Siemens SINUMERIK 828D Programming Manual page 173

G91 extension
For certain applications, such as scratching, it is necessary that only the programmed
distance is traversed in incremental dimensions. The active zero offset or tool length
compensation is not traversed.
This behavior can be set separately for the active zero offset and tool length compensation
via the following setting data:
SD42440 $SC_FRAME_OFFSET_INCR_PROG (zero offsets in frames)
SD42442 $SC_TOOL_OFFSET_INCR_PROG (tool length compensations)
Value
0
1
Examples
Example 1: Milling
Program code
N10 G90 G0 X45 Y60 Z2 T1 S2000 M3
N20 G1 Z-5 F500
N30 G2 X20 Y35 I0 J-25
N40 G0 Z2
N50 M30
Fundamentals
Programming Manual, 07/2010, 6FC5398-1BP40-0BA0
Meaning
With incremental programming (incremental dimensions) of an axis, the zero offset or the
tool length compensation is not traversed.
With incremental programming (incremental dimensions) of an axis, the zero offset or the
tool length compensation is traversed.
Comment
; Absolute dimension input, in rapid
traverse to position XYZ, tool selection,
spindle on with clockwise direction of
rotation
; Linear interpolation, feed of the tool.
; Clockwise circular interpolation, circle
end point in absolute dimensions, circle
center point in incremental dimensions.
; Traverse
; End of block
Geometry settings
8.3 Dimensions
173