Skip to content

intro.md

Latest commit

 

History

History
106 lines (79 loc) · 3.28 KB

intro.md

File metadata and controls

106 lines (79 loc) · 3.28 KB

Getting Started with SpiceSharpParser

SpiceSharpParser is a .NET library that parses SPICE netlists and simulates them using SpiceSharp. It supports a wide subset of PSpice and LTspice syntax including DC, AC, transient, noise, and operating-point analyses.

Installation

Install from NuGet:

dotnet add package SpiceSharp-Parser

Or via the NuGet Package Manager:

Install-Package SpiceSharp-Parser

Quick Example

using System;
using System.Linq;
using SpiceSharpParser;

var netlist = string.Join(Environment.NewLine,
    "Low-pass RC filter",
    "V1 IN 0 AC 1",
    "R1 IN OUT 1k",
    "C1 OUT 0 1u",
    ".AC DEC 10 1 1MEG",
    ".SAVE V(OUT)",
    ".END");

// Parse
var parser = new SpiceNetlistParser();
var parseResult = parser.ParseNetlist(netlist);

// Translate to SpiceSharp objects
var reader = new SpiceSharpReader();
var spiceModel = reader.Read(parseResult.FinalModel);

// Run simulation
var sim = spiceModel.Simulations.Single();
var export = spiceModel.Exports.Find(e => e.Name == "V(OUT)");
sim.EventExportData += (sender, args) => Console.WriteLine(export.Extract());
sim.Execute(spiceModel.Circuit);

Workflow Overview

Using SpiceSharpParser involves three steps:

  1. Parse — convert a SPICE netlist string into a parse-tree model with SpiceNetlistParser.ParseNetlist().
  2. Read — translate the parse-tree model into SpiceSharp simulation objects (circuit, simulations, exports) with SpiceSharpReader.Read().
  3. Simulate — run the SpiceSharp simulations and collect results via exports and events.

The SpiceSharpModel

SpiceSharpReader.Read() returns a SpiceSharpModel containing:

Property Description
Circuit The SpiceSharp Circuit with all components
Simulations List of simulation objects (DC, AC, Transient, etc.)
Exports Signal exports created by .SAVE, .PRINT, .PLOT
XyPlots Plot data from .PLOT statements
Prints Tabular data from .PRINT statements
Measurements Results from .MEAS / .MEASURE statements
Title Netlist title (first line)

Collecting Results

Export data during simulation using the EventExportData event:

var export = spiceModel.Exports.Find(e => e.Name == "V(OUT)");
sim.EventExportData += (sender, args) =>
{
    double value = (double)export.Extract();
    // process value
};

Parameter Sweeps (.STEP)

When .STEP is used, the simulation runs multiple times. Each sweep iteration fires EventExportData with appropriate parameter values:

sim.EventExportData += (sender, args) =>
{
    Console.WriteLine($"{export.Extract()}");
};

Supported Features

SpiceSharpParser supports a comprehensive set of SPICE statements and devices. See the individual documentation articles for details on each:

  • Analysis: .AC, .DC, .TRAN, .OP, .NOISE
  • Output: .SAVE, .PRINT, .PLOT, .MEAS
  • Parameters: .PARAM, .FUNC, .LET, .SPARAM
  • Circuit structure: .SUBCKT, .INCLUDE, .LIB, .GLOBAL
  • Simulation control: .STEP, .MC, .TEMP, .OPTIONS, .IC, .NODESET
  • Behavioral modeling: VALUE, TABLE, POLY(n), B sources
  • Devices: R, L, C, K, D, Q, M, J, V, I, E, F, G, H, B, S, W, T, X