Siemens SINUMERIK 840D sl Programming Manual page 130

Feed control
7.4 Positioning spindles (SPOS, SPOSA, M19, M70, WAITS)
Program code
....
N110 S2=1000 M2=3
N120 SPOSA=DC(0)
N125 G0 X34 Z-35
N130 WAITS
N135 G1 G94 X10 F250
N140G0 X34
N145 SPOS=IC(90)
N150 G1 X10
N155 G0 X34
N160 SPOS=AC(180)
N165 G1 X10
N170 G0 X34
N175 SPOS=IC(90)
N180 G1 X10
N185 G0 X50
...
Further information
Positioning with SPOSA
The block step enable or program execution is not affected by SPOSA. The spindle
positioning can be performed during execution of subsequent NC blocks. The program moves
onto the next block if all the functions (except for spindle) programmed in the current block
have reached their block end criterion. The spindle positioning operation may be programmed
over several blocks (see WAITS).
NOTICE
If a command, which implicitly causes a preprocessing stop, is read in a following block,
execution of this block is delayed until all positioning spindles are stationary.
130
Comment
; Switch on cross drilling attachment.
; Set main spindle to 0° immediately,
the program will advance to the next block straight
away.
; Switch on the drill while the spindle is taking up
position.
; Wait for the main spindle to reach its position.
; Feedrate in mm/min (G96 is suitable only for the
multi-edge turning tool and synchronous spindle, but
not for power tools on the cross slide.)
; The spindle is positioned through 90° with read halt
in a positive direction.
; The spindle is positioned at 180° relative to the
spindle zero point.
; The spindle turns in a positive direction through 90°
from the absolute 180° position, ending up in the
absolute 270° position.
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
Fundamentals