LTspice automation

Question

I have a battery-powered boost converter and I'm attempting to measure the maximum input (battery) voltage droop under various load conditions of high current draws (different duty-cycles/periodicities) in addition to over several battery types (various voltages/internal resistances).

Since I'm simulating such a (relatively) large amount of operational time the simulation files are getting pretty substantial, not to mention they take a while. I would like to automate LTspice so that I can change component values programatically and rerun simulations and capture data (values of things like voltage or current). I know that:

• WAV files can be used to input/output data from the program
• The program can be run from the command line

So far my best option seems to use a combination of these two options along with my own code/script in a fashion that accomplishes my goals, but I just wonder if there is a better way already out there.

Has anyone automated LTspice or know if there has been any kind of automation API written for it (either by the manufacturer or by 3rd parties)?

Ideally I would like to have a solver, such that I give it the desired parameters and it tries various component values until it has found the "optimal" solution to my constraints.

Answer 1

Running a simulation multiple times and changing multiple component values is a bit more involved than just changing one (which is not so bad)

Here is the concept for changing one value:

• Add a .param statement using the SPICE directive icon on the far right, e.g. for a resistance value .param X=R
• To use it you would enter {x} into the resistor value, then include e.g. .step param X 100 500 50 to step the value between 100 and 500 in increments of 50.

Example:

Result:

For multiple values, the only way I found to work was using a list of values for X, and using the table statement. This is probably best explained with an example (reading the help for the commands used will probably be helpful here). But note that the table command syntax is in the form table(index, x1, y1, x2, y2, .... xn, yn), takes index as input and returns an interpolated value for x=index based on the supplied x,y pairs.

In one of my simulations I needed to perform 12 simulations whilst changing 3 different component values, here are the commands:

.step param X list 1 2 3 4 5 6 7 8 9 10 11 12
.param Rin1 = table(X, 1, 1,1p, 2, 1p, 3, 1p, 4, 4478, 5, 4080, 6, 3400, 7, 2200, 8, 1p, 9, 1p, 10, 1p, 11, 1p, 12, 1p)
.param Rin2 = table(X, 1, 4997, 2, 4997, 3, 4997, 4, 499, 5, 897, 6, 1577, 7, 2777,  8, 4997, 9, 4997, 10, 4997, 11, 4997, 12, 4997)
.param Tval = table(X, 1, 56, 2, 56, 3, 27, 4, 1G, 5, 1G, 6, 1G, 7, 1G, 8, 1G, 9, 330, 10, 330, 11, 120, 12, 120)
.param Kval = table(X, 1, 316, 2, 147, 3, 147, 4, 6340, 5, 6340, 6, 6340, 7, 6340, 8, 6340, 9, 6340, 10, 825, 11, 825, 12, 316)

Result:

Hopefully you get the idea, you could maybe produce a script that would produce the necessary SPICE commands when you fill in your desired values. Or just create a template (e.g. I just copied and pasted the above into a few different simulations and changed the values)

If the above doesn't do what you want, then maybe look at something like NI's multisim (I think it has some batch simulation options, although I'm not sure how useful they are) It may also be helpful to ask on the LTSPice forum and see if someone knows of a better way of doing things.

Answer 2

I think it is actually possible to run LTSpice from the command line and have it run a transient simulation:

On Windows:

cd <wherever LTSpice is installed on your computer>
scad3.exe -Run -b MyCircuit.asc

On Linux:

cd ~/.wine/drive_c/Program Files (x86)/LTC/LTspiceIV
wine ./scad3.exe -Run -b MyCircuit.asc

Answer 3

LTSpice can be run in batch mode with the -b command line switch.

From the LTSpice Help file:

-b: Run in batch mode. E.g. "scad3.exe -b deck.cir" will leave the data in file deck.raw

How to read and interpret the .raw output is left as an excercise for the reader.

Also note, among the command line switches:

-ascii: Use ASCII .raw files. Seriously degrades program performance.

Answer 4

Have you tried "LTSpice Queue Manager"? (The link redirects to my own website where you can download the software but I'm not its author, who originally shared the program on a forum that is today closed. Sharing it through my website is a way to revive it).

This tool has been of much help to me in the past. You can prepare many simulation files and run them in a queue fashion.

Answer 5

PyLTSpice seems to be the hero of the day:

PyLTSpice is a toolchain of Python utilities designed to interact with LTSpice and NGSpice Electronic Simulator.

It's shipped as a bouquet of different modules. The one most relevant to your needs appears to be sim_batch.py.

sim_batch.py

Excerpt from its description:

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.

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 a previously added instruction
• reset_netlist() - Resets the netlist disarding all edits made to it.

A Full Example for a Similar Use-Case

...again, copied from the Pypi repository:

import os
from PyLTSpice 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))

The repo has seen 10 updates between 2022-2023 so be sure to check out its most current documentation and version: PyLTSpice

Answer 6

If it just has to be LT Spice and you can't get past the GUI I would recommend the script program AutoIt. I've used it to automate some critical Windows applications which were lacking active-x-DDE-COM.dll-whatever. You can set it up to wait for files, push windows buttons, menuitems, call programs with arguments, etc.

Have a look at:

http://www.autoitscript.com/site/

http://www.autoitscript.com/forum/

I would go for Winbatch if you want to pay for a script program.