Import 2d dxf dwg into sketch mode without overlap and open lines

[ptc-5221874]

I try to import some 2D data with the option "Data from File". I tried many things in autocad like closed polylines or blocks. However when I import the sketch there are open lines and overlaps between curves and lines. So I guess it has something to do with the import routine. Then I changed some config.pro settings but this didn't helped either. I have Creo Elements Pro 5 (m170 education).

I don't know what to do after 7 hours trying to import 2D data. Could it be that this expensive professional software cannot handle 2D files? Or has somebody a solution for a better import or an after import fix?

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[TomD.inPDX]

The sketcher has a solver and it is trying to solve the DXF import. Try opening it in a drawing instead. Edit it to what you want the sketch to be and then export it again to DXF. If the DXF is simple enough, the solver will only apply dimensions to the geometry. Sketcher is -not- a way to make a simple series of curves. It is a very sophisticated piece of software.

You can also open the DXF as a part. Next you create a sketch and you can project the imported curves to the sketch. the two will have an associativity until you break that associativity (such as saving that sketch to a *.sec file). But once you break the associativity, you also need to provide the data to make that sketch parametric.

Creo is -NOT- Autocad... Creo is a real CAD system

Welcome to the forum!

[ptc-5221874]

Thank you for your answer.

Open the DXF in the drawing mode and save it as DXF or DRW for reimport to sketcher doesn't help. It looks the same and sadly my DXF is not simple.

To open it as a part and create a sketch..., there I see the curves and lines but I don't know how to project it to gain a new sketch. Or do you mean I need to redraw it and the projection is only for the support?

Maybe I think to simple for this sophisticated piece of software. I only want to extrude an existing 2D-DXF to an 3D-part. I can understand that the sketcher has a solver (and take everything apart) but it would be nice that I could configure or teach it to solve my specific problem. "It looks to me that it can translate a sentence only to single words and is not able to form a sentence again."

I can also trimm the overlapping none closed sections but there are many of them and with some it is not working. And I think a software should make the work more easy and fast and not complex and time consuming.

[JonathanHodgson · Accepted solution]

Hi Christian,

Try this approach:

• Open the DXF as a part, or alternatively you can import it directly into a part (Insert -> Shared Data -> From File in WF4).
• Create a sketch on the same plane as the DXF.
• Select the Use Edge tool, choose Loop, and pick each closed loop in the DXF. This should give you a fully constrained sketch which references the DXF import (although there is no parametric link to the original DXF).
• Exit the sketch and select the Extrude tool (with the sketch still selected). Alternatively, you can create an extrude and then create an internal sketch as above.

HTH,

Jonathan

[ptc-5221874]

Hi Jonathan,

Thank you very much for explaining it in detail. It is really working and it seems that this way has the fewest mouse clicks to get the wanted result.

Cheers,

Christian

[TomD.inPDX]

Use Edge must be the WF term for Project in Creo sketcher.

[ptc-5221874]

Ok I see. I am using a german Creo and it is the edge term. That is why I couldn't find something with "Project" or similar in german.

Kante -> Verwenden

[JonathanHodgson]

I must admit that I didn't immediately 'get' the "project" instruction either - possibly because I chose to create the sketch on a plane coincident with the DXF, and therefore I didn't think of it as "projecting" the entities.

[TomD.inPDX]

Terminology in Creo can be very confusing. Throw in language differences and I don't know how you guys do it

Glad the problem is resolved.