I am designing motherboard for my preamplifier project and I want to setup PCB as follows:
What is the Eagle Design Rule Setup for such a board?
Obviously, a perfect analysis requires much more detail about your design than I have access to at the moment, but here are some general considerations.
I'm generally loathe to describe things as "analog" and "digital". Really, you should be classifying circuits by impedance and frequency (but that's a different topic).
The PCB is a 3D structure. If you want to minimize cross-talk, pick-up, and EMI, you need to minimize the current-paths' loop-area.
Allocating layers to functions as you have suggested results in much larger distances between the outgoing track (power-supply to load) and the return path (load to power-supply) as the return (should be) on the ground plane and that plane will be far from your signal layers.
You want to allocate functions laterally (same layer) and place that layer as close as possible to the ground plane as you can get it.
In virtually all of the "standardized" prototyping processes, the bulk of PCB thickness is in the core (the middle). So layers 1-2 and layers 3-4 are much closer together than 2-3.
Stop and think of what you are trying to accomplish with the four layers. Your list looks like something you found on the internet or something you dreamed up for religious reasons without really thinking about the science much.
You don't need whole layers for power supplies. What's the point as long as you observe proper bypassing at each place the power is used? A few mΩ of resistance between a part and the power supply is pretty much irrelevant, as long as that part is properly bypassed.
I'd probably dedicate layer 2 to be a pervasive ground plane. This is the master ground for analog and digital, except that it would be good to tie all the digital grounds together as a separate net, with each chip bypassed locally, then the digital ground connected to the main ground in one place. That will keep the high frequency digital ground currents off the main ground plane. Group the digital parts together, and this digtial ground net needn't be large, and shouldn't need its own plane. At worst, make it a polygon on layer 3 just under the digital section. However, if any of the digital chips are dense, you'll need three layers for the signals and still probably wish you had more.
Use the top layer for the immediate local interconnects as much as possible. The signals all start and end on the top layer anyway since that's where the pads are, so connect them there as much as you can. All analog ground pins get punched down to the ground layer immediately, which gives you more flexibility in routing signals on layer 1. Since all these signals are immediately above the ground plane with only the parts themselves above, this is the best place for sensitive signals.
Use layer 3 as the secondary signal layer, and layer 4 perferentially for traces that carry significant current.
You definitely don't want to start out boxing youself into a corner with heavyweight and arbitrary rules dedicating most of your planes before you start routing.
See this answer for more detail about a 4-layer stackup, and this answer goes into a lot more detail about local ground nets and proper bypassing.
