Drawing file fails to locate renamed part file

[Kishore_K]

Drawing file is not opening if its part model is renamed, it says "Model <filename.prt> is not in this directory". How to maintain the reference between the part models and its drawing files?

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[StephenW]

You must have the drawing "in session" when renaming the part model. After renaming the part model, you must save the drawing so it "remembers" the part name change.

I assume you are not using PDMLink (Windchill).

[Kishore_K]

Yes but if the file is not "in session" how does it remember the part name change?

[StephenW]

You must do the rename using FILE - Manage File - Rename from with Creo. You can't use window explorer or other file managers to do the rename.

A simple example would be to open a drawing of a part, open the part, rename the part from within Creo, save the drawing.

[MartinHanak]

If part's drawing is not "in session" during part renaming then you are in trouble ...

If you do not use Windchill, then RENAME action is very risky. You have to know, what drawings are necessary to open and save after part renaming. Nobody helps you ...

Martin Hanak

[Dale_Rosema]

If you need to find out where something is used, here is a good thread to a batch program that can be run to find out. As Martin mentioned, it is very risky.... proceed with caution.

Re: Where used?

Thanks, Dale

[Dale_Rosema]

What Stephen is trying to say is that if the file is not in session it will not remember that the part name has changed and the link between the two will be broken.

Thanks, Dale

[R.D.]

If you have already renamed the part, you will have to open the part, rename it to the original name that was associated with the drawing, open the drawing which should now find the part, and then (as mentioned) rename part with drawing open and save both.

[mpeterson]

Stephen answered the question in that you must do your renaming within Creo/Pro-E and have associated files in session and save. If you rename a part open the drawing and any assemblies the part is in before renaming and then after the part renaming save the drawing and assemblies. If you get this problem then what you can do is open the part again and rename it back to the old name the drawing or assembly is looking for and then open the drawing or assembly. Then you can rename again back to the desired new name and same the drawing and assembly files. Because of this issue it is also a good idea to only have one part detailed per drawing.