I wouldn't recommend creating a new version of the file. If you want to keep the previous revision I'd save as to an archive folder.
A 'revision' custom property in the assembly file will allow the assembly and the drawing to maintain a link by linking the revision note in the drawing by entering $PRPSHEET:"Revision"
There are two ways to do this:
If you are you trying to make a complete new copy of the assembly and all the parts. If so use Pack and Go, you can create a new working version or save what you have into a Zip file and keep working in the same locations. You can also use Pack and Go to just copy the assembly file and drawing if you want but it's going to be a little more work IMHO than the second method.
If you just want to a new copy of the assembly model and drawing without the part files the easiest is probably just open them both, save the drawing as the new name, and keep it open, then save the assembly as the new name. If you have the drawing open when you save the assembly it will update all of the links, I just recommend saving the drawing first so you don't accidentally save the assembly to the new name then save the drawing where it is. It's sort of working backwards from how everything was created, the last thing created is the first thing saved with a different name.
Thanks. This worked with both files open. FYI, I don't want to use pack and go since most of the parts in the assembly are from common folders of purchased parts that are used in multiple assemblies. Pack and Go breaks those links.
Like the correct answer says, the only way for you to rev your old drawing file up to the next level is to save it as a new file. Putting the rev letter or number in the file name of drawings is always a good idea. The assembly on the other hand, while it can be saved as a new file, it doesn't have to be, and some may find that this way is preferable. The assembly file can simply have a configuration added to it. Name that config the rev letter or number. After you've made the new config in your assembly and your new rev to your drawing file, click on views in your drawing file and change them to the appropriate config.
Additionally, you mentioned in your original post that you "can't find a way to change the assembly links on a drawing file". If you have SW 2014 or later this function exists. I don't have SW on this computer so I can't show you what the icon looks like but if you search the help or just look around, you will find it.