Surface to Solid

Try sewing with a loser tolerance if possible
Someplace there is a gap that needs to be fixed
Here is a thread that you may have missed

If you Sew and there are gaps, NX cannot enclose a volume to create a solid body. If you repair the gaps AFTER the Sew command as you outlined in the steps above, NX still will not create a solid because you're not performing the operations in the correct order. The Sewing is the last step before you want the solid body to exist. Fix ALL gaps FIRST then Sew. It's OK to try some testing by creating a Sew then deleting it (to see if the surfaces will Sew into a solid) or using Make Current Feature to roll the history back prior to the Sew taking place and "inserting" additional features or operations to help repair the surfaces and enclose the volume.

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

Thank you for the answers.

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?

If you simply change the tolerance by way of Edit Feature, NX probably will NOT convert the body into a solid (at least it didn't for me in NX9 - can't speak for NX10). You may have to delete the Sew feature with the 0.001 tolerance and recreate the Sew with a looser (0.01) tolerance. Some features in NX allow you to switch between body types (Solid or Sheet) but I do not believe Sew is one of them - why, I cannot say. Might be a good suggestion for an Enhancement Request.

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

Last question: Yes/No ???
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

Toost,

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

Sorry Tim, your last post were not there yet when i replied.
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

Toost,

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

I do the check this way, I just make a section through my sewed suraface. if I see the empty space between the two walls, then It's not a solid. if yes, then its a solid. The funny way is that I convert my enclosed surface to step file and open it again, I extracted all faces again and sew it them back with the same tolerance as I did in original part(*.prt). After making a section through the surface the result was a solid body, for which I was able to add material.

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

For a non-technical check like you're doing, you don't even have to go that far. Hover your cursor over the Sewn body until the 3 dots appear next to the cursor. Now, select the body. The Quick Pick dialog should appear - if the Sew was successful in converting sheets to a solid, you will see a Solid Body in the list. If the Sew wasn't successful, you will see Sheet Body.

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

Finally it worked but with a tolerance of 0.05 mm.

Thank you for your support