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

5. AUTOMATIC OPERATION

B-64693EN-1/01

- 906 -

Function name

Search

method

Direct

jump

method

Remarks

Axis synchronous control

In the search method, program restart can be
restarted if the synchronization is always ON. If
on/off of synchronization is changed by M code
etc. in the program, the position of the master
axis and the slave axis might shift after restart.

Synchronous/Composite control

If on/off is changed by M code etc. in the
program, the position of the master axis and
the slave axis might shift after restart.

Superimposed Control

If on/off is changed M code etc. in the program,
the position of the master axis and the slave
axis might shift after restart.

Synchronous/Composite/Superimposed
control by program command

If on/off is changed in the program, the position
of the master axis and the slave axis might shift
after restart.

Flexible synchronization control

See item “Flexible synchronization control”.

Hobbing/Electric gear box

The machining is executed with the function is
invalid after restarted.

Electric gear box 2 pair

Same as the above-mentioned

Electric gear box automatic phase
synchronization

Same as the above-mentioned

Spindle electric gear box

Same as the above-mentioned

Machining condition selecting function

Spindle positioning

The spindle must be positioned to the restart
position by MDI operation in advance.

Cs contouring control

See item “Cs contour control” for details when
the search method is selected.

Spindle speed fluctuation detection

Spindle synchronous control

Live tool control with servo motor

Servo/spindle synchronous control

Macro executor

A program cannot be restarted from a block in
an execution macro.

Tool radius / Tool nose radius compensation

When bit 4 (INT) of parameter No. 13117 is set to 1, the interference check on cutter/tool nose radius
compensation can be disabled during search by search method.

Cs contour control

For details, see Item, “Cs contour controlled” in Section, “PROGRAM RESTART”.

Flexible synchronization control

Setting bit 0 (FRS) of parameter No. 13421 to 1 enables program restart by search method in a program
containing an M code for turning the flexible synchronization mode on or off.
1.

Before starting program restart, set the flexible synchronization control mode selection signal MTA
<Gn197.0>, MTB <Gn197.1>, MTC <Gn197.2>, or MTD <Gn197.3> to set the synchronization
mode specified in the program command in the block where the program is to restart (the state
specified by an M code for turning the flexible synchronization mode on or off). If the signal setting
is inconsistent with the state specified by the M code, alarm PS5374 occurs. The synchronization
mode is assumed to be off in the program from the beginning of the program until the first M code
for turning the flexible synchronization mode on or off is specified.

When program restart is executed (when signal SRNMV <Fn002.4> is set to “1”), the flexible
synchronization mode cannot be changed. If an attempt is made to change the mode, alarm PS5375
occurs.

B-64693EN-1/01

5. AUTOMATIC OPERATION

- 907 -

When a block in the flexible synchronization mode is specified as the restart block, the restart travel
distance for the slave axis is set to 0. In addition, “********” is displayed as the restart position for
the slave axis.

To restart a program from a block after the flexible synchronization mode is canceled, an absolute
command must be specified for the slave axis after the mode is canceled. If no absolute command is
specified for the slave axis, alarm PS5378 occurs.

3-dimensional coordinate system conversion / Tilted working plane command

When the block where the program is to restart is in 3-dimensional coordinate system conversion mode
G68 (machining center system) or G68.1 (lathe system) or Tilted working plane command, bit 1 (3DD) of
parameter No. 7301 can be set to select whether to move the tool to the restart position along each axis
according to the program coordinate system or workpiece coordinate system. When the bit (3DD) is set to
0, the tool moves to the restart position along each axis according to the program coordinate system;
when it is set to 1, the tool moves according to the workpiece coordinate system.
The “DESTINATION” and “DISTANCE TO GO” values are displayed according to the setting of this bit
(3DD).
The "ABSOLUTE" values are displayed according to the setting of bit 6 (DAK) of parameter No. 3106.

Tilted working plane indexing

To restart a program from a block in the tilted working plane indexing mode using a direct jump, follow
the procedure below:

1.  Return the tool to the restart position.
2.  Execute a direct jump.
3.  Specify the tilted working plane indexing mode using the MDI unit after the program has been

restarted (blinking RSTR disappears).

4. If the program is restarted from block after tool axis direction control, please command tool axis

direction control.

5. The present absolute coordinate is matched to the absolute coordinates of the restart block.

Presetting the relative coordinate values after the search

If bit 3 (RPR) of parameter No.7301 is 1, relative coordinate values are preset by absolute coordinate
values after the search in quick program restart. However, this preset function is invalid in direct jump
method of quick program restart.

Signal

Program restart under way signal SRNMV<Fn002.4>

[Classification] Output signal

[Function] Indicates the program is being restarted.

[Output cond.] The program restart under way signal becomes “1” when:

The program restart signal is set to “0” after the screen changes to the program
restart screen.

The signal is set to “0” when:
-

The program restart sequence ends (the tool has been moved to the restart point on
all controlled axes).

Quick program restart under way signal SRNEX<Fn534.1>

[Classification] Output signal

[Function] Indicates the quick program restart is executing.

[Output cond.] The program restart under way signal becomes "1" when:

Press the soft key [SEARCH EXEC], and quick program restart is begun.

The signal is set to "0" when:
-

The quick program restart sequence ends (the tool has been moved to the restart
point on all controlled axes).

5. AUTOMATIC OPERATION

B-64693EN-1/01

- 908 -

Signal address

Fn002

SRNMV

Fn534

SRNEX

Parameter

3106

DAK

[Input type] Setting input

[Data type] Bit

#6 DAK

Specifies whether to display coordinates in the program coordinate system or workpiece

coordinate system as absolute coordinates when the 3-dimensional coordinate conversion
mode or the tilted working plane indexing mode is set.
0:

Display coordinates in the program coordinate system.

Display coordinates in the workpiece coordinate system.

3712

CSF

[Input type] Parameter input

[Data type] Bit

#2 CSF

In the Cs contour control mode, the function for setting machine coordinates and absolute

coordinates based on the machine position of the spindle if the origin is already set up is:
0:

Disabled.

Enabled.

4353

CSP

[Input type] Parameter input

[Data type] Bit

#5 CSP

The function for transferring Cs axis positional data is:

Disabled.

Enabled.

When this parameter is used, set the bit 7 (RFCHK3) of parameter No.4016 is to 0.

7300

CCS

[Input type] Parameter input

[Data type] Bit path

#5 CCS

When the Cs contour control axis is used in the spindle mode or when the origin of the Cs

contour control axis is not established, program restart is:

Disabled.

Enabled.

7301

RPR

3DD

ROF

B-64693EN-1/01

5. AUTOMATIC OPERATION

- 909 -

[Input type] Parameter input

[Data type] Bit path

#0 ROF

When the coordinates for restarting are displayed on the program restart screen:

Tool length compensation (M series), tool position compensation (T series), cutter
compensation (M series), and tool-nose radius compensation (T series) are
considered.

Whether these compensation values are considered depends on the settings of bit 6
(DAL) of parameter No. 3104, bit 7 (DAC) of parameter No. 3104, and bit 1 (DAP)
of parameter No. 3129 (parameters for specifying whether to consider each
compensation value).

#1 3DD

In program restart operation, when the restart block is in 3-dimensional coordinate

conversion mode G68 (machining center system) or G68.1 (lathe system), the tool moves
to the restart point along each axis:
0:

According to the program coordinate system in dry run.

According to the workpiece coordinate system in dry run.

The restart coordinates and restart travel distance are also displayed in the coordinate
system set in this parameter.

NOTE

The change made to this parameter in program restart operation is
ignored.

#3 RPR

When the search is completed in program restart or quick program restart, relative

coordinate values are:
0:

Not preset.

Preset by absolute coordinate values.

NOTE

This parameter is invalid in direct jump method of quick program
restart.

7310

Ordinal number of an axis along which a movement is made in dry run after program restart

[Input type] Setting input

[Data type] Byte axis

[Valid data range] 1 to (Number of controlled axes)

This parameter sets the ordinal number of an axis along which a movement to the restart
point is made in dry run after the program is restarted.

WARNING

1 When there is two or more axes which has the same setting value in

this parameter, the movement to the restart point is not executed in
the second or more axis.

2 When the quick program restart is effective and bit 6 (SAV) of

parameter No.11250 is set to 1, the movement to the restart point is
not done in the axis which this parameter is set negative value(-1 to
-(Number of controlled axes)).

5. AUTOMATIC OPERATION

B-64693EN-1/01

- 910 -

NOTE

When this parameter is 0, alarm SR5020, "PARAMETER OF
RESTART ERROR" or the warning "ORDINAL NUMBER ERROR
(RESTART)" is displayed.

7331

RPS

[Input type] Setting input

[Data type] Bit

#1 RPS

In moving to the restart point of quick program restart, when the single block operation is

invalid, the axes
0:

do not stop by the restart point.

stop in state of the single block by the restart point.

NOTE

When this parameter is set to 1, the axes stop once in state of the
single block in starting after restart operation even if these don’t
move to the restart point.

11250

OAA

[Input type] Parameter input

[Data type] Bit path

#7 OAA

In the program restart function, the approach to the program restart position for each

arbitrary axis is:
0:

Not used.

Used.

11251

NPN

[Input type] Parameter input

[Data type] Bit

#4 NPN In Quick Program Restart Function, when an interrupted program is restarted from the

block in the subprogram, the subprogram name is :
0:

specified.

not specified.

13117

INT

[Input type] Parameter input

[Data type] Bit path

#4 INT

During a program restart, the interference check on cutter/tool nose radius compensation

is:
0:

Enabled.

Disabled.

B-64693EN-1/01

5. AUTOMATIC OPERATION

- 911 -

13421

FRS

[Input type] Parameter input

[Data type] Bit path

NOTE

Set these parameters for the first path only. It will be effective to all
paths.

#0 FRS

In a program containing an M code for turning the flexible synchronization mode on/off,

a program restart is:

Disabled.

Enabled.

Alarm and message

Number

Message

Description

PS0060

SEQUENCE NUMBER NOT FOUND

In the program restart sequence number specification, the
specified sequence number could not be found.
Check the restart block.

PS0071

DATA NOT FOUND

In the program restart block number specification, the
specified block number could not be found.
Check the restart block.

PS0098

G28 FOUND IN SEQUENCE RETURN

A command of the program restart was specified without the
reference position return operation after power ON or
emergency stop, and G28 was found during search. Perform
the reference position return.

PS5374

FSC MODE MISMATCH IN RESTART

The current flexible synchronization mode differs from the
flexible synchronization mode specified in a programmed
command in the program restart block.
Check the restart block.

PS5375

FSC MODE CAN NOT CHANGED

The flexible synchronization mode was changed during the
execution of program restart.
Check the restart block.

PS5378

INVALID RESTART BLOCK

The block specified as the restart block after the flexible
synchronization mode was canceled was not a block after an
absolute command for the axis specified as the slave axis.
Check the restart block.

DS0024

UINT SIGNAL WAS ILLEGALLY
INPUT

An interruption type custom macro was called during
movement to the program restart position.
Please do not call the interruption type custom macro.

5. AUTOMATIC OPERATION

B-64693EN-1/01

- 912 -

Warning

WARNING

1 In principle, the tool cannot return to a correct position in the following cases.

Special care must be taken in the following cases since none of them cause an
alarm.
-  Manual operation is performed when the manual absolute mode is off.
-  Manual operation is performed when the machine is locked.
-  The mirror image is used. The tool can be returned by P type program restart,

however, when the program is restarted from a block after the mode is turned
on or off last. At this time, keep the state of the mirror image signal when the
machining is interrupted.

- A program in which main commands are executed in the incremental mode

does not begin with coordinate system setting.

- Manual intervention is performed while the tool is returning to the restart

position along an axis.

- Program restart is specified for a block between the block for skip cutting and

subsequent absolute command block.

- After program restart is specified in the machine lock state, the machine lock

state is canceled.

- In general, if a coordinate system is set up, changed, or shifted after search,

the tool cannot return to the correct position.

2 When macro variable #3008 (indicating the status of program restart) is used and

the behavior of the program during restart operation is different from that during
normal operation, the program cannot be restarted from the correct position using
the search method.
Example)

Program O0002 performs different operations between normal operation and
program restart operation. In the following examples, this program cannot be
restarted from the block of N998 or N999 using the search method. A main
program including such a subprogram can be restarted, however. In this
example, the program can be restarted from the block of N1.

O0001(MAIN)

O0002(SUB)

M98P0002

IF[#3008NE0]GOTO999

N1G00X100.Y100.

G53Z0

T#500

N998G00Z0

N999

B-64693EN-1/01

5. AUTOMATIC OPERATION

- 913 -

Caution

CAUTION

Keep the following in mind when restarting a program including a macro variable.
- Common variable

When a program is restarted, the previous values are inherited as common
variables without being preset automatically. For this reason, before restarting
the program, initialize the required variables to the original values used at the
start of the previous automatic operation.

- System variable

The following system variables are not updated during search for restart:
  #5021 to #5028 ABSMT
  #5041 to #5048 ABSOT
  #5061 to #5068 ABSKP

- DI/DO

During the restart of a program, DI can be read by a system variable, but DO
cannot be output.

- Clock

During the restart of a program, the clock time can be obtained by a system
variable, but the time cannot be preset.

Reference item

Manual name

Item name

OPERATOR’S MANUAL (B-64694EN)

Quick program restart

5.7.1

Suppress Motion of Quick Program Restart

Overview

Suppress motion is a function which prohibits the approach to the start point of the specified restart block.
In the conventional specification, the approach is performed to the start point of the restart block. To
perform the approach to the end point of the restart block, the next block must be specified as the restart
block. This function enables the tool to be moved to the end point of the specified restart block.
For example, when a block for approach is inserted in the machining program, the block for approach can
be specified as the restart block and the tool can be moved to the end point of the block.

NOTE

An approach block is used for moving the tool closer to the workpiece from an
arbitrary position (such as a tool change position). Normally, all axes used for the
interrupted machining are specified. An approach block may consist of more than
one block. In this case, select the first approach block as the restart block.

Example) Operation example

O1234;

N100 G91G28Z0.;

N110 G28X0.Y0.;

N120 T01M6;

N130 G90G00X-50.Y0;

Approach block for the X- and Y-axes

N140 Z-10.;

Approach block for the Z-axis

N150 G41G01X-50.F1000.D1;

N160 Y50.;

FANUC Series 0i-MODEL F Plus. CONNECTION MANUAL (FUNCTION) - page 119