Modeling logo as solid geometry on non-flat surface, given .eps file

[MikeLockwood]

Hello all - I'm 100% sure that others have already solved this problem well. Hoping to get a pointer to a how-to.

Given an .eps file with some simple artwork.

Need: Apply to a solid part model

Assumed technique:

- convert .eps to .dxf (this works - couldn't find a way to convert to .iges yet)

- import into a sketch (zillions of separate line / arc segments)

- project sketch onto part

- use offset, apply depth and draft

Appreciate anyone pointing me to a detailed how-to on this. There are some limited writeups on ptc.com about this - studying and trying them now.

thanks!

//////

One related set of info is: https://support.ptc.com/appserver/cs/view/solution.jsp?n=31610

It assumes that you are using IGES. So far I've only been able to convert .eps to .dxf.

"If logo is to be solid geometry (e.g. an impression on a block)

============================================

1) Obtain an IGES file of the logo, or .sec file from Pro/ENGINEER.

Create a cut or protrusion and while sketching the section, import

the .igs or .sec file with Sec Tools, Place Section. Dimension

appropriately."

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[psobejko]

There is a very recent discussion about importing DXF logos:

How to freeze a sketch

One useful video shows you to how to get the sketch geometry into the model:

Video Link : 6037

from there, you can use the offset tool to get the engraved/protruding shape w/ draft.

Embossed artwork on Cone shape?

How to emboss a text on circular surface similar to wrap by using offset?

Emboss text on solid cylinder, Creo parametric 2.0Embossed artwork on Cone shape?

...

and many more examples can be found on this forum.

[KenFarley]

Creo will let you open a DXF file, you could then use the "Save a Copy" functionality in the "File" menu to save it as an IGES file.

The difficult part will be if there are any unconnected line segments. I've tried to import complex logos into sketches before and this can be a real tough problem.

[mpeterson]

Yes the previous freeze a sketch discussions address this in many ways. I still think the best way to handle this is to just prepare this in a separate part and copy geometry into the target part. In a new part import a DXF or DWG file into a sketch and save as is with the default dimensioning. Then create the line art in simple sketches using the imported sketch as a template or guide to create simpler line segments. Recreate the line art in many separate sketches to make each sketch easier to control. Once the entire at is create then create other curves or datums planes and coordinate systems as reference in locating appropriately in the target part. Then you can make a copy of the original for each usage so it can be scaled for each part. If need be measure the art work and then compare it to the size desired and scale it accordingly. Copy geometry as preferred to get the line art in your part. I prefer to Publish Geometry from the line art part an then Copy Geometry in the target part. You can also assembly the part in an assembly with the target part and then use edge (now project) for your extrude or offset feature to create the artwork in your solid part.

It takes more time up front to do it this way, but if the art will be used many times or it might be modified it is well worth it later like with many modeling practices to get robust models that change easier and are more controllable.

[handel]

The zillion entities can be a real pain. Converting .eps to .iges is done with Rhino.

I found out that the Rhino route works the best for me. Rhino is even capable opening native AI files.

Also scaling, orienting an positioning of the artwork is done much easier in Rhino. Import in Rhino a drawing scale 1:1 of your Creo part, add the artwork and start placing it correctly. Hide your original part, save as .iges, import it in Creo, and you get exact the same number of entities as created in the original artwork. Far more easy as it has to be mapped on complex surfaces, with multiple tangent edges along it.