I find it very helpful to have a schematic with a PCB.
I'll repeat an observation from one of my PCB mentors: you are paying for a copper covered board. Copper is good. Rather than have most of it chemically removed to be disposed of, maybe to leach into the water supply, keep it on the board :-)
As soundcyst said, avoid right angle or tighter corners (including steps in tracks). PCB manufacture is a 'wet chemical process'. Try to think what happens when washing a strangely shaped object. Corners can trap etching chemicals, or be attacked by the chemicals from more than one side. Hence try to avoid sharp corners, and use mitres. Further, sharp corners can radiate electrical noise more strongly than rounded or straight tracks.
Also, set up the design rules; "Design rules are you friend" :-)
They help ensure the geometry of the tracks is within the capabilities of the manufacturing process. The tracks on that board look very, very narrow.
Also, the wider the track, the lower the resistance, and low resistance is good. Unless doing exotic design, it is always better to keep track resistance low.
I assume the picture was generated straight from the CAD, and it hasn't been changed in any way?
Some of the tracks seem to have little steps in them which suggest the parts aren't lined up.
If the CAD actually generates gerbers with those steps, the track corners will not come out as cleanly.
I'd recommend lining up the tops of the row of resistors, and routing with wide, wide tracks.
Also, most (all?) of those resistors are pulling pins to ground/Vcc.
You could save space by using a resistor array, e.g. SIL's:
one type has a shared common for all of the resistors. It might make the PCB smaller. Consider one for R1 to R6, and another for R7 to R9 (this one is less of a win).
Almost all of the signals on the top row of the 20-pin socket are common, joined together, with the actual signals on the lower row, on the opposite side. If either the 8 pin socket moved below (south) the 20-pin, or the 20-pin were rotated through 180 degrees, then the signal pins that need to be connected would have less 'wiring' in between, so it would be easier to connect because tracks can use both layers without obstruction, and easier to understand!
If you could use smaller resistors, e.g. a SIL, and move the socket, the resistors might be moved out of the space between the sockets, so the signals between the two sockets should be more direct. (Of course, there still needs to be some room for headers, so this might not work as well as I hope).
I tend to try to route the same signal on one side initially.
All of the connection between 9 of the pins on the 20-pin socket could be routed on one layer.
All the track between R1 to R6 (north end) could be on one layer.
All the tracks between R7 to R9 (south end) could be on one layer
After that, most of the signals will be on one side, so add a ground plane. That is a 'copper pour' made using a polygon, drawn around the board, connected to ground. Eagle (I think that's what you said you were using) will calculate it so that it doesn't touch any signals. So you could put one on both sides of the board. It will help reduce electrical noise, and reduce the amount of copper etched from the board.
My PCB mentor says that for best results, hatch large areas of copper (yes, I know what he said about removing copper) because this can help get more even etching in manufacture. Not critical, but does look more interesting :-)
I hope my comments don't put you off. I hope they help.