Siemens SINUMERIK 808D User Manual page 120

Sta rting the compensation
The tool travels in a straight line directly to the contour and is positioned perpendicular to the path tangent at the starting
point of the contour.
Select the starting point such that a collision-free travel is ensured.
See the following illustration for start of the tool radius compensation with G42 as example:
The tool tip goes around the left of the workpiece when the tool runs clockwise using G41; the tool tip goes around the right
of the workpiece when the tool runs counter-clockwise using G42.
In formation
As a rule, the block with G41/G42 is followed by a block with workpiece contour description. If, however, the block with
G41/G42 is followed by blocks without contour description, a maximum of five such blocks (for example, M commands and
infeed motions) are allowed; otherwise, the compensation will be interrupted.
Programming example
N10 T1
N20 G17 D2 F300
N30 X0 Y0
N40 G1 G42 X11 Y11
N50 X20 Y20
N60 M30
After the selection, it is also possible to execute blocks that contain infeed motions or M outputs:
N10 T1
N20 G17 D2 F300
N30 G0 X0 Y0
N40 G1 G42 X11 Y11
N50 Z20
N60 M08
N70 X20 Y20
N80 M30
120
; Correction number 2, feed 300 mm/min
; P0 - starting point
; Selection to the right of contour, P1
; Starting contour, circle or straight line
; End of program
; Correction number 2, feed 300 mm/min
; P0 - starting point
; Selecting right of contour, P1
; Infeed movement
; M command coolant on
; Starting contour, circle or straight line
; End of program
Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA6, 09/2017