KiCad Routing Tools
A fast Rust-accelerated A* autorouter for KiCad PCB files. Compatible with KiCad 9 and KiCad 10. Available as both a KiCad Plugin with full GUI and a Command-Line Interface for scripting and automation.
📊 Project metrics — installs, downloads and traffic, updated daily.
Free and MIT-licensed. Donations cover the ~$500/month of cloud compute and AI development behind it.
Also via GitHub Sponsors or PayPal — see Support.
Contents
- Support — donate via Ko-fi, GitHub Sponsors or PayPal
- Features
- Quick Start
- KiCad Plugin — GUI, the Auto tab (the Autorouter, AI routing and placement, labels), installation
- Command-Line Interface — routing, planes, verification
- Documentation — full guide for every feature
- Project Structure & Module Overview
- Performance
- Command Reference — options per tool (full list:
--help/ configuration.md) - Project metrics — installs, downloads and traffic
- Requirements · Limitations · Contributing · License
Support
KiCadRoutingTools is free and MIT-licensed, and it stays that way — there is no paid tier, no feature held back, and nothing in this repository is paywalled.
Donations go to what it costs to build and maintain it: about $500/month of cloud computing and AI-assisted development.
The compute is not incidental. Every change to the router is A/B-tested by replaying a corpus of real open-source boards on rented cores and grading each one for DRC violations and unconnected nets, and the ~770-file test suite fans out the same way. It is what stops a change that helps one board from quietly breaking ten others.
- ☕ Donate on Ko-fi — card or PayPal, no account needed.
- GitHub Sponsors — one-time or monthly, billed with any other projects you sponsor.
- Prefer PayPal directly? paypal.me/DrAndyHaas (the sender needs a PayPal account).
Features
Fast, grid-based A\* routing with a native Rust core (~10× faster than pure Python): octilinear (H/V/45°) multi-layer routing with automatic vias, and batch routing with incremental obstacle caching. Highlights below link to the full deep-dive docs.
Core routing
- Rust-accelerated A\* pathfinding, multi-layer with automatic via insertion
- Rip-up and reroute — progressive N+1 blocker analysis, ripped-corridor avoidance
- Net ordering strategies — MPS (crossing-aware), inside-out, original, or bus-first, with MPS layer swaps
- Stub layer switching, vertical track alignment, turn-cost straightening
- Board-edge (Edge.Cuts arcs/cutouts), keep-out rule areas, and auto BGA exclusion zones — see Configuration
- Direction-aware stub / BGA / track proximity penalties
- Pose-based A\* with a Dubins heuristic and adaptive setback angles for orientation-aware centerlines
- Bare-pad, multi-point (3+ terminals), and hybrid (coupled middle + single-ended legs) routing
- Automatic polarity resolution (opt-in pad swaps), U-turn prevention, GND return-via placement
- Electrically-short legs auto-defer to single-ended; per-layer impedance-controlled widths
- Wider power-net routing with automatic neck-down at fine-pitch pads
- Plane pours (pads are welded by the route step, #562) and plane layers several nets share (split round spines routed on the layer) with resistance / max-current reporting
- Disconnected-plane-region repair (region joins + pad taps) and GND return-via placement
- Length matching — trombone meanders, auto DQ/DQS grouping, via-barrel aware
- Time matching — propagation delay, microstrip vs stripline
- Bus routing, plus guide corridors and keep-out zones drawn on a User layer
- Placement by function: parts sorted into functional groups, one objective annealed (
place_simple.py) over 12 seeds (6 started scattered, 6 with each group gathered), and a fast route (route.py --quick 2) of the 6 the objective rates best to keep the best (/plan-pcb-placement) - The design brief — state what the board is FOR, in a sibling the toolchain reads: which connectors are user-facing, which edge each belongs on and where along it
- Parts under other parts — part heights read off the 3D models, so a low part may stand under a module or shield can where it fits; a card in its socket (M.2) or a module on a stacking connector is declared in the brief and moves with its connector, admitting only parts known to fit under it
- Floorplan intent, graded — declare where parts belong and check the board against it, so "the render looks fine" stops being a verdict
- BGA / QFN fanout with decoupling-cap placement cleanup, Hungarian target-swap, and schematic sync
- Post-route copper cleanup reconciled against the connectivity model (no orphaned or ripped-and-not-restored copper), with gap-snap connectors
- KiCad-oracle reconnect — routes the exact links KiCad's own DRC reports as unconnected
- Checkers for DRC, connectivity, orphan stubs, copper hygiene (
check_weird.py), and pad geometry
- Full KiCad plugin GUI (KiCad 9 & 10) and a scriptable CLI
- AI assistance — an Auto tab that runs the Autorouter, plans an entire routing workflow or places a board by function, per-field "Ask AI" helpers, and datasheet-driven power / high-speed / diff-pair analysis
- Board rendering — fast geometry PNG renderer (
route_render.py), placement stills (render_placement.py), a board's power components (render_power.py), and movies of a routing run (route_movie.py, made for every stress run) and of a placement, or the placement skill's whole flow through to the full route (place_movie.py) - Routing plans as files — save/load a whole routing chain as JSON: build one from a recorded command chain (
make_plan.py), run it headless through the real plugin (run_plan.py), or load it in the GUI
Quick Start
1. Get the Code
# Clone with git
git clone https://github.com/drandyhaas/KiCadRoutingTools.git
cd KiCadRoutingTools
Or download the ZIP and extract it.
Commands here use python3. On Windows, use py -3 (or python) if python3 is not found.
2. Install Python dependencies
Install dependencies into the interpreter that will run the CLI:
python3 -m pip install -r requirements.txt
The KiCad plugin uses KiCad's Python. See Requirements for details.
3. Install the Rust Router
python3 build_router.py
By default this downloads a prebuilt binary for your OS from the project's GitHub Releases — no Rust toolchain required. Prebuilts are published for:
- Linux x86_64
- macOS arm64 (Apple Silicon)
- macOS x86_64 (Intel)
- Windows x86_64
Building from source (optional)
If you'd rather build locally — or you're on a platform without a prebuilt — install Rust from rustup.rs:
# macOS / Linux
curl --proto '=https' --tlsv1.2 -sSf https://sh.rustup.rs | sh
Windows: Download and run rustup-init.exe from https://rustup.rs/
After installation, restart your terminal or run source ~/.cargo/env, then:
python3 build_router.py --from-source # build locally instead of downloading
python3 build_router.py --tag v0.15.0 # download a specific release
python3 build_router.py --clean # remove all build artifacts
4. Choose Your Interface
To route a whole board automatically, use one of two ways -- and an AI assistant asked to route a board with this package should do the same:
python3 py_router/autoroute.py board.kicad_pcb routed.kicad_pcb(Option C): no
- the
/plan-pcb-routingskill (Option B): an agent analyzes the board, plans the
Option A: KiCad Plugin (Recommended for interactive use)
# Install the plugin
python3 install_plugin.py
Then in KiCad: Tools → External Plugins → KiCadRoutingTools
Option B: Claude Code (AI-assisted routing)
Use Claude Code to analyze your PCB and generate a routing plan:
> /plan-pcb-routing kicad_files/my_board.kicad_pcb
Claude will:
- Analyze your board structure and identify components needing fanout (BGA/QFN/PGA)
- Detect differential pairs and DDR signals requiring length matching
- Identify power/ground nets and recommend plane vs trace routing
- Assess signal speeds and recommend GND return via placement
- Generate a step-by-step routing plan with explanations
- Run the commands and verify results
> /find-high-speed-nets kicad_files/my_board.kicad_pcb # Identify high-speed nets via datasheet lookup
> /analyze-power-nets kicad_files/my_board.kicad_pcb # Identify power nets and track widths
> /identify-diff-pairs kicad_files/my_board.kicad_pcb # Find diff pairs by pin function, recommend gap/impedance
> /recommend-stackup kicad_files/my_board.kicad_pcb # Stackup advice for impedance/time-matching accuracy
> /recommend-plane-mappings kicad_files/my_board.kicad_pcb # Which nets get planes, on which layers
> /diagnose-routing-failures my_board.kicad_pcb /tmp/route_output.txt # Root-cause failed routes, get a retry command
> /review-routed-board my_board_routed.kicad_pcb # Post-route QA: DRC, connectivity, length match, GND vias
> /plan-pcb-placement full kicad_files/my_board.kicad_pcb # Group, place 12 seeds, fast-route the 6 cheapest, keep the best, route end to end
See Claude Skills for what each skill does and how they fit together.
All of these are also available inside KiCad without leaving the plugin - see AI assistance in the plugin below. The plugin can run the analysis and routing skills through opencode instead of Claude Code (issue #503) - a Backend dropdown on the Auto tab selects the agent CLI, and opencode's provider/model strings open the door to other model providers. The placement runs need Claude Code, because they write files and opencode's analysis agent may not. The skills' output contracts are tuned on Claude models; smaller models may follow them less reliably.
Option C: Command Line -- route a whole board with autoroute.py
# Route the whole board: planes, fanouts, decap clearance, diff pairs and route
passes, chosen from the board's own rules, footprints and nets
python3 py_router/autoroute.py my_board.kicad_pcb routed.kicad_pcb
See its plan first, without running anything
python3 py_router/autoroute.py my_board.kicad_pcb routed.kicad_pcb --dry-run
Every step it ran, with its log and board, is in routed.kicad_pcb.autoroute/
(plan.json there records the chain and each pass's grade), and its last line,
AUTOROUTE_SUMMARY, names the shipped step with its open nets and DRC. See
autoroute.py. The
plugin's Auto › Autorouter tab runs the same script on the open board.
Option D: A hand-built chain (the manual / expert path)
When a board needs steps autoroute.py does not take -- impedance control, length
matching, keep-away rules, buses, a particular plane map, or a net class that is a
real requirement rather than aspirational -- run the tools yourself, the kind of chain
/plan-pcb-routing plans:
If the parts need placement, place them first by their functional groups (see the
placement guide) and use the placed board as
my_board.kicad_pcb in this chain:
python3 py_placer/place_simple.py unplaced.kicad_pcb my_board.kicad_pcb --groups groups.json --intent intent.json
# Pour the planes FIRST (#562): the fanout's plane-drop vias then land on
real fill, and the route step welds plane pads into it.
python3 py_router/route_planes.py my_board.kicad_pcb poured.kicad_pcb --nets GND --plane-layers B.Cu
Fan out a BGA, then tidy decoupling caps off the new vias (issue #130)
python3 py_router/bga_fanout.py poured.kicad_pcb -c U1 -o fanned.kicad_pcb --clearance 0.1
python3 py_placer/place_fanout_clearance.py fanned.kicad_pcb capclean.kicad_pcb --clearance 0.1
Route differential pairs (the output is positional: route_diff's -o is --ordering)
python3 py_router/route_diff.py capclean.kicad_pcb diffed.kicad_pcb --nets "lvds"
Route ALL remaining nets, plane nets included (their widths via --power-nets).
This step ends with the in-run plane finalize that completes the planes.
python3 py_router/route.py diffed.kicad_pcb routed.kicad_pcb --nets "*" \
--power-nets GND --power-nets-widths 0.3
KiCad Plugin
The plugin provides a full graphical interface for all routing features, running directly within KiCad 9 or 10.
AI assistance (Auto tab)
With Claude Code or opencode installed, the routing dialog gains AI assistance throughout (the plugin spawns the selected agent CLI headless, streams a live transcript, and fills GUI controls from the results). The Backend dropdown on the Auto tab picks the CLI: Claude Code runs Anthropic models; opencode takes provider/model strings for many providers (including its built-in free tier), with opencode auth login adding provider accounts. Both discover the same .claude/skills/; opencode runs them under a read-only pcb-analysis agent defined in opencode.json (the equivalent of the Claude run's read-only tool allowlist). Neither grants a dedicated write tool, though both grant Bash, so neither is a sandbox — the allowlist states intent, and --allowedTools auto-approves rather than restricts. Both can dispatch a subagent, so an analysis skill can hand its close-out to an independent verifier (#552): the Claude allowlist grants the dispatch tool per run, and the pcb-analysis agent grants opencode's task tool in opencode.json. A caller asking opencode for a tool set naming Write/Edit is refused rather than silently downgraded.
The tab has two sub-tabs:
- Routing - Plan Routing runs
/plan-pcb-routing: the plan fills the parameter fields across the tabs and appears as a checkable step list, which Run Selected Steps executes sequentially in-process on the live board with per-step status marks. Review Routed Board and Diagnose Routing Failures give post-route QA and failure root-causing. Backend, model, and effort selectors control every AI run and persist with the dialog settings (model/effort remembered per backend). - Placement - Place (AI) and Place + Route (AI) run
/plan-pcb-placement place/fullheadless into akrt_placement/folder beside the board. The tab shows the seed candidates with a preview, a status line read from the run's milestone ledger, and at the end REPORT.md; Apply Result to Board moves the open board's parts to the result's poses and locks (and, after Place + Route, its routed copper). These two need Claude Code. Beautify Labels (no AI) tidies the reference-designator silkscreen (py_placer/beautify_labels.py). - Save / Load a plan - Save… writes the generated step list to a JSON file; Load… reads one back and runs it with no Claude call — handy for replaying a workflow that worked on another board. A recorded command chain converts to a loadable plan too (
python3 py_router/make_plan.py; see Plans from the command line). - Per-field "Ask AI" buttons - power nets/widths (Route tab), stackup check (Layers), differential-pair verification by pin function (Differential tab), net-to-plane layer mappings and GND return via distance (Planes tab).
Installation
Three ways to install:
A. KiCad Plugin and Content Manager (PCM) — the recommended path for end users, and it needs no extra repository URL: the package has been in the official KiCad repository (the one KiCad ships with, gitlab.com/kicad/addons) since v0.15.6. Open the PCM from the KiCad main window, leave the repository dropdown on KiCad official repository, go to the Plugins tab, search for routing, select KiCad Routing Tools and click Install, then Apply Changes at the bottom. If it is not listed, the PCM is serving a cached catalogue — press Refresh and look again. Versions are published with status testing rather than stable, which the PCM shows in the Status column but does not hide or block; kicad_version is a minimum, so the 9.0 entry installs on KiCad 10 as well. On first launch, the plugin checks the Python packages listed in requirements.txt (numpy, scipy, shapely, and the optional Pillow, without which only board renders and the placement preview are off) and offers a one-click pip install for any that are missing or too old into KiCad's Python. Do not assume KiCad supplies them: what it bundles varies by version and platform, and KiCad 10 on macOS ships no numpy at all. The check reports the version and the file path the running interpreter imports — KiCad's Python is often not the one pip show numpy answers for in a terminal.
B. PCM "Install from File…" using the release zip — for a release newer than the one the official catalogue currently carries, for a pinned older version, or for an offline machine. Each GitHub Release ships a ready-to-install PCM package zip named KiCadRoutingTools- (a single cross-platform archive bundling the prebuilt Rust binaries for all platforms — not the auto-generated "Source code (zip)"). To install it:
- From the Release's Assets, download
KiCadRoutingTools-(e.g..zip KiCadRoutingTools-0.15.13.zip). - In KiCad, open Plugin and Content Manager from the main window.
- Click Install from File… (bottom of the PCM dialog) and select the downloaded zip.
- Click Apply Pending Changes, then restart KiCad if prompted.
scipy/shapely dependency check described in (A) applies. This path keeps the plugin manageable from the PCM (you can update or uninstall it there), unlike the manual install below.
C. Manual install from source — for development or for using the CLI tools as well:
# Install the plugin (copies to KiCad plugins directory)
python3 install_plugin.py
For development: create symlink instead of copying
python3 install_plugin.py --symlink
Remove the plugin
python3 install_plugin.py --uninstall
Skip installing the Python dependencies
python3 install_plugin.py --no-deps
The installer installs into every KiCad version it finds (version directories and install roots are discovered, not taken from a fixed list), under:
- macOS:
~/Documents/KiCad//3rdparty/plugins/ - Linux:
~/.local/share/kicad//3rdparty/plugins/ - Windows:
~/Documents/KiCad//3rdparty/plugins/
requirements.txt into KiCad's Python with pip, and skips pip when that Python already has everything. On Linux, KiCad runs the system Python, which Debian 12+, Ubuntu 23.04+, Fedora 38+ and Arch mark as externally managed (PEP 668) so pip refuses to install into it; there the installer runs no pip and prints the apt / dnf / pacman command for whatever is missing, plus the explicit --break-system-packages override for a package your distribution does not carry.
If you previously installed this plugin through the Plugin & Content Manager, that copy sits next to the local install and would shadow it on sys.path (causing stale-code errors). The installer detects any such PCM copy and moves it aside to , leaving it recoverable. Pass --keep-pcm to skip this.
Releasing a new version (maintainers)
The full release flow — version bump, GitHub Release, and the merge request to the official KiCad PCM repository — is documented step by step in docs/release-pipeline.md.
Short version:
- Bump
VERSIONand theversions[]entry inmetadata.json(andrust_router/Cargo.tomlonly when the Rust crate changed);python3 check_release_version.py --tag vX.Y.Zchecks they agree. git tag v0.15.6 && git push --tags— CI builds all 4 platform binaries, packages a singleKiCadRoutingTools-(the PCM validator rejects duplicate version strings, so we ship one cross-platform zip), patches.zip metadata.jsonwith real sha256/size values, and attaches everything to the GitHub Release.- Append the new version to the metadata file in your fork of
gitlab.com/kicad/addons/metadataand open an MR. See the docs page for the exact commands.
python3 package_pcm.py --binary-dir ./path/to/release/artifacts
Usage
- Open KiCad (9.0 or later)
- Open a PCB in Pcbnew
- (Optional) Select one or more nets in the PCB editor first — for example by
- Go to Tools → External Plugins → KiCadRoutingTools
- To route the whole board hands-off: **Auto › Autorouter ›
- Or, by hand: configure routing parameters, select (or adjust) the nets to route,
Plugin Tabs
Auto Tab (the first tab; a fresh dialog opens on it, a reopened one on the page it was closed on):
- Autorouter sub-tab: route the whole board with no agent. Run Autorouter runs
autoroute.py as a
subprocess on a snapshot of the open board (with its .kicad_pro / .kicad_dru),
in a temp work folder. Its Plan pane shows what it read off the board -- the
design rules and where they came from, the planes, the parts it fans out and the
ones it does not, with why, the diff pairs and power nets -- and its Steps
checklist one row per step, pending / running (time ticking) / done / FAILED /
skipped, with each step's result (escapes and grazes, caps moved, pairs routed,
each route pass's open nets and DRC, which pass shipped, why a pass did not run);
the rows the run adds (a fanout's next rung, a re-fan) appear as they start.
Selecting a row shows its command line, decisions, summary and log tail (a failed
one its exit code and error). Options: Finish only (--finish), Effort factor
(--effort-factor), Plane layer cost (--plane-layer-cost), Board's own rules
(--board-rules), Start at the fab floor (--floor-first), Keep placement (--keep-placement), Write filled zones
(--write-fill). Stop kills the
run and its steps. Apply Result to Board makes the open board match the shipped
result -- footprint poses (the decap step moves caps), tracks and vias (live copper
the result does not have is removed), the zones with their fills (not refilled), and
the design rules the result was graded against -- after listing every change.
- AI Routing sub-tab: plan a routing chain with
/plan-pcb-routingand run its steps; review and diagnose; save/load plans (see AI assistance above) - AI Placement sub-tab: place (and route) the board with
/plan-pcb-placement - Labels sub-tab: Beautify Labels -- uniform, non-overlapping reference-designator silkscreen, the CLI's
py_placer/beautify_labels.py
- Net selection with filtering and component filtering
- Nets selected in the PCB editor before opening the plugin are pre-checked automatically (also applies to the Fanout, Planes, and Differential tabs)
- Option to separate nets by net class (organizes into tabs per class)
- Track width, clearance, via size/drill from net class or manual override; impedance; the fab tier, escalation policy and clearance ceiling (the CLI's
--fab-tier,--escalation,--clearance-ceiling) - Layer selection with per-layer cost multipliers
- Options: stub layer swaps, copper text moving, teardrops, DRC-settings fix, power net widths and neck-down, no-BGA zones, smoothing
- Guide corridor - draw a polyline on a User layer (e.g.
User.1) and tick "Follow User-layer guide path" to route the selected nets along it (waypoints, avoiding obstacles, packed non-overlapping) - Keepout zones - draw one or more closed polygons on a User layer (e.g.
User.2) and tick "Keep out of User-layer polygon(s)" to keep routed tracks out of those areas (hard keepout, all routed nets) - Clear guide/keepout layers - optional "Clear guide layer after routing" / "Clear keepout layer after routing" checkboxes (unchecked by default) delete the drawn guide/keepout graphics from their User layer after a successful route, so you can draw fresh ones for the next run
- Swappable nets configuration for target swap optimization
- Routing parameters: iterations, heuristic weight, rip-up, probe iterations
- MPS ordering options, direction control, length matching
- Proximity settings: BGA, stub, track, via proximity costs
- Debug options
- Differential pair selection with filtering
- Pair width and gap, differential impedance, turning radius, setback angle configuration
- Options: polarity fix, GND vias, intra-pair length matching, AC-coupled end-to-end matching
- Ask AI confirms pairs by pin function
- BGA fanout with exit margin, escape direction, differential pair support, and plane-net ball drops
- Escape method: auto (channel router, under-pad retry), channel, under-pad for dense fully-populated BGAs (issue #122), or dog-bone — see BGA Fanout
- "Optimize decoupling cap placement" option (off by default) — after fanout, nudges decoupling caps off foreign-net fanout vias and toward same-net balls — see Decap Clearance Repair
- QFN fanout with extension length, escape layer, and an under-pad (via-drop) escape
- Net selection for fanout operations
- Net-to-layer assignment for power/ground planes (Ask AI recommends one)
- Create the pours (plus thermal via arrays under exposed pads, optional thermal-relief connections)
- Area via stitching, a board-edge via fence, and GND return via placement near signal vias
- Via size/drill, zone clearance configuration
- Real-time routing output display
- Color-coded messages (errors, warnings, success)
- Version information and credits
- Window transparency, Validate PCB Data (the pcbnew-built board model against the file parser's, reported in the Log tab) and Reset All Settings to Defaults
- Settings persistence (parameters and selections preserved between sessions)
- Cancel button to stop routing operations mid-progress
- Results applied directly to the open PCB in KiCad
Command-Line Interface
Net Pattern Syntax
All --nets options support fnmatch-style wildcards and exclusion patterns:
| Pattern | Description |
|---------|-------------|
| * | All nets |
| DATA | Nets containing "DATA" |
| /* | Nets starting with "/" (hierarchical) |
| Net-(U1-*) | Nets matching "Net-(U1-...)" |
| !GND | Exclude net named "GND" |
| !VCC | Exclude nets containing "VCC" |
| "*" "!GND" "!VCC" | All nets except GND and VCC |
Notes:
- Exclusion patterns (starting with
!) remove matching nets from the result - Order matters: include patterns add nets, exclude patterns remove them
- Nets starting with "unconnected-" are automatically excluded
- Use quotes around patterns with special characters
Route a Whole Board
autoroute.py routes a whole board with no agent (the other way is the
/plan-pcb-routing skill): it reads the board's rules, footprints and nets, plans the
chain (planes, fanouts, decap clearance, diff pairs, route passes) and runs it, each
step as its own process. The commands below are the tools it runs, for a hand-built
chain.
python3 py_router/autoroute.py kicad_files/input.kicad_pcb kicad_files/output.kicad_pcb
python3 py_router/autoroute.py kicad_files/input.kicad_pcb kicad_files/output.kicad_pcb --dry-run
Route Nets
# Route all nets (default) - outputs to input_routed.kicad_pcb
python3 py_router/route.py kicad_files/input.kicad_pcb
Route all nets, overwrite input file
python3 py_router/route.py kicad_files/input.kicad_pcb --overwrite
Route all nets to a specific output file
python3 py_router/route.py kicad_files/input.kicad_pcb kicad_files/output.kicad_pcb
Route specific nets (using --nets option)
python3 py_router/route.py kicad_files/input.kicad_pcb kicad_files/output.kicad_pcb --nets "Net-(U2A-DATA_0)" "Net-(U2A-DATA_1)"
Route with wildcard patterns
python3 py_router/route.py kicad_files/input.kicad_pcb kicad_files/output.kicad_pcb --nets "Net-(U2A-DATA_*)"
Route all nets on a component (auto-excludes GND/VCC/VDD/unconnected)
python3 py_router/route.py kicad_files/input.kicad_pcb kicad_files/output.kicad_pcb --component U1
Route specific patterns on a component (no auto-exclusion)
python3 py_router/route.py kicad_files/input.kicad_pcb kicad_files/output.kicad_pcb --nets "/DDAT*" --component U1
Route ALL nets on a component including power (use "*" pattern)
python3 py_router/route.py kicad_files/input.kicad_pcb kicad_files/output.kicad_pcb --nets "*" --component U1
Exclusion-pattern SYNTAX demo (! prefix). NOTE: in the #562 chain you do
NOT exclude plane nets from the route step -- see the chain example below.
python3 py_router/route.py kicad_files/input.kicad_pcb kicad_files/output.kicad_pcb --nets "*" "!GND" "!VCC"
Route one placement BLOCK -- a schematic sheet, a KiCad group, a net-name prefix, an IC and
its decaps (--group-by kicad,sheet,netprefix,decap; auto = kicad,sheet; --list-groups shows them)
python3 py_router/route.py kicad_files/input.kicad_pcb kicad_files/output.kicad_pcb \
--group-by sheet --list-groups # what blocks exist?
python3 py_router/route.py kicad_files/input.kicad_pcb kicad_files/output.kicad_pcb \
--group sheet:558c3023 --group-by sheet --group-scope internal
PREVIEW any routing run: route it, report what it WOULD add, write no board
python3 py_router/route.py kicad_files/input.kicad_pcb kicad_files/output.kicad_pcb \
--group sheet:558c3023 --group-by sheet --preview --preview-png preview.png
UNDO: strip the scoped nets' copper back to unrouted (needs an explicit scope;
defaults to --group-scope internal, since a block's "touching" nets include
GND/VCC and undoing those would strip their copper across the whole board)
python3 py_router/route.py kicad_files/input.kicad_pcb kicad_files/undone.kicad_pcb \
--group sheet:558c3023 --group-by sheet --undo
Route differential pairs (use route_diff.py)
python3 py_router/route_diff.py kicad_files/input.kicad_pcb kicad_files/output.kicad_pcb --nets "lvds" --no-bga-zones
Route with wider tracks for power nets
python3 py_router/route.py kicad_files/input.kicad_pcb kicad_files/output.kicad_pcb --nets "Net*" \
--power-nets "GND" "VCC" "+3.3V" --power-nets-widths 0.4 0.5 0.3 --track-width 0.2
Typical workflow: create GND plane first, then route all signals
python3 py_router/route_planes.py kicad_files/flat_hierarchy.kicad_pcb --nets GND --plane-layers B.Cu
python3 py_router/route.py kicad_files/flat_hierarchy_routed.kicad_pcb --overwrite
Create Power/Ground Planes
# Pour a GND zone on B.Cu (outputs to input_routed.kicad_pcb). The pour places no
per-pad taps: the route step that follows welds the plane pads into it (#562)
python3 py_router/route_planes.py kicad_files/input.kicad_pcb --nets GND --plane-layers B.Cu
Create GND zone, overwrite input file
python3 py_router/route_planes.py kicad_files/input.kicad_pcb --overwrite --nets GND --plane-layers B.Cu
Create GND zone to specific output file
python3 py_router/route_planes.py kicad_files/input.kicad_pcb kicad_files/output.kicad_pcb --nets GND --plane-layers B.Cu
Create multiple planes at once (each net paired with corresponding plane layer)
python3 py_router/route_planes.py kicad_files/input.kicad_pcb --nets GND +3.3V --plane-layers In1.Cu In2.Cu
VCC plane; --via-size/--via-drill size this step's own vias (thermal arrays, stitching)
python3 py_router/route_planes.py kicad_files/input.kicad_pcb --nets VCC --plane-layers In2.Cu --via-size 0.5 --via-drill 0.4
Multiple nets sharing one layer, split round spines routed on it (use | separator)
python3 py_router/route_planes.py kicad_files/input.kicad_pcb --nets GND "VA19|VA11" --plane-layers In4.Cu In5.Cu
Dry run to see what would be placed
python3 py_router/route_planes.py kicad_files/input.kicad_pcb --nets GND --plane-layers B.Cu --dry-run
GND return vias (--add-gnd-vias) and area stitching (--stitch-vias, --stitch-edge-fence) go in a re-run of the same pour after routing, so they place around the finished signals, and a return via needs GND poured on two layers — see Plane Routing.
Repair Disconnected Plane Regions
Since #562 you normally do not run this step. Every route.py run
finishes with an in-run plane finalize that applies this same engine
(pad taps + region joins), the plane-copper cleanup, and a KiCad-oracle
completion check — so a pours-first chain repairs its planes automatically.
KICAD_PLANE_FINALIZE=0 is the kill switch. The finalize runs even when
the route step finds nothing else to route (#1112), so a chain should end
on route.py, never on this script. Use the standalone script below for a
board routed OUTSIDE that chain (e.g. hand-edited copper); its track and
via default to the board's Default net class, not to the sizes a chain
routed at, so pass--track-width/--via-size/--via-drillif they
differ.
After creating power planes, regions may become split by vias and traces from other nets. Use repair_planes.py to reconnect them:
# Auto-detect all zones in PCB and repair disconnected regions (outputs to input_routed.kicad_pcb)
python3 py_router/repair_planes.py kicad_files/input.kicad_pcb
Auto-detect all zones, overwrite input
python3 py_router/repair_planes.py kicad_files/input.kicad_pcb --overwrite
Auto-detect all zones to specific output file
python3 py_router/repair_planes.py kicad_files/input.kicad_pcb kicad_files/output.kicad_pcb
Specific nets and layers
python3 py_router/repair_planes.py kicad_files/input.kicad_pcb --nets GND --plane-layers B.Cu
Customize track width and clearance
python3 py_router/repair_planes.py kicad_files/input.kicad_pcb kicad_files/output.kicad_pcb \
--track-width 0.5 --clearance 0.2
Review a Placement
Placement deltas are invisible in a board file; render them instead.
# what moved, and did it help? (ghosts at the seed poses, arrows, metrics caption)
python3 py_tools/render_placement.py placed.kicad_pcb --before seed.kicad_pcb -o delta.png
zoom to one placement block; same block names as route.py --group
python3 py_tools/render_placement.py board.kicad_pcb --list-groups --group-by sheet
python3 py_tools/render_placement.py board.kicad_pcb --zoom-group sheet:58d913ec --per-side -o out/
everything a placement author reads, in one artifact: escape lanes, groups, and
lock advice (which parts should NOT move) -- locks nothing, writes no board
python3 py_tools/board_brief.py board.kicad_pcb
Toggles for --borders / --labels / --ratsnest / --arrows / --ghosts;
--per-side gives F and B panels rather than one flattened projection.
The render is triage, and so are the caption's crossings / hpwl: a
placement is judged by routing it.
Verify Results
# Check for DRC violations. With no -c, grades at the Default net-class clearance
the routing steps wrote into the sibling .kicad_pro (the clearance the board was
routed to), plus the board's .kicad_dru layer rules; falls back to 0.2mm if
there's no project. Pass -c to override.
python3 py_router/check_drc.py kicad_files/output.kicad_pcb
Cross-check with KiCad's own DRC engine (requires KiCad; --refill-zones avoids
bogus zone-clearance errors from stale pours - see tests/README.md for details)
kicad-cli pcb drc --refill-zones --format json -o drc.json kicad_files/output.kicad_pcb
...because a routed board ships zone OUTLINES with no filled_polygon, so an
unrefilled grade reports plane opens that are not real (#910). To ship a
board that already carries its fills, add --write-fill to the route step, or:
python3 py_tools/fill_for_delivery.py kicad_files/output.kicad_pcb -o delivered.kicad_pcb
Check connectivity (detects unrouted nets, broken routes, and T-junctions)
python3 py_router/check_connected.py kicad_files/output.kicad_pcb
Check connectivity for specific nets
python3 py_router/check_connected.py kicad_files/output.kicad_pcb --nets "DATA"
Check connectivity for all nets on a component
python3 py_router/check_connected.py kicad_files/output.kicad_pcb --component U1
Only check routed nets (skip unrouted net detection)
python3 py_router/check_connected.py kicad_files/output.kicad_pcb --routed-only
Check for orphan stubs (dead-end traces with no pad/via/trace at the loose end).
Connection is judged by actual copper extent (via radius, pad size, trace
half-width), so T-junction taps and copper-overlap joints are not miscounted.
python3 py_tools/check_orphan_stubs.py kicad_files/output.kicad_pcb
Other-net copper inside the screw-head ring of each mounting hole (KiCad checks
a hole's clearance only). Declare the ring before routing with
add_rule_area.py --name MOUNT --mounting-holes. --ring MM sets how far past the
hole edge the head reaches (default 0.4 x the drill).
python3 py_tools/check_mounting_holes.py kicad_files/output.kicad_pcb --ring 1.3
Pad-geometry sanity check: flags same-footprint, different-net pads whose copper
overlaps (a short). A non-zero result almost always means a pad's rotation/size
is modelled wrong - the usual cause is a QFN/QFP/BGA placed at a non-orthogonal
angle. The fanout tools run this automatically on their component first; run it
yourself before fanout (or board-wide) as a standalone check:
python3 py_router/check_pads.py kicad_files/board.kicad_pcb # whole board, per footprint
python3 py_router/check_pads.py kicad_files/board.kicad_pcb --component U23 # one footprint
python3 py_router/check_pads.py kicad_files/board.kicad_pcb --cross-footprint # also across parts
Flag long non-orthonormal tracks. An on-grid router emits only 0/45/90-degree
segments; the only legitimate non-orthonormal segment is a short (<=1 grid cell)
terminal connector to an off-grid pad/ball. Anything longer is a routing defect
(it can cut diagonally across foreign copper). qfn_fanout escape stubs are
excluded automatically; bga_fanout's short stub-end jogs clear the 0.25mm default.
python3 py_tools/check_orthonormal.py kicad_files/output.kicad_pcb
Copper hygiene (read-only): dangling stubs, same-net soft joints, redundant
cycles, and removable / stacked / floating copper the routing left behind.
python3 py_router/check_weird.py kicad_files/output.kicad_pcb
Is the board DONE? One verdict over board_score and the checkers above, which
fails closed: exit 0 done, 4 incomplete, 5 graded clean only against floors
the routing lowered (--authored-from names the board the chain started from)
python3 check_complete.py kicad_files/output.kicad_pcb --authored-from kicad_files/input.kicad_pcb
See Utilities for every checker and its options, and
python3 krt_registry.py for every runnable tool in the clone with its purpose.
Power Net Analysis
Use the /analyze-power-nets skill to identify power nets and get track width recommendations:
# Ask the AI to analyze your board with datasheet lookup
/analyze-power-nets kicad_files/my_board.kicad_pcb
The skill:
- Auto-classifies obvious components (resistors, capacitors, inductors, etc.)
- Uses WebSearch to look up datasheets for unknown components (ICs, connectors, transistors)
- Classifies each component's role (power source, current sink, pass-through, shunt)
- Traces power paths from sinks to sources
- Generates ready-to-use
--power-netsconfigurations
High-Speed Net Analysis
Use the /find-high-speed-nets skill to identify high-speed nets and get GND return via recommendations:
# Ask the AI to analyze signal speeds with datasheet lookup
/find-high-speed-nets kicad_files/my_board.kicad_pcb
The skill:
- Pre-classifies nets by name patterns (DDR, USB, SPI, CLK, etc.)
- Pre-classifies components by footprint (FPGA, DDR, PHY, etc.)
- Uses WebSearch to look up datasheets for ICs and extract max clock rates and rise times
- Traces high-speed signals through series passives (termination resistors, AC coupling caps)
- Generates a speed classification (ultra-high/high/medium/low) with recommended
--gnd-via-distance
/plan-pcb-routing skill includes a lightweight version of this analysis (net name and
footprint pattern matching only, no datasheet lookup) and automatically includes a GND return
via step when GND planes are present. Run /find-high-speed-nets first for more accurate
recommendations based on actual component specifications.
Integration Tests
# Run full integration test (fanout + routing + checks)
python3 tests/test_fanout_and_route.py --all
Quick mode for faster testing
python3 tests/test_fanout_and_route.py --all --quick
The whole suite (~770 files, about 40 minutes on one machine when last measured)
python3 tests/run_all.py
See tests/README.md for detailed documentation of all test scripts.
Documentation
The documentation index is organised by task (install, route, place, check, test, release); the table below describes each document.
| Document | Description |
|----------|-------------|
| Routing Architecture | Module structure, obstacle maps, A* algorithm |
| Python API | Using the modules as a library: parser, writer, modification, config, net analysis, impedance — with runnable examples |
| Configuration | Command-line options, GridRouteConfig parameters |
| Differential Pairs | P/N pairing, polarity swaps, via handling |
| Net Ordering | MPS algorithm, inside-out ordering, strategy comparison |
| Rip-Up and Reroute | Blocking analysis, progressive N+1 escalation, reroute loop |
| Length Matching | Trombone meanders, via barrel lengths, DDR auto-grouping, time matching |
| Bus Routing | Bus detection and filter, corridor planning, middle-out ordering, corridor attraction; the topo bus step |
| Guide Corridor | User-layer guide paths, waypoints, best-effort following |
| Power/Ground Planes | Copper zones with automatic via placement |
| Utilities | Every checker (DRC, connectivity, completion, hygiene, pads), the fanout generators, placement tools, renderers, the DRC-settings fixer |
| Design Brief | Declare what the board IS -- the facts a board file cannot contain -- and compile them into the intent () |
| Floorplan Intent | Declare the floorplan, grade the board against it (check_floorplan.py) |
| BGA Fanout | BGA escape routing generator |
| QFN Fanout | QFN/QFP escape routing generator |
| Rust Router | Building and using the Rust A* module |
| Power Net Analysis | Power net detection, AI analysis, track width guidelines |
| Claude Skills | All eleven AI skills: placement and routing end to end, routing plans, power/high-speed/diff-pair analysis, stackup, plane mappings, failure diagnosis, board review, the 3D movie |
| Placement | Placement by function: groups, one annealed objective, legality, the floorplan intent's grade |
| Integration Tests | Test scripts and performance benchmarks |
| Release Pipeline | How to tag a release and submit it to the KiCad PCM (maintainers) |
Project Structure
``` KiCadRoutingTools/ ├── py_router/ # Routing engine + CLI entry points (~130 modules) │ ├── route.py # Main CLI - single-ended routing (ends with the in-run plane finalize, #562) │ ├── route_diff.py # Main CLI - differential pair routing │ ├── route_planes.py # Main CLI - power/ground plane pours │ ├── repair_planes.py # Standalone utility - repair disconnected plane regions (the chain step is absorbed into route.py's finalize, #562) │ ├── route_render.py # PNG still of a board from its geometry │ ├── route_movie.py # Movie of a routing run, step by step (route_trace.py records the router's events) │ ├── make_plan.py # Recorded command chain -> GUI routing plan (plan.json) │ ├── run_plan.py # Run a GUI routing plan headless, through the real plugin dialog │ ├── autoroute.py # Build a routing chain from the board itself and run it, no agent │ ├── add_rule_area.py # Write a copper keep-out rule area onto a board │ ├── plane_io.py # Plane I/O utilities (zone extraction, output writing) │ ├── plane_obstacle_builder.py # Obstacle map building for plane via placement │ ├── plane_blocker_detection.py # Blocker detection and rip-up for plane vias │ ├── plane_zone_geometry.py # Voronoi cells for a shared plane layer's split │ ├── plane_split_raster.py # Raster finishing of a shared plane layer's split │ ├── plane_resistance.py # Plane resistance and current capacity calculations │ ├── plane_region_connector.py # D
... (README truncated for length)