neospice

A SPICE circuit simulator written from scratch in C++20 -- not a fork of ngspice or any Berkeley SPICE derivative. Clean architecture, native Python bindings, and MIT licensed with no LGPL baggage.

Reads standard SPICE netlists and produces ngspice-compatible results, but runs 1.2--8x faster per-analysis in-process with a custom sparse solver, auto-differentiation in behavioral sources, and a modern embeddable API designed for integration into EDA tools, optimization loops, and notebooks.

Features

10 analysis types -- DC OP, DC sweep, transient (adaptive Trap/Gear-2/BE), AC small-signal, noise (adjoint method), transfer function, sensitivity, pole-zero, Fourier/THD, parameter sweep (.step), and .measure post-processing
32 device models -- passives, independent/dependent/behavioral sources, switches, transmission lines, diodes, BJTs, JFETs, MESFETs, HFETs, and MOSFETs through BSIM4v7
Embeddable C++ API -- Simulator/Circuit/Result types with handle-based and string-based accessors, typed device methods, and circuit introspection
High performance -- NeoSolver (dense + sparse column-LU with AMD ordering), G/C matrix caching for AC, adjoint-method noise
ngspice-compatible -- reads standard SPICE netlists, writes .raw files in ngspice format
972 tests validated against ngspice with tolerances as tight as 1e-6

Quick Start (C++)

Prerequisites

C++20 compiler (GCC 12+ or Clang 15+)
CMake 3.20+
OpenBLAS
SLEEF (vectorized math library)

See docs/building.md for platform-specific install commands.

Build

cmake -B build -DCMAKE_BUILD_TYPE=Release
cmake --build build -j$(nproc)

Run

# Simulate a netlist
./build/neospice circuit.cir

# Specify output file
./build/neospice circuit.cir -o result.raw

# Split output by analysis type
./build/neospice circuit.cir --split

Output is written in ngspice-compatible .raw format, viewable in any waveform viewer (e.g. GTKWave, KST, ngspice's built-in plot).

Test

cd build && ctest -j$(nproc)

Analyses

Analysis	Netlist Command	Description
DC operating point	`.op`	Newton-Raphson with GMIN/source stepping fallback
DC sweep	`.dc V1 0 5 0.1`	1D and nested 2D parameter sweeps
Transient	`.tran 1n 100n`	Adaptive timestepping with LTE control
AC small-signal	`.ac dec 10 1 100meg`	DEC/OCT/LIN frequency sweeps
Noise	`.noise v(out) V1 dec 10 1 100meg`	Adjoint method, per-device breakdown
Transfer function	`.tf v(out) V1`	Gain + input/output impedance
Sensitivity	`.sens v(out)`	DC sensitivity to all parameters
Pole-zero	`.pz`	Transfer function poles and zeros
Fourier	`.four 1meg v(out)`	Harmonic decomposition + THD
Parameter sweep	`.step param R1 1k 10k 1k`	Sweep any parameter across analyses

Device Models

Category	Models
Passives	R (with TC, AC resistance, flicker/thermal noise), C, L, K (mutual inductance)
Sources	V, I -- DC, PULSE, SIN, PWL, EXP, SFFM, AM waveforms
Dependent sources	E (VCVS), G (VCCS), F (CCCS), H (CCVS) -- linear, POLY, TABLE
Behavioral	B-source -- expression-based with auto-diff Jacobians, DDT, IDT, PWL, TABLE
Switches	S (voltage-controlled), W (current-controlled) -- hysteresis
Transmission lines	T (lossless Branin), O (LTRA lossy -- RC/RG/LC/RLC)
Diode	Standard diode (level 1)
BJT	Gummel-Poon, VBIC (levels 4/9/12/13)
JFET	JFET (Shichman-Hodges), JFET2 (Parker-Skellern)
MESFET	MES (GaAs MESFET -- NMF/PMF)
HFET	HFET1 (Curtice Cubic), HFET2 (Chalmers)
MOSFET	MOS1, MOS3, MOS9, BSIM3v32, BSIM3, BSIM4v7, BSIMSOI, HiSIM2, HiSIM_HV

C++ API

Running a netlist

#include "neospice/neospice.hpp"

neospice::Simulator sim;
auto ckt = sim.load("amplifier.cir");
auto result = sim.run(ckt);

// Typed access to results
auto& ac = std::get<neospice::ACResult>(result.analysis);
auto gain_db = ac.magnitude_db("out");
auto phase = ac.phase_deg("out");

Individual analyses

auto dc = sim.run_dc(ckt);
double vout = dc.voltage("out");

auto tran = sim.run_transient(ckt, 1e-9, 1e-6);
auto vout_wave = tran.voltage("out");   // vector<double>

auto ac = sim.run_ac(ckt, neospice::ACMode::DEC, 10, 1.0, 100e6);
auto gain = ac.magnitude_db("out");     // vector<double>

Building circuits programmatically

using namespace neospice;

Circuit ckt;
auto in  = ckt.node("in");
auto out = ckt.node("out");

ckt.V("V1", in, GND, 0.0, 1.0);  // DC=0, AC=1
ckt.R("R1", in, out, 1e3);
ckt.C("C1", out, GND, 100e-12);

Simulator sim;
auto ac = sim.run_ac(ckt, ACMode::DEC, 10, 1.0, 100e6);
auto gain = ac.magnitude_db("out");

Handle-based result access

// String-based (works with any circuit)
double vout = dc.voltage("out");

// Handle-based (O(1) dense array access, type-safe)
NodeId out_id = ckt.find_node("out");
double vout_h = dc.voltage(out_id);
auto vout_ac  = ac.magnitude_db(out_id);

Measurement utilities

#include "neospice/measure.hpp"

NodeId out_id = ckt.find_node("out");
double bw     = measure::bandwidth_3db(ac, out_id);
double rt     = measure::rise_time(tran, out_id, 0.5, 4.5);
double st     = measure::settling_time(tran, out_id, 5.0, 0.05);
double vrms   = measure::rms(tran, out_id);

Circuit introspection

auto nodes   = ckt.node_names();            // {"in", "out", ...}
auto devices = ckt.device_names();          // {"R1", "C1", "V1"}
auto info    = ckt.device_info("R1");       // type, nodes, value
auto conn    = ckt.devices_at_node("out");  // {"R1", "C1"}

// Handle-based introspection
NodeId nid   = ckt.find_node("out");
DevId  did   = ckt.find_device("R1");
auto   name  = ckt.name(nid);              // "out"
auto   dinfo = ckt.device_info(did);       // DeviceInfo struct

Python

pip install neospice

import neospice as ns

# One-liner convenience functions
dc = ns.dc("amplifier.cir")
print(dc.voltage("out"))

ac = ns.ac("filter.cir", mode="dec", npoints=100, fstart=1, fstop=1e9)
plt.semilogx(ac.frequency, ac.magnitude_db("out"))

tran = ns.transient("osc.cir", tstep=1e-9, tstop=1e-6)
plt.plot(tran.time, tran.voltage("out"))

# Parse inline netlists directly
dc = ns.dc("Divider\nV1 in 0 DC 10\nR1 in mid 1k\nR2 mid 0 1k\n.op\n.end\n")
print(dc.voltage("mid"))  # 5.0

# Or use the full Simulator API
sim = ns.Simulator()
ckt = sim.load("amplifier.cir")          # from file
ckt = sim.parse("...\n.op\n.end\n")      # or from string
result = sim.run_ac(ckt, ns.ACMode.DEC, 100, 1, 1e9)

# Build circuits programmatically with typed methods
ckt = ns.Circuit()
ckt.V("V1", "in", "0", 0.0, 1.0)        # DC=0, AC=1
ckt.R("R1", "in", "out", 1e3)
ckt.C("C1", "out", "0", 100e-12)

# SPICE engineering notation
from neospice import parse_value
r = parse_value("4.7k")                  # 4700.0

All result vectors are returned as NumPy arrays. Supports Python 3.10+ on Linux (x86_64, aarch64) and macOS (x86_64, arm64).

Performance

Benchmarked in-process against ngspice-42 on Intel Core Ultra 9 285K, GCC 14, -O3. Both simulators linked as libraries -- no subprocess overhead, no file I/O in timed sections. Median of 10-30 runs.

Benchmark	ngspice	neospice	Speedup
Parse THS4131 (77 nodes)	431 us	199 us	2.2x
Parse resistor divider	44 us	8 us	5.1x
DC OP THS4131 (14 BJTs)	620 us	363 us	1.7x
DC OP resistor divider	49 us	6 us	7.8x
AC THS4131, 81 points	964 us	523 us	1.8x
AC THS4131, 8001 points	21.6 ms	19.3 ms	1.1x
AC RC lowpass, 91 points	111 us	14 us	7.9x
Transient RC lowpass, 500 us	1.11 ms	607 us	1.8x
Transient RLC series, 100 us	1.56 ms	1.96 ms	1.3x ngspice
Transient pulse source, 100 us	992 us	334 us	3.0x
Noise resistor divider, 91 pts	89 us	56 us	1.6x
DC sweep V1, 1001 pts	816 us	197 us	4.1x
E2E THS4131 (.op + .ac)	726 us	524 us	1.4x
E2E OPA1632 (.op + .ac)	6.42 ms	5.90 ms	1.1x

See docs/performance-comparison-with-ngspice.md for the full methodology and results.

Netlist Compatibility

neospice reads standard SPICE netlists:

.param expressions with arithmetic, functions (sqrt, log, exp, sin, if, ...)
.subckt / .ends with parameter defaults (recursion limit 100)
.include / .lib with section selection and circular-inclusion detection
.global, .ic, .nodeset, .options, .func, .save
SPICE suffixes: T, G, MEG, k, m, u, n, p, f

Project Structure

cli/            Command-line interface
include/
  neospice/     Public API headers (types.hpp, neospice.hpp, measure.hpp)
src/
  api/          C++ API (Simulator, typed device methods, measurement utils)
  core/         Analysis engines and linear solvers
  devices/      32 device models, each self-contained with factory registration
  parser/       Netlist parser and expression evaluator
  output/       Raw file writer
python/
  bindings.cpp  nanobind C++ → Python bridge
  neospice/     Python package (convenience API, SPICE notation parser)
tests/
  unit/         Unit tests for all components (970+)
  devices/      Per-device validation against ngspice
  circuits/     Integration test netlists
  python/       Python binding tests
  bench/        Performance benchmarks
docs/           Architecture, performance, and design documentation
tools/          Device migration tooling (ngspice model auto-porter)

Examples

Comparator Relaxation Oscillator

A TLV3201-based Schmitt trigger oscillator simulated with the Python API. Comparator relaxation oscillator.

Contributing

See docs/building.md for platform-specific setup instructions, including building libngspice from source on macOS.

Documentation

Roadmap

Phase	Feature	Status
—	Handle-based API redesign (NodeId/DevId, typed methods, dense results, measurements)	Done
1	Python bindings (nanobind, PyPI wheels, typed construction)	Done
2	Parallel parameter sweeps / Monte Carlo	Planned
3	WebAssembly build for browser simulation	Planned
4	Adjoint sensitivity / gradient computation	Planned
5	Incremental re-simulation	Planned
6	GPU-accelerated simulation (CUDA)	Planned
7	Extended devices (BSIM-CMG, Verilog-A)	Ongoing

See docs/ROADMAP.md for details.

Name		Name	Last commit message	Last commit date
Latest commit History 517 Commits
.claude/commands		.claude/commands
.github/workflows		.github/workflows
cli		cli
docs		docs
examples		examples
include/neospice		include/neospice
python		python
scripts		scripts
src		src
tests		tests
tools		tools
.gitignore		.gitignore
CLAUDE.md		CLAUDE.md
CMakeLists.txt		CMakeLists.txt
CONTRIBUTING.md		CONTRIBUTING.md
LICENSE		LICENSE
NOTICE		NOTICE
README.md		README.md
pyproject.toml		pyproject.toml

Provide feedback

Saved searches

Use saved searches to filter your results more quickly

Repository files navigation

neospice

Features

Quick Start (C++)

Prerequisites

Build

Run

Test

Analyses

Device Models

C++ API

Running a netlist

Individual analyses

Building circuits programmatically

Handle-based result access

Measurement utilities

Circuit introspection

Python

Performance

Netlist Compatibility

Project Structure

Examples

Comparator Relaxation Oscillator

Contributing

Documentation

Roadmap

About

Uh oh!

Releases

Packages

Uh oh!

Contributors

Uh oh!

Languages

Folders and files

Latest commit

History

Repository files navigation

neospice

Features

Quick Start (C++)

Prerequisites

Build

Run

Test

Analyses

Device Models

C++ API

Running a netlist

Individual analyses

Building circuits programmatically

Handle-based result access

Measurement utilities

Circuit introspection

Python

Performance

Netlist Compatibility

Project Structure

Examples

Comparator Relaxation Oscillator

Contributing

Documentation

Roadmap

About

Resources

License

Contributing

Uh oh!

Stars

Watchers

Forks

Releases

Packages 0

Uh oh!

Contributors

Uh oh!

Languages

Packages