Calculating inductance of a Ferrite Bead

[nickthamma]

Hello,

From my understanding of Ferrite Beads, it is typically specified by an impedance value @ 100 MHz. If I wanted to replicate the same circuitry as a Ferrite Bead (inductor with a resistor in series), how would I go about calculating the inductance. Looking at a particular ferrite bead's datasheet (**broken link removed**), I see that there is a DC resistance which I assume that this would be the maximum equivalent series resistance of the inductor. In addition, the datasheet also gives me the impedance value @ 100 MHz. Could I technically calculate the inductance knowing that the impedance of the inductor is (ZL = j*2*pi*freq*L)?

 

[FvM]

Could I technically calculate the inductance knowing that the impedance of the inductor is (ZL = j*2*pi*freq*L)?

Yes, but only as a low frequency estimation. At high frequency, the ferrite works as a lossy inductor which can't be represented by a series resistor.

 

[nickthamma]

Yes, but only as a low frequency estimation. At high frequency, the ferrite works as a lossy inductor which can't be represented by a series resistor.

What do you mean by low frequency estimation? I had thought that resistance is dominant at high frequencies in a ferrite bead.

 

[FvM]

I had thought that resistance is dominant at high frequencies in a ferrite bead.

Yes and inductance at low frequencies.

 

[nickthamma]

Sorry, I misunderstood. So therefore, technically, I could have an inductor with a series resistor and it would work the same as a ferrite bead? Is my assumption correct?

 

[FvM]

No. A series resistor can't represent the behaviour at high frequencies. A parallel resistor fits better, but not exactly. You have the Z,X,R curves of most ferrite beads, just try to model it with different LR circuits.

What do you want to achieve? Why don't you use a ferrite bead if you want it's behaviour?

 

[nickthamma]

No. A series resistor can't represent the behaviour at high frequencies. A parallel resistor fits better, but not exactly. You have the Z,X,R curves of most ferrite beads, just try to model it with different LR circuits.

What do you want to achieve? Why don't you use a ferrite bead if you want it's behaviour?

I would like to create a spice model that will represent a particular ferrite bead for simulation.

 

[FvM]

Some time ago, a needed to derive a SPICE model from manufacturer ferrite bead specifications, in this case a Murata part that comes with S-parameter measurements.

I found that a dual RLC circuit could fairly represent the impedance curve and fitted the model parameters partly manually, partly using the Excel solver.

.SUBCKT BLM03AG241   1 2
RS   1  11  0.8
RP1 11 12 210
LP1 11 12 1.001u
CP1 11 12 0.9p 
RP2 12 2 236
LP2 12 2 0.106u
CP2 12 2 0.54p 
.ENDS

 

[nickthamma]

Thank you very much! That helps a lot. Though, I am quite curious how you came up with these component values. Did you just play around with the values or is there some mathematical method in approximating these values?

 

[FvM]

As said, I used the MS Excel Solver to adjust parameter values for meeting the empirical impedance curve. A least square sum "distance" criterion must be implemented manually. The PSpice optimizer is another tool that can be used for similar purposes. By nature of the model a fully automated parameter optimization doesn't necessarily converge or not converge to best solution. This it's helpful to use a meaningful estimation as starting point and fix or at least constraint some of the parameters.