FANUC Series 16/18/160/180-Model C Machining Center Operators Manual

PROGRAMMING
B–62764EN/01
12. AUXILIARY FUNCTION
151
When a numeral is specified following address M, code signal and a
strobe signal are sent to the machine. The machine uses these signals to
turn on or off its functions.
Usually, only one M code can be specified in one block. In some cases,
however, up to three M codes can be specified for some types of machine
tools.
Which M code corresponds to which machine function is determined by
the machine tool builder.
The machine processes all operations specified by M codes except those
specified by M98, M99,M198 or called subprogram(Parameter No.6071
to 6079), or called custom macro (Parameter No.6080 to 6089). Refer to
the machine tool builders instruction manual for details.
The following M codes have special meanings.
This indicates the end of the main program
Automatic operation is stopped and the CNC unit is reset.
This differs with the machine tool builder.
After a block specifying the end of the program is executed,
control returns to the start of the program.
Bit 5 of parameter 3404 (M02) or bit 4 of parameter 3404 (M30) can be
used to disable M02, M30 from returning control to the start of the
program.
Automatic operation is stopped after a block containing M00 is executed.
When the program is stopped, all existing modal information remains
unchanged. The automatic operation can be restarted by actuating the
cycle operation. This differs with the machine tool builder.
Similarly to M00, automatic operation is stopped after a block containing
M01 is executed. This code is only effective when the Optional Stop
switch on the machine operators panel has been pressed.
This code is used to call a subprogram. The code and strobe signals are
not sent. See the subprogram
II– 13.3 for details .
This code indicates the end of a subprogram.
M99 execution returns control to the main program. The code and strobe
signals are not sent. See the subprogram
section 13.3 for details.
NOTE
The block following M00, M01, M02, or M30 is not pre–read
(buffered). Similarly, ten M codes which do not buffer can
be set by parameters (Nos. 3411 to 3420). Refer to the
machine tool builder’s instruction manual for these M codes.
12.1
AUXILIARY
FUNCTION
(M FUNCTION)
Explanations
D M02,M03
(End of program)
D M00
(Program stop)
D M01
(Optional stop)
D M98
(Calling of sub-
program)
D M99
(End of subprogram)

Leave a Reply

Your email address will not be published. Required fields are marked *