## Ceramic Filter SPICE Model

##### October 1, 2015

As part of a larger project I’m working on, I’ve found myself needing to use a ceramic filter on a 10.7 MHz IF (intermediate frequency) signal. Specifically, I’m using a Murata CERAFIL SFECF10M7GA00-R0 to provide 230 kHz of bandwidth in a ~40 dB IF amplifier. To test the design, I opted to do a SPICE simulation. Murata does not publish a SPICE model of their filters so I had to approximate one myself. This post discusses that model.

### The Model

Unfortunately the manufacturer didn’t provide much in the way of details on how one might model a three terminal filter. The Cerafil Applications Manual, however, offers an “equivalent” circuit for the two terminal device. It is simplified to a series RLC circuit with a parallel capacitance as shown in figure 1.

The specification sheet for the filter specifies frequency independent input and output impedances of 330 Ω. I have trouble believing this but for my purposes it doesn’t really matter; so long as the impedance is as specified within the passband. Insertion loss is specified at 3.5 dB. From this I’ve extrapolated an “equivalent” circuit in figure 2 for the three terminal device.

The input and output impedances are modelled as simple resistors. The output is modelled by a VCVS (voltage controlled voltage source) that transforms the input voltage \(V_i\) via \(H(s)\) and applies a fixed gain \(a\). \(H(s)\) is a simple bandpass second order system defined by

\[\begin{align*} H(s) &= \frac{2\pi Bs}{s^2 + 2\pi Bs + \left(2\pi f_0\right)^2} \\ &= \frac{2\pi (230\;\mathrm{kHz})s}{s^2 + 2\pi (230\;\mathrm{kHz})s + \left(2\pi \left(10.7\;\mathrm{MHz}\right)\right)^2} \\ &= \frac{\left(1.45\times10^6\right)s}{s^2 + \left(1.45\times10^6\right)s + 4.52\times10^{15}} \end{align*}\]while the gain, \(a\), compensates for the insertion loss and the voltage division effect of the circuit. It is defined as

\[\begin{align*} a &= 2\times10^{-3.5\div20} \\ &= 1.34 \end{align*}\]Thus the SPICE model is

```
.SUBCKT SFECF10M7GA00-R0 1 2 3
R1 1 3 330
R2 4 2 330
A1 %vd(1, 3) %vd(4, 3) filter
.MODEL filter s_xfer(
+num_coeff=[
+1.44513262065130e+006
+0.00000000000000e+000]
+den_coeff=[
+1.00000000000000e+000
+1.44513262065130e+006
+4.51988403152288e+015]
+gain=1.3366878)
.ENDS
```

### Results

In order to test the model, the circuit in figure 3 was used. Since the model contains no non-linear elements I only bothered to do AC tests and neglected the transients.

Ultimately it suffers from a few significant flaws. As mentioned above, the input and output impedances are completely independent of frequency. Although specified as such, I find this hard to believe. Perhaps I’ve interpreted the spec sheet incorrectly. Another issue lies in the possibility for the model to behave as an active element. If it is connected to a load impedance of more than 330 Ω it behaves as such. I can’t see myself being prompted to load this device with anything other than a matched impedance but it is something to keep in mind.

As far as the frequency domain goes, the response, as seen in figure 4, does not quite match that in the specifications. In all fairness a second order system is not an accurate model for this filter. I tried using a type II Chebyshev filter instead but it turned out to be quite ill-conditioned and became unstable due to computational error. Beyond that it was actually less accurate in the passband than the second order system. Perhaps a Butterworth or Bessel reponse would be more appropriate. I didn’t bother to account for phase/delay in the filter since it isn’t all that relevant for my purposes.

In the end the model works well enough for this project but could certainly use some improvement. Perhaps in the future I’ll need to tweak it a bit and I’d certainly appreciate any advice or feedback anyone has to offer.