rename a part: the drawing is lost!

[paoloz]

Hi all,


I have a big problem with Proe2001.


I had a drawing called "filename1.prt". I created a drawing associated with this file called "drawing1.drw".


Then I renamed (on session and on the dsk) the file "filename1.prt" into "filename2.prt".


Then I went home... (close ProE, erased all in memory,...)


Well, now if I try to open the file "drawing1.drw", I cannot open it! There is the terrible white-cross message "Model <filename1.prt> is not in this directory"


How can I solve my problem? I want back my drawing1.drw!


Many thanks,


Paolo

 

[dr_gallup]

You have to rename the part back to the original name. Then open the drawing. Now rename the part. Save the part AND the drawing. All will be well.

You will have the same problem if there are any assemblies that use your part. You must have every object that references a part open while you do the rename and then save them after the rename so that they look for the new name.

 

[adriansima]

isn't there a config parameter to be set up in config.pro that changes the name of the drawing when the part is renamed?I think this isrename_drawings_with_object?


Adrian

 

[ankarl]

isn't there a config parameter to be set up in config.pro that changes the name of the drawing when the part is renamed?I think this isrename_drawings_with_object?


Adrian

True, but only when you save a copy (copies the related drawing together with the part or assy). You still have to save the drawing after renaming the part otherwise you looose the link.