ltspice-mcp

Work in progress. Core functionality is usable but expect rough edges and breaking changes.

An MCP server that connects LLM assistants (Claude, and any other MCP client) to real circuit simulation: LTspice and ngspice, plus direct editing of LTspice .asc schematics. Simulation results come back as structured numbers — cutoff frequencies, overshoot, phase margin, rise times — so the assistant can design, verify, and iterate on circuits in the same files you open in LTspice. Built on spicelib.

Quick start

1. Install the server:

uv tool install ltspice-mcp     # or: pip install ltspice-mcp / pipx install ltspice-mcp

2. Add it to your MCP client:

# Claude Code
claude mcp add -s project ltspice -- ltspice-mcp

// Claude Desktop (claude_desktop_config.json) and most other clients
{
  "mcpServers": {
    "ltspice": { "command": "ltspice-mcp", "args": [] }
  }
}

3. Have LTspice or ngspice installed. Both are auto-detected on Windows, Linux, and macOS; on WSL the LTspice path must be set explicitly (WSL notes). Circuit editing works with no simulator at all.

That's the setup. Python 3.13+ required. Verify with ltspice-mcp --help.

Claude Desktop config lives at ~/Library/Application Support/Claude/ (macOS), %APPDATA%\Claude\ (Windows), or ~/.config/Claude/ (Linux). Cursor, Windsurf, Gemini CLI, Continue, Cline, Zed and others take the same JSON snippet in their respective config files. Web clients (claude.ai, ChatGPT) need a stdio→HTTP bridge such as mcp-proxy — only expose this server on a network you fully control, since it writes files and spawns processes inside allowed_paths.

Using it

Once connected, you ask for circuit work in plain language. The assistant chooses the tools; the server runs the simulator and measures the results.

"Design a 1 kHz RC low-pass filter and verify its cutoff."

The assistant writes the netlist, validates it, runs an AC simulation, and reads the measurements back: cutoff 1000.4 Hz, −19.9 dB/decade roll-off, first-order response. If the cutoff is off-target, it changes a component value and re-runs — each iteration is a couple of seconds.

Other requests that work the same way:

• "What's the overshoot and settling time of this regulator's step response?" — runs a transient analysis and measures both from the waveform, plus rise time, ringing frequency, and the final value.
• "Run a 200-run Monte Carlo with 5% resistors and tell me the output spread." — perturbs components per run, simulates the batch, and reports mean, sigma, and worst-case values per measurement.
• "Sweep the load from 100 Ω to 10 kΩ and find where efficiency drops." — parameter sweep with per-run results.
• "Turn this netlist into a schematic I can open in LTspice." — generates a wired .asc file that produces the same circuit.
• "Is this loop stable?" — AC analysis of the loop gain; reports phase and gain margin at every crossover, not just the first.

Co-design on the same files

Everything operates on ordinary LTspice and SPICE files, so the work passes back and forth between you and the assistant instead of living inside a chat:

• Sketch a schematic in LTspice, then hand it over: "what's the bias point?", "why doesn't the output move?", "add compensation and check the phase margin."
• Or the reverse: the assistant designs and verifies the circuit and writes the .asc; you open it in LTspice, inspect it, and tweak by hand. Your manual edits are simply the file's new state — the assistant picks up from there on the next request.
• Changes can flow either direction mid-design: adjust a value in the GUI and ask for re-verification, or have the assistant sweep a change you're considering before you commit to it.

What it does

Simulation and measurement. Runs LTspice or ngspice and parses the binary output directly. Measurements are computed server-side and returned as numbers: time-domain (rise/fall, overshoot, settling, delay, period/duty/jitter, RMS), frequency-domain (filter cutoffs and roll-off, gain and phase at any frequency, stability margins, resonance peaks with Q), DC operating points, and .MEAS directive results including the ones that failed.

Schematic and netlist editing. Creates and edits real LTspice .asc files — place components, wire pins, label nets — with validation before anything is written: wiring that would collide with a pin, overlap a junction, or run diagonally is refused, and every edit returns warnings about floating pins or dangling labels. A netlist converts to a working schematic in one step; a session's edits can be reverted. Plain netlists (.cir/.net) get the same operations at text level, plus a static validation pass that catches malformed cards before a simulation is spent.

Sweeps and Monte Carlo. Multi-dimensional parameter sweeps and Monte Carlo with per-component tolerances, .MODEL process variation, and Pelgrom W·L device mismatch. Per-measurement statistics are aggregated across runs, and any single run can be pulled out and analyzed like a standalone simulation.

Jobs and trust. Simulations run as cancellable jobs with timeouts and a concurrency cap; long runs return a job ID immediately and job state survives a server restart. Results report facts, not verdicts: a completed run carries the simulator's own warnings, measurements that produced nothing, and extreme node values as structured observations. Judging whether a result is trustworthy is left to the model reading it.

Supported simulators

Simulator	Status
LTspice	Primary. Windows native, WSL2 (Windows LTspice.exe via interop), Linux via Wine. Required for .asc schematic editing (needs .asy symbol libraries).
ngspice	First-class: simulate, parse, diagnose, analyze. Open-source path with no LTspice install.
QSPICE, Xyce	Supported but secondary.

Configuration

Works with defaults out of the box. To customize, copy ltspice-mcp.example.toml to ltspice-mcp.toml; any setting can be overridden with an LTSPICE_MCP_-prefixed environment variable, and --config PATH or LTSPICE_MCP_CONFIG picks the file. Key options:

[simulator]
default = "ltspice"      # ltspice, ngspice, qspice, xyce (null = auto-detect)
path = ""                # explicit executable path (required on WSL)

[security]
allowed_paths = ["."]    # sandbox: only these directories are accessible

[simulation]
max_parallel = 4
timeout = 300.0          # seconds

[tools]
profile = "full"         # or "agentic"

[state]
persist_jobs = true

See src/ltspice_mcp/config.py for the full option list ([analysis], [schematic], [logging], ...).

<details> <summary><strong>WSL specifics</strong></summary>

On WSL, LTspice.exe runs via Windows interop (not Wine), and spicelib can't auto-detect it across the WSL boundary. Set the Windows-side path explicitly:

[simulator]
path = "/mnt/c/Program Files/ADI/LTspice/LTspice.exe"

Simulation output is automatically redirected to a Windows temp directory: LTspice's .MEAS results go through SQLite .db files that fail on UNC paths (\\wsl.localhost\...), and without the redirect measurement data silently disappears from the logs.

.asy symbol paths for .asc editing are auto-detected on Windows and WSL; override with [schematic] symbol_paths or LTSPICE_MCP_SYMBOL_PATHS.

</details>

Tool profiles

Profile	Tools	Use case
full (default)	48	Any MCP client, automation, non-agent LLMs
agentic	32	LLM agents with native file access (Read/Edit/Write)

The agentic profile drops netlist-editing wrappers and library session management — work a capable agent does through direct file edits — and keeps simulation lifecycle, binary .raw parsing, batch orchestration, and the .asc geometry tools. The skills/ directory (skills/ltspice/SKILL.md, skills/ngspice/SKILL.md) contains the domain knowledge that pairs with it: copy the relevant skill into your client's persistent-instructions location.

Under the hood: the tool-level loop

What the assistant actually does for "design a 1 kHz RC low-pass and verify it". It writes the netlist (R=1k, C=159.155n → fc = 1 kHz):

* rc.cir — RC low-pass
V1 in 0 AC 1
R1 in out 1k
C1 out 0 159.155n
.ac dec 50 1 1Meg
.end

then drives three tools:

validate_netlist(path="rc.cir")
  → OK: directives valid, element arities check out — safe to simulate

run_simulation(netlist="rc.cir")
  → {"job_id": "sim_a3f1", "status": "completed", "raw_file": ".../rc.raw", ...}

bode_metrics(raw_file=".../rc.raw", signal="V(out)", mode="filter")

and gets back scalars, not a plot:

{
  "signal": "V(out)",
  "filter_type": "lowpass",
  "passband_gain_db": 0.0,
  "passband_ripple_db": 0.02,
  "cutoff_low_hz": null,
  "cutoff_high_hz": 1000.4,
  "stopband_rejection_db": 59.97,
  "rolloff_slope_db_per_decade": -19.9,
  "estimated_order": 1,
  "warnings": []
}

(abridged — the full response also includes passband bounds and transition bandwidth)

Off-target → set_component_value, re-run, re-measure. Long simulations return a job ID instead of blocking; check_job/cancel_job manage them. Job metadata persists in per-circuit sidecars ({dir}/.ltspice-mcp/jobs/ — add .ltspice-mcp/ to your .gitignore), and MCP resources (ltspice://results/..., ltspice://netlists/..., ltspice://config) expose jobs, signals, measurements, and config for browsing.

<details> <summary><strong>All 48 tools</strong></summary>

Every tool declares MCP annotations (readOnlyHint, destructiveHint, idempotentHint, openWorldHint); data-returning tools declare an outputSchema for structuredContent introspection.

Tool	Description
create_netlist	Create a new netlist from a content string
create_schematic	Create an empty .asc ready for incremental editing
schematic_from_netlist	Generate an .asc from SPICE netlist text — grid-places R/C/L/V/I/D and wires pins by net label
read_circuit	Read a circuit file (netlist text for .cir, schematic layout for .asc)
list_components	List components (optional prefix filter) or look up one by reference
set_component_value	Set one component value, or batch-set many via a values dict
parameter	Read all .PARAM values or set one
edit_directive	Add or remove SPICE directives (.tran, .ac, .lib, ...)
remove_component	Remove a component (warns about orphaned wires)
move_component	Move or rotate a component in an .asc schematic
set_component_attribute	Set a component attribute (SpiceLine, Value2, ...)
add_component	Add a component; returns pin positions, bounding box, overlap warnings
connect	Wire two pins by reference with waypoint routing; validates pin collisions, junctions, diagonals
add_net_label	Add/remove net labels and ground flags (supports pin-reference placement)
symbol_info	Symbol pin positions, directions, bounding box, description
component_info	Placed component pin positions, bounding box, attributes
export_netlist	Export .asc to .net via LTspice (with diff against previous export)
validate_netlist	Static pre-flight checks on a netlist or schematic before simulation
trace_net	Every pin/label/wire on a net at a pin / net:NAME / (x,y); flags accidental shorts
reset_schematic	Revert an .asc to its pre-edit snapshot from this session
diff_circuit	Structural diff between two circuit files
apply_schematic_ops	Apply many .asc edits in one transaction
run_simulation	Run a simulation — sync for short runs, async (job ID) for long ones
check_job	Check a job's status by ID, or list all jobs
cancel_job	Cancel a running simulation or batch; kills the simulator process(es)
signal_stats	Min, max, mean, RMS, peak-to-peak (dB/phase for AC)
query_value	Signal value at a specific time/frequency; step_axis+step_value picks a .step run
operating_point	DC operating point: all node voltages and branch currents
simulation_summary	Full summary: simulation type, signals, measurements, warnings
edge_metrics	Rise/fall time and slew rate for one transient edge
pulse_response	Overshoot, undershoot, settling time for a step response
timing_between	Propagation delay between two transient signals
periodic_metrics	Period, frequency, duty cycle, jitter of an oscillating signal
measurement_stats	Aggregate .MEAS scalars across a sweep or Monte Carlo run
bode_metrics	AC/Bode analysis by mode: filter, slope, point, crossing; all_steps=true for per-step results
stability_metrics	Loop-gain stability: all unity-gain / -180° crossings with per-crossing margins
resonance	AC peaks with Q factor and -3 dB bandwidth per peak
configure_sweep	Configure a multi-parameter sweep (linear or log)
run_sweep	Execute a configured sweep (async, returns job ID)
configure_montecarlo	Configure Monte Carlo: tolerances, .MODEL variation, Pelgrom mismatch
run_montecarlo	Execute a configured Monte Carlo analysis (async, returns job ID)
batch_results	Sweep/MC job progress, per-signal statistics, or per-run data
find_model	Find model candidates by name (fuzzy by default, exact=true for exact)
load_library	Load a .lib/.mod file or a directory of libraries
unload_library	Unload a previously loaded library
list_libraries	List loaded libraries, optionally with model names
server_status	Detected simulators, config, sandbox paths, runtime state
recent	Recently-used circuits and jobs from the persistent index

</details>

Development

uv sync                        # install runtime + dev dependencies
uv run pytest tests/ -v        # tests
uv run pyright                 # type checking
uv run ruff check src/ tests/  # lint
uv run ltspice-mcp             # run the server (stdio)

More: docs/DESIGN.md (scope, architecture, non-goals) and docs/spice_lex.md (SPICE parser internals).

License

GPL-3.0