I have designed a charge amplifier to convert the charge from the force sensor into voltage. The force of the sensor is dynamic from 0 to 100N which is modelled as a voltage source V3 with a sine wave oscillating from 0 to 1KHz. C2 is the sensor static capacitance. The current source B1 is differentiating the voltage from V3. The system need to be able to respond between 0.1 to 1KHz. The problem is as shown in the AC simulation result the circuit on the right hand side does not give a low pass filtered response with a cut off frequency of 1KHz. I have made the circuit on the left hand side with a current source just to confirm that the charge amplifier is designed properly and the response is is as expected so the problem seem to be coming from the charge source. What could be the problem?

 

Can you give a part number or data sheet for your force sensor?

 

Can you give a part number or data sheet for your force sensor?

This is a theoretical simulation, I don't have a specific force sensor in mind yet. More details below.

A force sensor, based on a piezoelectric crystal, generates 10pC/N, and is required to measure up to 100N of force. The force is dynamic and the system needs to be able to respond between 0.1Hz and 1kHz. The sensor has a static capacitance of 20pF.

 

A charge amplifier is essentially an integrator. Having designed plenty of them for instrumentation to interface with piezoelectric accelerometers and dynamic pressure transducers, I have to ask: why are your DC feedback resistors (R1 and R2) so small? I would have expected dozens, even hundreds, of megohms, perhaps even gigohms considering the lower end of your required frequency response. 1K ohms doesn't make sense, as that would give you a lower frequency rolloff of 1 KHz, not 0.1 Hz.

What gives?

 

A force sensor, based on a piezoelectric crystal, generates 10pC/N, and is required to measure up to 100N of force. The force is dynamic and the system needs to be able to respond between 0.1Hz and 1kHz. The sensor has a static capacitance of 20pF.

Ah. If the sensor has a static capacitance of 20 pF, and a charge sensitivity of 10 pC/N, then it must therefore have an open-circuit voltage sensitivity of (10 pC/N / 20 pC/V) = 0.5 volts/N. For simulation purposes, model the sensor as a 20 pF capacitor in series with a 0.5V/N voltage source.

The feedback capacitor, **NOT*** the feedback resistor, in your opamp circuit is what sets the output V/N scale factor. All the resistor does is provide a DC return path for the opamp integrator, so it doesn't end up saturating against the positive or negative rail. Its value determines the lower frequency rolloff (not the upper rolloff) of the charge amplifier.

Upper frequency response limit (1 KHz) is best established by a separate filter fed by the output of the charge amplifier stage.

 

Ah. If the sensor has a static capacitance of 20 pF, and a charge sensitivity of 10 pC/N, then it must therefore have an open-circuit voltage sensitivity of (10 pC/N / 20 pC/V) = 0.5 volts/N. For simulation purposes, model the sensor as a 20 pF capacitor in series with a 0.5V/N voltage source.

The feedback capacitor, **NOT*** the feedback resistor, in your opamp circuit is what sets the output V/N scale factor. All the resistor does is provide a DC return path for the opamp integrator, so it doesn't end up saturating against the positive or negative rail. Its value determines the lower frequency rolloff (not the upper rolloff) of the charge amplifier.

Upper frequency response limit (1 KHz) is best established by a separate filter fed by the output of the charge amplifier stage.

-by modelling the sensor as a voltage source in series with a capacitor to measure the force up to 100N, does the voltage source need to be configured as PWL function? In other words how can the range be dynamic?

-Is the gain defined as 1/Cf?

-are you saying that the lower cut off frequency is defined as: Fl(0.1Hz)=1/(2*pi*RfCf)

 

-by modelling the sensor as a voltage source in series with a capacitor to measure the force up to 100N, does the voltage source need to be configured as PWL function? In other words how can the range be dynamic?

Ummm... if you're doing an AC analysis in SPICE, then the source should have an AC voltage value; if you're doing a TRAN analysis, give it one of the TRAN time-domain functions: PWL, SIN, PULSE, whatever is appropriate for the analysis you want to do.

-Is the gain defined as 1/Cf?

Yes, the charge gain would be 1/Cf.

-are you saying that the lower cut off frequency is defined as: Fl(0.1Hz)=1/(2*pi*RfCf)

Yes.

Let's do an example:

You say you need to measure up to 100N of force (I assume this means +/- 100N). Let's say, arbitrarily, that we want to represent 100N of force by 1V on the output of your charge amplifier. The sensor produces 10 pC/N, so at 100N it produces 1000pC. To get an amplifier output of 1V at 1000pC, Cf will then be 1000pF.

If Cf = 1000 pF and your desired low frequency limit is 0.1 Hz, the Rf must be R = 1 / (2 * pi * f * Cf) = 1590 Mohms.

 

Ummm... if you're doing an AC analysis in SPICE, then the source should have an AC voltage value; if you're doing a TRAN analysis, give it one of the TRAN time-domain functions: PWL, SIN, PULSE, whatever is appropriate for the analysis you want to do.


Yes, the charge gain would be 1/Cf.


Yes.

Let's do an example:

You say you need to measure up to 100N of force (I assume this means +/- 100N). Let's say, arbitrarily, that we want to represent 100N of force by 1V on the output of your charge amplifier. The sensor produces 10 pC/N, so at 100N it produces 1000pC. To get an amplifier output of 1V at 1000pC, Cf will then be 1000pF.

If Cf = 1000 pF and your desired low frequency limit is 0.1 Hz, the Rf must be R = 1 / (2 * pi * f * Cf) = 1590 Mohms.

After running AC simulation I am not sure why the gain is -34dB. 1/Cf provides a gain of 10^9.


In the trans analysis I have put a sine wave to model the pressure applied but the gain is also negative.

 

After running AC simulation I am not sure why the gain is -34dB. 1/Cf provides a gain of 10^9.

Yes, the voltage gain, if you're modeling the sensor as a voltage source in series with 20 pF, will be -34dB; that's 20 * log (20pF/1000pF). The charge gain, regardless, is 1V/1000pC which, multiplied by your sensor sensitivity of 10 pC/N, gives a charger amplifier output scaling of 0.01V/N.

In the trans analysis I have put a sine wave to model the pressure applied but the gain is also negative.

Yes, the sign of the gain is inverted, because you are (by necessity) feeding the sensor into the inverting input of an opamp.

 

Yes, the voltage gain, if you're modeling the sensor as a voltage source in series with 20 pF, will be -34dB; that's 20 * log (20pF/1000pF). The charge gain, regardless, is 1V/1000pC which, multiplied by your sensor sensitivity of 10 pC/N, gives a charger amplifier output scaling of 0.01V/N.


Yes, the sign of the gain is inverted, because you are (by necessity) feeding the sensor into the inverting input of an opamp.

Could you please explain why the gain is 20pF/1000pF. I want to drive an ADC operating at 3.3V after the low pass filter, therefore I want the gain to be controllable depending on the ADC input range.
In the trans analysis how come the range is between +/-498mV. Also since the voltage source amplitude should be 0.5V, Does that mean the sine wave amplitude should oscillate between +/-0.5

 

Could you please explain why the gain is 20pF/1000pF. I want to drive an ADC after the low pass filter, therefore I want the gain to be controllable depending on the ADC input range.

The voltage gain of the charge amplifier is equal to your sensor capacitance (20pF) divided by the amplifier feedback capacitance (1000pF). But what's really important, for determining the scaling for your sensor + amplifier, is the charge gain of the charge amplifier, and that's 1/Cf.

In the trans analysis how come the range is between +/-498mV. Also since the voltage source amplitude should be 0.5V, Does that mean the sine wave amplitude should oscillate between +/-0.5

Ummm... I don't see an output of +/- 498 mV; I see a much smaller output (hard to tell what, because you let the trace run off the scale on the bottom), superimposed on a roughly -480 mV DC offset caused, most likely, by the input bias current of the opamp multiplied by the 1.59 Gohm feedback resistor.

Whatever the DC offset, I would expect to see about a +/- 20mV 1 KHz AC signal on the output.

 

The voltage gain of the charge amplifier is equal to your sensor capacitance (20pF) divided by the amplifier feedback capacitance (1000pF). But what's really important, for determining the scaling for your sensor + amplifier, is the charge gain of the charge amplifier, and that's 1/Cf.


Ummm... I don't see an output of +/- 498 mV; I see a much smaller output (hard to tell what, because you let the trace run off the scale on the bottom), superimposed on a roughly -480 mV DC offset caused, most likely, by the input bias current of the opamp multiplied by the 1.59 Gohm feedback resistor.

Whatever the DC offset, I would expect to see about a +/- 20mV 1 KHz AC signal on the output.

so if the ADC operates at 3.3V, I would still look at the charge gain for scaling?

 

so if the ADC operates at 3.3V, I would still look at the charge gain for scaling?

You said your sensor puts out 10 pC/N, right? And you want a usable range, coming out of this charge amplifier, of +/- 100N, right? That means your range, in terms of charge, is +/- 1000 pC. How much output voltage do you want to represent that? I chose +/- 1 V, arbitrary but reasonable given your ADC. So for +/- 1000 pC to yield +/- 1 V, that means the capacitance has got to be 1000 pF.

 

I finally got it thanks.

the circuit so far is as shown above, the last part of the system remaining is an ADC, I was wondering if in LTspice it was possible to have a block such as SAR or FLASH converters or do I have to design the logic myself?
Also since the digital part of the system operate at 3.3V, how would that work in reality. Do I have to find an OP amp that works with 3.3V to have only one PSU?

 

LTSpice is SPICE; it's an analog simulator and won't help you at all with digital logic.

WRT to your opamp, I'd say if you want to have a single power supply then yes, you'll have to find an opamp that operates at 3.3V, if that's what your ADC requires. The circuit also needs work to adapt it to use more practical component values, and also to provide proper DC bias of the opamp inputs if you're going to operate off a single +3.3V supply.

 

Why do you want to use such a weird combination as 10meg and 15.9pF for that low pass? Usually ADCs have a significant input current when the sample is being taken, so you should aim for a lot smaller resistor and a larger capacitor, i.e. 10k and 16nF.
Also with such large impedance that part will be more susceptible to induced noise, so it is better to keep in some are with lower impedance.

As for your input stage, you need to get rid of any leakage going into the inverting pin of that opamp, usually this is achieved with either a guard ring around that sensitive node, or by having that node floating above the pcb on teflon standoffs.

 

LTSpice is SPICE; it's an analog simulator and won't help you at all with digital logic.

WRT to your opamp, I'd say if you want to have a single power supply then yes, you'll have to find an opamp that operates at 3.3V, if that's what your ADC requires. The circuit also needs work to adapt it to use more practical component values, and also to provide proper DC bias of the opamp inputs if you're going to operate off a single +3.3V supply.

Is there a software where I can simulate the whole system together? As I would like to do noise analysis and calculate the SNR.
What additional component are needed to provide a proper DC bias at 3.3V.

 

Why do you want to use such a weird combination as 10meg and 15.9pF for that low pass? Usually ADCs have a significant input current when the sample is being taken, so you should aim for a lot smaller resistor and a larger capacitor, i.e. 10k and 16nF.
Also with such large impedance that part will be more susceptible to induced noise, so it is better to keep in some are with lower impedance.

As for your input stage, you need to get rid of any leakage going into the inverting pin of that opamp, usually this is achieved with either a guard ring around that sensitive node, or by having that node floating above the pcb on teflon standoffs.

I will, it was just to test the frequency response quickly.

 

Is there a software where I can simulate the whole system together?

If there is, I'm not familiar with it.

What additional component are needed to provide a proper DC bias at 3.3V.

You would need to provide (via a resistive voltage divider, or some equivalent method) a "virtual ground" for the non-inverting opamp input such that the opamp will be running with its inputs inside the allowed common-mode input voltage range. Also, you will need to find an opamp that can operate off 3.3V which has EXTREMELY low input bias current.

Also, while that 1590 Mohm feedback resistor in the opamp circuit is theoretically correct for getting the low-frequency rolloff you specified, be aware that it is not a practical approach: in reality, you would use a much lower value resistor (say, somewhere between 10 Megs and 100 Megs) and get the effect of a higher resistor value by feeding it from a voltage divider connected to the opamp output. Take a look at the schematic on page 12 of this opamp data sheet, labeled "Accelerometer Amplifier with DC Servo", to see what I mean by that:

http://cds.linear.com/docs/en/datasheet/1793f.pdf

Also, I agree with kubeek's comments. Bottom line is, this is NOT a trivial design task.