Pour won't enclose pads and copper polygons of the same net

I have an oddly shaped footprint (MAX77715, FC2QFN) and I’m trying to connect the pads to a pour of the same net. However, the pads won’t connect to the pours even when the pour fully encloses them. They have to be manually connected by a track. While this satisfies the DRC, it leaves gaps highlighted by the yellow boxes in the image below. Any idea how I can resolve this? I have also attached the footprint and the project files.

Charger 18650 rev A.zip (27.8 KB)
MAX77751CEFG.kicad_mod (20.2 KB)

Is the zone associated with BATT+ net? looking at the clearance markers, its indicates it is not

Same problem with GND at pins 18,19.
Pads 13,14,18,19 are covered by filled polygons in the footprint. (Filled) polygons are graphic items, not zones or traces or pads or something.
To achieve what you want, you have to use custom shape pads.

1 Like

SnapEDA has a footprint that actually works available for download.
There is a symbol and a 3D model as well. You have to use their symbol along with the footprint for pin/pad naming reasons.
Download is free, you need to register but there is no spam or something.

I see. So even if they are on the copper layers, they do not act the same way as the pads and nets they are tied to. I had to change the Pad Connections to Solid in the SnapEDA footprint for it to work.

Thank you for your help!

They are not tied to any net. That’s the whole point. They are just graphics - like logos - that happen to be on a copper layer.

The way to fix this in KiCad is:

  1. Open the Footprint in the Footprint Editor.
  2. Combine the Graphic polygon with one of the pads to make it a “complex pad”.
  3. Turn the other pad into an “Aperture pad”.

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