in my experience having truly separate AGND and DGND nets almost never works out well in practice. 90% of the designs i see that try to do this end up with current loops that introduce EMI issues and can generate more noise in the analog portions of the circuit than using a single ground with careful part placement would.
Having two GND planes also creates a problem for routing in that signals referenced to a particular ground should only ever be run on layers that are adjacent to this plane or its associate power plane. This can result is a pretty funky stack up that can limit where you can run traces. Your best answer would be AGND,signal,?GND,POWER,signal,DGND but thats funky to layout, uses lots of vias, only gives 2 signal layers to route on.
What i would recommend is a single solid ground plane and careful part placement. High speed digital signals and noise will follow the path of least inductance to ground not the path of least resistance. The path of least inductance is the smallest loop area, for signals this is directly under the trace on the adjacent ground plane. In some cases a ground pour on top, bottom, or both can be helpful in reducing noise pick up as well. This is dependent on the components and the design layout.
Create virtual partitions, keep out areas, where you only run either analog or digital signals, keeping in mind that the return current path for the low frequency analog signals is the path of least resistance, while the return path for the high speed digital signals is the path of least inductance. As long as your careful to ensure that the return current paths don't cross, especially a digital return running under your analog sections. You shouldn't get much noise pick up at all.
If your have a particular device that is very sensitive to noise, such as a high resolution ADC, you can use a ground island to increase noise immunity, like this:
alt text http://www.hottconsultants.com/techtips/a-d%20gnd%20plane.gif
In cases where i have some sensitive analog circuitry i will usually also use a power island that is separated from the digital power supply by an LC filter of some sort, depending on the digital frequencies i'm wishing to block.
Best Answer
First, I would not waste whole layers for supplies, unless perhaps when they are unusually high current. With a good ground plane and good local bypassing, there is little purpose to power planes.
Second, I would use a single ground plane unless you are doing something unusual. If you want a capacitive shield, then you can dedicate the bottom layer to that, but it would be connected to ground at only one point near the middle of the board.
You can probably do your design with six layers. One of the two inner-most layers would be the ground plane, and then signals and power mixed everywhere else. I'd start with layer 3 being ground, layer 1 being the primary signal layer and layer 6 right behind it. I'd try to route as much of the power as possible in layer 4. Layers 2 and 5 are then left over for the router to use as it needs to make things work, although I'd set their costs higher so they only get used when needed.