How to build a customized pad? - pcb spark gap

Hello to everyone.

I’m new using Kicad and I was trying to do a PCB Spark Gap for my PCB but I have a problem.
My spark gap should look like that:


This is what I got:

The pad nº1 is fine, but the other one I can’t find a way to make it be marked as a pad.

I tried to do it with the customized option in pad properties but if it is not a polygon it isn’t marked as part of the pad.
Also, I did it with the right toolbar options but after selecting every line, I can not convert it into a pad because the anchor is not in the center (I tried to place it but still appears an error).

Any help is appreciated,

I added an image of a real example and changed the title a little, to get you more traffic :wink:

1 Like

Thank you, I noticed that now,
It looks more understandable! Really appreciated :slight_smile:

1 Like

If you create an anchor pad and arc like so:

then select them and right click, select “Create pad from selected shapes”.

1 Like

the reference pad needs to overlap with your graphical elements. All graphical elements need to overlap each other.

So how to build your part

First draw your arc from multiple arcs and a line. I chose to have an outer radius of 3mm and a with of 0.6mm but a maximum corner radius of 0.1mm (arbitrary for demonstration purposes.)
This means my line thickness of the arcs can be 0.2mm and i need 3 arcs to fill the “pad”.
Place 3 arcs with center at (0, 0), angle = -180°, linethickness=0.2 and starting points at (2.9, 0), (2.7, 0), (2.5, 0) respectively. The layer you place them on is unimportant for now. (I used F.SilkS)
At the end you should have something looking like this:

Now also add a line connecting the endpoints of the inner and outer arcs. Linethicknes again 0.2mm (best done using the grid setup with 0.1mm for my measurements)
After that it looks like this:

Add a polygon with your desired linewidth and shape to form the sharp point. (I chose 0 linewidth to get a really sharp point)

place a rectangular smd pad somewhere inside the covered are where the sharp point meets the arc.

Select the pad plus the arcs and lines and the polygon, right click -> create pad from selected shapes. The result will look like this:

An alternative option is the use of freecad and kicad stepup. This allows you to create the pad shape in a parametric CAD program and export it as a pad to kicad. Kicad StepUp: The Sketcher for Footprint generation


Could you explain how I can do that please?
I’m really new with the software and I don’t know all the functions.

I mean the first image, the second one is not the problem

Okey, reading it more carefully I think I understeand now what do you mean with your 2nd reply. I will try to do it and I will post here my results or if I get stucked at any point. Thanks!!

okey, thats my result:

the width should be less because I want it of 0,1mm but now I only have to play with the width of the filling arcs and try to be more accurate. Thanks @Rene_Poschl !

My question now is:
when I try to route the tracks, the track from the pad nº 2 will start from where I placed the little pad right? so in case I want to start the track from another part of this pad I have to descompound the pad, move the small pad and create the big one again right?


(I don’t have version 5.0 yet, so I don’t have experience with the Custom Pads feature and the following suggestion may not work for you.)
You should be able to scatter multiple instances of the “small pad” along the arc - say, every 45 degrees - to create places for tracks to start from. Just be certain that EVERY ONE of those multiple pads has “Pad 2” assigned as the pad number.


There can be only one special anchor pad for the custom pad, but once it’s ready it’s possible to add independent pads along the arc, as Dale said. At least in the latest self-compiled version it works so that when you draw a track to one of those pads they are all connected. So you can choose which pad you use when routing.

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