Hi. I’m a newby to the forum. Recently i started using my laptop for drawings and after i finish to cut the drawing the torch keeps cutting until its back at the start position X=0 and Y=0. I used to do my drawings with a PC. Probably something silly.
Cheers Colin
I’m not sure I understand your description.
Are you describing
A) that the torch cuts 1mm or so into the start point kerf after completing a 360 deg cut around the shape contour ?
or are you describing
B) that the torch cuts from the end of the last shape contour all the way back to a programmed finish point such as X0Y0 ?
and then, are you also describing that you had previously run sheetcam and the post processor on a different computer yielding good results on the CNC plasma table ?
It may be that you should just send a support.zip file to sales@sheetcam.com along with a photo or two of the problem.
Creating a Sheetcam Customer Support file
Hi Lou.
Answer B is the correct answer. When I run it in sheetcam it stops at the proper spot. But when I cut in mach 3 it keeps going back to the zero zero
ah. You are comparing Sheetcam menu Mode-Simulation to Mach3 controller/CNC table results, got it. Sheetcam simulation does not use the post processor assigned for gcode production in your settings, rather it uses a simple toolpath as represented in the drawing. Thus differences in the simulation vs. actual table motion is common, depending on the customization of the post processor you are using.
I suspect this also means on the “PC” you were using sheetcam simulation also.
Thus actual cutting on the CNC table w Mach3 has always produced the result of cutting back to the programmed finish point of X0Y0.
There may be a couple of features in sheetcam that may be mistakenly in use or there could be an error or incompatibility in the post processor. Either way, the easiest way to help you troubleshoot this is to send us a customer support file.
I have sent you the zip file.
No it has only started to do it since using the Laptop.
after reviewing and testing your job file and pp…
The problem is in your job file definition, in that the Options-‘Job Options’-‘Rapid clearance’ value is zero, and this is lower than the tool’s pierce height, aside from being very unusual to be defined as zero. This confuses sheetcam into behavior of NOT invoking OnPenUP() after the last contour is cut; OnPenUP() turns off the torch (M05). There were a few clues- M05 is missing in your .tap file after the last contour cut, and there were no motions to safeZ after any contour cuts.
Those results are running on v7.0.21 with your post processor (stock version of ‘Mach3 THC with scriber’).
Running on v7.1.40 (latest downloadable development version w fixes) a post processor runtime error is thrown stating that “Rapid clearance is below the pierce height”.