Plasma arc's look faceted when cut, not sure why?

[marbles]

Wow, your right! I rarely open the Mach3 toolpath window and its most definitely reading it as a series of straight lines. The question is why?

[magicniner]

I'm guessing that your Post Processor isn't outputting code that's compatible with your Mach3 configuration.
Sadly my expertise on these is limited to my own system but I'm sure someone with greater wisdom will enlighten us ;-)
Regards,
Nick

[marbles]

I just imported the dxf kindly uploaded by Web Goblin directly into Mach3, getting mach3 to generate the code. No segments, nice and smooth?

Indeed Hopfully someone with greater wisdom will enlighten us ;-)

Thanks

[Neale]

A quick look at the gcode immediately shows that it's a series of line segments - there's a G1 near the beginning, then just a series of coordinates thereafter which will also use the implied G1. Not a G2/G3 in sight.

My guess is that the DXF you are exporting, for some reason, is using straight line approximations and not curves or arcs. I've had that problem exporting from Adobe Illustrator and it turned out to be that I was not using the latest available DXF format. Can you explore that?

[Web Goblin]

I had a quick look at the original dxf and it is made from polylines. Most post processors cant understand them and break them down into loads of little lines. That way you get the kind of effect your are getting with it. Curves end up being made from straight lines. This also causes machines to stutter when trying to process the code also prevents them from reaching top cutting speed due to the amount of code they are trying to load and run.
Take your original drawing and then draw over it in cad using lines and arcs only. Then save it as a dxf and post process it again and try the results. Hopefully you will get a nice smooth contour.

[Neale]

One more thought - not sure about Aspire as I use VCarve, but in VCarve there is a "convert to curves" tool. Letters seem to be created as a series of line segments but you can use the "convert to curves" tool to, presumably, convert to curves... I have just done a quick trial but the CAM post-processor in VCarve itself seems to give straight line segments in the gcode in either case. However, it might be that the dxf written out is different which might help with a different CAM processor.

[Robin Hewitt]

Convert to curves usually means throwing away details of character and font so you are left with a fixed outline. If the outline is too steppy, look to see if there are any parameters you can tweak in the Convert to Curves command.

[magicniner]

I just imported the dxf kindly uploaded by Web Goblin directly into Mach3, getting mach3 to generate the code. No segments, nice and smooth?

That points the finger firmly at the software you're using to generate your dxf files, stop using it and use something people who don't have the issue use.