Electronic – Should vias be used for every GND connection

I'm not sure that I know the best way to build the board, but I know what I would do.

1. The location of the 12V-to-5V regulator, whether linear or switching, will not matter. The corner of the board is fine.
2. I would not bother with filling either top or bottom of the board with ground planes. The impedance of the signal traces is defined by the internal planes, not the extra copper you pour on the outside. The extra coper isn't shielding internal signals, all that is underneath are power and ground planes. Instead, connect ground and power pins of components directly, as close as possible to the pin, to the planes.
3. Don't share power and ground vias between different devices. One via per pin minimises noise on the pin and routing distance to the ground plane. If you are so worried about the manufacturing price that a few vias are going to be significant, you must be shipping in very high volume, so you can prototype a dozen different layouts to optimise it. If this is a one-off, the biggest cost risk is that you don't get it right first time, so be conservative and use lots of vias.
4. Put a via by every component ground pin (not necessarily every component signal pin that happens to need routing to ground). Minimum noise on power and ground planes comes from effective decoupling. High frequency noise is minimised by using physically small ceramic capacitors and keeping the power and ground vias close together - underneath the capacitor, if possible. The cross sectional area of the loop from power plane up through via to capacitor, along capacitor and down through via to ground plane, places the lower limit on how effective the decoupling is.
5. I would definitely not put any splits in the ground plane. Instead, if there are analog signals sensitive to noise, I would not route digital signals close to them. I would try and keep those sensitive analog signals just on the top layer if possible, no vias to the bottom at all. If I can isolate an area of sensitive connections all together on the top layer, I would route a single loop of trace all round there on the top layer, and connect that loop at one point with a via to the ground plane. That approach has worked well for me in the past with very sensitive signals.

And finally: it is conceivable that some clever technique of sharing ground connections might help noise in the analog wiring, but you'd need to know the exact circuit and think very hard about it to be confident. These rules of thumb have worked pretty well for me.

Good Luck!

It will probably be fine in your case to via down to the bottom layer and have a small slot in the ground plane. If you were running higher speed signals it could become a problem.

The issue to generally be concerned about with cutting a slot in the ground plane is that return currents will need to go around the slot, which can then act as an antenna and be an EMC problem. Return currents are concentrated on the paths of lowest impedance. For low frequencies, this is the path of lowest resistance. For high frequencies, inductance starts to dominate the impedance, so the return currents will flow in the direction that minimizes the loop area. This means that they will be concentrated directly underneath the signal trace until they reach the slot, then flow around to get back to the signal trace again. This will cause radiated energy and distort nearby signals (or farther nodes if they are high-impedance). With lower frequencies, the return currents will not even care to get close to the slot, though, instead making a diamond shape of lower current density centered on the slot.

That being said, 2-4 MHz is so slow I wouldn't worry about it. If you're running at 500+ MHz with fast edge rates, though, slots in the ground plane should be avoided, especially underneath high speed data lines.