On a board like this I always use ate least 4 layers. I make one internal layer a single ground plane. I normally also make a power plane on the other internal layer, but on this one I used this layer to route +5V and any other power signals. This way I could use this power layer for some signal routing, if needed. It's important to use an internal layer for any solid plane. It helps keep the board from warping, and a board this size can warp pretty easily.
I set my clearances to 6mils and distances to 8mils. I use .01" traces for signals and .024" for power (wider is less inductance). I use .015" drills for all signals. I usually use .023" drills for power. Not all board houses can make boards with these geometries, but most can.
Next I route the +5V layer. I have to make sure it is completely routed before using the autorouter. I only use the autorouter to verify my layout is routable. I save the the board right before I start the autorouter and then reload the board without saving to take me back to were I was before using the autorouter. As wonderful as the autorouter is, it does not route with any insight at all. It's a lot like using GPS, it will get you there, but takes the most unorthodox path to do it. It has a tendency to go around it's elbow to get to it's nose.
If the board routes 100% you could just generate Gerber file and order a board. It would also look butt ugly. Cleaning up after the autorouter is more work than hand routing.
I usually use the top layer for vertical traces and the bottom layer for horizontal traces. At first this will create a lot of vias, even for a board with a lot of through-hole parts. The vias will become fewer as you have to rip-up and re-route.
I've found on most boards signals, and their traces, are clumped around groups of parts. This leaves traces that connect the groups. I route the local groups first and then connect groups. This seems to minimize the amount of rip-up. If the longer interconnecting traces become 'squiggly', consider ripping it up and starting from the other end.
Routing PC boards is an art. It takes practice to get good at it. I have ripped up a completed board and started over just to get the experience. I often found the second, or even third, go at it produces a cleaner and neater route. I usually only do this on my own stuff at home, my boss isn't so understanding about taking two or three times longer to get it done just to make it look better.
I use Eagle and have done so for nearly twenty years. I've used Pads and Mentor professionally, but Eagle is the only affordable package to use at home. Even then it's worth spending the money and get the better version. I use pro and I probably have over $1,000 invested in it. It's worth every penny! For me, drawing schematics and laying out PCBs is the most fun I can have with my clothes on.
Let me know if you have questions or need any help. I'm glad to be of assistance.