I'll just comment on the design:
- Replace C5 with a 100nF ceramic capacitor and place it close to the power supply pin of the MCP6022.
- Put the designators on the PCB-Design, not values. Make it far
easier to understand the layout.
- Avoid 90° trace bends, they can cause problems when etching the
board. They're also bad for high-speed stuff (at least that's the
common opinion on the matter). Use two 45° bends instead.
- Consider flooding one side of the board with a GND-Plane.
- Use wide short traces for power supply connections.
- Use one side of the board for mostly vertical traces and the other
side for horizontal traces.
- Take more care of component placement. Place them in a way where
they are easier to route. Component placement is 70% of the job.
Place them BEFORE starting to route a single trace (Won't always
work out). Just use the ratsnest (the lines which indicate connections which
are not routed yet) as a rough guideline.
- Do not see a trace which is already routed as something which is fixed. If
its in the way or you don't like they way it looks, rip it up and try again.
- When in doubt, start from scratch, try not to rescue something which can't
be rescued anymore.
- Rule of thumb: Create something which pleases the eye. Others will have an
easier time to understand it and sometimes it will even work better.
There are two Books i can highly recommend for learning Electronics/PCB Design: The Circuit Designer's Companion and EMC for Product Designers. While the second one more about EMC compliance it helps to understand WHY these things should be done in a certain way.
A while back I hired an EE straight out of college. He asked me something like, "how do you prove out your designs? Do you breadboard them? Wire-wrap? How?"
My answer was, "Well, we build a PCB and if it works we go into production and ship it!"
Many circuits simple cannot be prototyped without making a custom PCB. Anything high-speed, low-noise, high switching currents, etc. are difficult or impossible to make any other way. Sometimes the logistics alone get in the way. You cannot, without a custom PCB or some crazy adapter/socket, prototype with a 1000+ ball BGA. Even if you could, you wouldn't want to. The odds of making 1000+ connections without error is very low. Doing it twice is almost impossible.
Making custom PCB's for prototypes seems expensive, but it isn't. Not compared with paying someone to make and debug several prototypes using breadboards or wire-wrap and even then ending up with something that is of questionable reliability.
So professional EE's usually go straight to designing a PCB and then doing everything they can to make sure that PCB works the first time. It almost never works the first time, but the closer it is to working the better it is. Then the board is modified (a.k.a. re-spun) and built again. With any luck a PCB goes through 2 or 3 respins before going into commercial production.
I recently did a custom PCB that used an Intel Atom PCB and all the usual PC type things. My approach was no different with this PCB. I designed it, tried very hard to get it to work the first time, and built it. The Rev 1 PCB's mostly worked, but has some minor issues. The Rev 2 board worked perfectly.
Best Answer
Howard Johnson has a massive collection of high-speed digital design newsletters.
http://www.sigcon.com/pubsAlpha.htm
One of my favorites visibly demonstrates the return currents that darron mentioned. DC will flow in a straight line (the path of least resistance; a straight line on the ground plane), while AC will flow underneath the signal conductor (the path of least inductance; a mirror image of the signal path on the ground plane) So avoid having that return path cross a split plane, avoid having it cross too many other high-speed return paths, etc. Also, power planes can act like ground planes for a return path, and the return path can jump planes through a capacitor (remember, cap is a short to high frequencies); the return path always chooses the plane closest to the signal. http://www.sigcon.com/Pubs/news/8_08.htm
I believe there are other newsletters. For instance, 90 degree angles aren't really that bad; they merely add excess capacitance to the trace. At "regular" high speed frequencies, this is no big deal. But when you hit microwave, the parasitic capacitance can do you in. http://www.sigcon.com/Pubs/edn/bigbadbend.htm
Regarding trace size, this largely depends on your stackup. If you use a solid reference plane (ground or power!), then your trace impedance is a function of trace width and distance from the plane. If you don't care about the impedance, then trace size largely doesn't matter, as long as it's not too small. Unless you're trying to carry obscene amounts of current (amps?), in which case you need traces big enough that they won't melt!
Try to keep signal planes adjacent to reference planes. i.e. for an 6 layer board, signal layers 1 and 3 reference ground plane 2, and signal layers 4 and 6 reference power plane 4. If signal planes are adjacent, be careful that there are no long parallel runs that could induce cross-talk. This is less of a concern if there's a reference plane (although the return currents can still cross-talk, it's not as bad)
Keep clock traces and other strong sources of noise as far away from other traces as you can (I think the rule of thumb is 5x the trace width away for clocks and 3x for other switching signals).