I am trying to convert the attached file from a lofted solid to a sheet metal part. Seems like this should be pretty simple, however, I've failed at all attempts. What am I doing wrong? I tried to convert, but the model is missing a transition radius from the top to the sides, I tried to create curved surfaces which worked well, but I could not join the 5 sheet metal parts into one part that can be flattened.
Any help would be greatly appreciated,
thank you
Steve
Steve,, I did this with surfaces then converted to sheet metal. In order to make the surfaces I created some planes to bisect your model. Moved some faces on your solid in order to have the sheet metal part match yours when done. Then on those planes sketched a couple of 3 point arcs Pierce on the ends and coincident at the mid point of the arc. You can see that these arcs very closely matches the curve of your solid.
Did some surface offsets, trims delete faces etc. the converted to sheet metal. I may have been a bit off on some of my offsets and I don't know your material thickness so guessed at .025" since your part is small.
I'm quite sure you can get exactly what you want by following my model and making the necessary adjustments.
Oh I also guessed at to which end you want open..
I created a solid with fillets.
Then shelled.
Use Convert to Sheet Metal.
Pick the fixed face and it is important to pick the fillet for the bends and not the corners then add curved sides.
Hi John,
Outstanding, that worked great and was very simple to perform. I was almost to the point of creating a flat pattern and inserting bends which is a real pain in the tush.
Again, thank you all who replied I appreciate the help.
Steve
Hi Steve,
Your best bet would be to use "Lofted Bends" found under 'Insert', 'Sheet Metal' but if you look inside that command you will see that it does not have some of the more interesting options that a solid Loft feature has. It will only allow you to select two profiles and not the three you have modeled here. You would not be able to create that complex curve without being able to select more than two profiles. From the looks of it I don't see how you would make the program produce this as a sheet metal object.
If you have SOLIDWORKS Premium though you could use the 'Surface Flatten' feature to create a flat pattern(-ish) of the Loft like the attached example.