We are trying to get a graphic from .DXF molded into a part. Pre Creo we were able to select the whole sketch, or at least select loops. Now we are selecting little individual entities. What is the trick I forgot here? Thanks.
When selecting edges use the loop option for a better chance of getting the entire letter per selection.
Also I would highly consider using the imported DXF as a template and then create the text in Pro/E sketch. You will need to copy the correct text file from your windows fonts into the Pro/E font folder and restart Pro to get it available. Because these imported DXF's and DWG's always have tons of small segments and missing pieces and stuff out of line, etc I typically will use the import as a template and recreate with multiple sketches in Pro/E. If its something used many times over you can put it in a library and import the Pro/E file and resize it for reach application. I have typically made a flat surface of logos to Copy Geom from and than place in each new part and resize and use edges. Takes extra time up front but it's worth it in the long run like most good modeling practices.
Mark A. Peterson Design Engineer Varel International
I have had good luck reading in the dxf or dwg file as a Pro/E drawing, with an empty format. Then save the new file as an IGES file. Next, in your target part, you will need to create a new CSYS that has adjustability built in so that you can both move and rotate the new CSYS. Now import the IGES curves and attach them to the new CSYS you created. Now all you need to do is move and / or rotate the new CSYS into the proper location and the new datum curves will follow along for the ride. Next, create the protrusion or cut using the imported curves and select "loop". Sometimes the loop option will not catch everything and you may need to select individual entities in your sketch.
Bob Schwerdlin Sr. Design Engineer Dukane Corp. 2900 Dukane Dr. St. Charles, IL 60174 USA 630-679-1941 direct - www.dukane.com/us