FANUC Series 30i/300i/300is-MODEL A. Machining Center System. User's manual - page 81

17.REAL-TIME CUSTOM MACRO

PROGRAMMING

B-63944EN/03

- 604 -

Sample program

The sample program below exercises the following three control
operations at the same time.
(1) A cutting operation is performed on the X-axis and Z-axis.
(2) On each rising edge of the X signal 5.2, 20 is fed on the

peripheral axis A.

(3) When the workpiece coordinate on the X-axis (#100101) is equal

to or less than 50, the Y signal 2.3 is set to 1.

The operation of (1) is coded in the main NC statement.
The operation of (2) is coded in the first modal RTM command (//1).
The operation of (3) is coded in the second modal RTM command
(//2).

O0001 ;
G90 G00 X100 Z100;

//1 ZWHILE[1] ZDO ;
ZEDGE [#IOX[5,2] EQ 1 ] ZDO ;
G91 G00 A20. ;
ZEND ;
ZEND ;

//2 ZWHILE[1] ZDO ;
ZEDGE [ #100101 LE 50.0 ] #IOY[2,3] = 1 ;
ZEND ;

#100=100 ;
WHILE [ #100 GT 0 ]) DO1
G91 G01 Z-#100 F200. ;
Z#100. ;
#100 = #100 - 10 ;
X-10. F100;
END1
M02 ;

Workpiece

50
(Y signal is
turned on
when tool
enters this
range.)

RTM command (2)
operation
(On each rising edge of
X5.2, 20 is fed on peripheral
axis A.)

RTM command (3)
operation
(When X coordinate is 50 or
less, Y signal 2.3 is set to 1.)

Command for cutting on
X-axis and Z-axis

Peripheral axis A

Signal switch
(Address X5.2)

Signal lamp
(Address
Y2.3)

B-63944EN/03

PROGRAMMING

17.REAL-TIME CUSTOM MACRO

- 605 -

17.5

MACRO CALL

A series of RTM statements can be formed into a subprogram, which
can be called from the main program.

When G65 is specified in an RTM command, the real time macro
specified in address P is called.

Explanation
- Calling

In address P after G65, specify the program number of a real time
custom macro to be called.

NOTE

1 In argument P of G65, only a constant value can

be used. No value can be specified through a
variable.

  Example:
  // G65 P9010 ; Correct
  // G65 P#RV[0] ; Incorrect
2  The inclusion of another NC command (such as

G01 X100.0 G65 Pp) is not allowed. If another
NC command is included, PS0127 alarm is issued.

3 The G65 block for calling a real time macro does

not make a single block stop.

4 On the other hand, a real time macro program

called by real time macro calling makes a single
block stop.

P : Number of real time macro program to be called

O0001 ;
:
:
//1 G65 P9010 ;
G04 P2000 ;
:
:
M30 ;

O9010 ;
:
:
:
:
:
:
M99 ;

G65

P p ;

The execution of real time macro //1 including O9010 starts simultaneously
with the G04 block of main program O0001.

Code real time macro
statements.

17.REAL-TIME CUSTOM MACRO

PROGRAMMING

B-63944EN/03

- 606 -

- Call destination real time program

In a called real time macro program, only an RTM statement can be
coded.

In a called real time macro program, no additional RTM command
may be executed. (The RTM command symbol ‘//’ may not be
coded.) For example, do not execute the following program:

O0001 ;

O9010 ;

// G65 P9010 ;

// #RV[0]=1 ;

M02 ;

M99 ;

Code M99 in the last block only.
For example, do not execute the following program:

O0001 ;

O9010 ;

// G65 P9010 ;

ZEDGE [#RV[0] EQ 1] M99 ;

M02 ;

G91 G00 X50. ;

M99

;

When executing an RTM statement in a subprogram, code an NC
statement before the M99 block for returning to the calling program.

O0001 ;

O9010 ;

G65 P9010 ;

// #RV[0] = 20 ; Real time macro statement

M02 ;

G04 ; NC statement

M99

;

- Format

Specify G65 at the start of a block.

- Call nesting level

Macro call nesting is not allowed.

- Differences from macro call using a custom macro

Macro call using a real time custom macro and macro call using a
custom macro differs as described below.

•

In macro call using a custom macro, an argument (data to be
passed to a macro) and the number of repetitions can be specified.
In macro call using a real time custom macro, such information
cannot be specified.

•

With a real time custom macro, other types of macro call (macro
call using G66, G66.1, G, and M code) and subprogram call are
not allowed.

B-63944EN/03

PROGRAMMING

17.REAL-TIME CUSTOM MACRO

- 607 -

17.6

OTHERS

If an axis control command is followed by a macro command in an
RTM command, the execution of the macro command starts when the
axis control command is completed or deceleration starts.
If deceleration on the X-axis starts upon completion of distribution
according to the axis control command of (1), for example, the macro
command of (2) is executed. If acceleration/deceleration is not
applied on the X-axis, (2) is executed upon completion of distribution
on the X-axis.
// ZDO ;
G91 G00 X30 ;

(1) Axis control command of the RTM statement

#RV[0] = 1 ;

(2) Macro command of the RTM statement

ZEND ;

If an RTM command is executed in a custom macro WHILE DO to
END loop, and the same RTM is looked ahead while the RTM
command is being executed, a PS alarm may be issued.
For example, if the command below is executed, a PS alarm is issued.

WHILE [1] DO1 ;
// #RV[0] = #RV[0] + 1 ;
#100=#100+1 ;
END1 ;

In this example, insert G04 ; block between a #100=#100+1; and
END1;.

17.REAL-TIME CUSTOM MACRO

PROGRAMMING

B-63944EN/03

- 608 -

17.7

AXIS CONTROL COMMAND

In an RTM statement, a G code for specifying a movement can be
specified. For axis control, the PMC axis control interface is used.
The specifications differ from the specifications for the G code used
with an NC statement.

Format

// ZDO ;
G_

_ F_ ;

:
ZEND ;

For an axis control command, ZDO...ZEND of multi-statement
structure is used for coding even if a single statement (single RTM
statement) is used.

CAUTION

Do not specify an NC statement for an axis to be
controlled with an RTM statement. Moreover, do
not exercise axis control with an RTM statement on
an axis to be controlled with an NC statement.

NOTE

1 In one block, only one axis may be specified. Do

not specify two or more axes in the same block.

2 In the three-dimensional coordinate conversion

mode, the polygon mode, etc., an RTM statement
concerning that axis cannot be specified.

Explanation
- Setting

For an axis control command in an RTM statement, the interface of a
PMC axis control group set by a parameter beforehand is used.
For an axis to be controlled with an RTM statement, set a group to be
used with parameter No. 8010. Then, set bit 0 (XRT) of parameter
No. 8011 for the axis to 1.

NOTE

An axis for which bit 0 (XRT) of parameter No.
8011 is set to 1 is dedicated to real time custom
macros, so that such an axis cannot be used with
PMC axis control.

B-63944EN/03

PROGRAMMING

17.REAL-TIME CUSTOM MACRO

- 609 -

- Relationship with PMC axis control

Axis control based on an RTM statement uses the PMC axis control
interface. So, the specifications for a move command in each block
within an RTM statement are generally equivalent to the specifications
for the PMC axis control command.
For the detailed specifications and restrictions related to axis control,
refer to the specifications of PMC axis control as well.

NOTE

1 An axis used with an RTM statement must not be

specified from PMC axis control.

2 A PMC axis control group used with an RTM

statement must not be specified from PMC axis
control.

- Operation command code

The table below indicates the G codes that can be specified in an RTM
statement.
The mark in the table indicates modal G codes when an RTM
command starts.

Code Group

Meaning

G00 Positioning
G01

Feed at specified feedrate

G28

Reference position return

G53

Machine coordinate system selection

G90 Absolute

command

NOTE 1

G91

Incremental command

NOTE 2

G94

Feed per minute

G95

Feed per revolution

NOTE

1 The absolute command (G90) is valid for machine

coordinate system selection (G53) only.

2 The incremental command (G91) is valid for

positioning (G00), linear interpolation (G01), and
reference position return (G28) only.

3 In T series G code system A as well, not G98/G99

but G90/G91 are valid with an RTM command.

- Modal information

Basically, modal information such as F and modal G codes in an RTM
statement is independent in an NC statement and each RTM statement.
Modal information in an RTM statement is initialized when the
execution of the RTM statement is started (when a block specified
with // is executed).
The initial value of modal information in an RTM statement is as
follows:

State of the G codes marked with in the operation command
code list

code

17.REAL-TIME CUSTOM MACRO

PROGRAMMING

B-63944EN/03

- 610 -

CAUTION

With the G codes (inch input/metric input) of group
06, the same information as the modal information
of an NC statement is used in an RTM statement.
Do not change the modal information of group 06
with an NC statement in a block after the first RTM
statement coded in a program.

NOTE

With an RTM command, bit 0 (G01), bit 3 (G91),
and bit 4 (FPM) of parameter No. 3402 are invalid
when the power is turned on or in the cleared
state.

Example 1)

Modal information can be controlled independently in an NC
statement and each RTM statement.

O0001 ;

G90 G01 X100. Y100. F500. ;

(1)

//1 ZDO ;

Z50. ;

(2)

G01 Z100. F100. ;

(3)

ZEND ;

//2 ZDO ;

G01 A30. F200. ;

(4)

A50. ;

(5)

ZEND ;

X200. ;

(6)

The modal information of command (2) is G00, G91, and G94,
regardless of the modal information (G90 G01 set in (1)) of the
NC statement.

The modal information of command

(5)

is G01, G91, G94, and

F200.. This modal information is not affected by the modal
information (command (1)) of the NC statement and the modal
information (commands (2) and

(3)

) in the RTM statement with

modal ID=1.

The modal information of command

(6)

is not affected by the

modal information (commands

(2)

to (5)) in the RTM statement,

so that the modal information is G01, G90, and F500..

B-63944EN/03

PROGRAMMING

17.REAL-TIME CUSTOM MACRO

- 611 -

Example 2)

Modal information is initialized when the execution of each
RTM command is started. Even if the same program includes
RTM commands with the same ID, the modal information of the
RTM command executed first is not inherited by the RTM
command executed next.

O0001 ;

G90 G01 X100. Y100. F500. ;

//1 ZDO ;

G01 Z100. F3000. ;

(1)

ZEND ;

X200. ;

//1 ZDO ;

Z200. ;

(2)

ZEND ;

X300. ;

The modal information of command (2) is G91 and G00,
regardless of command

(1)

- Single block stop

If an NC statement is placed in the single block stop state, for example,
by the single block stop signal SBK, the axis control command of an
RTM statement also comes to a single block stop.
However, the automatic operation start signal STL is turned off when
all conditions on the NC statement side are satisfied, even if the axis
control command of an RTM statement is not terminated.
If an RTM command consists of multiple statements and an axis
control command is coded in multiple blocks, only the block of the
RTM statement that is currently executing an axis command can be
brought to a single block stop by setting the group-by-group single
block stop signal (ESBKg) for PMC axis control corresponding to the
axis to 1.

- Feed hold

Even when an NC statement enters the automatic operation halt state,
the axis control command of an RTM statement does not stop
immediately but stops at the time of termination of the block currently
being executed. To stop also the axis control command of an RTM
statement immediately when the NC statement enters the automatic
operation halt state, control the temporary stop signal (ESTPg) for
PMC axis control of the related group by monitoring the automatic
operation halt in-progress signal (SPL).

Content .. 79 80 81 82 ..