Invisible Object in Entire Part reference set

[TechieGeek]

I have an assembly which I am editing, which was originally created by someone else. It is exhibiting some very bizarre behaviour, as follows:-
[ul]
[li]If I view the child part from within the parent assembly with the Model reference-set I can see the solid-body of interest.[/li]
[li]If I view the Entire-part reference-set, the solid-body is no longer visible.[/li]
[li]If I make the child the displayed part, I still cannot view the solid body.[/li]
[/ul]
Its almost as if the body has been excluded from the Entire-part reference-set, which by my reckoning should not be possible.

I have ensured all layers are visible, and "visible in view" also has all layers on. I even ran this journal which was suggested on a previous posting, however it didn't manage to reveal the solid geometry I'm expecting to see.

Can anyone offer any suggestions?

Cheers,
TechieGeek

 

[JohnRBaker]

Did you check to make sure that the solid body is not hidden?

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.

 

[TechieGeek]

I have tried all the "normal" methods to the depth of my knowledge ie. right-mouse-button>Show and Edit>Show and Hide>Show All... Still invisible.


Cheers,
TechieGeek

 

[Toost]

Can you create a new "dummy" assembly and add that specific component and see if it displays the same behavior there ?
Can you upload that specific component ? ( Or Confidential.)

Regards,
Tomas

 

[TechieGeek]

Ps. I have tried adding a 2nd copy of the child part beneath the parent, and it behaves in exactly the same way.

Cheers,
TechieGeek

 

[TechieGeek]

I created a brand new empty part, and added my dodgy part as an child. The solid is still visible in Model reference-set, but absent with Entire Part.

Cheers,
TechieGeek

 

[TechieGeek]

I will try to remove all the confidential geometry and upload the model.
I'm not that familiar with this website... how do I upload a file?


Cheers,
TechieGeek

 

[cowski]

The easiest way to share the file is to use the "upload your file to ENGINEERING.com" link below the reply box. Clicking this link will pull up a dialog box that will allow you to browse to your file and upload it; it will then report the link to your file which you can copy & paste into your reply or simply hit the 'add link to post' button and it will add the link to the bottom of your reply text.

www.nxjournaling.com

 

[TechieGeek]

The offending object is actually a wave-linked solid from another file, however if I break the link and reassociate to a different solid body, the behaviour is the same... visible in Model ref-set, but still invisible in Entire Part ref-set!
I have stripped out all of the other geometry, and uploaded the file here for you all to interrogate.

Thanks for all your help so far... but still looking for a fix, as there's a lot of history within my original file which I can't afford to recreate.

Cheers,
TechieGeek

 

[TechieGeek]

Just in case it matters, I am using NX7.5 with Teamcentre 8.
I've no idea which version of NX was used to create the original part from which I've inherited this problem.

Cheers,
TechieGeek

 

[Toost]

This is a VERY weird one, i have never seen anything like it.
I have found the solid. It' view dependent on the drawing.
I have not found a way to get is model dependent..



Regards,
Tomas

 

[JohnRBaker]

This file is a Drawing which contains nothing but 'view-dependent' objects, period. There appears to be nothing in the 'Entire Part' Reference Set simply because Reference Sets can only be used in the context of an Assembly. Simply opening the Reference Set dialog and selecting 'Entire Part' and not having anything highlight means NOTHING. Take a regular part where you're NOT having any problems and open the Reference Set dialog and select 'Entire Part' and see what happens. I'll give you a hint; NOTHING will happen. That's just the way it works. There is NO need to highlight anything because the term 'Entire Part' already says it all.

Bottom line, There is nothing wrong with your Part file! The only problem is that in the case of a Drawing with only View Dependent objects, Reference Sets are all but meaningless. After all, what was it that you thought you were going to benefit from whether the Drawing was or was not included in any of the Reference Sets? I hope you weren't thinking of creating an Assembly where one of the the Components would be a Drawing. If so, what were you going to do with it? What benefit were you going to gain? How was this going to be used in your product design and manufacturing workflow?

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.

 

[TechieGeek]

John - please try introducing this part as a child into a new blank Assembly, and see if you think it is still behaving normally. Forget about Drafting-mode (I had intended to remove all that stuff), and look within Model-mode. There is a wave-linked solid body which does not display properly. I hope you have the answer, but Toost and myself both think it is very strange behaviour.
Why is the offending wave-linked solid view-dependant, and how can I make it model-dependant?

Cheers,
TechieGeek

 

[JohnRBaker]

I can't explain it. At this point, the only people who may be able to help is GTAC. They've got tools to look deeper into a part as well as tools to 'reset' certain aspects and behaviors.

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]

Yes, it time to speak to GTAC. This partfile is not normal.
- I doubt that they can explain why it got this way but i think that they can help you repair the original part.

Regards,
Tomas

 

[Nethajisubash]

SIR YOUR MODEL WAS IMPORTED IN DRAFTING MODE
I ATTACHED THE PPT FILE

 

[Xwheelguy]

This was the ONLY way I was able to get the solid OFF of the dwg and into the Modeling application:

1. Open a new, blank part file.
2. Use File -> Export -> Part and export ONLY the solid to the new part file, do not choose any dwgs, however make sure to retain internal parameters.
3. Go over to the new part file and enter Drafting and Open the drawing named SHT001.
4. Edit -> View -> View Dependent Edit and pick the dwg sheet.
5. From the View Dependent Edit dialog, pick View to Model. Select the solid.
6. Your solid should now be visible in Modeling.

I tested the visibility of the solid body by adding it as a component to a new part file and it behaved normally. Hopefully everything you require will somehow export over to the new part. If not, try copy/paste. With the mess you have, you may have to recreate some things. Be mindful to NEVER import solid geometry or entire parts into Drafting into the future. IMO, if importing a part into Drafting behaves this way, then this is a bug in the Drafting application, as solids should NEVER be allowed to appear on a sheet.

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB

 

[Xwheelguy]

I went back and tried my steps again, and left out something important:

Perform a View Update (Edit -> View -> Update and allow all views to update. You will get a message that the update fails. Click Suppress after each update, then begin the steps above.

Tried to include a movie, but the file is too large I guess - won't upload.

Tim Flater
NX Designer
NX 8.0.3.4
Win7 Pro x64 SP1
Intel Xeon 2.53 GHz 6GB RAM
NVIDIA Quadro 4000 2GB