Custom Pads in footprints


I am trying to use “flower pads” like this:

Not sure how to do it. I tried to make an arc, then a polygon, but the polygon does not fill in footprints… How would you do it?

Thank you very much!

1 Like

I think you can approximate it with a trapezoidal pad, but I don’t think there is a way to create a semi-circle.

with soldermask: (618 Bytes)
without soldermask: (666 Bytes)

for RM 2.54 mm
remaining dam between pads is 0.12 mm then… might need tweaking

Thinking about this a bit more, there is no real need to have all those copper areas defined as pads if a fp_poly could do the same and probably more economical, as those aren’t pads that need to be able to be connected with tracks in pcbnew… I’ll be back.

Yep, that works… (776 Bytes)

If anyone needs a different RM or more detailed arcs (I used 9 sides there) the code is on github.
That python script only produces the 4 leaves… you need to take care of the remainder manually (in the footprint editor) and need to paste the output of the script into the kicad_mod file (with a text editor).

1 Like


I tried the footprint! awesome work and it opens a lot of ideas for me!

where can i get more information about the format of the new kicad modules? I see that the flowerpad is only on the copper layers, but it should be also on the soldermask. Can I extend the fp_poly to other layers and define a pad with size 0?

thank you very much

Prototype boards usually don’t have soldermask, as it just adds to the cost and possible problems due to slices of the soldermask to fail/fall off during manufacturing and causing bad pads… you don’t want those problems. The solder won’t stick to the FR4, no worries, it will work ‘like’ soldermask.

Check the file and the python code… fp_poly seems to only allow one layer per fp_poly definition. That’s why there are the same polys for top and bottom copper. So if you need/want soldermask, you just have to add another fp_poly definition with the layer you want it on… but I wouldn’t do it with those sharp/pointed corners there.

Thank you, i will try to make it. Other software have something like “solder mask expansion” to make the solder mask a little bit bigger to avoid this.

For this board, I will try the solder mask and see the results on the final pcb…

have a nice day!