assembly-tree drops items that are still on the drawing?

[cyril009]

NX 7.5

Greetings
I am creating a drawing that shows a weldment on the first page, and then detail its parts on subsequent pages.

I create a drawing referencing the weldment (assembly), and place the views as desired.
I create the individual drawing views of the subsequent parts and place them as I wish.
the assembly tree shows me different icons for the drawing model and the view models. <-- good
when I "make displayed part" for any of the non-assembly parts, then return to the drawing, the assembly tree no longer shows me any of the subsequent parts. do I have a setting incorrect? am I doing something wrong here? is there a better way to show separate files on the same drawing?

-Cyril

 

[cyril009]

no feedback at all? is this expected behavior? have I explained my situation poorly? is this covered and my searches haven't been thorough enough?

I'd love some insight here
-Cyril

 

[cowski]

when I "make displayed part" for any of the non-assembly parts, then return to the drawing, the assembly tree no longer shows me any of the subsequent parts

When you say "return to the drawing", are you making the assembly the displayed part again and switching to the drafting module?

From the above quote, it sounds like you may be switching to one of the component parts and simply going to the drafting module; in which case, none of the other parts will show up since you are no longer in the assembly file.

Can you upload any screenshots? We may need more info here.

www.nxjournaling.com

 

[cyril009]

 

[cyril009]

... it sounds like you may be switching to one of the component parts and simply going to the drafting module; in which case, none of the other parts will show up since you are no longer in the assembly file.

My explanation was unclear, I hope the screenshots help.

No, I don't bother with the drafting module of the component part, we utilize the system where the drawing is a completely separate file.

After leaving the master drawing to view a sub-component, then returning to the master drawing, "reference only" objects are no longer shown in the assembly navigator, but the views are still on the drawing.

that's the part that I don't understand.

 

[Toost]

There must happen something that's either invisible to you the user, or something that NX does that you don't show in the images above. This behavior is not expected.
Can you do repeat the entire procedure in a new NX session and when it has happened, go Help - NX logfile and upload that text file here ?
( It will be a long textfile so attach is as a file instead of pasting the text.)
The log contains some information about your license, you can cut that part out, the section begins :
************** Licensing Information **************
and ends some 5-6 lines below :
****************************************************


Regards,
Tomas

 

[cyril009]

I appreciate your time toost,

I have repeated the sequence in a new session and saved the log text.
I'm working on adding it as an attachment, drag-and-drop doesn't wanna play well, and it seems to prefer a url in the box below? standby...

 

[cyril009]

take-2...

 

[cyril009]

take-3 (hosted on google drive)

 

[Toost]

I can't read any of your attempted uploads...
Pick the textline "...or upload your file to ENGINEERING.COM" below the "reply field" in the bottom of the thread.
It should then ask for what file you like to upload, then a second prompt when the file has been selected "upload-something".

 

[cyril009]

thx for breaking it down. fourth attempt...

 

[cyril009]

I can reproduce the issue on my pc easily.
I cannot reproduce the issue on any other PC here.
I cannot reproduce the issue logged in to my PC as someone else.
I called GTAC;
GTAC was unable to reproduce the same issue using my own configuration files, while I was still able to reproduce the issue.
GTAC had me change a few configuration items, effectively restoring my NX sessions to fresh-out-of-the-box, and voila, no more problems.

Thank you all for your time, it seems this is an isolated incident with no proper explanation.
-Cyril

 

[Toost]

Hm, mystery. I cannot see anything that , in my laymans perspective, seems wrong in the logfile either.
Maybe it reloads the drawing file from disk ?
Send the logfile to Gtac and ask them to help interpret.

Regards,
Tomas

 

[cyril009]

Date: 17-apr-2013 10:55:47
IR Number:[removed]
Short Description: Drafting Components are disappearing from the ANT

Hi Cyril, Good news! I was finally able to reproduce your problem. I tested again with your configuration and it turns out it was an ANT display setting: "Include Reference-only Components" which had been disabled. When the drawing was reopened in the state where the component were missing, I selected "Tools > Assembly Navigator" and enabled the setting "Include Reference-only Components" and now the missing components are displayed.

With best regards,
[removed]
NX Applications Support - GTAC