How to prevent G81 crashes from incorrect plane setting (G18 / G19)

[Daniel_E]

The other day my (HAAS) machine crashed doing a G81 canned drill cycle. I'm not sure how to fix it, but I can't be the first to run into this issue.  Hopefully one of you can suggest a reliable way to fix this.

Here is what happened: I had a G19 in the program which changed to the YZ plane.  But there were no circular movements in XY before the G81, so the post processor never added in a G17 code to change back to the XY plane.  When the G81 was called, the drill cycle happened in the YZ plane instead of XY, which crashed the drill.  Later, there was a circular movement, so the G17 code showed up there, but it was too late for my drill cycle.

So apparently, the post processor doesn't realize that canned cycles are affected by the active plane.  Is there a checkbox for this somewhere?  Is there some better way to address this problem?

Thanks for any help!

[KenFarley]

The post-processor as it is now is probably doing what it is intended to do, allowing for holes to be drilled in whatever plane is currently active. Maybe to allow for things like a 90 degree head, etc.?

If you want to guarantee that only the X-Y plane will be used for drilling, which makes sense for a 3-axis machine I suppose, you might want to do any of these things:

(1) edit the FIL to check. If G17 is currently active, do nothing, otherwise output a G17 before the drill cycle.

(2) add a CL command in an auxiliary sequence right before your drill cycle sequence

(3) add a CL command at the end of the sequence where you switched to the G19 plane specification, to switch back to G17.

Which one is best will depend on your particular needs.

[Daniel_E]

These are excellent points and suggestions -- thank you Ken! 

As far as suggestions 2 and 3, I didn't know that YZ plane had been selected.  I had a trajectory tool path that had a very slight arc in the YZ plane, so the postprocessor output an arc on this plane.  But then later when I was drilling in the XY plane, it didn't change back to that plane.   Is there a way that I could/should be checking for this from within Creo?

For suggestion 1, yes, I think this would achieve what I originally asked for.  Thanks!  But you make a good point about this possibly not being what I want.  Perhaps there is a way to force the active plane callout (G17, G18, G19) with each drill cycle?  My problem in this instance was that the post processor posted code as if it was in the XY plane, but never output the G17 to switch back to the XY plane.

[Daniel_E · Accepted solution]

I emailed AustinNC about this, and they suggested adding a G17 after each tool change.  I think this will work quite well in my case, since I will always change tools when changing from milling to drilling.  I guess if I have a mill/drill combo tool, I'll have to be wary.  Here are the steps they gave me:

Open the post in the Option file generator and go to the Machine Codes -> Tool change -> User Blocks and add a block that outputs G17 after tool change.