CRYSTAL LADDER FILTER SIMULATION WITH SPICE

For the purposes of this exercise, I’ll assume that the crystal parameters have been measured, and are as follows:

Frequency 4 MHz

Lm (motional inductance) 0.1971 H

Cm (motional capacitance) 8.03554e-15 F

Rm (motional resistance) 48 ohms

Co (static capacitance) 3.5 pF

The filter configuration is as follows:

 

Calculated capacitor values for this filter are:

C3 = 94 pF

C2 = C4 = 60 pF

C1 = C5 = 14 pF

The terminating resistance is 1200 ohms.

The Pulsonix package I use for PCB design came with Pulsonix SPICE, which I’ll be using here. I created the following schematic for the SPICE analysis:

Each crystal is represented by its equivalent circuit, with its parameters. The five shunt capacitors have been added, and the input resistance (1200R) is in series with the signal source. A 1200R load is placed across the output. The 1G resistors across the shunt capacitors are required by SPICE; it doesn’t like ‘floating’ nodes, and such a high resistance won’t affect the simulation.

Running SPICE gave the following plot:

It appears to be quite a useful filter, with a reasonable shape factor, and a 3 dB bandwidth of about 500 Hz.

Lets see what happens if we change the terminating resistances to 330R:

As you can see, a real mess has been made of the response. The terminating impedance of this type of filter is quite critical.

I've extracted the netlist for this filter from Pulsonix:

R7 $4 $0 1200
L3 $0 $1 0.1971H
C5 $0 $27 3.5p
C6 $1 $2 8.0355114e-15
R5 $2 $27 48
V1 $4 0 AC 1 0
C7 $7 $8 8.03554e-15
R6 $8 $28 48
L4 $27 $7 0.1971H
C8 $27 $28 3.5p
C9 0 $27 60p
C10 $15 $16 8.0355114e-15
C11 $28 $26 3.5p
L5 $28 $15 0.1971H
R9 $16 $26 48
C12 0 $28 94p
R10 0 $27 1G
R11 0 $28 1G
C13 $24 $25 8.0355114e-15
.graph $23 nowarn=true
L6 $26 $24 0.1971H
C14 $26 $23 3.5p
R12 0 $26 1G
R13 $25 $23 48
R14 0 $23 1200
C15 0 $26 60p
C16 0 $0 14p
C17 0 $23 14p
.ac lin 10000 3.998Meg 4.001Meg

With a few minor changes you should be able to use it with any flavour of SPICE.

Here are some free SPICE packages:

SPICE OPUS http://fides.fe.uni-lj.si/spice/
SIMetrix Intro http://www.newburytech.co.uk/
PSPICE Student Version http://www.cadencepcb.com/products/downloads/PSpicestudent/default.asp

SIMetrix is the SPICE used with the Pulsonix package.

Hosted by www.Geocities.ws

1