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!
So long as you pay attention to trace impedance, signal return paths, and all of the other usual signal integrity things then you can really do anything with the stackup. Of course, some stackups make it easier to do...
I have done several PCIe designs and what I do is this:
- Signal
- Ground Plane
- Signal
- Signal
- Power Plane
- Signal
The spacing between all layers, except between 3-4, is small. Maybe 3 to 10 mils (not mm). The reason for this is to give the signal layers a low trace impedance with respect to the planes. This also means that the space between layers 3 and 4 is large-- large enough to make your total PCB thickness correct. You will have to do the math to figure out what exactly works for you-- balancing trace width with trace impedance and stackup height.
Best Answer
There is no requirement to use GND and PWR for the internal layers. That seems to be a commonly repeated recommendation, but isn't necessary.
Most of the 4-layer PCBs I tend to make have both inner layers as ground planes to allow high-frequency routing on the outer layers, and then when not required to form an unbroken plane, get chopped up to use for power and signal routing as required. You can also route ground and power on outer layers too.
Basically, you can use all layers as required, don't feel that you can only use one layer for just power, or just signals.
I see a suggestion for using one layer for horizontal and one layer for vertical traces, however this is again a case of "that was then, this is now". Its a useful starting point for simple boards, however when you start using predominantly surface mount components, and throw into the mix high speed signals or fast edges, the concept rapidly falls apart.
My approach is as follows:
I also tend to route from both ends - with the components grouped together like little cities, you can route traces within each city as needed, and try to escape signals which share a common destination out of each city like little highways. These can then be connected up afterwards.
The thing to bare in mind is this is an iterative process. Keep looking at the whole picture to see how each chunk of the board is likely to connect up.
Don't be afraid to move traces and components as you go along. You might discover that if you rotate a chip or reorganise some of the blocks that the routing begins to untangle.