Multiple output noise analysis with LT spice

Question

If I want to do a noise analysis I do this in LT spice:

.noise V(adc1) V6 dec 12 0.01 1e9

Where V(adc1) is the voltage for the output node of the analysis and V6 is the source.

Question: Is there a way to have two nodes in the analysis?

Sometimes I copy circuits modify one and and compare the two circuits.

Answer 1

This can be done with switches and a step parameter that toggles the switches.

You won't be able to integrate the noise over a bandwidth in the plot window anymore, but you can use .meas to output the integrated noise to the error log e.g.

.meas out_noise INTEG(V(onoise))

Answer 2

Not having tried this, I can't guarantee it will work... but here is an idea:

Create a behavioral voltage source that acts as a mux between the two nodes, and use a swept parameter to control the mux. Set the output of the mux to be the output node for your noise analyis. Something like this:

BX Vmux 0 V={k*V(out1)+(1-k)*V(out2)}
.noise V(Vmux) V1 dec 12 0.01 1e9
.step param k list 0 1

Let me know if it works!

Answer 3

This tool lets you examine all the noise sources, simultaneously, and show final SNR/ENOB for a given Input VoltPP at a given FrequencyOfInterest (FOI). I've not activated the "gargoyles", the magnetic/electric/VDD/GND trash sources.

Here are thermal distortion (opamp shifts in input offset voltage, because of heating; and resistor value shifts that cause changes in Closed Loop Gain.) and the unified presentation of all the KT/Boltzmann/Johnson random noise.

Here is the 3 opamp signal chain, to amplify a 100uVpp signal to fit a 5vpp ADC. For low noise, the first opamp uses params (UGBW, Rnoise, Rout, DC_gain) of OPA211. The Gain Set resistors are also very low values.