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

[MM_13015271]

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:

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): 

• 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! 

[Chris3 · Accepted solution]

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.

[MM_13015271]

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

[KenFarley]

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.