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[NX8.5] Hollow a solid swept feature?

[NX8.5] Hollow a solid swept feature?

[NX8.5] Hollow a solid swept feature?

(OP)
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!

RE: [NX8.5] Hollow a solid swept feature?

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 smile )
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

RE: [NX8.5] Hollow a solid swept feature?

(OP)
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!

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