This article is about technical aspects of KiCad only, not about using GND or power planes in general.
- KiCad uses zones for planes
- Zone is a copper area which can have an associated net and which can be filled automatically
- KiCad doesn’t normally fill isolated areas (and normally you shouldn’t even try that because it’s not electrically good)
- For a zone to be filled, a pad of the same net must be inside it or connected to it
- A via triggers filling, too, if it’s connected to a pad directly or indirectly
- Zone fill does not update automatically; use the B hotkey to (re)fill (Or run DRC with the refill option selected)
- You can have zones of the same net in different layers which overlap and put a via there, the via will automatically be in the same net (that kind of connection with vias is called via stitching)
In KiCad a layer cannot be set up as a power plane functionally. You can select something which looks like it in the board setup, but actually it does nothgin in KiCad (it just gives information for autorouters when exporting data for them).
Instead, you have to create a zone.
Select the layer as active layer, here In2.Cu is active:
Select the zone tool, click on the board and select the net for the zone. You can select the layer here, too, and the same zone can exist in several layers:
Click OK, draw a polygon and you have a plane for your selected net. Just draw a rough rectangle outside the board edges if you want the plane to fill the whole board area.
Planes only fill if they have a connection to a pad of the correct net in some way. This connection can be done by having the center of a pad inside the zone area, by connecting using a trace or by the use of a via.
Not shown in the picture is the new option of version 5 to connect two zones of the same net using a via (so called stitching vias).
Use the B hotkey to (re)fill all zones; make sure that the visibility setting is set as “Show filled areas” with the relevant left hand toolbar button.