PCB Design - Do I need a power plane, if only one component uses the power rail?
If the chip has a lot of power pins, then a power &quot;island&quot; under it, with decoupling caps, makes sense.
However if it has only one power pin, then it doesn't make sense.
You say &quot;RF&quot; so I assume the inductance of the path between the power pin to the nearest decoupling cap is going to matter. In this case, from the pin, one via down to layer3, then another via (or maybe the same via) to a cap, then vias from the other side of the cap to ground... all this will probably have more inductance than a small decoupling capacitor placed right next to the power (and ground!) pins on the same layer as the chip. If the cap is right against power and ground pins, loop area is minimum, which is good.
Especially since on your 4 layer board, decoupling caps on top layer have the ground plane just below, so the inductance of their ground vias is lower than the ground vias of decoupling caps on the other side of the board, which have to go through almost all the board to connect to the ground plane. If the chip has power and ground pins next to each other, that's the way.
Note you can also use a feedthrough cap as decoupling cap. For example NFM21PS106 from Murata. In this case it does triple duty: decoupling, prevents HF from the chip from getting into the supply, prevents noise from the supply from getting into the chip.