Oval mounting holes

I hereby certify that I am not simply asking someone else to design a footprint for me.

This is an auto-generated message that is in place on the “footprints” section of the KiCad.info forum. If I remove it and ask for a footprint to be designed anyway, I understand that I will be subject to forum members telling me to go design my own footprint or referring me to a 3rd party footprint site.
Is there a way to allow a little adjustment by using oval mounting holes? All the many sizes of mounting hole footprints appear to be round.

Set pad type, shape and hole shape like this and tweak away

You can draw oval holes, but that does not mean they can also be made (for a reasonable price)

Round holes are drilled, and this can be done from fairly small diameters upwards (somewhere around 0.2mm, but that’s pushing the limit).

“Oval” holes are made with a router bit, and this router has to move sideways through the hole. And for this it needs strength, which means more thickness. The width of 0.5mm that qu1ck gussests may be too narrow for a router bit.

For the actual limits for drills and routing you need to have a look at the website of your PCB manufacturer.

1 Like

If space is available, perhaps you can overlap a few footprints with slightly different spacing of round holes? DRC would probably give you errors but my guess is that this is not a board for mass production anyway.

Nope. Won’t work.
Drilling a hole halfway through another hole is a recipe that almost guarantees broken drills. Even if you disregard the DRC violations, then your PCB manufacturer wont. This is very likely to just get your PCB rejected.

I have plated slotted holes in a few pcb, and they have not incurred extra cost. DC barrel sockets, USB sockets, 30A Anderson power sockets. Also mounting holes with some XY adjustment.

I was not talking about interfering holes. I was talking about 2, 3, 4, or 5 footprints (all with slightly different hole spacing) overlaid so that the bodies and courtyards would interfere but with the holes spaced adequately and pads properly connected.

This would be easier to fabricate than holes with a 9-pointed star shape.

Oops, my fault.

Yes you can overlap footprints but make sure the holes of the footprints do not overlap.

DRC will complain about overlapping courtyards (if there are overlapping courtyards).

Using multiple overlapping footprints is quite common, for example to have the option to mount a differently sized capacitor, or an RS485 chip in both DIP (which can be easily replaced if damaged) or SO-8.
If you also put such parts twice in the schematic and connect them in parallel it looks ugly. There is quite a simple way around this though:

  1. Copy one of the footprints to a personal library.
  2. Save the part in your library.
  3. Browse to the other footprint.
  4. Drag a box aound the graphics (pads, silkscreen, etc) you want and copy it.
  5. Go back to the footprint you put in your personal libary.
  6. Paste the stuff from the other footprint there.
  7. Point the schematic symbol to your new footprint so it gets used.

If you do this you have to check the pin numbers very carefully. IC’s and transistors in different packages may have different pin numbers for the same functional pin.

This topic was automatically closed 90 days after the last reply. New replies are no longer allowed.