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Drawing Exporting DXF Issues

caz_waskowiczcaz_waskowicz Member Posts: 2
I have an issue exporting an Onshape drawing for a vendor to waterjet. My vendor uses BobCAD and Mastercam and cannot see the geometry in my exported drawing in either program.  I'm thinking this has something to do with how Onshape handles "model" and "paper" space and which it exports to? --- there aren't any options when exporting, it just does it.

I work with this particular vendor a lot at my job where we use Solidworks. I send my vendor .dxfs all the time from Solidworks without issue. Any ideas?

(only thing I found that works is going to a part studio and exporting the face of the part I want to a .dwg and then manually compiling all my faces in a 2D cad program---would like to just be able to export the Onshape drawing instead)



  • michael_mcewenmichael_mcewen OS Professional Posts: 76 PRO
    I'm having the same issue.  I'm new to CAD (20 yrs hand drafting), I learned Onshape specifically to send dxf files to our waterjet cutter.  I sent him the following Onshape Drawing file:


    Here wass his response:

    I was able to open this file on one of our newer software packages but the file came in pretty bad.  All the arcs were generated with short straight lines and also did not define the arc very well.  They were choppy.

    I'm not sure what software he's using, and I'll find out, but this is a considerable set back for me.  I love Onshape, especially its browser based platform.  But, after putting in 50+ hrs self training, this is an extremely disappointing discovery.  

    In Drawings, does the "Refine Graphics" have any effect on the dxf export?  Any suggestions?


  • michael_mcewenmichael_mcewen OS Professional Posts: 76 PRO
    The software my waterjet cutter uses is called "OMAX Intelli-MAX Layout."
  • john_mcculloughjohn_mccullough Moderator, Onshape Employees Posts: 38
    The DWG or DXF export from Onshape drawings is still using graphical "proxy objects" instead of basic AutoCAD entities. The proxy graphic objects in the DWG/DXF can be exploded (if you have the right software) but exploding results in short segment polylines which sounds like the problem you are seeing. 

    For CAM-friendly DWG/DXF output from Onshape today you'll need to export the face of your 3D model to DWG/DXF instead of exporting the drawing. In the Part Studio select the face and right-click. Select Export as DXF/DWG from that menu. This DWG/DXF output will give you nice clean arcs. 

    If you want to send the drawing too (with the dimensions) you could use PDF for that or just explain that there are two types of DXF/DWG files you are sending. The Part Studio exported DXF/DWG should work great with OMAX Layout. 
  • martin_feathers599martin_feathers599 Member Posts: 2
    I think it would be helpful if there was a way to choose which version of AutoCAD to export DWG/DXF files to. Our Shop currently has engineers using AutoCAD 2004
  • martin_feathers599martin_feathers599 Member Posts: 2
    edited February 2016
    OOPS Guess I should of investigated before I posted. I see that exporting a face as a DWG gives you the choice of versions when exporting a face. It would help to be able to do that from a drawing
  • michael_mcewenmichael_mcewen OS Professional Posts: 76 PRO
    Thank you john_mccullough, This is very helpful.  In exporting the DXF from Part Studio, I see multiple versions (see screenshot).  I have no idea what these are.  Any suggestions on which to chose?  Thanks again,  Michael
  • john_mcculloughjohn_mccullough Moderator, Onshape Employees Posts: 38
    Exporting simple profiles like you are doing will generally work the same with any of those DXF/DWG versions. Some older controllers need Release 9, which will convert smooth spline curves into short straight polyline segments. It sounds like the OMAX software can support all or nearly all of these. I'd suggest using Release 14. 

    The differences between these versions are mostly related to drawings. 
  • michael_mcewenmichael_mcewen OS Professional Posts: 76 PRO
    Thanks again John.  By the way, I did successfully send out my first 2 dxf files to my vendor, and he was able to read them!
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