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!
In high frequency microstrip components, the "cavity" (that is, the area to the side of and above the trace) can lead to a lot of radiation in certain circumstances. The ground to the side of the trace can act as a "wall" and help mitigate the radiation (especially in situations where you may want to solder a cover over a sensitive area of the circuit. You can pour ground on the top/bottom with provisions for later soldering on a shield.)
As for the impedance matching, it shouldn't really impact the signal circuit if the pour is more that 2 to 3 times the tracewidth away from the signal trace.
And, a bit of an anecdote, but I've found that the top/bottom pour helps make the copper distribution a bit more symmetrical about the middle layer which helps with flexing over a large operating temperature range (even though the risk of bending at assembly is increased, as you pointed out).
Best Answer
Adding copper between signals to reduce crosstalk only works if the copper is effectively grounded at the frequency of interest. For audio, it can potentially help. But for high speed clocks, it will likely make the crosstalk worse since the fill copper has high impedance to GND (relatively speaking).
To reduce crosstalk, focus on leaving lots of space around the potential aggressor signals such as clocks. The worst thing you can do is route them along side each other or directly over/under without a ground plane between.
Think of it this way. Two traces next to each other act as terminals of a capacitor. The gap between them is the dielectric. A wider gap means less capacitance, and therefore less crosstalk. Adding copper to the gap has the same effect as using a thinner gap (more crosstalk), unless that copper is grounded well. And at high frequencies, it is just not possible to ground that copper well.
So there may be good reasons to flood the outer layers with GND copper. It is often done. But adding copper between aggressor and victim signals will probably not reduce crosstalk. Use a large gap instead.