Programming and Operating Manual (Milling)
6FC5398-4DP10-0BA1, 01/2014
101
Programming example
N10 G0 X20 Y20 T1 D1 M3 S500
N20 G41 G1 X10 Y10 F100
N30 G2 X20 Y20 CR=20
; Last block on the contour, circle or straight line, P1
N40 G40 G1 X10 Y10
; Switch off tool radius compensation, P2
N50 M30
8.10.7
Special cases of the tool radius compensation
Repetition of the compensation
The same compensation (e.g. G41 -> G41) can be programmed once more without writing G40 between these commands.
The last block in front of the new compensation call ends with the normal position of the compensation vector at 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
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.
Change of the compensation direction
The compensation direction G41 <-> G42 can be changed without writing G40.
The last block with the old compensation direction ends with the normal position of the compensation vector at the end point.
The new compensation direction is executed as a compensation start (default setting at starting point).
Cancellation of compensation by M2
If compensation mode is canceled using M2 (end of program) without writing the command G40, the last block with
coordinates of the plane (G17 to G19) will end in the normal position of the compensation vector. No compensating
movement is executed. The program ends with this tool position.
Critical machining cases
When programming, pay special attention to cases where the contour travel is smaller than the tool radius;
Such cases should be avoided.
