# Using LTspice to Characterize Capacitor Banks

Jul 12th 2016

Capacitor banks are used to filter noise and provide energy storage for fast load transient response. For modeling the stability of a DC/DC converter the ESR of the capacitor bank is needed. This can be easily done if only one type of capacitor is used with multiple capacitors in parallel. This is difficult if many different types of capacitors are used in a parallel configuration. Using LTspice, the capacitor bank can be characterized and key parameters can be extracted. This is very helpful when using the LTpowerCAD tool for stability analysis.

### Example

In the schematic below, five different capacitors are in parallel. For stability analysis, it is desired to model this as one capacitor.

Running the simulation, the impedance is plotted below. This is simply the source voltage divided by the source current; V(n001)/I(V1).

Using the curser measurement tool, the self-resonant frequency of the network is 243KHz, and the amplitude of the impedance is -49.65dB. It is important to note at self-resonance the imaginary impedance of the capacitive reactance and the inductive reactance cancel resulting in the ESR of the LC network as the only impedance. Solving for the impedance in Ohms, the resultant ESR is 3.29mΩ.

Quick note on algebra:

`20log(x) = -49.65`

`log(x) = -2.4825`

`x = 0.00329`

A couple of other insights can be gained from this impedance approach. The plot below shows the current in two of the capacitors, I(C3) and I(C4), as a function of frequency. This is intuitively obvious, but helpful to quantify. The 4.7uF ceramic capacitor has a low impedance up to 2.3MHz, whereas the 330uF capacitor is inductive at 2.3MHz and provides a higher impedance for energy transfer compared to the 4.7uF capacitor.

### Conclusion

By using LTspice to characterize the self-resonance of a bank of parallel capacitors the equivalent ESR can be easily determined. LTspice is a powerful tool that provides an easy format for defining the problem, and an intuitively obvious graphical solution that allows a simple analysis for a complex problem.

## 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.

### LTpowerCAD

The LTpowerCAD design tool is a complete power supply design tool program that can significantly ease the tasks of power supply design. It guides users to a solution, selects power stage components, provides detailed power efficiency, shows quick loop bode plot stability and load transient analysis, and can export a final design to LTspice for simulation. Click here to download LTpowerCAD

### View More LTspice Solutions

**View All** - List View