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Creo Parametric 5.0 - Copy of assembly and drawing link

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Creo Parametric 5.0 - Copy of assembly and drawing link

Is there a way to create a copy of an existing assembly for a new part number, as well as the drawing, while maintaining the link between the new part number and drawing? I tried to make a copy of each, but when I look at the new drawing, it still references the old assembly.

1 ACCEPTED SOLUTION

Accepted Solutions

Re: Creo Parametric 5.0 - Copy of assembly and drawing link

Are you using Windchill or not?

 

If not:

1. Go into the folder where the drawing and model exist.

2. Copy the drawing and the model into the folder. ( I usually add ZZZZZ in the front of the names.)

3. In Creo, pull up the drawing and model you are going to rename.

4. Rename the drawing and model. Save the drawing and the model.

5. Go into the folder and change copied (not renamed) drawing and model back (scrubbing the ZZZZZ).

6. You should be good to go.

 

If it is Windchill: 

Someone else will have to chime in.

5 REPLIES 5

Re: Creo Parametric 5.0 - Copy of assembly and drawing link

I resolved the issue. Apparently you can't directly link a new assembly with it's associated drawing through the "Save copy" feature in creo. You have to go through Windchill directly and rename the files there simultaneously. 

Re: Creo Parametric 5.0 - Copy of assembly and drawing link

Are you using Windchill or not?

 

If not:

1. Go into the folder where the drawing and model exist.

2. Copy the drawing and the model into the folder. ( I usually add ZZZZZ in the front of the names.)

3. In Creo, pull up the drawing and model you are going to rename.

4. Rename the drawing and model. Save the drawing and the model.

5. Go into the folder and change copied (not renamed) drawing and model back (scrubbing the ZZZZZ).

6. You should be good to go.

 

If it is Windchill: 

Someone else will have to chime in.

Re: Creo Parametric 5.0 - Copy of assembly and drawing link

Definitely use windchill to do the save-as, it does a great job of handling the relationships and shows you if you have "unintended" relationships also.

You can also pull in related drawings for sub-components, if desired. It's a great way to take a fully completed design and drawing package and create a copy of the entire package for a new version of the design.

You'll want to learn about the save-as functionality in windchill also. You can use the save as on components in an assembly and during the save as, if you use the "next" button, you can auto-magically replace the old component within your next level assembly with the new component. If your old component has multiple next levels, you can select which ones get replaced with the new component and which ones keep the old component.

 


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

Re: Creo Parametric 5.0 - Copy of assembly and drawing link

Sounds like the way to go if..... you have Windchill.

Re: Creo Parametric 5.0 - Copy of assembly and drawing link

There's an easier way: you can add to config.pro option rename_drawings_with_object and set it's value to "part", "assem" or "both". That way you can open a model, save a copy and in the target folder you'll get the model with a new name along with a renamed drawing referencing newly copied model. On the other hand, this will work only, if the model (part or assembly) and the drawing have the same name. If they don't, drawing will not get copied.