Exporting T-Spline models to PRO/E: spread the smooth shiny goodness
By Kyle Houchens
Owner and principal designer
The Outside Digital Art and Design LLC
A frequent question tossed at the T-Splines crew is, “how does T-Splines work with _______” (insert favorite CAD product here). T-Splines obviously works great with Rhino, but more and more I hear people looking to expand the application of super smooth T-Splines goodness into other programs like PRO/E and SolidWorks.
There is really no magic; T-Splines objects are by their very nature smooth and watertight. The fidelity of the surfaces is fantastic, and transfers to other CAD packages work great!
To demonstrate this process, I consulted my good friend Paul Dowd at Creative Engineering. Paul is a brilliant engineer and true PRO/E magician.
Let’s look at a typical transfer to PRO/E. The process would start in Rhino. I am using an extremely simple part for this demo, but the process works just as well for complicated models.
Using the T-Splines plug in, create a model, then push and pull it until you are happy. Add thickness (Thicken tool) if you are creating a shell, or leave it as a watertight solid volume. From here you simply select the T-Splines object and export selected (file>export selected). In my experience, STEP AP214 automotive design CC2 works quite well and is more reliable than IGES. Rhino will also export ASIS and Parasolid, which both have worked well for me as needed.
Once in PRO/E, simply import the file where it is treated as an imported solid. The easiest way to do this is to drag the STEP file to a modeling window and select “append” from the import dialog.
To import from the menu, use insert>shared data>from file.
You can shell the model, add features, or perform any operation that you can with any other imported solid.
You will not have any parametric association on the imported object, and as such cannot make parametric modifications to the imported part. Anything you build on the part (bosses etc) can be parametric, just not the imported object.
If in the process of engineering the model, the imported object needs to be modified, simply go back to your original file, modify the part as needed, and export the model again. In this case only a few surface patches were modified, so I extracted and exported just the surfaces that changed.
Back in PRO/E, drag the new surfaces into the modeling window as before.
Once the surfaces import, use the “replace” operation. To get to this screen select the surface to be replaced and then hit Edit>Offset, then pick the “Replace Surface Feature” represented by the white and blue icon in the lower left hand corner of the screen. Click on the little box that says “1 item(s)” and select the new surface to use as a replacement. Hit the Green Check in the lower right corner and this is what it looks like right after the replace.
You can see that the model is all white, no surface geometry, all solid geometry. The next step is to resume all the features. If you have not made any references to imported geometry that got changed, and if your features still “make sense” in the new context, the features will resume without complaint.
This is an extremely effective process for common design/engineering issues like dealing with packaging issues or making a mechanism fit.