -

B-64304EN-1/01

OPERATION

2.SETTING AND DISPLAYING DATA

- Changing offset values during automatic operation

When offset values have been changed during automatic operation,

bits 4 (LGT) and 6 (LWM) of parameter No.5002 can be used for

specifying whether new offset values become valid in the next move

command or in the next T code command.

Fig. 2.1.1 (a)

When geometry

compensation values and

LGT

LWM

wear compensation values

are separately specified

are not separately specified

Become valid in the next T code

block

Become valid in the next T code

block

Become valid in the next T code

Become valid in the next move

block

command

Become valid in the next move

command

- 373 -

FANUC Series 0i-MODEL D, Series 0i Mate-MODEL D. For Lathe System USER’S MANUAL - page 13