so I can use capacitors with 2.5, 5, 7.5, 10 and 15 mm pitch.
What would be the most elegant way to do this? If possible I’d like to keep the standard capacitor symbol. In this example, I have simply duplicated pad 2 several times in a 2.5 mm grid. Could I do this or is there a more elegant way?
There are a handful of threads on this topic, like multiple pads for one schematic pin (SO8 transistors for example), but I’m not sure if there is a consensus how to handle those best.
The size of a capacitor is determined by type of capacitor, working voltage and capacitance. Having a size range between 2.5mm and 15mm for a capacitor in any sort of application is very unlikely. Having multiple pads with the same number is perfectly normal in KiCad, but you have to respect the clearance between pads with different numbers, and the simplest way to achieve a proper clearance is to remove the second pad from the left.
For the rest, there are several possibilities which all work properly.
Leave as is. During routing KiCad will prompt you to connect all pads with the same pad number.
You can make one of the pads oval an very long and with an offset in the hole (in the footprint editor) (Figuring the right offset combined with pad size is a bit fiddly).
Use the pad edit mode in the footprint editor to add some graphic lines to one of the pads (this is probably the simplest).
Add an elongated SMT pad in the footprint editor, and then disable mask layers. (I think option 3 is a bit more logical).
So the reason why you are suggesting oval pads or an elongated SMT pad (options 2-4) are so they are connected in the footprint? I simply connedted them with a track, which is easy enough.
Spacing between pads 1 and 2 (leftmost) is still only 0.2 mm, which however is fine for JLCPCB.
Out of curiosity, could one make a “cut-off” circular pad (D-shape) to increase the spacing between 1 and 2?
There is no built-in support specifically for a D shape, but you could make the outer ring very small and then draw the rest of the D in pad edit mode manually.
If I bought some electronic kit and was soldering it. I would probably put the capacitor in the rightmost pads. It is easy to assume that the rightmost pad is “pin 1” and the 5 pads from the left side are all “pin 2”. And this makes it a badly designed footprint. And again: There is simply no way that a capacitor for any given application has a pitch between 2.5mm and 15mm.
I see footprints for capacitors like this quite often in the world of DIY audio. My guess is it gives builders more options to fit in the capacitor they happen to have. Apparently there is also a cadre of folks that experiment with different input coupling capacitors with the belief that there is a different sound to each. Assuming they are all film type capacitors of the same value, I would doubt the difference would be audible.
Mainly for the reason paulvdh points out, I don’t think footprints like this are a good idea.
I guess my thoughts here don’t really help Martinn with his questions.
It is common in DIY audio, and not just for “experimentation”, but because similar (capacitance, voltage) are available in different sizes, and your not limited to a particular size or brand when ordering. With Chippageddon and the virus thing from a few years back, there were several threads about combining two IC footprints, to have more options when ordering parts.
This is an experimental board, so I assume you will be hand soldering.
You will probably be cursing over the .2 mm spacing when you start soldering through hole wires between 1 and the closest 2 pad, even with a resist layer.
You could make your work much easier with a symbol like below, with a 1 mm spacing. You have a lot of real estate inside your courtyard, you might as well use some. Copper is free on a PCB.
