New versions of files

Are you inadvertantly modifying the part file without changing the geometry? If you have a common layer name on the .asm file and .prt file and you change the layer status in the .asm, it will reflect that same change in the .prt. Thus modifying the .prt. Perhaps that is it?

Are the parts being modified of a certain type...like Family Tables? These are notorious for the "marked as modified but untouched" scenario.

The parts have been saved because the parts have been modified, even when you did not explicitly open and change them.

Changing layer status at the assembly level is a great way to change the display of layers in parts in an assembly, which changes the part level. Something typical is hiding datums and then saving status; every part in the assembly with the datums layer is now modified. You can avoid this by setting the status of only the assembly.

Family tabled parts are sometimes built incorrectly or were not verified, causing them to be updated when they are retrieved. For example, if mass is calculated, but not part of the table, this is a new calculation of those parts whenever they are retrieved. If the table is not verified, items that were added are new items and are seemingly new when retrieved.

It there are relations in the parts that refer to the assembly it can drive assembly changes into part changes.

If using a PDM system like PDMLink, I lock all the entries in the workspace and then unlock only the ones that I will explicitly change.

Thank you all. I'll need to look in the files, which are constantly saved and find some common patterns. As our database dates back to 2001 on PROE 2000 i2, and then we moved through PROE 2001, Wildfire 4.0 and Creo 2.0, could this migrating be a reason for the above?