Component names that are not up to date in the Feature Manager of an assembly

3D Design Volume Model
1

Hello world

 

When I have an assembly, I open one of its parts on which I have a new name "saved as". I have the "save copy as" option unchecked. Once saved, the window in my room has the new name.

 

When I go back to my assembly, the part still has its old name!!

 

If I re-open this part from the Feature Manager, it shows me the part with the new name!!

 

No matter how hard I try to close, re-open it doesn't change anything: the ASM Feature Manager doesn't update.

 

In "tree display" I did check "Show component names" but without any more effect on this manip.

 

If I now do "Replace with" a new part, the Feature Manager updates well.

 

I'm on SolidWorks 2013 SP4.0, I work outside EPDM.

 

If anyone knows how to do it...

 

Thanks in advance

2

Hello

 

SolidWorks 2013 SP4, the first thing to do would be to update to SP5...

3

Secondly, is it a problem with the configuration of the workstation?

Can you try another position? Do you reproduce the problem?

 

If you don't have another workstation available, you can reset the configuration by renaming the registry, and I'll explain in another post.

4

Hello

 

If the assembly is open, normally it updates well.

If it is closed, it is normal that it keeps the first piece.

 

The part was not created in the assembly, then rename, and then manip to change the name by saving as?

I think I've seen this once before, he kept the name changed in the assembly...

 

OPEP

5

Hello

Was the part saved in the assembly or as an outside file the first time (before saving as)?

I had the case where he had saved my subassembly in a folder other than the one of the set, and when I opened it he went to get the save as.... Weird

So what I did I had the component replaced and indicated the new one, then after I deleted this nasty backup. 

It may not be the right handling but it worked.

6

More info...

 

I submitted a . SLDREG from my old company, and it works again...

 

Do you have any idea what option this kind of prank can do? If it can avoid redoing all the settings...

7

you should go to the "system options", chapter "file location" then "referenced documents" and check the address(es): this is the place of search of Solidworks when it has finished all its "automatic" searches for references

 

Then check the option of the file save window: "Save copy as" is checked? if so; The problem comes from there


capture.jpg
8

Hello

It happened to me again yesterday. When resuming a project. On several occasions when the part was replaced, the name did not change.

A simple [Ctrl] [Q] solved the problem.

[Ctrl] [Q] = Rebuild

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9

As in the original message, the "save copy as" option is unchecked...

 

As for the component replacement, the name updates well, the phenomenon only happens when I register a part under it.

 

And of course I make this recording with the assembly open behind...

10

In Solidworks, go to Tools, Option, External Reference, and check the box "Update component names when documents are replaced"

2 Likes
11

It works after a SoidWorks reboot,

 

Thank you very much fthomas,

 

Have a nice day

12

You're welcome Benoit ;o)

1 Like