cascadco
Automotive
- Oct 26, 2007
- 16
- 0
- 0
Does anyone know, how can I replace drawing links correctly?
Thanks.
Thanks.
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CATIA V5 Drawing links replace
- Thread starter cascadco
- Start date
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cascadco
Take a look at this post.
Regards,
Derek
Take a look at this post.
Regards,
Derek
You question is quite short and I don't know wheter this explanation is obvious to you, but this is the normal procedure:
Open the 3D model.
Open the drawing and drawing as active document:
Edit / Links
Replace / With loaded document
Sometimes (if error occures) you have to first remove the links and then try again.
Open the 3D model.
Open the drawing and drawing as active document:
Edit / Links
Replace / With loaded document
Sometimes (if error occures) you have to first remove the links and then try again.
- Thread starter
- #5
sorry but you cannot change or access the UUID.
With a script you can actually change the link of the view but you will have to relink dimension...
To avoid further problem :
When a drawing is made from 3D file A, if you have to change the geometry, use the same 3D file A in order to create 3D file B, then your drawing can be link to 3D file B.
With a script you can actually change the link of the view but you will have to relink dimension...
To avoid further problem :
When a drawing is made from 3D file A, if you have to change the geometry, use the same 3D file A in order to create 3D file B, then your drawing can be link to 3D file B.
Eric N.
indocti discant et ament meminisse periti
indocti discant et ament meminisse periti
i still get error message "drawing refuses the link" when 3d file A is used to make 3d file B. Is there a setting that is preventing a re-link? I am a converted solidworks user now using catia, solidworks relinks drawings with ease and saves a ton of time detailing. Catia is made by the same company, don't understand why this is so difficult.
weavedreamer
Automotive
Perhaps one day, a disgruntled software user will program a better approach. Untill then, consider packaging your part inside a product and pointing the drawing back to the product. New part - Open Product, change Part, open Drawing, Smile. Then just add extra files to manage into your scenario.
create file A, then: file, save as, new file name (file B). I didn't modify file B in any way from file A except change the file name. I created dwg A then saved as dwg B in the same way as the part file. Then I go to dwg B and try to change link from part A to Part B. Thats when I get the error message, am I doing something wrong? In solidworks you had an option to redirect the link as you opened the dwg. I don't see this option in catia, does it exist somewhere?
liquidlunch
Industrial
If you created file b with the "save as new document" selected you gave file b a new uuid. I also think if you created file b before you made the drawing of file a it won't link up to file b. Try creating the drawing of file a before you create file b because when you do a save as on file a to file b it will prompt you to tell you of the impacts it has on the links and ask if you want the links to be applied to the new part.
I always use save management when trying to maintain links. Since you haven't changed file b in any way it should be the same as file a, correct? Since the drawing was created from file a you should be able to use save management to save both as new file b. I always start with a fresh session of v5, open both the part and drawing and then you can right click on the drawing and select all pointed. You will see that the part will highlight with the drawing showing they are linked. Using the pattern name type *-rev1 (just an example) then select apply pattern. Both the drawing and part will have -rev1 added to the end of the part name. You will be able to see the path it will save to in the next column. Now do a save as on both of the files to a directory (example //part#-rev1). Make sure the new path shows up in the location column and action states "save" on both of your files then select ok. If the save as is greyed out you have to click in the epmty area below the parts to deselect the files. I always exit out of catia and open a new session and the new files as a sanity check.
Hope this helps
I always use save management when trying to maintain links. Since you haven't changed file b in any way it should be the same as file a, correct? Since the drawing was created from file a you should be able to use save management to save both as new file b. I always start with a fresh session of v5, open both the part and drawing and then you can right click on the drawing and select all pointed. You will see that the part will highlight with the drawing showing they are linked. Using the pattern name type *-rev1 (just an example) then select apply pattern. Both the drawing and part will have -rev1 added to the end of the part name. You will be able to see the path it will save to in the next column. Now do a save as on both of the files to a directory (example //part#-rev1). Make sure the new path shows up in the location column and action states "save" on both of your files then select ok. If the save as is greyed out you have to click in the epmty area below the parts to deselect the files. I always exit out of catia and open a new session and the new files as a sanity check.
Hope this helps
liquidlunch
Industrial
I guess I am not a fast enough typer. Glad it worked out for you.
CatMann
Aerospace
- Nov 16, 2007
- 23
- 0
- 0
Infact, I also have redrawn the entire drawing again and agian many times, but with no changes. Im irritated much with DS.
This especially does not work out if the drafting goes at a differnt end than the design end. When a designer updates his design again and again with the modifications and sends the file(which is a with a new name(that name with rev added), certainly with a different uuid. But the drawing at the other end does not accept this new file.
Moral of the story is: Like parent child relationship. its always catious of working on only one design file that has been used previously for creating this drawing. So, keep shuffling the same design model file between drafter and designer.
Do you understand? or Have I confused you further?
Thanks,
CatMann
This especially does not work out if the drafting goes at a differnt end than the design end. When a designer updates his design again and again with the modifications and sends the file(which is a with a new name(that name with rev added), certainly with a different uuid. But the drawing at the other end does not accept this new file.
Moral of the story is: Like parent child relationship. its always catious of working on only one design file that has been used previously for creating this drawing. So, keep shuffling the same design model file between drafter and designer.
Do you understand? or Have I confused you further?
Thanks,
CatMann
Very annoying but UUID will dictate your work unfortunately.
I also thought it was stupid because you could use the same drawing format even views and sections in v4 and save a lot of time.
But even more annoying is that sometimes you get the "drawing refused the link" without any reason. In fact I shouted and called one of our designers an idiot because I thought he had broken the link by doing a "new from" but I was wrong he managed to relink it from a new location to the released and locked file. I felt really bad about it because I thought it was impossible to cheat the system.
I also thought it was stupid because you could use the same drawing format even views and sections in v4 and save a lot of time.
But even more annoying is that sometimes you get the "drawing refused the link" without any reason. In fact I shouted and called one of our designers an idiot because I thought he had broken the link by doing a "new from" but I was wrong he managed to relink it from a new location to the released and locked file. I felt really bad about it because I thought it was impossible to cheat the system.
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