Odd-shaped pad required


So I’m designing a dot matrix display. Better a strip of them. The displays do communicate via a serial connection. The board will be a strip of several dot matrix displays. This strip can be sawn into smaller parts (say 3 for example) as needed. Or they can be soldered together to form longer strip. Also, the can be stacked in the Y-direction to form even bigger displays. Thats for the background.

This is a very fninnicky design, and I’ll have some challenges in routing. Anyhow, here is my problem:

The first pictures shows two such boards (just copied so the build a strip for two displays). Between those two sections (a single PCB) you see those 5 odd-shaped connections. You might saw right at that vertical line and get two boards, still working. After having sawn them apart, you might change your mind and solder them back together to get a fully two display board again. Also, on the left or right edge, those 5 pads serve as a connection to some MCU. +3V3, GND, LinkLeft, LinkRight, Tx and Tx.

But I don’t get it how I design such a footprint. In the schematic, it is a generic 1 pin connector. Draw a footprint as a poligon, but that one has no pin number, so can’t connect a trace to it.
Thought to put a small SMD-pad within that shape. But the result is shown in picture two:

KiCAD won’t show a ratsnet line. And if I force a connect it doesn’t work too. So I tried a placing a filled zone (net +3V3) over that pad, but, well, no thermal relief for the filled zone of the 3V3 net. Makes sense!

So long storry short:
How do I make a pad with that shown shape that behaves like all the other pads in footprints I have made so long?

Edit: KiCAD 8.0.1 on MacOS.

Thanks for any suggestions.

1 Like
  1. Open the footprint in the Footprint Editor.
  2. Click on the pad to select it.
  3. Press: [Ctrl + E] twice to enter and exit the Pad edit mode.

At the moment you exit the Pad edit mode, graphics that overlaps with the pad will become part of the pad. As a result, also the other layers such as solder mask and solder paste are adjusted to the size of the pad. if you want different aperture sizes for these layers, then disable them in the pad, and draw a new “aperture pad”. (Aperture pads do not have copper, nor pad numbers, and are only for the other technical layers).

From your intention, I inver it’s probably best to enable the solder mask layer (so a cutout in the solder mask is made), but disable the paste layer, because you do not want to use these pads during initial production.

1 Like

That was easy! I didn’t know of that edit mode.

Thanks a lot for your quick solution!

A lot of things are easy once you’ve learned how to do it. even communicating in a foreign language becomes easy after a bunch of years of practice :slight_smile:

1 Like

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