Typically outer layer pours are a bad idea. Outer layers have lots of components and traces that tend to chop up the pour. Little islands of pours lead to EMI issues.
If you do a star topology for your +5V (branch from the supply rather than creating loops) with really thick traces (0.020" min) then you could possibly do away with a couple of pour layers. It will certainly reduce board costs. Depending on your supply usage, you might be better pouring the GND and delivering one of the 15V supplies via traces.
In the end you'll have to build a board to see if it meets EMI, and performance specs.
You will hate yourself if you do stack up number two ;) Maybe that's harsh but it's a going to be a PITA reworking a board with all internal signals. Don't be afraid of vias either.
Let's address some of your questions:
1.Signal layers are adjacent to ground planes.
Stop thinking about ground planes, and think more about reference planes. A signal running over a reference plane, whose voltage happens to be at VCC will still return over that reference plane. So the argument that somehow having your signal run over GND and not VCC is better is basically invalid.
2.Signal layers are tightly coupled (close) to their adjacent planes.
See number one I think the misunderstanding about only GND planes offering a return path leads to this misconception. What you want to do is keep your signals close to their reference planes, and at a constant correct impedance...
3.The ground planes can act as shields for the inner signal layers. (I think this requires stitching ??)
Yeah you could try to make a cage like this I guess, for your board you'll get better results keeping your trace to plane height as low as possible.
4.Multiple ground planes lower the ground (reference plane) impedance of the board and reduce the common-mode radiation. (don't really understand this one)
I think you've taken this to mean the more gnd planes I have the better, which is not really the case. This sounds like a broken rule of thumb to me.
My recommendation for your board based only on what you've told me is to do the following:
Signal Layer
(thin maybe 4-5mil FR4)
GND
(main FR-4 thickness, maybe 52 mil more or less depending on your final thickness)
VCC
(thin maybe 4-5mil FR4)
Signal Layer
Make sure you decouple properly.
Then if you really want to get into this go to amazon and buy either Dr Johnson's Highspeed digital design a handbook of black magic, or maybe Eric Bogatin's Signal and Power integrity Simplified. Read it love, live it :) Their websites have great information as well.
Good Luck!
Best Answer
Back in the days, pouring all layers was done in order to minimize the amount of copper etched during the PCB manufacturing process. The more homogeneous amount of copper across the PCB the better is the etching process.
Nowadays there is no point in pouring with copper all layers
Pouring outer layer doesn't improve the shielding and the impedance necessarily. These are critical points and they must be considered in a proper way.
In general, you don't need to pour outer layers.