Electronic – Power origin and power planes placement on PCB

The layout you showed looks like what's called copper-backed coplanar waveguide (CBCPW). That means the ground return for the waveguide is not just in the coplanar grounds (the ground fills on the same layer as the signal traces) but also in the plane layer immediately "below" the signal layer. This structure is fairly esoteric, in the sense that I've only seen it used in digital systems when data rates exceed 20 Gb/s.

I found what looks like a reasonable discussion on the differences between CBCPW and microstrip in a Microwave Journal article by Rogers Corp engineers.

This article shows that the CBCPW has lower loss than microstrip at frequencies where radiation loss becomes important in the microstrip, roughly from 25 GHz and up, which explains why CBCPW is not widely used at lower frequencies.

Addressing your question, the article points out some special requirements for grounding vias in CBCPW structures:

For proper grounding, CBCPW circuits employ vias to connect the top-layer coplanar ground planes and the bottom-layer ground plane. The placement of these vias can be critical for achieving the desired impedance and loss characteristics, as well as for suppressing parasitic wave modes.

This basically means that without frequent stitching vias between the coplanar ground and the backing ground, power could be transferred to undesired propagation modes, which would cause either excess insertion loss or strong dispersion in the transmission line characteristics.

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.