Tool Radius Compensation Off: G40 - Siemens SINUMERIK 802D sl Programming And Operating Manual

Programming
10.6 Tool and tool offset
10.6.6

Tool radius compensation OFF: G40

Functionality
The compensation mode (G41/G42) is deselected with G40. G40 is also the switch-on
position at the beginning of the program.
The tool ends the block before G40 in the normal end position (compensation vector vertical
to the tangent in the end point); independently of the start angle.
If G40 is active, the reference point is the tool tip. The tool tip then travels to the programmed
point upon deselection.
Always select the end point of the G40 block such that collision-free traversing is
guaranteed!
Programming
G40 Y... Z...
Remark: The compensation mode can only be deselected with linear interpolation (G0, G1).
Program both axes. If you only specify one axis, the second axis is automatically completed
with the last programmed value.
S
Figure 10-40 Ending the tool radius compensation with G40, with the example of G42, cutting edge position =3
Programming example
...
N100 Y... Z...
N110 G40 G1 Y... Z...
270
; Tool radius compensation OFF
S
;Last block on the contour, circle or straight line, P1
;Switch off tool radius compensation,P2
Programming and Operating Manual, 11/2012, 6FC5398-5CP10-3BA0
Surface grinding