How should I separate the DGND and AGND?
You are asking two separate questions here

Can I place passive components on the 4th layer and can I put the crystal there as well?


This will depend on your production capabilities as some build houses are not equipped to handle it.  But, assuming the facility you use can.  There are several advantages to having components on both sides of the PCB.  It saves space and can allow you to place decoupling nearer to where you want it.
Typically I place a mixture of Surface mount components on the top of the board then flow solder, Next I place Surface mount components (SMT) on the bottom of the board glued in place.  I try to limit these to 0805 size and larger and place them such that they are 90 degrees to the direction of travel over the wave to minimize soldering problems.  Finally I place conventional pin through hole (PTH non-SMT) components on the top side of the board.  The top side PTH and the bottom side SMT get soldered together at flow solder.


Secondly you asked about Ground and power planes.


Except in special circumstances we are not usually overly concerned about trying to maintain controlled impedances on tracks.  What we are concerned with is minimising loop area. This is because a loop leads to inductance.
At high frequencies to minimise the energy in a signal (and hence the noise it can generate) the return current will want flow such as to minimise this area.  One possibility is to individually consider each current loop and place the return 0V track directly underneath the signal track.  The signal is therefore going out on the top of the board and returning on the bottom of the board directly underneath the outgoing signal.
You do see this on some boards; for example switch mode power supplies but for general digital circuits this becomes impractical as it rapidly becomes too difficult to understand all the return paths.
This is why we have ground planes: because if the the entire area is 0V then the return current will naturally find the optimum path.
The reason why crossing split ground planes is a bad idea is that you are forcing current to flow in a large loop as there is no direct path for the return current; it has to find an indirect path.

My personal preference would be to have the top layer signals trying to keep the analogue and digital signals as separate as possible.  This may be easy if the only point where analogue meets digital is at an ADC. Depending on the amount of analogue circuitry we may have a single 0VD plane or the 0VA may be on a signal layer with the analogue and digital grounds being joined together at a single point near the ADC.