Summary: What is the preferred technique for modeling very thin parts?
Although this summary is late, I needed to experiment with several techniques before issuing this post.
Here are some edited suggestions from several other users:
Sheetmetal:
a.. I believe in sheet metal you can define the part and then later revise it to reflect a combination of internal and external dims that would work very well for us also. Our experience with the thicken command using surfaces is similar to shelling, but with the surfacing you can do some pretty interesting things like merging, trimming and even free form surfaces.
a.. I tend to make them solid. If it is a curved label, and you want to show it in the flat form in the drawing, but the curved in the assembly, sheetmetal works great. The main con of the sheetmetal version is that you will then have a family table of the flat and formed parts, so you BOM will call out the formed name in the assembly. a.. I'd suggest the sheet metal package since it allows you to create both flat and formed parts. We've used it for labels on assemblies and it works OK. Keep in mind that you'll need to create a simplified rep for the part that adds the flat pattern. That simplified part cannot be used by itself. It has to be used in an assembly-simplified rep. You could also use a family table, which includes the flat pattern. It does work but I'd stay away from it if you were using Intralink.
Surface Modeling:
a.. For layers of material such as composites the surfacing modules will offer more flexibility where needed. If you have a series of layers as parts make sure the parts are independent or you will be creating circular references or .crc files. Which will slow down the assemblies by multiple regenerations. If this is the case where you have multiple layers of materials may want to refer to conforming geometry thru skeletons with data sharing copy geometry or inheritance copies to avoid .crc's
a.. A user suggested this module. However, I could not find good examples, and PTC tech. support indicated it cannot fold and unfold (form and unform) a part, so I did not experiment with this module. a.. Not sure if you have access to the Pro/COMPOSITE module but what you describe is why it exists.
General comment:
a.. I'd personally go with Option A--thin protrusion. I'd stay away from Sheetmetal, as it will be too much of a pain in the end. Option C (surface modeling) is pretty much the same as Option A in Wildfire. Summary: Although thin protrusion was an option, I needed the part in a formed condition (bonded to a curved surface) and in a flat state in the drawing. So I chose to use the Pro/Sheetmetal option. In sheetmetal, a form punch (PTC suggested that form punch is preferable over the form die) needs to be created to produce the desired form in a thin part, which is an elastomeric pad in this application.
Also in surface modeling, there is an option to flatten quilt. When I inquired about this with PTC tech. support, it was indicated that the quality of the geometry is better using the sheetmetal module for this particular application as opposed to using surface modeling, then flattening the quilt.
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