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

LTspice: Simple Idealized Diode

Gabino Alonso - Strategic Marketing Engineer May 2nd 2017

LTspice semiconductor diode models are essential for simulations, especially when you want to see results that include breakdown behavior and recombination current. However, as complete as the semiconductor diode model is in LTspice, there are times when you need a simple “idealized diode” model to quickly simulate, for example, an active load, a current source or a current limiting diode. To assist, LTspice provides a representation of an idealized diode model.

To use of this idealized model in LTspice, insert a .model statement for a diode (D) with a unique name and define one or more of the following parameters: Ron, Roff, Vfwd, Vrev or Rrev.

.model MyIdealDiode D(Ron=1 Roff=1Meg Vfwd=1 Vrev=2)

The idealized diode model in LTspice has three linear regions of conduction: on, off and reverse breakdown. The forward conduction and reverse breakdown can further be specified with current limit parameters Ilimit and revIlimit.

.model MyIdealDiode D(Ron=1 Roff=1Meg Vfwd=1 Vrev=2 Ilimit=1 RevIlimit=1)

Furthermore, to smooth the switch between the off and conducting states the parameters epsilon and revepsilon can also be defined.

.model MyIdealDiode D(Ron=1 Roff=1Meg Vfwd=1 Vrev=2 Ilimit=1 RevIlimit=1 Epsilon=1 RevEpsilon=1)


Ideal Diode Schematic


A quadratic function is also used between the off and on state such that the idealized diode IV curve is continuous in value and slope, so that the transition occurs over a voltage specified by the value of epsilon and revepsilon.

Once you have inserted your .model statement in your schematic you can edit the diode symbol’s Value in the component attributes (Ctrl + Right Click) to match the name you specified in your statement. For more information on LTspice diode models, please refer to the help topics (F1).


Ideal Diode Waveform


Just for fun, in the circuit example below an idealized diode model is used to simulate a MOSFET’s RDS(ON) in an otherwise nonsynchronous step-down controller. By using an idealized diode model instead of the traditional Schottky diode, the conduction losses of synchronous rectification can be easily compared.


Ideal Diode Example




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.