FANUC Series 0i-MODEL F. For Lathe System OPERATOR'S MANUAL (B-64604EN-1/01)

B-64604EN-1/01

PROGRAMMING

- 297 -

6.MEMORY OPERATION

USING Series 10/11 FORMAT

6.5.9

Canned Cycle for Drilling Cancel (G80)

G80 cancels canned cycle for drilling.

Format

G80 ;

Explanation

Canned cycle for drilling is canceled to perform normal operation. Point R and point Z are cleared.
Other drilling data is also canceled (cleared).

6.5.10

Precautions to be Taken by Operator

Reset and emergency stop

Even when the controller is stopped by resetting or emergency stop in the course of drilling cycle, the
drilling mode and drilling data are saved ; with this mind, therefore, restart operation.

- Single block

When drilling cycle is performed with a single block, the operation stops at the end points of operations 1,
2, 6 in Fig. 6.5 (a).
Consequently, it follows that operation is started up 3 times to drill one hole. The operation stops at the
end points of operations 1, 2 with the feed hold lamp ON. If there is a remaining repetitive count at the
end of operation 6, the operation is stopped by feed hold. If there is no remaining repetitive count, the
operation is stopped in the single block stop state.

- Feed hold

When "Feed Hold" is applied between operations 3 and 5 by G84/G88, the feed hold lamp lights up
immediately if the feed hold is applied again to operation 6.

- Override

During operation with G84 and G88, the feedrate override is 100%.

7.AXIS CONTROL FUNCTIONS

PROGRAMMING

B-64604EN-1/01

- 298 -

AXIS CONTROL FUNCTIONS

Chapter 7, "AXIS CONTROL FUNCTIONS", consists of the following sections:

7.1

POLYGON TURNING (G50.2, G51.2) .........................................................................................298

7.1

POLYGON TURNING (G50.2, G51.2)

Polygon turning means machining a workpiece to a polygonal figure by rotating the workpiece and tool at
a certain ratio.

Workpiece

Tool

Fig. 7.1 (a) Polygon turning

By changing conditions which are rotation ratio of workpiece and tool and number of cutters, the
workpiece can be machined to a square or hexagon. The machining time can be reduced as compared with
polygonal figure machining using the polar coordinate interpolation. The machined figure, however, is
not exactly polygonal. Generally, polygon turning is used for the heads of square and/or hexagon bolts or
hexagon nuts.
As the tool rotary axis, one of the following can be used:
-

CNC controlled axis (servo axis)

Second spindle (Two serial spindles are connected.)

Polygonal machining performed using a servo axis as the tool rotary axis is referred to as polygon turning.
Polygonal machining performed using the second spindle as the tool rotary axis is referred to as polygon
turning with two spindles.

Function name

Workpiece axis

Tool rotary axis

Polygon turning

Spindle
(Either an analog spindle or serial spindle
is usable. However, a detector equivalent
to a position coder is required.)

Servo axis

Polygon turning with two spindles

Spindle
(Serial spindle)

Explanation

A CNC controlled axis (servo axis) is assigned to the tool rotary axis.
This rotary axis of tool is called Y-axis in the following description. As the workpiece axis (spindle),
either a serial spindle or analog spindle can be used.
The Y-axis is controlled by the G51.2 command, so that the ratio of the rotation speeds of the spindle
(previously specified by S-command) and the tool becomes the specified ratio.
When simultaneous start is specified by G51.2, the one-rotation signal sent from the position codes set on
the spindle is detected. After one-rotation signal detection, the Y-axis is controlled using the rotation ratio
of the spindle and Y-axis specified by P and Q. So, a position coder needs to be attached to the spindle.

B-64604EN-1/01

PROGRAMMING

7.AXIS CONTROL FUNCTIONS

- 299 -

This control will be maintained until the polygon turning cancel command is executed (G50.2). Polygon
turning is cancelled by any of the following in addition to the G50.2 command:
(1) Power

off

(2) Emergency

stop

(3) Servo

alarm

(4) Reset (external reset signal ERS, reset/rewind signal RRW, and RESET key on the MDI unit)

In polygon turning with two spindles, setting bit 0 (RPL) of parameter No.7603 to 1 prevents
polygon synchronization mode from being released by reset.

(5) Occurrence of alarms PS0217 to PS0221, PS0314, and PS05018

NOTE

1 Before polygon turning, reference position return operation on the Y-axis needs

to be specified to determine the rotation start position of the tool. This reference
position return operation is performed by detecting a deceleration limit as in the
case of manual reference position return operation. (By setting bit 7 (PLZ) of
parameter No. 7600, reference position return operation can be performed
without detecting a deceleration limit.)

2 The rotation direction on the Y-axis is determined by the sign of Q, and is not

affected by the rotation direction of the position coder.

3 Among the current position display of the Y axis, the display for the machine

coordinate value (MACHINE) changes from a range of 0 to the amount of
movement per revolution as the Y axis moves. Absolute and relative coordinate
values are not updated. So, when specifying an absolute programming for the
Y-axis after polygon turning mode cancellation, set a workpiece coordinate
system after reference position return operation.

4 For the Y-axis engaged in polygon turning, jog feed and handle feed are

disabled.

5 For the Y-axis not engaged in polygon turning, a move command can be

specified as in the case of other controlled axes.

6 The Y-axis engaged in polygon turning is not counted in the number of

simultaneously controlled axes.

7 One workpiece must be machined using a fixed spindle speed until the

workpiece is finished.

8 G50.2 is the G code for suppressing buffering.
9 The following functions must be commanded with polygon turning cancel mode.

- Inch/metric

conversion

- AI Advanced Preview Control (M Series)/AI Contour Control I/AI Contour

Control II

-  Tilted working plane indexing (M series)
-  Nano smoothing (M series)
-  Flexible path axis assignment

7.AXIS CONTROL FUNCTIONS

PROGRAMMING

B-64604EN-1/01

- 300 -

CAUTION

1 During polygon turning, threading cannot be performed.
2 For the Y-axis engaged in polygon turning, the signals below are valid or invalid:

Signals valid for the Y-axis
- Machine

lock

- Servo-off
Signals invalid for the Y-axis
- Feed

hold

- Interlock
- Override
- Dry

run

(In the dry run, workpiece might not be processed to the expected shape
because the one-rotation signal is not awaited though the speed of a dry run
is invalid.)

Format

G50.2

Polygon turning cancel

G51.2 P_ Q_ [R_] ;

Start of polygon turning

P,Q: Rotation ratio of spindle and Y-axis
R    : Relative phase difference between spindle and Y-axis (*1)
Specify range:
P:    Integer from 1 to 999
Q:    Integer from -999 to -1 or from 1 to 999

When Q is a positive value, Y-axis makes positive rotation.

When Q is a negative value, Y-axis makes negative rotation.

R: 0 to 360 degrees

The unit of data is depend on the increment system of the reference axis.

The decimal point can be used.

If a value out of range is specified, it is rounded in 0 to 360 degrees.

(*1) R can be specified in polygon turning with two spindles.

The least command increment of R is 360/4096 degrees, and the value less than
the least command increment is rounded off.

R may be omitted. If R is not specified after starting polygon turning with two
spindles, the phase difference is assumed to be 0. Even if R is not specified, phase
adjustment is performed.

If bit 5 (COF) of parameter No. 7602 is 1 to disable phase control, R is ignored.

NOTE

Specify G50.2 and G51.2 in a single block.

B-64604EN-1/01

PROGRAMMING

7.AXIS CONTROL FUNCTIONS

- 301 -

Example

G00 X100. 0 Z20.0 S1000.0 M03 ;

(Workpiece rotation speed 1000 (min

-1

))

G51.2 P1 Q2 ;

(Tool rotation start (tool rotation speed 2000 (min

-1

))

G01 X80.0 F10.0 ;

(X-axis infeed)

G04 X2.0 ;

(Waiting 2 seconds)

G00 X100.0 ;

(X-axis escape)

G50.2 ;

(Tool rotation stop)

M05 S0 ;

(Spindle stop )

Principle of polygon turning

The principle of polygon turning is explained below. In the figure (Fig. 7.1 (b)) below the radius of tool
and workpiece are A and B, and the angular speeds of tool and workpiece are

and

. The origin of XY

Cartesian coordinates is assumed to be the center of the workpiece.
Simplifying the explanation, consider that the tool center exists at the position
P

(A, 0) on the workpiece periphery, and the tool nose starts from position P

(A-B, 0).

(0,0)

Angular speed

A : Workpiece radius
B : Rool radius

Angular
speed

Workpiece

Tool

: Workpiece angular speed

: Tool angular speed

Po (A, 0)
Pto (A-B, 0)

Fig. 7.1 (b) Principle of polygon turning

(0, 0)

Start point

Pt (Xt, Yt)

Fig. 7.1 (c) Tool nose position

In this case, the tool nose position Pt (Xt, Yt) after time t is expressed by equations 1 and 2:

cos

cos(

)

(Equation

sin

sin(

)

(Equation

Assuming that the rotation ratio of workpiece to tool is 1:2, namely,

, equations 1 and 2 are

modified as follows:

cos

-Bcos

A-B

)cos

(Equation

1)'

sin

+Bsin

A+B

)sin

(Equation

2)'

These equations indicate that the tool nose path draws an ellipse with longer diameter A+B and shorter
diameter A-B.
Then consider the case when one tool is set at 180

symmetrical positions, for a total of two. A square can

be machined with these tools as shown below.

B-64604EN-1/01

PROGRAMMING

- 303 -

8.MUITI-PATH CONTROL

FUNCTION

MUITI-PATH CONTROL FUNCTION

Chapter 8, "MUITI-PATH CONTROL FUNCTION", consists of the following sections:

8.1 BALANCE CUT (G68, G69) ...........................................................................................................303

8.1

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 Fig. 8.1 (a)). 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 1

Tool post 2

Fig. 8.1 (a)

NOTE

1 This function is an optional function.
2 The balance cut is available when bit 0 (NVC) of parameter No.8137 is 0.

Though, when the mirror image for double turret is selected, the balance cut
cannot be used. To use the mirror image for double turret, set 0 to bit 0 (NVC) of
parameter No. 8137 to disable the balance cut.

Format

G68 ; Balance cut mode on

G69; Balance cut mode cancel

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.

PROGRAMMING

B-64604EN-1/01

- 304 -

8. MUITI-PATH CONTROL

FUNCTION

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.
If G68 or G69 is specified incorrectly, alarm PS0163 occurs.

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.

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 at the start of 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.

B-64604EN-1/01

OPERATION

1.DATA INPUT/OUTPUT

- 307 -

DATA INPUT/OUTPUT

By using the memory card interface and the USB memory interface on the left side of the display,
information written in a memory card and USB memory is input into the CNC and information is written
from the CNC to a memory card and USB memory.
The following types of data can be input and output:
1. Y-axis offset data
2. Tool offset / 2nd geometry data
3. 4th/5th 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 ...........................................................................................307

1.1.1 Inputting and Outputting Y-axis Offset Data........................................................................307

1.1.1.1 Inputting Y-axis offset data ...................................................................................307
1.1.1.2 Outputting Y-axis Offset Data...............................................................................308

1.1.2 Inputting and Outputting Tool Offset / 2nd Geometry Data.................................................309

1.1.2.1 Inputting tool offset / 2nd geometry data ..............................................................309
1.1.2.2 Outputting tool offset / 2nd geometry data............................................................310

1.1.3 Inputting and Outputting 4th/5th Axis Offset Data ..............................................................311

1.1.3.1 Inputting 4th/5th axis offset data...........................................................................311
1.1.3.2 Outputting 4th/5th Axis Offset Data .....................................................................312

1.2 INPUT/OUTPUT ON THE ALL IO SCREEN ................................................................................314

1.2.1 Inputting and Outputting Y-axis Offset Data........................................................................315
1.2.2 Inputting and Outputting Tool Offset / 2nd Geometry Tool Offset......................................316

1.1

INPUT/OUTPUT ON EACH SCREEN

Data can be input to and output from the Y-axis offset and tool offset/second geometry operation screens.

1.1.1

Inputting and Outputting Y-axis Offset Data

NOTE

When bit 1 (YOF) of parameter No.8132 is 1, "Y-axis offset" can be used.

1.1.1.1

Inputting Y-axis offset data

Y-axis offset data is loaded into the memory of the CNC from such as 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 inputting.

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

Press function key

1.DATA INPUT/OUTPUT

OPERATION

B-64604EN-1/01

- 308 -

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 inputting the Y-axis offset data, and "INPUT" blinks in the lower right part of the screen.
When the input operation ends, the "INPUT" indication disappears.
To cancel the input, press soft key [CANCEL].

Inputting Y-axis offset data (for 15-inch display unit)

Procedure

Make sure the input device is ready for inputting.

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

Press function key

Press vertical soft key [NEXT PAGE] several times until soft key [Y OFFSET] is displayed.

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

Press horizontal 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.

Press horizontal soft key [EXEC].
This starts inputting the Y-axis offset data, and "INPUT" blinks in the lower right part of the screen.
When the input operation ends, the "INPUT" indication disappears.
To cancel the input, press horizontal soft key [CANCEL].

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 such as 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 output operation ends, the “OUTPUT” indication disappears.
To cancel the output, press soft key [CANCEL].

B-64604EN-1/01

OPERATION

1.DATA INPUT/OUTPUT

- 309 -

Outputting Y-axis offset data (for 15-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 vertical soft key [NEXT PAGE] several times until soft key [Y OFFSET] is displayed.

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

Press horizontal 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.

Press horizontal soft key [EXEC].
This starts outputting the Y-axis offset data, and “OUTPUT” blinks in the lower right part of the
screen. When the output operation ends, the “OUTPUT” indication disappears.
To cancel the output, press horizontal soft key [CANCEL].

1.1.2

Inputting and Outputting Tool Offset / 2nd Geometry Data

NOTE

"2nd Geometry Tool Offset" is an optional function.
To use the "2nd Geometry Tool Offset", this option and "Tool geometry offset
and Tool wear offset" are required. "Tool geometry offset and Tool wear offset"
can be used, when bit 6 (NGW) of parameter No.8136 is 0.

1.1.2.1

Inputting tool offset / 2nd geometry data

Tool offset / 2nd geometry data is loaded into the memory of the CNC from such as memory card. The
input format is the same as the output format. The tool offset / 2nd geometry data that is registered in
the memory and has a corresponding data number is replaced with data input by this operation.

Inputting tool offset / 2nd geometry data (for 8.4/10.4-inch display unit)

Procedure

Make sure the input device is ready for inputting.

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

Press function key

Press the continuous menu key

several times until soft key [2ND GEOM] appears.

Press soft key [2ND GEOM] to display the offset / 2nd geometry 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 "SEC_GEOM.TXT" is assumed.

10 Press soft key [EXEC].

This starts inputting the 2nd geometry data, and "INPUT" blinks in the lower right part of the screen.
When the input operation ends, the "INPUT" indication disappears.
To cancel the input, press soft key [CANCEL].

1.DATA INPUT/OUTPUT

OPERATION

B-64604EN-1/01

- 310 -

Inputting tool offset / 2nd geometry data (for 15-inch display unit)

Procedure

Make sure the input device is ready for inputting.

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

Press function key

Press vertical soft key [NEXT PAGE] several times until soft key [2ND GEOM] is displayed.

Press vertical soft key [2ND GEOM] to display the Y-axis offset data screen.

Press horizontal 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 "SEC_GEOM.TXT" is assumed.

Press horizontal soft key [EXEC].
This starts inputting the 2nd geometry data, and "INPUT" blinks in the lower right part of the screen.
When the input operation ends, the "INPUT" indication disappears.
To cancel the input, press horizontal soft key [CANCEL].

1.1.2.2

Outputting tool offset / 2nd geometry data

Tool offset / 2nd geometry data is output in a output format from the memory of the CNC to such as
memory card.

Outputting tool offset / 2nd geometry 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 [2ND GEOM] appears.

Press soft key [2ND GEOM] to display the offset / 2nd geometry 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 "SEC_GEOM.TXT" is assumed.

10 Press soft key [EXEC].

This starts outputting the 2nd geometry data, and “OUTPUT” blinks in the lower right part of the
screen. When the output operation ends, the “OUTPUT” indication disappears.
To cancel the output, press soft key [CANCEL].

Outputting tool offset / 2nd geometry data (for 15-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 vertical soft key [NEXT PAGE] several times until soft key [2ND GEOM] is displayed.

Press vertical soft key [2ND GEOM] to display the Y-axis offset data screen.

Press horizontal soft key [F OUTPUT].

Type the file name that you want to output.
If the file name is omitted, default file name "SEC_GEOM.TXT" is assumed.

Press horizontal soft key [EXEC].
This starts outputting the 2nd geometry data, and “OUTPUT” blinks in the lower right part of the

B-64604EN-1/01

OPERATION

1.DATA INPUT/OUTPUT

- 311 -

screen. When the output operation ends, the “OUTPUT” indication disappears.
To cancel the output, press horizontal soft key [CANCEL].

1.1.3

Inputting and Outputting 4th/5th Axis Offset Data

NOTE

"4th/5th axis offset" is an optional function.

1.1.3.1

Inputting 4th/5th axis offset data

Tool offset values can be input through an I/O device. Tool offset values can also be input by using the
ALL IO function.

Inputting 4th/5th axis offset data (for 8.4/10.4-inch display unit)

Procedure

Make sure the input device is ready for inputting.

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

Press function key

Press the continuous menu key

several times until soft key [OFFSET] or [EXTEND OFFSET]

is displayed.

Press soft key [OFFSET] or [EXTEND OFFSET] to display the offset screen or 4th/5th axis offset
screen.

Press soft key [(OPRT)].

Press soft key [F INPUT].

Press soft key [EXEC].

The input format for tool offset values based on the G10 command is used.

NOTE

When a program written in the input format for tool offset values based on the
G10 command is input, all offset values corresponding to the axis addresses and
offset numbers specified in the program are rewritten.
However, the data of a function with no option specified is ignored.

Inputting 4th/5th axis offset data (for 15-inch display unit)

Procedure

Make sure the input device is ready for inputting.

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

Press function key

Press vertical soft key [NEXT PAGE] several times until vertical soft key [OFFSET] or [EXTEND
OFFSET] is displayed.

Press vertical soft key [OFFSET] or [EXTEND OFFSET] to display the offset screen or 4th/5th axis
offset screen.

Press horizontal soft key [F INPUT].

Press horizontal soft key [EXEC].

The input format for tool offset values based on the G10 command is used.

1.DATA INPUT/OUTPUT

OPERATION

B-64604EN-1/01

- 312 -

NOTE

1.1.3.2

Outputting 4th/5th Axis Offset Data

Tool offset values can be output to an I/O device.

Outputting 4th/5th axis offset data (for 8.4/10.4-inch display unit)

Procedure

Make sure the input device is ready for inputting.

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

Press function key

Press the continuous menu key

several times until soft key [OFFSET] or [EXTEND OFFSET]

is displayed.

Press soft key [OFFSET] or [EXTEND OFFSET] to display the offset screen or 4th/5th axis offset
screen.

Press soft key [(OPRT)].

Press soft key [F OUTPUT].

Press soft key [EXEC].

The output format used is the absolute tool offset value format based on the G10 command.

•

Example of output data

When the 4th/5th axis offset function are specified, and 32 sets of tool offsets are used

G10 P01 X1.250 Z1.750 R12.254 Y2.250 E2.750 F12.600 ;

⋮

G10 P32 X0.840 Z1.240 R11.435 Y1.640 E2.040 F7.675 ;

G10 P10001 X9.680 Z9.280 R12.224 Y8.880 E8.480 F24.345 ;

⋮

G10 P10032 X9.450 Z9.000 R13.017 Y8.550 E8.100 F10.123 ;

Tool geometry/wear offset values as many as the number of tool offset sets are output.

NOTE

When compared with the G10 format used for output of tool offset values,
address E for indicating a 4th axis offset value and address F for indicating a 5th
axis offset value are added in the output format.

Address name changing of output format

When bit 2 (OFN) of parameter No.11403 is set to 1, the specification address in "Y-axis offset and
4th/5th axis offset" can use address name 'A' or 'B' instead of default specification address 'Y','E'and'F'.

Example) When parameter is set to follow, the address is changed.

Parameter No.5044 is set to 4 (4th axis offset is the 4th axis)

Parameter No.5045 is set to 5 (5th

axis offset is the 5th axis)

Parameter No.1020 (4th

axis ,5th

axis) = 65, 66 (Address name of 4th /5th

axis offset is 'A' and

'B')

B-64604EN-1/01

OPERATION

1.DATA INPUT/OUTPUT

- 313 -

Bit 2 (OFN) of parameter No.11403 is set to 1 (Address depend on parameter No.1020)

G10 P01 X_ Z_ A_ B_

G10 P02 X_ Z_ A_ B_

...

G10 P__ X_ Z_ A_ B_

A_ :

Tool compensation data (4th axis offset value in example).

B_ :

Tool compensation data (5th axis offset value in example).

The other addresses are the same as for the tool compensation amount.

NOTE

1 The axis name that can be used as a specification address is only 'A', and 'B'.

If specification address 'A' or 'B' is used, the address 'V' (incremental command
of Y-axis offset) cannot be used.

2 When setting is the following condition, the default specification addresses 'Y', 'E'

and 'F' are used.
- Parameter No.1020 is set to axis name other than 'A(65)' or 'B(66)'.
- An extended axis name is used.

3 When bit 2 of parameter No.11403 is set to 1, conventional offset data cannot be

read. If conventional offset data is read, Please set 0 to bit 2 (OFN) of parameter
No.11403.

Outputting 4th/5th axis offset data (for 15-inch display unit)

Procedure

Make sure the input device is ready for inputting.

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

Press function key

Press vertical soft key [NEXT PAGE] several times until vertical soft key [OFFSET] or [EXTEND
OFFSET] is displayed.

Press vertical soft key [OFFSET] or [EXTEND OFFSET] to display the offset screen or 4th/5th axis
offset screen.

Press horizontal soft key [F OUTPUT].

Press horizontal soft key [EXEC].

The output format used is the absolute tool offset value format based on the G10 command.

•

Example of output data

When the 4th/5th axis offset function are specified, and 32 sets of tool offsets are used

G10 P01 X1.250 Z1.750 R12.254 Y2.250 E2.750 F12.600 ;

⋮

G10 P32 X0.840 Z1.240 R11.435 Y1.640 E2.040 F7.675 ;

G10 P10001 X9.680 Z9.280 R12.224 Y8.880 E8.480 F24.345 ;

⋮

G10 P10032 X9.450 Z9.000 R13.017 Y8.550 E8.100 F10.123 ;

Tool geometry/wear offset values as many as the number of tool offset sets are output.

1.DATA INPUT/OUTPUT

OPERATION

B-64604EN-1/01

- 314 -

NOTE

Address name changing of output format

When bit 2 of parameter No.11403 is set to 1, the specification address in "Y-axis offset and 4th/5th axis
offset" can use address name 'A' or 'B' instead of default specification addresses 'Y', 'E' and 'F'.

Example) When parameter is set to follow, the address is changed.

No.5044 is set to 4 (4th axis offset is the 4th axis)

No.5045 is set to 5 (5th

axis offset is the 5th axis)

- No.1020

(4th

axis ,5th

axis) = 65, 66 (Address name of 4th /5th

axis offset is 'A' and 'B')

Bit 2 of No.11403 is set to 1 (Address depend on parameter No.1020)

G10 P01 X_ Z_ A_ B_

G10 P02 X_ Z_ A_ B_

...

G10 P__ X_ Z_ A_ B_

A_ :

Tool compensation data (4th axis offset).

B_ :

Tool compensation data (5th axis offset).

The other addresses are the same as for the tool compensation amount.

NOTE

1 The axis name that can be used as a specification address is only 'A', and 'B'.

If specification address 'A' or 'B' is used, the address 'V' (incremental command
of Y-axis offset) cannot be used.

2 When setting is the following condition, the default specification addresses 'Y',

'E', and 'F' are used.
- Parameter No.1020 is set to axis name other than 'A(65)' or 'B(66)'.
- An extended axis name is used.

3 When bit 2 of parameter No.11403 is set to 1, conventional offset data cannot be

read. If conventional offset data is read, Please set 0 to bit 2 of parameter
No.11403.

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

Press function key

Press the continuous menu key

several times until soft key [ALL IO] is displayed.

FANUC Series 0i-MODEL F. For Lathe System OPERATOR'S MANUAL (B-64604EN-1/01) - page 20