M Functions Of Spindle Control (M19, M29); M Functions For Subroutine Calls (M98, M99) - Siemens SINUMERIK 808D Programming And Operating Manual

The NC-specific M functions are described below.
M functions to stop operations (M00, M01, M02, M30)
A program stop is triggered with this M function and the machining is interrupted or ended. Whether the spindle is also
stopped depends on the specification of the machine manufacturer. Details are available in the documentation of your
machine manufacturer.
M00 (program stop)
The machining is stopped in the NC block with M00. One can now, e.g., remove chips, re-measure, etc. A signal is output to
the PLC. The program can be continued with the following key:
M01 (optional stop)
M01 can be set via the following methods:
● HMI/dialog box "Program control" or the
● VDI interface
The program processing of the NC is maintained with M01 only when the corresponding signal of the VDI interface is set or
"Program control" was selected in the HMI/dialog box.
M30 or M02 (end of program)
A program is ended with M30 or M02.
Note
A signal is output to the PLC with M00, M01, M02 or M30.
Note
Data on whether spindle is stopped with the commands M00, M01, M02 or M30 or the coolant supply is interrupted is
available in the documentation of your machine manufacturer.
4.3.5.4

M functions of spindle control (M19, M29)

M function
M19
M29
The spindle is traversed to the spindle position defined in the setting data 43240 $SA_M19_SPOS[spindle number] with M19.
The positioning mode is stored in $SA_M19_SPOS.
The M function number for the changeover of the spindle mode (M29) can also be set over a machine data variable.
MD20095 $MC_EXTERN_RIGID_TAPPING_N_NR is used to pre-set the M function number. Only the M function numbers
that are not used as standard M functions can be assigned. For example, M0, M5, M30, M98, M99 etc are not allowed.
4.3.5.5

M functions for subroutine calls (M98, M99)

M function
M98
M99
In ISO mode, the spindle is switched to the axis mode with M29.
120
Function
Positioning the spindle
Changeover of spindle to the axis/open-loop control mode
Function
Subprogram call
Subprogram end
Programming and Operating Manual (ISO Turning/Milling)
01/2017