How to re-associate a drawing with a model that has been re-named?

[David_M]

Hi all

Does anyone know how to re-associate a drawing with a model if the drawing cannot find the model because the name has changed? When I open the drawing it just closes again. WF5.

Thanks

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[KshetrabasiMaha]

Hi

When you open the drawing it will ask for a specific part number.

Note that part number.

then close the drawing.

Now open the renamed part(if you remember which was the associated part)

Rename or save as the part to the old name(you have noted from the drawing)

Now open the drawing

If you have any doubt please reply

Regards

K.Mahanta

[MohanMB]

Hi,

You are telling someting like doing a correction. But what if that is the intended requirement? I mean what if genuinely the part file name needs to be what it is changed to and the drawing should simply refer the new file name. How to do that?

And moreover if you use intralink or Windchill PDM then the dynamics would change even more i guess.

Although i have a different issue but it appears to be somewhat related to this original query so i thought of continuing based on the above discussion.

Regards,

Mohan

[KshetrabasiMaha]

Hi

If you will work in proper sequence then association will never break.

If you are talking about part and drawing association:-

1.Open the part

2.Open the drawing

3.Rename the part

4.(Rename the drawing if required)Regenerate and save the drawing

This process will not break the assocition.

If you rename the part without opening the drawing(drawing not in session) then the association will be broken.

In this situation you have to follow the steps I have suggested in earlier reply

(After reassociation you can again rename back the required name)

Regards

K.Mahanta

[SylvainA.]

Working even with PDM link (near kshetrabasi mahanta solution):

1. Note the name of the part the drawing refers to.

2. Open the renamed part.

3. Rename the part in session with the old name.

4. Open the drawing.

5. Rename the part in session with its new name (thus this is still the part that is in PDMlink).

6. Save the drawing (now refering to the renamed part).

7. You could check-in the new iteration of the drawing. It will now refer to the renamed part.

[BrianMartin]

Also David...

Check the status of the config.pro option rename_drawings_with_object to both. In the future if you're renaming a part or assembly, the drawing with automatically rename. This also works for saving a copy of the part/assembly. As long as the drawing is in the current working directory, this option does well.

You'll still have to use one of the techniques mentioned above to fix the problem you have now. But in the future this can stop it from happening again.

Thanks!

-Brian

[ReinhardN]

Brian,

the drawing must be in session, tested in WF4, WF5, Creo1 M020, else renaming will not do. For saving a copy you are right.

Reinhard

[BrianMartin]

I've actually only ever used it for saving a copy. I must have been mistaken that it also worked for a rename. The techniques the other people above have recommended should work. There was a time when you could open the drawing file in a text editor and just replace the model names and have it work. Sadly, we're beyond that now.