This general topic can quickly get overwhelmed by the details of a particular situation. (E.g., “Track width advice for 12v&5v rail 100ma” at Track width advice for 12v&5v rail 100ma .)
Yes, the place that fabricates your boards sets limits on some of these factors. And, like @davidsrsb points out, there is typically little to be gained by asking your vendor to operate right on the edge of his capabilities when he makes your boards - so build in a little margin between what you ask for and his advertised capabilities.
But there are other practical reasons for designing with larger feature sizes. One such reason is ergonomics. If a real live person of the homo sapiens persuasion must interact with your board during soldering, troubleshooting, modification, or repair then larger traces, spacing, and pads, should be considered. (When you read the following list of my opinions, remember that 10 mils (0.25 mm) is approximately the thickness of a business card, or the thickness of 3 sheets of common printer paper.)
-
Hand-soldering SMT components can be done more reliably if the pads are enlarged to expose more copper beyond the component body. And while you’re at it, don’t pack them in so tightly that you can’t get a soldering iron onto the pad.
-
The same idea applies to test equipment probes, even if the board is machine-assembled. You may try to anticipate which nodes are likely to be investigated by a 'scope or DMM, and which aren’t, but when things don’t behave quite as you expected then the node you want to look at is usually the least-accessible node on the board. Or, you can’t probe it without shorting to adjacent components.
-
A 10-mil (0.25 mm) annulus on a through-hole pad may be fine for automated soldering processes but taxes the abilities of a manual soldering operator. With so little copper to contact the soldering iron’s tip and conduct heat into the joint, the time needed to complete the joint is longer and the risk of component damage is greater. I use 15 to 20 mil annulus for manually-assembled prototypes, and 30 mils for wire attachment points.
-
Find out what “standard” hole sizes your board fabricator uses, and limit your hole sizes to exactly those values. In particular, identify his standard value in the range of 0.030" to 0.035" (0.75 to 0.90 mm) and use this size as much as possible - it’ll probably work well for 90% of your through-hole parts.
-
A 10-mil trace of 1-ounce copper is suitable for a bit less than 1 amp in most applications. Narrower traces are more likely to de-laminate from the fiberglass substrate when components are removed or replaced during prototyping or repair activities.
-
10 mils is probably the minimum copper-to-copper clearance you should use for hand-soldered boards. (And some production engineers will thank you, perhaps with a serving of your favorite malt beverage, if you stick to 10-mil spacing on machine-assembled boards.) Even at 10 mils you need to watch carefully for solder bridges.
Dale