SUMMARY: Adobe Illustrator files for datum curves...
Thanks for all the replies. I have included all the replies for your review. The one I ended up using was using the config option:
It worked like a charm.
Here is the summary:
We export as dxf from illustrator. Then import into a 2d drawing in ProE (this is the important step). Cleanup the 2d as you see fit and move your referencing location to 0,0 on the drawing, then export the drawing as another dxf. Then import this second dxf into the part. I'm an advocate of importing into the part, not directly into a sketch. To do this, you will need to create a csys where you want it imported.
Also, don't forget that if it's coming out of Illustrator before CS, you need to scale to 3.938% of the original.
I've never had the above method break splines and arcs into segments.
When you sketch was broken into little fragments where they broken up & totally unusable?
What might work, if you have an access to illustrator, save the file as a dxf or dwg, then start sketcher & click sketch>data from file, select or dxf/dwg & see how it comes in. It may still be busted up with 1000 gray dims but it should be accurate & usable.
Not sure if this is on one of your menus, but if it is, make sure you aren't exporting as polylines as that would turn any curves into many small chordal lines that approximate the curve.
When I was using WF2 a year ago there was an option to import an ".ai" file format into a part/sketcher, but the time I tried it, it didn't work and I didn't have the time to check out why not. With a new job change I am back on 2000i now so I can't try it at the moment. I would be very interested in learning if this works or what a more effective method is. Please advise or post a summary/result.
I use this config option.
This seems to help some in most cases.
Use the .ai file in sketcher. Sketcher allows you to insert "data from file". Find your .ai file and dimension/constrain and you're done.
There's an option when either exporting from AI (to a DXF) or from drawing mode (to an IGES) of keeping the curves and/or text as splines or making them line segments. It's non-obvious and defaults to the segmented version. Choose splines and most of your worries will go away quickly.
I would suggest exporting the file as a DWG file, then importing the DWG into a Pro-E sketch. If there are too many segments, create a second sketch using the first sketch as a template.
In the attached example, a group feature in the model tree containes the two sketches. The second sketch is projected onto a surface for laser marking. After importing the DWG into a sketch, I prefer to save the sketch as a Pro-E sketch for future use. Also, I suggest creating a "dummy" part to use for copying & pasting the sketch onto the part that requires the logo.
If a registered trademark symbol, "(r)" is needed, this can be done by typing in the ALT keystroke for the character with your keyboard. Do this by holding down an ALT key on your keyboard, then typing "company trademark" (without quotes) on your number pad, then letting go of the ALT key.