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!
Unless there is a compelling reason otherwise, I use the same ground everywhere.
You have not stated just what digital circuitry is used, but if it is modern it will very likely be fast. The way to make sure analogue and digital parts do not interfere with each other is by shaping the plane layers. This shaping applies just as much to the power rails as ground.
If you have sensitive analogue circuitry, then make the plane such that there is no current return path from that point except by going back under the digital section.
Single Point Ground by Dr. Howard Johnson is an excellent article on planning the planes.
The point of the exercise is to make the return currents flow where you want them to go, not where they would go if otherwise uncontrolled. Remember that current flows in a loop[note]; control where that loop goes.
If you have a mixed signal part (such as an ADC), using separate planes tied together somewhere relatively remote is asking for trouble. You can find another great article ADC Grounding on this subject by the same author.
At the switch mode converters, follow the guidance from the datasheet (or better yet, the layout of an evaluation kit if one is available). Some manufacturers are better than others for this. As an example, see page 19 of this LTC3630 Step-Down Converter Datasheet for guidance, or the design files for its demonstrator circuit.
[note] I am not trying to insult anyone here - this seems to get forgotten but is the critical factor in successful plane layout.
Also, regarding separate planes:
There are some instances where separate planes with a star point are appropriate. One of my designs had three high brightness LEDs, each with their own power source. The noise in each of these was sufficiently high that I used a separate ground for each and tied them together at the power inlet to the main board.
The noise was insufficient to trouble the control logic, but would have induced very noisy crosstalk across the LEDs without a great deal of trouble and effort in the layout with a single plane; in this case. separate grounds made sense.
Some guidance on shaping planes:
Make the ground follow this logical path:
Power Converter <<<< Digital <<<< Analogue
For the power, if you are powering both digital and analogue from a single power rail, then I would normally do this:
Power converter >>> Digital >> Ferrite Bead and Decoupling >>> Analogue
Here is how I achieved the plane shaping on a video recorder:
The return current can only flow back in the direction of the arrow, and the digital return has no path back to the power source through the analogue area, so no digital currents flow in the analogue area.
Note how I have cut judicious voids in the ground plane to force the current to flow where I want it to flow.
Best Answer
At connectors narrow traces are used to connect terminals to the planes to allow wave or hand soldering to heat the joint sufficiently, if oven reflow soldering is used instead these thermal releifs are not needed. as the thermal releifs are symmetrical they do not have a dipole moment and thus do not radiate significantly.
There's nothing that two ground planes can do that one ground plane and one correctly bypassed power plane cannot do better.
if you need to split the power plane into regions for different voltages that can work well too.