This set of articles has been referenced a number of times on this site and it's quite a good primer. Read through it and decide which goals you are content to optimize for.
http://www.hottconsultants.com/techtips/pcb-stack-up-1.html
http://www.hottconsultants.com/techtips/pcb-stack-up-2.html
http://www.hottconsultants.com/techtips/pcb-stack-up-3.html
... read on for more layers.
Here is an excerpt of the objectives of stackup design:
When using multi-layer boards there are five objectives that you
should try to achieve. They are:
- A signal layer should always be adjacent to a plane.
- Signal layers should be tightly coupled (close) to their adjacent planes.
- Power and Ground planes should be closely coupled together.
- High-speed signals should be routed on buried layers located between planes. In this way the planes can act as shields and contain
the radiation from the high-speed traces.
- Multiple ground planes are very advantageous, since they will lower the ground (reference plane) impedance of the board and reduce the
common-mode radiation..
If you read through the articles, you'll find that there is no one "best" way to stack up your design. There are just a number of possibilities with different characteristics and tradeoffs.
This split up arrangement would help from noise traveling between the modules?
If you have multiple power voltages and a 4-layer board you don't have much choice. You have to deliver different voltages to the different loads. Whether it reduces or increases noise has a lot to do with the details of how you lay it out, it's not possible to just give a blanket answer to this question. Better to look at it as, you have to split your power plane --- what's the best way to do that?
Would pouring up ground copper in the top and bottom sides help reduce EMI noise external to the board?
It can, if you provide multiple vias to connect the outer layer ground area to the ground plane. It will also make your fab vendor happy because it will reduce the amount of copper they have to etch to make your board.
Be careful of bringing the outer-layer ground too close to your 2.4 GHz traces because if it's closer than, say, 5 tracewidths it will change the characteristic impedance of your controlled-impedance line.
Would be better to also split up the ground plane (and NO ground pouring on top and bottom sides to avoid a loop), and connect it in a star fashion? I heard that is better to keep the ground plane whole, but everyone seems to have his own version.
Short answer: no.
If you pay special attention to how you split up the power plane, and if your circuit demands it, then there are cases where it can improve things.
But if you want a single answer from somebody who knows almost nothing about the circuit you're designing, then the best answer is not to split the ground plane.
One more thing to watch for
Your stack up is signal-ground-power-signal. With splits in the power plane.
When you route on the bottom layer, try not to cross the splits in the power plane, because those bottom layer traces will actually be using the power net, not ground, as the return path for high-frequency components of the signal.
Also, be careful of (high-speed) signals jumping from top to bottom layer, because this will also require a transition of the return current from the power net to the ground net. This return current will probably pass through the nearest decoupling capacitor --- so the second best thing is to put a decoupling capacitor near each place where return current needs to cross between planes. (Best thing is not cross between planes at all).
Edit
I am making sure all the HF signals don't cross splits, but there are a few DC tracks which unavoidably cross them. Can that be a problem?
Think about this: when you say it's a dc track, do you mean the voltage doesn't change or the current doesn't change? Current changes are what causes problems with running over a split. (Voltage changes are problem only because they usually cause current changes)
So it depends if you're talking about a "dc" signal like an enable line for a power supply that's turned on once at start-up and then left at the same voltage forever, or a power track for some extra rail that wasn't worth making a split for.
A DC control signal will be no problem.
If it's a power signal with a varying load current, you can fix the problem with decoupling capacitors. A decoupling capacitor allows the high-frequency changes of the current to come through the short path through the capacitor instead of the long path through the track.
Best Answer
I second the advice to use a single ground plane. It is very difficult to get a split ground plane correct. In most situations a continuous ground plane will perform just as well -- if designed properly. Properly mostly means that digital signals and their return paths are kept separate from analog signals and their return paths. One way to think about it is to design as if you were going to use a split ground plane: designate analog and digital regions, and traces are not allows to cross the boundary without heavy filtering, but then simply neglect to do the split.
Splitting power planes is a good idea, especially on a 4 layer board. Try to arrange your PCB so that the various power rails can be nice contiguous regions. Concentrate first on the highest frequency, highest current, lowest voltage rails -- for instance, CPU and FPGA core logic voltages. Next, any power rail that supplies a large number of non-differential IOs. These are the power supplies that need especially low inductance. For less critical rails like opamp power supplies or low speed digital logic, you can just run traces for the power supply.
The other thing to keep in mind is that in a 4 layer stack like this signals on one side will be referenced to the power plane, not the ground plane. This means a few things. First, if you have noise on your power plane, signals referenced to it will see that noise. Second, if you have a split your power plane as suggested any traces that cross the gap won't have a suitable return path. If possible, avoid crossing breaks in the plane, but if you have to, use bypass capacitors. A special case of this issue is that if you use a via to go from the top to the bottom layer your reference plane changes from ground to power. Any signal vias like this need a bypass capacitor as close as possible.
In some cases, I have used a 4 layer PCB with both inner planes dedicated to ground, and run the power as traces. This won't work for a lot of applications, but this was a low density analog board and it worked great. I have also used a continuous ground + split power plane, but in one area placed a second ground on the power layer to accommodate ground referenced analog signals.
The advantage of having two ground planes is that when your signal goes through a via, the reference is ground on both sides. You still need to provide a path for the return current, but it can be a via rather than a bypass capacitor.