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CREO 3.0 drw Assembly Association

SOLVED
Regular Member

CREO 3.0 drw Assembly Association

For instance, I copied over four files, into a new folder),  (2 prt's., 1 asy and 1 drw), renamed them and had to "Replace" the prt's in the asy, but, how can the renamed asy be re-associated in the drw, it doesn't seem to give you any option to do this. It won't even allow the new drw to be opened, it is looking for the old asy.

  Thanks,

 

  Craig

1 ACCEPTED SOLUTION

Accepted Solutions

Re: CREO 3.0 drw Assembly Association

You may wanna use rename with object option. Config option rename_drawing_with_object

 

Basically if this this option is set to both, on saving a part as new copy an associated drawing with new part will create on own. 

E.g. There is a part A.prt and associated drawing is A.drw, if that option is set accordingly on saving part A as X.prt a new drawing x.drw will create and that will be associated to X.prt. 

For this part/assembly and drawing name should identical and data should be in same location. 

5 REPLIES 5

Re: CREO 3.0 drw Assembly Association

You may wanna use rename with object option. Config option rename_drawing_with_object

 

Basically if this this option is set to both, on saving a part as new copy an associated drawing with new part will create on own. 

E.g. There is a part A.prt and associated drawing is A.drw, if that option is set accordingly on saving part A as X.prt a new drawing x.drw will create and that will be associated to X.prt. 

For this part/assembly and drawing name should identical and data should be in same location. 

Re: CREO 3.0 drw Assembly Association

You can't re-associate the model once you done the rename.

The way to do this is open the drawing. open the models one at a time. Rename each model using creo. Rename the assembly in creo. rename the drawing. Save the models and assembly. Save the drawing. It's always important to save the drawing last, and double make sure the drawing actually did save after the renames, I usually make a minor drawing change (move a view or text) and then re-save, just to make sure.


Steve Williams
Pro/E Version 15/16 (Circa 1995/1996)

Re: CREO 3.0 drw Assembly Association

If you are not using Windchill, put the files you want to rename and their associated drawings in a separate folder.

Set your working directory to that folder.

Open up all models (part and ass'y) and all drawings.

Rename the drawings, rename the models. (Save everything - I usually save several times in the process).

Now you can close out of all the drawings and models and they should have all their associations attached.

Re: CREO 3.0 drw Assembly Association

Dale is correct - also, emphasis on Rename from the Creo interface, not the file-system.

 

PTC partitioned rename management into Windchill where it will take care of a lot more than drawing associations. There is no product or other method for patching drawings to use models with other names.

Re: CREO 3.0 drw Assembly Association

Thank you