Not able to connect traces to this antenna footprint

I hereby certify that I am not simply asking someone else to design a footprint for me.

This is an auto-generated message that is in place on the “footprints” section of the forum. If I remove it and ask for a footprint to be designed anyway, I understand that I will be subject to forum members telling me to go design my own footprint or referring me to a 3rd party footprint site.

I created this nrf24L01P antenna footprint based on the reference application and layout given in the datasheet. Since I could not draw tracks in the footprint, I created lines on the F.Cu layer and then merged a connection pad with them. However, pcbnew won’t let me connect a trace to that pad. I know I can create a copper fill but is there a way to use this footprint since this has precise lengths and shape?

nRF24L01P-antenna.kicad_mod (635 Bytes)

[Edit] Brainfart:
The proper way to modify your footprint is to select the pad and the lines, then right click on it and select “Create pad from selected shapes” from the popup menu.

I am having some issues with your footprint in V5 after I opened it in KiCad V5.99, and did not investigate further. This should be enough info to get you going.

I could indeed not draw a track to the pad in your footprint.
The line was preventing me to do so.

I think the “NetTie” footprints use a polygon to draw some copper to connect two nets together, but it’s also quite a kludge, and on the list of things to be fixed at some time in the future.

A common way to make complicated pads in KiCad is to use multiple pads with the same pad number. So I did a little test to replace the first line segment with a pad, then put it in a schematic and on a PCB and I could draw a track to the (first) pad normally.
It looks like:

I also ran DRC and got no errors. It could be because DRC accepts a line and a pad that overlap as as normal, or maybe DRC is not able to check for lines at all.

Your modified Footprint:
nRF24L01P-antenna_copy.kicad_mod (1.0 KB)

It was just a quick check. For a full conversion it’s probably better to use pads only to draw your footprint, and then also turn of the solder mask layer so the copper is not exposed.

1 Like

This really worked well! Thanks!

1 Like

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