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Part to unbend

Forum|Forum|12 years ago
June 2, 2014
8 replies
8056 views

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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1_Unbend-rar.zip

General

Best answer by TomD.inPDX

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.

T

TomD.inPDX

17-Peridot

I find it strangely difficult to make a shape like this in Creo Sheetmetal.

I

Inoram

14-Alexandrite

I can't test it (so I flattened the quilt), but here's my idea.

1_blendy-prt.zip

M

mhucik

Author

1-Visitor

Hi Matt, i´m sorry for to late answer. Thank you very much for your idea. This was applicable for me case and i can use it for worst unbend component. One more time thanks.

Michal

T

TomD.inPDX

17-Peridot

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.

1_prt0375-prt-3.zip

T

TomD.inPDX

17-Peridot

Okay, now I'm scaring myself

1_prt0376-prt-2.zip

T

TomD.inPDX

17-Peridot

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:

M

mbonka

2-Explorer

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).

T

TomD.inPDX

17-Peridot

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

D

dschenken

1-Visitor

I think the problem is that the original bends are elliptical relative to the faces - take a section normal to the top and side faces and it won't show the bends as true arcs.

I made a demo part with a blocky protrusion, parallel blend; then created the rounds using a variable radius fillet; and finally a sheetmetal conversions with shell to remove the interior. Worked well.

The downside is the slight taper means that while the part flattens OK, the end opening is slightly elliptical.

The perfectly shaped item is a cone (two radii) that is cut at an angle. In my case the cone is tangent to the top and sides. In the original case it is not a true cone, but one that is distorted to an elliptical section.