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!
What is the minimum clearance between this vcc via and inner ground plane ?
This depends on the drill registration capability of your vendor, plus a bit of margin.
A typical figure at a shop capable of 0.1/0.1 space/trace and 0.2 mm drills is 0.25-0.3 mm for clearance from the hole to the plane (assuming no pad on the inner layers).
Another common way to deal with it is just include pads on the inner layers, and let the 0.1 mm copper-to-copper clearance, plus the pad annular ring, set the hole-to-plane clearance. Your fab shop might then ask to remove the inner layer pads to reduce drill wear, which I've always allowed them to do without issues.
Best Answer
Your stackup is a poor choice in most cases.
Most 4 layer stackups are like
So your stackup places your signal traces far away from any reference plane.
The most common arrangement would be to use mid1 for ground and mid 2 for power, this means that all signal traces are close to a reference plane, but it has the downside that you can't just couple the two reference planes directly with a via, but instead they can only be coupled through a capacitor. This impacts signal integrity when a signal changes planes.
Another option would be to use both mid1 and mid2 for ground. This would allow better signal integrity on reference plane changes, but would mean your power would need to be routed on a signal layer.
It can make sense to swap the layers around, for example if you want EMI shielding on the bottom then you might put the ground on the bottom, ground or power on mid1 and signals on top and mid2 but you should generally always have one signal layer and one power/ground layer in each pair.