Help with KiCAD Oddly Shaped Custom Pad Creation

I have a need to create a copper pad that is oddly shaped. Seems like KiCAD is setup to create pads that are square or circle but I’m having a hard time making a pad that is oddly shaped (semi circular to be exact).

My best guess is to draw the shape manually on the copper layer and then embed a small square or circle standard pad within the odd shape that I draw on the copper layer.

Wondering if anyone has any better ideas that are a bit cleaner or easier to implement?

See the attached image. I imported a DXF of the board, so I have the shape of the copper pads… just need a way of turning the shape into an actual pad that KiCAD will recognize.

yes, that is the current workaround. since the request for fully custom shaped pads is rather frequent it might be included in a future release.
for now draw the shape in copper and embedd a pad.

In KiCad 6.0 and Latter you can edit the pad as a graphic shape.
once you are in this mode you can draw on the copper plane and the Drawing will be converted to part of the pad once you exit this mode.

Thank you both for your replies… much appreciated!

I have a follow up question to this topic, wondering if any of you KiCAD power users know of a slick way to overcome this issue I ran into while trying to make my custom oddly shaped pad.

I created a custom footprint to make a semi-circle like pattern using the polygon tool to have a copper fill in the shape I need. Then I just put a regular pad inside the semi-circle pattern to allow KiCAD to recognize I need to connect a net to this semi-circle like pattern.

However, when I run DRC checks I get a bunch of errors because KiCAD does not realize I want the semi-circle pattern that encompass the pad to all be the same net. It has associated the net to the pad but there doesn’t seem to be a way for me to assign the semi-circle copper pattern that I drew with the polygon tool to a specific net.

So the semi-circle copper pattern has no net assignment where as the pad inside of the semi-circle copper pattern does have a net.

I suspect if I built the board with these DRC errors it would actually work just fine as the tool just doesn’t understand what I am trying to do… but I’m a perfectionist and would like to have zero DRC errors if possible.

Anyone know of a work around for this? Is there a way to assign a net to the semi-circle copper pattern in the footprint editor that I didn’t see?

The curved copper polygon area is not a trace or pad, so KiCAD doesn’t understand that it connects the end vias to the centre pad. One way to join this is to add traces inside the polygon area that connect the via to the centre pad, or another option would be to use a pad at each end, where you’re going to connect the vias anyway.

Yes, when the board is made, the vias will connect to the copper area that they appear inside of.

you can specify custom DRC rules to deal with that. a Defproc said it will work as intended but DRC will think there is an error.
Custom DRC rules allow to ignore those, I have set them to ignore silkscreen that goes over board edges. and you shoudl be able to make arule for your desires as well.

Can you post the source DXF? I am curious about a couple options. (1.6 KB)

Here is the DXF file in question.

To be clear, I already have traces inside the semi-circle polygon that connect from the pad in the center to the vias on the ends of the polygon. The traces don’t appear as they are the same red color as the polygon. All the DRC error flags are pointing to the traces within the polygon.

Thanks to everyone for their thoughts, its much appreciated! I will give some of these a try.

Ok, I seem to have it working. Can I upload a video of this to imgur, or is the design private? This forum won’t let me post mp4 videos.

Amazing… thank you!

Yes, you can post it. The DXF doesn’t contain anything particularly proprietary, just board shape.

However, this forum does allow posting of .zip files. So if you zip the mp4 you should be able to post it here.

Whatever option is easiest for you is fine by me.

Many thanks for your help!

Ok, the key here is to turn the outlines of each pad into a filled polygon on the copper layer. Then you can create a pad. Move the pad so it is touching the polygon or inside it. Right click, click “Edit Pad as Graphic Shape”, then right click again and click “Finish Pad Edit”. This will merge the existing pad shape with the other polygon around it.

Now the bad news, I tested this on 7.0RC1. I’m not sure if/how this works in 6.0. I’ve never done pads this way, I was just vaguely aware of the ability.

1 Like

I have done this (or equivalent) in 6.x. You should be fine. If you aren’t seeing the same options in 6.x @kundro85 , let me know and I will go and check what they look like in 6.

Mike, I just implement the steps in your video. Thank you very much for this! You really helped me out here… don’t think I would have ever figured out all those steps on my own! Much appreciated!

I’m glad it worked… I really need to implement a polygon-to-pad easy button or something for 8.0 (7.0 releases soon). I know other devs are working in that area, too.