Spectrum Software
Industrial Strength Simulation




Spectrum Software has released Micro-Cap 11, the eleventh generation of our SPICE circuit simulator.

For users of previous Micro-Cap versions, check out the new features available in the latest version. For those of you who are new to Micro-Cap, take our features tour to see what Micro-Cap has to offer.




Creating Ferrite Bead Models


A ferrite bead is a passive device used to suppress high frequency signals. It is often used to reduce electromagnetic interference (EMI) or radio frequency interference (RFI) signals within a system. A common equivalent circuit of a ferrite bead is a lumped element parallel RLC circuit. This circuit produces a reasonable match for the impedance curve of the ferrite bead. However, a more precise model for the impedance curve can be created by adding a second parallel RLC to the equivalent circuit along with a series resistance. The modified equivalent circuit is shown below.

Lumped element representation of the ferrite bead

While the equivalent circuit is simple, determining the component values to use to appropriately model a specific ferrite bead can be onerous. Fortunately, the capability of the Model program to optimize any user created model is designed to handle such complexity. The first step is to create a basic template of the ferrite bead model. A subcircuit model that represents the equivalent circuit is defined as:

.subckt Bead 1 2
L1 1 3 1u
R1 1 3 10
C1 1 3 1p
R2 3 4 10
L2 3 4 1u
C2 3 4 1p
R3 4 2 1

Either a subcircuit or macro could have been used as the template. The advantage to using a SPICE subcircuit in this instance is that multiple ferrite bead models can then be stored within a single library file.

The next step is to create a schematic that simulates an important measurement of the model. For a ferrite bead, the main specification is the impedance versus frequency characteristic. This characteristic can be easily measured in Micro-Cap through the schematic below.

Ferrite bead impedance measurement circuit

The circuit consists of just a Current Source component and the ferrite bead subcircuit model. The Current Source component has its AC magnitude parameter set to 1A. Therefore in an AC analysis, the voltage across the ferrite bead will be equivalent to the impedance of the ferrite bead since:

V = Z*I
I = 1A
V = Z

Also present in the schematic is the following define statement:

.define Zb V(Out)

This define variable is used as an alias. It just maps the expression V(Out) to the variable Zb, so that the AC analysis can then plot Zb versus Frequency instead of V(Out) versus Frequency. While both would produce the exact same results, this might help prevent any confusion later when the expression being plotted is used within the Model program.

Next, the analysis limits need to be setup for the AC analysis simulation. For this example, all that needs to be done is to setup the impedance versus frequency expression to be plotted. On a waveform line, the X Expression is set to F, and the Y Expression is set to Zb. The impedance of the ferrite bead model is now ready to be optimized in the Model program.

A new model file is created by selecting New from the Model menu. The New Part dialog box will be invoked automatically which prompts for the device type to specify for the first part in the model file. For a user created part, the part type selected should be User. At this point, the Analysis Type, Circuit, Waveform, and Graph Title can be specified. The Circuit field should be set to the test circuit that was created, in this case FerriteBead.cir. Next, the Analysis Type field is specified as AC Analysis since that was the analysis type used in the test circuit. In the Waveform field, the expression F vs. Zb is selected. Finally, the Graph Title is defined as Impedance vs. Frequency. This title simply labels the plot in the Model program. The final settings for the dialog box are shown below.

New Part dialog box settings for the ferrite bead subcircuit

All of the component values in the ferrite bead subcircuit need to be optimized. In the Parameters section of the model file, the ... buttons can be clicked to add a parameter to be optimized. In the test circuit, the ferrite bead component has the part name X1, so the following component parameters are set to be optimized: X1.R1, X1.C1, X1.L1, X1.R2, X1.C2, X1.L2, and X1.R3.

The MPZ1608S601A ferrite bead from TDK was chosen as the device to model. The input data and results for this device are shown below. As can be seen in the figure, the optimized results produce a good match to the input data. Using the Create Model for this Part command under the Model menu, the following subcircuit model is produced.

.SUBCKT MPZ1608S601A 1 2
L1 1 3 1.047996547u
R1 1 3 612.3746753794
C1 1 3 798.1766699999f
R2 3 4 302.00781172
L2 3 4 2.246831281u
C2 3 4 4.317152502p
R3 4 2 5.0318715819
.ENDS MPZ1608S601A

The Save Part to Template Library command under the Model menu can be used to save the current configuration as a template for easy reuse in optimizing other ferrite bead models.

MPZ1608S601A ferrite bead optimization

TDK also has a SPICE model available for the MPZ1608S601A device. Their model uses a single parallel RLC with a series resistor. The analysis plot below compares the impedance versus frequency curves for the Micro-Cap and TDK models. The Micro-Cap model provides a much closer fit to the data sheet curve.

Micro-Cap model versus TDK model

Download Winter 2011 Circuit Files
Return to the main Newsletter page