Help with this custom pad


Today I was trying to make a custom footprint for an inductor

This is the recommended layout:

I tried to create a dxf, and then, import on my board. But I dont know how to make a pad or a polygon with this :?

I dont know how to continue here. Maybe I can use only few squared pads, and forget the semi circular area, or there is a way to generate a pad with that particular shape.

Any idea?

have a nice day!

In kacad stable your options are very limited.
I fear the best you can do is to approximate the pad shape with a lot of small overlapping pads.

I think kicad nightly already includes polygon pads. (Not sure how well implemented the interface for these is.)

There is an example for such a connector in the official lib.
See Connectors:SMA_SMD_Jack_Straight

1 Like

it seems this is just done as a patchwork of rectangles, not with polygon pads…
(I probably misunderstood your comment :slight_smile: )

I’m not sure if the polygonal pads feature is fully implemented in nightly

The example is from the old kicad 4.x repo. So yes it shows how this can be done in 4.x stable

1 Like

Instead of making outline pads, make them as solid areas. Import the dxf into the footprint editor, change the layer to F.Cu.

Then add a (tiny) pad from the editor onto each pad.

Now for each pad you have a tiny pad and a pad with your custom shape overlapped. The tiny pad will be the logical pad, the track should be connected to its centre. Be careful with the DRC, since it is likely the DRC will only check the tiny pad inside the custom shaped one.


Yes this is the case. DRC does not support copper features other than pads. (At least in 4.x stable)

I suspect that a reasonable approximation can be done by overlapping a pair of trapezoidal pads with a rectangle or two.

What is the technical justification for this pad shape? I’m guessing that the circular gap in the center is to avoid the “shorted turn”, or induced current, effect of placing copper directly under the inductor core, but there may be other reasons. Do the component contacts actually have this shape? Are they perhaps trying to increase copper area, for heatsinking? I suspect that straight-line approximations to the circle are quite adequate.


my point was only on the polygon pads, which I would like to know how to create, not on the fact that the suggested method would give a good approximation of the required pads (by the manufacturer DS).

The pads of type Custom Shape have the clearance around all the shape. Violations are caught by DRC. (This all, of course, in daily builds.)

This is how a custom shaped (polygon) pad can be created:

  1. Create a filled polygon on other than copper layer.
  2. In its Properties change the layer to a copper layer.
  3. Still in Properties, change one of the points to other than 0 (don’t ask me what they are and why, you can try with all zeros…).
  4. OK. Accept.
  5. It’s on a copper layer. Select it and in the context menu select Create Pad from Selected Shapes.
  6. Open Properties of the created pad. Open the Custom Shape Primitives tab.
  7. Select the polygon and click the Edit Primitive button.
  8. Change outline thickness to 0. Accept.

However, I don’t know if it’s possible to create or use closed shapes with arcs.



I tried some of your answers, and I got this solution, with rectangles and trapezoids

Not the most beautiful footprint on the planet, but it will work

cant wait to see the custom pad feature in the stable version :slight_smile:

Have a nice day!