Skip to main content

A set of tools to Automate LTSpice simulations

Project description


PyLTSpice is a toolchain of python utilities design to interact with LTSpice and NGSpice Electronic Simulator.

What is contained in this repository

  • An utility that extracts from LTSpice output files data, and formats it for import in a spreadsheet, such like Excel or Calc.

  • A pure python class that serves to read raw files into a python class.

  • A class to write RAW files that can be read by LTSpice Wave Application.

  • A python script that uses numpy and matplotlib to create an histogram and calculate the sigma deviations. This is useful for Monte-Carlo analysis.

  • This is a script to launch Spice Simulations. This is useful because:

    • Can overcome the limitation of only stepping 3 parameters
    • Different types of simulations .TRAN .AC .NOISE can be run in a single batch
    • The RAW Files are smaller and easier to treat
    • When used with the and, validation of the circuit can be done automatically.
    • Different models can be simulated in a single batch, by using the following instructions:
      • set_element_model('D1', '1N4148') # Replaces the Diode D1 with the model 1N4148
      • set_component_value('R2', '33k') # Replaces the value of R2 by 33k
      • set_parameters(run=1, TEMP=80) # Creates or updates the netlist to have .PARAM run=1 or .PARAM TEMP=80
      • add_instructions(".STEP run -1 1023 1", ".dc V1 -5 5")
      • remove_instruction(".STEP run -1 1023 1") # Removes previously added instruction
      • reset_netlist() # Resets all edits done to the netlist.

    Note: It was only tested with Windows based installations.

How to Install

pip install PyLTSpice

Updating PyLTSpice

pip install --upgrade PyLTSpice

Using GITHub

git clone

If using this method it would be good to add the path where you cloned the site to python path.

import sys
sys.path.append(<path to PyLTSpice>)

How to use

Here follows a quick outlook on how to use each of the tools.

More comprehensive documentation can be found in


GNU V3 License (refer to the LICENSE file)

The example below reads the data from a Spice Simulation called "TRAN - STEP.raw" and displays all steps of the "I(R1)" trace in a matplotlib plot

from PyLTSpice import RawRead

from matplotlib import pyplot as plt

LTR = RawRead("TRAN - STEP.raw")


IR1 = LTR.get_trace("I(R1)")
x = LTR.get_trace('time')  # Gets the time axis
steps = LTR.get_steps()
for step in range(len(steps)):
   # print(steps[step])
   plt.plot(x.get_wave(step), IR1.get_wave(step), label=steps[step])

plt.legend()  # order a legend

The following example writes a RAW file with a 3 milliseconds transient simulation sine with a 10kHz and a cosine with 9.997kHz

import numpy as np
from PyLTSpice import Trace, RawWrite

LW = RawWrite(fastacces=False)
tx = Trace('time', np.arange(0.0, 3e-3, 997E-11))
vy = Trace('N001', np.sin(2 * np.pi * * 10000))
vz = Trace('N002', np.cos(2 * np.pi * * 9970))

This module is used to launch LTSPice simulations. Results then can be processed with either the RawRead or with the LTSteps module to read the log file which can contain .MEAS results.

The script will firstly invoke the LTSpice in command line to generate a netlist, and then this netlist can be updated directly by the script, in order to change component values, parameters or simulation commands.

Here follows an example of operation.

from PyLTSpice import SimRunner
from PyLTSpice import SpiceEditor

# select spice model
LTC = SimRunner(output_folder='./temp')
netlist = SpiceEditor('')
# set default arguments
netlist.set_parameters(res=0, cap=100e-6)
netlist.set_component_value('R2', '2k')  # Modifying the value of a resistor
netlist.set_component_value('R1', '4k')
netlist.set_element_model('V3', "SINE(0 1 3k 0 0 0)")  # Modifying the
netlist.set_component_value('XU1:C2', 20e-12)  # modifying a define simulation
        "; Simulation settings",
        ".param run = 0"

for opamp in ('AD712', 'AD820'):
    netlist.set_element_model('XU1', opamp)
    for supply_voltage in (5, 10, 15):
        netlist.set_component_value('V1', supply_voltage)
        netlist.set_component_value('V2', -supply_voltage)
        print("simulating OpAmp", opamp, "Voltage", supply_voltage)

for raw, log in LTC:
    print("Raw file: %s, Log file: %s" % (raw, log))
    # do something with the data
    # raw_data = RawRead(raw)
    # log_data = LTSteps(log)
    # ...

        "; Simulation settings",
        ".ac dec 30 10 1Meg",
        ".meas AC Gain MAX mag(V(out)) ; find the peak response and call it ""Gain""",
        ".meas AC Fcut TRIG mag(V(out))=Gain/sqrt(2) FALL=last"

# Sim Statistics
print('Successful/Total Simulations: ' + str(LTC.okSim) + '/' + str(LTC.runno))

enter = input("Press enter to delete created files")
if enter == '':

# Sim Statistics
print('Successful/Total Simulations: ' + str(LTC.okSim) + '/' + str(LTC.runno))

This module defines a class that can be used to parse LTSpice log files where the information about .STEP information is written. There are two possible usages of this module, either programmatically by importing the module and then accessing data through the class as exemplified here:

from PyLTSpice.LTSteps import LTSpiceLogReader

data = LTSpiceLogReader("Batch_Test_AD820_15.log")

print("Number of steps  :", data.step_count)
step_names = data.get_step_vars()
meas_names = data.get_measure_names()

# Printing Headers
print(' '.join([f"{step:15s}" for step in step_names]), end='')  # Print steps names with no new line
print(' '.join([f"{name:15s}" for name in meas_names]), end='\n')
# Printing data
for i in range(data.step_count):
    print(' '.join([f"{data[step][i]:15}" for step in step_names]), end='')  # Print steps names with no new line
    print(' '.join([f"{data[name][i]:15}" for name in meas_names]), end='\n')  # Print Header

print("Total number of measures found :", data.measure_count)

The second possibility is to use the module directly on the command line python -m PyLTSpice.LTSteps <filename> The <filename> can be either be a log file (.log), a data export file (.txt) or a measurement output file (.meas) This will process all the data and export it automatically into a text file with the extension (tlog, tsv, tmeas) where the data read is formatted into a more convenient tab separated format. In case the <logfile> is not provided, the script will scan the directory and process the newest log, txt or out file found.

This module uses the data inside on the filename to produce an histogram image.

Usage: [options] LOG_FILE TRACE

 --version             show program's version number and exit
 -h, --help            show this help message and exit
 -s SIGMA, --sigma=SIGMA
                       Sigma to be used in the distribution fit. Default=3
 -n NBINS, --nbins=NBINS
                       Number of bins to be used in the histogram. Default=20
 -c FILTERS, --condition=FILTERS
                       Filter condition writen in python. More than one
                       expression can be added but each expression should be
                       preceded by -c. EXAMPLE: -c V(N001)>4 -c parameter==1
                       -c  I(V1)<0.5
 -f FORMAT, --format=FORMAT
                       Format string for the X axis. Example: -f %3.4f
 -t TITLE, --title=TITLE
                       Title to appear on the top of the histogram.
 -r RANGE, --range=RANGE
                       Range of the X axis to use for the histogram in the
                       form min:max. Example: -r -1:1
 -C, --clipboard       If the data from the clipboard is to be used.
                       Name of the image File. extension 'png'

A tool to convert .raw files into csv or Excel files.

Usage: [options] <rawfile> <trace_list>

  --version             show program's version number and exit
  -h, --help            show this help message and exit
  -o FILE, --output=FILE
                        Output file name. Use .csv for CSV output, .xlsx for
                        Excel output
  -c, --clipboard       Output to clipboard
  -v, --verbose         Verbose output
                        Value separator for CSV output. Default: "\t" <TAB>
                        Example: -d ";"

This module is used to read from LTSpice log files Semiconductor Devices Operating Point Information. A more detailed documentation is directly included in the source file docstrings.

To whom do I talk to?


  • Version 4.0.3
    Fixing issue in elapsed time calculation. Fixing issue with the import of LTSpiceLogReader from

  • Version 4.0.2
    Changing list of Library dependencies.

  • Version 4.0.1
    Bug fix on CLI for the and

  • Version 4.0.0
    Separating the SimCommander into two separate classes, one for the spice netlist editing (SpiceEditor) and another for the simulation execution (SimRunner).
    Implementing simulation server to allow for remote simulation execution and the respective client.
    Supporting Wiggler element in the new LTSpiceXVII.
    Renaming all files into lowercase.
    Creating Error classes for better error handling.
    Adding support for other simulators (ex: ngspice) where the simulator is defined by a class. This support class needs to be a subclass of the abstract class Simulator.
    Enormous improvement in the documentation of the code.

  • Version 3.0
    Eliminating the LTSpice prefixes from files and classes.
    Adopting the lowercase convention for filenames.

  • Version 2.3.1
    Bug fix on the parameter replacement

  • Version 2.3
    Supporting the creation of RAW Noise Analysis
    Bug Fixes (See GitHub Log)

  • Version 2.2
    Making numpy as an requirement and eliminating all code that avoided the use of numpy
    Using new packaging tool
    Fixes on the LTSpice_RawWrite
    Fixes in the handling of stepped operating point simulations

  • Version 2.1
    Adopting minimum python version 3.7
    Starting to use unit tests to validate all modules and improving testbenches
    Compatibility with NGSpice
    Avoiding the use of as per PEP517 and PEP518
    Bug Fixes (See GitHub log for more information)
    Improvements on the management of stepped data in the

  • Version 2.0.2
    Improvements on Encoding detection

  • Version 2.0
    International Support using the correct encoding when loading log files.
    Code Optimizations on the LTSpice_RawReader that allow faster data loading.
    Improving the functionality on the
    Adding support to editing components inside subcircuits (.subckt)
    Supporting resistors with Model Definitions
    Fixing problem with LTSpiceLogReader that would return messed up data
    Fixing problem with replacing the file extension in certain names
    Correcting problem with deprecations on the numpy functions used by the
    Adding back the that somehow was deleted

  • Version 1.9
    Adding support for µ character in the SpiceEditor.
    Adding get_component_floatvalue() method in the netlist manipulating class that handles the conversion of numeric fields into a float. This function takes into account the engineering qualifiers 'k' for kilos, 'm' or milis, 'u' or 'µ' for microns, 'n' for nanos, 'f' for femtos and 'Meg' for Megas.

  • Version 1.8
    Uniforming License reference across files and improvements on the documentation
    An enormous and wholehearted thanks to Logan Herrera (lpherr) for the improvements in the documentation.
    Bugfix on the add_LTspiceRunCmdLineSwitches() ; Supporting .param name value format
    Allowing the LTSpiceRawRead to proceed when the log file can't be found or when there are problems reading it.

  • Version 1.7
    Running in Linux under wine is now possible

  • Version 1.6
    Adding LTSpice_RawWrite. Adding documentation.

  • Version 1.5
    Small fixes and improvements on the class usage. No added features

  • Version 1.4
    Adding the LTSpice_SemiDevOpReader module
    Re-enabling the Histogram functions which where disabled by mistake.

  • Version 1.3
    Bug fixes on the SpiceEditor Class

  • Version 1.2 Adding link to readthedocs documentation
    All files: Comprehensive documentation on how to use each module

  • Version 1.1 Updated the description Corrected the name of the returned raw file.
    Added comments throughout the code and cleanup

  • Version 1.0 Implemented an new approach (NOT BACKWARDS COMPATIBLE), that avoids the usage of the file. And allows to modify not only parameters, but also models and even the simulation commands. Added the get_time_axis method to the RawRead class to avoid the problems with negative values on time axis, when 2nd order compression is enabled in LTSpice. Modified the LTSteps so it can also read measurements on log files without any steps done.

  • Version 0.6 now has an option to make the histogram directly from values stored in the clipboard

  • Version 0.5
    The now uses the struc.unpack function for a faster execution

  • Version 0.4
    Added to the collection of tools

  • Version 0.3
    A version of LTSteps that can be imported to use in a higher level script

  • Version 0.2
    Adding and

  • Version 0.1
    First commit to the bitbucket repository.

Project details

Download files

Download the file for your platform. If you're not sure which to choose, learn more about installing packages.

Source Distribution

PyLTSpice-4.0.3.tar.gz (133.5 kB view hashes)

Uploaded source

Built Distribution

PyLTSpice-4.0.3-py3-none-any.whl (138.0 kB view hashes)

Uploaded py3

Supported by

AWS AWS Cloud computing and Security Sponsor Datadog Datadog Monitoring Fastly Fastly CDN Google Google Download Analytics Microsoft Microsoft PSF Sponsor Pingdom Pingdom Monitoring Sentry Sentry Error logging StatusPage StatusPage Status page