DXF export not working properly ?

[TrippyLighting]

I am trying to export sketches of a certain logo into a dxf file for laser etching. The original sketch including a number of splines is this:

The exported DXF seems to be missing either the splines or segments of the outer circle depending on which viewer I use. I've used Inkscape, eDrawings and the A360 DXF viewer.

Then I extruded the Logo and projected that onto a second sketch and saved it, but it also returns imperfect DXF that is also 180 rotated on it's head. Both DXF files are attached.

Are there any settings that need to be observed for proper DXF export ? (I have not found any)

[PhilProcarioJr]

I have this exact same problemif its not extruded into a 3d object.

Also make sure your sketch is oriented on the front plane.

If you do a simple push/pull and give it a thickness it should solve your problem of missing lines/splines.

After extrusion I don't project it, just export the 3d object as a dxf and then open it in inkscape this should work. At least it did for me yesterday on two projects I was working on.

It seems we have found a bug in the dxf export. I found it yesterday but I was busy and didn't have time to report it.

[jeff_strater]

Hi @TrippyLighting.  I know that Inkscape does not handle splines in our DXFs:  splines-removed-when-saving-as-dxf.

I can't explain why you don't see the splines in the A360 DXF viewer.  I admit that I am not familiar with that particular tool.

However, I re-imported those DXFs into Fusion, and it looks to me as if the results match your original:

Or, am I missing something here?

I did notice that your second DXF is, indeed, "backwards", when viewed from the "front":

But, without seeing the F3D that it comes from, it's hard to say whether this is an accurate result

Jeff Strater (Fusion development)

[PhilProcarioJr]

Hi Jeff,

One problem is that other apps that export dxf files can and do export the splines.

For people that do laser engraving this is essential, I understand if you reopen it in fusion 360 it works but that doesn't help us use it for laser engraving.

When this happened to me I wasn't even using splines, it was a simple box and a circle yet it was still missing two lines.

This problem is also reproducable and its not just inkscape, I tried 7 different programs including the viewer on the cloud and all were missing lines.

[HughesTooling]

Rhino reads the file but I get this error message.

I get the image above if I click continue reading but if I click stop reading I get the error report.

I've attached the file exported from Rhino, see if that's usable.

The import looks OK but there are some extra short lines in some places, shown in red in this image.

[jeff_strater]

Sorry, my point here was only that the data is inside the DXF, so it's not like Fusion is dropping curves entirely.

Now, it's a different question about what other tools do with this data.  One possibility is for Fusion to expose a "DXF version" in this command, so that we can fall back to an older version of DXF, or possibly an "approximate curves" option so that you can produce a DXF that any tool can read.

Jeff

[TrippyLighting]

Here's the F3D

[daniel_lyall]

fusion has a hard time with dxf import or export the only program I dont have problems with is takeing them in and out of V carve pro in or out it`s fine. autodesk 360 has problem`s with dxf as well.

if I have a dxf that fusion or autodesk 360 does not like I run it through V carve pro and save it back out as a dxf then fusion and autodesk 360 like them same in reverse take a dxf out of fusion to get it to work in other program`s running it through V carve pro first fixes it.

I can show it quet easyly if you wont.

@TrippyLighting if you wont send me the dxf I will run it through V carve pro for you Ill test the one`s you have posted now.

give me 5 mins

[HughesTooling]

Here's another export from Rhino. The first file I attached converted the splines to lines, this one should still have all the splines in it.

[daniel_lyall]

spline are the problem I changed the spline`s to 3 point arc and it came right on a .dxf export attached image you can see the spline handles the 2 straight short lines, the curves are arc`s and the short line you can see down lower is another handle. so splines don't work with .dxf export but arc`s do another hatted work around. so @jeff_strater there`s the problem spline`s get lost and the handles get left behind another thing to add to the list to get fixed.

also export to .dxf (splines as Polylines) works you just get left with some handle to get ride of see b.dxf

now that was a good bug finding session 

[PhilProcarioJr]

When I had lines dropped off they were not curves, just regular lines. and even the viewer in the cloud for fusion 360 did not show the lines.

On another note not sure if it would help at all, but in other programs I always use Auto CAD R14 as the export compatibility and rarely if ever have problems.

Maybe this is an option to help fix the export...idk

[HughesTooling]

I experimented with your file and created 2 planes either side of the part and projected sketches onto those planes. Both of those sketches come out wit the correct orientation you only get the upside down problem if you select a face for the sketch rather than a plane. I guess when you select a face the Z direction is reversed.

File attached with extra planes and sketches.

[TrippyLighting]

Thanks for all the help!

It looks like the projected sketch dxf should be fine, however the export of the original sketch actually looks like that some of the spline handles are exported.

the friend who helps me with his laser citter reported that the projected sketch imports fine without loss of lines/data into the laser cutter software BTW.

I'll checkout how things look in Geomagic desing tonight (or so).

[TrippyLighting]

@jeff_strater

I just checked the DXF exports in Geomagic Design.

#2 is perfectly fine wiht the exception that it's turned on it's head but as has alredy been expleined that would be an easy fix.

#1 clearly exports the spline handles as line elements and that would appeare to be undesireable if not a bug.

[jeff_strater]

Thanks for the clarification @TrippyLighting.  I agree, if we are exporting the spline handles, that's a bug.  Thanks for bringing this out.  I am planning on some meetings next week with the sketch team, and we will also discuss what can be done to make the DXF export more forgiving for other tools that don't support all of the entities that we export.

Jeff

[TrippyLighting]

Thanks. The #2 export worked fine for the laser cutter software of my friend's laser. It is basically an inlay of darker acrylic into a pinkish acylic as we did not have any clear on hand.