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Any ways to avoid startin from scratch?


New member
hi guys, i've been asked to modify an existing part but it will be used under a new part number. I did the modification in Pro/E but when it comes to engineering drawing, is it necessary to start from scratch or is there a way to save my effort and time to use the existing drawing (only added a few extra cuts, the size n other bits remain the same)? I'm not sure have I explain this clearly. In other words,the drawing is model related (file name) and can I fool pro/e to use the new part number as the orginal one. I hope sum1 out there could save me as the drawing consist of 2 whole pages of dimensions
. many thx in advance. in the mean time, i'll get a crack on to start from a new drawing....Marvin


The easiest way to do this is to plan for your drawing (and assemblies!) BEFORE you modify the part. Retrieve both the model and drawing then rename them both IN SESSION ONLY (nothing on disk is changed so your original part & drawing are unchanged). Then you can redefine to your hearts content.

Since you have already copied and changed the model you have broken the link between part and drawing. To fix it, create a new subdirectory (I'll call it temp), COPY your old drawing to it and MOVE your new part to it. Rename the new part to the old part name. Start Pro/E up and change your working directory to temp. Now you can open the copied drawing which will use the new model but with the old name. Rename both the drawing and model (both in session and on disk this time because you are working in temp). After you are done you can move the new drawing and part back to the original directory and delete temp directory.
You made a copy of a part but not it's drawing?

For clarification,
Let's call your original part 'a.prt' with 'a.drw'
You made copy of 'a.prt' to 'b.prt' but you did not copy the drawing.

I think your best bet is to copy 'a.drw' & 'a.prt' (together) as 'c.drw' & 'c.prt'.
Then copy features you addedfrom 'b.prt' to 'c.prt'.
Then on 'c.drw' you just need to show dimensions for new features.

BTW, are you using Intralink or other file managing software?

Good luck,



New member
Thanks very much for the reply, Dr. Gallup! Yeh, I'm a total novice on Pro/E. My colleague taught me to rename the part 'in session' also. Somehow, the pro/e won't let me do it tht way because it is controlled by some sort of PDM, intralink over the other side of the ocean. So I tried my own method (me 2 lazy 2 start from scratch). I useda HexEditor to replace the drawing file the old part number with the new part number. Normal text editor won't do the job as it wont be save in binary format. I was still sceptical because I was thinking Pro/E might have checksum, etc to validate the filename it called up. Luckily, it hasn't and I have fooled Pro/E to call up my new part and remain all the dimensions which were on it...


New member
Thanks very much Charles. yeh, it was the PDM thing, otherwise I could just simply rename the part, etc like your method. anyway, cherz again.


New member
Sounds like a good option for you would be to "File > Backup" the drawing, this will save the part also. Erase the old drawing/part from memory and open the backup drawing/file. Do a renameof both the part and drawing and you should be OK.


New member
I hope I understand you correctly. If not sorry.

set the option "rename_drawings_with_object" to both in the config.pro file. (<tools<options).

Then when you open a part and select "save as" the drawing will be saved with the new part with the same name.

123.prt has a drawing 123.drw associated with it. If you save 123.prt as abc.prt the drawing 123.prt will also be saved as abc.drw in one step. Now you have a new part and drawing to work with and the original is not affected.


I fool Pro/E all the time with this. Say you have part a. You take a copy of this part, do all your modifications, call it part b. You didn't bother to copy the drawing of part a at the same time (if you're using Intralink) but it doesn't matter. So long as you used stable features to set up your drawing, for example default datum planes, then all you need to do is rename your new part b temporarily in session to part a whilst you pull in the drawing of part a. Renameback to part b,rename the drawing and make sure you save the drawing.