S3 is cutting faceted line segments instead of smooth spline

[danelectro]

I've had my Shapeoko 3 XL for a few months now and I'm finally finding time to play around with it. I make custom pickguards for guitars and the outlines are generally flowing shapes which I model using spline features in my CAD system. The splines are smooth in the CAD data. When I view them in Carbide Create while programming the tool path they also appear to be smooth so I know the the CAD file is being imported cleanly, however when I cut them with the S3, the splines come out as faceted line segments.

CAD:


MDF template cut on the S3


Arc features cut smoothly so I know its not a mechanical issue with the machine. Either Carbide Create is converting the splines to segments when it generates the toolpath, or else the machine controller is segmenting the splines. There are no accuracy or resolution settings in Carbide Create so I'm not sure how to resolve this. I think first I need to identify if the problem is with Carbide Create or the GRBL controller on the machine. I'm well versed in CAD design, but the CNC thing is all new to me. I like the simplicity of programming with Carbide Create, but if I need to upgrade my CAM software I guess that's what I'll have to do. Any thoughts?

[WillAdams]

What Settings are used in the CAD app when exporting?

There are some notes here: http://www.shapeoko.com/wiki/index.php/ ... e#Features

How does it look in Carbide Create's preview?

Possible to get a .eps or .pdf out of the CAD app, import that into Inkscape, then save as a .svg which Carbide Create will open?

[SmokyRick]

You really need to read your program and find out whether it is calling for a smooth arc or a series of lines. If it is calling for a series of lines, the problem is in that end of your process. If the program calls for a smooth arc, then you may be feeding it too quickly and the tool is actually flexing until it leaves what you see. At least this will start the process of tracking down the problem.

[danelectro]

Thank you for the advice. One problem is resolved, but another has popped up.

First of all, I was mistaken in my comment above when I said the spline appeared to be smooth in Carbide Create. I took a look at the file again and the spline actually did become faceted when the DXF file was imported into Carbide Create. Here is a screen shot of Carbide Create with a direct import of my DXF file. Note the faceting of the spline that is most apparent on tight bends:



I imported the same DXF file into Inkscape and the spline is smooth as it was in the CAD program in which it was created:


From Inkscape I saved the geometry as an SVG file which I then opened in Carbide Create. The spline now looks perfectly smooth, however for some reason all of the straight lines have disappeared. The spline and arcs are present, but there are no line elements. In Inkscape there are several different options for saving SVG files (Inkscape SVG, Plain SVG, Optimized SVG). I tried saving each type and they all result in the same output:


As a check of the file's integrity, I imported the same SVG file into MakerCam and the spline, arcs, and line segments are all intact (the centerlines are missing, but that is probably because they were created as draft entities rather than true line geometry elements) :


Even though DXF and SVG are supposed to be neutral file formats, its apparent that each program looks at them in a different way. I'll keep playing around with various ways of importing and exporting the files and hopefully come up with a combination that brings all of the geometry into Carbide Create.

[WillAdams]

We've had this come up in the past --- in Inkscape, you should be able to select a path, and it should be a single continuous thing (which is closed)

I prefer to only send compound paths in (old habit from the MakerCAM days).

Unfortunately, the only app which properly handles selecting and joining lines automatically (Macromedia FreeHand) got bought and buried by Adobe.

[danelectro]

Update: I've tried this a 100 different ways with no success. The CAD program I'm using is older (ANVIL 1000MD) and there must be some parameter in the DXF export that Carbide Create doesn't like. I can import the file into Inkscape and it looks perfectly fine, but when I export the file as an SVG then bring it into CC certain drawing entities disappear. I have two other CAD programs (2D DraftSight and 3D ProEngineer) and I've tried importing the pickguard dxf into them (it looks fine), exporting a new dxf from there, importing it into Inkscape (it still looks fine), exporting an SVG, but then when I open the SVG in Carbide Create, those same entities are missing. On a side note; Carbide Create doesn't remember the last file path and keeps reverting to the desktop, so every time I want to test another imported file, I have to navigate to the full folder path (which happens to be a fairly long path). Hopefully that can be fixed in the next cut of CC.

In the meantime, I've found a workaround: I've given up on trying to run my DXF file through Inkscape. Instead, I took a closer look at how Carbide Create is faceting the spline feature and I've determined that it breaks a spline element into 100 facets. The part was modeled with a single spline entity that makes up 80% of the part's perimeter and thus those segments become very noticeable as the spline bends around tight corners. As an experiment, I broke the spline up into short lengths that are all connected end-to-end. I imported the DXF into Carbide Create and as I hoped it converted each individual spline segment into 100 facets which are now much smaller in length. In the image below, I broke the spline up into 23 segments, so now there are 2300 facets running around the perimeter rather than 100. Even though the perimeter is still faceted, they are so small that they are insignificant. I created a toolpath using this geometry and it didn't seem to take any longer to generate and the file size isn't overly large, so I think this is going to be my workaround.

[WillAdams]

Out of curiousity, did you try saving the SVG out of MakerCAM?

[danelectro]

SUCCESS! That's one translation path that I hadn't tried and it did the trick. Processing the DXF through both Inkscape and MakerCAM results in long single entity spline being smooth and all lines and arcs are present. Here are the steps the led to a successful translation:

1) Import the DXF file into Inkscape

2) Save the file as an SVG in Inkscape

3) Open the SVG file in MakerCAM

4) Save the file as an SVG in MakerCAM

5) Open the SVG file in Carbide Create. Everything looks good. WooHoo!

Its bizarre that when Carbide Create opens the SVG file directly from Inkscape that some geometry features disappear, yet I can take the exact same SVG file and simply open then save it in MakerCAM, and now it will open in Carbide Create and all entities come across. There's a bug in there somewhere (I think on the Inkscape side), but Its just a couple of extra steps to post-process the DXF file so that it can be opened in Carbide Create with all features intact so I can deal with that. Its a better solution than breaking the spline into multiple segments as I outlined above. In the future I'll be cutting a lot of parts comprised of spline features, so I'm happy to have a way to get accurate geometry into Carbide Create.

Thank for your assistance Will!

Here is the clean geometry in Carbide Create after processing the DXF as noted above:

[WillAdams]

Very glad it worked, and my apologies for not thinking to suggest this earlier.

MakerCAM seems to stitch SVG files together nicely / pre-emptively, while Inkscape tries hard to honour the original file, while Carbide Create (as I noted) expects files to be properly put together (left-hand fill rule / winding, and composite paths).