Tracks
There is no recommended standard for track sizes. What size track you use will depend upon (in order of importance) the electrical requirements of the design, the routing space and clearance you have available, and your own personal preference. Every design will have a different set of electrical requirements which can vary between tracks on the board. All but basic non-critical designs will require a mixture of track sizes. As a general rule though, the bigger the track width, the better. Bigger tracks have lower DC resistance, lower inductance, can be easier and cheaper for the manufacturer to etch, and are easier to inspect and rework.
The lower limit of your track width will depend upon the "track/space" resolution that your PCB manufacturer is capable of. For example, a manufacturer may quote a 10/8 track/space figure. This means that tracks can be no less than 10 thou wide, and the spacing between tracks (or pads, or any part of the copper) can be no less than8 thou. The figures are almost always quoted in thou’s, with track width first and then spacing. Real world typical figures are 10/10 and 8/8 for basic boards. The IPC standard recommends 4thou as being a lower limit. Once you get to 6thou tracks and below though, you are getting into the serious end of the business, and you should be consulting your board manufacturer first. The lower the track/space figure, the greater care the manufacturer has to take when aligning and etching the board. They will pass this cost onto you, so make sure that you don’t go any lower than you need to. As a guide, with "home made" PCB manufacturing processes like laser printed transparencies and pre-coated photo resist boards, it is possible to easily get 10/10 and even 8/8 spacing.
Just because a manufacturer can achieve a certain track/spacing, it is no reason to "push the limits" with your design. Use as big a track/spacing as possible unless your design parameters call for something smaller.
As a start, you may like to use say 25 thou for signal tracks, 50 thou for power and ground tracks, and 10-15 thou for going between IC and component pads. Some designers though like the "look" of smaller signal tracks like 10 or 15 thou, while others like all of their tracks to be big and "chunky". Good design practice is to keep tracks as big as possible, and then to change to a thinner track only when required to meet clearance requirements.
Changing your track from large to small and then back to large again is known as "necking", or "necking down". This is often required when you have to go between IC or component pads. This allows you to have nice big low impedance tracks, but still have the flexibility to route between tight spots.
In practice, your track width will be dictated by the current flowing through it, and the maximum temperature rise of the track you are willing to tolerate. Remember that every track will have a certain amount of resistance, so the track will dissipate heat just like a resistor. The wider the track the lower the resistance. The thickness of the copper on your PCB will also play a part, as will any solder coating finish.