• State TI Thinks Resolved
  • Locked Locked
  • Replies 4 replies
  • Answers 2 answers
  • Subscribers 41 subscribers
  • Views 2516 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/LMH5401: Calculating noise figure with TINA-TI (LMH5401)

Mark Krangle
Prodigy 50 points
Part Number: LMH5401
Other Parts Discussed in Thread: TINA-TI,

Tool/software: TINA-TI or Spice Models

Hello,

I'm trying to figure out how get noise figure from the TINA noise analysis, using the LMH5401 as an example.  However, I've been unable to get the simulation to match the datasheet and I'm not sure what I'm doing wrong.

I'm using the LMH5401 TINA Reference Design from the product page as an example.  I ran a noise analysis and the input-referred voltage is pretty close to the figure in the datasheet, although not exact (for example, TINA shows 5.8 nV/Hz at 1 kHz, whereas the datasheet shows about 4 nV/Hz).

Next I tried to calculate noise figure using SNR_Vin (dB) - SNR_Vout (dB).  Using numbers from the TINA SNR plots at 200 MHz, this works out to a NF of 15.1 dB.  However, according to the datasheet it should be 9.6 dB.

The difference I'm seeing in input-referred noise should explain part of this discrepancy, but not all of it.  Am I doing something wrong with my noise analysis and NF calculation, or is this just due to the model?

On a related note, is is possible to add noise figure to the diagram with a post processor function?

I should mention that I'm not necessarily planning to use the LMH5401 in my design.  For now I'm just using that reference design as a test to see if I can get a NF from TINA that agrees with the datasheet.

Thanks,

Mark

  • 0
    TI__Mastermind 35885 points

    Mark,

    The data sheet noise figure spec references Figure 59, the test circuit for noise figure and harmonic distortion.
    The test circuit uses the same configuration as the reference circuit, with the exception of a balun to convert the 100 ohm diff signal into a 50 ohm single-ended signal for the test equipment.

    If you haven't used something like this in your TINA circuit, that might be the source of the 6dB discrepancy.

    TINA-TI has a built-in ideal transformer that could possibly serve as a balun.
    Please try using that in your circuit. If it doesn't work we will move to plan B.

    Regards,
    John

  • 0 in reply to John Miller - Sensing
    Prodigy 50 points

    John,

    Thank you for your reply.  I tried your suggestion and it did affect the SNR and NF, but I'm still confused about the results I'm seeing.

    It seems that the ideal transformer model only allows an integer voltage ratio, so I tried it with ratios of 1 and 2.

    With a transformer ratio of 1, I put a 100 ohm resistor across the secondary winding (to present 100 ohm differential to the amplifier output) and measured the SNR.  The SNR at the transformer output increased by 5.1 dB (relative to the baseline reference design) and the resulting NF decreased to 10.2 dB.  This is much closer to the datasheet.

    Next, with a transformer ratio of 2, I put a 25 ohm resistor across the secondary (which should also present 100 ohm differential to the amplifier).  This time the SNR at the transformer output increased by 17.7 dB (relative to the baseline), and if I calculate NF the same way I now get a negative number which does not make sense

    One final thing I tried was to go  back to the reference design (without transformer) and add a second voltmeter (VOUT2) to the right of the 40 ohm series resistors.  This measurement point and termination resistance should be equivalent to the 1:1 transformer case I tried earlier. Indeed, I get the same exact results for SNR and NF (10.2 dB), so is this the correct way to determine NF?  Is the problem simply that it is incorrect to measure SNR and NF at the point of the original voltmeter in the reference design (VOUT)?  That voltmeter is placed directly at the amplifier output, so it is after the internal 10 ohm resistors but before the external 40 ohm.  Still, I don't really understand why SNR would be different between VOUT1 and VOUT2.  Is this due to the noise contribution of the 40 ohm resistors?

    I appreciate any help you can provide.  I really just want to make sure that I am determining NF correctly and that I can trust the simulation results.

    Thanks,

    Mark

    100 ohm differential to the amplifier

  • 0 in reply to Mark Krangle
    TI__Mastermind 35885 points

    Mark,

    Noise figure is usually defined for the conditions of a DUT matched to the signal source and the test load.

    As an experiment the ref circuit was modified to give a 50 ohm differential load on the amp output, which was in turn loaded by a 50 ohm test load.
    The single-ended input is already matched to a 50 ohm signal source, so no changes there.

    So unlike the original test circuit, the modified one will have 50 ohms at the input and output, and it will be matched to a 50 ohm source and a 50 ohm load.
    The circuit is shown in the first image below..
    Running a noise sim on that circuit gave an input SNR of 97.36dB (at 200MHz) and an output SNR of 87.06dB, or a calculated noise figure of 10.3dB.
    This is about 0.7dB higher than the data sheet.
    Inserting a 1:1 ideal transformer between the output resistors and the 50 ohm load (2nd image below) did not change the results. The noise figure was about the same as the previous case at the input and the output of the transformer.

    I am still looking  impact of adding an ideal transformer with a turns ratio of 0.707 to the default circuit, which should be the same as the test circuit given in Figure 59 of the data sheet. No results to report yet.

    Regards,
    John

  • 0 in reply to John Miller - Sensing
    Prodigy 50 points

    John,

    Thank you for your detailed response.  That makes sense about the load impedance, and I'm glad to see the results match the datasheet.

    I was hoping the version with the transformer would be closer, since that is how NF is actually measured.  I tried it myself, but the result was off by about 3 dB.  The only thing I did differently was to use a ratio of 0.5, since that parameter specifies the voltage ratio (and not the turns ratio), but that didn't make a big difference.

    Thanks,

    Mark