What's considered the maximum number of parts on a single page?
Depends on the size of the page. You can fit more on a D-sized plotter sheet than a B-sized (roughly A4) sheet. Don't crowd things to the point it gets difficult to read.
What to consider when making a schematic multiple pages?
Almost all my designs end up as multiple sheets. Sometimes the manufacturing guys cut them all up and paste them together in one big plotter sheet to make it easier to follow the signal flow. But normally I don't print out bigger than 11x17 so I work at that size.
Something you didn't ask: I tend to make the first sheet be the critical input and output connections of my circuit, and work up towards more complex circuits on later pages. Other people like to put the critical signal path parts on the first page, and the input and output connections end up deep in the stack of schematics. I'm not sure which is really better.
When should I consider putting multiple tracks into a buss?
I rarely do this, but its a matter of style (and convention in your workgroup).
How should I name busses, netlists, and the references to other pages?
I tend toward all-caps net names, but otherwise I don't have fixed rules. More disciplined organizations might have more detailed rules.
How should I place components to minimize the number of nets?
I prefer to place components to make the signal flow clear. I don't worry about the number of named nets.
What kind of comments should I include on a schematic?
Anything important for the layout guy to know (matched length traces, place bypass caps near ICs, etc.) Anything a future engineer might need to know if they're looking to replace an obsolete part. Non-obvious critical specs like higher-than-normal resistor power requirements or tight tolerances. Anything that has to be tuned in production (Like "tune pot to achieve 50% duty cycle" or whatever).
Where should I place the designation and value for horizontal and vertical components? Does it matter as long as I stay consistent?
I use vertical text for vertical components to allow more parts to fit cleanly on a sheet. Others (apparently) consider this a grave sin. Be consistent and be consistent with others in your organization.
Should I note component packaging & rating on the schematic? Meaning discrete vs SMD or if a specific resistor is high powered?
Specifying the package type for each part visibly on the schematic would be clutter. But obviously that information has to be in the design to get transferred to layout. As mentioned above mention nonobvious specs that might trip someone up if they have to replace an obsolete part or find an alternate vendor due to a shortage.
Your BOM (Bill of Materials) will need to specify an exact manufacturers part number (or a list of acceptable alternates called an AVL "approved vendor list") for each part.
Should I customize nets in different colors or widths?
I don't recommend this. I'd prefer to get schematics that make sense if printed out in black & white.
How should I version control schematics?
I store datecoded backups (like "mydesign_20120205.zip" on my own pc and a remote share drive. Definitely store a backup whenever you release a design (either to layout or to manufacturing).
Edit: There are better ways to do this (see comments) but a simple process like dated zip files is also perfectly workable.
What workflow should a single person use to keep designs organized?
Keep backups. Use all the tools you have available. If you aren't doing your own layout, keep good communication with the layout guy.
Best Answer
I'm a professional electrical engineer who routinely designs new circuits for volume production, and have been for over 35 years.
Yes, I frequently do calculations to determine the exact part specs. There are also many cases where experience and intuition are good enough and the requirements loose enough that I just pick a value. Don't confuse that with a random value, though.
For example, for a pulldown resistor on the MISO line of a SPI bus, I'll just spec 100 kΩ and be done with it. 10 kΩ would work fine too, and someone else picking that wouldn't be wrong either. If I'm using a 20 kΩ resistor elsewhere, then I might spec another one on the MISO line to avoid adding another part to the BOM. The point is sometimes you have a lot of leeway, and intuition and experience are good enough.
On the other hand, looking at the schematic of my latest design, which I'm in the middle of bringing up first boards of now, I see a case where I spent some time not only specifying the part value but calculating the result of variance on the rest of the system. There were three cases of two resistors used in the feedback to a switching power supply. Here is the problem worded like homework:
That's a genuine real world problem that took a few minutes with a calculator. By the way, I determined that 1% resistors were good enough. That's actually what I expected, but did the calculations anyway to make sure. I also noted the full nominal range for each supply right on the schematic. Not only might this be useful to refer to later, but it also shows that this issue was considered and the calculations done. I or someone else won't have to wonder a year later what the tolerance of the 3.3 V supply is, for example, and re-do the calculations.
Here is a snippet from the schematic showing the case described above:
I just picked R2, R4, and R6, but did the calculations to determine R1, R3, and R5, and the resulting power supply nominal ranges.
Added about the SHx parts (response to comment)
The SH parts are what I call "shorts". These are just copper on the board. Their purpose is to allow a single physical net to be broken into two logical nets in the software, which is Eagle in this case. In all three cases above, the SH parts connect the local ground of a switching power supply to the board-wide ground plane.
Switching power supplies can have significant currents running across their grounds, and these currents can have high frequency components.
Much of this current just circulates locally. By making the local ground a separate net connected to the main ground in only one place, these circulating currents stay in a small local net and do not cross the main ground plane. The small local ground net radiates far less, and the currents don't cause offsets in the main ground.
Eventually power has to flow out of a power supply and return via the ground. However, that current can be filtered much more than the high frequency internal currents of a switching power supply. If done right, only the well behaved output current of the switcher makes it out of the immediate vicinity to other parts of the overall circuit.
You really want to keep local high frequency currents off the main ground plane. Not only does that avoid the ground voltage offsets those currents can cause, but it prevents the main ground from becoming a patch antenna. Fortunately, many of the nasty ground currents are also local. That means they can be kept local by connecting the local ground net to the main ground in only one spot.
Good examples of this include the path between the ground side of a bypass cap and the ground pin of the IC it is bypassing. That's exactly what you don't want running across the main ground. Don't just connect the ground side of a bypass cap to the main ground thru a via. Connect it back to the IC ground via its own track or local ground, then connect that to the main ground in one place.