Stitching Layers Between Copper Zones

Stitching is the practice of adding vias between filled zones on adjacent layers of a PCB to assure that everything is at equal potential throughout both zones. This is something you typically do if you have filled (i.e., flooded) the unused spaces on both top and bottom of your board with copper and have connected the floods to ground or some other reference.

The KiCad FAQ outlines a process for doing this, and it works fine until you refill (i.e., re-pour) the zones–or the DRC refills them for you. When the zones are refilled, the vias you added for stitching become isolated from the zones and end up as little pads floating in space.

The problem and a workaround was discussed in a thread on the kicad-users mailing list. Here's a slightly less terse summary of what you need to do:

1. Route the board and define your zones as you always have.
2. Fill the zones as you always have.
3. Select “Add tracks and vias” from the toolbar on the right.
4. Click on an existing pad that’s connected to the zone’s net, drag the pointer a little bit to create a short track, then either right-click and select “Place Via” or type the ‘V’ shortcut.
5. To add more stitching vias, continue to drag the pointer and type ‘V’ where you want to drop vias (or right-click and select “Place Via”).
6. When you are done placing vias, hit the ‘End’ key on your keyboard (or right click and select “End Track”).

You can repeat this as many times as you want to create different clusters of stitches. When you refill zones, the vias will retain the connectivity information and work as expected.