# How to verify noise modelling in fully differential op-amp Spice models?

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.

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

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?

• 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. Commented Jul 10, 2022 at 15:22
• @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? Commented Jul 11, 2022 at 6:12

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>.
• 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. Commented Jul 11, 2022 at 9:53
• 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. Commented Jul 11, 2022 at 9:56
• @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 -- Commented Jul 11, 2022 at 12:34