Splitting in two a surface from a solid model

Hi,
Is there an easy way (without having to create surface copy of my solid) to split in two a surface that belongs to solid model? I have
projected a datum curve to the surface but it doesn't split the surface in two? I'm using WF2. Thanks for your help.
Pablo,
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Could be wrong, but don't think so.
Why do you want to split the face / solid geometry surface?
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Hi,
I want to use half of the surface to applied a pressure in a FEA software, instead of doing it in the FEA software, I would like to do it in the CAD software if possible. Thanks.
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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.
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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.
Ron M.
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