1. Skip to navigation
  2. Skip to content
  3. Skip to sidebar

LTspice: Using an Intrinsic Symbol for a Third-Party Model

Gabino Alonso - Strategic Marketing Engineer Sep 9th 2014

LTspice IV can automatically create a symbol for a third-party model, or you can associate a third-party subcircuit with an LTspice intrinsic symbol, as long as the third-party .SUBCKT model and the intrinsic symbol share an identical pin/port netlist order. For example, to add an N-channel MOSFET transistor symbol to a schematic and define it with an IRF_7401 .SUBCKT statement:

  1. Add an instance of the N-channel MOSFET transistor symbol to your schematic.

    Instance of the N-channel MOSFET transistor symbol

  2. Move the cursor over the body of the MOSFET symbol and Ctrl + Right-Click. A dialog box appears.

    NMOS Component Attribute

  3. Change Prefix: “MN” to “X”. The symbol now netlists as a subcircuit instead of an intrinsic NMOS transistor.
  4. Change “NMOS” to be “IRF_7401”, corresponding to the name on the .SUBCKT line.


  5. Click OK.
  6. Either add the .SUBCKT IRF_7401 lines to your schematic or reference the library containing it (.INCLUDE third_party.lib) as a SPICE directive.

    SUBCKT IRF_7401

Again, this assumes the third-party model you’re adding follows popular pin order conventions. When in doubt, use the automatic symbol generation feature because it takes care of any discrepancies with regard to pin and port netlist order. For more about automatic symbol generation, see Help > Schematic Capture > Creating New Symbols > Automatic Symbol Generation.





LTspice® software is a powerful, fast and free simulation tool, schematic capture and waveform viewer with enhancements and models for improving the simulation of switching regulators. Click here to download LTspice

To launch a ready to run LTspice demonstration circuit for this part:

  • Step 1: If you have not installed LTspice on this computer, download and install LTspice
  • Step 2: Once LTspice is installed, click on the link(s) below to launch the simulation
  • Step 3: If LTspice does not automatically open after clicking the link above, you can instead run the simulation by right clicking on the link and selecting "Save Target As." After saving the file to your computer, start LTspice and open the demonstration circuit by selecting 'Open' from the 'File' menu

To explore other ready to run LTspice demonstration circuits, please visit our Demo Circuits Collection.