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drawing names


New member
I'm using student version Proe2000i

I changing my part naming scheme from descriptive names to part numbers.

I can easily copy the.prt and .drw files and assign part number to the copies. But the drawing is still linked to the original .prt file. I want to link the newly named drawing (w/part number)to the newly named part (w/part number). I could of course just make a new drawing, but I want avoid the hassle of cleaning it up.

There must be a straight-forward way to accomplish this, but it's not obvious to me. I'm alearn-from-a-tutorial user, soI'm a little light on the fundamentals and a lot of other stuff.

Suggestions will obviously be appreciated.

Denny L. Graham


Use the file/rename within Pro/E, otherwise all is FUBAR. Pro/E uses the file name to find all associated objects.

You have to have all objects that reference your part (drawings and assemblies) open in memory BEFORE you rename your part. Then you can rename your part through File/Rename. Then save all the drawings & assemblies. The same applies to assemblies. You have to open all upper level assemblies and drawings, rename the assembly and save the upper level assemblies and drawings.

Alternately, since you are using 2000i, you can use a text editor to change all the instances of old_part_name to new_part_name in a drawing or assembly but it is not supported, the chance of screwing it up is high and it will not work in newer versions.


New member
Thanks for the prompt and detailed reply.

If I understand you correctly, I can rename a part and if the part drawing is in memory, the drawing will also be renamed.However, I get the feeling I can't do what what to do, i.e., keep the old part, as-is,and use copy to generate a new part name because the drawingwill not copied and assigned the new name, unless-- .

I go to thesecond approach, where I'm likely to screw up. The good and bad news is that I'm not familar with file typewhere I could make the changes, and it's not because I haven't looked. The only file that I could locate and readis the .inf file. I suppose .inf means information. Note: I only have .inf files for a few parts, so apparently I unintentionally created them. Any way back to the issue of changing all instances of old_part_name to new_part_name, which file? Is there a text editor within Pro/e that must be used?I have come across an editor, but it seemsto be a bitof a kludge.

As you can tell I'm still a novice, although I'm been using Proefor over four years. I've tended to learn only what I needed to accomplish the task. An approach that leaves some big gaps.

Thanks again.



New member
hi denny,

first open the assembly file where the part you want to rename is assembled.then open the part, and then open the drawing file of that part.now you rename the part you want and save it.then activate the drawing and regenerate both the drawing and model in drawing.now you can see the changed model name in the model tree. then save it. similerly activate the assembly and regerate it. then save it.

thats all. you are done. still if you afraid of data missing and want to play safe, copy the directory in windows and save some where as a reference.

best wishes


If tou want to copy a part with it's drawing to another name, there is an option in the config.pro called rename_drawing_with_object - set this to both and it will save assemblies &parts with their associated drawings.


Just a note about editing part, drawing & assembly files. Use a good ascii text editor, I use TextPad from Helios Software but there are dozens. You need something that will allow you to open large files (windoz notepad will not work). TextPad changes your windoz RMB menu to let it open ANY file regardless of extension. Older Pro/E files are pure ascii, WF files have an ascii header but are binary farther down. You CAN NOT edit the binary files because there is a checksum that will be wrong if you make any changes.

Say you have renamed a part from old_part_name.prt.1 to new_part_name.prt.1 but you have just one assembly that you forgot about during the rename that is still looking for part old_part_name. You could open the assembly and go through all the Pro/E failure recovery stuff but do you know how the part was assembled originally? Maybe, maybe not. So instead, you edit the assembly file in your ascii editor and do a global search & replace of every instance of the text string OLD_PART_NAME with NEW_PART_NAME. Note that Pro/E file names are all lower case but inside the files they are all UPPER case. Save the editied assembly file with a higher index number and see if Pro/E will open it successfully.

I have done this many times with about 95% success rate. Good file (re)naming practices eliminate the need to do this.