Stats

  • Locked Locked
  • Replies 7
  • Subscribers 65
  • Views 10094
  • 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 from ADE assembler does not work as explained in cadence support website

NewScreenName

Hi,

I am trying to get the noise summary of a noise/pnoise simulation to be automatically plotted, or at least to be like any other output waveform where I could just double click after the simulation and have it to pop up without having to do for every simulation/corner the procedure RMB, print noise summary, enter which devices to include, which integration limits etc.

I have followed the instructions given here: https://support.cadence.com/apex/ArticleAttachmentPortal?id=a1Od0000007MViHEAW&pageName=ArticleContent 

However, it seems to me that this is just creating a noisesummary directory, and stores there the results. When the simulation finishes it will plot automatically the instances noise vs frequency (for those instances where I explicitly defined the output like (ocnGenNoiseSummary(1 ?result 'noise) && getData("R0:total" ?result "noisesummary")).

However if my test is called noise_summary_1, I noticedthat upon double-click on (ocnGenNoiseSummary(1 ?result 'noise) && getData("R0:total" ?result "noisesummary")) nothing will be plotted (and it seems to be because it tries to retrieve the data from directory ./noise_summary/maestro/results/maestro/Interactive.0/psf/noise_summary_1/psf rather than from ./noise_summary/maestro/results/maestro/Interactive.0/1/noise_summary_1/psf. How to fix this? 

Also, according to what I understood this should have allowed me to get directly a form like the one in picture below, as also it seems like me the output noiseSummary('integrated ?result "noise" ?from 1000 ?to 100000 ?output "./integ_noise.txt" ?hierLevel 1 ?deviceType 'all ?noiseUnit "V^2") has all the required information to do that

but after simulation it just shows an empty row in the output tab

Have I misunderstood it, or should I be able to automatically get a tab like the one from the first picture I posted? And if so, which steps am I making wrong here?

In case it was useful information, this is the netlist:

virtuoso version:

Thank you very much

Best regards

Parents

  • Dear NewScreenName,

    NewScreenName said:
    I am trying to get the noise summary of a noise/pnoise simulation to be automatically plotted,
    NewScreenName said:

    I have followed the instructions given here: https://support.cadence.com/apex/ArticleAttachmentPortal?id=a1Od0000007MViHEAW&pageName=ArticleContent 

    However, it seems to me that this is just creating a noisesummary directory,

    There are two sets of instructions from my interpretation of your reference.

    The first uses the ocean command noiseSummary() and writes the requested noise summary (i.e., integrated or spot) to a filename you specify or a port (i.e., a file you opened with the command outfile() and will eventually close with the close() command). This command does not display the data written to the file nor the port to the display.

    The second uses the ocean ocnGenNoiseSummary() command which writes the noise summary for a given hierarchy level you specify to the current results directory. It will write it in a format that is recognized by ViVA and hence will appear in the Results Browser. As such, it will be written to the directory Interactive.X/<test_name>/psf and not the individual subdirectories of Interactive.X/<test_name>/<simulation_number>.

    NewScreenName said:
    Also, according to what I understood this should have allowed me to get directly a form like the one in picture below, as also it seems like me the output noiseSummary('integrated ?result "noise" ?from 1000 ?to 100000 ?output "./integ_noise.txt" ?hierLevel 1 ?deviceType 'all ?noiseUnit "V^2") has all the required information to do that
    NewScreenName said:
    but after simulation it just shows an empty row in the output tab

    Neither of these options, in my understanding, will write a noise summary in a display window following a simulation. For that, you might consider writing a SKILL script or a UNIX shell script to run at the end of your simulation. The command you included in your post writes the information to the file "./integ_noise.txt" as it is specified to do and hence it makes sense there is an "empty row" in the output tab line for the output.

    NewScreenName said:
    However, it seems to me that this is just creating a noisesummary directory, and stores there the results.

    Yes. This is what the command documentation indicates.

    Shawn

Reply

  • Dear NewScreenName,

    NewScreenName said:
    I am trying to get the noise summary of a noise/pnoise simulation to be automatically plotted,
    NewScreenName said:

    I have followed the instructions given here: https://support.cadence.com/apex/ArticleAttachmentPortal?id=a1Od0000007MViHEAW&pageName=ArticleContent 

    However, it seems to me that this is just creating a noisesummary directory,

    There are two sets of instructions from my interpretation of your reference.

    The first uses the ocean command noiseSummary() and writes the requested noise summary (i.e., integrated or spot) to a filename you specify or a port (i.e., a file you opened with the command outfile() and will eventually close with the close() command). This command does not display the data written to the file nor the port to the display.

    The second uses the ocean ocnGenNoiseSummary() command which writes the noise summary for a given hierarchy level you specify to the current results directory. It will write it in a format that is recognized by ViVA and hence will appear in the Results Browser. As such, it will be written to the directory Interactive.X/<test_name>/psf and not the individual subdirectories of Interactive.X/<test_name>/<simulation_number>.

    NewScreenName said:
    Also, according to what I understood this should have allowed me to get directly a form like the one in picture below, as also it seems like me the output noiseSummary('integrated ?result "noise" ?from 1000 ?to 100000 ?output "./integ_noise.txt" ?hierLevel 1 ?deviceType 'all ?noiseUnit "V^2") has all the required information to do that
    NewScreenName said:
    but after simulation it just shows an empty row in the output tab

    Neither of these options, in my understanding, will write a noise summary in a display window following a simulation. For that, you might consider writing a SKILL script or a UNIX shell script to run at the end of your simulation. The command you included in your post writes the information to the file "./integ_noise.txt" as it is specified to do and hence it makes sense there is an "empty row" in the output tab line for the output.

    NewScreenName said:
    However, it seems to me that this is just creating a noisesummary directory, and stores there the results.

    Yes. This is what the command documentation indicates.

    Shawn

Children
No Data

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.