Electronic – Power planes in PCB

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!

An advantage of a local power plane is that you can leave all the power routing out of your signal layers and in stead focus on the coupling, routing and impedance control of your signals.

Other than that the best advice is always based on your complete and exact design, so I'll tell you some of my preferences and their reasons, and leave them for you to consider.

For reasons of know-variables I prefer to keep no other layers between the GND and important signals, so in complex designs I try to make as many Signal layers directly next to a ground that fits my stack-budget (of course I'm not spending the money for 16 layers on each design I make!). And if I can only get 1 reliable layer like that, I make sure that layer has only signals and hosts at least the signals that are most important or highest frequency.

For the distances of the stack-up you best call the fab you are having the PCB made at, they know what they can do and what they stock. Once you have those numbers you can use them for your impedance control if you need to.

They can also tell you how accurate their PrePreg procedure is. If it's not very accurate or the layer it is spread on has a lot of copper areas and a lot of gaps as well (this makes PrePreg harder to get uniform) sometimes you will want your Signal and GND on either side of a normal plate, to be able to perform good impedance control. If that is a demand you might want to go for your first choice, but swap the "SIG" and "Sig/Pwr/Gnd" layers.

Another thing you put in your title is Analogue, if you have high-fidelity requirements of analogue signals you are not going to regret splitting your Analogue and Digital power domains completely, including the ground planes and only connecting them at the power-input of your board. You'll be thanking yourself for the extra effort once you find you measure very little digital noise in your analogue signals.