"High speed" return currents will follow the path of least impedance. "Low speed" return currents will follow the path of least resistance. This means that high speed signals tend to return on the return path that is closest to the signal path. In other words, if you had an S shaped signal above a ground plane, the return current for a high speed signal would follow an "S" shape whereas the return current for a low speed signal would be a straight line.
There's a really good note about this here:
High Speed Layout Techniques
(in some sources I read that return current will split between layers based on their distance from routing layer)
So, if you have a signal on SO2, its high speed currents will return on GND1 because it is closest - and in fact, the really high speed currents will only be on the surface of GND1 that is closest to SO2. If you have a signal on SO3, its high speed currents will return on GND2 - but its low speed currents may return on GND1 or be split between GND1 and GND2, etc. To be honest, I'm not quite sure what qualifies as "low speed" versus "high speed" - maybe someone else can answer that. There are a lot of equations that would
whether high speed return current will couple into signal layer also equally as like in surrounding GND plane.
Your gnd currents will not "return" through your signal layers unless they are bypassed to gnd for some reason like power pours (which makes them high frequency gnds).
One more...I read return current can couple any PCB trace (may be like cross talk).
To avoid crosstalk and signals coupling between routing layers, make sure that you rout adjacent layers perpendicular to eachother. Avoid having traces run "on top of eachother" as much as possible.
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.
Best Answer
As long as GND and VCC are connected by several capacitors at both sending and receiving end of signal lines (as they should be, will be in high speed design), AND where the return current changes planes (which you should try to avoid) then it doesn't matter which plane the return current flows in. The return current is only interested in the AC impedance of the path.
Note that signals carried in layers 3 and 4 will be referenced to both return planes. You have the opportunity to choose core and pre-preg thicknesses so that the same widths on all layers could give you the same impedance, but if not, use different widths on 3 and 4 (which are offset stripline) to 1 and 6 (which are microstrip).