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Sheet metal bends in drawing

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DanDR

Mining
Jan 14, 2004
1
I got a question: I have a part with two bends (flanges). In the drawing, I want to show the intermediate stage (the part dimensions after the first bend) in a separate view so the part can be checked after the first step. Of course I need the formed view(s) plus the flat pattern to be shown, too. Is there a simple way to do that in UG?
 
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I am not familiar with the sheet metal package, but one way that may work is to create the flat part first, add that as a component in the drawing file. Use the wave geometry linker and extract that body, perform your first bend, use insert -> form feature -> extract -> body, and add your second bend to this body. Using this method would ensure that the bodies are linked, any change to the flat body will be reflected in the bent bodies.
 
I answered without fully thinking out the problem, and assumed that you are using the master model approach. Regardless, it would probably be better to extract the bodies while in the original file than to use the wave geometry linker in this case.
 
DanDR,

Using Extract you can check the option to At Timestamp and not have the extraction change with features added after the extraction. In this way you can Extract at timestamp and show that Body on a separate layer. Then you can add the bend to the original part solid and do another extraction at timestamp onto a different Layer. Then in your drawing hide the extract layers on the finished part view and show only the Extracted body layers in your views for showing the Fabrication stages.

With this method all your changes can be done in one part file and not have to have several parts to manage with wave links.

Michael
[2thumbsup]
 
You may also want to read up on Part in Process functionality in the help docs. Use the PIP function, which, if I remember correctly, uses part families to create a part at any given fold/unfold state of a part. Then the parts are all added to a "parent" assembly, and using "hide component", any given state can be shown in a view.... Sorry for the vague description, but it has been a while since I've had to do this...

-Derek
DL Engineering Services

specializing in CAD Design Consultation Services
 
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