Welcome to MCAD Central

Join our MCAD Central community forums, the largest resource for MCAD (Mechanical Computer-Aided Design) professionals, including files, forums, jobs, articles, calendar, and more.

Register Log in

Renaming Manufacturing Files


New member
I have a parametric assembly of one of our standard products, that we manufacture in different sizes. We would like to preserve the manufacturing files when we create a new version of our assembly to save programming time. We have been loading all the files from the last assembly and renaming them to a new set offile names. The model is them modified slightly to size the assembly properly. The drawings are adjusted as necessary and the programmers adjust the existing manufacturing files rather than programming allthe parts from scratch.

This is time consuming and occassionally produces defects in the parametric links between parts and the assembly.

Is there a better way to this?


New member
Good Morning dmiller327,

How do you model your products? Do you create a family of parts or do you create each instance separately? If I remember correctly, you can do a REPLACE of the model to bring in the new part you want to create and then maybe do a SAVE AS??? I am not sure if this will work since I have not used ProMan in a while. I believe this will keep you associations and parametric parameters while giving you a way to rename all of the files at once. Good Luck!



New member
Thank you for your response Christopher,

The model has about 10 parts whose features are driven by each other. For example the assembly has one cylinder that fits inside another cylinder. There are two end caps that hold the cylinders together and seal the space between them. The clearance holes in the end plates are coaxial to the threaded holes in the ends of the cylinders. There are quite a few other features that are driven by part ods and other feature sizes.

I could be mistaken, but I don't think the assembly lends itself to family tables. The part and assembly relations would conflict with family table parameters. ...


I spent some time and built a family table for the top level assembly and parts. I added a new assembly instance which used new instances of each of the parts. Upon modifying a couple key dimensions the assembly regenerated to the new size but some of the part features did not update to new locations.

It seems that assembly level relations updated but part relation are still looking atthe part generic model rather than the part instance used in the assembly.

Any ideas how to fix this? Do I need to move all relations to the assembly level?


New member
The only way that I know of to maintain the parametrics between the models and the manufacturing files, is to create the new assembly and parts while in Pro manufacture.

I have done this a lot because we also machine several parts that are very similar.

While in manufacturing, do a "SAVE AS", and give it a new filename. When the dialog box comes up to rename the assemblies and/or models, give them the name of the new part that you want to machine. When all files are renamed, click done.

If you have your "config.pro" option set correctly, the drawings will be created automatically along with the new parts and models. Just open up the models, make your changes, and save. Open the new manufacturing file and generate the new cutter paths. DONE.
Edited by: appinmi