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How do you rename a ProE model file.


How do I go about changing model names alredy created and saved. I already created an assembly of the parts and I now want to change the names. Is it possible to rename your ProE files already created and saved?


Active member
Yes renaming a part or parts in the assembly is possible.

In the File menu click on Rename.

By default it will ask to rename the assembly , so you can change the the name of the assembly but if you want to rename the part or parts right click on the right top icon in this dialogue box and click on part.

Now you click on the part you want to change the name of.

After that it asks change the name in session or session and disk.

Don't forget to save and purge your assembly.



when renaming parts without pro/intralink just be careful, and be sure to open all your assemblies that the file is used, otherwise if you rename a part and the assembly is not open, when you retrieve the assembly proe will not be able to find the component (with its old name) and proe puts you in resolve environment...



New member
If you're using Intralink the default is to not allow you to rename objects in session. You can change this with a option but I think that's playing with fire.

If an object is checked into the common space then you have to rename it there and update the workspace.



New member
Just as you need to have an assembly in session when renaming parts, remember too also have the part drawing in session as well. Else the same problem will result.


New member
You can rename the top level assembly and rename components in the SAVE A COPY dialog box. The ASSEMBLY SAVE AS dialoge box opens up in a model tree structure. The existing assembly is in the left column.The names for the new assembly are in the right column.

* Select to reuse the names of existing components

* Select and edit a single component name.

* Use the suffix edit box to assign all new names at one time.

But this will create a copy!! of your assembly!!


New member
If you are using a PDM, you would query where the part/assy/dwgs you want to rename was used. You would then retain ownership of these parts/assy's/dwgs and bring them ALL into session. This is the way I was taught and still believe in it. Start with your parts you need to rename and rename them, save them if there is no parent assy or dwg. Close the windows, go to your assy's next, rename them if necessary. Save the assy's if you have no drawing related to them. Close the windows after you complete the rename. The reason for closing the windows, is not to confuse yourself with something you have already completed. Go onto the next higher level, drawing or assembly and save. Eventually, you will have changed the name of and saved every file you needed to save because of name changes.

If you have no PDM, how do you know what parts are related to what assy's and what assy's are related to what drawings? If you are on Windows 98 or greater, use the windows search utility to search for text within files. As far as I know, all PTC part/assy/dwg files have header information with part/assy/dwg names as text before the binary information. If I knew I had a part named CON_ROD, I would use the search facility of Windows to find the text CON_ROD in my Parts/Sub-Folders folder. Wherever CON_ROD was used, an assy or dwg, it would show in my search. I would then use the search facility to search for the part(s), assembly(s) and dwg(s) needing renamed.

If I need to copy a part/assy/dwg, I would bring the necessary parts/assy's/dwg's into session and use File>Rename In Session, save the parts/assy's/dwg's in succession. Same old Save/Close scenario. You can also rename Family Table Instances by using File>Rename or just edit the Family Table and change the names.

Don't forget to Erase when done :)