Siemens SINUMERIK 840D sl Programming Manual page 102

Fundamentals
2.6 Spindle motion
If any of the G96/G961/G962 functions are active, SCC[<axis>] can be used to assign any
geometry axis as a reference axis. If the reference axis changes, which will in turn affect the
TCP (tool center point) reference position for the constant cutting rate, the resulting spindle
speed will be reached via the set braking or acceleration ramp.
Axis exchange of the assigned channel axis
The reference axis property for G96/G961/G962 is always assigned to a geometry axis. In the
event of an axis exchange involving the assigned channel axis, the reference axis property for
G96/G961/G962 is retained in the old channel.
A geometry axis exchange will not affect how the geometry axis is assigned to the constant
cutting rate. If the TCP reference position for G96/G961/G962 is affected by a geometry axis
exchange, the spindle will reach the new speed via a ramp.
If no new channel axis is assigned as a result of a geometry axis exchange (e.g. GEOAX(0,X)),
the spindle speed will be frozen in accordance with G97.
Examples for geometry axis exchange with assignments of the reference axis:
Program code
N05 G95 F0.1
N10 GEOAX(1, X1)
N20 SCC[X]
N30 GEOAX(1, X2)
N40 G96 M3 S20
Program code
N05 G95 F0.1
N10 GEOAX(1, X1)
N20 SCC[X1]
N30 GEOAX(1, X2)
N40 G96 M3 S20
Program code
N05 G95 F0.1
N10 GEOAX(1, X2)
N20 SCC[X1]
Program code
N05 G0 Z50
N10 X35 Y30
N15 SCC[X]
N20 G96 M3 S20
N25 G1 F1.5 X20
102
Comment
; Channel axis X1 becomes the first geometry axis.
; First geometry axis (X) becomes the reference axis
; for G96/G961/G962.
; Channel axis X2 becomes the first geometry axis.
; Reference axis for G96 is channel axis X2.
Comment
; Channel axis X1 becomes the first geometry axis.
; X1 and implicitly the first geometry axis (X) becomes
the reference axis for G96/G961/G962.
; Channel axis X2 becomes the first geometry axis.
; Reference axis for G96 is X2 or X, no alarm.
Comment
; Channel axis X2 becomes the first geometry axis.
; X1 is not a geometry axis, alarm.
Comment
; Reference axis for G96/G961/G962 is X.
; Constant cutting rate ON at 10 mm/min.
; Face cutting in X at 1.5 mm/revolution.
Programming Manual, 12/2019, 6FC5398-2EP40-0BA0
NC programming