4 layer board

RF network on layer 4 (BOTTOM LAYER)
Power trace on layer 1 (TOP LAYER)

Power trace outlined in white

also on a side note... How are my vias looking? The RF Vias and the general stitching Vias.

 

IF there is enough other layer circuitry to provide shielding then there should not be a problem. BUT is the RF signal high impedance or low impedance?? That often matters.

 

I strongly recommend not to route your digital power supply as a long, thin trace. It is the best to have a separate power layer with power planes. In your case I recommend the following stack up:

Layer 1: signals
Layer 2: power plane(s) (digital, RF-supply, 5V, 3.3V, whatever you need) as partial power planes
Layer 3: GND-plane
Layer 4: signals, esp. RF

Unless you have some constraints for your stack up concerning controlled impedances or so, I recommend to have a distance of 100 - 150 µm (4 - 6 mils?) between layer 2 and 3. This acts as a high-Q capacitor for your power supply which reduces spurious emissons at EMC tests. Long thin power supply traces may act as an antenna for those emissions. The can also cause inductive voltage drops or overshoots due to rapidly changing current requirements in digital circuits. (dV = L * dI/dt)

A power plane reduces these voltage drops due to the minimum possible inductance for the power supply.

A good GND-plane without holes and cutouts will deliver sufficient shielding between the RF part and the rest of your circuit.