SPICE Netlist Syntax Reference

Complete reference for LTspice netlist structure, conventions, and syntax rules.

Netlist Structure

A netlist is a plain-text file describing the circuit to be analyzed.

First line: Always treated as a comment (title line)
Last line: Usually .END (can be omitted; anything after .END is ignored)
Line order: Between the title and .END, line order is irrelevant
File extensions: .cir (standard), .net, .sp

Example Netlist

* RC Circuit driven with a 1MHz square wave
R1 n1 n2 1K        ; 1K resistor between nodes n1 and n2
C1 n2 0 100p       ; 100pF capacitor between n2 and ground
V1 n1 0 PULSE(0 1 0 0 0 .5u 1u)  ; 1MHz square wave
.tran 3u           ; 3us transient analysis
.end

Text Encoding

LTspice accepts three encodings:

Encoding	Notes
UTF-8	Recommended. Used exclusively by the built-in netlister
UTF-16 LE	Little-endian, with or without BOM
Latin-1 (ISO 8859-1)	Assumed only if file contains byte sequences invalid for UTF-8

LTspice conforms to Unicode standard version 14. Text comparison uses canonical equivalence and Unicode case folding for case insensitivity. The parser is based on grapheme clusters.

Comments and Line Continuation

Syntax	Meaning
`*` at line start	Entire line is a comment
`;` anywhere in line	Rest of line is a comment
`+` at line start	Continuation of previous line (the `+` is removed and remainder appended)

Special Netlister Comments

The LTspice netlister may append machine-readable comments that begin with ;§. These are ordinary comments (ignored by the simulator) but carry structural metadata:

;§pnba on a subcircuit (X) instance line lists the symbol’s pin names, delimited by ), in the same order as the net assignments. See CIRCUIT-ELEMENTS-REFERENCE.md for details and an example.

Line Types by Leading Character

The first non-blank character of a line defines what it represents:

Character	Element Type
`*`	Comment
`A`	Special function device
`B`	Arbitrary behavioral source
`C`	Capacitor
`D`	Diode
`E`	Voltage-dependent voltage source
`F`	Current-dependent current source
`G`	Voltage-dependent current source
`H`	Current-dependent voltage source
`I`	Independent current source
`J`	JFET transistor
`K`	Mutual inductance
`L`	Inductor
`M`	MOSFET transistor
`O`	Lossy transmission line
`Q`	Bipolar transistor
`R`	Resistor
`S`	Voltage-controlled switch
`T`	Lossless transmission line
`U`	Uniform RC-line
`V`	Independent voltage source
`W`	Current-controlled switch
`X`	Subcircuit invocation
`Z`	MESFET or IGBT transistor
`@`	Frequency Response Analyzer
`&`	Frequency Response Analysis Probe
`.`	Simulation directive (e.g., `.options reltol=1e-4`)
`+`	Line continuation

Engineering Multipliers

Numbers can use scientific notation (e.g., 1e12) or engineering multipliers (e.g., 1K for 1000):

Suffix	Multiplier	Example
`T`	1e12	`1T` = 1,000,000,000,000
`G`	1e9	`2.2G` = 2,200,000,000
`Meg`	1e6	`1Meg` = 1,000,000
`K`	1e3	`4.7K` = 4,700
`mil`	25.4e-6	`1mil` = 25.4e-6
`m`	1e-3	`10m` = 0.01
`u`	1e-6	`100u` = 0.0001
`n`	1e-9	`47n` = 47e-9
`p`	1e-12	`100p` = 100e-12
`f`	1e-15	`1f` = 1e-15

Important Rules

Suffixes are case-insensitive (except Meg vs m — see warning below)
Unrecognized letters after a number are ignored: 10V, 10Volts, 10Hz all equal 10
Common pitfall: 1M means 1 milliohm (1e-3), NOT 1 megaohm. Use 1Meg for megaohms.
Embedded decimal: 6K34 means 6.34K (works for all multipliers)
No unit suffixes needed: Just the number and multiplier (e.g., 100p not 100pF)
Use .options reject_number_tails to make LTspice report unrecognized trailing letters as syntax errors

Pitfall Example

C23 N1 N2 4Farads

This creates a 4 femtofarad capacitor (the F is parsed as the femto multiplier, arads is ignored). Always use just the number and multiplier: C23 N1 N2 4.

Node Naming

Node names are arbitrary character strings
Case-insensitive (via Unicode case folding)
Node 0 is the global circuit common (ground)
GND is a special synonym for 0
0 and 00 are distinct nodes (string comparison, not numeric)
Can use alphanumeric characters and underscores
Avoid spaces in node names

Creating and Running Netlists

Creating a Netlist

Use any text editor that produces ASCII or UTF-8 encoded files
In LTspice: View > SPICE Netlist shows the netlist for the current schematic
Copy to clipboard: Select all text, then Ctrl+C

Running a Netlist

Open the .cir file in LTspice and run it
Command line: ltspice.exe "C:\path\to\circuit.cir"

Externally Generated Netlists

LTspice can open netlists from other schematic capture programs or hand-written netlists.

Accepted extensions: .cir, .net, .sp
The built-in text editor colorizes SPICE syntax
Adjust editor colors: Tools > Color Preferences
Unicode is fully supported

Netlist Options

These options control how LTspice generates netlists from schematics:

Option	Description
Convert ‘µ’ to ‘u’	Replace all ‘µ’ instances with ‘u’ for compatibility with simulators that don’t support the µ character as 1e-6
Reverse comp. order	Netlist elements in reverse order from how they were added to schematic
Default Devices	Include default model statements (e.g., `.model D D`) to suppress missing-model messages
Default Libraries	Auto-include standard and user component libraries for all component types used

Library Paths

Standard library: %LOCALAPPDATA%\LTspice\lib\cmp\standard.dio (and similar for BJT, MOSFET, JFET)
User library: Documents/LTspice/user.dio (configurable in Search Paths tab)

Notation Conventions Used in This Documentation

Symbol	Meaning
`<name>`	Required data field to be filled with specific information
`[optional]`	Enclosed field is optional
`a \\| b`	Alternatives — either `a` or `b`