PyLTSpice 1.1

An set of tools to Automate LTSpice simulations

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,s uch like Excel or Calc.

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

• 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, validattion 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

LTSpice_RawRead.py

Include the following line on your scripts

from matplotlib import plot


LTR = LTSpiceRawRead("Draft1.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_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.

from PyLTSpice.LTSpiceBatch import LTCommander
from shutil import copyfile

# get script absolute path
meAbsPath = os.path.dirname(os.path.realpath(__file__))
# select spice model
LTC = LTCommander(meAbsPath + "\\Batch_Test.asc")

LTC.set_parameters(res=0, cap=100e-6)  # Redefining parameters in the netlist
LTC.set_component_value('R2', '2k')  # Redefining component values
LTC.set_component_value('R1', '4k')

# define simulation
LTC.add_instructions(
   "; Simulation settings",
   ".param run = 0"  # Commands can be set directly with the .param command instad of the set_parameters(...)
)

for opamp in ('AD712', 'AD820'):
   # Setting a model of the U1 Component. Note that subcircuits need the X prefix
   LTC.set_element_model('XU1', opamp):
       for supply_voltage in (5, 10, 15):
           LTC.set_component_value('V1', supply_voltage)  # Set a voltage source value
           LTC.set_component_value('V2', -supply_voltage)
           rawfile, logfile = LTC.run()  # Runs the simulation with the updated netlist
           # The run() returns the RAW filename and LOG filenames so that can be processed with
           # the LTSpice_ReadRaw and LTSteps modules.

LTC.reset_netlist()  # This resets all the changes done to the checklist
LTC.add_instructions(  # Changing the simulation file
   "; 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"
)

raw, log = LTC.run()
LTC.wait_completion()

LTSteps.py

python -m PyLTSpice.LTSteps <logfile or directory where last simulation was made

Histogram.py

python -m PyLTSpice.Histogram

To whom do I talk to?

• Tools website : https://www.nunobrum.com/pyspicer.html
• Repo owner : [e-mail]
• Alternative contact : [e-mail]

History

• 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.