Is there a general rule as to how much clearance you should add to through-hole components' holes to allow them to fit easily?
For example, if I have a component with 1mm pin diameter, what should the diameter of the holes for it's pads be?
Using my calipers on a PCB I have handy, it looks like about 0.1mm is added to some holes, but I don't know if that's "normal" or not.
That (0.1mm) is too tight More like 0.25 to 0.4mm, and towards the high end if you're designing for automatic insertion of parts with bent leads. Usually 0.8mm is okay for most leads except fat diode leads, for which you can use 1.0mm.
Usually 1.3mm holes are specified for 1mm pins (for example on terminal block datasheets), sometimes 1.5mm which is really, really loose. Data sheet recommendations often err on the side of making the holes on the loose side, especially for parts like terminal blocks and relays.
If the leads are flat or square rather than round you can go a bit tighter on the diagonal dimension, assuming a round hole. For really flat leads it's better to specify a slot, of course.
Here are some recommendations (in inches, unfortunately, but 25.4 is fast to key in).
Of course if you're using some kind of special part such as a staked connector or press-fit part, follow the recommendations on the datasheet and pay attention to the tolerances too.
Typical recommended clearance for throughole pins is 0.15 mm (which is equal to 6 mils, or 0.006 inch). Keep also in mind the shape of the pin and tolerances.
If a pin has a rectangular cross-section, then the hole should be sized to the length of diagonal \$ \textstyle \sqrt{x^2 + y^2} \$.
Often the datasheet for your throughole would specify the dimension of the pin with tolerances. You should use the max possible size (which is the worst case). For example, if the datasheet specifies 2 ± 0.1 mm, the hole should be sized for 2.1 mm pin.
The PCB fab, in turn, will specify the tolerances for finished hole size (example). You should use the min possible hole size (which is the worst case). For example, if the fab specifies 2 ± 0.1 mm, the actual hole can be as small as be 1.9 mm.
In addition to desired clearance, you must also take into account the tolerances (variances) in your part. There are engineering standards for fits and tolerances (ISO 286-1 (2010) and ANSI B4.2-1978) which are nicely summarized here.
There are three main classes of fits- clearance (never overlaps), transition (sometimes overlaps, within part tolerance) and interference (always overlaps). In your case, you're definitely looking at a clearance fit since PCB is brittle and won't withstand strong compression forces. A 0.1 mm clearance as you mentioned would correspond to a loose running or free running fit. Which one you choose depends on the requirements for assembly time compared to locational accuracy- it's a tradeoff. Without knowing the specifics of your project, I wouldn't recommend using a larger clearance than that in a practical engineering application.
Once you decide which fit you'd like, use this calculator to determine what amount of clearance you need, taking into account the tolerances of your parts.
