LTspice Waveform Viewer Guide

Complete reference for viewing, analyzing, and exporting simulation results.

Trace Selection
Zooming and Navigation
Waveform Arithmetic
User-Defined Functions
Axis Control
Plot Panes
Cursors
Executing .MEAS Scripts
Color Control
Plot Configurations
Fast Access File Format
Exporting Data

Trace Selection

Probing from Schematic

Action	Result
Click wire	Plot node voltage
Click component body (2-terminal)	Plot current through component
Click component pin	Plot current into that pin
Double-click same trace	Isolate it (erase other traces)
Alt+Click component body	Plot instantaneous power (Watts)
Alt+Click wire	Plot wire current
Click node, drag to another	Differential voltage V(a,b)

Mouse cursor icons indicate measurement type (voltage probe, current clamp, thermometer for power).

Plot Settings > Visible Traces — Select initial traces; pattern matching filter available
View > Add Trace — Add traces without removing existing ones; click trace names to build expressions

Managing Traces

Click trace label with Delete command active to remove individual traces
Undo/Redo work across all trace selection methods

Action	Result
Drag box	Zoom to enclosed region
Esc before release	Cancel zoom
Toolbar zoom out	Step back to previous zoom
Auto-range	Reset to automatic scaling
Undo/Redo	Navigate zoom history
Ctrl+Mouse wheel	Preview zoom (bitmap, fast for large files)

Zoom box dimensions shown on status bar (quick measurement without cursors)
Time differences automatically converted to frequency display

Waveform Arithmetic

Right-click on a trace label or use View > Add Trace to enter expressions.

Available Functions

Category	Functions
Trig	sin, cos, tan, asin, acos, atan, atan2, sinh, cosh, tanh, asinh, acosh, atanh
Log/Exp	ln, log, log10, exp
Power	sqrt, pow, pwr (abs(x)^y), pwrs (sgn(x)*abs(x)^y)
Abs/Round	abs, ceil, floor, round, int
Logic	buf, inv, u (unit step), uramp
Conditional	if(x,y,z), limit, max, min
Calculus	d() (derivative via finite difference)
Lookup	table(x, a,b, c,d, …)
Distance	hypot(x,y)
Noise	rand, random, white
Complex	Re, Im, Ph, Mag, conj

Operators (ascending precedence)

Operator	Description
`&`, `\\|`, `^`	Boolean AND, OR, XOR
`>`, `<`, `>=`, `<=`	Comparison
`+`, `-`, ``, `/`, `*`	Arithmetic
`!`	Boolean NOT
`@`	Step run selector (e.g., `V(out)@3`)

Built-in Constants

Name	Value
E	2.71828…
pi	3.14159…
K	1.3806503e-23 (Boltzmann)
Q	1.602176462e-19 (electron charge)

Keywords

time — horizontal axis for transient analysis
omega or w — angular frequency for AC analysis

Dimensional Analysis

The viewer performs dimensional analysis on expressions and labels results with calculated units (V, A, W, Ohm, etc.). Traces with the same units share a vertical axis.

Example: -2*pi*pow(V(out),2)/abs(V(n001))/Ie(x1:Q1) → identified as Ohm

Average and RMS

Zoom to a region of interest, then Ctrl+Left-click on the trace label to compute average and RMS over the visible window. RMS only reported for V or A units.

FFT (Fourier Transform)

View > FFT to compute frequency spectrum.

Proprietary algorithm: works with arbitrary number of datapoints (not limited to power of 2)
Noise floor exceeds 300dB
Enter desired number of bins directly

For best FFT results:

.options plotwinsize=0   ; disable compression
.tran 0 10m 0 1u        ; specify max timestep
.options numdgt=15       ; double precision

User-Defined Functions

Custom functions and parameters for the waveform viewer.

Menu: Plot Settings > Edit Plot Defs File

File location: %LOCALAPPDATA%\LTspice\plot.defs

Syntax (same as SPICE .param and .func):

.func Pythag(x,y) {sqrt(x*x+y*y)}
.func dBV(x) {20*log10(abs(x))}
.param twopi = 2*pi

Axis Control

Move cursor beyond the data area until it changes to a ruler icon
Left-click on the ruler to open axis configuration dialog

Horizontal Axis (Real Data)

Manually set range and scale type
Enables parametric plots (plot one trace vs another)

Vertical Axis (Complex/AC Data)

Left-click left vertical axis to switch between:
- Bode plot
- Nyquist plot
- Cartesian plot
Right vertical axis options: phase, group delay, or none

Plot Panes

Multiple plot panes can be displayed in one window for better trace organization.

Action	Result
Right-click plot area	Add pane above/below, move panes
Drag trace label to another pane	Move trace
Ctrl+release in another pane	Copy trace to that pane

Each pane has independent autoscaling.

Cursors

Attaching Cursors

Action	Result
Left-click trace label	Attach single cursor
Right-click label > “1st & 2nd”	Attach both cursors to one trace
Right-click label > Attached Cursor	Choose 1st, 2nd, or both

Moving Cursors

Drag with mouse
Arrow keys for fine positioning
Up/Down keys navigate between .step/.dc/.temp runs

Readout

Cursor position shown in readout window
Difference between cursors reported
Right-click cursor to see step information for that run

Status Bar Readout (No Cursor Needed)

Mouse position always displayed on status bar
Drag-zoom box size shown (quick measurement)
Time differences converted to frequency

Executing .MEAS Scripts

.MEAS statements are evaluated in post processing on the saved waveform dataset, so they can be run against data already on disk — no re-simulation required.

Menu: With the waveform window active, File > Execute .MEAS Script

This runs a script of .MEAS statements against the displayed dataset and writes the results to the log (View > SPICE Output Log, Ctrl+L). Use it to add or revise measurements after a long run, or to iterate on measurement expressions against a fixed dataset.

Script file: can be a plain netlist — LTspice reads only the .MEAS statements and ignores every other line, so the circuit’s own .net or .cir file works as-is.

Accuracy: results are limited by the accuracy of the waveform data after compression. Disable compression for precise measurements:

.options plotwinsize=0   ; disable compression

See MEAS-REFERENCE.md for .MEAS syntax and examples.

Color Control

Menu: Tools > Color Preferences

Click objects in sample plot to select them
Adjust colors with RGB sliders

Plot Configurations

File Format

Extension: .plt (text files)
Default name: same as .raw file with .plt extension
Automatically loaded when data file opens (if file exists)

Per-Analysis Settings

Each analysis type (.tran, .ac, .noise, etc.) has its own section. Cannot load settings from one analysis type to another, but can load .plt from a different simulation of the same analysis type.

Plot Settings > Save Plot Settings
Plot Settings > Open Plot Settings

Fast Access File Format

Optimizes random-access performance for large waveform files.

When to Use

After simulation completes
For files with many traces where you only view a few at a time
Example: 5GB file with 2000 traces — load time drops from 4 minutes to ~1 second

How to Convert

GUI: Make waveform window active > Files > Convert to Fast Access
Command line: ltspice.exe -FastAccess <file>

Characteristics

File size increase: only 11 bytes larger
Speed improvement: factor roughly equal to number of saved traces
Requires disk space equal to file size during conversion
Can use up to 1/4 of physical RAM
Conversion time may exceed original simulation time

Limitations

Real data only (not complex data from .AC analysis)
Cannot append new data after conversion
Standard format required during simulation

Exporting Data

Image Export

Method	Format	How
Clipboard bitmap	BMP	Right-click > Copy Image to Clipboard
Metafile (vector)	EMF	Tools > Write image to .emf file

For metafile: use Arial font (Tools > Settings > Waveform > Font) — system fonts don’t scale.

Numerical Data Export

Built-in: Waveform menu > File > Export (ASCII file)

Getting Equally-Spaced Timesteps

LTspice uses variable timesteps. To get uniform spacing:

Perform FFT on desired trace
Perform FFT on the FFT result (recovers equally-spaced time data)
Export that result

This is bit-accurate to double precision.

Third-Party Tools

Helmut Sennewald’s free utility (http://groups.io/g/LTspice) supports data manipulation including merging waveforms from different simulation runs.