[duivenhok]

I have the following question.
When stopping an automated operation with nose radius compensation the compensation is not cancceld by the reset button.
I have to G40 by MDI to cancell the nose radius compensation.
Is there a parameter setting that has to be changed so that G41/G42 is cancceld by reset , and if so is there also one for automated cancelling the radius compensation when the program end and rewinds with M30.

just wondering.

[dcoupar]

Why not add the G40 to the program?

[duivenhok]

I do. but when I interrupt the program before the G41 is cancelled and decide not to continue but restart the programm ( for example because of a material/ workpiece defect) by using Edit-reset the radius compensation is not cancelled but remains active.

[txcncman]

Also avoiding resetting during the G41/G42 is helpful. You really should not have to reset very often if you are getting your programming and machining methods right the first time.

I usually put G40 in the start code for each tool process. Same with G80. That way when I do have to restart, I know everything is in the proper condition.

[beege]

I usually put G40 in the start code for each tool process. Same with G80. That way when I do have to restart, I know everything is in the proper condition.

+1 on this. A start block for any single operation should have what you need for recovery to a prior setting, like a G40, G80, even inch versus metric if you use it, and G90 vs. G91 if applicable.

Beege

[zooloader]

ditto txcncman.

best practice would be to start each tool in a state that YOU have set.

[duivenhok]

I agree that the best way is to start with G40 when no radius comp. is needed but thats not realy a answer to the question if it's possible to cancel G41/42 with the restet button regardless of what would be the smartest thing to do

[txcncman]

I do not have a manual for an 18iT control. I suggest you consult the manual to find your answer or contact your nearest service center.

[dcoupar]

I agree that the best way is to start with G40 when no radius comp. is needed but thats not realy a answer to the question if it's possible to cancel G41/42 with the restet button regardless of what would be the smartest thing to do

I haven't tried this myself...

3402 bit 6 (CLR)=1
3406 bit 7 (C07)=0

See attachments.

Let us know, please.

Dave

[angelw]

I haven't tried this myself...

3402 bit 6 (CLR)=1
3406 bit 7 (C07)=0

See attachments.

Let us know, please.

Dave

Hi Dave,
I tested this on an 0i control today. Prepared a program to use cutter rad comp and no G40 prior to the cutter rad comp being initiated. On this particular machine 3402.6 and 3406.7 were already set 1 and 0 respectively and Reset could be launched during cutter rad comp without any consequence when running the cutter rad comp part of the program again.

Setting these parameter bits mirror to that shown above made no difference whatsoever, the machine still ran the program again without error after Resetting when cutter rad comp was active.

Regards,

Bill

[fordav11]

the manual has no specific parameter setting to cancel G41/G42 with reset.

parameter 5003 might help.

bit 6 and bit 7 when set to 1 will clear wear and geometry offsets when reset is pressed.
bit 2 when set to 1 *will* cancel tool nose radius compensation but only when the machine is zero-returned.

[sinha_nsit]

Not sure, but
3402#6(CLR)=1 and 3409#7(CFH)=0 might work.