Siemens SINUMERIK 840D sl Programming Manual page 173

Example 2: Turning
Program code
N5 T1 D1 S2000 M3
N10 G0 G90 X11 Z1
N20 G1 Z-15 F0.2
N30 G3 X11 Z-27 I-8 K-6
N40 G1 Z-40
N50 M30
Note
For information on the input of the circle center point coordinates I and J, see Section
"Circular interpolation".
Example 3: Incremental dimensions without traversing of the active zero offset
Settings:
• G54 contains an offset in X of 25
• SD42440 $SC_FRAME_OFFSET_INCR_PROG = 0
Program code
N10 G90 G0 G54 X100
N20 G1 G91 X10
N30 G90 X50
See also
Absolute and incremental dimensions for turning and milling (G90/G91) [Page 174]
Fundamentals
Programming Manual, 09/2011, 6FC5398-1BP40-2BA0
Comment
; Loading of tool T1, spindle on with clockwise direction
of rotation.
; Absolute dimension input, in rapid traverse to position
XZ.
; Linear interpolation, feed of the tool.
; Counterclockwise circular interpolation, circle end
point in absolute dimensions, circle center point in
incremental dimensions.
; Traverse
; End of block
Comment
; Incremental dimensions active, traversing in X of 10 mm
(the zero offset is not traversed).
; Absolute dimensions active, traverse to position X75 (the
zero offset is traversed).
Geometry settings
8.3 Dimensions
173