How close is too close for traces on a PCB?
It really depends entirely on what the signals are carrying and what the manufacturer says they are capable of.

The general rule of thumb is that you should maintain a minimum of the width of the trace. If you are using 10mil traces, then you should also have 10 mil of space between them. If your traces are carrying sharp-edged waveforms (i.e. square waves, digital signals, data buses) or sensitive networks (A/D, sensor or op-amp inputs) then you want to maintain more of a distance and perhaps add a guard ring (ground traces) on either side of the trace in question.

I am a (very) happy customer of Sunstone; their manufacturing process allows me to use 5 mil trace with 5 mil space without any trouble, and they can do 3/3 if you're willing to pay extra. A 5 mil trace is a damned thin trace and pretty much at the level of most commercial boards these days, so there is little reason to go thinner unless you have some specialized application. For most of my boards I try to stick to 8, 12 or even 16 mil traces since they're much more rugged and easier to work with should you have to modify the board. If you're carrying high current or routing supplies I will make the traces as wide as I can afford to, from a board real-estate perspective. Wide traces are good.

I see from your picture that you're running traces between the pads of 0603 components. This isn't verboten, but it's also generally something you will want to avoid. It's too easy to end up either bridging some solder to the trace underneath (soldermask failure) or damaging the trace if you have to lift the component off (e.g. a bit of flux sticking under the part and effectively "gluing" the trace to the bottom of the component. The trace from R15 also goes awfully close to the pad for R8, and the trace that goes around the top right-hand side of the board seems to come awfully close to the via. It would be wise of you to find out what the board manufacturer is capable of doing, and what the recommend (these are not the same thing) and programming that into your layout's DRC. If the DRC flags something, fix it. This is Design For Manufacture (DFM) 101. If you violate the DRC you end up with higher manufacture wastage and in the end, more expensive boards.  Sunstone is really nice here; they provide eagle-format DRC rule files. You simply download it and use them.

The DRC can be a real pain in the ass, but it's like eating your veggies; your project will be better off for it in the end.