Hi Everybody,
Please can somebody help me and give me an advise with sheetmetal unbending?
I try to do this in both solid and then convert and sheetmetal, but Creo cant unbend it.
I uses Blend feature to create this shape.
I use Creo Parametric 2.0
Or some advise how i should create it?
Please see attach file.
Thanks for your ineterest.
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ACCEPTED SOLUTION
Accepted Solutions
Interesting: It is a subtle but crucial detail I overlooked in sketch1.
Have a careful look at the construction arc guiding the small radius on the rectangle's corners.
Then look at the construction arc in sketch2. Notice their is no tangent on either construction arcs.
So the problem is that I was trying to twist the surface which could not be unfolded. I suspect there is some tolerance for this, but I exceeded it as soon as the round end was properly defined as representing a true round.
Again, Creo 2 attached.
I had to give this another try (probably attempt No. 37)... and I was finally successful using a different technique. Probably worth a document!
In this case it was a quilt (1/4) and offset with bend-radii after converting to sheetmetal.
Mirror x3 and merging the seams.
Flat pattern recognized the features.
It is a bit touchy about material thickness but if there is enough margin, no problem.
Creo 2.0 full version attached.
Why is it every time I figure something out, I find a new bug to report 
When I tried correcting "sketch2" to be truly round, the unfold/flat-pattern fails.
I reported this to CS:
Interesting: It is a subtle but crucial detail I overlooked in sketch1.
Have a careful look at the construction arc guiding the small radius on the rectangle's corners.
Then look at the construction arc in sketch2. Notice their is no tangent on either construction arcs.
So the problem is that I was trying to twist the surface which could not be unfolded. I suspect there is some tolerance for this, but I exceeded it as soon as the round end was properly defined as representing a true round.
Again, Creo 2 attached.
Hello Antonius, thank you very much for answer and iam sorry for to late my answer. I had to stady it at first 
But it was cool and i did it.
Michal
In my opinion it´s waste of time to sketch each bend radius separetly. Maybe you need some marks for bending machine manufacturing ---> create them in unbend state like a sketch and bend it back.
General:
Check curvature of your sheet. Curvature of circle part must looks like a smooth circle, not like a hedgehog 
.
l was also in fight with thise sheetmetal "duct" transitions. Discovered, that it´s better to use TANGENT condition everyvere in sketch. It´s better than use point align to point and two same radius. Logicaly it´s the same, but Creo works better with tangets conditions in sketch (maybe just my personal feelings).
Funny enough during some recent travels I saw exactly the "hedgehog" pattern on some huge construction beam being transported down the highway.
Remember, we use CAD to do what we want it to do, not what it wants to provide for us 
Hi Steven,
Thank you for answer and your advice. No edges did´t have to be in transition so i did it.
