Before split

kicad-tools

Tools for AI agents to work with KiCad projects.

🌐 Live demo gallery: kicad-tools.org — explore example boards built end-to-end by these tools, with 2D/3D renders, routing & manufacturing metrics, downloadable fabrication packages, and an interactive in-browser PCB viewer.

This project provides standalone Python tools that enable AI agents (LLMs, autonomous coding assistants, etc.) to parse, analyze, and manipulate KiCad schematic and PCB files programmatically. All tools output machine-readable JSON and require no running KiCad instance.

Why Agent-Focused?

Traditional EDA tools require GUIs and manual interaction. kicad-tools bridges the gap by providing:

• Structured data access - Parse KiCad files into clean Python objects
• Machine-readable output - Analysis and query commands offer JSON output; check each command’s --help for supported formats
• Programmatic modification - Edit schematics and PCBs without a GUI
• LLM reasoning interface - Purpose-built module for LLM-driven PCB layout decisions

Whether you're building an AI assistant that reviews PCB designs, automating DRC checks in CI, or experimenting with LLM-driven routing, these tools provide the foundation.

Installation

# Base install (CPU only)
pip install kicad-tools

# With CUDA GPU acceleration (NVIDIA GPUs on Linux/Windows)
pip install kicad-tools[cuda]

# With Metal GPU acceleration (Apple Silicon Macs)
pip install kicad-tools[metal]

# With native C++ router backend
pip install kicad-tools[native]

# With CMA-ES placement optimization (kct optimize-placement / kct build --optimize-placement)
pip install kicad-tools[placement]

# Everything (all optional dependencies)
pip install kicad-tools[all]

The placement extra pulls in cmaes (and, transitively, scipy). It is required by kct optimize-placement and the placement step of kct build --optimize-placement; without it those commands exit with a clear message naming the extra. The dev and all extras already include it, so uv sync --extra dev is sufficient for development.

To check GPU acceleration status:

kct calibrate --show-gpu

In a board (consumer) repository

The supported setup for a PCB-design repo that depends on kicad-tools is PyPI plus a committed uv.lock: pyproject.toml carries a lower bound (kicad-tools[<extras>]>=X) and uv.lock is the exact pin. Install it, with the agent skills, CI gates and conventions, from a kicad-tools checkout:

./scripts/install-kct.sh /path/to/board-repo        # PyPI floor (default; same as --pypi)
./scripts/install-kct.sh --upgrade-workflow /path/to/board-repo  # + weekly upgrade PR
cd /path/to/board-repo && uv lock && uv sync && uv run kct build-native

The installer keeps the repo's existing extras and removes any [tool.uv.sources] kicad-tools entry. Re-running it is a no-op when the floor is already current. --upgrade-workflow adds .github/workflows/kct-upgrade.yml, which opens a PR for each new PyPI release; the PR raises the floor, refreshes uv.lock and the vendored files, and lists the release's upgrade notes. kct doctor checks that the vendored files match the installed version.

Git and SHA pins (--tag vX.Y.Z, --rev <sha>) and local checkouts (--path ../kicad-tools) are escape hatches for short-lived use. If you need a fix that is not on PyPI yet, ask for a patch release rather than carrying a SHA pin. Run ./scripts/install-kct.sh --help for every option.

Quick Start

Command Line (kct)

# List symbols in a schematic
kct symbols project.kicad_sch
kct symbols project.kicad_sch --format json

# Trace nets
kct nets project.kicad_sch
kct nets project.kicad_sch --net VCC

# Generate bill of materials
kct bom project.kicad_sch
kct bom project.kicad_sch --format csv --group

# Run ERC (requires kicad-cli)
kct erc project.kicad_sch
kct erc project.kicad_sch --errors-only

# Run DRC with manufacturer rules
kct drc board.kicad_pcb
kct drc board.kicad_pcb --mfr jlcpcb
kct mfr compare  # Compare manufacturer rules

Python API

from kicad_tools import load_schematic, Schematic

# Load and parse a schematic
doc = load_schematic("project.kicad_sch")
sch = Schematic(doc)

# Access symbols
for symbol in sch.symbols:
    print(f"{symbol.reference}: {symbol.value}")

# Access hierarchy
for sheet in sch.sheets:
    print(f"Sheet: {sheet.name}")

PCB Autorouter

from kicad_tools.router import Autorouter, DesignRules

# Configure design rules
rules = DesignRules(
    grid_resolution=0.25,  # mm
    trace_width=0.2,  # mm
    trace_clearance=0.15,  # mm
)

# Create router and add components
router = Autorouter(width=100, height=80, rules=rules)
router.add_component("U1", pads=[{"number": "1", "x": 10, "y": 10, "net": 1}])
router.add_component("U2", pads=[{"number": "1", "x": 20, "y": 10, "net": 1}])

# Route all nets
routes = router.route_all(timeout=30)
print(f"Created {len(routes)} routes")

LLM-Driven PCB Layout

The reasoning module enables LLMs to make strategic PCB layout decisions while tools handle geometric execution:

from kicad_tools import PCBReasoningAgent

# Load board
agent = PCBReasoningAgent.from_pcb("board.kicad_pcb")

# Reasoning loop
while not agent.is_complete():
    # Get state as prompt for LLM
    prompt = agent.get_prompt()

    # Call your LLM (OpenAI, Anthropic, local, etc.)
    command = call_llm(prompt)

    # Execute and get feedback
    result, diagnosis = agent.execute(command)

# Save result
agent.save("board_routed.kicad_pcb")

CLI usage:

# Export state for external LLM
kct reason board.kicad_pcb --export-state

# Interactive mode
kct reason board.kicad_pcb --interactive

# Auto-route priority nets
kct reason board.kicad_pcb --auto-route

See examples/llm-routing/ for complete examples.

MCP Server for AI Agents

Enable AI assistants like Claude to interact with KiCad designs via the Model Context Protocol:

# Install with MCP support
pip install "kicad-tools[mcp]"

# Run the MCP server
kct mcp serve

Register the server with your agent harness. kct mcp setup finds the absolute kct path, merges into the existing config without touching other servers, and is a no-op when re-run (--dry-run previews, --format json for scripts):

kct mcp setup --client claude-code      # ~/.claude.json via `claude mcp add-json` (default; --scope project for ./.mcp.json)
kct mcp setup --client claude-desktop   # Claude Desktop config
kct mcp setup --client codex            # [mcp_servers.kct] in $CODEX_HOME/config.toml
kct mcp setup --client opencode         # ~/.config/opencode/opencode.json (--project for ./opencode.json)

Or configure Claude Desktop by hand (~/Library/Application Support/Claude/claude_desktop_config.json):

{
  "mcpServers": {
    "kicad-tools": {
      "command": "python",
      "args": ["-m", "kicad_tools.mcp.server"]
    }
  }
}

Available MCP tools:

• Analysis: board_summary, get_drc_violations, measure_clearance
• Export: export_gerbers, export_bom, export_assembly
• Placement: placement_analyze, placement_suggestions
• Sessions: start_session, query_move, apply_move, commit, rollback
• Routing: route_net, route_net_auto, get_unrouted_nets
• Optimization: optimize_placement, evaluate_placement

See docs/mcp/ for complete documentation.

Circuit Blocks

Build schematics using reusable, tested circuit blocks:

from kicad_tools.schematic.models import Schematic
from kicad_tools.schematic.blocks import (
    MCUBlock,
    CrystalOscillator,
    LDOBlock,
    USBConnector,
    DebugHeader,
    I2CPullups,
    ResetButton,
)

sch = Schematic("My STM32 Design")

# Add an MCU with bypass capacitors
mcu = MCUBlock(
    sch, x=150, y=100, part="STM32F103C8T6", bypass_caps=["100nF", "100nF", "100nF", "4.7uF"]
)

# Add crystal oscillator
xtal = CrystalOscillator(sch, x=100, y=100, frequency="8MHz", load_caps="20pF")

# Add power supply
ldo = LDOBlock(sch, x=50, y=100, input_voltage=5.0, output_voltage=3.3)

Available blocks:

• MCUBlock: Microcontroller with bypass capacitors
• CrystalOscillator: Crystal/oscillator with load capacitors
• LDOBlock: Linear regulator with input/output capacitors
• USBConnector: USB-B/Mini/Micro/Type-C with optional ESD protection
• DebugHeader: SWD/JTAG/Tag-Connect programming headers
• I2CPullups: I2C bus pull-up resistors with optional filtering
• ResetButton: Reset switch with debounce capacitor
• BarrelJackInput/USBPowerInput/BatteryInput: Power input circuits
• LEDIndicator: Status LED with current-limiting resistor
• DecouplingCaps: Decoupling capacitor placement

See boards/04-stm32-devboard/ for a complete design example.

Project Workflow

Work with complete KiCad projects using the unified Project class:

from kicad_tools import Project

# Load a KiCad project
project = Project.load("myboard.kicad_pro")

# Cross-reference schematic to PCB
result = project.cross_reference()
print(f"Unplaced components: {result.unplaced}")

# Export manufacturing files
project.export_assembly("output/", manufacturer="jlcpcb")

Progress Callbacks

Monitor long-running operations with progress callbacks:

from kicad_tools import ProgressCallback, ProgressContext
from kicad_tools.router import Autorouter


def on_progress(progress: float, message: str, cancelable: bool) -> bool:
    print(f"{progress * 100:.0f}%: {message}")
    return True  # Return False to cancel


# Use with context manager
with ProgressContext(on_progress):
    router = Autorouter(...)
    router.route_all()  # Progress reported automatically

# Or create JSON-formatted callbacks for automation
from kicad_tools import create_json_callback

callback = create_json_callback()

Parametric Footprint Generators

Create KiCad footprints programmatically with IPC-7351 naming:

from kicad_tools.library import create_soic, create_qfp, create_chip

# Generate SOIC-8 footprint
fp = create_soic(pins=8, pitch=1.27)
fp.save("SOIC-8.kicad_mod")

# Generate LQFP-48
fp = create_qfp(pins=48, pitch=0.5, body_size=7.0)
fp.save("LQFP-48.kicad_mod")

# Generate 0402 chip resistor
fp = create_chip("0402", prefix="R")
fp.save("R_0402.kicad_mod")

Available generators: create_soic, create_qfp, create_qfn, create_sot, create_chip, create_dip, create_pin_header.

Symbol Library Management

Create and edit KiCad symbol libraries programmatically:

from kicad_tools.schema.library import SymbolLibrary

# Create a new symbol library
lib = SymbolLibrary.create("myproject.kicad_sym")

# Create a symbol with pins
sym = lib.create_symbol("MyPart")
sym.add_pin("1", "VCC", "power_in", (0, 5.08))
sym.add_pin("2", "GND", "power_in", (0, -5.08))
sym.add_pin("3", "IN", "input", (-7.62, 0))
sym.add_pin("4", "OUT", "output", (7.62, 0))

# Save the library
lib.save()

# Load and edit existing library
lib = SymbolLibrary.load("existing.kicad_sym")

Pure Python DRC

Run design rule checks without requiring kicad-cli:

# Check against manufacturer rules
kct check board.kicad_pcb --mfr jlcpcb --format json

# Check against a 4-layer, 2 oz manufacturer rule set
kct check board.kicad_pcb --mfr jlcpcb --layers 4 --copper 2

Python API:

from kicad_tools.schema.pcb import PCB
from kicad_tools.validate import DRCChecker

pcb = PCB.load("board.kicad_pcb")
checker = DRCChecker(pcb, manufacturer="jlcpcb")
results = checker.check_all()

print(results.summary())
for violation in results:
    print(f"  {violation.rule_id}: {violation.message}")

Placement Optimization

Optimize component placement using physics-based or evolutionary algorithms:

from kicad_tools.optim import PlacementOptimizer, EvolutionaryPlacementOptimizer
from kicad_tools.schema.pcb import PCB

pcb = PCB.load("board.kicad_pcb")

# Physics-based optimization (force-directed)
optimizer = PlacementOptimizer.from_pcb(pcb)
optimizer.run(iterations=1000, dt=0.01)

# Get optimized placements
for comp in optimizer.components:
    print(f"{comp.ref}: ({comp.x:.2f}, {comp.y:.2f}) @ {comp.rotation:.1f}°")

# Evolutionary optimization (genetic algorithm)
evo = EvolutionaryPlacementOptimizer.from_pcb(pcb)
best = evo.optimize(generations=100, population_size=50)

# Hybrid: evolutionary global search + physics refinement
physics_opt = evo.optimize_hybrid(generations=50)
physics_opt.write_to_pcb(pcb)
pcb.save("optimized.kicad_pcb")

CLI usage:

kct placement optimize board.kicad_pcb --iterations 1000

Trace Optimization

Optimize routed traces for shorter paths and fewer vias:

from kicad_tools.router import TraceOptimizer
from kicad_tools.schema.pcb import PCB

pcb = PCB.load("board.kicad_pcb")
optimizer = TraceOptimizer(pcb)
optimizer.optimize()
pcb.save("optimized.kicad_pcb")

CLI usage:

kct optimize-traces board.kicad_pcb -o optimized.kicad_pcb

Datasheet Tools

Search, download, and parse component datasheets:

# Search for datasheets
kct datasheet search STM32F103C8T6

# Download a datasheet
kct datasheet download STM32F103C8T6 -o datasheets/

# Convert PDF to markdown
kct datasheet convert datasheet.pdf -o datasheet.md

# Extract images and tables
kct datasheet extract-images datasheet.pdf -o images/
kct datasheet extract-tables datasheet.pdf

Python API:

from kicad_tools.datasheet import DatasheetManager, DatasheetParser

# Search and download
manager = DatasheetManager()
results = manager.search("STM32F103C8T6")
datasheet = manager.download(results[0])

# Parse PDF
parser = DatasheetParser("STM32F103.pdf")
markdown = parser.to_markdown()

# Extract images and tables
images = parser.extract_images()
tables = parser.extract_tables()
for table in tables:
    print(table.to_markdown())

Parts Lookup (LCSC / JLCPCB)

Look up LCSC part numbers, check BOM availability, and pull pricing/stock:

from kicad_tools.parts import LCSCClient

client = LCSCClient()
part = client.lookup("C2040")
if part:
    print(f"{part.mfr_part}: {part.stock} in stock, best ${part.best_price:.4f}")

Part lookups resolve through a tiered chain (each tier falls back to the next):

1. Local response cache — previously fetched parts.
2. Official JLCPCB open-platform API — only when you supply your own API key (see below). Off by default; inert without keys.
3. Anonymous scrape API — the public JLCPCB web endpoints (requires the parts extra: pip install "kicad-tools[parts]"). Note: as of July 2026 JLCPCB's public endpoint returns 404 — treat this tier as best-effort/deprecated and rely on tier 2 (BYO key) or tier 4 (offline).
4. Offline jlcparts catalog — a locally synced mirror (kct parts sync-catalog, ~620 MB download, ~5 GB on disk, ~7.1 M components), usable fully offline.

Using your own JLCPCB API key

kicad-tools can talk to the official JLCPCB open-platform API using credentials you register yourself at the JLCPCB developer portal (https://jlcpcb.com/ → developer/open platform). This is strictly opt-in: you bring your own key, kicad-tools ships only the signed client. Without keys, behavior is unchanged — the official tier is simply skipped.

Set all three environment variables (kicad-tools reads them via os.environ; it does not load a .env file itself, so use your shell, direnv, or a dotenv runner — see .env.example):

export JLCPCB_APP_ID="your-app-id"
export JLCPCB_ACCESS_KEY="your-access-key"
export JLCPCB_SECRET_KEY="your-secret-key"

All three must be set (and non-empty) to activate the official tier; if any is missing it stays inert. Once set, LCSCClient.lookup() / lookup_many() prefer the official API for part-detail-by-code, falling back down the chain above on any failure.

Notes and caveats:

• What it unlocks: authenticated part detail lookup by LCSC code only. There is no confirmed official keyword/MPN search endpoint, so LCSCClient.search() always uses the anonymous/offline path even with keys.
• IP whitelisting: the developer portal offers an IP-whitelist feature. If you enable it, your machine's public IP must be whitelisted or requests are rejected (surfaced as a distinct, actionable error).
• Never commit credentials. .env is gitignored; the secret key is used only as HMAC key material and is never transmitted.
• The request-signing scheme is not first-party-documented by JLCPCB; the client implements the best-available community-reverse-engineered variant for the Parts surface, with the two ambiguous parameters isolated as single flip-points in parts/jlcpcb_api.py (see that module and issue #4118).

CLI Commands

Unified CLI (kct or kicad-tools)

The commands below are the ones most workflows reach for. The authoritative full list (every command and subcommand) lives in CLI Reference → Commands Overview.

Inspection and validation

Layout and routing

Repair

Parts and manufacturing

Environment

Every kct subcommand that produces a result accepts --format json for machine-readable output (some older commands also keep --json as a legacy alias). A few commands are deliberately exempt -- e.g. interactive, mcp serve and run -- see Machine Output for the inventory, exemptions and per-command JSON shapes.

PCB Tools

Library Tools

Modules

What's New

Release notes live in CHANGELOG.md (one section per release, newest first) and on the GitHub Releases page. Changes merged since the last release are collected as fragments under changelog.d/ until the next release assembles them.

Features

• Pure Python parsing - No KiCad installation needed
• Round-trip editing - Parse, modify, and save files preserving formatting
• Full S-expression support - Handles all KiCad 8.0+ file formats
• Schematic analysis - Symbols, wires, labels, hierarchy traversal
• Circuit blocks - Reusable blocks for MCU, power, USB, debug headers, I2C, reset
• PCB analysis - Footprints, nets, traces, vias, zones
• Manufacturer rules - JLCPCB, PCBWay, OSHPark, Seeed design rules
• PCB autorouter - A* pathfinding with net class awareness
• Pure Python DRC - Design rule checking without kicad-cli
• Placement optimization - Physics-based and evolutionary algorithms
• Trace optimization - Path shortening and via reduction
• Footprint generation - Parametric generators for common packages
• Symbol library creation - Programmatic symbol creation and editing
• Datasheet tools - Search, download, and PDF parsing
• Progress callbacks - Monitor and cancel long-running operations
• JSON output - Machine-readable output for automation

Requirements

• Python 3.10+
• numpy (for router module)
• KiCad 8+ (optional) - for running ERC/DRC via kicad-cli

Development

This project uses uv for fast, reproducible Python environment management.

Quick Start

# Clone repository
git clone https://github.com/rjwalters/kicad-tools.git
cd kicad-tools

# Set up development environment (installs all dev dependencies)
uv sync --extra dev

# Build the C++ router backend (REQUIRED for production routing speed,
# delivers 10-100x A* speedup vs pure-Python; takes ~30s on first build,
# cached thereafter). uv sync does NOT build this — fresh checkouts and
# fresh worktrees need this step explicitly.
uv run kct build-native

# Verify the C++ backend is installed
uv run kct build-native --check
# Expected: "C++ backend: available (version 1.0.0)"

# Run tests
uv run pytest

# Run linter
uv run ruff check .

# Format code
uv run ruff format .

Routing performance note: Without the C++ backend, board routing falls back to pure-Python A* — typically 5-10x slower per net, which can push medium boards (e.g. board 07 in boards/07-matchgroup-test/) past the default 6-minute CI cap. If kct route appears stuck or per-net log lines take tens of seconds, run kct build-native --check first — a missing extension is the most common cause.

Fresh worktree checklist

Pinned renders and kct pcb model-audit --env pinned also need the checksum-verified KiCad 3D model subset: run uv run kct models sync --sparse once (about 14 MB; cached under ~/.cache/kicad-tools/kicad-3dmodels/). Without it they report pinned model set not synced; nothing else breaks.

1. Sync the lock-pinned dev environment first:

   uv sync --frozen --extra dev

   A fresh worktree performs no Python env setup, and a stale or drifted .venv/ (e.g. a mypy newer than the uv.lock pin) produces spurious mypy-baseline noise that looks like real type regressions (issue #4558). --frozen guarantees the resolved set matches uv.lock exactly — the same environment CI uses. Loom-created worktrees run this automatically via the .loom/hooks/post-worktree.sh hook; run it manually for hand-made worktrees or if the hook reported a failure.

2. Build the native extension. The worktree's .venv/ does not inherit the C++ extension built in the main checkout, and uv sync does not build it. After cd into the worktree, run uv run kct build-native once before any routing benchmarks.

3. If a local mypy error names a file outside your diff, rm -rf .mypy_cache and re-run before investigating it. .mypy_cache/ is gitignored, so it survives git reset --hard, git clean -fd, a rebase, and a worktree reuse — bare mypy / pnpm typecheck can replay an error computed against an older tree. CI is always cold (no actions/cache), so it will not reproduce the phantom. scripts/ci/check_mypy_baseline.py is already immune (it runs --no-incremental); see docs/contributing/development.md.

4. Know where kicad-cli's library tables come from before trusting native ERC/DRC results. kicad-cli resolves stock nicknames (Resistor_SMD:) through the global fp-lib-table/sym-lib-table in its config home, which the GUI writes on first launch -- or never, on a fresh host, CI container or docker run --user 0:0. Without them every stock footprint becomes a lib_footprint_issues DRC warning and every stock symbol an ERC warning that reads like a real defect (issues #5860, #6962; board 03 once gained 37 of them). The library configuration is part of the pinned toolchain, not of the host:

   • Where it comes from. src/kicad_tools/data/kicad-config/10.0/ holds flat copies of the stock tables shipped in CI's pinned image (CI's KICAD_IMAGE digest in .github/workflows/ci.yml).

   • How producers isolate it. Every evidence producer (kct readiness, scripts/boards/refresh_readiness.py, the scripts/boards/regenerate_* scripts) and every KiCad CI job runs kicad-cli with a scratch KICAD_CONFIG_HOME holding exactly those tables, and never reads or writes your GUI config. kct's Docker fallback (KCT_KICAD_DOCKER=1) runs the same pinned digest, not the floating kicad/kicad:10.0 tag.

   • Native evidence needs the pinned toolchain. Producers refuse (exit 2, nothing written) a kicad-cli other than the image's release (10.0.6), and refuse any DRC report with lib_footprint_issues. On a host with another KiCad release, route kicad-cli through the image: KCT_KICAD_DOCKER=1 uv run kct readiness boards/<board> --verify --checked-at <ISO>. A fixed --checked-at makes two runs byte-identical.

   • How to check it.

     uv run python -m kicad_tools.cli.kicad_toolchain --check            # host kicad-cli
     KCT_KICAD_DOCKER=1 uv run python -m kicad_tools.cli.kicad_toolchain --check

   For ad-hoc kct check runs outside a producer, point the current shell at the pinned tables (CI's container jobs do this in their "Initialize stock KiCad libraries" step):

   eval "$(python3 scripts/ci/init_kicad_libraries.py --shell)"

The build's nanobind dependency is composed into the default dev dependency-group, so a plain uv sync keeps it resolved and a later uv sync (e.g. adding --extra placement) will not prune it. If you installed with only a subset of groups, add the native extra explicitly so nanobind stays lockfile-tracked:

uv sync --extra native            # repo/dev worktree
pip install "kicad-tools[native]" # consumer / installed wheel

Avoid a bare pip install nanobind — it is not recorded in the resolved set and a subsequent uv sync will uninstall it, breaking the next kct build-native (issue #4412).

Opening a PR from a fork? Fork PRs run on GitHub-hosted runners rather than this project's self-hosted one, which makes the Test job roughly 2.2x slower (~50 min, with a 90-minute budget). Nothing is skipped and nothing extra is required of you — see docs/contributing/development.md for the details and the maintainer fallback if a run still cannot finish.

Available Commands

If you have pnpm installed, you can use these convenience scripts:

Direct uv Commands

# Run tests with coverage
uv run pytest --cov=kicad_tools --cov-report=term-missing

# Run benchmarks
uv run pytest tests/test_benchmarks.py --benchmark-only

# Type checking
uv run mypy src/

# Full CI check
uv run ruff format . --check && uv run ruff check . && uv run pytest

Agent Skills (kct namespace)

kicad-tools ships its own Claude agent skills under .claude/commands/kct/ (invoked as /kct:<name>), a harness-agnostic namespace kept separate from any installed orchestration framework. Seven skills ship today — /kct:tapeout (complete fab-ready export bundle or loud refusal), /kct:manufacturing-readiness (sign-off gates), /kct:hv-isolation-loop (mains/HV creepage design loop), /kct:board-recipe-scaffold, /kct:layout-journal, /kct:ee-review (advisory EE decision document for analog/placement-blocked boards), and /kct:help (introspective guide to the namespace). See .claude/commands/kct/README.md for the full contracts. The skill text is harness-neutral; docs/agent-surfaces.md lists what each skill needs from Claude Code, Codex CLI or opencode.

The skills ship inside the kicad-tools wheel (kicad_tools/agent_skills/kct/), so a plain pip install kicad-tools is enough; no clone of this repository is needed. Install them with kct skills install:

kct skills install                       # ./.claude/commands/kct/*.md (Claude Code, project)
kct skills install --user                # ~/.claude/commands/kct/
kct skills install --target /tmp/x       # /tmp/x/kct/*.md
kct skills install --harness codex       # ./.agents/skills/kct-<name>/SKILL.md
kct skills install --harness opencode    # ./.opencode/commands/kct/*.md, run as /kct/<name>
kct skills install --list                # packaged skills and their install state
kct skills install --check               # exit 1 if the installed copy has drifted

Re-running is idempotent. --prune removes kct skill files the package no longer ships, and --dry-run previews. Edit skills in src/kicad_tools/agent_skills/kct/; .claude/commands/kct/ is a synced copy (uv run python scripts/sync_agent_skills.py --write).

Using kicad-tools from Claude Code, Codex and opencode

Each harness needs two setup commands: one registers the MCP server, the other installs the kct skills in that harness's own format. The skill sources are shared, so every harness gets the same skills.

Add --user to kct skills install to install for every project. Then start the agent with the primer:

kct agent-guide                   # workflow, JSON contract, sign-off rule, pitfalls
kct agent-guide --harness codex   # with skill examples in Codex syntax
kct agent-guide --format json     # {"version", "harness", "sections": [...]}

kct agent-guide ships in the wheel and reads the same in every harness. Point your agent at it from CLAUDE.md or AGENTS.md instead of copying it.

Related Projects

kicad-tools is one piece of a fast-moving KiCad automation ecosystem. This section is generated from src/kicad_tools/ecosystem/data/projects.toml -- run kct ecosystem where-we-sit for our invariants and non-goals, kct ecosystem show <id> for any entry below, and see docs/ecosystem.md for the full positioning narrative. Where we have evaluated a project in depth, the linked note carries the method, the measurements and the verdict, including the cases where the other tool wins.

Licenses are the SPDX id from the upstream LICENSE file, and are load-bearing: an AGPL or unlicensed neighbour is studied at the capability level only, never copied from. Facts below were last verified on the date each registry entry records; .github/workflows/ecosystem-drift.yml re-checks them weekly.

Autorouters

• KiCadRoutingTools (MIT, Python + Rust, 488★) -- Benchmarked against us. The closest peer to kct route: octilinear multi-layer A* with via insertion, diff pairs, length matching, BGA/QFN fanout and plane pours, shipped as both a KiCad 9/10 action plugin and a CLI. Benchmarked head-to-head against us on eight demo boards under one shared kicad-cli referee: it is faster and completes more nets on the sparse and medium boards, while on the dense boards it emits literal shorts where we instead run out of time. Our evaluation: docs/research/kicad-routing-tools-comparison.md.
• TraceMaker (GPL-3.0-or-later, C++20 + CUDA, 42★) -- Benchmarked against us. C++20/CUDA KiCad 9/10 router that reads and writes .kicad_pcb directly and is judged by kicad-cli DRC. Octilinear-lattice A* with exact legality checks, negotiated rip-up, an 8-variant deterministic portfolio under a --work budget, min-cost-flow escape-corridor reservation, a nogood cache, coupled diff-pair search, and a SQLite bandit that learns which variant to pick across runs; the GPU only accelerates cost fields. On PCBWorld D3 the circuit-skills author reports 0.99 / 1.00 / 0.90 clean on the small / medium / large splits, against about 0.7 / 0.7 / 0.2 for Freerouting 2.2.4 -- third-party, single 60 s runs, not reproduced by us, and on PCBench boards TraceMaker was developed against (its own held-out figure is 73-78% clean). Its "clean" also excludes DRC errors already in the input board, looser than our 0-DRC bar. Days old; copyleft, so ideas only, and run only as an external binary. Our evaluations: docs/research/kct-route-escape-flow-experiment.md, benchmarks/external/fleet_routers/verdict.md.
• freerouting (GPL-3.0, Java, 2068★) -- the long-standing Specctra DSN/SES autorouter and the baseline most KiCad users try first. Has a headless CLI, but the DSN round-trip is a lossy interchange boundary: it routes a translated view of the board rather than the .kicad_pcb itself. We operate on the board file directly, which is what lets LVS and the manufacturing gates run against the same artifact that gets fabricated. PCBWorld's paper reports it as the strongest published rule-based baseline on real boards (Clean Pass 0.80 / 0.78 on D3-A / D3-B). fastroute is a faster Rust port of it with a byte-identical parity mode.
• OrthoRoute (MIT, Python + CUDA/Metal, 411★) -- GPU-accelerated PathFinder routing, with plugin and headless modes. Its author is explicit that it targets a narrow class of very large, dense, highly regular multilayer backplanes and BGA escape patterns and does poorly on typical boards -- the opposite end of the board-size spectrum from our demo fleet.
• DeepPCB KiCad plugin (Apache-2.0, Python, 66★) -- Evaluated and not adopted. An open-source plugin in front of a closed, credit-metered cloud router. The plugin is local; the routing is not. It requires an account and API key, so it cannot participate in an offline or air-gapped CI pipeline. DeepPCB's own published benchmark numbers are recorded in benchmarks/external/boards.toml for side-by-side comparison. Our evaluations: benchmarks/external/README.md, benchmarks/external/results/report.md.
• tscircuit autorouter (MIT, TypeScript, 85★) -- Benchmarked against us. Tscircuit's built-in router (@tscircuit/capacity-autorouter): a pipeline of hypergraph / successive-approximation solvers rather than net-by-net A*, fed a SimpleRouteJson problem instead of a KiCad file. It ships a public benchmark (dataset-srj18, derived from real Arduino and Antmicro KiCad boards) and a bug-report-to-fixture workflow. Partly benchmarked against us (Arduino Nano only): SRJ drops netclass width, clearance, zones and keepouts, so its completion is not comparable. Our evaluation: docs/research/tscircuit-evaluation.md.

Design as code (upstream of us)

• atopile (MIT, Python, 3964★) -- Ideas adopted. A language and compiler for describing boards as code (.ato), with constraint solving, a package registry and parametric part selection via its Faebryk library; it emits a netlist and updates a KiCad layout, but deliberately stops at "place and route in KiCad". That is exactly where we start, which makes the two complementary rather than competing. Our MCP server exists because of this evaluation. Our evaluations: docs/research/atopile-research-synthesis.md, docs/research/faebryk-component-library.md, docs/research/atopile-constraint-solving.md, docs/research/atopile-interface-patterns.md, docs/research/atopile-layout-reuse.md, docs/research/atopile-lsp-analysis.md, docs/research/atopile-mcp-analysis.md, docs/research/atopile-package-registry.md, docs/research/atopile-error-handling.md.
• SKiDL (MIT, Python, 1675★) -- the original Python-as-schematic-capture tool: a program describes the circuit and SKiDL emits netlists, XML BOMs and (for KiCad 6-10) editable schematics, with its own ERC. Another upstream producer of the files we consume.
• tscircuit (MIT, TypeScript, 2776★) -- Evaluated and not adopted. "React for Electronics" -- circuits described in TypeScript/React and compiled to its own Circuit JSON. Its circuit-json-to-kicad converter emits .kicad_sch, .kicad_pcb (with traces, vias and pours) and .kicad_pro, and kicad-to-circuit-json reads them back, so it is an upstream producer of the files we consume, like atopile and SKiDL. Gated and not yet usable as a front end: five representative designs were run through kct check --mfr, LVS and kicad-cli pcb drc --refill-zones, before and after re-routing with kct route, and all five failed. The blocking defect is that its schematic and PCB converters name the same net differently, so no emitted project can pass LVS at all; vias, netclass and silkscreen defaults also sit below every mainstream fab floor. Our parser reads the files without complaint, and kct route produced opens where tscircuit's own autorouter produced shorts. Six upstream defects were recorded with reproducers and re-verified on upstream HEAD (2026-10-18): three confirmed and tracked upstream, two fixed or covered upstream, one not a bug. The relation stays upstream/complementary. Our evaluation: docs/research/tscircuit-evaluation.md.
• component-importer-for-kicad (MIT, Python, 55★) -- Evaluated and not adopted. Evaluated as a vendor-ZIP (SnapEDA / Ultra Librarian) ingestion backend for symbol and footprint import. Verdict was borrow-with-refactor rather than vendor: its headless modules are PyQt6-free and close to the surface we need, but a clean-room re-implementation of roughly 600 LoC plus a kct ingest-zip CLI is the smaller change. Not built yet. Our evaluation: docs/research/component-importer-for-kicad-evaluation.md.

Agent and MCP interfaces

• Zeo (AGPL-3.0, C++, 31★) -- a KiCad fork with an integrated AI agent sidebar and MCP server. Takes a complementary approach: live editor manipulation via IPC vs. our offline file-based analysis and optimization.
• Konnect (AGPL-3.0, Rust, 1424★) -- Ideas adopted. Upstream was archived on 2026-10-26 (read-only, no further releases expected); it continues as Konnect-EDA (Orchis-ai-LLC), which is commercial closed-source software, so there is no source left to audit and no further capability audits are planned. The open replacement is our own clean-room openkonnect, with Konnect-EDA as the closed-source successor. The ideas we adopted stand on their own, and KiCAD-MCP-Server is now our agent-interface reference. A single-binary native KiCad 10 plugin exposing a very large LLM tool surface (228 tools in 21 toolsets) across schematic, layout, routing, placement, review and manufacturing. AGPL means no code can move between it and this MIT repo in either direction, so our engagement is capability-level only: we audited its connectivity primitives, its tool-economy design and its design-rule handling against our own surface. Five of its six connectivity primitives we already had; the sixth (near-miss auto-snap repair) was a real gap. Re-checked at v0.13: four new ideas adopted as follow-ups (visual baselines, truth-contract audit, honest-schema CI guard, SES provenance). Our evaluations: docs/research/konnect-connectivity-audit.md, docs/konnect-item1-toolset-economy-audit.md, docs/konnect-item8-design-rules-audit.md, docs/research/konnect-v013-delta.md.
• copperhead (Apache-2.0, TypeScript, 312★) -- Ideas adopted. "cursor for circuit boards": a natural-language brief drives direct edits to .kicad_sch / .kicad_pcb, gated by an LLM-free check and wrapped in a git snapshot that auto-rolls-back on failure. It does not route, and verifies with kicad-cli ERC/DRC only -- no LVS, no manufacturing cross-gate. Its process design (design memory as committed artifacts, a constraints registry, a per-run audit trail) is the part worth borrowing. Note: moved from chouhanindustries/copperhead since our note was written. Our evaluation: docs/research/copperhead-workflow-ideas.md.
• Seeed-Studio/kicad-mcp-server (no LICENSE committed, Python, 135★) -- the closest peer to kct mcp serve: an MCP server that reads schematic and PCB files offline (shelling out to kicad-cli for validation) to trace pin-level connections and edit designs. Overlaps our read/analyze tools; carries no router, LVS or fab-readiness gates. Its README claims MIT but the repo commits no LICENSE file, so we treat it as all-rights-reserved and copy nothing.
• circuit-skills (no LICENSE committed, Python, 9★) -- Claude Code skills for code-driven electronics: ngspice/Falstad circuit simulation, a tscircuit-placement -> KiCad IPC (kipy) route-and-DRC loop, board/enclosure fit co-design and 3D renders. Its route_eval harness now runs five routing backends on any KiCad board (two Freerouting versions, TraceMaker, the tscircuit router, and an experimental srj-legal that has TraceMaker re-route what KiCad's DRC rejects in tscircuit output) and keeps the best, with an optional fastroute backend and a PCBWorld D3 harness; it self-reports 0.98 Clean Pass on D3-A for srj-legal, unreproduced by us. Overlaps our /kct:* skills, but still assumes the tail is hand-finished in KiCad -- the opposite of our fully automated bar. No LICENSE committed, so ideas only; mining tracked in issue #5886. Our evaluations: docs/research/circuit-skills-evaluation.md, docs/research/placement_score_calibration.md.
• Backplane (MIT, Bend + TypeScript, 430★) -- an agentic KiCad/FreeCAD hub: Claude Code, Codex and others work on a local project while board, schematic and 3D viewers redraw each save in a browser, phone or desktop app. It snapshots the KiCad files after every tool call onto a hidden git ref (private index, never the user's) and compares any two versions as a uuid-keyed removed/changed/added board diff -- geometric only, no DRC or LVS. Agents get the exact kicad-cli, the canonical files and the KiStack skills. Its board diff is the idea we lacked for reviewing routing PRs (#6417). Note: moved from i2cjak/Backplane since our note was written. Our evaluation: docs/research/backplane-kistack-evaluation.md.
• KiStack (MIT, Markdown (agent skills), 397★) -- Evaluated and not adopted. Ten human-written KiCad agent skills (553 lines of prose) for schematics, symbols (KLC), footprints (kicad-library-tools), layout, BOM, exports, Gerber review, panelizing and product renders; Backplane and kicadmium both ship it. Overlaps our /kct:* skills, but its layout skill tells agents to route by hand and avoid autorouters -- the opposite of our fully automated bar. Our evaluation: docs/research/backplane-kistack-evaluation.md.
• KiCAD-MCP-Server (MIT, Python + TypeScript, 2978★) -- actively developed again (pushed 2026-10-26) and now our agent-interface reference in place of the archived Konnect. The most-starred KiCad MCP server: ~250 fine-grained tools for project setup, schematic and board editing, Freerouting, DRC/ERC, export, symbol and footprint creation and JLCPCB parts lookup. It is the MIT predecessor of Konnect. Compared tool-by-tool with kct mcp serve (pinned 628d320f): a wide imperative editing surface against our narrow session/verification one, so complementary; parts alternatives, symbol library writes and schematic cosmetic lint are worth borrowing under MIT with attribution. Its Freerouting runner is not: we improve our own router rather than add a fallback (#7991). Our evaluation: docs/research/kicad-mcp-server-evaluation.md.

Fabrication and CI

• KiBot (AGPL-3.0, Python, 747★) -- the mature, scriptable fabrication- and documentation-output generator for KiCad (gerbers, drill, position, BOM, 3D, plots), with a GitHub Action. Deeper than kct export on output variety and configuration; it assumes a board that is already routed and signed off, which is the part we automate.

KiCad bindings

• kipy (MIT, Python, 19★) -- Evaluated and not adopted. The official KiCad Python bindings (kicad-python on PyPI) for the KiCad IPC API. Requires a running KiCad instance with the IPC API enabled and a document open in an editor -- every accessor is an RPC to the live editor; there is no offline file-reading path, so it cannot participate in headless/CI workflows. Our evaluation: docs/research/kipy-ipc-api-evaluation.md.

Benchmarks and evaluation protocols

• OmniLayout / OmniRouting (no LICENSE committed) -- Ideas adopted. A published routing benchmark and leaderboard. We adopted its metric vocabulary and evaluation protocol -- the sharpest external definition of "routed well" we have found -- and declined the dataset and tooling: no license grant on the data, and the evaluation harness is unpublished. Our evaluation: docs/research/omnilayout-recon.md.

3D model tooling

• easyeda2kicad (AGPL-3.0, Python, 1714★) -- Ideas adopted. EasyEDA/LCSC to KiCad converter (symbol, footprint, 3D model), v1.0.1 at our read. AGPL-3.0: ideas only, never copy code. We took its documented 3D flow as a design input (model uuid from the footprint SVGNODE; OBJ from modules.easyeda.com/3dmodel/{uuid} converted to WRL; STEP passed through from the same bucket). Our evaluation: docs/research/3d-model-coverage.md.
• kicad-library-tools (GPL-3.0-or-later, Python (CadQuery), 80★) -- headless CadQuery generators for KiCad's official 3D packages (DIP, chip R/C/L, diodes, crystals, connectors, QFN/QFP/BGA, terminal blocks). Successor to the archived kicad-packages3D-generator. GPL-3.0-or-later: run as an external tool only, never import or vendor. Our evaluation: docs/research/3d-model-coverage.md.

Watching

Recorded in the registry with a re-evaluation trigger, deliberately not featured above yet:

• fastroute (GPL-3.0, Rust, 73★) -- Rust port of freerouting: Specctra DSN in, SES out, with a --parity mode it claims is byte-identical to Freerouting on its 20 benchmark boards. Its own measurements show about 4-5x less wall time (2102 s vs 510 s over those boards, 420 s with PGO) in 20-300 MB instead of 1-2 GB, and it adds fixes for several Freerouting optimizer bugs, multi-start, length tuning, diff pairs and impedance-derived widths. A pcbnew plugin patches the gaps in KiCad's lossy Specctra export (DRU clearances, keepouts, planes). Like freerouting it routes a translated view rather than the board file. Copyleft, so ideas only. Our evaluation: benchmarks/external/fleet_routers/verdict.md.
• AutoRoute (MIT, Rust, 0★) -- Rust negotiated-congestion router with an exact-DRC clearance model, a headless CLI and DSN/SES KiCad integration. Recorded rather than featured: 8 commits and no adoption signal yet, so there is nothing stable to measure against.
• Topola (MIT, Rust, 33★) -- work-in-progress interactive topological (rubber-band) router and autorouter in Rust, funded through NLnet's NGI0 Entrust fund. Routing topologically before committing geometry is a different shape of search from our grid A*, and the license is permissive -- but it is pre-release and we have not run it.
• circuit-synth (MIT, Python, 279★) -- Python-defined circuits (@circuit functions over KiCad library symbols and footprints) compiled to KiCad projects, built around Claude Code with slash commands for symbol search and design help. Another upstream producer of the files we consume, in the SKiDL mould; no pushes since March 2026, and we have not run its output through our gates.
• 2040-ArtNode (no LICENSE committed, Python, 0★) -- a Codex-assisted RP2354A Art-Net LED node whose KiCad 9 files come from hand-rolled Python S-expression generators, plus a SKiDL attempt. The 4-layer board is placed but carries no traces, and fails kct check --mfr jlcpcb with 255 errors, mostly stitching vias dropped onto pads -- a worked example of how hand-rolled generators drift. Not a benchmark candidate: no license and no reference copper.
• openkonnect (MIT) -- our own clean-room project: an MIT-licensed MCP server that lets LLM agents drive a running KiCad 10 over its IPC API, built on kicad-tools. It owns the live-editor surface that kicad-tools deliberately does not, and is the open replacement for Konnect's live-editor tool surface. Its clean-room rules are in its CLEANROOM.md: no Konnect source is read in either repo, and our Konnect audits stay capability-level.
• kicadmium (no LICENSE committed, Rust, 0★) -- an Agent Portal plugin: a single Rust binary that wraps a user's own KiCad install with a browser workbench and agent skills. Its kct/ crate is a ~137k-line Rust port of kicad-tools taken from our commit 37665de5, keeping our command names, flags and JSON keys, and it claims parity on several command families. It adds a 101-rule lint engine whose reviewed exceptions go stale when their evidence changes, and porting surfaced four bugs in our code (#5937-#5940). Useful as a second implementation to diff our output against.
• kicad-happy (MIT, Python, 1343★) -- agent skills (Claude Code, Codex and others) for design-level review of KiCad projects: power trees computed from feedback dividers, connector-by-connector ESD audits, passive-network checks, SPICE and EMC pre-compliance, plus datasheet and distributor lookups. That is the circuit-level review our /kct:ee-review does not yet do; it does not route or gate manufacturing.
• KiCad MCP Pro (MIT, Python, 119★) -- an MCP server for KiCad with staged permission profiles: a default of 24 read-only review tools, a build profile for controlled edits, and a release profile for human-gated manufacturing export. Those stages map onto our sign-off gates. It is candid that its SI/PI/EMC/thermal tools are first-order estimates rather than sign-off.
• KiCad AI Assistant (MIT, Python, 112★) -- a KiCad 10 action plugin that embeds an LLM chat panel inside the editor and exposes a built-in MCP server (also runnable standalone) with schematic and PCB editing, placement, zones and DRC/ERC tools. Live-editor surface, so it sits on the GUI side of our non-goals; read from README only, not run. Our evaluation: docs/research/reporecon-kicad-ai-sweep.md.
• kicad-harness (AGPL-3.0, Python, 33★) -- an Agent Skill plus a Python tool (kh) that gives an agent library lookup, region renders to PNG, DRC/ERC, IPC editing of an open board and datasheet-to-footprint generation; its distinctive idea is a repo the agent is expected to edit and push while using it. AGPL: ideas only, read from README only. Our evaluation: docs/research/reporecon-kicad-ai-sweep.md.
• blwfish/kicad-mcp (MIT, Python, 25★) -- an MCP server (18 domain-router tools, 2,000+ tests) that takes an agent from schematic to placed, Freerouting-routed, zoned and panelized board; its own README recommends Freerouting v2.2.3 for routing. Same end-to-end promise as kct, routed through an external router. Read from README only. Our evaluation: docs/research/reporecon-kicad-ai-sweep.md.
• mcp-server-kicad (GPL-3.0, Python, 13★) -- a 109-tool MCP server that edits KiCad files on disk (schematic capture, PCB layout, libraries, ERC/DRC, exports) with Freerouting for routing and an auto_place_decoupling_cap helper. File-based like us. GPL: ideas only, read from README only. Our evaluation: docs/research/reporecon-kicad-ai-sweep.md.
• KiCad Copilot (MIT, JavaScript, 16★) -- a file-oriented MCP server (no IPC, no plugin) for schematic generation, a JavaScript placement DSL with PNG/SVG preview, local routing through eda-copilot-router with a managed KiCadRoutingTools backend, simple pours, and integrated kicad-happy analysis. Its router is KRT, which we have already benchmarked, so there is no separate router to measure. Read from README only. Our evaluation: docs/research/reporecon-kicad-ai-sweep.md.
• KiPilot MCP (Apache-2.0, Python, 11★) -- a 135-tool MCP server over KiCad 10's official kicad-python IPC API, including export jobs, design-rule access and netlist import. Live-GUI session by design, the opposite of our offline stance. Apache-2.0: ideas only. Read from README only. Our evaluation: docs/research/reporecon-kicad-ai-sweep.md.
• traces (MIT, Python + TypeScript, 6★) -- local, bring-your-own-key tooling for KiCad: a semantic component-sourcing MCP server, a KiCad plugin and a /src semantic rule-check skill. Sourcing and schematic review, not layout, so it complements kct rather than competing. Read from README only. Our evaluation: docs/research/reporecon-kicad-ai-sweep.md.
• Agentic KiCad Skills (MIT, Python, 6★) -- modular agent skills (board-regime classifier, high-current, high-speed, RF, datasheet-to-footprint) with verification scripts for KiCad 10. Same shape as our /kct:* skills; content is design-rule guidance. Read from README only. Our evaluation: docs/research/reporecon-kicad-ai-sweep.md.
• kicad-llm-plugin (MIT, Python, 22★) -- a KiCad plugin that sends the schematic to a chosen local or remote LLM and renders a design-review report (fatal flaws, good practice, nice-to-haves). Review only; no editing. Read from README only. Our evaluation: docs/research/reporecon-kicad-ai-sweep.md.
• IronEmperor (MIT, Python, 11★) -- an LCSC/JLCPCB-centred generator that turns a plain-language brief into a BOM, KiCad project and 3D-printed enclosure through a multi-agent pipeline. Generator, not a layout tool; its value is parts sourcing. Read from README only. Our evaluation: docs/research/reporecon-kicad-ai-sweep.md.
• kicad-agentic-mcp (AGPL-3.0, Rust, 5★) -- a Rust MCP server and agentic control layer for KiCad 10 that mixes LLM planning with deterministic tools. Days old, AGPL: ideas only. Listed from its description and licence file; README not studied. Our evaluation: docs/research/reporecon-kicad-ai-sweep.md.
• ai-circuit-design-tests (no LICENSE committed, Python, 6★) -- a third-party test bench that runs AI KiCad tools (copperhead, kicad-happy, kicad-harness, KiCad AI Assistant, kicad-mcp-pro, kicad-mcp-server, Konnect, skidl-skills) on real design prompts and records transcripts, cost and an executive summary per run. kicad-tools is not among the tools tested; the README invites outside evaluations as issues. No LICENSE: all rights reserved, ideas only. Our evaluation: docs/research/reporecon-kicad-ai-sweep.md.
• KiKit (MIT, Python, 2038★) -- the standard KiCad panelization tool, as a library, plugin and CLI: regular and oddly-shaped panels, fab-data export from manufacturer presets, stencils, multi-board projects and presentation pages. Overlaps kct panel and kct export; we have not compared feature or fab-preset coverage.
• kicad-jlcpcb-tools (MIT, Python, 2096★) -- a KiCad plugin that generates JLCPCB Gerbers, drill, BOM and CPL files, and assigns LCSC part numbers to footprints by searching the JLCPCB parts database. A GUI-plugin take on what our JLCPCB export and /kct:tapeout BOM checks do headlessly.
• jlcparts (MIT, Python, 837★) -- a parametric-search front end over the JLCPCB/LCSC assembly catalogue, regularly rebuilt. A candidate data source for the LCSC part-number and stock checks in /kct:tapeout, if its terms and refresh cadence suit us.
• PCBWorld (BSD-3-Clause, Python, 25★) -- a Gymnasium environment around KiCad's push-and-shove router, scored by KiCad's own DRC (arXiv:2607.05915). It ships synthetic sets D1/D2 and a recipe to rebuild D3: 679 PCBench boards converted to KiCad 9, keeping their human reference copper. Its headline metric, Clean Pass (fully connected and 0 error-level DRC), matches our bar. Published Clean Pass on D3-A / D3-B (best-of-5): Freerouting 0.80 / 0.78, KiCadRoutingTools 0.74 / 0.20. The most direct public leaderboard for kct route.
• PCBSchemaGen v2 (MIT, Python, 12★) -- 227 schematic-synthesis tasks (62 hand-written, 165 from public schematics) with a deterministic 5-layer verifier that needs no LLM: ERC invariants, pin-role compatibility, per-IC connection templates, topology motifs and power rules. Tasks are scored as SKiDL designs. A ready-made eval for our schematic generation.
• PCB-Bench (no LICENSE committed, Python, 49★) -- an ICLR 2026 benchmark of LLM knowledge about PCB placement and routing: about 3,700 text questions, about 500 image-and-text questions, and 174 OSHWHub designs to describe from screenshots. It measures what a model knows about layout, not what a tool produces, so it bears on our agent-facing docs rather than on kct route. No LICENSE, so ideas only.
• KiPI (GPL-3.0-or-later, Python, 83★) -- a power-integrity analyzer (DC voltage drop and current density, AC PDN impedance, switcher coupled noise) that runs as a KiCad IPC plugin or standalone. No solver CLI, but its DC solver is importable without the GUI and solved one rail of our board 09 in 0.1 s. GPL-3.0: ideas only, no code in either direction. Our evaluation: docs/research/kipi-evaluation.md.
• JLC2KiCadLib (MIT, Python, 488★) -- generates KiCad symbols, footprints and STEP/WRL models from EasyEDA (v1.3.2, maintenance-only). MIT, so code may move with attribution, but its licence does not grant any rights to the EasyEDA/LCSC content it fetches. Our evaluation: docs/research/3d-model-coverage.md.
• kicadStepUpMod (no LICENSE committed, Python (FreeCAD), 696★) -- FreeCAD workbench for aligning 3D models to footprints, the manual analogue of our transform calibration. The README claims AGPLv3 but no LICENSE file is committed (hence license = "NONE"); ideas only either way. Our evaluation: docs/research/3d-model-coverage.md.
• cq-electronics (MIT, Python (CadQuery), 20★) -- small CadQuery set of electronic-component parts (v0.2.0). MIT, so it is a candidate source of parametric bodies for our own 3D pipeline. Our evaluation: docs/research/3d-model-coverage.md.

License

MIT