I have tried everything I can think of to build a part like this that I can unfold in sheet metal to get the flat layout. If I do it with a seam parallel to the axis it is easy. But that's not what we need in real life.
Any suggestions? This seems like a pretty common real life sheet metal situation, the program should be able to handle it.
Thanks
Rick
Since no other answers yet, I assum that its a challenge for SWx Sheetmetal.
As usual attached is my approch using my sheet metal basics.
Going old school Michael. I like it...
Cheers,
Anna
Yes Anna, it's quite a bit of work and but was reminiscing the golden oldies.
Fortunately now we have flattening software to get quick results.
I'm surprised to see that it's impossible for standard SWx sheetmetal to handle such a part.
This is how I would normally do this.
Good afternoon Rick,
One way is, you could lay it out as a flat and add a bend sketch and make the radius what you need, you would have a lot more trial and error with this method and changes would be difficult or time consuming.
Unfortunately you need to add a small work around and that is a vertical cut at either the top or bottom of the slanted cut. Select the top face to add the sketch then draw a very small rectangle and cut. The depth of the cut only needs to be .015 more or less, then select the outer vertical edge of that cut and insert the sheet metal bends.
I did try the lofted bend feature, which didn't work, unless there is a setting that I missed,
Later,
John
If you start in sheet metal, make a base flange that is really short (.0001) and then Hem it, then use a second Hem to complete the circle, Do a cut extrude to put in your surface cut in the side and flatten. Might not be perfect, but gets you the result.
Hopefully you can see the image well enough.
Thanks to everyone for the suggestions. I feel like the double hem method that Glenn suggested gives the cleanest, most versatile model.
I've been using SW sheetmetal for years, and know most of the tricks, but I've never had a real life use for the hem feature, so I wasn't aware of its capabilities.
Thanks again
Rick
Hello Rick ,
Simply model you split sheetmetal pipe with a straight gap first. Now unfold the pipe selecting the straight edge of the seam. Add a cut feature that represents your contour but leave a tiny bit of the straight edge at the bottom. You will need this to fold the model back up. Make a derived sketch of the contour.
Now add a extrude feature with the proper gap distance to model the actual seam. Since you remained the straight edge you should now have the pipe with a curved seam.
Elmar
If you start in sheet metal, make a base flange that is really short (.0001) and then Hem it, then use a second Hem to complete the circle, Do a cut extrude to put in your surface cut in the side and flatten. Might not be perfect, but gets you the result.
Hopefully you can see the image well enough.