NX10 Sheet Metal problem

[Karlis]

Hi,
I am having problems flattening a split pipe.
Basically what I have is a tapered tube (0.4 degrees of taper), with each end cut off at angles.
The tube itself was created by extruding a circular section using draft and then trimming it to angled planes. The split was created by extruding a very narrow cut at the shortest side of the tube.
For some reason NX won't let me convert it to sheet metal (error - "please select planar base face" when I select one of the faces from my rip). I really need this simple shape flattened so that I can cut it with laser and weld the loose ends together forming this shape.
I have attached the model as parasolid file.
Any help will be appreciated. Thank you for your time.

 

[HercalloY]

Karlis,

I had a bit of a quick look. It doesnt seem that your part is of uniform thickness. This might be the main deal-breaker. So i'd check that. If that still doesnt work, i'd look at how you modeled the part as the OD and ID seem to be NURBS surfaces and not normal faces which might make the Sheet Metal "not like" it. (and why you're getting the 'no planar face' error)

 

[carlharr]

This would be best modelled using contour flange I think.

You can then select an edge at the split, unbend, add the shape, rebend.

http://www.jcb.com

NX 8.5 with TC 8.3

 

[Karlis]

Well, the actual geometry was made by extruding a sketch with a draft. As I said, the ends were cut off at an angle. So that makes it very unlikely for the thickness to vary. Or am I wrong?
It will be very hard to make each part as a separate flange since I have a lot of these parts, each slightly different. And each one of them must maintain associativity with the design.
Would it be better if I revolved the section and then cut off the ends at angle? I am currently at work so I have no chance to try it.
Thanks.

 

[HercalloY]

well if there is a draft... then it must vary. Don't you think?

There is none uniform thickness... i do not know why you would need draft on an extruded shape that is meant to be aheet metal part. that just wont work... Well, unless you wish to lathe the part instead of roll it out of sheet metal.

"Would it be better if I revolved the section and then cut off the ends at angle?" <- This would be ideal, and likely the simplest method.

It would be nice to have the native model to be able to see "where it went wrong" and give any advice. If you could post that, it may be of benefit.


EDIT: here is an image to highlight the none uniform thickness.

https://www.dropbox.com/s/d5vah8w8sr2f7fm/sm-error.png?dl=0

 

[Karlis]

Well, here is a revolved cone (.4 deg), from a rectangular section (wall thickness = 1 mm), and a it has an extruded - planar cut at the shortest side. It has also been cut at both ends under angle. All of these things are absolutely necessary to perform. No thickness variation whatsoever, everything is planar and uniform. And I still get the same error.
Can any sheet metal wizard please take a look? I have attached the file as parasolid. Because that is the file format that I will have to work with. I am beginning to think that this is going to be impossible.
Thanks.

 

[HercalloY]

I just imported that file, used Convert to Sheetmetal, then added a "Flat Pattern" feature. Changed to the flat pattern model view it created. All worked fine in NX10. Your first model wont do this though, as it has none uniform thickness. The second model you attached seems to have uniform thickness.

Link