Instrumentation Amplifier improper frequency response

Question

Followup to this question.

I have an instrumentation amplifier.

When conducting an AC Sweep, this is the response.

There are two issues with this. Firstly, the signal magnitude is far too low. Secondly, the signal somehow grows on higher frequencies.

I lack any reactive passive components and reactance of the op-amp used (the ADA4091) is not significant until exceeding 100kHz. If there is a parameter in the op-amps that would affect this, I am unaware of it.

Bode plot with PR8 and PR9 included, points within the Instrumentation Amplifier.

Addendum: The input voltages (V17 and V20) are offset by +2.5V. Unfortunately Multisim does not display that properly. Thank you to Andy aka for reminding me to specify that.

Addendum 2: I've isolated the issue to the latter half of the circuit, as disconnecting the two shows that the first half acts within reason with a magnitude of around -1dB for an AC Sweep, while the latter half still has a -100dB loss.

Based on suggestions that Multisim is not as commonly used, I simulated the latter half of this circuit (which is just a differential amplifier) in LTSpice. I removed all offsets and provided a +5V and -5V voltages as inputs.

The AC Sweep remains unsatisfactory despite a reasonable transient response.

One thing of note is that the power source powering the Op-Amp (An ADA4091) is returning the following response in AC Sweeps:

The LTSpice simulation file in question: https://ufile.io/640sx0l3 (I can put it somewhere else if this site is not too familiar with ufile)

Addendum 3: Other things attempted include

1. Changing values and ratio of resistor. Changing values of resistor while maintaining ratio did not improve magnitude. Increasing gain of system with resistor ratio changes did improve the magnitude to an extent in the AC Sweep (I was able to get -20dB) but due to application issues, the gain of the diff. amplifier cannot be over 20.

2. Change input voltage to 5V and -5V. No change observed.

3. Change input voltage to it's own loop. This improve the magnitude greatly, but the output voltage became dependent on the voltage source, which varied significantly.

4. Change input offset from 2.5V to 0V. This had no effect.

5. Attempt to switch to 2-opamp Instrument Amplifier circuit. Magnitude was similarly low.

Answer 1

Your two sources spec "AC 1", so in AC mode they have the same phase. You are simulating the common mode rejection of the differential amplifier. As expected, CMRR decreases with rising frequency, so the "gain" you plot starts from very low (high CMRR) at low frequency and then rises as frequency increases.

Solution: define one of the AC sources as "AC -1" so you have an AC differential signal at the input.

Note the phase specified in SINE(...) is only for transient and is ignored in AC mode. In fact everything you put in the left side of this box is only for transient, it will be ignored in AC and DC modes. For AC you can specify amplitude and phase, likewise these are ignored in transient and DC modes.

Better solution: use a bunch of defines like so

.define test_cmrr 0
.define test_diff 1
.define test_psrr 0

Then for each source you set the AC value to the relevant variable. For example these two input sources would have "AC test_cmrr+test_diff/2" and "AC test_cmrr-test_diff/2".

Power supply sources have "AC test_psrr". Then you can change a define, and that sets your sources properly to plot what you want.

Or you can put a voltage source for the common mode, and two voltage sources for the differential mode (same definition for both but one has polarity switched), which is a lot more convenient if you want to make a transient sim with a non-constant common mode, or signals with different amplitude/frequency on both common and differential modes, for example to check for saturation.

Here is a crummy model of LM358 which uses a spice current source to model the input stage tail current source, so it allows unrealistic input common mode:

Answer 2

There are two issues with this. Firstly, the signal magnitude is far too low.

Your input signals must be centred around half the op-amp supply. You op-amp is powered from 5 volts and 0 volts and therefore you need to centre the input signals to 2.5 volts or they might not won't work correctly. Try looking at the transient response and you will see ugly half wave rectified sinewaves at the outputs or, maybe you won't see anything if the model is designed to ignore any input signal close to 0 volts.

Secondly, the signal somehow grows on higher frequencies.

This also may be due to your lack of input biasing.

Answer 3

One thing that can appear to be frequency response problems is slew rate issues. As frequency goes up, slopes go up, too, requiring higher slew rates. So, something that works for small output signals may not work for large output signals.

Peek at the slew rate of your final output op amp, and make sure the peak value of the derivative of you output "fits".