2
\$\begingroup\$

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.

\$\endgroup\$
2
  • \$\begingroup\$ haven't done spice in a while, but wouldn't you have two of these lines? \$\endgroup\$ Commented Apr 21, 2017 at 21:20
  • \$\begingroup\$ No, you can only have 1 analysis line \$\endgroup\$
    – Voltage Spike
    Commented Apr 21, 2017 at 21:21

3 Answers 3

1
\$\begingroup\$

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))

enter image description here

\$\endgroup\$
3
  • \$\begingroup\$ Can I run this in one sim? or do I have to run the sim twice? If I have to run the sim twice then it's probably easier to change the noise statement \$\endgroup\$
    – Voltage Spike
    Commented May 19, 2018 at 4:03
  • \$\begingroup\$ @laptop2d it is one simulation. \$\endgroup\$
    – DavidG25
    Commented May 19, 2018 at 4:06
  • \$\begingroup\$ @DavidG25 It's actually two simulations, disguised by the .step command. I'm a bit pedantic now, but it's about the same: change a .step or change a .noise card. It's still half-automated, and could be done for more than two I/O. \$\endgroup\$ Commented May 19, 2018 at 6:54
2
\$\begingroup\$

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!

\$\endgroup\$
1
  • 1
    \$\begingroup\$ This is what Mike Engelhardt does but with voltage controlled switches. \$\endgroup\$
    – DavidG25
    Commented May 9, 2018 at 0:22
-1
\$\begingroup\$

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.

enter image description here

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.

enter image description here

\$\endgroup\$
3
  • 1
    \$\begingroup\$ The question was about LT spice, thanks for playing. \$\endgroup\$
    – Voltage Spike
    Commented Apr 22, 2017 at 7:28
  • \$\begingroup\$ They wanted to do noise analysis. \$\endgroup\$ Commented Apr 22, 2017 at 12:24
  • \$\begingroup\$ I wanted to do a specific type of noise analysis in LT spice, if you would take the time to read the question and answer the question you would have known that \$\endgroup\$
    – Voltage Spike
    Commented Apr 26, 2017 at 20:00

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.