Catia V5 Drawing

[robcp]

I have renamed the CATPart files, but I cannot relink the CATdrawing files to the renamed files. If I change something in 3D, the drawing will not be updated.
Would you please let me know how I can change the links of the drawing files.
Thank you.

 

[1oldcaduser]

Were the drawings linked to the original CATParts before you renamed them? Because if you opened the drawing first then opened the CATParts by edit links then you should have no problems

 

[robcp]

Thank you for the answer.
Let me tell you what I did.
I have moved some files from one director to another with Copy, then Paste. I have renamed the files and I have recreated the links for the drawings with Edit/ Link/ Replace, but for the CATProduct files I had to replace each component with the files that i renamed. I did not like this job, but I did not know how to do it in other way.
Now I got another issue, if I re-open the product files, the components are unloaded and I cannot upload them and if I use Save Management for the product files, the files located in the old director are saved too. I do not know why? Any suggestions?
Thank you

 

[Archangelz]

robcp,

There are several ways to move files from one directory to another. You actually picked one of the worst ways, using Windows, and that is why you're having these problems.

I'll let someone else give you the solution to your current problem. In the meanwhile, when you need to move files from one directory to another, try File pull-down menu > Send To > Directory. Here you can specify what files you need to move (which I assume will be all of them), where they need to go, and if you want to rename them on the fly.

Another method you may want to consider is through File pull-down menu > Save Management. From here you can use the Propagate Directory button to move your files to a new directory.

I'm being kinda high-level on these two functions. You'll want to go through the Dassault documentation to get the nitty-gritty stuff.

Archangel

 

[catiajim]

When using Save Management to move a product and a CATDrawing, you need to do the following:
Load the CATProduct and all of the Parts
Load the CATDrawing(s)
FILE, SAVE MANAGMENT
Select the Product
SAVE AS
Choose a directory for the Product
Select PROPOGATE DIRECTORY
Select Enable Independant Saves
Make sure that your CATDrawings are not selected to save!
SAVE.
Now, go back to FILE, SAVE MANAGEMENT
Select your Drawing
Select SAVE AS
Choose the new directory
Repeat for any other Drawings
Select SAVE.

This will make sure that all of the links between the Product, Parts, and Drawings are correct.

If your files are already moved, you can sometimes use the "Search Order" under TOOLS --> OPTIONS --> GENERAL --> DOCUMENTS and make sure that CATIA is looking first in the "Folder of the Originating Document" (same folder as the document you are opening). You might also try disabling "Folder of the Link" (the folder that everything was in before you moved it - if the links were not fixed correctly).

When you try to use EDIT LINKS REPLACE, what error do you get? If you get the "Document refused the link" then I think you are SOL. You can create a script that will re-link the view, but it does it by first isolating the view, then creating brand new links - not always the ideal solution.

 

[robcp]

Thank you very much for all the information.
I have tried to move the files with File/ Send to/ Directory and also with Save Management. In the same time, I have renamed them. It worked but still, if I check the link of the views in the drawing files(I used "Query Object Links"), it nothing changed. Each drawing is linked to the file from the old directory. Did I do something wrong???
Should I relink the drawings to the relocated CatPart files?

 

[catiajim]

If they will re-link, yes.

 

[robcp]

For some of the drawings, the Edit/ Link/ Replace worked, but for the others did not. I got "Document refused the link" error message. Is this the right command to be used to re-link the files? Is any other available? Please tell me which is the best way to re-link a CATDrawing with the CATPart file?

 

[catiajim]

Yes, Edit/Link/Replace is the proper command. You will occasionally find that you get the "Document refused the link" error. I have never found a way around this error without resorting to the script I mentioned earlier.

As a general rule, if you follow these steps, it seems to work better:
[ol]
[li]Copy your Part and Drawing [/li]
[li]Load your New Part and New Drawing[/li]
[li]Re-link your Drawing (Edit/Links/Replace)[/li]
[li]Update your Drawing[/li]
[li]Save and Close your Drawing[/li]
[li]Make the modifications to your Part[/li]
[li]Load and update your Drawing.[/li]
[/ol]
Note: you don't need to close your drawing while you change the part. The key here is that you need to relink the drawing before you make any modifications to the parts.

 

[robcp]

Thank you catiajim !!!