2
\$\begingroup\$

Texas Instruments explains in one of their videos how to verify the noise model of op-amps in Tina-TI. T For this, the op-amp is wired in a buffer configuration. A voltmeter (voltage pin) is placed at the output and an ampmeter is placed at the non-inverting input of the op-amp.

Noise Test Circuit

The noise analysis shows the voltage and current noise densities of the op-amp.

enter image description here

I want to use a fully differential op-amp and do some noise calculations. Can anyone tell me how I can verify the noise model of a fully differential op-amp?

\$\endgroup\$
2
  • \$\begingroup\$ Use one noise source and several VCVS or VCCS for driving in differential mode. If the output is also differential then use a summer to output into one node. If you're using LTspice don't forget about the noiseless flag. Other simulators might have their own. \$\endgroup\$
    – a concerned citizen
    Commented Jul 10, 2022 at 15:22
  • \$\begingroup\$ @aconcernedcitizen Thanks for your hint. I tried to think of some way how to drive the fully differential op-amp with vcvs. Do you mean replacing the resistors which set the gain with vcvs controlled by the source? \$\endgroup\$
    – FrüchteTony
    Commented Jul 11, 2022 at 6:12

1 Answer 1

Reset to default
3
\$\begingroup\$

For a differential input you can split the input source with two VCVSs, like this:

diff. input noise

I've used a .step command to show both output nodes, side by side. They would have been perfectly overlapped if it weren't for the slightly higher value of R3, which was supposed to be 3k || 6k = 2k.

If your output is also differential, either use a behavioural source (voltage or current) with V=V(1)+V(2) (or whatever nodes there are), or sum them up with two totem-pole VCVS, or with two VCCS into one shunt resistor, <insert_any_other_method>.

\$\endgroup\$
6
  • \$\begingroup\$ I was looking for a method to verify an FDA's noise modelling and compare it to the datasheet to see if it is modelled correctly. For a normal op amp it is easy as it can be wired in a buffer configuration. Voltage and current noise can be measured easily. For a FDA this is not that simple. In your example the input referred noise caused by the voltage noise and current noise is amplified by the noise gain. Or am I wrong? \$\endgroup\$
    – FrüchteTony
    Commented Jul 11, 2022 at 9:33
  • \$\begingroup\$ What current noise? Generated by what current source? V1 is the only noise source, the one needed for the analysis to work. The .step command uses, separately, voltages at nodes 1 and 2, coming from the same V1, but on different, nonintersecting paths. The bottom example has a gain of 3, the top also 3. The input is split into differential noiseless sources of 0.5, each, to account for differential input. The resistors contribute noise but if that's a problem use what I said in the other comment: add noiseless (e.g. 6k noiseless). This is LTspice, others may have it different. \$\endgroup\$
    – a concerned citizen
    Commented Jul 11, 2022 at 9:53
  • \$\begingroup\$ With noiselss you'll see that both traces will completely overlap, since the only difference in the plots was given by the slight imbalance of R3 -- intended, precisely to show the imbalance, so that you know that the resistors contribute noise and that the only difference between the circuits is due to the resistors. That's why I said "They would have been perfectly overlapped if it weren't for the slightly higher value of R3". That should give you a clue. \$\endgroup\$
    – a concerned citizen
    Commented Jul 11, 2022 at 9:56
  • \$\begingroup\$ How would you measure the op-amp's current noise then, if there is no current noise source? I have seen a tutorial where one large resistor (10Meg) was added to the noninverting input of an op amp to cause a voltage drop of the current noise. allaboutcircuits.com/technical-articles/… \$\endgroup\$
    – FrüchteTony
    Commented Jul 11, 2022 at 11:36
  • \$\begingroup\$ @FrüchteTony If you need a current source then you use a current source. The syntax in SPICE, in general, for .noise is .noise <output_quantity> <input_source> ... , meaning there can only be one source. If you look at the command I have used you will see .noise V(o) V1 ... , therefore my source is V1, a voltage source. If you mean to analyze the current then you need a current source. If you need it for FDA then use a voltage source of apppropriate magnitude and two VCCS, instead of VCVS, transforming the input voltage into current. If you wish to keep the voltage but -- \$\endgroup\$
    – a concerned citizen
    Commented Jul 11, 2022 at 12:34

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

Not the answer you're looking for? Browse other questions tagged or ask your own question.