LTspice FAQ and Tips
Frequently asked questions, simulation speed, efficiency calculations, SMPS Bode plots, platform notes, and resources.
Table of Contents
- Program Updates
- License and Distribution
- Running Under Linux
- Settings Overview
- Speeding Up Simulations
- 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 |
Speeding Up Simulations
Pointers to the measures documented elsewhere in this reference, grouped by what each one costs you. Nothing here is a new setting — follow the links for syntax and caveats.
Reduce the work the simulator does
These change how much gets simulated, not how accurately.
- Skip the startup transient with
loadstate. Save the settled state once, then start every later run from it. For iterative work — tuning a compensation network, sweeping a component value, repeating an FRA sweep — this is usually the largest single saving available: the startup transient is often most of the run, and it is otherwise re-simulated from scratch every time. Component and parameter values may differ from those the state was saved with, and the run will usually still converge — see Changing the Circuit Between Save and Load. See also State Management, and Step 1 for priming an.frasweep this way. - Stop the run when the circuit settles, using the
steadymodifier rather than guessing aTstopand overshooting it. See Steady-State Detection. - Prefer LTspice’s native devices and SMPS macromodels over generic SPICE/PSpice equivalents — the native models exist largely for simulation speed. See Speed Considerations.
Trade accuracy for speed — validate the setup first
These change the simulation results. Establish a result you trust, then apply them and confirm the answer did not move.
The cost need not apply to the whole run. .options take effect for an entire run, but a run can
be split into segments with savestate/loadstate, each with its own tolerances: loose through
the non-critical or troublesome portions — a startup transient, a settling interval, a
hard-to-converge transition — and tight through the portions you measure. See
State Save/Load for Partial Relaxation.
- Raised
trtollets the simulator take larger time steps by tolerating more truncation error per step. Fast edges, ripple, and ringing are the first details to lose resolution, so compare them against a run at the default value. See .OPTIONS. - Relaxed
reltolloosens the error criterion every node and branch must meet at each time point, so the run both goes faster and gets through hard-to-converge stretches more easily. The accuracy loss is just as broad, which makes it a candidate for confining to the segments described above rather than setting for the whole run. See Improve Transient Convergence for typical values.
Not run-time savings
.save and Tstart shrink the stored data, but the circuit is still simulated in full. Turning
off marching waveforms makes a negligible difference to both run time and memory. See
Memory and Performance.
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.
Save the settled state while you are here. Steps 3-8 re-run the circuit many times, and every run otherwise repeats the whole startup transient:
.tran 2m savestate ; verify startup, save the state at the end of the simulation
Then start the FRA runs from it:
.fra loadstate
The FRA device’s delay is absolute simulation time measured from t=0, not time elapsed since the
run began, so a state saved at or after delay has already satisfied it: the state above is saved
at t=2m, so an FRA device with delay=1m starts injecting immediately when that state loads. Leave
delay at the value the un-primed circuit genuinely needs to settle — it costs no run time once the
state is loaded past it. (Use savestatetime=<time> if you need the state captured at a particular
time rather than at the end of the run.) State files are interchangeable between .tran and .fra; see
State Management.
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 to10/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.
See also: TROUBLESHOOTING-GUIDE.md for convergence solutions, SIMULATION-COMMANDS-REFERENCE.md for .FRA command details
Documentation source: github.com/analogdevicesinc/ltspice-reference