Skip to main content

kicad-splitplane

Split a KiCad power layer into exactly one continuous copper zone per voltage, computed from where your vias are.

Documentation →

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

Plain Voronoi vs. kicad-splitplane on the demo board

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 and through-hole pad of its net,
  • contain nothing of the other nets,
  • be one continuous surface.

Drawing those outlines by hand is trial and error. kicad-splitplane does it for you and writes the zones straight into a copy of your .kicad_pcb.

Quick start

git clone https://github.com/atuzlak/kicad-splitplane
cd kicad-splitplane
pip install -r requirements.txt        # shapely>=2.0, numpy, scipy, matplotlib

python kicad_splitplane.py examples/demo_board.kicad_pcb --nets +5V +3V3 +1V8

On your own board:

python kicad_splitplane.py board.kicad_pcb --list-nets                      # find the supply 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; the original is untouched), board_splitplane.png (preview) and a copy of the project files (board_splitplane.kicad_pro/.kicad_prl) that keeps your design rules and shows every zone in its preview colour. Open the new board in KiCad, press B to fill the zones and run DRC.

Or install it as a command from PyPI:

pip install kicad-splitplane
kicad-splitplane board.kicad_pcb --nets 5V 3.3V VBUS

(The latest development version: pip install git+https://github.com/atuzlak/kicad-splitplane.)

KiCad plugin

The same tool also runs inside the PCB editor (KiCad 9 or newer). It works on the open board, shows a preview and writes the zones directly into the board as one undo step, so Ctrl+Z removes them again.

  1. In KiCad: Preferences → Plugins → Enable KiCad API.
  2. Open the Plugin and Content Manager, search for kicad-splitplane under Plugins and press Install, then Apply Pending Changes. It is listed in KiCad's official plugin repository, so KiCad offers new versions as updates there. Offline, or to try a version before it is listed: download kicad-splitplane-<version>-pcm.zip from the releases and use Install from File… (uninstall a zip-installed copy before installing from the list, so updates work). KiCad installs the Python dependencies on first use, which takes a minute.
  3. In the PCB editor, click the Split power plane toolbar button, pick the layer and nets, press Preview, then Apply.

The dialog has the same options as the command line, including Gap and edge from design rules (read from the saved project file), Leave keepout areas free and Save HTML report next to the board. It uses the wxPython that ships with KiCad, so nothing else needs to be installed.

For development, link the folder into KiCad's plugin directory instead of installing the zip (e.g. ~/.local/share/kicad/10.0/plugins/, or ~/.var/app/org.kicad.KiCad/data/kicad/10.0/plugins/ for the Flatpak; a Flatpak cannot follow a symlink, so copy the folder together with kicad_splitplane.py there), or run python plugin/splitplane_action.py while KiCad has a board open.

Options

Option Default Meaning
--layer In2.Cu Copper layer to split
--nets Supply nets that share the layer
--list-nets Print supply-like nets with their via / SMD pad counts
--gap 0.5 mm Copper gap between neighbouring zones
--edge 0.5 mm Clearance to the board edge
--min-neck 1.0 mm Warn where a zone gets narrower than this
--res 0.5 mm Routing grid. If a via gets trapped, try 0.3–0.6
--include-smd off Treat SMD pads as vias: preview before you place the power vias
--no-smooth off Keep the raw grid outlines instead of smooth 0°/45°/90° edges
--plain off Skip connecting the vias (faster, may create islands)
--keep-old off Keep existing zones of these nets on the layer (default: replaced)
--rules off Take the gap and the edge clearance from the board's design rules in <board>.kicad_pro: the largest clearance of the chosen nets' net classes (and the board minimum), and the copper-to-edge clearance. --gap/--edge then act as minimums. Custom rules (.kicad_dru) are not read; the log says so
--keepouts off Leave the layer's keepout areas free (rule areas that forbid copper pours, on the board or in footprints): zones are planned around them. Without it, KiCad cuts the zones there when filling, which can disconnect part of a net
--report [FILE] off Also write an HTML report: preview, zones per net, warnings, settings and log on one page (default <out>_report.html; print it from the browser for a PDF)
--no-colors off Don't colour the nets in the copied project file
--out <board>_splitplane.kicad_pcb Output file
--json off Print one JSON object instead of text: ok, zones per net (parts, area_mm2, seeds), warnings, log and the written files. Same files and exit codes; errors give {"ok": false, "error": ...}. With --list-nets: the nets as JSON

Exit code is 0 when every net got one clean zone, 1 when there are warnings.

--rules, --keepouts and --report are opt-in: without them the output is exactly as before. For a board with a project file and keepouts, a typical call is

kicad-splitplane board.kicad_pcb --nets +5V +3V3 +1V8 --rules --keepouts --report

Use with AI agents (MCP)

kicad-splitplane includes an MCP server, so AI agents (Claude Code, Claude Desktop, Cursor, VS Code, …) can split power planes for you: "split In2.Cu between +5V, +3V3 and +1V8 on board.kicad_pcb".

Add it to your client as a stdio server (needs uv):

{
  "mcpServers": {
    "kicad-splitplane": { "command": "uvx", "args": ["kicad-splitplane-mcp"] }
  }
}

Claude Code: claude mcp add kicad-splitplane -- uvx kicad-splitplane-mcp. Without uv: pip install "kicad-splitplane[mcp]" and use the command kicad-splitplane-mcp.

It has two tools:

  • list_power_nets(board_path, all_nets=False): the supply-like nets with their via/THT and SMD pad counts, and the copper layers.
  • split_plane(board_path, nets, layer="In2.Cu", gap, edge, min_neck, res, include_smd, plain, keep_old, out_path, use_rules, keepouts, report): the same as the command line; returns the result as with --json. It always writes a new board (<board>_splitplane.kicad_pcb by default) and never overwrites the input.

The agent cannot fill zones or run DRC; open the new board in KiCad, press B and run DRC afterwards. Agents that read skills can use skills/kicad-splitplane/SKILL.md, which describes the whole workflow and what to do about each warning; llms.txt is a short overview for language models. Scripts can use --json or sp.summary(result) instead.

Each release is published to the MCP Registry as io.github.atuzlak/kicad-splitplane and to PyPI as kicad-splitplane and kicad-splitplane-mcp.

How it works

  1. Seeds. Read the board (a small S-expression parser, no KiCad needed) and collect every via and through-hole pad of the chosen nets that reaches the layer, plus the outline from Edge.Cuts. All other vias, pads and holes on the layer (signals, GND, mounting holes) are read with their real size as obstacles.
  2. Spines. For each net, join all its vias with a tree of 45° paths on a grid (Prim's algorithm with Dijkstra). Paths keep clear of other nets' vias and pads and of spines routed before, never squeeze through gaps too narrow for copper (e.g. between header pins), avoid passages narrower than --min-neck and prefer the middle of free space. All routing orders of the nets are tried; the one with the fewest trapped vias and the shortest spines wins.
  3. Split. Every pad and via keeps a ring of its own net around it. Every other grid cell goes to the nearest spine, measured around obstacles rather than through them, i.e. a Voronoi diagram of the spines instead of the vias. A region grown from one connected spine is connected. The borders are then simplified together (so neighbours keep a shared border) and bent into 0°/45°/90° segments, keeping the exact grid border only around pads where the smooth one would cut a pad ring. The regions are clipped to the outline, shrunk by half the gap and written as KiCad zones.
  4. Check. The tool estimates what KiCad will actually fill (zone minus clearance around other nets' copper) and warns about zones running over another supply's pad, pads/vias cut off from their zone, copper split by rows of pads, and necks narrower than --min-neck.

If a via is completely enclosed by other nets, no continuous split exists. The tool reports it and suggests where to move it:

! 5V: via at (87.59, 56.06) is trapped by other nets -> move it to ~(92.60, 65.46) (10.6 mm fanout)

Library use

import kicad_splitplane as sp

text = open("board.kicad_pcb", encoding="utf-8").read()
r = sp.process(text, "In2.Cu", ["5V", "3.3V", "VBUS"], gap=0.5)

print("\n".join(r.log))
open("board_split.kicad_pcb", "w").write(r.board_text)
sp.render_png(r, "preview.png")
sp.summary(r)        # {"ok": ..., "zones": {...}, "warnings": [...], "log": [...]}

# opt-in: design rules, keepout areas, HTML report
gap, edge, notes = sp.apply_rules(sp.design_rules("board.kicad_pcb", ["5V", "3.3V", "VBUS"]))
r = sp.process(text, "In2.Cu", ["5V", "3.3V", "VBUS"], gap=gap, edge=edge, keepouts=True)
sp.write_report("report.html", r, "board.kicad_pcb")

Website

web/ contains the documentation page; python web/make_figures.py renders its figures. ./deploy.sh builds it as one self-contained file (dist/kicad-splitplane.html), ./deploy.sh --serve previews it locally, ./deploy.sh user@host:public_html uploads it.

Tips and limitations

  • Awkward zones usually mean awkward via placement. Keep each net's vias grouped and use short fanout tracks.
  • Signals on the neighbouring layer use the split plane as return path; avoid routing them across the gaps.
  • Keepout areas are only respected with --keepouts; the edge clearance is also kept from them. Design rules are read from the saved project file, so save the board after changing them.
  • Zones are written as outlines without holes. Smaller zones get a higher priority so an enclosed island still fills; check the order in KiCad's Zone Manager.
  • The command line tool is tested with KiCad 10 files; KiCad 7–9 net syntax is supported too. The plugin needs KiCad 9 or newer. Arcs in the outline are approximated, blind/buried vias are handled roughly.

Tests

python -m pytest tests/        # plugin tests run when kicad-python is installed, MCP tests when mcp is

Feedback and contact

Found a bug, have an idea for an improvement, or interested in collaborating? Write me an email at atuzlak@ethz.ch. Issues and pull requests are welcome too.

License

MIT, © 2026 Aleksandar Tuzlak

Metadata

Release files for kicad-splitplane 0.6.0

For a detailed explanation of source distributions (sdists) and built distributions (wheels), please see the package formats documentation.

Source distribution (sdist)

Source distribution for kicad-splitplane 0.6.0
File Size Uploaded Provenance Actions
kicad_splitplane-0.6.0.tar.gz 35.1 kB With provenance Details for kicad_splitplane-0.6.0.tar.gz

Built distribution (wheel)

Table of built distributions (wheels) for kicad-splitplane 0.6.0
File Interpreter ABI Platform Actions
kicad_splitplane-0.6.0-py3-none-any.whl Python 3 none any Details for kicad_splitplane-0.6.0-py3-none-any.whl

Total release size: 64.4 kB

Release files / kicad_splitplane-0.6.0.tar.gz

Download URL kicad_splitplane-0.6.0.tar.gz
Size 35.1 kB
Tags Source
SHA-256 checksum
How to use checksums
d3ae1740c487b4fb5eba6737b8002b6a2318b1603a5045ad1361be26b12120cf
BLAKE2b-256 checksum
How to use checksums
91ce9f684a78ff8968d5d8db8a06d1a9646f290d6c8bc670670a0bd706b5b84c
Upload date
Uploaded using Trusted Publishing?
What is trusted publishing?
Yes
Uploaded via twine/7.0.0 CPython/3.13.16

Provenance

Provenance describes where a file came from. On PyPI, provenance is shared via attestations, which provide a verifiable record of the build or publishing details. View details, limitations and caveats.

PyPI Publish Attestation

PyPI verified that this artifact, at this checksum, originated from the publisher listed below.

Signed by GitHub Actions, verified by PyPI on Nov 19, 2026.

Transparency log

Release files / kicad_splitplane-0.6.0-py3-none-any.whl

Download URL kicad_splitplane-0.6.0-py3-none-any.whl
Size 29.3 kB
Tags Python 3
SHA-256 checksum
How to use checksums
8c6d4789caded6336a4ec90b399ed0b0297afdb44335eb1695681e9fcb9eb17d
BLAKE2b-256 checksum
How to use checksums
9c552d15d827e81887ee8e05a71d7b226a178de1da6622e031ca8fcbe690ae82
Upload date
Uploaded using Trusted Publishing?
What is trusted publishing?
Yes
Uploaded via twine/7.0.0 CPython/3.13.16

Provenance

Provenance describes where a file came from. On PyPI, provenance is shared via attestations, which provide a verifiable record of the build or publishing details. View details, limitations and caveats.

PyPI Publish Attestation

PyPI verified that this artifact, at this checksum, originated from the publisher listed below.

Signed by GitHub Actions, verified by PyPI on Nov 19, 2026.

Transparency log

Security for kicad-splitplane 0.6.0

Provenance

Provenance describes where a file came from. On PyPI, provenance is shared via attestations, which provide a verifiable record of the build or publishing details. View details, limitations and caveats.

Full provenance

Both files in this release have been uploaded with provenance metadata.

Select from 2 files

Attestation for kicad_splitplane-0.6.0.tar.gz

PyPI Publish Attestation

PyPI verified that this artifact, at this checksum, originated from the publisher listed below.

Signed by GitHub Actions, verified by PyPI on Nov 19, 2026.

Transparency log

A note on package security

PyPI is a repository for distributing packages, not a service for auditing them. While third-party security researchers and our staff do their best to detect and remove malicious packages, PyPI cannot guarantee the quality, security or suitability of any given package.

To learn more about protecting yourself from malicious actors, visit our package security documentation.

Release history Release notifications | RSS feed

This release

0.6.0 This release

2 release files Full provenance

Anthropic, PBC Visionary sponsor Bloomberg Visionary sponsor Hudson River Trading Visionary sponsor Meta Visionary sponsor NVIDIA Visionary sponsor Microsoft Sustainability sponsor Depot Continuous Integration AWS Cloud computing and Security Sponsor Datadog Monitoring Fastly CDN Google Download Analytics Sentry Error logging StatusPage Status page