Problems with curved/round toolpaths in Sheetcam gcode

[859Design]

New to Cnc plasma cutting, but not Cnc cutting in general.
I'm having trouble getting any file I make in any of the design software I have to come out with a nice smooth radius. Straight lines cut fine.

I have used several versions of Dxf, SVG, and Plt from Corel, inkscape, freecad, Vm4, Drawplus X8, and my Laser cutting software.
The files that import look like they should on Sheetcam I believe but come out with a mix of curves and straight lines in CncSimulator where they should all be curved.
I'm not sure if it is the import settings, files, or a post processor problem but I have spent 4 days trying to figure it out and need some help now. Thanks

[plasmanewbie]

I had that problem using CorelDRAW and started saving files as SVG rather than DXF and it fixed it. Can't see the problem your describing in your pics unless those diamonds are supposed to be circles.

[SegoMan DeSigns]

CorelDraw exports DXF files as splines / polylines and not as Arcs . This is easily viewable when you open their exports with Draftsite or other CAD software. Torchmate CAD software will fix this as it is imported, a lot of programs don't. When I outsource files to be cut I either clean them up with the TM software or use this (free trial version available):

https://www.cadkas.com/dxf-splines-to-arcs.php

A vid on it:

https://www.youtube.com/watch?v=dKUXnKHwkOI

I wasted a good part of a day trying to explain this to a level 5 tech at CorelDraw but he would have nothing to do with it..

[859Design]

I had that problem using CorelDRAW and started saving files as SVG rather than DXF and it fixed it. Can't see the problem your describing in your pics unless those diamonds are supposed to be circles.

Yes, the diamonds all should of been a hole like the bottom left one and all corners should of been rounded.
The other picture was just to show the machine is capable of cutting holes decent.
The holder file was made in Corel and it was an Svg.

[859Design]

I just got Draftsight (free) and will try again.

[859Design]

CorelDraw exports DXF files as splines / polylines and not as Arcs . This is easily viewable when you open their exports with Draftsite or other CAD software. Torchmate CAD software will fix this as it is imported, a lot of programs don't. When I outsource files to be cut I either clean them up with the TM software or use this (free trial version available):

https://www.cadkas.com/dxf-splines-to-arcs.php

A vid on it:

https://www.youtube.com/watch?v=dKUXnKHwkOI

I wasted a good part of a day trying to explain this to a level 5 tech at CorelDraw but he would have nothing to do with it..

I actually ran across the Cadkas the other day, what are good settings to use in it? Default or are they even close?
I can believe it, they think the software is perfect at Corel..

[SegoMan DeSigns]

Using CAD-KAS creates a book keeping challenge.

You will want to start a folder that you put your CorelDraw exported files into (call it CADKAS)
Do a sub folder in that folder and call it "Converted" When prompted put the CADKAS exported files there (you might want add a"C" at the end of the file name to show it has been converted)

Try converting a file with the default values, when complete there will be a list of minimal values of the last conversion, try a second conversion with something in between the two values (I normally just ad a 0 after the "." for a .01%). You can always reset to default values with the tab.

I use the free version of DraftSight for viewing the results. The splines / polylines has stumped many of CNC professionals, some programs like AutoCad has a dongle that will fix them. Do a search on the inkscape site for Importing Splines / Polylines they may have a work around for it as well. Keep me updated as the current 6x12 build will use CorelDraw & Inkscape like you are..

[beefy]

Are we getting a bit off track here ??

The op says he's used a variety of file formats from a variety of different cad programs, yet he still has the same issue.

I use Coreldraw all the time and export as DXF. >> SOMETIMES << the DXF export is a bit screwed up, but most of the times it's not, at least it imports into Sheetcam fine, and generates a cut path fine. Is Sheetcam fixing any issues with the Coreldraw DXF export, I don't know.

Here is a quick drawing I did in Coreldraw and the subsequent DXF import into Sheetcam.

Size is perfect, circles are perfect, and cut path generated perfect. For me that is normal most of the time.

Seeing as a variety of files from a variety of softwares are all resulting in the same issue, I'd guess the problem lies elsewhere.

[Les Newell]

If the files look correct in SheetCam it is most likely a post processor issue. What controller does your machine use? What post are you using?

[859Design]

If the files look correct in SheetCam it is most likely a post processor issue. What controller does your machine use? What post are you using?

Richauto A12 for the controller and I picked the Richauto post processor from the menu. I was thinking it might be a post issue since multiple files from multiple sources had issues once viewed in the Cnc Simulator.
I made a simple bracket in Draft Sight and it opened in Sheetcam but had an extra box around it that was not part of the original drawing. It was a separate layer. I got the code and ran it through the simulator, it looked fine so I ran it on the machine and it cut perfect.

[859Design]

I tried using other post processors and then run them through the simulator. The results were much better but still not perfect, it has to be a post processor issue then wouldn't it? Or how sheetcam and the PP are integrated.
Not being able to do anything after spending the money on a license is a pain.

[Les Newell]

I just tested the richauto post and found a bug in it. I have attached a copy that should work correctly. To install this post, open the attached zip file and extract the post any convenient folder on your computer. Run SheetCam and go to Options->machine->post processor. Click on the 'Import post' button. Using the box that appears, navigate to your post and open it. Go back to Options->machine->post processor and make sure your post is selected. It should say 'Richauto (edited)'

[859Design]

Thank you Les, I will give it a shot and report back.

[859Design]

That seems to have fixed it for all the files I have used so far. Thanks