Is it normal for a big drawing to freeze up every time I hit save?

I manage a few 30 to 40 sheet drawings for work and yeah, the model running fine while the drawing chokes is exactly how it plays out. The drawing file has to rebuild and re-evaluate every view on every save, and shaded or detailed views are way more expensive than wireframe ones. Your coworker is half right that it gets slow at this size, but 20 minutes per save is not just the price of admission, there's stuff you can do.

First thing I'd check is wheather your views are shaded with edges. That's the single biggest killer. Switch everything you can to hidden lines removed or hidden lines visible instead of shaded, and drop the edge display quality in the document properties. On a drawing this big those two changes alone ussually cut save time massively.

Second, look into detached drawings. When you save, there's an option to detach the drawing from the models, and from then on the drawing doesn't need to load the whole assembly to open or save. You have to reattach manually if you change the model and want the views to update, but for a monster file like yours it's a huge difference. Detailing mode is also worth knowing about, it lets you open the drawing without loading the models at all so you can add dimensions and notes while the file's in that state. Also check that you're not on automatic rebuild during editing, and turn off any backup or auto-recover settings while you're actively working, since those trigger extra saves of the whole file.

On splitting it up, honestly I'd still consider it long term. I break mine into one drawing per major subassembly, maybe 8 to 12 sheets each, and they save in seconds. You don't have to rebuild views either, you can just drag existing sheets between drawing files in the feature tree, or cut and paste views. It's less painful than it sounds, and the day your coworker's theory gets tested by a crashed save, you'll be glad you did it.

One thing I'd throw in: check where the file's actually living. I had a drawing that took forever to save and it turned out I was working straight off a network drive. Copied it to my local disk, saved in like 30 seconds, then moved it back over when I was done. Made a bigger difference than anything else I tried.

Also curious what the file size is on disk. If it's bloated way beyond what 40 sheets should be, there might be junk in there that never got cleaned out.

The local copy thing is huge, I second that. I used to work off a shared drive and every save felt like the file was being uploaded from scratch each time. Now I keep the drawing and all its references in a folder on my desktop while I'm actively in it, then copy the whole folder back to the server at the end of the day. Went from saves taking forever to saves taking about as long as a coffee sip. Only headache is remembering which copy is newest if I touch it from two machines, so I rename with the date before copying back.

Gotta push back on the dragging sheets between drawing files part. I tried that exact move last year on a set of assembly sheets and it went sideways fast. The views move over, sure, but my section views came across without thier parents and the detail views just showed error marks. Had to re-anchor half of them anyway. Maybe it works better if the views are simple, but anything with cut views or broken views is basially a rebuild with extra steps. Worth testing on one sheet before trusting it with 40.

One thing that fixed a similar slog for me was the antivirus doing a full scan every single time the file got touched. Opened task manager while a save was running, watched the scanner eating the CPU, and asked IT to exclude our CAD folders. Saves dropped from ages to under a minute. Worth ruling out before you go chopping the drawing up, expecially if the company has aggressive security software.