Result of sectioning two parts 1

[cubalibre000]

Hi,
it's normar this result ?
I've the pin sectioned and the nut not.
Why NX give this result ?

Thank you...

Using NX 8 and TC9.1

 

[JohnRBaker]

Without the parts there is little that anyone could advice you about.

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.

 

[cubalibre000]

Here the parts and drafting.

Thank you...

Using NX 8 and TC9.1

 

[JohnRBaker]

Have you 'refiled' your fastener libraries? If not, try doing that and see if that changes anything.

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.

 

[cubalibre000]

Yes...super refiled all fastener libraries.

Thank you...

Using NX 8 and TC9.1

 

[cowski]

Is there any interference between the pin and the nut? Drafting views can give some unexpected results when there is interference between the bodies.

www.nxjournaling.com

 

[jerry1423]

Check if there is a SECTION-COMPONENT sttribute on the fastener model set to NO
Typically there is no need to section a fastener.

 

[cubalibre000]

Hi guys,
for normative, fasteners must not to be sectioned.
Why other CAD doesn't have this problem ?

Thank you...

Using NX 8 and TC9.1

 

[cowski]

Are these the same parts that you have been deleting the hatch & reapplying in thread561-364041?

www.nxjournaling.com

 

[cubalibre000]

Yes, but I deleted the section view and recreated with this unexpected behavior.

Thank you...

Using NX 8 and TC9.1

 

[SDETERS]

I assume the Nut being crossed section is a solid? Could it be a sheet body?

 

[ewh]

I have to agree with cowski; if there is interference, odd things happen (and threaded components are usually modeled with interference). I have yet to find a solution to such situations other than view-dependent editing as needed.
Do you need to have the pin sectioned?

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

 

[cubalibre000]

We have created fasteners like the real world, like normative, school instruct.
Then when we put screw in nut, some CAD (Siemens NX) interprets like interference (no Solid Edge and no SolidWorks).
For normative, fasteners and pin must not sectioned, but in some case, pin can be sectioned for show internal shape.
This is the case, but if you are designer case like mine there are lots.
Then why you ask me to understand if I created parts in a strange method and not discover this situation like thousand of your and ask to Siemens to resolve drafting problems, still present in the 2014 ?
I'm very tired to open ER that aren't implemented where mid-range CAD have from always ?
The strange is that Solid Edge is part of Siemens PLM.
Why Siemens PLM doesn't make like Microsoft where improvement are shared form XBOX, Windows Phone and Windows ?
Synchronous Technology is a great tool. Solid Edge support this technology in Sheet Metal from many years, but NX no.
For company that use sheet metal component is very important.
This is another simple example.
Siemens PLM focus all for automotive company and for machine company we have to hope.
Another thread where a user ask for make a spline tangent from two line.
Studio spline in NX is a tool poor clear with strange behavior.
Have you tried create spline in other CAD ? Very simple.
Engineering in Siemens PLM have lost the important tool in the CAD market and focus for tool used only for marketing purpose.


Thank you...

Using NX 8 and TC9.1

 

[cowski]

As a long time UG/NX user, I'm simultaneously excited about new developments and annoyed at existing functions that don't seem to get the polish they need. UG/NX has a larger overall scope than many other CAD packages and it has been around longer; I get the feeling that it is 'creaking and groaning' under its own weight...

www.nxjournaling.com

 

[Toost]

This is how it looks in NX9.0.1 when i open it. I have not touched anything.
!?!


Regards,
Tomas

 

[Bwsh]

When the original nut is sectioned by itself, it doesn't show the cross-hatching lines.
However if the original nut is exported to parasolid file and re-imported into NX, and then do the sectioning again, it does show the cross-hatching lines. See attached snapshots. It seems like the original nut part file has to change some attribute setting in order to have it to display the cross-hatching lines.

 

[cubalibre000]

Toost,
the drafting I've attached it's the result after the manipulation because the section result was improbable.
Try to delete the section view and recreate it and tell me if the result it's correct.


Thank you...

Using NX 8 and TC9.1

 

[Toost]

Bwsh, I think you have misunderstood this thread. Re-read from start. The nut is correct, not sectioned.

Cuba,
I have played around in NX8.5. I don't have 8.0 installed.
I created a new Section and :

I have noticed the following in NX8.5, :
If i select the view - Style -
- Section tab : "Hidden Line Hatching" = on, the crosshatch gets correct.
( This is logical since the hatching is hidden by the non-sectioned nut. Maybe this option should be on by default.)
- Threads tab : Render True Hidden line = on, the thread inner contour gets correct.
( Why this option is needed is unknown to me. Not really logical.)


I know that there is a "general warning" about the "Render True hidden line" and that it might give long update times. I have no experience of this.

I also tested the case in NX9.0.1.
Exactly the same results as 8.5.
The main difference is that "Hidden line hatching" has been renamed to "Process hidden Crosshatch" , which is far better.
( actually the new name gave me the lead to try it.)


Regards,
Tomas

 

[Bwsh]

Tomas, Cubalibre00 first stated"

it's normar this result ?
I've the pin sectioned and the nut not.

Why NX give this result ?"

I thought he meant when sectioned the parts, NX has the pin sectioned but the nut is not sectioned.

So I thought he meant the nut has some issues. Even SDETERS thought the nut was the question here.

Anyway, the English wording was not very clear. Just try to help.

 

[cubalibre000]

Tomas,
your support was very functional.
Options unknow for me.
thanks again.

Thank you...

Using NX 8 and TC9.1