Ah. I think I'd simply copy the surface and trim / split it. If it's the
part you want to split you can either do a solid operation (suppress /
delete after export) or select a solid face / surface, RMB, select Solid
Surfaces, then ctrl+c, ctrl+v to copy the entire shell then trim or split
that. When you export you can write out just the quilt you are interested
in instead of the entire model.
Although there are modules for FEA applications such as ANSYS that allow the
user to import Pro/E models directly, I still generate 3-D IGES files of
Pro/E models and bring them into ANSYS. So when I have a task such as yours
where I want to split up a surface, I just export the Pro/E model to IGES,
import this IGES file back into a new Pro/E part file, and then perform
surface trim operations making sure to keep the resulting surface geometry
on both sides of the trim curve(s). Next, I simply generate a new, 3-D IGES
file and bring the second IGES file into the ANSYS FEA application.
An alternative approach to this would be to create a Publish Geom feature
consisting of all of the model's surfaces, and then create a new Pro/E part
file that contains an External Copy Geom feature that references the Publish
Geom feature in the solid model. This would allow you to keep your 'all
surfaces' model associative to the solid model. If you made changes to the
solid model, the Publish Geom feature in it would update and also force the
External Copy Geom feature to update.
It would be nice if solid surfaces of regular Pro/E Part models could be
broken up into regions in the same manner in which Pro/SHEETMETAL solid
surfaces can with the Deform Area functionality. Deform Area works great in
Pro/SHEETMETAL for creating Edge Rip features that do not extend to the
exterior solid edges of the sheetmetal model. As an example, a three-sided
Edge Rip feature that references a Deform Area's edges would allow you to
ultimately create a retention barb/lance feature that simulates a real-world
sheetmetal sheer and bend operation sequence.
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