Power traces through GND layers:
Bad idea. This is the same problem as splitting GND planes, just the difference is that the voltages are not the same. From a signal integrity perspective the problem is the same - where do the displacement currents flow for the signals adjacent to the split plane? If they cross from travelling next to GND and cross the split so they are now travelling next to VCC, the displacement current cannot follow, so the energy spreads out sideways and you get EMC issues. Also for the signal crossing the split, it will see an impedance discontinuity and you’ll get reflections. The only way you can make this work is if there are no signals that cross the split in the plane.
Low frequency signal layers dedicated to GND:
If by this what is meant is that a signal layer is converted to be a plane layer carrying GND, the obvious concern is matching this elsewhere in the stack-up. For example, on an 8-layer board where layer 6 is a signal layer, then by symmetry, so is layer 3. If you turn layer 6 into a plane (GND or otherwise), you also need to turn layer 3 into a plane layer. Failure to do this results in a mismatch of the amounts of copper in the board. The consequence of that is seen when you put the board through the manufacturing process and the mismatch creates an imbalance in tensions within the PCB that result in it coming off the line bent like a banana.
Solid planes versus Routed power:
Routed power is a very useful approach if the currents are not likely to cause a significant rise in the trace temperatures. There are tools that will tell you the temperature rise for a given trace geometry per unit length. Note that this is always worst for traces on the outer layers because the PCB insulating materials (mostly glass and resin) are a better thermal conductor than air. So if it works for an outer layer, having the same trace width and thickness on an inner layer will always work better. To get the best out of routed power, maximise the space around the power traces and when you’ve finished routing the board, you can apply a pour over the power tracks to make them much thicker. Some PCB tools have the ability to automatically remove tracks that it thinks you have duplicated, so make sure that this is turned off when you route the power traces since you are trying to crete a mesh.
If you are routing high current power traces, remember that there will be an IR based voltage drop, so the voltage at the device may be lower than you think. This approach means your choice and positioning of decoupling capacitors around a device become more significant because you will not have the buried capacitance of the power plane - GND plane coupling that would give you the best capacitance present on (or rather “in”) your board.
Done properly, routed power can be very nearly as good as a plane, but if it saves you two more layers on your board, it’s money in the bank.
When it comes to which power signals are best distributed as planes and which as traces, to say highest current are planes and lowest current are traces is a good starting point. But it is more a matter of what will the voltage look like at the device as the current demand changes? In the end, do the maths and see whether you can make it work using routed power. If it just doesn’t work, you know that supply must be a plane. Don’t forget, you can specify thicker copper for planes and/or signals layers, but at the same time remember that thicker copper may mean that the trace and gap rules for those layers are different.