Siemens Sinumerik 840D sl Programming Manual page 346

Auxiliary function outputs
14.1 M functions
Example 2: M function as high-speed output
Program code
N10 H=QU(735)
N10 G1 F300 X10 Y20 G64
N20 X8 Y90 M=QU(7)
M7 has been programmed as fast output so that the continuous-path mode (G64) is not
interrupted.
Note
Only use this function in special cases as, for example, the chronological alignment is changed
in combination with other function outputs.
Further information about the predefined M commands
Programmed stop: M0
The machining is stopped in the NC block with M0. You can now remove chips, remeasure,
etc.
Programmed stop 1 - optional stop: M1
M1 can be set via:
● HMI / dialog box "Program Control"
or
● NC/PLC interface
The program execution of the NC is stopped by the programmed blocks.
Programmed stop 2 - an auxiliary function associated with M1 with stop in the program
execution
Programmed stop 2 can be set via the HMI / dialog box "Program Control" and allows the
technological sequences to be interrupted at any time at the end of the part to be machined.
In this way, the operator can interrupt the production, e.g. to remove chip flows.
End of program: M2, M17, M30
A program is ended with M2, M17 or M30. If the main program is called from another program
(as subprogram), M2/M30 has the same effect as M17 and vice versa, i.e. M17 has the same
effect in the main program as M2/M30.
Spindle functions: M3, M4, M5, M19, M70
The extended address notation with specification of the spindle number applies for all spindles.
Example:
Program code
M2=3
If an address extension has not been programmed, the function applies for the master spindle.
346
Comment
; Fast output for H735.
; Fast output for M7.
Comment
; Clockwise spindle rotation for the second spindle
Programming Manual, 01/2015, 6FC5398-1BP40-5BA2
Fundamentals