PCB Design Power Plane Question
The ground plane is most important, as you recognized.  Not only does it allow the shortest return path, but the lowest impedance, and it also creates minimal loop current which reduces EMI.

The next most important is often the power plane(s).  Usually, once you go to 4-layers, and assign two of them as ground and power, it frees up a lot of routing on the top and bottom layers that you don't need to use the middle planes for routing.  But if it gets tight, yes you can use the power plane for routing some traces.  Often you will have circuits with multiple power rails, and in that case usually the power plane is split into different domains, e.g. the MCU may sit on a section of the board where the power plane is at 3.3V, where other parts of the board are at 12V for I/O.

If the density of the board increases to the point that you find you need more internal layer routing, it might be advisable to go to 6 or more layers.  

Again, for most low to medium density boards, having two layers just for routing is usually enough, if your routing strategy is sound.  So if you feel you need additional layers and you aren't packing 0402 or smaller parts close together, then maybe there are better ways to route the traces.  If you do want to put some routing on the power plane (and you can also use the ground plane but I would try to avoid that), just be careful that you aren't cutting of or overly-restricting current paths.

And finally, yes, you could just use one ground plane and three routing layers, if you feel you need more routing area but not enough to justify 6-layers.  So you would just route the power traces as you would normally on a 2-layer board.  Or you could route your signals, then do a copper pour of the power rails in the remaining area.  Remember again to check the current paths.  Usually you route the power traces anyway to be sure you can get sufficient trace widths through everywhere, and maybe do a DRC, then pour the remainder.

EDIT:  Further explanation of the return path.
Current will return along the path of lowest impedance.  In DC or low-frequency circuits, impedance is essentially just the resistance, so current follows the path back with the lowest resistance.  This is usually a ground trace or ground plane.  Current doesn't jump through the air to return on a power trace just because it's closer.

However, when dealing with higher frequencies, impedance is more than just resistance, it includes inductance and capacitance.  Now, the capacitance of a trace will be influenced by a nearby power plane.

If you want to calculate characteristic impedance for example of a 4-layer board with internal ground and power planes, the calculation considers the closest 'reference' plane, which could be either.  So if it is a symmetrical stack up (with equal height from top to first plane as from bottom to second plane), then the impedance of a given track would be the same.  But this assumes the tracks are carrying high-frequency signals, such as USB, Ethernet, etc.

This is where perhaps the confusion in what you have heard or read comes from.  It's sometimes difficult to expand basic electrical theory from the Ohm and Kirchhoff laws, to high-frequency AC circuits, from the DC or time domain, to the frequency domain.