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

B-64604EN-1/01

APPENDIX

A.PARAMETERS

- 381 -

NOTE

When a roughing allowance (

k) is specified using the Series

10/11 program format, roughing is performed, regardless of the
setting of this parameter.

#3 M5T

When the rotation direction of the spindle is changed from forward rotation to reverse

rotation or from reserve rotation to forward rotation in a tapping cycle (G84/G88):
0: M05 is output before output of M04 or M03.
1: M05 is not output before output of M04 or M03.

#7 #6 #5 #4 #3 #2 #1 #0

5106

NT2

NT1

[Input type] Parameter input

[Data type] Bit path

NOTE

When this parameter is set, the power must be turned off before
operation is continued.

#2 NT1

In the multiple repetitive cycle G71/G72/G73 (G-code system A), when the tool nose

radius compensation G40/G41/G42 is commanded in the target figure program:
0: The alarm PS0325, “UNAVAILABLE COMMAND IS IN SHAPE PROGRAM” is

occurred.

1: No alarm is occurred. However, the tool nose radius compensation command in the

target figure program is ignored.

#3 NT2

In the multiple repetitive cycle G70 (G-code system A), when the tool nose radius

compensation G40/G41/G42 is commanded in the target figure program:
0: The alarm PS0325 is occurred.
1: No alarm is occurred. The tool nose radius compensation command is valid.

NOTE

Make the program by following ways to enable the tool nose radius
compensation in the finishing cycle G70 by commanded the tool
nose radius compensation in the target figure program.
- The tool nose radius compensation cancel G40 is selected as

the modal when the finishing cycle G70 is commanded.

- Command G41/G42 at the first block of the target figure

program (commanded by P address).

- Command G40 at the last block of the target figure program

(commanded by Q address).

#7 #6 #5 #4 #3 #2 #1 #0

5108

NSP

DTP

R16

[Input type] Parameter input

[Data type] Bit path

A.PARAMETERS

APPENDIX

B-64604EN-1/01

- 382 -

#0 R16

In the cutting up movement of the multiple repetitive cycle G71/G72 (G-code system A)

of type

Ⅱ

, if there is the block that commands just the movement of the first axis on the

plane in the finishing shape:
0: The cutting up movement is executed before the cutting of the first axis on the plane.
1: The cutting up movement is not executed and the cutting is continued along the

finishing shape of the first axis on the plane.

#1 DTP

In the multiple repetitive cycle G71/G72 (G-code system A) of type

Ⅰ

, after rough

cutting of the finishing shape program is finished, the tool return to the cycle start point:
0: After the tool moves to (cycle start point + distance of the finishing allowance) in

order X-axis, Z-axis.

1: Directly from the end point of the finishing program.

#3 NSP

In the multiple repetitive cycle G71/G72 (G-code system A) of type

Ⅱ

, the cutting is

executed:
0: By conventional path. (The same cutting path might be executed.)
1: Not to repeat the same cutting path.

5110

M code for C-axis clamping in canned cycles for drilling

[Input type] Parameter input

[Data type] 2-word path

[Valid data range] 0 to 99999998

This parameter sets the M code for C-axis clamping in canned cycles for drilling.

NOTE

When bit 4 (CME) of parameter No. 5161 is 1, the M code for
C-axis clamping for the first pair is assumed.

5111

Dwell time when C-axis unclamping is specified in drilling canned cycle

[Input type] Parameter input

[Data type] 2-word path

[Valid data range] 0 to 32767

[Unit of data]

Increment system

IS-A

IS-B

IS-C

Unit

0.1

msec

(The increment system does not depend on whether inch input or metric input is used.)

This parameter sets the dwell time when C-axis unclamping is specified in a drilling
canned cycle.

5114

Return value of high-speed peck drilling cycle

[Input type] Parameter input

[Data type] Real path

[Unit of data] mm, inch (input unit)

[Min. unit of data] Depend on the increment system of the reference axis

B-64604EN-1/01

APPENDIX

A.PARAMETERS

- 383 -

[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting table (A))

(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets the return value in high-speed peck drilling cycle.

G83 (when the bit 2 (RTR) of parameter No. 5101 is set to 0)

5115

Clearance value in a peck drilling cycle

[Input type] Parameter input

[Data type] Real path

[Unit of data] mm, inch (input unit)

[Min. unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting table (A))

(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets a clearance value in a peck drilling cycle.

G83 (when the bit 2 (RTR) of parameter No. 5101 is set to 1)

#7 #6 #5 #4 #3 #2 #1 #0

5125

PRS

[Input type] Parameter input

[Data type] Bit path

PRS In Pattern repeating cycle G73 (G-code system A), the stop position of single block

operation are:
0: The end point of each cycles and the end point of each blocks in the finishing shape.
1: The end point of each cycles and the end point of escape from the cycle start point.

(FS16i compatible specification)

5130

Cutting value (chamfering value) in thread cutting cycles G92 and G76

[Input type] Parameter input

[Data type] Byte path

q : Depth of cut
d : Clearance value

R point

Z point

q : Depth of cut
d : Return value

R point

Z point

A.PARAMETERS

APPENDIX

B-64604EN-1/01

- 384 -

[Unit of data] 0.1

[Valid data range] 0 to 127

This parameter sets a cutting value (chamfering value) in the thread cutting cycle (G76)
of a multiple repetitive canned cycle and in the thread cutting cycle (G92) of a canned
cycle.
Let L b a lead. Then, a cutting value range from 0.1L to 12.7L is allowed.
To specify a cutting value of 10.0L, for example, specify 100 in this parameter.

5131

Cutting angle in thread cutting cycles G92 and G76

[Input type] Parameter input

[Data type] Byte path

[Unit of data] Degree

[Valid data range] 1 to 89

This parameter sets a thread cutting angle in a thread cutting cycle (G92/G76).
When 0 is set, an angle of 45 degrees is specified.

5132

Depth of cut in multiple repetitive canned cycles G71 and G72

[Input type] Parameter input

[Data type] Real path

[Unit of data] mm, inch (input unit)

[Min. unit of data] Depend on the increment system of the reference axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard parameter setting table

(B))
(When the increment system is IS-B, 0.0 to +999999.999)
This parameter sets the depth of cut in multiple repetitive canned cycles G71 and G72.
This parameter is not used with the Series 10/11 program format.

NOTE

Specify a radius value at all times.

5133

Escape in multiple repetitive canned cycles G71 and G72

[Input type] Parameter input

[Data type] Real path

[Unit of data] mm, inch (input unit)

[Min. unit of data] Depend on the increment system of the reference axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard parameter setting table

(B))
(When the increment system is IS-B, 0.0 to +999999.999)
This parameter sets the escape in multiple repetitive canned cycles G71 and G72.

NOTE

Specify a radius value at all times.

5134

Clearance value in multiple repetitive canned cycles G71 and G72

[Input type] Parameter input

[Data type] Real path

[Unit of data] mm, inch (input unit)

[Min. unit of data] Depend on the increment system of the reference axis

B-64604EN-1/01

APPENDIX

A.PARAMETERS

- 385 -

[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard parameter setting table

(B))
(When the increment system is IS-B, 0.0 to +999999.999)
This parameter sets a clearance value up to the cutting feed start point in multiple
repetitive canned cycles (G71/G72).

NOTE

Specify a radius value at all times.

5135

Retraction distance in the multiple repetitive canned cycle G73 (second axis on the plane)

[Input type] Parameter input

[Data type] Real path

[Unit of data] mm, inch (input unit)

[Min. unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting table (A))

(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets a retraction distance along the second axis on the plane in the
multiple repetitive canned cycle G73. This parameter is not used with the Series 10/11
program format.

NOTE

Specify a radius value at all times.

5136

Retraction distance in the multiple repetitive canned cycle G73 (first axis on the plane)

[Input type] Parameter input

[Data type] Real path

[Unit of data] mm, inch (input unit)

[Min. unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting table (A))

(When the increment system is IS-B, -999999.999 to +999999.999)
This parameter sets a retraction distance along the first axis on the plane in the multiple
repetitive canned cycle G73. This parameter is not used with the Series 10/11 program
format.

NOTE

Specify a radius value at all times.

5137

Number of divisions in the multiple repetitive canned cycle G73

[Input type] Parameter input

[Data type] 2-word path

[Unit of data] Cycle

[Valid data range] 1 to 99999999

This parameter sets the number of divisions in the multiple repetitive canned cycle G73.
This parameter is not used with the Series 10/11 program format.

5139

Return in multiple repetitive canned cycles G74 and G75

[Input type] Parameter input

[Data type] Real path

[Unit of data] mm, inch (input unit)

A.PARAMETERS

APPENDIX

B-64604EN-1/01

- 386 -

[Min. unit of data] Depend on the increment system of the reference axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard parameter setting table

(B))
(When the increment system is IS-B, 0.0 to +999999.999)
This parameter sets the return in multiple repetitive canned cycles G74 and G75.

NOTE

Specify a radius value at all times.

5140

Minimum depth of cut in the multiple repetitive canned cycle G76

[Input type] Parameter input

[Data type] Real path

[Unit of data] mm, inch (input unit)

[Min. unit of data] Depend on the increment system of the reference axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard parameter setting table

(B))
(When the increment system is IS-B, 0.0 to +999999.999)
This parameter sets a minimum depth of cut in the multiple repetitive canned cycle G76
so that the depth of cut does not become too small when the depth of cut is constant.

NOTE

Specify a radius value at all times.

5141

Finishing allowance in the multiple repetitive canned cycle G76

[Input type] Parameter input

[Data type] Real path

[Unit of data] mm, inch (input unit)

[Min. unit of data] Depend on the increment system of the reference axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard parameter setting table

(B))
(When the increment system is IS-B, 0.0 to +999999.999)
This parameter sets the finishing allowance in multiple repetitive canned cycle G76.

NOTE

Specify a radius value at all times.

5142

Repetition count of final finishing in multiple repetitive canned cycle G76

[Input type] Parameter input

[Data type] 2-word path

[Unit of data] Cycle

[Valid data range] 1 to 99999999

This parameter sets the number of final finishing cycle repeats in the multiple repetitive
canned cycle G76.
When 0 is set, only one final finishing cycle is executed.

5143

Tool nose angle in multiple repetitive canned cycle G76

[Input type] Parameter input

[Data type] Byte path

[Unit of data] Degree

B-64604EN-1/01

APPENDIX

A.PARAMETERS

- 387 -

[Valid data range] 0, 29, 30, 55, 60, 80

This parameter sets the tool nose angle in multiple repetitive canned cycle G76.
This parameter is not used with the Series 10/11 program format.

5145

Allowable value 1 in multiple repetitive canned cycles G71 and G72

[Input type] Parameter input

[Data type] Real path

[Unit of data] mm, inch (input unit)

[Min. unit of data] Depend on the increment system of the reference axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard parameter setting table

(B))
(When the increment system is IS-B, 0.0 to +999999.999)
If a monotonous command of type I or II is not specified for the axis in the roughing
direction, the alarm PS0064, “THE FINISHING SHAPE IS NOT A MONOTONOUS
CHANGE(FIRST AXES)” or PS0329, “THE FINISHING SHAPE IS NOTA
MONOTONOUS CHANGE(SECOND AXES)” is issued. When a program is created
automatically, a very small unmonotonous figure may be produced. Set an unsigned
allowable value for such an unmonotonous figure. By doing so, G71 and G72 cycles can
be executed even in a program including an unmonotonous figure.

[Example] Suppose that a G71 command where the direction of the cutting axis (X-axis) is minus

and the direction of the roughing axis (Z-axis) is minus is specified. In such a case, when
an unmonotonous command for moving 0.001 mm in the plus direction along the Z-axis
is specified in a target figure program, roughing can be performed according to the
programmed figure without an alarm by setting 0.001 mm in this parameter.

NOTE

A check for a monotonous figure is made at all times during G71
and G72 cycles. A figure (programmed path) is checked. When tool
nose radius compensation is performed, a path after compensation
is checked. When bit 2 (FCK) of parameter No. 5104 is set to 1, a
check is made before G71 or G72 cycle operation. In this case, not
a path after tool nose radius compensation but a programmed path
is checked.

Note that no alarm is issued when an allowable value is set.

Use a radius value to set this parameter at all times.

5146

Allowable value 2 in multiple repetitive canned cycles G71 and G72

[Input type] Parameter input

[Data type] Real path

[Unit of data] mm, inch (input unit)

[Min. unit of data] Depend on the increment system of the reference axis
[Valid data range] 0 to cut of depth

If a monotonous command of type I is not specified for the axis in the cutting direction,
the alarm PS0064, “THE FINISHING SHAPE IS NOT A MONOTONOUS
CHANGE(FIRST AXES)” or PS0329, “THE FINISHING SHAPE IS NOTA
MONOTONOUS CHANGE(SECOND AXES)” is issued.
When a program is created automatically, a very small unmonotonous figure may be
produced. Set an unsigned allowable value for such an unmonotonous figure. By doing so,
G71 and G72 cycles can be executed even in a program including an unmonotonous
figure.
The allowable value is clamped to the depth of cut specified by a multiple repetitive
canned cycle.

A.PARAMETERS

APPENDIX

B-64604EN-1/01

- 388 -

[Example] Suppose that a G71 command where the direction of the cutting axis (X-axis) is minus

and the direction of the roughing axis (Z-axis) is minus is specified. In such a case, when
an unmonotonous command for moving 0.001 mm in the minus direction along the
X-axis is specified in a target figure program for moving from the bottom of cutting to the
end point, roughing can be performed according to the programmed figure without an
alarm by setting 0.001 mm in this parameter.

NOTE

Note that no alarm is issued when an allowable value is set.

Use a radius value to set this parameter at all times.

#7 #6 #5 #4 #3 #2 #1 #0

5161

CME

[Input type] Parameter input

[Data type] Bit path

#4 CME

For drilling canned cycles, the M code for C-axis clamping/unclamping is set to:

0: Value set by parameter No. 5110/value set by parameter No. 5110 + 1.
1: Value set by parameter No. 5110/value set by parameter No. 13543 (first pair), or

the value set by parameter No. 13544/value set by parameter No. 13545 (second
pair).

5176

Grinding axis number in Traverse Grinding Cycle(G71)

[Input type] Parameter input

[Data type] Byte path

[Valid data range] 0 to Number of controlled axes

Set the Grinding axis number of Traverse Grinding Cycle(G71).

5177

Grinding axis number of Traverse direct constant-size Grinding cycle(G72)

[Input type] Parameter input

[Data type] Byte path

[Valid data range] 0 to Number of controlled axes

Set the Grinding axis number of Traverse direct constant-size Grinding cycle(G72).

5178

Grinding axis number of Oscillation Grinding Cycle(G73)

[Input type] Parameter input

[Data type] Byte path

[Valid data range] 0 to Number of controlled axes

Set the Grinding axis number of Oscillation Grinding Cycle(G73).

5179

Grinding axis number of Oscillation Direct Fixed Dimension Grinding Cycle(G74)

[Input type] Parameter input

B-64604EN-1/01

APPENDIX

A.PARAMETERS

- 389 -

[Data type] Byte path

[Valid data range] 0 to Number of controlled axes

Set the Grinding axis number of Oscillation Direct Fixed Dimension Grinding
Cycle(G74).

#7 #6 #5 #4 #3 #2 #1 #0

5200

FHD PCP DOV

G84

[Input type] Parameter input

[Data type] Bit path

#0 G84

Method for specifying rigid tapping:

0: An M code specifying the rigid tapping mode is specified prior to the issue of the

G84 (or G74) command. (See parameter No. 5210).

1: An M code specifying the rigid tapping mode is not used. (G84 cannot be used as a

G code for the tapping cycle; G74 cannot be used for the reverse tapping cycle.)

#4 DOV

Override during extraction in rigid tapping:

0: Invalidated
1: Validated (The override value is set in parameter No. 5211. However, set an

override value for rigid tapping return in parameter No. 5381.)

#5 PCP

Address Q is specified in a tapping cycle/Rigid tapping:

0: A high-speed peck tapping cycle is assumed.
1: A peck tapping cycle is assumed.

NOTE

In a tapping cycle, this parameter is valid when bit 6 (PCT) of
parameter No. 5104 is 1. When bit 6 (PCT) of parameter No.
5104 is 0, a (high-speed) peck tapping cycle is not assumed.

#6 FHD

Feed hold and single block in rigid tapping:

0: Invalidated
1: Validated

#7 #6 #5 #4 #3 #2 #1 #0

5201

OV3

OVU

[Input type] Parameter input

[Data type] Bit path

#3 OVU

The increment unit of the override parameter No. 5211 for tool rigid tapping extraction is:

0: 1%
1: 10%

#4 OV3

A spindle speed for extraction is programmed, so override for extraction operation is:

0: Disabled.
1: Enabled.

#7 #6 #5 #4 #3 #2 #1 #0

5203

OVS

[Input type] Parameter input

[Data type] Bit path

A.PARAMETERS

APPENDIX

B-64604EN-1/01

- 390 -

#4 OVS

In rigid tapping, override by the feedrate override select signal and cancellation of

override by the override cancel signal is:
0: Disabled.
1: Enabled.
When feedrate override is enabled, extraction override is disabled.
The spindle override is clamped to 100% during rigid tapping, regardless of the setting of
this parameter.

#7 #6 #5 #4 #3 #2 #1 #0

5209

DWP

RTX

[Input type] Parameter input

[Data type] Bit path

#0 RTX

In rigid tapping in a lathe system, the tapping axis is:

0: Selected by selecting a plane.
1: Always assumed to be the Z-axis for G84 or the X-axis for G88.

NOTE

This parameter becomes invalid when bit 1 (FCV) of parameter
No.0001 is set to 1, and rigid tapping is specified using the Series
10/11 program format.

#2 DWP

When a dwell (address P) command is not included in a block for lathe-system rigid

tapping:
0: Dwelling at the bottom of a hole is not performed.
1: The dwell (address P) command specified in the block for drilling is valid.

NOTE

This parameter becomes invalid if rigid tapping is specified in the
Series 10/11 program format with bit 1 (FCV) of parameter No.
0001 set to 1.

5211

Override value during rigid tapping extraction

[Input type] Parameter input

[Data type] Word path

[Unit of data] 1% or 10%

[Valid data range] 0 to 200

The parameter sets the override value during rigid tapping extraction.

NOTE

The override value is valid when bit 4 (DOV) of parameter No. 5200
is set to 1. When bit 3 (OVU) of parameter No. 5201 is set to 1, the
unit of set data is 10%. An override of up to 2000% can be applied to
extraction.

5213

Return in peck rigid tapping cycle

[Input type] Setting input

[Data type] Real path

[Unit of data] mm, inch (input unit)

B-64604EN-1/01

APPENDIX

A.PARAMETERS

- 391 -

[Min. unit of data] Depend on the increment system of the drilling axis
[Valid data range] 0 or positive 9 digit of minimum unit of data (refer to the standard parameter setting table

(B))
(When the increment system is IS-B, 0.0 to +999999.999)
This parameter sets the escape value of a high-speed peck tapping cycle or the clearance
value of a peck tapping cycle.

When the parameter PCP (bit 5 of No.5200) is
set to 0.

When the parameter PCP (bit 5 of No.5200)
is set to 1.

q : Depth of cut

d : Return value

R point

Z point

q : Depth of cut

d : Clearance value

R point

Z point

NOTE

1 In a tapping cycle, this parameter is valid when bit 6 (PCT) of

parameter No. 5104 is 1.

2 For the diameter axis, set this parameter using the diameter value.

5241

Maximum spindle speed in rigid tapping (first gear)

5242

Maximum spindle speed in rigid tapping (second gear)

5243

Maximum spindle speed in rigid tapping (third gear)

5244

Maximum spindle speed in rigid tapping (fourth gear)

[Input type] Parameter input

[Data type] 2-word spindle

[Unit of data] min

-1

[Valid data range] 0 to 9999

Spindle position coder gear ratio
1 : 1    0 to 7400
1 : 2    0 to 9999
1 : 4    0 to 9999
1 : 8    0 to 9999
Each of these parameters is used to set a maximum spindle speed for each gear in rigid
tapping.
Set the same value for both parameter No. 5241 and parameter No. 5243 for a one-stage
gear system. For a two-stage gear system, set the same value as set in parameter No. 5242
in parameter No. 5243. Otherwise, alarm PS0200, “ILLEGAL S CODE COMMAND”
will be issued.

5321

Spindle backlash in rigid tapping (first-stage gear)

5322

Spindle backlash in rigid tapping (second-stage gear)

A.PARAMETERS

APPENDIX

B-64604EN-1/01

- 392 -

5323

Spindle backlash in rigid tapping (third-stage gear)

5324

Spindle backlash in rigid tapping (fourth-stage gear)

[Input type] Parameter input

[Data type] Word spindle

[Unit of data] Detection unit

[Valid data range] -9999 to 9999

Each of these parameters is used to set a spindle backlash.

#7 #6 #5 #4 #3 #2 #1 #0

5400

RIN

[Input type] Parameter input

[Data type] Bit path

#0 RIN

Coordinate rotation angle command (R) :

0: Specified by an absolute method
1: Specified by an absolute method (G90) or incremental method (G91)

5410

Angular displacement used when no angular displacement is specified for coordinate system rotation

[Input type] Setting input

[Data type] 2-word path

[Unit of data] 0.001 degree

[Valid data range] -360000 to 360000

This parameter sets the angular displacement for coordinate system rotation. When the
angular displacement for coordinate system rotation is not specified with address R in the
block where G68 is specified, the setting of this parameter is used as the angular
displacement for coordinate system rotation.

#7 #6 #5 #4 #3 #2 #1 #0

5431

MDL

[Input type] Parameter input

[Data type] Bit path

#0 MDL

The G60 code (single direction positioning) is:

0: One-shot G code (group 00).
1: Modal G code (group 01).

#7 #6 #5 #4 #3 #2 #1 #0

5450

PLS

[Input type] Parameter input

[Data type] Bit path

#2 PLS

The polar coordinate interpolation shift function is:

0: Not

used.

1: Used.
This enables machining using the workpiece coordinate system with a desired point
which is not the center of the rotation axis set as the origin of the coordinate system in
polar coordinate interpolation.

B-64604EN-1/01

APPENDIX

A.PARAMETERS

- 393 -

5460

Axis (linear axis) specification for polar coordinate interpolation

[Input type] Parameter input

[Data type] Byte path

[Valid data range] 1 to number of controlled axes

This parameter sets control axis numbers of linear axis to execute polar interpolation.

5461

Axis (rotation axis) specification for polar coordinate interpolation

[Input type] Parameter input

[Data type] Byte path

[Valid data range] 1 to number of controlled axes

This parameter sets control axis numbers of rotation axis to execute polar interpolation.

5463

Automatic override tolerance ratio for polar coordinate interpolation

[Input type] Parameter input

[Data type] Byte path

[Unit of data] %

[Valid data range] 0 to 100

Typical setting: 90% (treated as 90% when set to 0)
Set the tolerance ratio of the fastest cutting feedrate to the speed of the rotation axis
during automatic override of polar coordinate interpolation.

5464

Compensation for error on hypothetical axis of polar coordinate interpolation

[Input type] Parameter input

[Data type] Byte path

[Unit of data] mm, inch (input unit)

[Min. unit of data] Depend on the increment system of the reference axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting table (A))

(For IS-B, -999999.999 to +999999.999)
This parameter is used to set the error if the center of the rotation axis on which polar
coordinate interpolation is performed is not on the X-axis.
If the setting of the parameter is 0, regular polar coordinate interpolation is performed.

#7 #6 #5 #4 #3 #2 #1 #0

6000

HGO

MGO

[Input type] Parameter input

[Data type] Bit path

#1 MGO

When a GOTO statement for specifying custom macro control is executed, a high-speed

branch to 20 sequence numbers executed from the start of the program is:
0: A high-speed branch is not caused to n sequence numbers from the start of the

executed program.

1: A high-speed branch is caused to n sequence numbers from the start of the program.

#4 HGO

When a GOTO statement for specifying custom macro control is executed, a branch to 30

sequence numbers just before the GOTO statement or to up to 10 sequence numbers
saved by a sequence number search previously made with a GOTO statement is:
0:  Not made at high speed.
1:  Made at high speed.

A.PARAMETERS

APPENDIX

B-64604EN-1/01

- 394 -

#7 #6 #5 #4 #3 #2 #1 #0

6240

IGA

[Input type] Parameter input

[Data type] Bit path

#7 IGA

Automatic tool length measurement (M series) or automatic tool compensation (T series)

is:
0: Used.
1: Not

used.

6241

Feedrate during measurement of automatic tool compensation (for the XAE1 and GAE1 signals)

6242

Feedrate during measurement of automatic tool compensation (for the XAE2 and GAE2 signals)

[Input type] Parameter input

[Data type] Real path

[Unit of data] mm/min, inch/min, deg/min (machine unit)

[Min. unit of data] Depend on the increment system of the applied axis
[Valid data range] Refer to the standard parameter setting table (C)

(When the increment system is IS-B, 0.0 to +999000.0)
These parameters set the relevant feedrate during measurement of automatic tool
compensation.

NOTE

When the setting of parameter No. 6242 or 6243 is 0, the setting of
parameter No. 6241 is used.

6251

value on the X axis during automatic tool compensation

6252

value on the Z axis during automatic tool compensation

[Input type] Parameter input

[Data type] 2-word path

[Unit of data] mm, inch, deg (machine unit)

[Min. unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting table (A))

(When the increment system is IS-B, -999999.999 to +999999.999)
These parameters set the relevant

value during automatic tool compensation.

NOTE

When the Reference axis (parameter No.1031) is Diameter
specification, specify the diameter value. When the Reference axis
(parameter No.1031) is Radius specification, specify the radius
value.

6254

value on the X axis during automatic tool compensation

6255

value on the Z axis during automatic tool compensation

[Input type] Parameter input

[Data type] 2-word path

[Unit of data] mm, inch, deg (machine unit)

B-64604EN-1/01

APPENDIX

A.PARAMETERS

- 395 -

[Min. unit of data] Depend on the increment system of the applied axis
[Valid data range] 9 digit of minimum unit of data (refer to standard parameter setting table (A))

(When the increment system is IS-B, -999999.999 to +999999.999)
These parameters set the relevant

value during automatic tool compensation.

NOTE

When the Reference axis (parameter No.1031) is Diameter
specification, specify the diameter value. When the Reference axis
(parameter No.1031) is Radius specification, specify the radius
value.

#7 #6 #5 #4 #3 #2 #1 #0

7600

PLZ

[Input type] Parameter input

[Data type] Bit path

#7 PLZ

Reference position return based on a G28 command on the tool rotation axis for polygon

turning is:
0: Performed in the same sequence as manual reference position return.
1: Performed by positioning using the rapid traverse rate.
The synchronous axis returns to the reference position in the same sequence as the
manual reference position return when no return-to-reference position is performed after
the power is turned on.

#7 #6 #5 #4 #3 #2 #1 #0

7604

PCG

[Input type] Parameter input

[Data type] Bit path

NOTE

When this parameter is set, the power must be turned off before
operation is continued.

#7 PCG

If both the spindle-spindle polygon turning and the polygon turning are specified:

0: Spindle-spindle polygon turning is performed.
1: Either of the functions is enabled depending on the setting of parameter No. 7605.

NOTE

The spindle-spindle polygon turning is enabled, when bit 6 (SPG) of
parameter No. 8133 is 1).

7605

Polygon turning type selection

[Input type] Parameter input

[Data type] Byte path

[Valid data range] 0, 1

If both the spindle-spindle polygon turning and the polygon turning are specified, this
parameter can be used to select one of the functions for use. A type of polygon turning is
selected according to the setting as follows:
0: Polygon machining with two spindles
1: Polygon

turning

A.PARAMETERS

APPENDIX

B-64604EN-1/01

- 396 -

If a value other than 0 or 1 is specified, 0 is assumed.

NOTE

1 The spindle-spindle polygon turning is enabled, when bit 6 (SPG) of

parameter No. 8133 is 1).

2 Before re-setting this parameter, using the PMC window function or

the G10 command, cancel polygon turning (G50.2). In addition,
when re-setting this parameter, using the PMC window function,
use the M code not involving buffering.

7610

Control axis number of tool rotation axis for polygon turning

NOTE

When this parameter is set, the power must be turned off before
operation is continued.

[Input type] Parameter input

[Data type] Byte path

[Valid data range] 1 to number of controlled axes

This parameter sets the control axis number of a rotation tool axis used for polygon
turning.
However, when a G51.2 command is executed by setting 0 in this parameter, operation
stops with the alarm PS0314, “ILLEGAL SETTING OF POLYGONAL AXIS”.

7640

Master axis in spindle-spindle polygon turning

[Input type] Parameter input

[Data type] Byte path

[Valid data range] 0 to Maximum number of controlled axes (Within a path)

This parameter sets the master axis in spindle-spindle polygon turning.

NOTE

1 Spindle-spindle polygon turning is enabled only for serial spindles.
2 When any one of parameters Nos. 7640 and 7641 is set to 0,

polygon turning is performed using the first spindle (master axis)
and the second spindle (polygon synchronous axis) in the path to
which the parameter belongs.

3 When a spindle other than the first serial spindle is used as a

master axis, the multi-spindle control is required to specify an S
command for the master axis.

4 When the PMC window function or G10 command is used to

rewrite this parameter, rewrite this parameter before the block
specifying the spindle-spindle polygon command G51.2. When the
PMC window function is used to rewrite this parameter in the block
immediately before G51.2, specify the rewriting of this parameter
by using an M code (parameter No. 3411 and up) without buffering.

FANUC Series 0i-MODEL F. For Lathe System OPERATOR'S MANUAL (B-64604EN-1/01) - page 25