A set of tools to Automate LTSpice simulations
Project description
README
PySpicer is a toolchain of python utilities design to interact with LTSpice Electronic Simulator.
What is contained in this repository
-
LTSteps.py An utility that extracts from LTSpice output files data, and formats it for import in a spreadsheet, such like Excel or Calc.
-
LTSpice_RawRead.py A pure python class that serves to read raw files into a python class.
-
LTSpice_RawWrite.py A class to write RAW files that can be read by LTSpice Application.
-
Histogram.py A python script that uses numpy and matplotlib to create an histogram and calculate the sigma deviations. This is useful for Monte-Carlo analysis.
-
LTSpiceBatch.py This is a script to launch LTSpice 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 LTSpiceRaw_Reader.py and LTSteps.py, 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 https://github.com/nunobrum/PyLTSpice.git
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 https://pyltspice.readthedocs.io/en/latest/
LICENSE
GNU V3 License (refer to the LICENSE file)
LTSpice_RawRead.py
The example below reads the data from a LTSpice Simulation called "TRAN - STEP.raw" and displays all steps of the "I(R1)" trace in a matplotlib plot
from PyLTSpice.LTSpice_RawRead import LTSpiceRawRead
from matplotlib import pyplot as plt
LTR = LTSpiceRawRead("TRAN - STEP.raw")
print(LTR.get_trace_names())
print(LTR.get_raw_property())
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_time_axis(step), IR1.get_wave(step), label=steps[step])
plt.legend() # order a legend
plt.show()
LTSpice_RawWrite.py
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.LTSpice_RawWrite import Trace, LTSpiceRawWrite
LW = LTSpiceRawWrite()
tx = Trace('time', np.arange(0.0, 3e-3, 997E-11))
vy = Trace('N001', np.sin(2 * np.pi * tx.data * 10000))
vz = Trace('N002', np.cos(2 * np.pi * tx.data * 9970))
LW.add_trace(tx)
LW.add_trace(vy)
LW.add_trace(vz)
LW.save("teste_w.raw")
LTSpice_Batch
This module is used to launch LTSPice simulations. Results then can be processed with either the LTSpiceRawRead 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.
import os
from PyLTSpice.LTSpiceBatch import SimCommander
def processing_data(raw_file, log_file):
print("Handling the simulation data of %s, log file %s" % (raw_file, log_file))
# select spice model
LTC = SimCommander("Batch_Test.asc")
# set default arguments
LTC.set_parameters(res=0, cap=100e-6)
LTC.set_component_value('R2', '2k')
LTC.set_component_value('R1', '4k')
LTC.set_element_model('V3', "SINE(0 1 3k 0 0 0)")
# define simulation
LTC.add_instructions(
"; Simulation settings",
".param run = 0"
)
for opamp in ('AD712', 'AD820'):
LTC.set_element_model('XU1', opamp)
for supply_voltage in (5, 10, 15):
LTC.set_component_value('V1', supply_voltage)
LTC.set_component_value('V2', -supply_voltage)
# overriding he automatic netlist naming
run_netlist_file = "{}_{}_{}.net".format(LTC.circuit_radic, opamp, supply_voltage)
LTC.run(run_filename=run_netlist_file, callback=processing_data)
LTC.reset_netlist()
LTC.add_instructions(
"; 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"
)
LTC.run()
LTC.wait_completion()
# Sim Statistics
print('Successful/Total Simulations: ' + str(LTC.okSim) + '/' + str(LTC.runno))
LTSteps.py
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 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 is not provided, the script will scan the directory and process the newest log, txt or out file found.
Histogram.py
This module uses the data inside on the filename to produce an histogram image.
Usage: Histogram.py [options] LOG_FILE TRACE
Options:
--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.
-i IMAGEFILE, --image=IMAGEFILE
Name of the image File. extension 'png'
LTSpice_SemiDevOpReader.py
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?
- Tools website : https://www.nunobrum.com/pyspicer.html
- Repo owner : me@nunobrum.com
- Alternative contact : nuno.brum@gmail.com
History
-
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 setup.py as per PEP517 and PEP518
Bug Fixes (See GitHub log for more information)
Improvements on the management of stepped data in the LTSpice_RawRead.py -
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 LTSpice_RawWriter.py
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 Histogram.py
Adding back the README.md 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) logan.herrera.github@gmail.com 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
README.md: Adding link to readthedocs documentation
All files: Comprehensive documentation on how to use each module -
Version 1.1
README.md: Updated the description
LTSpiceBatch.py: Corrected the name of the returned raw file.
Added comments throughout the code and cleanup -
Version 1.0
LTSpiceBatch.py: Implemented an new approach (NOT BACKWARDS COMPATIBLE), that avoids the usage of the sim_settings.inc file. And allows to modify not only parameters, but also models and even the simulation commands.
LTSpice_RawRead.py: 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.
LTSteps.py: Modified the LTSteps so it can also read measurements on log files without any steps done. -
Version 0.6
Histogram.py now has an option to make the histogram directly from values stored in the clipboard -
Version 0.5
The LTSpice_RawReader.py now uses the struc.unpack function for a faster execution -
Version 0.4
Added LTSpiceBatch.py 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 LTSteps.py and Histogram.py -
Version 0.1
First commit to the bitbucket repository.
Project details
Release history Release notifications | RSS feed
Download files
Download the file for your platform. If you're not sure which to choose, learn more about installing packages.