Incorrect View

[cosmarchy]

Hi,

I've deleted parts from my SolidEdge assembly and saved it away, some time back. When I come to put this assembly into a draft, the parts I have deleted still show on the draft however when you open the assembly they are not there!!

There is no evidence of these deleted parts in Revision Manager and the view is up to date.

Anyone have any ideas why these parts are still showing?

Thanks

 

[KENAT]

Is the drawing view fed by a configuration? You may need to right click on the view, select the display (?) tab and tell it to check configuration or whatever the wording is at the bottom.

You can change the setting to auto check configurations if I recall correctly.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​

 

[cosmarchy]

Hi Kenat,

Thanks for the suggestion. I tried what you suggested and there was no change; I even deleted the configuration and started again but this also didn't work!!

It appears as if there is some corruption in the assembly. It looks like the assembly file is not linked to the deleted parts (not showing them) which is correct but the draft somehow has links to the deleted parts - whether this is a link to the part or some cached geometry I don't know.

Is there any software to 'check' the assembly file for corruption do you know?

Thanks

 

[swertel]

Under the MANAGE tab (from the upper left Gem menu) is EDIT LINKS.
Check there and look for any links to files that may or may not still exist.

If there aren't any there, check for empty drawing view and delete them.
I do this by changing my Select Options. Keep ALL LAYERS checked and uncheck everything else but DRAWING VIEWS, then select all.

Otherwise:
[ul][li]Is something on a layer that you need to delete that was linked (like a property text) to the file?[/li]
[li]Is something on your background sheet, 2D model sheet, or draw in view?[/li]
[li]Do you import a block or symbol that has a link to an external file?[/li]
[li]Are you using Family of Assemblies?[/li][/ul]

If none of the above work, then create a file with the same filename as the file with the bad link. Put some geometry in the file (just so you it renders on the draft). Once the link has been re-established to a file, you may be able to delete it.

Otherwise, bad links was a known bug in earlier versions of Solid Edge. Send it to GTAC and the developers can sometimes go in and correct the code and send the file back to you. That may take longer than just recreating the file yourself.

--Scott
www.wertel.pro

 

[cosmarchy]

All sorted

One of my 'esteemed' colleagues decided in his infinite wisdom to copy an assembly as a part (god only knows why). The net result of this is once this part is buried many levels down in an assembly and the bits that are in the copied assembly are deleted higher up in the assembly the copied part is contained in, it still looks like the original pieces are still there and so does the draft. The draft was showing the construction surfaces in the part.

Confused? We certainly were

Thanks for all your responses guys.