bending a sheet over rounded surface

[bataattila]

Hi all,

The rubber part seen on the attached picture has two states: delivery and mounted.
In mounted state the part attached to a rounded surface, which geometry is given (radius and center of radius).

How can I reach the desired form starting from the planar state (using sheet metal or modeling)? It seems like an obvious task, yet I can't find the solution.


Thank you in advance,
Attila

NX6

 

[SvenBom]

The part, that is shown in the Picture, looks like a 'sheet metal part. There you have bended and flattened state of the part. So maybe, you could 'simulate' your rubber part with sheet metal application.
Then there is also Global Shaping (Edit/Surface). Since you are using NX6, I don't know how good it was in that version. In NX8.5 works Quite good. One thing, that I remember from older version is, that it worked fine with bending the surface, but not the solid body.

 

[bataattila]

I would be happy to use Sheet Metal to achive this effect, but I haven't figured out how yet.
As for Global Shaping, I have to look into it in the Help, there are a lot of options Meanwhile I'm waiting for further suggestions.

Thank you,

Attila​

p.s.: I'm also on 8.5, my signature is outdated (probably not anymore).

NX6

 

[SvenBom]

To learn global shaping, maybe the attached movie can help you. In the movie, i have been using only curves. But it works great also if you select surfaces (By Surface method).

 

[JohnRBaker]

OK, you can use NX Sheet Metal but just approach the problem from its 'as-formed' state, that is the shape that it will be when it's assembled, but simply create a 'Flat Solid' feature as well which you would use for the detailed drawing of the unformed piece. When creating this model in NX Sheet Metal the system will automatically create TWO Reference Sets, one for the formed state, the 'Model' Reference Set, and one for the flat state, the 'FLAT_SOLID' Reference Set. Attached are three files, one the design model, a Drawing in the Flat state and an Assembly in the Formed state. Look at this workflow and see if it might work for you. The only part that you have to watch for is that since you're creating the model in its 'as formed' state, you'll need to play with the 'Length' parameter a bit to get the correct 'as-flattened' length for your drawing.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[SvenBom]

And about sheet metal. If you have metaform command, you can do this:
1. model your flat rubber part
2. place it in the assembly.
3. now, make your rubber part work part.
4. copy the revolved surface from the assembly. Make any adjustements to the revolved surface, if need it.
5. use metaform to deform your flat part according to copied surface.

 

[bataattila]

I learned a lot today, much appreciated.

@John: am I right that you used Perimeter Dimension for your first sketch? NX doesn't seem to show it. And you are very right, I need a drawing about the flat object and also the input dimensions come from the flat model. So your guide works great for me -just what I needed.

@SvenBom: the video about shaping seems super useful (saved it for later), but I think I'm gonna stick with John's solution.


Thank you again guys, I could hug you right now.

Have a nice day,

Attila​

NX8.5

 

[JohnRBaker]

Yes, I used a 'Perimeter Dimension' to control the 'length' of the sheet and yes, in NX while it is a Sketch Dimension, it's treated more like a Constraint.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.