I am unable to flatten the part after performing an extrude cut as shown in the attached image. Any suggestions would be deeply appreciated.
If I am looking at this correctly you are cutting into the material thickness. For SWX bending to work (fold/unfold) the thickness MUST be uniform.
I read the same. Looks like this would be better off as two sheetmetal parts overlapping and bonded.If it must be one, use configurations. One for bending, and the second for the machining. Even though the machining may happen first in real life, the SolidWorks folding/unfolding won't like the machining operation so you'd want to do that after its folded. You want to keep that suppressed in config 1 so you can maintain the sheetmetal functionality.
Thank you. I am quite new to SW, so could you please explain what do you mean by 'doing the m/c operation after its folded'? The part is already in the 'folded' state when created. My vendor needs a flat, actual thickness (non uniform) to perform the bending operation. From the responses, I am assuming that it is not possible to flatten a part with non uniform thickness. Or am I missing something here?
Again, thank you for all the responses.
What I mean with doing the M/C operations after it is folded is, make thecomplete formed sheetmetal part, you'll be able to flat-pattern this. Once you add the cuts, which effectively change the thickness in those areas, the flat-pattern will no longer work as you have found. As a workaround, if you add these cuts in a new configuration, in such a way that the feature is suppressed in the first configuration. then the first config will still flatten.
What is your intended fabrication process for this part?
Robins Kalathil wrote:Any suggestions would be deeply appreciated.
Robins Kalathil wrote:
Any suggestions would be deeply appreciated.
Attach your *.sldprt file here if you can't figure it out and end all doubt.
Thank you, please find the attached part.
Here is a possible solution.
Create different configurations.
Use those on your drawing to communicate design intend.
You add dimensions - part is example - please check dimensions I have used prior to using this as I designed it.
I agree with the comments by the others, it will not flatten. But will it not be constructed from two pieces? Then it is an assembly possibly spotwelded together.
I guess my first thought would be to make it a multi-body sheet metal part, with a very small gap between the two bodies.
Like Bernie said, it looks to be two pieces spot welded together - just draw it like they will actually build it.
(I would probably make two separate sheet metal parts, and have this be the assembly to show how everything goes together.)
Are you familiar with the Sheet Metal Process in a Fabrication Shop, how it is made out of a uniform flat sheet stock? Is that truly the design requirements or just a design element?
The only way that this part is made as a sheet metal part would to do all the bending first and then machine the offset (thinner section). If the part is only a small strip, this wouldn't be that big of a deal, however if the pc has considerable length then there would be a re-design needed. etc...
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