Siemens SINUMERIK 840DE Programming Manual page 335

Programming
G450 DISC=...
Or
G451
Parameters
G450
DISC=
G451
DISC=... is effective only when G450 is called, but can be programmed in a preceding block
without G450. Both commands are modal.
Example
In this example a transition radius is added to all outside corners (progr. in block N30). This
prevents the tool from having to stop and free cut when changing direction.
N10 G17 T1 G0 X35 Y0 Z0 F500
N20 G1 Z-5
N30 G41 KONT G450 X10 Y10
N40 Y60
N50 X50 Y30
N60 X10 Y10
N80 G40 X-20 Y50
N90 G0 Y100
N100 X200 M30
Fundamentals
Programming Manual, 10.2004 Edition, 6FC5 298-7AB00-0BP1
8.10 Compensation at the outside corners (G450, G451)
Transition circle: the tool travels around workpiece
corners on a circular path with tool radius
Flexible programming of the approach and retraction
instruction. In steps of 1 from DISC=0 circle to DISC=100
intersection
Intersection, the tool backs off from the workpiece corner
;Start conditions
;Tool infeed
;Activate compensation mode
;Cut contour
;Deactivate compensation mode, retract on
;transition circle
Tool offsets
8-39