Addressing the question that was originally asked:
These footprints are generated using calculations from IPC 7351B, which is not the only way to do it. In fact, the KiCad library footprints assume component sizes in IPC SM-782, but that same document has very different footprints recommended, with an inter-pad spacing of 1.2mm, but that’s also a much older document from 1996 and PCB assembly has changed a bit in the last 29 years)
First, definitions:
I’ll use the IPC SM-782 1206 capacitor component sizes and tolerances, as that’s what the library uses. Your manufacturers differ a little.
- L: 3 to 3.4 mm
- T: 0.25 to 0.75mm
The spacing G is calculated from a number Gmin. Gmin requires to know Smax, which is the maximum space between the leads.
Worst case tolerances:
- Ltol = Lmax - Lmin = 0.4mm
- Ttol = Tmax - Tmin = 0.5mm
- Smin = Lmin - 2Tmax = 3.0 - 2 * 0.75 = 1.5mm
- Smax = Lmax - 2Tmin = 3.4 - 2 * 0.25 = 2.9mm
- Stol = Smax - Smin = 2.9 - 1.5 = 1.4mm
IPC 7351B uses an RMS error propagation method rather than worst case:
- Stol (RMS) = sqrt(Ltol ^ 2 + 2Ttol ^ 2) = sqrt(0.4^2 +2 * 0.5^2) = 0.812
Now, we find the difference between Stol and Stol (RMS) = 1.4 - 0.812 = 0.588mm
Then we add/subtract half of that each to the worst-case min and max (caution: IPC 7351 not-B is different here) to get a “more realistic” (IPC’s words) description of the expected range of S:
- Smin (adj) = Smin + 0.588 / 2 = 1.794mm
- Smax (adj) = Smax - 0.588 / 2 = 2.606mm
Jh is the heel fillet goal, which is 0 for a 1206 capacitor footprint at medium density.
Then, Gmin is found from the max lead spacing, minus the heel fillet, minus tolerance adjustment:
- Gmin = Smax (adj) - 2Jh - sqrt(Stol RMS^2 + F^2 + P^2) = 2.606 - 0 - 0.812 = 1.786mm
F and P are an additional couple of terms here for board manufacturing tolerance and pick and place placement tolerance, but they contribute almost nothing in this case (they start to dominate in smaller footprints). KiCad currently sets these to 0.1mm and 0.05mm respectively.
Finally, round off to 0.05, so 1.8.
This is how the footprint pad spacing is calculated. There are lots of choices embedded in this process:
- Choice of the component size and tolerances - your part has different sizes and tolerances on BW (aka T)
- Choice of error propagation method - you can choose to do worst-case rather than the RMS-based system, or bias more towards worst-case
- Choice of heel fillet allowance - you can choose to have more or less (in fact IPC 7351 non-A had a negative fillet of -0.05).
- IPC density levels can affect this, but in the case of capacitors like this, it’s 0 at all three levels (most, nominal, least)
- Choice of using a completely different system (e.g. manufacturer guideline or IPC SM 782 footprints or whatever your boss read on the back of a cereal box this morning)
You may find the library choices unsuitable for your needs, and that’s completely reasonable.
For example, you may not agree that the RMS tolerance system’s assuming that worst-case tolerances won’t usually co-exist is a “safe” thing to do and worry about the worst possible in-spec case: a 3.0mm part with two 0.75mm terminals:
Even this edge case probably would solder just fine, as you still have plenty of terminal overlapping there. But you may wish to add some heel, or be more careful with traces passing near the inner edges, which could touch the terminals and be separated by only solder mask.
The good news is probably many millions of these parts have been used on KiCad PCBs (and 1206 is a very, very common part to use), and we aren’t inundated with complaints, so they probably work well for most people. You are always right to check, however.
Then isn’t the distance between the center of the pads 3.2-0.5=2.7?
This is meaningless for hand soldering variants, as they have an extra extension on the outer edges for your soldering iron, so the centres are always going to be further out.
Even without that, the IPC 7351B toe fillet goal at medium density for a 1206 capacitor is 0.35 and the heel is 0, so the pads will be slightly biased towards the outside. You can see this in the footprint with nominal 0.5mm leads drawn in:
Also, by the way, IMO 1206 is a completely fine size to use if you don’t mind the space it takes. But you will probably find the the handsoldering variant is not required even if you want to handsolder the boards. At the 1206 size, anyone with good motor function and more than a day or two of soldering time will not struggle to solder onto the normal footprint. If you have a struggle with fine parts physically (motor function, vision, etc), or you want people who have never soldered before to do it, then the handsoldering variant may be a good idea. On the other hand, such longer toe fillets can increase the chances of tombstoning during reflow.
