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

LTspice: Simple Steps for Simulating Transformers

Gabino Alonso - Strategic Marketing Engineer Jul 1st 2014

Here is the simple approach to simulate a transformer in LTspice IV:

  1. Draft an inductor for each transformer winding
  2. Couple them using a single mutual inductance (K) statement via a SPICE directive:

    K1 L1 L2 L3 1

    The last entry in the K statement is the coupling coefficient, which can vary between 0 and 1, where 1 represents no leakage inductance. For practical circuits, it is recommended you start with a coupling coefficient of 1.

    Only a single K statement is needed per transformer; LTspice applies a single coupling coefficient to all inductors within a transformer. The following is an equivalent to the statement above:

    K1 L1 L2 1
    K2 L2 L3 1
    K3 L1 L3 1

  3. Adjust the inductor positions to match the transformer polarity by using move (F7), rotate (Ctrl + R) and mirror (Ctrl + E) commands. Adding the K statement displays the phasing dot of the included inductors.
  4. LTspice simulates the transformer using individual component values, in this case, the inductance of the individual inductors, not the turns ratio of the transformer. The inductance ratio corresponds to the turns ratio as follows:

    Inductance & Turns RatioInductance to Turns Ratios

    For example, for a 1:3 and 1:2 turns ratios, enter inductance values to produce a one to nine and one to four ratios:

    K Statements ExampleExample of a 1:3 and 1:2 Turns Ratios

For more information on how to simulate a transformer you can view the Using Transformers video




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.