HiI've created a sheet metal feature which has bends going in opposing directions from each other, see the attached image. The feature is essentially a rip across a bend with the corners of each bend folding at 90 degrees in opposite directions. When I try to flatten this part it gives an error.I have tried creating this in two ways:By adding a flange and then joining the open end using the join tool.Making a form tool and punching the one shape into the other.Both methods worked to create the feature but neither method works when I try to flatten the part.What would be the best way to create this feature in order to create a flattened state?RegardsDavid

1-Visitor

Question

Sheet metal opposing bends feature creation

Forum|Forum|9 years ago
December 6, 2016
3 replies
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Hi

I've created a sheet metal feature which has bends going in opposing directions from each other, see the attached image. The feature is essentially a rip across a bend with the corners of each bend folding at 90 degrees in opposite directions. When I try to flatten this part it gives an error.

I have tried creating this in two ways:

By adding a flange and then joining the open end using the join tool.
Making a form tool and punching the one shape into the other.

Both methods worked to create the feature but neither method works when I try to flatten the part.

What would be the best way to create this feature in order to create a flattened state?

Regards

David

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This topic has been closed for replies.

B

BenLoosli

23-Emerald III

Try adding bends on the inward facing portion where it is pulled from the larger outward bend. I only see 2 bends and you need 4.

D

dwiseman

Author

1-Visitor

There are actually 4 bends but I was using a zero internal bend radius. See the below image with internal bend radii added. Still the same problem. It seems as though Creo needs to have one end of the flange open in order to allow a flattened state.

Any ideas?

Sheetmetal part.png

P

psobejko

1-Visitor

You can't get a flat pattern from your part because Creo isn't able to model the deformation you are imagining. The developed length of the inward bent section does not match the developed length of the outside corner section. You can see that if you add a sketched rip, for example, on one of the inward-facing walls - then you'll get your flat pattern. There will be a gap in it that "butts-up" when the part is "folded". You can affect the size of this gap - even get the flat pattern to overlap itself there - by changing the various bend radii in the part. But all this is subject to the assumptions about deformations and bend allowances and might not be at all how the reality (un)folds...

L

lbrown-2

1-Visitor

I have made the part with following features:

- extrude (wall)

first wall.png

- extrude (cut)

- flange (wall) which is attached to both edges - this wall is sketched with radii, no bend reliefs. The image next to it is the flat instance - for whatever reason it is not attached on one side, but it is attached in unflatten state. Not sure if this will help you any.

D

dwiseman

Author

1-Visitor

Thanks for all the replies.

What I have ended up doing is similar to the above solution but I managed to get the flange to line-up in the flattened state by playing with the flange settings. I think this will work for now since it looks right in the folded state and flattened state when taken into a drawing, though it is a bit of a "cheat" method.