Post Go back to editing

AD8606 LtSpice


I am working on the AD5933 Impedance Converter Module but specifically testing the AD8606 portion of the Module board. To test the AD8606 amplifier portion(the part that is circled in red), I input 0.2 Volt AC and the output shows up as ~234mV using the ltspice simulation. The AC analysis does not work when I add RFB SEL resistor to see how it affcects the output voltage. Is my circuit model incorrect or did I miss something? 

ad8606 8-17-21.asc

  • The model as attached does not have feedback resistor for U2, which turns it into an inverting amplifier of Gain=0. If a feedback resistor of 1k is attached it turns it into a unity gain amplifier and the model works as expected. The output load for U2 does not accurately represents the AD5933 input: the 20k resistor is connected to VIN pin, which is a virtual ground created by the AD5933 internal OPAMP and another 20k resistor connected between the VIN and RFB pins.
    Also if you want your model to be more precise, you may want to account for the AD5933 internal resistance, which at 0.2V excitation is about 600 Ohms, you can add that as the parasitic series resistance for your voltage source V3 (page 4, table 1 in the datasheet).
    Also notice that C4R6R7 network is a high-pass filter with cut-off frequency of about 135Hz and your range starts at 100 Hz, so the frequency response should be expected frequency-dependent.

    ad8606 8-17-21-edits.asc