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M
MM_130152715-Regular Member
5-Regular Member
February 18, 2026
Solved

(Creo12) DXF Export from Drawing - Sketched outline turns into blurry image

  • February 18, 2026
  • 2 replies
  • 132 views

Hello everyone,

 

I am working with Creo Parametric 12.4.2.0 and I want to export a .dxf file from a drawing, using:

File > Save as > Export > DXF 

I usually use a sketch or a solid from a .prt file and place it in my drawing to do so. This works perfectly fine in Creo 3 and 6. 

My problem is, that whatever is contained on my drawing, gets turned into a image, when exporting it via Creo12. 

So if I open the .dxf file in another software, I do not have single splines or curves anymore, I have one big, very blurry, image, as seen on top here:

 

MM_13015271_1-1771420789820.png

 

What have I tried:

  • using a solid part as a base
  • using a sketch as a base
  • trying different dxf versions
  • deleting layers for the export 
  • checking unit is the same between .prt and .drw 
  • export without drawing boarder
  • export with drawing boarder

 

What I found out:

  • creating the sketch directly in the drawing file returns a clean assembly of lines - but I do not want to re-draw my designs from the .prt. So this is not a solution. It looks like this (top - image, bottom - sketch as it should be): 

MM_13015271_2-1771420996432.png

 

  • creating a sketch directly in the drawing files AND adding a solid from a .prt combines both problems and also creates a new problem: in the preview of the dxf, I see my sketch and the solid. if I open the dxf in a different software, the solid does not get exported but instead the sketch in the .prt gets exported, which is not even visible on the drawing.

 

So I assume something goes wrong in the communication between .prt and .drw. 

I have checked the config options, but so far I have found nothing that sounds like it would fix my problem.

Does anyone have experiences with this or may know a config setting I could try?

 

Every idea is very welcome - thank you very much! 

 

Best answer by Chris3

Is it possible that you are placing the view as a shaded view in Creo 12? That would make it an image.

 

If it is a no hidden lines or wireframe view it should export out as splines.

2 replies

C
Chris321-Topaz IAnswer
21-Topaz I
February 18, 2026

Is it possible that you are placing the view as a shaded view in Creo 12? That would make it an image.

 

If it is a no hidden lines or wireframe view it should export out as splines.

    M
    MM_130152715-Regular MemberAuthor
    5-Regular Member
    February 19, 2026

    This was it, thank you so much! 

    I tried it and it worked. 

    I also cross-checked with Creo 6 again and saw that even if the part is shaded, the view on the drawing is automatically set to "wireframe". This is still missing in our Creo12 set-up, so I will go searching for this setting now. 

     

    Again - thank you so much for your help! 

     

    Edit: if somebody comes across this problem in the future, the config setting is:

    enable_shaded_view_in_drawings -> no

    K
    KenFarley21-Topaz II
    21-Topaz II
    February 18, 2026

    It's not an elegant solution, but a possible way to get the DXF you need might be to select the view, then use

     

    Edit -> Convert to Draft Entities

     

    This will take all the stuff that's visible in the view and render it into a bunch of "dumb" curves. There's no going back to the regular view after doing this, so either don't save or do the work with a temporary copy of the drawing.

    Sorry I can't try this stuff with Creo 12, we are on Creo 9.

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