Stats

  • Locked Locked
  • Replies 6
  • Subscribers 125
  • Views 18512
  • Members are here 0
This discussion has been locked.
You can no longer post new replies to this discussion. If you have a question you can start a new discussion

How can I get the input referred noise of dynamic comparator by pnoise?

charlieWu

Hello everyone,

I need to calculate dynamic comparator noise with pnoise, I have read "Keeping Things Quiet: A New Methodology for Dynamic Comparator Noise Analysis" and follow the steps, but I just only get output noise.

There is a statement in Spectre manual : "If the input-referred noise or noise figure is desired, specify the input source by using the iprobe parameter. For input-referred noise, use vsource or isource as the input probe;" "Use refsideband=0 when the input and output of the circuit are at the same frequency(such as with amplifiers and filters)."

but I still can't find out the input referred noise in the simulation result, I can just only see "out" signal , as below: 

I use the following pnoise, pss settings:

simulator lang=spectre
parameters p_vdif=1m ratio=50
sw_vdif sweep param=p_vdif start=1m stop=10m dec=2 {
pss_comp pss period=p_tp harms=100
sampleN_comp (OUTP_LAT OUTN_LAT) pnoise start=0.1 stop=0.5/p_tp noisetype=pmjitter \
crossingdirection=rise thresholdvalue=(p_vdif*ratio) \
pnoisemethod=fullspectrum refsideband=0 iprobe=VINP
}

OUTP_LAT &  OUTN_LA are outputs of comparator and VINP is the voltage source applied to  comparator input , other save settings :

saveOpt options save=allpub currents=all useprobes=yes
save all
save *

Any ideas where I'm going wrong with the simulation setup?

Thanks

  • Dear charlieWu,

    Two quick comments...

    1.There is a more recent example from March 2018 that compares the dynamic noise performance of a comparator using both a transient noise and a pss analysis. This might provide a more recent reference. The Cadence On-line support URL is  at:

    support.cadence.com/.../ArticleAttachmentPortal

    charlieWu said:
    but I still can't find out the input referred noise in the simulation result, I can just only see "out" signal , as below: 

    2. The "out" is the database containing the noise you specified. The input referred noise must be computed from the output noise and gain of your comparator. Page 20 of the note at the URL I provided in [1] provides a specific example.

    I hope this provides a little help!

    Shawn

  • in reply to ShawnLogan

    Dear ShawnLogan

    Thank you for your reply, page 22 of the note says "Calculate equivalent input noise, 1.5mVrms / 3 = ~500μVrms" , I think "3" is the gain of the comparator?

    It seems that I should find out the gain of my comparator first,  originally I thought the gain will be calculated automatically .

    Thanks

  • in reply to charlieWu

    Dear CharlieWu,

    charlieWu said:

    page 22 of the note says "Calculate equivalent input noise, 1.5mVrms / 3 = ~500μVrms" , I think "3" is the gain of the comparator?

    It seems that I should find out the gain of my comparator first,  originally I thought the gain will be calculated automatically .

    Yes, "3" is the gain of the comparator just after its metastable state for the particular input voltage selected in the analysis. A few more details follow if it helps...

    The methodology that is described for computing the latched comparator input referred noise in the URL I sent, does not "automatically" compute the gain. There is an explicit step shown on page 15 indicating that you need to compute the gain and use it to determine the input referred noise. Referring to page 19 which shows the result of sweeping the input differential voltage from 1 nV to 10 mV on a log y axis scale, the relation for a positive feedback latch is given by an exponential relationship (due to the positive feedback). You determine the slope of the "exponential" region for the particular input voltage you are analyzing to find the gain.

    I hope this makes it a bit more clear!

    Shawn

  • in reply to ShawnLogan

    Dear ShawnLogan

    Thanks a lot, your explicit really helps. I don't catch that "ratio" and "gain" are the same before.

    Thank you again

  • in reply to charlieWu

    Dear charlieWu,

    I am very happy to read what I wrote makes sense and helps a little with your understanding! Good luck - this type of simulation is not trivial and do take some effort - so don't give up!

    Shawn

  • in reply to ShawnLogan

    Dear ShawnLogan

    I have another question after simulating. page 20 of the note says "Select fullspectrum method. This option eliminates the need to tune the maxsidebands option", but simulation results are the same no matter that I use pnoisemethod=default or pnoisemethod=fullspectrum.

    I can't find the description about the relationship between "fullspectrum method" and  "maxsideband" in spectre manual.

    Thanks

Community Guidelines

The Cadence Design Communities support Cadence users and technologists interacting to exchange ideas, news, technical information, and best practices to solve problems and get the most from Cadence technology. The community is open to everyone, and to provide the most value, we require participants to follow our Community Guidelines that facilitate a quality exchange of ideas and information. By accessing, contributing, using or downloading any materials from the site, you agree to be bound by the full Community Guidelines.