Siemens SINUMERIK 840D Function Manual page 743

SPOS, M19 and SPOSA have the same functionality but differ in their block change behavior:
● SPOS and M19
The block change is carried out if all functions programmed in the block have reached their
end-of-block criterion (e.g. all auxiliary functions acknowledged by the PLC, all axes have
reached their end points) and the spindle has completed its positioning motion.
● SPOSA
The program moves to the next block if all the functions (except for spindle) programmed in
the current block have reached their end-of-block criterion. If SPOSA is the only entry in the
block, block change is performed immediately. The spindle positioning operation may be
programmed over several blocks (see WAITS).
Coordination
A coordination of the sequence of motions can be achieved with:
● PLC
● MD configuration
● Programming in the part program
PLC
If the NC/PLC interface signal:
DB31, ... DBX83.5 (spindle in the setpoint range)
is not available, then the channel-specific NC/PLC interface signal:
DB21, ... DBX 6.1 (read-in inhibit)
can be set in order to wait for a spindle to reach a certain position.
MD configuration
Setting:
MD35500 $MA_SPIND_ON_SPEED_AT_IPO_START = 1
is used to perform path interpolation taking the tolerance:
MD35150 $MA_SPIND_DES_VELO_TOL
into account only if the spindle has rotated up to the preselected speed.
The setting
MD35500 $MA_SPIND_ON_SPEED_AT_IPO_START = 2
is used to stop traveling path axes before the start of machining at the last G0.
Machining continues:
● With the next traversing command.
● If the spindle speed is reached.
● When MD35510 $MA_SPIND_STOPPED_AT_IPO_START = 1
(path feed enable, if spindle stationary).
Programming in the part program
Axes and spindles
Function Manual, 06/2019, A5E47437747B AA
S1: Spindles
18.2 Operating modes
743