Charge Amplifier - Spice vs. App Note

[geo_leeman]

Hey folks - I'm messing with a charge amplifier design and found a great app note by TI: https://www.ti.com/lit/an/sloa033a/sloa033a.pdf Within it has some simple formula for the lower/upper rolloff points for the gain. (See attached). I made up a quick spreadsheet and modeled the circuit in LTSpice (granted, with a different opamp, but with high GBP and FET input) and my numbers don't quite agree. The lower point is close, but the higher side is way way off. I've tried with several different setups and always get this result. Am I missing something fundamental, am I mental, or a combination?

[moffy]

Your input high pass filter (C2 & R2) has a 3db pt of about 36Hz. Your low pass filter/integrator(C1 & R1) has a 3db pt of about 14mHz. So what you are seeing is correct.
Also the ratio of C2/C1 sets the gain in the flat region for these values.

[sdouble]

remove your serie resistance and add a cap to ground to mimic your sensor cap.
your feedback cap is huge meaning that the sensitivity of your apparatus will be rather low.

[geo_leeman]

I've added a cap to ground and used a current source instead so now it should be *exactly* like the schematic in the app note, but I'm not getting anything that makes much more sense. The series resistor is in the schematic as Ri. See Attached.

[SiliconWizard]

I think a correct way to model the charge source would be to use an arbitrary behavioral current source instead, and set the function to the derivative of a voltage source modeling the charge Q(t). The current is obviously the derivative of the charge. The derivative of a function such as: A*sin(2*pi*F*t+phi) is: 2*pi*A*F*cos(2*pi*F*t+phi). You instantly see that it's not going to be just a scaled version of the original, but its amplitude grows as the frequency grows. An AC analysis with a basic current source will thus not give you the same result!

Attached is an LTSpice schematic of what I mean. It looks like it gives a frequency response pretty close to what's in the app note. (With your values: Flow ~ 0.145 Hz, Fhigh ~ 361 Hz.)

Edit: added a picture for quick preview.

[geo_leeman]

That makes sense and I can get the proper output then - the only thing not in alignment now is that the gain should be 40dB and we're seeing around 155dB. Looking at the input to the op-amp we see it's at about 40dB in the 1-100Hz region. So I'm guessing we're still not quite capturing the charge source right?

[SiliconWizard]

The gain given in the app note is 1/Cf, which in this case equates to: 20*log(1/22e-9) ~ 153 dB, which is what we get here in simulation.

Just consider it's not a voltage gain per se, it's the gain between the input charge and the output voltage.

[geo_leeman]

The gain given in the app note is 1/Cf, which in this case equates to: 20*log(1/22e-9) ~ 153 dB, which is what we get here in simulation.

Just consider it's not a voltage gain per se, it's the gain between the input charge and the output voltage.

Ah, I see. Helpful PDF breadcrumb for myself and others as well: https://www.hamamatsu.com/resources/pdf/ssd/charge_amp_kacc9001e.pdf

[sdouble]

your Cc is far too high.
i should be in the (tens to hundreds of) pF range

[geo_leeman]

your Cc is far too high.
i should be in the (tens to hundreds of) pF range

Actually assuming Cc to be zero, the other cap is the sensor/transducer capacitance.

[sdouble]

your Cc is far too high.
i should be in the (tens to hundreds of) pF range

Actually assuming Cc to be zero, the other cap is the sensor/transducer capacitance.

yep, my bad.
Are you sure that it is of 20 uF ? That seems rather high.

[geo_leeman]

In this case it is, just was working with some "nice" values for simulation. Real sensor is a plate about 10" in diameter.

[sdouble]

a plate is not capacitive.
are there 2 parallel plates ?

[Zero999]

I made up a quick spreadsheet and modeled the circuit in LTSpice (granted, with a different opamp, but with high GBP and FET input) and my numbers don't quite agree.

For future reference, use LTSpice's UniversalOpamp model and set the gain, roll-off, input impedances to the same as the real op-amp you intend to use. It's not perfect, but better than using a random op-amp model, substantially different to the op-amp you're going to use.