37503 wrote: SW will not convert this kind of geometry into a sheet metal part. The problem is that the bends are not flat, they are curved around the centerline of the part while they bend. SW cannot unfold this kind of sheet metal forming. SW will only handle flat formed flanges, like what you would be able to do on a press brake with standard tooling.
SW Sheet Metal can produce (and unbend) flanges formed with a curved folding line. See attached picture and part file (which unfold to a perfect flat pattern).
The part I posted is not "converted" is is a 100% done with Sheet Metal features and fold / unfold correctly and without any errors. I do not understant from where are getting the error.
Attached is another "exotic" thing you can do with sheet metal... (or SW), the attached is an example of a "bended" honeycomb pannel (which is a 3 layer composite). Open the assembly and change the configuration from "default" to "flat" (this will take sometime depending on your machine, since it will need to regenerate the "honeycomb", but it works).
The problem my friend, is that curved-to-curved forming is not a Sheet Metal bending forming process it is a Sheet Metal Stamping process (in fact a flat-to-curved is also a stamping process) and as you already mentioned on a previous post, SW Sheet Metal module is (as it is on all other CAD systems I know such as Pro-E, Catia, Alibre, etc.) a module to use for "bending" processes. In fact, even when SW allow to do a flat-to-curved flage, the flat pattern produced by SW cometimes is not good at all since SW can not calculate the deformations of the material on this type of forming.
You are correct, SW Sheet Metal module is for press-brake (or any other straingth line bending) formed parts, not to model parts to be produced by stamping or deep-draw forming. SW allow the use of "tools" to do this, but it can not produce the "blank" required to produce the formed part.
For example, one of th products we manufacture is Hermetic Refrigeration Compressors, on which as you know the casing is build with two dep-draw shells, for that we have a special software which produces the blank requred for the formed part (modeled in SW and exported as IGES), SW can not do that type of work.
A work around solution for your problem is possible with Solidworks.
The solution to your problem lies in modelling two separate sheetmetal bodies and then flattening them individually.
The combined flat pattern is the solution to your problem.
If you are using Solidworks 2010 you can do everything in a single part file. However if your are using any other
version you will have to model two separate parts to accomplish your requirement. The lock washer can be modelled
and flattened though.
Find the solution attached.
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