If you’re using a switchmode regulator IC, the manufacturer will usually provide quite detailed guidelines on PCB layout. You’ll need to provide more specific information for us to be able to help further.
Normally people here are happy to give advice, but not actually do the PCB design work for you. Providing the Eagle files (as well as JPGs for those of us that use other CAD packages) is a good idea.
If you have 4 layers you’d normally dedicate one inner layer to a ground plane and another to a power plane (with the outer 2 layers for signals). These planes should be unbroken, and all connections to components made with vias very close to the component leads. Decoupling capacitors should be placed close to these vias.
When you have only 2 layers, you should try to dedicate one layer (the bottom layer) as a ground plane as much as possible and minimise any breaks in this plane. While you’ll sometimes need to run tracks on the bottom layer, these sections should be as short as possible, even if you need to use more vias. Looking at your circuit you should be OK with 2 layers, if you move the tracks currently on the bottom layer to the top layer as much as possible.
Some other comments on your circuit:
It’s a bit hard to comment on it, as the ICs aren’t labelled, and there are a lot of signals going to connectors that I don’t know the purpose of. I’d suggest labelling the nets with meaningful names.
You should add decoupling capacitors to the power supply pins of the ICs. 10 or 100nF is normally fine.
The width of power tracks should be increased, to reduce their inductance & resistance. The ground connections should be using a ground plane as described above.
You could reduce the size of the PCB substantially if you wanted to (there’s a lot of empty space on the PCB).
It’s hard to read as a number of nets have vanished due to the screen resolution when you did the screen capture. If you can’t fix that, try attaching a PDF
(use CutePDF or something similar)
ICs are missing both reference designators (U1, U2) and part type
Using power symbols (Vp/Vn or Vss/Vdd) rather than drawing the nets connecting all Vp pins will make the schematic easier to read. Likewise, use separate power and ground symbols rather than showing nets connecting unrelated parts of the circuit that just happen to share a grouind
In general, try to avoid 4-way junctions
Avoid drawing nets through components (ie, R54)
You have a number of places where nets are drawn through text (values, refdes). I’d move the text to make it more readable
As mentioned, you need decoupling caps at every IC. Since you are combining analog with a switcher, you may also want ferrite beads or 10R resistors at each IC as well
C14 should be a polarized cap (tantalum or aluminum).
PCB:
As mentioned, your power and ground traces need to be much thicker; I would also use a ground plane on the back side with as few traces as possible cutting it
Will you be able to plug in the cable to PL2 with it in that orientation? Will the ejector ear hit the caps?
Add mounting holes
Add a note with the board name, date, rev, etc
traces should connect to other traces and pads at 90 degree angles; acute connections can form acid traps
There are some places where spacing is very close (pad2, r48)
You have silkscreen on solder pads. Make sure your CAM job will mask the silk layer with the mask layer. Some board houses will happily put silk on pads, which will float off during soldering and make a huge mess
C13 and C14 are the wrong size. Verify the size of L1.
Look for the recommended layout for the swicher. Pay attention to pour size and part placement.