Different clearence for TOP/BOTTOM of pad

Hi all.
I have a large pad where i will solder a wire for a power output.
The power output in at TOP of the pad and at the BOTTOM there is GND plane.

I would like to change only the bottom of the pad clearance, from the GND plane.
This is because the pad will soldered/unsoldered many time, and eventually will touch the GND plane.

Is this possible? I have not been able to do this.

Yes, with custom design rules.

Try something like:

(rule bottom_pad_zone_clearance
   (layer B.Cu)
   (constraint clearance (min 1mm))
   (condition "A.Type == 'Pad' && B.Type == 'Zone'"))

KiCad also has some mounting holes with via’s inside:

The via’s will keep the pad on the PCB a lot stronger then only the epoxy of the FR4. That epoxy gets quite weak and soft at soldering temperatures.

It is also possible to use different sized pads on top and bottom. KiCad does not support a full padstack (yet), but you can draw a THT pad, and then put a bigger SMT pad with the same pin number on the same location. (You can also turn off the copper on one or more layers of the THT pad)


Thank you for the reply.
I have found a simple solution.
First i have changed the clearance of the pad.
Than, on the top, i placed a fill-zone with no clearance (as i wanted).
This not very elegant , but works.

And also i placed vias in the pad.

1 Like