# LTspice: Modeling Constant Power Loads

Jun 4th 2017

There are several types of constant loads used in simulating a power supply system: constant resistance, constant current and constant power loads. For instance, a constant current load dynamically adjusts its resistance as the load voltage varies, such that the load current remains constant, I = V/R. Constant resistance and constant current loads are available as dedicated symbols in LTspice, while a constant power load is available via the arbitrary behavioral source.

A constant power load is designed to dynamically adjust the load current inversely with the load voltage so that the load power is constant, *P = VI*. It is this inverse property of a constant power load that is often useful in stability analysis of simulations like those of a switching mode power supply.

Normally, arbitrary behavioral voltage and current sources are defined by the syntax of *V = <expression>* or *I = <expression>*. However, you can modify either of these behavioral source symbol attributes to define a constant power load, *P = <expression>*. It does not matter which arbitrary (current or voltage) sources symbol you use for the expression, since the syntax (V, I or P) describes the behavior, not the symbol.

In the schematic shown, a DC source sweep analysis is performed to plot the characteristic curves.

Shown here are the current and instantaneous power in the constant power load, *B1*, vs voltage. (To plot instantaneous power, Alt-Left Click a symbol.)

Notice that the waveform shows the constant power load smoothly transitioning from a constant power load to zero watts at zero volts. This prevents the constant power load from drawing infinite load current as it nears zero output voltage. This foldback point is by default set to 1V, but can be modified by using the *vprxover* parameter.

The schematic above uses the *.step* command to perform repeat simulations of the *vprxover* parameter with waveform results shown here for comparison.

## Software

### LTspice

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.

### View More LTspice Solutions

**View All** - List View