kicad-tools 0.18.0

Standalone Python tools for parsing and manipulating KiCad schematic and PCB files

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 - All CLI commands support --format json
• 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

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 --strict

# Run DRC with manufacturer rules
kct drc board.kicad_pcb
kct drc board.kicad_pcb --mfr jlcpcb
kct drc --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
    clearance=0.15,        # mm
)

# Create router and add components
router = Autorouter(width=100, height=80, rules=rules)
router.add_component("U1", pads=[...])

# Route all nets
result = router.route_all()
print(f"Routed {result.routed_nets}/{result.total_nets} nets")

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

Configure Claude Desktop (~/Library/Application Support/Claude/claude_desktop_config.json):

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

Available MCP tools:

• Analysis: analyze_board, 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)

# Add USB connector with ESD protection
usb = USBConnector(sch, x=50, y=150,
    connector_type="type-c", esd_protection=True)

# Add debug header for programming
debug = DebugHeader(sch, x=200, y=100, interface="swd")

# Add I2C pull-ups
i2c = I2CPullups(sch, x=180, y=150, pullup_value="4.7k")

# Add reset button with debounce
reset = ResetButton(sch, x=120, y=50, debounce_cap="100nF")

# Connect via ports
sch.add_wire(ldo.port("VOUT"), mcu.port("VDD"))
sch.add_wire(xtal.port("OUT"), mcu.port("OSC_IN"))

sch.save()

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 with custom rules
kct check board.kicad_pcb --clearance 0.15 --trace-width 0.2

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 board.kicad_pcb --optimize --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 pin tables
kct datasheet extract-pins datasheet.pdf

# 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)

Command	Description
kct symbols <schematic>	List symbols with filtering
kct nets <schematic>	Trace and analyze nets
kct bom <schematic>	Generate bill of materials
kct erc <schematic>	Run electrical rules check
kct drc <pcb>	Run design rules check (requires kicad-cli)
kct check <pcb>	Pure Python DRC (no kicad-cli needed)
kct creepage <pcb>	HV surface-path (creepage) audit vs IEC 60664-1 / 62368-1
kct analyze <pcb>	Signal-integrity + current-sense analog layout lint
kct route <pcb>	Autoroute a PCB (--nets/--skip-nets to select nets)
kct reason <pcb>	LLM-driven PCB layout reasoning
kct placement <pcb>	Detect and optimize component placement
kct optimize-placement <pcb>	CMA-ES/Bayesian global placement optimization
kct route-auto <pcb>	Orchestrator-based multi-strategy autorouting
kct optimize-traces <pcb>	Optimize routed traces
kct datasheet <subcommand>	Search, download, parse datasheets
kct parts <subcommand>	LCSC/JLCPCB part lookup, cache, offline catalog sync
kct export <pcb>	Manufacturing bundle export (gerbers, BOM, CPL)
kct mfr <subcommand>	Manufacturer rule profiles (apply-rules, validate)
kct fleet status	Routing + manufacturing readiness across all boards
kct mcp serve	Start MCP server for AI agent integration

All commands support --format json for machine-readable output.

PCB Tools

Command	Description
kicad-pcb-query summary	Board overview
kicad-pcb-query footprints	List footprints
kicad-pcb-query nets	List all nets
kicad-pcb-query traces	Trace statistics
kicad-pcb-modify move	Move component
kicad-pcb-modify rotate	Rotate component

Library Tools

Command	Description
kicad-lib-symbols	List symbols in library

Modules

Module	Description
core	S-expression parsing and file I/O
schema	Data models (Schematic, PCB, Symbol, Wire, Label)
schematic.blocks	Reusable circuit blocks (MCU, LDO, USB, debug headers, etc.)
project	Unified Project class for schematic+PCB workflows
library	Footprint generation and symbol library management
drc	Design Rule Check report parsing (kicad-cli output)
validate	Pure Python DRC checker (no kicad-cli needed)
erc	Electrical Rule Check report parsing
manufacturers	PCB fab profiles (JLCPCB, OSHPark, PCBWay, Seeed)
operations	Schematic operations (net tracing, symbol replacement)
router	A* PCB autorouter with trace optimization
optim	Placement optimization (physics-based, evolutionary)
reasoning	LLM-driven PCB layout with chain-of-thought reasoning
progress	Progress callbacks for long-running operations
datasheet	Datasheet search, download, and PDF parsing
mcp	MCP server for AI agent integration
layout	Layout preservation for PCB regeneration

What's New (v0.16.0, July 2026)

Recent additions an agent reading these docs cold should know about:

• Router feasibility & coupling flags on kct route — --monotone-certificate-order (certify a bundle's escape feasibility and derive a constructive net order), --cross-package-pair-corridor, and --slack-corridor-widening (all default off). Coupled diff-pair attempts that all budget-exit now early-abort to a plain single-ended route instead of degrading the result.
• JLCPCB parts stack — kct parts sync-catalog mirrors the full jlcparts dataset for offline lookups; set JLCPCB_ACCESS_KEY/JLCPCB_SECRET_KEY to use the official open-platform API (see Parts Lookup below).
• kct check --refill-zones — refill zone fills via kicad-cli before the pure-Python checks, killing stale-fill clearance false positives; a loud advisory now fires when copper is measured against possibly-stale fills.
• Hierarchical-schematic LVS — multi-sheet designs are no longer vacuous.
• /kct:tapeout skill — one command that produces a complete, fab-ready export bundle or refuses loudly.
• kct fleet status — survey routing + manufacturing readiness across every board in boards/. The "are we ship-ready?" entry point. See Manufacturing Export → ship-ready check.
• kct route --auto-layers / --auto-mfr-tier — automatic layer-count and manufacturer-tier escalation when routing hits a wall. --auto-layers defaults to enabled; opt out with --no-auto-layers. See Routing → Strategy Escalation.
• kct route --checkpoint-interval — atomic best-so-far writes every N seconds; SIGINT leaves a valid PCB on disk. See Routing → Long-Running Routes.
• kct optimize-placement --anchor-weight — CMA-ES placement optimizer biased toward locked footprints. The validated recipe (lock perimeter parts only, weight 1.0, --allow-infeasible) lifted board-05 BLDC from 40% → 60% routing completion. See Placement Optimization → Anchoring Perimeter Footprints.
• kct stitch --mfr / --copper — stackup-aware via dimensions; the manufacturer YAML drives via geometry. See CLI Reference → stitch.
• kct build --step preflight-routing — routing-completeness gate that blocks manufacturing artefacts when nets are unrouted. Override with --allow-incomplete. See Manufacturing Export → Routing Completeness Preflight.
• Footprint.locked + siblings round-trip through PCB.save (locked, dnp, exclude_from_pos_files, exclude_from_bom, plus preserved unknown (attr ...) tokens). See API → Footprint attributes.

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

When creating a new git worktree (e.g. via ./.loom/scripts/worktree.sh), the worktree's .venv/ does not inherit the C++ extension built in the main checkout. After cd into the worktree, run uv run kct build-native once before any routing benchmarks.

Available Commands

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

Command	Description
pnpm setup	Set up dev environment (uv sync --extra dev)
pnpm test	Run tests
pnpm test:cov	Run tests with coverage
pnpm test:benchmark	Run performance benchmarks
pnpm lint	Check code with ruff
pnpm lint:fix	Auto-fix lint issues
pnpm format	Format code with ruff
pnpm format:check	Check formatting
pnpm typecheck	Run mypy type checking
pnpm check:ci	Run full CI suite (format + lint + tests)

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. Five skills ship today — /kct:tapeout (complete fab-ready export bundle or loud refusal), /kct:manufacturing-readiness (sign-off gates), /kct:board-recipe-scaffold, /kct:layout-journal, and /kct:ee-review (advisory EE decision document for analog/placement-blocked boards). See .claude/commands/kct/README.md for the full contracts.

Related Projects

• Zeo — 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.
• kipy — Python bindings for the KiCad 9.0+ IPC API. Could be used to push kicad-tools optimization results into a running KiCad instance.

License

MIT