Tool Radius Compensation Off: G40; Special Cases Of The Tool Radius Compensation - Siemens SINUMERIK User Manual

11.11.6

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 X... 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.
See the following illustration for ending the tool radius compensation with G40:
Programming example
N10 T4 D1 M3 S1000 F0.1
N20 G0 X50 Z50
N30 G1 G42 X30 Z40
N40 G2 X20 Z20 R15
N50 G1 X10 Z10
N60 G40 G1 X0 Z0
N70 M30
11.11.7

Special cases of the tool radius compensation

Change of the compensation direction
The G41 ↔ G42 compensation direction can be changed without writing G40 in between.
The last block that uses the old compensation direction will end at the normal end position of the compensation vector in the
end point. The new compensation direction is executed as a compensation start (default setting at starting point).
Repetition of G41, G41 or G42, G42
The same compensation can again be programmed without writing G40 in between.
The last block before the new compensation call will end at the normal position of the compensation vector in the end point.
The new compensation is carried out as a compensation start (behavior as described for change in compensation direction).
Changing the offset number D
The offset number D can be changed in the compensation mode. A modified tool radius is active with effect from the block in
which the new D number is programmed. Its complete modification is only achieved at the end of the block. In other words:
The modification is traversed continuously over the entire block, also for circular interpolation.
Programming and Operating Manual (Turning)
01/2017
; Tool radius compensation OFF
;Last block on the contour, circle or straight line, P1
;Switch off tool radius compensation,P2
121