PCB Design: When having a power plane, should I only be doing vias or also route?
Usually if there is a plane, I would not route a redundant trace in addition to the plane in normal circumstances.
There ARE cases where it might be done. I don't want to confuse you. So if the following doesn't make sense just ignore it. Your example does not seem to warrant redundant traces.
Sometimes you may route a ground trace from a current shunt (along with the signal from the other side of the shunt) to a current sense amplifier rather than use the ground plane. This is because the signal from the current shunt is very low amplitude, and the amplifier gain will amplify any voltage noise that couples in. So you route from the shunt to the amplifier almost like a differential pair.
If you have very large currents, it may be advantageous to route them on multiple layers from point to point to lower the resistance. But in this case you would use a very wide trace or a fill with many vias. This would be the kind of thing you might see when you get to multiple Amps as opposed to 1 Amp and below.
Sometimes in switching power supplies, there may be a ground fill on a signal layer where the input and output capacitors are tied. This is an effort to keep high switching currents off of the actual ground plane. This fill will still be tied to ground with vias. But the hope is to avoid creating voltage gradients on the actual ground plane as current sloshes back and forth between input and output capacitors. The fill is kind of like an express lane for the high currents. The normal digital or analog currents flow on the ground plane, unbothered by the switcher currents.
That is all I can think of at the moment.