Surface to Solid
Surface to Solid
(OP)
After reading a lot of posts regarding this issue, I still don't get it how to generate a solid from a surface. I will explain my steps(It's about NX 10):
1 Import the Step data
2 Heal geometry
3 Reopen the healed geoemtry and extract surfaces
4 Sew with tight tolerance (0.001) - no problem in sewing Operation
5 After Sewing Operation is complete - I observed that there are two gaps in the geometry - fixed the gaps
6 I tried to heal again the geometry, but there were nothing to heal
Now I'm in the position that I don't know what would be the next step - how to generate a solid body form this surface. Since in Catia there is a simply way to do it (Join face and afterwards Close surface). I don't think that NX Siemens do not have such kind of option.
Could you please help me with this issue.
Kind regards,
Abbarth
1 Import the Step data
2 Heal geometry
3 Reopen the healed geoemtry and extract surfaces
4 Sew with tight tolerance (0.001) - no problem in sewing Operation
5 After Sewing Operation is complete - I observed that there are two gaps in the geometry - fixed the gaps
6 I tried to heal again the geometry, but there were nothing to heal
Now I'm in the position that I don't know what would be the next step - how to generate a solid body form this surface. Since in Catia there is a simply way to do it (Join face and afterwards Close surface). I don't think that NX Siemens do not have such kind of option.
Could you please help me with this issue.
Kind regards,
Abbarth





RE: Surface to Solid
Someplace there is a gap that needs to be fixed
Here is a thread that you may have missed http://www.eng-tips.com/viewthread.cfm?qid=335092
RE: Surface to Solid
Since you're working with imported data, and we don't know from where the 3D originated nor do we know how well the original model was created, you may have to Untrim some surfaces and re-trim them to fill in gaps. There isn't a set process for what you're trying to do - you'll have to experiment a bit and find out what works best for each model.
A tip: use the Apply button with the Sew command and the NX cue/status line will display "Solid Body created" upon a successful Sew to solid operation. Otherwise, you probably won't know for sure if the body was sewn into a solid or just a bunch of sewn sheets without interrogating the object to see what it is.
Tim Flater
NX Designer
NX 9.0.3.4 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB
RE: Surface to Solid
I still got a question regarding sewing operation while creating a solid body. If with the sew command having tolerance of 0.001 mm there are small gaps in my surface and with a tolerance of 0.010 mm the operation see no gaps, shall the sew operation convert the enclosed surface to solid body or not?
RE: Surface to Solid
I wouldn't recommend mixing tolerances (changing them on the the fly / as needed). If you can't Sew at 0.001 then set your Modeling Tolerance to a larger/higher value and perform all tasks at the larger/higher tolerance (0.01 rather than 0.001, for example). I've ran into cases where changing tolerances on the fly leads to further geometry/topological issues later on. Pick a tolerance and stick with it. I believe John Baker used to recommend a Modeling Tolerance that was no smaller than your smallest manufacturing tolerance. Some of the OEM automakers use 0.01 or 0.02mm as default.
Tim Flater
NX Designer
NX 9.0.3.4 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB
RE: Surface to Solid
IF the gaps are SMALLER than the tolerance the result shall be a solid body. ( I think you wrote the opposite above)
Now, note that the "ONLY" difference between a Sheet Body and a Solid Body is that the Solid Body is "watertight" within the tolerance used when sewn.
- Since this "body" has faces covering all openings , and that all faces have a normal which point outwards, we can consider these faces a "Solid body", BUT, it will still be empty!, -There is no material inside.
If there are gaps along the edges, and if the gap is smaller than the tolerance, NX considers (!) this watertight, but, the gap will still be there!
( You can test this by sewing two sheets together on which you design the gap to be a specific size, then sew with a tolerance slightly larger. Then test using the Examine Geometry...)
How do you know that the result is a sheet body and not a Solid body ?
I assume that you know that if you run the Examine Geometry... there is a check for Sheet Boundaries where you can highlight the open edges.
Regards,
Tomas
RE: Surface to Solid
Me or the OP wrote the opposite? I read that he tried to Sew with a tolerance of 0.001 and there were gaps still showing so he loosened the tolerance to 0.01 and that removed the gaps, which makes sense to me - he had gaps larger than 0.001. I was assuming he was editing the Sew feature and simply adjusting the tolerance value without creating an entirely new Sew feature with the 0.01 tolerance.
Tim Flater
NX Designer
NX 9.0.3.4 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB
RE: Surface to Solid
I replied to Abbarths last post.
and, I think now that i misunderstood Abbarth's last post and what the mentioned values did.
Regards,
Tomas
RE: Surface to Solid
Not a problem, buddy - was just wanting to make sure I wasn't feeding inaccurate information. Easy to misread questions - I've done it hundreds of times before.
You are spot on about the gaps technically existing even though a solid body is created. Can drive an OCD designer nuts when that occurs.
Tim Flater
NX Designer
NX 9.0.3.4 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB
RE: Surface to Solid
From older post I have understood that after sew command the enclosed surface shall be converted into a solid if there are no gaps greater than the given tolerances. The Examine Geoemtry Feature gives me No result for sheet bondaries - the part is green :) - there shall be any other Information instead: No result
RE: Surface to Solid
The attached movie shows a cube Sewn into a solid from 6 sheet bodies and the use of Quick Pick for body type interrogation.
QuickPickNX9.avi
Tim Flater
NX Designer
NX 9.0.3.4 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB
RE: Surface to Solid
Thank you for your support