kicad-splitplane

Split a KiCad power layer into one continuous copper zone per voltage, computed from where your vias are. Runs as a KiCad plugin or from the command line.

Available in KiCad's official Plugin and Content Manager: search for kicad-splitplane and press Install. See Install.

On a 4-layer board the inner power layer is often shared by several supplies (5V, 3.3V, 1.8V…). Each supply needs its own zone, and each zone has to contain every via of its net, nothing of the other nets, and be one continuous piece of copper. Drawing those outlines by hand is trial and error. This tool does it for you: it connects each net's vias with a path, splits the layer around those paths, and draws the borders with straight 0°/45°/90° edges.

KiCad plugin

Needs KiCad 9 or newer on Windows, macOS or Linux. The plugin works on the board that is open in the PCB editor and writes the zones straight into it as one undo step.

1. Enable the KiCad API (once)

In KiCad: Preferences → Preferences… → Plugins, tick Enable KiCad API, press OK and restart KiCad.

2. Install the plugin

kicad-splitplane is listed in KiCad's official plugin repository, so you can install it from within KiCad:

1. In the KiCad project manager open Plugin and Content Manager.
2. On the Plugins tab, search for kicad-splitplane and press Install.
3. Press Apply Pending Changes.

Updating: when a new version is out, KiCad offers it as an update in the Plugin and Content Manager.

Without the Plugin and Content Manager (offline, or to try a version before it is listed): download kicad-splitplane-<version>-pcm.zip from the latest release on GitHub, don't unzip it, and use Install from File… (bottom left of the Plugin and Content Manager). If you installed the zip before, uninstall that copy first and then install from the list, so KiCad can offer updates.

3. First run

Open a board in the PCB editor. A new Split power plane button appears in the top toolbar (also under Tools → External Plugins). The first time you press it, KiCad installs the plugin's Python packages (numpy, scipy, shapely, matplotlib) in the background. That takes a minute or two and shows nothing; just wait, then press the button again if no window has appeared.

Using it in KiCad

1. Place the power vias first. Each supply needs at least one via or through-hole pad that reaches the plane layer. If you have not placed them yet, tick Use SMD pads as stand-in vias to get a first impression of the split.
2. Press Split power plane in the toolbar.
3. Choose the Layer to split (e.g. In2.Cu).
4. Tick the nets that share this layer. The list shows supply-like nets with their number of vias/THT pads and SMD pads; tick show all nets if yours is missing.
5. Press Preview. The split appears on the right, other nets' pads and vias in grey, and the log below. OK: one zone per net means the split is clean.
6. Press Apply. The zones are written into the board and filled. Existing zones of the selected nets on that layer are replaced.
7. Close the window, check the result and run the Design Rules Checker. Ctrl+Z removes all zones of one run at once.
8. Optional: zones in their own colours. In the Appearance panel open the Nets tab, right-click each supply net → Set Net Color…, and set Net colors at the bottom to All. The log after Apply lists the colours of the preview. (The command line does this for you.)

Settings in the dialog

What the warnings mean

Command line

Needs Python 3.9+. Works on Linux, macOS and Windows; you don't need KiCad installed.

git clone https://github.com/atuzlak/kicad-splitplane
cd kicad-splitplane
pip install -r requirements.txt

# which supply nets does the board have?
python kicad_splitplane.py board.kicad_pcb --list-nets

# split In2.Cu between three nets
python kicad_splitplane.py board.kicad_pcb --layer In2.Cu --nets 5V 3.3V VBUS

This writes board_splitplane.kicad_pcb (your board plus the zones), board_splitplane.png (preview) and a copy of the project files that keeps your design rules and shows every zone in its preview colour. Your original files are left alone. Open the new board in KiCad and press B to fill the zones.

Options

From Python

import kicad_splitplane as sp

r = sp.process(open("board.kicad_pcb").read(), "In2.Cu", ["5V", "3.3V", "VBUS"])
print(r.log)
sp.render_png(r, "preview.png")

How it works

1. Read the board. All vias and through-hole pads of the chosen nets on the layer, the board outline, and every other via, pad and hole with its real size. Other nets' copper is an obstacle: a zone has to keep its clearance to it.
2. Connect each net. The vias of each net are joined by a tree of 45° paths that keep away from other nets, never squeeze between pins where no copper fits, and avoid narrow passages. All orders of the nets are tried and the best one wins.
3. Split. Every pad keeps a ring of its own net. The rest of the layer goes to the nearest path, measured around obstacles. A region grown from one connected path is itself connected, so no net breaks into islands.
4. Clean up and check. The borders are straightened into 0°/45°/90° segments, but only where that does not cut a pad or create a neck. Finally the tool estimates what KiCad will actually fill and reports anything that would not work.

Good to know

• If the zones look awkward, move the vias: keep each net's vias together and use short fanout tracks.
• Don't route signals on the neighbouring layer across the gaps between zones. The split plane is their return path.
• Smaller zones get higher priority, so an island inside a bigger zone still fills correctly. Check the order in KiCad's Zone Manager.
• The plugin needs KiCad 9 or newer. The command line works with files from KiCad 7 to 10. Arcs in the board outline are approximated.

Changes

• November 2026: listed in KiCad's official Plugin and Content Manager.
• 0.4.1: the command line also writes a copy of the project files, so the new board keeps your design rules and shows every zone in its own colour; the plugin explains how to colour the zones and gives a clear message when two KiCad windows compete for the API.
• 0.4.0: pads and vias are handled with their real size; every pad keeps a ring of its own net; other nets' pads, vias and holes are obstacles (no more zones squeezed between header pins); smooth 0°/45°/90° outlines; more precise warnings. Thanks for the feedback from testing it on a 5-supply course project.
• 0.3.1: fixes the plugin window not opening in KiCad.
• 0.3.0: first version of the KiCad plugin.

Thanks

Thanks to Alfonso Blanco Fontao for teaching the Applied PCB Design course at ETH Zürich, which got this project started, and for reviewing the first version and testing it on the course project. His feedback shaped version 0.4.0.

Feedback and contact

Found a bug, have an idea for an improvement, or interested in working together on this? I'd be glad to hear from you. Write me an email at atuzlak@ethz.ch.

Bug reports and pull requests are also welcome on GitHub.