[NX8.5] Hollow a solid swept feature?

[Ionada]

Hi all!

Really at my wits end here, and don't have anyone to turn to in the office/locally.

I'm trying to create a custom sized wye pipe - similar to this image:

I found the "Tube" feature to be unable to join the three sides. Instead, I used the "Swept" feature to create the initial line, followed by "Pattern" and "Trimmed Sheet" to get nearly what I'm looking for:

For me to be satisfied with this, I need two things: a wall thickness and to removed the scratched out portions. I've tried making a solid swept feature with a nested sheet inside - no dice. None of the youtube videos I've watched have covered this, and I've poured over this forum - this is as close as I could find:

http://www.eng-tips.com/viewthread.cfm?qid=138575

I've learned a heck of a lot through Google searches leading me here, any help or advice is greatly appreciated!

 

[mmauldin]

Attached are two ways to create this part fairly easily. These were done in 7.5, but should be comparable to 8.5.

 

[Toost]

If I look carefully at the image above, the difference between that and the examples that Mmauldin uploaded,is that Mmauldins models have a couple of edges where the bends start/end.
This tells me that these faces are of simpler internal math than the ones without the edges.
The simpler the math, -the simpler the follow up features. ( Blends, Shell, offset etc)

If you open the attached part. ( I borrowed Mmauldins part and created a new sweep, thanks Mmauldin )
then : Information - object , select the Face ( Note : "Face", not the feature) OK
You will then get a report that :
Degree in u 3
Degree in v 3
....
Number patches in u 22
Number patches in v 21

Which means that this face has 461 sub-faces, all in degree 3x3.
The "degree" is the highest exponent that occurs in the specific equation. "Degree 3" is the "defacto standard" for regular CAD systems.
Why? Because i have asked NX to approximate ALL the input data info ONE face. And a single 3x3 degree face simply cannot stretch into this shape, NX then has to use multiple patches to keep the set distance tolerance.
If you edit the sweep ( double click the sweep) tick the Preserve Shape Option. ( this option is what that other thread mentioned as entering "0" in the tolerance field)
Then repeat the Information -Object,
The result will, depending of which face you select be 4x2 or 4x1 patches which is far simpler than before, and i would suspect that your Hollow feature on the combined body would succeed.


Regards,
Tomas

 

[Ionada]

Holy cow!
Mmauldin, thank you so much for the files. I've had time to look at them, the approach you took to creating the wye was not one I had thought of.
Thomas, thank you for for the detailed look at how NX interprets inputs and turns them into math - genuinely fascinating. I like knowing how my tools work, and NX is no exception. I'll be testing the hollow feature shortly.

Cheers to you both, and thanks again!