sheetcam.com

Posted: **Thu Mar 01, 2018 9:53 pm**

Backstory:
We've been using Sheetcam on our in-house built cnc plasma for the last year and it's worked without issue. We now need to modify our post (attached), but I haven't been able to figure out how to omit the feedrate plunge that happens after piercing, or omit the rapid move up to the safeZ after the cut is done.

I need this:

Code: Select all

N0230 M03
N0240 G01 X5.2194 Y0.3387 Z0.0600 F100
N0250 G02 X5.2194 Y0.3387 I0.0000 J0.1613 F63.0
N0260 M05
N0270 G00 Z0.2500

to become this:

Code: Select all

N0230 M03
N0250 G02 X5.2194 Y0.3387 I0.0000 J0.1613 F63.0
N0260 M05

Is this something that can be done in the post, or is this integral to Sheetcam? And if so, how can I turn these off?
Thanks,
Josh Taylor
Turner & Taylor Metal Works, Inc.

Posted: **Fri Mar 02, 2018 3:20 pm**

Those moves are gaenerated from within SheetCam but they can be bypassed. Are you trying to remove the Z moves completely or do you just want to remove those specific moves?

Posted: **Fri Mar 02, 2018 5:36 pm**

Hi Les,
Thanks for responding. I need to remove those specific Z movements put in by Sheetcam as relates to the plunge & retract. In practice, that equates to all of them, however, I would prefer to omit them directly rather than search and delete all Z movements in the tap file for instance. How can those be bypassed?
Thanks,
Josh Taylor
Turner & Taylor Metal Works, Inc.

Posted: **Fri Mar 02, 2018 8:32 pm**

Go to Options->Machine->post processor and click on the 'Edit post' button.
Look for lines like this:

Code: Select all

post.ModalNumber (" Z", (endZ + toolOffset) * scale, "0.000")

and delete them. This will remove all Z moves. Most posts have 3 of these lines. Just doing this will cause the post to sometimes output a line that is just G00 or G01 with no coordinates. If that is a problem try adding this code to the beginning of function OnRapid() and function OnMove():

Code: Select all

   if (math.hypot(endX - currentX, endY - currentY) < 0.01) then return end

Posted: **Tue Mar 13, 2018 4:40 pm**

Les,
Thank you. This all works perfectly. I can't foresee needing to actually post Z movements, but if it comes up, I'll post back here to see if there is a fix. I'll also upload my post-processor in case anybody else searches for the same thing.
Thanks again,
Josh Taylor

sheetcam.com

Remove pierce plunge & return to rapid.

Remove pierce plunge & return to rapid.

Re: Remove pierce plunge & return to rapid.

Re: Remove pierce plunge & return to rapid.

Re: Remove pierce plunge & return to rapid.

Re: Remove pierce plunge & return to rapid.