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rename a part


New member
hello every body

i made a part and made it's 2d draft and i rername the part

when i opening the drafting file it's not opening a message is coming

(xxxx.prt is not avail in this directory)

again i rename the part and when i open the drw file its giving the

same message

how can i open my drw files


New member
Renaming only works when both model and drawing are open AND the drawing name is the same as the model name.

The entire renaming/copying/part switching behaviour in ProE is a real PITA if you ask me. In my other CAD, if I want to build an alternative construction,I can copy the assembly file, get intoa part I want to design differently, copy the part to a new name, get back to the assembly, replace the original part with the copy and then safely go about "playing" with the part copy. Since the files are originally identical there is no problem for the softwarerecognizing assembly links. When you change a part in ProE, it doesn't check if the relations can be kept, not even when replacing in session. The only possible solution is through family tables, but there are plenty of occasions where you can't or don't want to do so. The same goes for drawings. You can't force ProE to accept an alternative file as source, even if you know that they have the same features and references, and all links regarding views and dimensions could easily be re-established.

Oh well, you learn to live with it ...



New member

Rename the part to the Old name and while the part is in session, try to open the Drawing file.(do open the part first)

If you want to rename the part and some assembly or drw is referred to that part, then you have to open all the files referring the Part and Then you have to rename the part and Save all the assmblies/drws after regenerating once.

Might this will work.

Even if you do the same and drw is giving the same error.put the part and drw in the same directory and then open the Part ,rename it.then open the drw file.

Check the Following careully,

1.whether the part anme entering is sme that of old one,which is displayed in the error msg while opening the drw file?

2. are you referring more than one model i the drw?

3.do you referring any family table instances in the drw?




New member
There is a work around with replacing a part in a assembly without going through the painfull repeating process of reconstraining objects.

Lets see if I can explain this correctly.

Say you have a assembly A you have multiple parts in the assembly. You have two parts say B and C. B is in the assembly and C is not, but you want C in place ofB. You can take partC and B and copy them to a seperate file, deletepart C out ofthe directory, so in general BACK-UP Parts B and C, this is so pro-e will not recognize that partC exists and at the same time you Back them up. Next you open the assembly and then part B. Rename part B to C. Save and Close the assembly, delete part B and C out of the dirctory and put parts B and C back in from the Back-ups. Reopen the assembly and you will find that part C is in place of part B.

WARNING: this method usually works only if you use the save a copy from the original but it does work because I do it all the time.

Note: you will also find that the drawing will update automatically from the assembly without pulling it up when renaming the part.

Using this method as a back bone Pro-E has given us a loop hole for copying assemblies and replacing copied parts or even replacing parts that are not in a family table.

Note: if you do copy a assembly and only generate maybe half the parts as new parts I suggest using a temp directory to do this. For example if you have assembly A. Open assembly change your working directory to the temp. Save a copy and then you will find that all the parts that you must work on are in the same location without haveing a hundred files in one place. Work on them change them replace with other parts or do to what you want. This gives you a chance to mess things up and know exactly what you need to do to fix them.

Note: These suggestions are from a user that has never used a file management system like winchill or Intralink, the short cuts come from past learning expeience. You may not want to try this if you are useing a file management system. I personally dont know what will happen

hope this helps