LTspice Device Models Guide

Using, creating, and integrating device models — MOSFETs, inductors, op-amps, transformers, and third-party models.

MOSFET Models
Inductor Models
Universal Op-Amp Models
Simulating Transformers
Third-Party Models
Model Compatibility

MOSFET Models

Intrinsic VDMOS

LTspice includes a proprietary MOSFET model that directly encapsulates the charge behavior of vertical double-diffused MOS transistors. Power devices are modeled as intrinsic VDMOS devices (no subcircuit wrapper needed), giving faster simulation than generic SPICE approaches.

Standard SPICE MOSFETs

All standard SPICE MOSFET levels (1–73) are also available. See CIRCUIT-ELEMENTS-REFERENCE.md for the full level table.

Adding Custom MOSFET Models

Create the file:

Documents\LTspice\user.mos

Use the same format as the standard library at %LOCALAPPDATA%\LTspice\lib\cmp\standard.mos.

Do not edit standard.mos — it is overwritten on updates.

Using Subcircuit-Based MOSFET Models

For third-party MOSFET models provided as .subckt:

Change the component Prefix attribute from M to X (Ctrl+right-click on symbol)
Set the Value attribute to match the subcircuit name
Include the model file via .include or .lib directive

Inductor Models

Default Parasitic Resistance

LTspice adds a default series resistance to inductors for SMPS transient analysis:

Default Rser: 1 milliohm (for inductors NOT in a mutual inductance statement)
This allows integration as Norton equivalent (smaller matrix, faster simulation)

To disable: Set Rser=0 explicitly on the inductor instance (forces Thevenin equivalent integration).

To disable globally: Tools > Settings > Hacks! → uncheck “Supply a min. inductor damping if no Rpar is given”

Adding Custom Inductor Models

Create: Documents\LTspice\user.ind

Access custom inductors: right-click inductor on schematic > “Select Inductor”

Do not edit %LOCALAPPDATA%\LTspice\lib\cmp\standard.ind.

Coupled Inductors

Draw independent inductors, then add a mutual inductance statement:

K1 L1 L2 1

See CIRCUIT-ELEMENTS-REFERENCE.md for K element syntax and hysteretic core model parameters.

Universal Op-Amp Models

LTspice provides four levels of universal op-amp models with increasing fidelity:

UniversalOpAmp1 — Simple Gain Block

Single pole in gain/phase response
Nearly ideal gain stage with realistic rise/fall times
Input voltage noise and current noise

UniversalOpAmp2 — With Limits

Level 1 features plus:

Slew rate limiting
Output voltage limiting
Output current limiting

Useful as a realistic gain block or for voltage/current limiting applications.

UniversalOpAmp3a / 3b — Two-Pole Response

Level 2 features plus:

Second pole in gain/phase response (both 3a and 3b)
Propagation delay (3b only)

Useful for basic small-signal stability or gain/phase analysis.

UniversalOpAmp4 — Full Intermediate Model

Level 3 features plus:

Input capacitance
Output resistance
Virtual ground support

Useful for:

Intermediate stability analysis across loads and feedback networks
Floating power supply applications (e.g., 4-20mA transmitters)

Parameters

All levels include input voltage noise and input current noise parameters. Complete parameter documentation is in the example circuit:

File > Open Examples > Educational > UniversalOpAmp.asc

Simulating Transformers

Basic Transformer

Draft two or more inductors, then add a mutual inductance SPICE directive:

K1 L1 L2 1

Inductors in a K statement display phasing dots
Coupling coefficient K=1 means zero leakage inductance
Turns ratio = sqrt(L1/L2). Example: 1:3 turns ratio → 1:9 inductance ratio

Practical Transformer Modeling

Parameter	How to Measure	How to Use
Winding inductance	DC LCR meter	Use directly as L value
Winding ESR	Ohmmeter	Use 2x DC value (frequency effects)
Leakage inductance	Short all but one winding, measure with LCR meter	Adjust K coefficient
Resonant frequency & Q	Measure	Set Cpar and Rpar on most inductive winding

Calculating Coupling Coefficient from Leakage

K = sqrt(1 - Lleak / sqrt(L1 * L2))

Or equivalently:

Lleak = sqrt(L1 * L2) * (1 - K^2)

Example

* 1:3 transformer (1:9 inductance ratio) with K=0.99
L1 pri1 pri2 10u
L2 sec1 sec2 90u
K1 L1 L2 0.99

Non-Linear Transformer

See example: File > Open Examples > Educational > NonLinearTransformer.asc

Uses the hysteretic core model parameters (Hc, Br, Bs, Lm, Lg, A, N) on the inductor element.

Third-Party Models

Type 1: .MODEL Statements (Intrinsic Devices)

For diodes, transistors, and other primitive SPICE elements where the model is a .model statement.

Usage:

Edit component Value to match the model name
Include the model definition via one of:
- SPICE directive pasted on schematic
- .include <filename> directive
- Add to user library (e.g., Documents\LTspice\user.bjt)

Example — NPN Transistor:

* On schematic: set Q1 Value = "BC547C"
* Then add directive:
.model BC547C NPN(Is=1.8e-14 Bf=400 Vaf=80)

Or:

.include "C:\models\BC547C.mod"

Type 2: .SUBCKT Statements (Complex Models)

For op-amps, regulators, and other models composed of multiple internal devices.

Usage:

Edit component Value to match the subcircuit name
Change component Prefix to X (Ctrl+right-click)
Include the subcircuit definition:
- Paste full .subckt ... .ends as multi-line SPICE directive
- .include <filename> directive

Example — Op-Amp:

* Set component Value = "TL072", Prefix = "X"
.include "TL072.sub"

Creating Symbols for Third-Party Models

Recommended approach for subcircuit models:

Open the netlist file containing the .subckt definition
Place cursor on the .subckt line
Right-click > Create Symbol
LTspice generates the .asy file automatically with correct pin order

For auto-include library symbols: Set symbol attributes:

Prefix: X
SpiceModel: <library_filename>
Value2: <subcircuit_name>

Pin Order

Critical: Symbol pin netlist order must match the .subckt port order. Automatic symbol generation handles this correctly. If creating symbols manually, verify pin order matches.

User Library Files

Device Type	User Library File
Diodes	`Documents\LTspice\user.dio`
BJTs	`Documents\LTspice\user.bjt`
MOSFETs	`Documents\LTspice\user.mos`
JFETs	`Documents\LTspice\user.jft`
Inductors	`Documents\LTspice\user.ind`
Resistors	`Documents\LTspice\user.res`

Never edit files in %LOCALAPPDATA%\LTspice\lib\cmp\ — they are overwritten on update.

Model Compatibility

LTspice SMPS Models

LTspice switching regulator macromodels use proprietary native devices for optimal simulation speed. These models are not compatible with PSpice or other simulators.

PSpice Models in LTspice

LTspice can run PSpice semiconductor and behavioral models. Standard SPICE model statements (.model) and most subcircuit models work without modification.

Speed Considerations

LTspice native SMPS models: fastest simulation speed
Generic SPICE/PSpice macromodels: functional but slower
LTspice can often run third-party switching regulator models faster than their original simulator