• State Resolved
  • Locked Locked
  • Replies 3 replies
  • Subscribers 40 subscribers
  • Views 2913 views
  • Users 0 members are here
Support feedback
Options
Options
Similar topics

This thread has been locked.

If you have a related question, please click the "Ask a related question" button in the top right corner. The newly created question will be automatically linked to this question.

TINA/Spice/opa330: Noise Analysis

Bryan Hsieh
Prodigy 120 points
Part Number: OPA330
Other Parts Discussed in Thread: TINA-TI

Tool/software: TINA-TI or Spice Models

Hi all,

Sorry for asking such a basic question but how does noise analysis work in TINA?

Below is the filter circuit I am trying to do the noise analysis on.

But from the results I seem to be getting more input noise than output noise. Isn't input noise = output noise/gain?

Is the input noise the noise from the source or is it the input referred noise, ie output noise =

gain*( noise from source + system added noise), input noise = noise from source or

is it output noise =gain*( noise from source + system added noise), input noise = (noise from source + system added noise).

I am assuming the total noise is the total integral output noise, is this correct?

Also how would I work out the noise factor from the SNR graph as the noise factor is SNRin / SNRout but in the analysis the amplitude of

SNR is set to 1 but SNR from my graph is in hundreds of dBs which would give a negative noise figure ( 0 - SNR from the graph). 

Do I need to integrate across my BW?

Thanks for your help.

Regards,

Bryan Hsieh

  • 0
    TI__Mastermind 33170 points
    Bryan,
    Would you please upload your TINA circuit file to this thread?
    I will take a look at it and try to answer your questions.
    Regards,
    John
  • 0 in reply to John Miller - Sensing
    Prodigy 120 points
    To John,

    Hi thanks for the prompt response, I have uploaded my TINA circuit.

    Regards,
    Bryan
  • 0 in reply to Bryan Hsieh
    TI__Mastermind 33170 points

    Bryan,

    The input and output noise should be related by the small-signal gain over the frequencies of interest.
    For noise sims, you have to identify an output node and an input source.
    The simulator uses these to estimate the simulated gain, and to have reference points for the noise.
    The simulator assumes the relationship between input-referred noise and output-referred noise is:
    OutputNoise = Gain*InputNoise.
    When Gain > 1, the output noise is greater than the input noise.
    When Gain < 1 (stop-band) the input noise is greater than the output noise since the "gain" is really and attenuation of the forward signal. At these frequencies, the input noise will be greater than the output noise.

    To check your circuit, first run an AC response, which shows a band-pass response, with -3dB points at 50mHz and 188 Hz.
    The pass-band shows a gain of 2 V/V, or 6dB.

    If you compare the input and output noise in the pass-band (10 Hz), the output noise is 105 nV/rt(Hz), while the input noise is 52.8 nV/rt(Hz).
    So for the pass-band, the output noise is greater than the input noise by a factor equal to the gain.

    Looking at the low-frequency stop-band (1mHz), the input noise is 8.5uV/rt(Hz) and the output noise is 342 nV/rt(Hz).
    The ratio is 342n/8.5u = 0.0402 & this agrees with the gain curve at 1mHz.

    So it looks like the ratios of your input & output noise are okay.

    I hope this helps. Please let me know if you have any questions.

    Regards,
    John