Thickening sheets to form a solid.

[skanskan]

Hi.

How can I get a solid body from sheets?
For example I have I create a curved duct-like sheet sweeping a circle along a curved line.
(I know I could directly create a solid with the seep dialog).
But if I want to create a solid from the sheet I find it impossible.
I have the same problem with more difficult geometries.

If I use the "thicken" option with a offset large enough to cover all the void I get the error "cannot offset face. The offset value may be greater than the radius of curvature..."

I've also tried covering the extremes and sewing without luck.

The only way I know, though more complex, is to create a larger solid body and trimming it with the sheets.

 

[JohnRBaker]

Sorry, but you can't 'fill a void' in a hollow, tube-like surface using the Thicken command. That being said, why are you suggesting that creating a Swept solid is not acceptable? If your end state needs to be a solid and creating a Swept body will give you that result, what's the problem? For complex shapes created using surfaces, which cannot not be done by 'swepting' a shape through one or more planar profilez, the general workflow involves closing a volume on all sides and then sewing the surfaces together to form a solid body.

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.

 

[skanskan]

Hello JohnRBraker.

I didn't mean that creating a solid while sweeping is not acceptable. I just did it that way in order to show that I can't thicken that sheet, but it was a quick example. In general, I'm speaking about sheets or any solid with voids.

 

[JohnRBaker]

Thicken Sheet is intended to be used to convert slab-surfaces into something that looks like it was formed from sheet metal or was molded with a constant wall thickness. It was not intended to take a complex model and sort of 'grow' the faces until they come together to form a solid body. Perhaps if you could show us a more typical type of shape that you're wanting to create then perhaps more appropriate advice could be given as to how one would go about getting that desired result.

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.

 

[mmauldin]

If I were creating a complex duct, I would probably create it as a solid and then use Insert> Offset/Scale> Shell to create a tube with a constant wall thickness.

Example attached.

 

[Toost]

When you sweep and in other freeform methods, if the "end sections" are both planar and closed, you can create a solid body. I.e NX "understands" how to close the volume.
If the ends are non planar, one must create the closing shape, sheet body. The contact edges of this sheet must be within the modeling distance from the target sheet when sewing.
The sewing operation will not trim or extend the edges in any way. - One can sew "anything" together by increasing the tolerance, but the deviation will still be there after the sew. It might not be visible in shaded mode though. Static Wireframe will show the deviation.
If you use the "trim and extend- make corner" and the final trim makes a watertight body, it will then become a solid body.


Regards,
Tomas