LTspice FAQ and Tips

Frequently asked questions, efficiency calculations, SMPS Bode plots, platform notes, and resources.

Program Updates
License and Distribution
Running Under Linux
Settings Overview
Efficiency Calculation
SMPS Bode Plots (FRA)
Additional Resources

Program Updates

Updating LTspice

Three methods:

Download latest from https://www.analog.com/ltspice
Help > Check for LTspice updates
Windows Start Menu shortcut

Updating Components and Models

Tools > Update components downloads the latest component libraries and models.

Change Logs

Help > Show LTspice Change Log — program changes
Help > Show Model Change Log — model/component updates

Important Warnings

Older versions cannot be recovered after update
All library databases are overwritten automatically
Do not edit files in %LOCALAPPDATA%\LTspice — they may be overwritten on update
Store custom files in Documents\LTspice\ (user library directory)

License and Distribution

Classification: EAR99 (no export restrictions)
License: Non-exclusive, non-transferable for internal use and circuit simulation
Free: No cost, no license limits
Restrictions:
- No modification, reverse engineering, or decompilation
- Not licensed for semiconductor manufacturers for product design/promotion (requires special permission from ADI)
- Not suitable for high-risk applications (nuclear, aircraft, life support, weapons, autonomous driving)
Jurisdiction: Massachusetts, USA

Third-Party Components

LTspice includes code from:

Berkeley SPICE (University of California)
NXP MEXTRAM model
Hiroshima University HiSIM
ZLIB compression
SQLiteC++ database

Running Under Linux

Analog Devices does not provide an official Linux version. LTspice runs under WINE.

Installation

# Install WINE
# (from http://www.winehq.com)

# Download LTspice
wget https://LTspice.analog.com/download/latest/LTspice64.msi

# Install
wine msiexec /i LTspice64.msi

Running

Launch from desktop icon or:

wine ltspice.exe

Known Issues

Font scaling less smooth than on Windows
PWL editor display issues — fix with native Windows DLLs:
```
wine -dll commctrl,comctl32=n ltspice.exe
```

Settings Overview

Access via gear icon or Tools > Settings. Configuration sections:

Tab	Purpose
Compression	Waveform data compression tolerances
Save Defaults	Default trace saving behavior
SPICE	General-purpose simulation settings
Schematic	Drafting options (grid, snap, pen, undo)
Netlist	Netlist generation options
Search Paths	Symbol and library paths
Waveforms	Waveform viewer appearance
Operation	Application behavior (marching waveforms, auto-delete, etc.)
Hacks	Internal development settings (deprecated)
Internet	Update behavior

Efficiency Calculation

Quick Method

Add steady keyword to .tran command:

.tran 10m steady

Requirements

Exactly one voltage source (identifies as input)
Exactly one current source or Rload resistor (identifies as output)

How It Works

Simulation runs until steady state is detected (via switching regulator macromodel)
Energy stored in reactances noted at clock edges
Efficiency = output power / input power, adjusted for reactance energy changes
Report displayed as comment block on schematic

Viewing Results

View > Efficiency Report after simulation completes.

Manual Adjustment

If automatic detection is too aggressive or not critical enough:

.options sstol=0.0001      ; tighter steady-state tolerance
.options ststdelay=100u    ; wait before starting detection

Checking Individual Losses

After efficiency report, check individual device power dissipation by Alt+clicking on component bodies in the schematic.

Detailed Efficiency Analysis

For more precise efficiency estimates including switching and parasitic losses, use LTpowerCAD: https://www.analog.com/en/design-center/ltpowercad.html

SMPS Bode Plots (FRA)

Frequency Response Analysis for measuring loop gain and phase margin of switched-mode power supplies.

Concept

Uses Middlebrook’s method (voltage injection) to measure the loop transfer function of a feedback system in the time domain. A sinusoidal stimulus is injected at the feedback loop break point, and Fourier analysis extracts gain and phase at each frequency.

Example Circuits

*File > Open Examples > Educational\FRA*

Procedure

Step 1: Verify Basic Operation

Run a standard .tran simulation to confirm the SMPS starts up and reaches steady state.

Step 2: Insert FRA Component

Break the feedback loop and insert the FRA device (prefix @) at the injection point. Valid placement must satisfy two criteria:

The device must completely interrupt the feedback. Every feedback path has to pass through it. If any path bypasses the device — a feedforward capacitor around the divider, a second sense connection, an auxiliary loop — part of the loop stays closed and what you measure is not the loop gain.
The device must point from lower impedance to higher impedance. Connect the OUT terminal to the low-impedance side of the break and the IN terminal to the high-impedance side — typically OUT toward the converter output and IN toward the feedback divider or error-amplifier input. If the source impedance at the break is not small compared with the load impedance, the injection loads the loop and the measured response is corrupted.

Step 3: Initial Exploratory FRA

Start with 2-3 frequencies to verify the setup works — use flist on the FRA device to apply just those frequencies individually:

.fra

Key FRA device parameters (see CIRCUIT-ELEMENTS-REFERENCE.md for the full list):

fstart: Starting frequency (typically 100Hz-1kHz for SMPS)
fend: Ending frequency (typically 100kHz-1MHz)
tsettle: Settling time at each frequency before analysis begins. Start at 2/fcross, where fcross is the expected 0dB crossover. Defaults to 10/fend.
tavgmin: Minimum analysis time per frequency. For an SMPS, start at 100/fsw, where fsw is the switching frequency.

Step 4: Check for Nonlinearity

Inspect FRA transient waveforms — stimulus should be small enough to not disturb the operating point significantly.

Step 5: Initial Bode Plot

Analyze the gain/phase plot. Identify the 0dB crossover frequency (f0dB).

Step 6: Adjust Stimulus Amplitude

Use the frequency-dependent amplitude parameters (pp0, pp1, f0, f1 — the recommended method) to inject a larger stimulus at low frequencies and a smaller one at high frequencies. Where loop gain is high, the loop suppresses the injected perturbation, so a larger stimulus is needed to get a measurable response; near and above crossover the loop no longer attenuates it, so the same amplitude would disturb the operating point and distort the result.

* 2mV up to 1kHz, tapering to 1mV above 2kHz
@1 A B fstart=1k fend=500k pp0=2m pp1=1m f0=1k f1=2k

Step 7: Add More Frequencies

Use 2-3 points per octave (oct=2 or oct=3) for a smooth Bode plot.

Step 8: Speed Up (Optional)

Reduce tsettle and tavgmin where the circuit responds quickly, and use fcoarse (set to 2-10× fstart) to coarsen the sweep at low frequencies, where each point is most expensive.

Only at this point — with the setup already validated by the steps above — consider raising nmax above its default of 1 to inject harmonics alongside the fundamental. It trades accuracy for speed, because the circuit’s own harmonic distortion then falls on the measured frequencies and cannot be separated from the real response. See nmax before using it.

Reference

R.D. Middlebrook, “Measurement of Loop Gain in Feedback Systems,” International Journal of Electronics, 1975.

Additional Resources

Official

Resource	URL
LTspice downloads & training	https://www.analog.com/ltspice
EngineerZone support forum	https://ez.analog.com/design-tools-and-calculators/ltspice/
LTpowerCAD efficiency tool	https://www.analog.com/en/design-center/ltpowercad.html

Community

Resource	URL
Independent users’ group	https://groups.io/g/LTspice
Simon Bramble tutorials	http://www.simonbramble.co.uk

The groups.io Files section contains tutorials, additional component libraries, and user-contributed example circuits.