Splitting power planes on PCB
I second the advice to use a single ground plane.  It is very difficult to get a split ground plane correct. In most situations a continuous ground plane will perform just as well -- if designed properly.  Properly mostly means that digital signals and their return paths are kept separate from analog signals and their return paths.  One way to think about it is to design as if you were going to use a split ground plane: designate analog and digital regions, and traces are not allows to cross the boundary without heavy filtering, but then simply neglect to do the split.
Splitting power planes is a good idea, especially on a 4 layer board.  Try to arrange your PCB so that the various power rails can be nice contiguous regions.  Concentrate first on the highest frequency, highest current, lowest voltage rails -- for instance, CPU and FPGA core logic voltages.  Next, any power rail that supplies a large number of non-differential IOs.  These are the power supplies that need especially low inductance.  For less critical rails like opamp power supplies or low speed digital logic, you can just run traces for the power supply.
The other thing to keep in mind is that in a 4 layer stack like this signals on one side will be referenced to the power plane, not the ground plane.  This means a few things.  First, if you have noise on your power plane, signals referenced to it will see that noise.  Second, if you have a split your power plane as suggested any traces that cross the gap won't have a suitable return path.  If possible, avoid crossing breaks in the plane, but if you have to, use bypass capacitors.  A special case of this issue is that if you use a via to go from the top to the bottom layer your reference plane changes from ground to power.  Any signal vias like this need a bypass capacitor as close as possible.
In some cases, I have used a 4 layer PCB with both inner planes dedicated to ground, and run the power as traces.  This won't work for a lot of applications, but this was a low density analog board and it worked great.  I have also used a continuous ground + split power plane, but in one area placed a second ground on the power layer to accommodate ground referenced analog signals.
The advantage of having two ground planes is that when your signal goes through a via, the reference is ground on both sides.  You still need to provide a path for the return current, but it can be a via rather than a bypass capacitor.