Ground in PCB 4 layers
Your stackup is a poor choice in most cases.
Most 4 layer stackups are like
Top
thin insulator
Mid 1
Thick insulator
Mid 2
Thin insulator
Bottom.

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.