symbolic NPT threads won't show on iso view

[sam5a1]

Does anybody know how to get schematic NPT threads to show in an iso view? So far the only NPT threads I can get to show in an iso is simplified. we would like to have them detailed but we've found that if the pipe is in any position other than straight horizontal or vertical, in any view, the NPT detailed, or schematic, threads won't show. And in an iso view only the simplified view is available. Anybody got some ideas?



Scott
NX 7.5.4
Tc 8.3.2

 

[JohnRBaker]

I'm not aware of any Drafting standard which supports any sort of 'symbolic' representation of ANY sort of thread in anything BUT orthgraphic views.

That being said, I assume this is the case (in the view on the right) that you're referring to (both views are of the same model with the same 'Thread' style settings):

BTW, as you can clearly see (in the view on the left), your comment that "...we've found that if the pipe is in any position other than straight horizontal or vertical, in any view, the NPT detailed, or schematic, threads won't show." is not accurate (these Drawing views were created using NX 7.5.5.4).

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.

 

[sam5a1]

You are correct in my miss-statement. It should have been "in any plane other than flat, such as XY". If it is viewed in any angle as shown in the attached file, the threads don't show. As you can see, there is more wrong than just the detailed threads missing. If the render true hidden line is set, and sometimes we want it, the entire end of the pipe is missing. If it is turned off, the pipe is shown straight.

 

[sam5a1]

Sorry about that, I forgot to upload the file before posting.

 

[JohnRBaker]

As I said, none of the 'symbolic' thread styles are shown in anything other than an orthograhic view (that is normal to the viewer).

That being said, if you wish to see any sort of thread in an isometric view, you're going to need to physically model them, like I did hear:

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.

 

[sam5a1]

That's what we've been doing, I was hoping there was a different method that I didn't know of.

 

[JohnRBaker]

If it will help, attached is the part file from which the picture above were taken. It's a feature-based model so all you need to is edit the parameters to reflect the values for the pipe and thread-size desired.

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.

 

[Toost]

A qualified guess is that when one turns on the "Symbolic" display mode of, what NX does is a "2D manipulation" of the view/thread - the silhouettes of the threaded face. The thread display is flat. It will not cut an true 3D thread since that needs quite some processing. ( Which one notices if the thread is modeled as detailed.)
that would explain why the "symbolic" display only shows up in "2D views".

I have seen other attempts to simplify this issue, "some other cad system" quite often models "threads" as revolved non helical grooves. the operation is far simpler to compute and equally faster. The result looks weird in 2D/flat views but quite ok in 3D views.

Regards,
Tomas

 

[sam5a1]

Thanks John, that is appreciated. this is something that I can work with. Add the switch for changing between symbolic thread and detailed thread (like fasteners in the reuse library). Maybe one day I will get time to set it up like the fasteners in the reuse library or maybe as a NPT thread cutter for existing pipes.