With experience, you'll find there is often no black and white answer to many of these questions. You have to understand something about the signals you're carrying to make educated decisions about how to treat the traces and components that carry those signals.
I just want to second some of the opinions expressed already because they bear repeating. With screw holes, print your design 1:1 and poke a hole through your mounting locations. Insert the fastening hardware you plan to use and verify the mechanical clearance to every part in proximity. I also do not recommend ever putting traces beneath the head of a screw/bolt, due to the possibility of conducting an exposed trace, or wearing through solder mask (on a produced board) and then conducting with the exposed trace. Remember to provide clearance for nuts, if the bolt head is on the mating surface and not the PCB. Remember also any tool clearance if you'll be tightening a nut with pliers, etc.
So, back to traces and such. It has long been good practice to use 45deg. angles instead of right angles. Do they have to be 45deg? No. With low-speed (say, less than 10MHz) circuits, you can get away with many sins. The higher the frequency, the more these nits need to be picked. For high-current traces (power supplies and such), gentler curves are better than sharp angles because of the thermal stresses and thus opportunity for "weak spots". Mostly, just make sure the trace is always wide enough, even when changing orientation, and you'll be OK.
In general, I strive for 100% 45deg. angles. Partly because it just looks nice, and it never hurts to develop good habits when it doesn't matter so it's second nature when it does. Of course, I'll bend the rules and use 20-70deg angles when a 45 would put a trace too close to a neighboring pin. That's almost entirely a cosmetic dispute. Furthermore, I'll try to avoid too many bends (I think of it as avoiding electrical turbulence) and too-long straight lines (subject to inductance and capacitance with things near and parallel to that trace), although I'm not sure my logic is entirely sound on either point there. It just feels like the right thing to do, and I could very well be wrong.
On proximity of holes... Always leave space around the board edge. Different fabrication houses have different requirements here, but they're almost always way more lenient than you should strive for. You don't want the board to have weak support around a component hole, so make sure not to perforate the board with too many holes in too small a space. That principle covers hole-to-hole clearance, grouping many holes too close together (Swiss-cheese style), and being too close to the edges. If it feels like you could snap a chunk out of the board, provide more solid substrate.
On proximity of traces... When two traces ride alongside each other, they will tend to couple capacitively. This is detrimental to high-frequency signals. Things that change rapidly, ala digital transitions, certainly apply as well as true HF analog waveforms. In rare cases, you can benefit from this -- like power and ground traces -- but it's better to use a capacitor when you want coupling, rather than taking advantage of the side effects of layout.
There's also inductive coupling, where the signal from one trace (or component!) can "echo" onto another trace (or component). This is usually to be avoided at all costs. Placing grounds between bleed-prone signal traces is a good approach, as is ample distance. Digital signals have (in theory) infinitely high-frequency spikes caused by low-to-high and high-to-low transitions. In reality, those transitions aren't perfect square waves, but they can still cause radiation into other signals -- especially analog. High-current traces will tend to bleed more than low-current, so keep your low and high level traces well apart from each other.
Routing between the pins of ICs, and underneath the body of components, is a common practice. As long as the trace has adequate clearance (10 mil is typical) from other traces and pads, you'll minimize the chance of shorts. Most professional fab houses can get closer, and most home etching attempts should probably be a little further. Remember of course to respect the nature of the signals on those pins. High current and high frequency signals should not be near low-level signal and analog signals. Sometimes you can't help it, so just do the best you can.
For grounding, I have a few principles I follow. The bigger the better. I'll sometimes have larger ground traces than power traces. You want your grounds to have as little impedance as possible. Strive for having every ground go back to the common ground point individually. In most cases, this is impossible to accomplish, so you have to group similar grounds and bring them back in bulk. Prioritize here. Power supply grounds should be as separate as possible from signal grounds. Analog and digital should not be shared. High frequency and low frequency will benefit from separation. Areas that are subject to crosstalk should be separate. Etc... Really try to avoid "daisy chaining" grounds from one component to another to another. Connect them to a plane instead, and bring that plane home to the supply ground. Good grounding is the art of compromise, so try to always follow best practices and bend the rules where you must. Again, prioritize.
A good thing to do is try alternate layouts. The hardest part of designing a PCB (for me) is the blank canvas, so just dive in and start working outward from there. Place your components such that they are logically grouped well. Things that attach should be near each other, and things that can disturb each other should be far apart. Rotate things and try alternate arrangements until you find a way to prevent snaking traces everywhere. Many people advise, when using two layer boards, to route traces North/South on one layer, and East/West on the other. This provides a way to keep traces from having to cross each other too much. Vias will bring top signals to bottom, and back again. But, I avoid vias as much as conveniently possible. That may or may not be necessary. In general, for less dense boards, I try to keep all my traces on one side, so I have a whole other layer to fall back on when I run out of area for grounds or power distribution, etc. There are no hard rules here, it's just a matter of what works for you and the layout demands of your project.
Most of all, it takes practice. :-)