Question: I am designing a two layer PCB with high speed signals with rise and fall times as low as 3ns.

I was doing some studying and learned that for better signal intergrity and EMI a good grounding strategy is critial. To lower the effects of displacment current lowering crosstalk, routing a ground element along with each high speed tracks helps. May it be a ground plane underneath or ground track along side it.
(Do correct me if I am wrong with my understanding.)

Would it be a better strategy to have both layers as ground plane? A ground plane forces a return path next to most signals. Stitching vias make for even better return paths.

Is there any other benefits to having power and ground plane? I understand that this strategy has the advantage of creating decoupling capacitence.

EDIT:
What is meant by 2 ground planes, I actually meant Signal-Ground/Signal-Ground.
AND
What is meant by 1-power 1-ground planes, I actually meant Signal-Power/Signal-Ground.

Answer: 
If a 2 layer PCB is your only option: make the second layer ground and route your signals and power on the first. A proper ground/return plane is key for every signal and avoid sharing of the return path as much as possible. (A GND plane is preferable compared to a return trace)

High speed signals tend to follow underneath the signal trace, in the dielectric the energy will travel: between the two layers. Any obstacles will produce problems.

The higher the frequency, the more the return path of the signal will follow the signal trace:

[![enter image description here](https://i.stack.imgur.com/Vsny2.jpg)](https://i.stack.imgur.com/Vsny2.jpg)
Image source: <https://www.signalintegrityjournal.com/ext/resources/article-images-2020/A-Simple-Demonstration-of-Where-Return-Current-Flows/F1.jpg>

The nice thing of a 4-layer pcb is the distance between layer 1-2 and 3-4, very close. In a signal-gnd-gnd-signal configuration any inductance related to your traces will have less effect in 3D perspective compared to the much bigger distance between layer 2 and 3 and in case of a 2 layer pcb between both layers.

Inductance around traces, stopped by the gnd layers top/bottom:

[![enter image description here](https://i.stack.imgur.com/5KiST.jpg)](https://i.stack.imgur.com/5KiST.jpg)
Image source: <https://www.signalintegrityjournal.com/ext/resources/Blogs/2020/What-is-Differential-Impedance-and-Why-do-We-Care/F1.jpg>

Compare the distances between the layers:

4-layer:

[![enter image description here](https://i.stack.imgur.com/Q2lWz.png)](https://i.stack.imgur.com/Q2lWz.png)
Image source: <https://www.bitweenie.com/wp-content/uploads/2013/04/4LayerPCB_Stackup.png>

2-layer:

[![enter image description here](https://i.stack.imgur.com/apju1.png)](https://i.stack.imgur.com/apju1.png)
Image source: <https://manage.pcbgogo.com/img/js/ueditor/ueditor1.4.3.3/net/upload/image/20200114/6371460255595880006009080.png>

In that way I don’t believe in ground poured next to traces and pads; the effect is too small and a possible cause of trouble if not designed very carefully.
A 2-layer PCB will be insufficient for fast signals when the design is dense using recent tiny surface-mount chips.

On a 2-layer PCB, you won't have the luxury of having a power plane and a ground plane unless the design is rather simple.

The separation between the ground plane and signal traces on a 2-layer PCB is several times larger than you'll get on a 4-layer PCB, and this negatively affects signal integrity.

In your design, you'll likely need to use series termination resistors at least on the source end of signal traces, to keep the ringing to a minimum. This will require careful measurement on a prototype board, and optimizing the part values manually.

There's always a benefit to have two reference planes, i.e. a ground and one or more power planes, or even multiple ground planes in a multi-layer design. The general idea is to "short" the planes together at AC by distributing small coupling capacitors across the board. I call it "sprinking the board" with caps. Imagine you have a spice shaker and you've shaken some 0402 capacitors on the board. Those capacitors would go between the power and ground planes, independently of any decoupling caps next to the chips. These "sprinkles" will provide the distributed capacitance needed to make the power and ground planes equally good at routing return currents of fast signals.