show non-sectioned detail on section view

[bataattila]

Hi,

I'd like to find the best solution for dimensioning an adapter plate as shown in the attachement -the original drawing is made in ProE.
In your opinion what would be the best realization in NX (8.5), which is elegant and preferably involves only standard NX-tools (no tinkering).
(break-out section doesn't have a section line, half-section doesn't allow segments in the sect-line)


Thank you in advance,
Attila

NX6

 

[JohnRBaker]

First, I suspect that this don't comply with any specific Drafting Standard.

That being said, see the attached example where I created a normal Stepped Section view. Then I broke that view to remove a portion of it. I then broke a normal side view at the same location only removing the other 'side'. This second broken view I then moved so as to superimpose it over the top of the first broken view.

Anyway, take a look and see if this meets your criteria.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
Siemens PLM:
UG/NX Museum:

To an Engineer, the glass is twice as big as it needs to be.

 

[KhimaniMohiki]

Alternativly move your stepped section to exclude the area in the red circle then apply a break out section to show the chamfer detail

Khimani Mohiki
Design Engineer - Aston Martin
NX8.5

 

[bataattila]

Hi again,

thanks for the answers, always feels good not to be alone.

@KhimaniMohiki: I already tried the method which I attached this time. It's the closest and easiest I did so far, but doesn't seem like elegant (it's an ugly solution to be honest).

I'm experimenting with John's version now -which looks fine; only problem is the two views are aligned together nicely, but they're not moving together (this can be a mistake-opportunity on user's side).


Thanks again,
Attila

NX6

 

[ewh]

I would create two "breakouts" in the projected side view and eliminate the need for a named section view.

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

 

[Toost]

The last example from Attila is technically correct, which his first example isn't.
In NX 7.5 ( i think it was 7.5) there is an option to display "Bend Lines" under Style- Section for the particular view.
Another trick i have used before this option was added was to add a 2-D centerline in the section view which shows where the step is.
Some people want this line whilst some other people don't.
See attached image.

Regards,
Tomas