Flat pattern tube

[domac]

Hy to all,
I have problem with one part, NX doesn't allow command "FLAT PATTERN".
Pipe starts with one diameter and ends with bigger and I make it with extrude + draft feature. Then I add a thickness of 1.5mm, and I use command CONVERT TO SHEET METAL.
But when I try to flatten the part, NX popup with "UNABLE TO CREATE BODY"

Can someone help me with this issue/part?

Thanks

 

[Lockdain]

Hi,

It seems to me, that it happens because you're trying to unfold a cone. I can offer you to unfold inner or outer surface using Fabric flat pattern, create an bounding surface and thicken it by 1.5 millimeters then. Looks a bit weird, but supposed to deliver a result.
Unwrap a section curves would also give good results.

 

[domac]

Ciao,
thanks on answer. I try it with FABRIC FT, but doesn't give me correct dimension. Exactly, I need to draw this model, and flat pattern dimension should be same as on attachment PDF (see it).
Second, I have to made this cutout and holes, which is possible only if I draw 3D, make FT and draw a cutouts on FLAT SOLID.

 

[Lockdain]

Tried to unwrap your tube using Isoparametric curves (on the outer surface) and Unwrap curve feature, see the result:

Are the flat dimensions correct?

 

[Lockdain]

In that case, why don't you start from flat drawing of your pattern and then thick and fold it according to the blueprint?

 

[domac]

Your dimension is a little different.
I made it finally, difference in flat patter shape is only 0.6 mm according to original drawing, which is good for me.
Thanks for your help

 

[deedub777]

This is possible however you need to be on NX10 or later. Convert to sheet metal was enhanced in NX10 to identify more complex shapes.

See attached file for solution.

The method:
- Create sketches at each end of tube
- Create ruled surface between them
- Thicken to desired material thickness
- Change to Sheet Metal application
- Convert to Sheet Metal
- Create flat pattern.