Stats

  • Locked Locked
  • Replies 12
  • Subscribers 126
  • Views 11939
  • 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

Print Noise Summary after "ANALYSIS DURING TRAN"

msharma

Hi,

I need to simulate the noise of my circuit at specific points in time after transient analysis. For this I use the "ANALYSIS DURING TRAN", (analysis->tran->options-?output->"ANALYSIS DURING TRAN"). I specifiy a time in actimes, and specify acnames = noise. The analysis runs successfully. However, I am unable to use the "Print Noise Summary" feature. When choosing Print Noise Summary, no dialog pops up, just an empty result window.

How can I use the "Print Noise Summary" feature when running noise analysis at specific tran points?

Thanks,

Mohit

  • Hi Mohit,

    Which IC version are you using? In IC616 and IC617 (at least the latest ISRs which I have on my laptop) I get this:

    Regards,

    Andrew

  • Hi Andrew,

    Thanks for the quick reply. I am also using version 6.1.6-64bit(500.1), so it is strange, but I don't get the similar dialog. Also, if I run an stb or ac at actimes, I can't plot the results from "Results"->"Direct Plot". I have to use the "Results Browser". (Not a problem when I run these analylses the ususal (dc operating point) way).

    Mohit
  • Hi Mohit,

    Because I see this question a lot - and there's quite a bit of confusion around the topic of "transient noise summary", I wanted to bring this up. If you have access to http://support.cadence.com please see Article 11793398.


    Note that you can't get a transient noise contribution summary. The noise contribution summary is only possible in the Spectre small signal noise analyses (AC noise, hbnoise, pnoise).

    You may have heard that you can run ac noise at every time point during transient analysis and use the transient solution vector instead of the dc operating point bias. However, this is not equivalent to the device contributions in transient noise analysis and there is no way to calculate transient noise device contributions from this data. Because noise is modulated by varying the bias, and the noise correlations between the current time point and all previous time points must be accounted for. This is feasible when the circuit behavior is periodic (pss/pnoise, hb/hbnoise) and in steady state conditions.

    => Use the noise_on and noise_off options to find out how a particular device or sub circuit affects transient noise output.

    
    Now, if you are only interested in printing the noise summary at specific times in a transient analysis, you can use the "actimes" and "acnames" option. (This is essentially what you are doing currently, I believe).

    It will give you some time-dependent noise contributions, but it is very important to understand that this does NOT give the same results as transient noise.

    Best regards,
    Tawna

  • Hi Tawna,

    Thanks for clarifying a potential confusion in terminology (looks like I don't have access to the support portal). However, I am not running transient noise analysis. I am simply running noise (and stb and ac) analyses at specific timepoints. All I am interested in is small signal behaviour once the circuit is in a steady state. Thus, I use acnames, and actimes feature of the tran analysis. However, the analysis results are not accessible through "Results" menu in ADE. They are only accessible through "Results Browser" (e.g. "Results"->"Direct Plot"->"Equivalent Output Noise" doesn't plot anything, and CIW logs "*Warning* no noise results, can't plot equivalent output noise.").

    That works for most of my needs. But when trying to sort noise contributions, I need to use the "Results"->"Print"->"Noise Summary". Is it possible to understand why the small signal results are not available with the actimes feature?

    Thanks,
    Mohit

  • Hi Mohit,
    I am able to Results-Print-noise summary when using transient with acnames/actimes.
    I'm not sure why you aren't able to. You might want to open a Case with Customer Support to look into this.

    best regards,
    Tawna

  • I don't think this is something that has been implemented recently - certainly I didn't find anything that suggested that when I did a search. I'm on a plane so can't test some older versions such as ISR1 of IC616 that you're using. It's possible that there may have been a bug then or in the MMSIM version you're using (what is that? It should be shown near the top of the spectre output log file).

    I'll do some checks on this and the stb analysis once I'm back in the office - but it would be useful to know the MMSIM version to help correlate.

    Thanks,

    Andrew

  • Hi Andrew,

    From the spectre log, the MMSIM version is: 13.11.176 (Linux).

    Thanks for helping track this down.

    Mohit

  • Hi Tawna,

    OK thanks for checking. I will look into contacting customer support. Just FYI, I don't have direct knowledge of our license numbers etc., which is taken care by the computing support.

    Mohit

  • Hi Mohit,

    The problem is due to the version of MMSIM13.1 you're using. Doing some experiments with IC616 ISR1 (the version you're using), and MMSIM131 ISR9 (the version you're using), I see the problem. I see that it first broke in MMSIM131 ISR8 (13.1.1.117.isr8) and was working again in MMSIM131 ISR14 (13.1.1.420.isr14). It's possible that it was fixed in ISR13 too - I don't have that version lying around to test. This fixed version is about 2 years old, so using something more recent makes sense.

    There was clearly a difference in how the results were presented which causes the problem.

    You may be able to workaround this by using the noiseSummary function instead in the CIW. After simulation, check what sweep values you have (these should be the times):

    selectResult("tran_noise-tran_noise")
    sweepValues()

    In my case I get: (1.3e-06 1.9e-06)

    Then I can do:

    noiseSummary('spot ?result "tran_noise-tran_noise" ?frequency 1k ?paramValues list(1.9e-6))

    noiseSummary('integrated ?result "tran_noise-tran_noise" ?from 1k ?to 1G ?paramValues list(1.3e-6))

    noiseSummary('integrated ?result "tran_noise-tran_noise" ?from 1k ?to 1G ?paramValues list(1.3e-6) ?output "noiseSummary.txt")

    The ?paramValues needs to be one of the times you had from the sweepValues() call.

    The problem seems to be with this range of MMSIM versions that the results are called "tran_noise-tran_noise" and are not picking up the "aliased" name of "noise" which is what the noise summary form is expecting. By calling the underlying OCEAN (SKILL) function, you can tell it the result result name.

    Regards,

    Andrew.

  • Hi Andrew,

    Thanks for figuring out the issue. Regarding version upgrade, I will check with the computing support. The OCEAN code is very useful. However, the only output from noiseSummary function is "t". If a filename is given, the function does not create that file. To debug, I broke the function by giving bad parameters, and there were reasonable error messages. I also plotted the noise PSD from the CIW window to make sure that there is data from the simulation.

    What might be wrong here?

    Thanks,

    Mohit

    PS: I had a suspicion that the problem is in the names of result files. And, I renamed the tran_noise.tran_noise file to noise.noise. But that had not solved the issue. I guess there is a little more indirection while accessing the results..

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.