I am using the Swept Flange Feature to make a domed shape part but I am not able to get this to flatten. Does anyone know if this is possible?
That's a good question for Frank Ruepp
i was able to get the dome to flatten but i had to create a linear sketch line in the profile and use that line in the sweep flange feature as the Cylindrical/Conical edge selection.
Yes, this is exactly what I did. But obviously you have been faster than me . Another solution would be to use Surface Flatten which is available in SOLIDWORKS Premium:
When I measured the deviation of the swept flange and the surface flatten I figured that the result of the surface flatten is closer to the folded face. The reason behind the difference is that from a sheet metal perspective the flattened body becomes "longer" since the sketched arc in the profile gets developed (and the circular edge "moves" further away from the center point) and with it the outer diameter gets adjusted to the extended length.
In case of surface flatten we try to minimize the deviation based on a different algorithm and give back the actual folded edge length if possible.
I followed what Dan did and I was able to flatten it mainly because I don't have the Flatten Surface feature. However, I now want to add an edge flange to the Domed side and I am not able to do that. I know that the edge flange has to have a planar face and you can't do that on the domed side. How would one go about adding a bent tab on the dome side and then keep the part able to flatten? I was able to add another Swept Flange but now when I go to flatten the part, it only flattens the domed side. The tab disappears.
And lastly, thank you for the help with this. I know you don't have to spend time doing this but it is very much appreciated.
from your screenshots it looks like the second swept flange did create a second independent body and that is the reason why one body gets hidden when the other body is in "flat pattern state". You might want to check if you can merge the second swept flange feature with the first body (there should be an option in the swept flange feature). But to be honest, I would be surprised if it would work and you could flatten the whole body.
If merging the two swept flanges and flattening the single body fails I could imagine a tinker workflow that could work (but again, I am not very confident that it works out): We do have the unfold feature which allows you to flatten a body before the flat pattern (you would usually use this feature if you want to apply i.e. a cut that gets manufactured in the flat but requires i.e. folded geometry in order to place this cut). So if (and there is a big question mark behind that if because swept flange and lofted bend do not behave like ordinary sheet metal features and I think there might be limitations to the unfold feature for swept or lofted sheet metal bodies) you can unfold the swept flange bodies individually, you could move the unfolded bodies so that they line up like a flat pattern. But as I said there are a lot of question marks related to it.
But perhaps you want to give it a try...
SOLIDWORKS Product Definition Team
I tried your method on this and it worked - however I don't believe it is correct (at least for me, lol). I measured the arc length on the "path" and measure the arc length on the same edge in the flat and they came out to be way different. They should be somewhat the same depending on the thickness used.
Any thoughts on this?
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