How do i get surface is closed or opened ? 3

[sk258013]

Hi all

i imported iges and sewed A surface then by offset created B and c surface, later joined all sheets now how can i get the sheets are completely closed or not?
there is command called boundary in catia to check that, how in UG?
and after joining we can get solid by closing surface how can i do it in UG?
You can see the model in link its UG NX9 version


Thanks

 

[Xwheelguy]

Searching is your friend. Discussed this a week or two ago here: [URL unfurl="true"]http://www.eng-tips.com/viewthread.cfm?qid=400898[/url]

NX does it slightly different than CATIA. The Join and Close is done in one step called Sew. The surfaces MUST enclose a volume with NO GAPS greater than the modeling distance tolerance if you expect the Sew to result in a solid body.

Tips regarding Sewing:

1. Try to avoid adjusting individual feature distance tolerances on the fly (in this case the Sew tolerance). Adjust your main modeling distance tolerance before doing any modeling. 0.01mm is usually tight enough for MOST applications unless you're working with very small components - think time piece internals for example of small components. If you're modeling small components, then go smaller with the modeling distance tolerance, say 0.005mm or even 0.001mm. A former Siemens employee once told me a good gage for modeling distance tolerance was 10% of my smallest manufacturing tolerance.

2. When performing the Sew command, press the Apply button and check BOTH onscreen for any red curves which indicate gaps between sheet edges AND check the status line - if your sheets enclosed a volume without gaps (no red curves onscreen) the status line will respond with "Solid Body Created". If you're not fast enough for that, after the Sew is applied, cancel out of the Sew command, hover your cursor over the body until the 3 dots appear next to your cursor (don't move the cursor or you'll have to wait on the dots again) and make a pick of the body. The Quick Pick menu should come up and from there you'll either see Sheet Body (unsuccessful Sew into solid) or Solid Body (successful Sew into solid). If you don't like the hovering and waiting for the 3 dots, set a preselection filter for Solid Body and see if you can highlight your already Sewn body.

Finally, there really isn't an all in one tool to interrogate surfaces to see if they will Sew into a solid body. However once you Sew (and if you don't like the body type picking above in #2) then look into familiarizing yourself with Examine Geometry - will give you feedback on the quality of your model as well as identify gaps (distance tolerance) as well as tangency (angle tolerance) issues. It's important to remember (#1 above) that it's recommended to set these tolerances first (Preferences -> Modeling) rather than changing it on the fly (feature by feature) unless it's absolutely necessary. Probably wouldn't be the end of the world to increase the Sew distance tolerance just to get a solid body, but you might get an ugly result with Examine Geometry one day if you were to choose the on the fly method as a save all for distance issues.

Tim Flater
NX Designer
NX 9.0.3.4 Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[sk258013]

Thanks Xwheelguy
it really help me lot

I am in learning ZONE

 

[Toost]

I hope that the attached model is a test case where you try see the limits in NX compared to Catia ?
Else it would be a very-very awkward ( and slow) way of building a model.

1) correct and sew the imported sheets.
2) cap the voids.
3) sew the imports to the cap sheets.
4) perform solid commands such as shell. (and not 48 individual sheets.)

See attached version.
( also note that my file is smaller [kb] than the original. This indicates that my model contains simpler data)

Regards,
Tomas

 

[Rob_N]

Or simpler yet.

Import the sheets, your surface group A.
Sew them. and perform a Thicken.

 

[ewh]

I was having a similar issue with surfacing about 10 years ago and Tim's advice, then as now, was spot on.
While I can't blame him for any bad habits I've picked up using NX, I can credit him for enlightening me (numerous times) as to how to effectively work with surfaces.
Thanks again, (N)Xwheelguy!

"Know the rules well, so you can break them effectively."
-Dalai Lama XIV