Attached. Unsure as to why convert to sheet metal then 'create flat pattern' doesn't work?
The full part, from which the part is derived, is in the file too (suppressed).
(I believe all these panels should be identical so need a flat pattern profile for one of them only)
Solved! Go to Solution.
I can't open the part as I'm still on 2012 but did you make sure you set the proper material thickness in the sheet metal rules before attempting to flatten?
You should use Sheet Metal tools to create simple parts like this.
In particular you will be interested in Contoured Roll.
As Mcgyver noted make sure you set the sheet metal thickness and sometimes I have had to select a face before selecting flat pattern, especially if not in default orientation. Also, just because you can sometimes create a part, does not mean it can be bent out of a single sheet without stress cuts. I cant tell if your part has just one curve and is on an angle (preview is all I get- using 2011) or has curves in two directions. If all else fails try telling inventer the sheet is slightly thicker than the actual part is. Don't ask me why, but have had that make it work before on complex parts.
....make it work before on complex parts.
The part is a simple part modeled incorrectly.
Hi! For this particular case, Inventor should be able to unfold the sheet metal body. However, the body thickness is inconsistent with the one set in Sheet Metal Style. The problem here is with the Sweep path, which points slightly off the profile normal direction. As a result, the actual thickness (distance between front face and back face) is 1.191144677 mm, not 1.2mm.
There are a few ways to fix this issue without remodeling the geometry totally. Option A) Create Sweep surface instead of Solid Sweep. Then create Thicken on inner or outer face with the Thickness. Option B) Create Thicken (Join) from outer face with the Thickness and create Thicken (Intersect) from the same face with the same Thickenss. Either way should result in an unfoldable body.