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.
That's the Cypress FX2LP USB microcontroller (I recognize it because I use it myself). If you're using the Hi-Speed USB transceiver, then you should really go with a 4-layer board. Without that ground plane right below the top layer, it will be near impossible to get the 90 ohm differential impedance that you want for the USB D+/D- lines.
http://www.cypress.com/?id=4&rID=34128 flat out states that 4 layers is required. It also states that controlled impedance is required, but in my experience you can usually get away without it, so long as you carefully research your fab's typical stack-up and work out the right width, space, and height.
http://www.cypress.com/?docID=25406 also provides more info on calculating the width, space, and height for the D+ and D- lines.
4-layers isn't that much more expensive; Advanced Circuits has a 66 each deal for 4 layer boards that I use quite often for projects that use that very chip, as opposed to the 33 each deal for 2 layers.
In regards to your actual question...use plenty of bypass caps, as close to the pins as possible. If you split the bottom layer to have VCC and GND, don't have a trace cross the split on the top layer. Keep all high-speed signals on the top layer because the via inductance can kill what fragile signal integrity a 2-layer board has.
Best Answer
Ah the horror of trying to make DDR work in two layers :) The long answer is of course to learn about signal integrity and try to understand exactly what you are doing. I have seen this done before, and even pass EMI but with many caveats. First there was only a single DDR part. Second the controller was carefully designed to route out onto all signals in the first two rows of widely spaced balls such that all signals routed with no vias on the top layer to the DDR part. Then the bottom was used for a GND plane, even though it was 60 mils away. Routes were matched, but kept "extremely" short. Finally the part was run as slow as possible, basically the minimum frequency allowed by the DDR part. Oh and we had a spread spectrum clock for EMI.
I would say as a general rule that this is not a good idea and you should stick to four layers and cut cost elsewhere. If you are going to do it don't even expect to get to near full speed, and if you're trying to route multiple parts like a DIMM or clamshell. I would say it's not even worth trying.
Cost depends on so many factors from where you're doing it to how much, it's a much smaller issue at very high volumes than it is at low proto volumes. The headaches you will face trying to debug a two layer design are almost surely never worth it. The increased time to market you will face trying to get it to work is alone worth the cost of a 4 layer in many cases.
You mention volume of 100 like it is high, but it is not at all once you start moving into the thousands, hundreds of thousands there's a steep drop in price from a few hundred pieces. Same if you move off shore somewhere. Just as an example I can think of my US price on 10K units of a 10 layer board is around $50, but my offshore of the same is $25. Your price will also depend on how efficiently you use the panel ( your pcb house makes boards in standard sheet sizes.) If you only fit two per panel and have a lot of waste your cost will go up just as if you only order 2 and leave room for 20 on the panel. Incidentally that's how places that pool together pcb orders work.
Why does it cost more? Well it's a lot ore work, involves double the material and requires a bit more precision or skill. A two layer is just a piece of FR4 copper clad on both sides, just drill some holes, mask, etch away and post process. For a four layer board mask and etch the two layer, then laminate two more outer layers on either side mask and etch again being very careful that they line up properly, then drill and post process. That's just an example but the point is the process has more steps, more labor, more material and more cost.
It might be worth mentioning that there are chips for the mobile industry that take things like LPDDR4 mounted directly on top of them for an all in one solution. Still I would want a four layer board for proper power distribution, decoupling, and routing of other signals but it's an interrsting angle to consider.