Can you make a solid body from surfaces

[aluminum2]

I tried to make a solid body from a set of surfaces today and had no luck. The surfaces are all connected and look like a solid body. I tried "sheets to solid assistant", but had no luck. It seems that it sews the surfaces and only thickens them. Is there a way to do this? thanks.

 

[JohnRBaker]

Have you tried to simply 'sew' the sheet bodies (i.e. surfaces) together using the...

Insert -> Combine -> Sew...

...function?

Now in order for this to work you will need to have enough surfaces, without any openings, so as to form a 'water-tight' set of faces. All edges need to match other edges within the range of the Modeling Distance Tolerance.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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

 

[jerry1423]

There is probably a small gap between the surfaces someplace.
Try opening up your modeling tolerance Pererences -> modeling Prefernces -> distance tolerance
and try it again.
Can you show a pic of the surfaces?

 

[JohnRBaker]

But be careful, if the gaps are too large, even if you can still get it to sew by opening up the Modeling Distance Tolerance, there does come a point where the model is worthless. The surfaces have to be good quality and sufficiently complete to get a usable model. After all, no matter how good the software is, "you can't make a silk purse out of a sow's ear".

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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

 

[aluminum2]

I did try sew, but when I use section toggle, the part is hollow. I set the tolerance to .02 and the surfaces look good to me. Is Sew suppose to automatically create a solid or do I have to click on an option?

 

[jerry1423]

It will automatically create the solid.
You probably will need to have several sews in the model to properly sew it together - generally it won't work in "one fell swoop"

 

[JohnRBaker]

No, it'll work in "one fell swoop" IF all the surface edges are within the 'Modeling Distance Tolerance' and there are NO 'holes' or openings in your model (where edges are significantly further apart than the Distance Tolerance value).

Now if there are actual 'holes' or openings, you may have to sew together what you can and then create 'patches' to cover the 'holes' and openings and then sew these 'patch' surfaces to the current sewn body. Eventually, once all the gaps are closed, the holes filled and the openings patched, you WILL end up with a valid solid model.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

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

 

[Arkance/PhoeNX]

@aluminum2, when you say "I did try sew, but when I use section toggle, the part is hollow" it may be a solid, but the cap is turned off so it looks hollow.
In the View Section dialog (under the Cap Settings bar) you can turn on the cap display.
To check if it is a solid, change the selection filter to solid and see if the body highlights when you run the cursor over it.
Otherwise to check the body and highlight any openings use Analysis -> Examine Geometry and tick the box for Sheet Boundaries then select the whole sewn body. If it is a sheet body, it will show the openings that are stopping it from being a solid.



Anthony Galante
Technical Resource Coordinator

NX4.0.4MP10, NX5.0.6, NX6.0.5, NX7.0.1, NX7.5.0-> NX7.5.5 & NX8.0.0 -> NX8.0.1

 

[emenes]

Have you tried the 'trim and extend' function ?
If you set the 'make corner' option you able to create a solid out of surfaces.

Regards