I am trying to bend a sheet with some forms embossed in them. Using the 'sketched bend' sheet metal tool does not work. I can do this easily in another CAD program, but it does not seem possible with SolidWorks. Any suggestions?
Try Flex as sheet metal won't work with varying thicknesses .
But again if you use flex I'm not sure if the results will be as desired. Also you'll have to make configs for flattened and bend part manually.
Flex would not give me what I wanted so I added and subtracted bodies after the bend to create the 'dimples' I needed.
This was just way too much work for something that should have been so simple. As much as I like SolidWorks, I am amazed what is missing sometimes when compared to my other much cheaper CAD software. So why don't I use the other CAD software? Simple, it is not parametric and that is something that makes SolidWorks so much superior in most other ways.
The only way I would know how to show this in SW is to add additional configurations in the flat state and the bent state. In those configurations you would need to add the additional feature that you show. SW will not flatten that part as shown, so after you make a configuration called Flat, then suppress the bends or un-suppress the Flat Pattern bends then add the extrude boss as shown. You would need to do it the same way in the bent shape.
Thanks John. That is a good idea about showing two configurations, one for flat and one for bent. I may just create the part without the bend in SW and do the bend in my other software and bring it back into SW as a dumb part.
Don,, I know you are hesitant to name the other software (non-parametric) but I'm curious. Are you referring to Allibre? (not sure how that is spelled).
The other software where I can do this bend easily is TurboCAD (Platinum version).
I did experiment with Alibre back in its 2012 days, but I did not have the sheet metal functions, so I do not know if this type of bend is/was possible with it.
Interesting. Thank you.
try put your flange in first then use the unfold, put in your cut in then use fold
That works well Joe but the problem is what happens when you add the opposite side of the impression. I played with this and the part folds and unfolds with the cuts but not when you add the opposite side of the impression. It appears you can remove material but not add and have this behave.
That is what I found as well, Dennis
Could you then double the part thickness (or add double the emboss thickness), remove material off both sides and then have the part still fold instead of adding material?
Trying to convert something similar from solid to sheet metal doesn't work, I've tried that. So that's out.
If the corners aren't that important visually, you could also emboss the part in sections corresponding with the bend tangents.
Andrew,,, I think you are on to something with this idea. I can't believe I didn't think of that. It does seem to work. Thanks for slapping me around.
This part is a simplified version of Don's with no thought to correct locating of cuts.
Edit:.. Just wanted to add a little more info. The part flattens with ease.
Thanks Andrew. An interesting approach.
And thanks to everyone else too for all the info and insight into this topic.
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