FANUC Series 0i-MODEL F Plus. CONNECTION MANUAL (FUNCTION)

12. PROGRAM COMMAND

B-64693EN-1/01

- 2130 -

NOTE

A check for a monotonous figure is made at all times during G71
and G72 or G71.7 and G72.7 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, G72,
G71.7, or G72.7 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.

Alarm and message

Number

Message

Description

PS0061

P OR Q COMMAND IS NOT IN THE
MULTIPLE REPETIVE CYCLES
BLOCK

Address P or Q is not specified in multiple repetitive cycle
(G70, G71, G72, or G73) command.

PS0062

THE CUTTING AMOUNT IS
ILLEGAL IN THE ROUGH CUTTING
CYCLE

A zero or a negative value was specified in a multiple
repetitive canned rough-cutting cycle (G71 or G72) as the
depth of cut.

PS0063

THE BLOCK OF A SPECIFIED
SEQUENCE NUMBER IS NOT
FOUND

The sequence number specified by addresses P and Q in
multiple repetitive cycle (G70, G71, G72, or G73) command
cannot be searched.

PS0064

THE FINISHING SHAPE IS NOT A
MONOTONOUS CHANGE(FIRST
AXES)

In a shape program for the multiple repetitive canned
rough-cutting cycle (G71 or G72), the command for the first
plane axis was not a monotonous increase or decrease.

PS0065

G00/G01 IS NOT IN THE FIRST
BLOCK OF SHAPE PROGRAM

In the first block of the shape program specified by P of the
multiple repetitive canned cycle (G70, G71, G72, or G73),
G00 or G01 was not specified.

PS0066

UNAVAILABLE COMMAND IS IN
THE MULTIPLE REPETIVE CYCLES
BLOCK

An unavailable command was found in a multiple repetitive
canned cycle (G70, G71, G72, or G73) command block.

PS0067

THE MULTIPLE REPETIVE CYCLES
IS NOT IN THE PART PROGRAM
STORAGE

A multiple repetitive canned cycle (G70, G71, G72, or G73)
command is not registered in a tape memory area.

PS0069

LAST BLOCK OF SHAPE
PROGRAM IS AN ILLEGAL
COMMAND

In a shape program in the multiple repetitive canned cycle
(G70, G71, G72, or G73), a command for the chamfering or
corner R in the last block is terminated in the middle.

PS0315

ILLEGAL NOSE ANGLE COMMAND
IS IN THE THREAD CUTTING
CYCLE

An invalid tool tip angle is specified in a multiple repetitive
canned threading cycle (G76).

PS0316

ILLEGAL CUTTING AMOUNT IS IN
THE THREAD CUTTING CYCLE

A minimum depth of cut higher than the thread height is
specified in a multiple repetitive canned threading cycle (G76).

PS0317

ILLEGAL THREAD COMMAND IS IN
THE THREAD CUTTING CYCLE

A zero or a negative value is specified in a multiple repetitive
canned threading cycle (G76) as the thread height or the
depth of cut.

PS0318

ILLEGAL RELIEF AMOUNT IS IN
THE DRILLING CYCLE

Although an escape directions is set in a multiple repetitive
canned cutting-off cycle (G74 or G75), a negative value is
specified for Δd.

PS0319

THE END POINT COMMAND IS
ILLEGAL IN THE DRILLING CYCLE

Although the Δi or Δk travel distance is set to 0 in a multiple
repetitive canned cutting-off cycle (G74 or G75), a value other
than 0 is specified for a U or W.

PS0320

ILLEGAL MOVEMENT
AMOUNT/CUTTING AMOUNT IS IN
THE DRILLING CYCLE

A negative value is specified in a multiple repetitive canned
cutting-

off cycle (G74 or G75) as Δi or Δk (travel distance/the

depth of cut).

B-64693EN-1/01

12. PROGRAM COMMAND

- 2131 -

Number

Message

Description

PS0321

ILLEGAL REPEATED TIME IS IN
THE PATTERN REPEATING CYCLE

A zero or a negative value is specified in a multiple repetitive
canned closed loop cycle (G73) as a repeated time.

PS0322

FINISHING SHAPE WHICH OVER
OF STARTING POINT

An invalid shape which is over the cycle starting point is
specified in a shape program for a multiple repetitive canned
rough-cutting cycle (G71 or G72).

PS0323

THE FIRST BLOCK OF SHAPE
PROGRAM IS A COMMAND OF
TYPE II

Type II is specified in the first block of the shape program
specified by P in a multiple repetitive canned rough-cutting
cycle (G71 or G72). Z (W) command is for G71.
X (U) command is for G72.

PS0324

THE INTERRUPTION TYPE MACRO
WAS DONE IN THE MULTIPLE
REPETIVE CYCLES

An interruption type macro was issued during the multiple
repetitive canned cycle (G70, G71, G72, or G73).

PS0325

UNAVAILABLE COMMAND IS IN
SHAPE PROGRAM

1) Unusable command was issued in a shape program for a

multiple repetitive cycle (G70, G71, G72, or G73).

2) In the multiple repetitive cycle (G70), when the tool nose

radius compensation can be commanded in the target
figure program (parameter NT2(No.5106#3)=1), G41 or
G42 is commanded at the target figure program other
than the first block.

PS0326

LAST BLOCK OF SHAPE
PROGRAM IS A DIRECT DRAWING
DIMENSIONS

In a shape program in the multiple repetitive canned cycle
(G70, G71, G72, or G73), a command for direct input of
drawing dimensions in the last block is terminated in the
middle.

PS0327

MODAL THAT MULTIPLE
REPETIVE CYCLES CANNOT BE
DONE

A multiple repetitive canned cycle (G70, G71, G72, or G73)
was commanded in a modal state in which a multiple
repetitive canned cycle could not be commanded.

PS0328

ILLEGAL WORK POSITION IS IN
THE TOOL NOSE RADIUS
COMPENSATION

The specification for the blank side for a tool nose radius
compensation (G41 or G42) is incorrect in a multiple repetitive
canned cycle (G71 or G72).

PS0329

THE FINISHING SHAPE IS NOT A
MONOTONOUS CHANGE(SECOND
AXES)

In a shape program for the multiple repetitive canned
rough-cutting cycle (G71 or G72), the command of the second
plane axis was not a monotonous increase or decrease.

PS0330

ILLEGAL AXIS COMMAND IS IN
THE TURNING CANNED CYCLE

An axis other than the plane is specified n a canned
cycle(G90, G92, or G94).

Reference item

Manual name

Item name

OPERATOR’S MANUAL (B-64694EN)

Cutting feed

OPERATOR’S MANUAL For Lathe
System (B-64694EN-1)

Threading (G32)
Multiple threading
Canned cycle
Multiple repetitive canned cycle

OPERATOR’S MANUAL For Machining
Center System (B-64694EN-2)

Threading (G33)

Multiple threading

Multiple repetitive canned cycle

12.8.2

Reducing path for Multiple repetitive canned cycle

Overview

In multiple repetitive canned cycle, a path of cycle can be reduced.

12. PROGRAM COMMAND

B-64693EN-1/01

- 2132 -

Explanation

In stock removal in turning (G71, G71.7) of multiple repetitive canned cycle, conventional path was as
follows (Fig. 12.8.2 (a)Fig. 12.8.2 (a)Fig. 12.8.2 (a)).

1. Moving in the direction of the first axis on the plane (Z-axis for the ZX plane)
2. Moving in the direction of the second axis on the plane (X-axis for the ZX plane)

In this function, it directly moves from the retraction end point to the last turning start point (Fig. 12.8.2
(b), Fig. 12.8.2 (c)).
The cycle time can be reduced because moving path is reduced.
To use this function, set bit 6 (RPA) of parameter No. 5125 to 1.

Fig. 12.8.2 (a) Conventional operation

Movement from retraction end point to last turning start point

In a start block in the program for a target figure, the movement from the retraction end point to the last
turning start point is changed.

When a start block in the program for a target figure is G00 :
Axes move from the retraction end point to the last turning start point by rapid traverse.

Fig. 12.8.2 (b) Operation when this function is effective (Start block in the program for a target figure is G00.)

When a start block in the program for a target figure is G01 :
Axes move from the retraction end point by rapid traverse until becoming a value that the distance to the
last turning start point is set to parameter No.5126. These move from there to the last turning start point

Rapid traverse

Cutting feed

R: Retraction end point

C: Turning start point

Rapid traverse

Cutting feed

R: Retraction end point

C: Turning start point

B-64693EN-1/01

12. PROGRAM COMMAND

- 2133 -

by cutting feed. When 0 is set in parameter No.5126, this parameter is the distance that is 50% of
retraction distance.

Fig. 12.8.2 (c) Operation when this function is effective (Start block in the program for a target figure is G01.)

WARNING

Specify G01 in a start block in the program for a target figure when turning start
point is near the processing surface. The distance of cutting can be adjusted by
parameter No.5126.

Effect of reducing cycle time

In this function, it is more effective in reducing cycle time to assume a start block in the program for a
target figure to be G00.
Therefore, it is recommended that turning start point is separated from work piece, and it specifies G00 in
the start block in the program for a target figure.

Limitation

This function is valid only when bit 1 (LRP) of parameter No. 1401 is 1.

This function is valid only in stock removal in turning (G71, G71.7) and stock removal in facing (G72,

G72.7) of multiple repetitive canned cycle.

This function is invalid in type II of multiple repetitive canned cycle.

Parameter

Parameters which are used for this function are as follows.

5125

RPA

[Input type] Parameter input

[Data type] Bit path

#6 RPA

In type I of G71 (T series), G71.7 (M series), G72 (T series) and G72.7 (M series) of

multiple repetitive canned cycle, the axes :
0:

Don’t move directly from retraction end point to the last turning start point.

Move directly from retraction end point to the last turning start point.

Rapid traverse

Cutting feed

R: Retraction end point

C: Turning start point

12. PROGRAM COMMAND

B-64693EN-1/01

- 2134 -

NOTE

When the distance to the last turning start point reaches the value
of the parameter No.5126, the movement of the axis changes from
rapid traverse to cutting feed.

5126

Distance in which cutting to the last turning start point

in multiple repetitive canned cycles G71 and G72

Distance in which cutting to the last turning start point

in multiple repetitive canned cycles G71.7 and G72.7

[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 retraction distance

In type I of G71 (T series), G71.7 (M series), G72 (T series) and G72.7 (M series) of
multiple repetitive canned cycle, the distance in which cutting to the last turning start
point is set to this parameter. When 0 is set in parameter No.5126, this parameter is the
distance that is 50% of retraction distance.
When the setting value is out of range, this parameter is the distance in which cutting to
the last turning start point is the same distance as retraction distance.

NOTE

This parameter is valid when bit 6 (RPA) of parameter No. 5125 is
set to 1 and start block in the program for a target figure is G01.

12.9

IN-FEED CONTROL (FOR GRINDING MACHINE)

Overview

Each time an external signal is input at the table swing end point, a workpiece is cut by a constant depth
of cut along a programmed figure on the specified Y-Z plane. This makes it possible to perform grinding
and cutting in a timely manner and facilitating the grinding of a workpiece with a profile.

•

(2)

(3)

(1) (4)

•

External

signal input

X=0

Sensor placement

X=a

B-64693EN-1/01

12. PROGRAM COMMAND

- 2135 -

For example, it is possible to machine a workpiece with a profile programmed with linear interpolation,
circular interpolation, and linear interpolation on the YZ plane, such as that shown in the figure above.
A sensor is placed at a X = 0 position so that the external signal is input when the sensor detects the
grinding wheel. When the program is started at point A, the machine is first placed in the state in which it
waits for the input of the external signal. Then, when the sensor detects the grinding wheel, the external
signal is input, and the machine makes a cut by the constant amount

along the programmed profile on

the specified YZ plane and moves to point B (operation (1)). The machine is then placed in the state in
which it waits for the input of the external signal again, and performs a grinding operation along the
X-axis. It grinds from point B to point C (operation (2)) and grinds back from point C to point B
(operation (3)). When the machine returns to point B, the sensor detects the grinding wheel again, and the
external signal is input, so that the machine makes a cut by the amount of

and moves to point D

(operation (4)). At point D, the machine performs a grinding operation along the X-axis.
Afterwards, each time the external signal is input, the machine makes a cut by the amount of

along the

profile program, so that the workpiece is machined to a profile such as that shown in the figure above.

Signal

In-feed control cut start signal INFD<Gn063.6>

[Classification] Input signal

[Function] Exercises in-feed control.

[Operation] When this signal is set from 0 to 1, the control unit operates as follows:

A movement is made by a specified depth of cut along a program figure.

Signal address

Gn063

INFD

Alarm and message

Number

Message

Description

PS0230

R CODE NOT FOUND

Cut depth R is not specified in the block including G161.
Alternatively, the value specified for R is negative.
Modify the program.

Reference item

Manual name

Item name

OPERATOR’S MANUAL (For Machining Center System)
(B-64694EN-2)

In-feed control (for grinding machine)

12.10

CANNED GRINDING CYCLE (FOR GRINDING MACHINE)

Overview

With the canned grinding cycle, repetitive machining operations that are specific to grinding and are
usually specified using several blocks can be specified using one block including a G function. So, a
program can be created simply. At the same time, the size of a program can be reduced, and the memory
can be used more efficiently. Four types of canned grinding cycles are available:

Traverse grinding cycle

Traverse direct constant-size grinding cycle

Oscillation grinding cycle

Oscillation direct constant-size grinding cycle

12. PROGRAM COMMAND

B-64693EN-1/01

- 2136 -

Plunge grinding cycle

Direct constant-dimension plunge grinding cycle

Continuous-feed surface grinding cycle

Intermittent-feed surface grinding cycle

Parameter

5101

FXY

[Input type] Parameter input

[Data type] Bit path

#0 FXY

The drilling axis in the drilling canned cycle, or cutting axis in the grinding canned cycle

is:
0:

In case of the Drilling canned cycle:

Z-axis at all times.

In case of the Grinding canned cycle:

For the Lathe system

Z-axis at all times.

For the Machining Center system

G75,G77 command :Y-axis

G78,G79 command :Z-axis

Axis perpendicular to a specified plane (G17/G18/G19).

NOTE

In the case of the T series, this parameter is valid only for the
drilling canned cycle in the Series 15 format.

5105

GIJ

[Input type] Parameter input

[Data type] Bit path

#6 GIJ

When a grinding canned cycle in the machining center system is executed, if the signs of

I, J, and K are different:
0:

An alarm is issued.

An operation compatible with the FS16i is performed.

5106

GFX

[Input type] Parameter input

[Data type] Bit path

NOTE

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

B-64693EN-1/01

12. PROGRAM COMMAND

- 2137 -

#0 GFX

When the function of multiple respective canned cycle and grinding canned cycle are

both active, G71/G72/G73/G74 commands are:
0:

Multiple repetitive canned cycle.

Grinding canned cycle.

5176

Grinding axis number in Traverse Grinding Cycle(G71)

Grinding axis number in Plunge Grinding Cycle(G75)

[Input type] Parameter input

[Data type] Byte path

[Valid data range] 0 to Number of controlled axes

For the Lathe system:

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

For the Machining Center system:

Set the Grinding axis number of Plunge Grinding Cycle(G75).

NOTE

The axis number except for the cutting axis can be specified. When
the axis number which is same to cutting axis is specified, an alarm
PS0456 is issued at the time of execution. The Grinding Cycle is
executed when this parameter value is 0, the alarm PS0456 is also
issued.

5177

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

Grinding axis number of Direct Constant Dimension Plunge Grinding Cycle(G77)

[Input type] Parameter input

[Data type] Byte path

[Valid data range] 0 to Number of controlled axes

For the Lathe system:

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

For the Machining Center system:

Set the Grinding axis number of Direct Constant Dimension Plunge Grinding Cycle
(G77).

NOTE

5178

Grinding axis number of Oscillation Grinding Cycle(G73)

Grinding axis number of Continuous feed surface grinding cycle(G78)

[Input type] Parameter input

[Data type] Byte path

[Valid data range] 0 to Number of controlled axes

For the Lathe system:

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

For the Machining Center system:

Set the Grinding axis number of Continuous feed surface grinding cycle(G78).

FANUC Series 0i-MODEL F Plus. CONNECTION MANUAL (FUNCTION) - page 272