How to create a power plane (using zones)

This article is about technical aspects of KiCad only, not about using GND or power planes in general.

Working With Power Planes

In short:

  • 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.


Requirements for Zones to Fill

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.

From: Filled Copper Zones not showing up in Gerbers/Printouts/3D view - #9 by bobc

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.

Creating a solid region for one net
Difficulty filling F.Cu with filled zones
Copper pour/filled zone disappears after DRC run
Two questions about filled zones on PCB
PCB design - copper not filling all the board
Selecting pin selects the whole connector
Copper Fill Area Not Working
Aligning Arches In Edge Cuts? *Solved*
Through Hole Association with Power Layers
Change layers name
Tutorial: Introduction to PCB design with KiCad version 5.1 (Getting Started)
Can't fill power zone
Ground fill on F.Cu layer not working for me? [solved]
SMD components - ground plane
Polygons disappear on 'refill' in Gerber plotting
Is this the correct way to do layers and vias...(Basic question!)
How can I hide GND ratsnest or assign parts of ratsnest to different layers?
Ground Plane Setup
Filled areas logic
Copper pour doesn't connect pads, fails DRC
Copy a old board layout into KiCAD
Zone not filled
New fill problem
How do I make a "ground band" around the PCB?
[Solved] Can't place a via onto a copper filled zone
Vias in polygons
Copper zones won't pour
DC to DC converter
Feedback on FAQ topic: How to create a power plane
(Start Here) Frequently Asked Questions
Create Copper Zone from Outline
Filled areas not showing
Filled zones of different nets merge into single filled zone
New to PCB Design. Need Help understanding GND Planes
Insert new schematic into existing PCB design
How does the Copper Zone Properties dialog work?
Zone inside zone - both "no net"
Filled zones not working
Creating a solid region for one net
Can components be connected with a zone fill instead of tracks?

Overlapping zones

Zones can overlap. Overlapping zones on different layers don’t affect each other. If they belong to the same net, you can stitch them with vias; otherwise not.

Zone borders can also overlap on the same layer.


The behavior in that situation depends on the properties of each zone. Naturally the net is important. Another one is priority.

Zones with different nets

When zones belong to different nets, KiCad locigally can’t just know how they should be filled if you haven’t given information about which one should take precedence. If they have the same priority value, they are both just filled. This leads to a situation where you have a DRC violation.


Therefore you have to give them lower and higher priority values (lower value = lower priority). The higher priority zone is filled over the lower priority one, and the lower priority zone isn’t filled in the overlapping area.


Clearance values

Each zone has its own clearance value. This doesn’t override the net class clearance (which is set in the Board Settings). They are both used and the larger one is effective. Thefore, if you have two zones of different nets which have the same priority, the gap between them must be at least as wide as “max(zone1_clearance, zone2_clearance, net1_clearance, net2_clearance)” (i.e. the largest of the four clearance values).


Fine tuning the gap can be avoided by setting the priority values. Then the lower priority zone avoids the larger priority zone and the largest clearance value is effective.

Zones with the same net

If you draw two overlapping zones with the same net and the same priority, KiCad may fuse them together. (The behavior seems to be a bit unpredictable here in version 5.1.4, but you can’t expect them to remain as two distinct zones.)

Zones with different priorities are kept separate, but as of 5.1.4 the result when filling may be something you don’t want.