Stats

  • Locked Locked
  • Replies 27
  • Subscribers 127
  • Views 32400
  • 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 transient operating point is calculated in cadence

prashu

 When performing transient analysis with cadence my input is changing and accordingly its operating point should change but when i see its transient operating point than it only show one region throughout the transient analysis please expalin

  •  Hi prashu,

        have you solved your problem? it seems that a dc analysis should be excuated before the transient analysis. and the transient operation point should be a fixed point, the same meaning with the DC point. i don't know how to observe the operation region during the simulation either, but i suggest you to annotate the transient node voltage, and you can calculate it by hand. any way, you can know the transistor operation mode by this way, i hope this will be helpful.

    regards,

    zfeng

  • Normally the transient operating point is showing you the final operating point at the end of the simulation - this is if you have "Save Final Op Pt" enabled on the Transient Options Form.

    Additionally you can fill in "infotimes" on the Transient Options form to say which times you want it to output a full operating point. If you do this, you'll then get a choice when you annotate the transient operating points as to which one you wish to annotate.

    Regards,

    Andrew.

  •  Hi,

        yes, what andrew has said is right, you can set some "time info" in the option form. by the way, i notice there is also a "captab" option, can i save the "capinfo" -capacitance of any node into a file? if not, how can i monitor a node capacitance changes versus time?

    regards,

    zfeng

  • Zfeng,

    Spectre itself can do this - you would specify the infoname parameter on the tran analysis to whatever you've called the info analysis with what=captab. However, support for doing this through ADE is limited. You can do this:

    1. Enable captab on your DC analysis
    2. On the transient analysis, fill in the Additional Parameters field on the options form to be:
      infoname="capInfo_dc" infotimes=[1n 2n]
    3. Don't fill in the infotimes field (actually you can, but then you get a potential conflict as there will be two infoname parameters on the tran analysis line, so probably not a good idea, and then the results post-processing doesn't work).

    Interestly you can then use Results->Print Capacitance Table and choose which time to show. You can also access the data in the results browser and plot the capacitances versus the times specified in the infotimes.

    Regards,

    Andrew.

  • Hello, Andrew.

     I followed above steps you talked and it woks fine at the firtst time.

     It failed when I tried to do another other simulation. The error message

    shows the following

    Warning from spectre at time= 10us during transient analysis 'tran'

    Warning: The analysis 'info-captab'  is not supported in infoname in this mode.

    Hope you can give me something to fix it.

    Regards,

    Richard

  • Richard,

    Please post the analysis statements (everything at the bottom of the netlist, from the options onwards) in your input.scs file - that way I can see what the setup is.

    Thanks,

    Andrew
  • Andrew

    I guess the previous problem is caused by APS because the problem is gone when I switched APS to spectre. I think that the info-captab is not supported by APS.

    Thanks for your quick reply.

    Richard.
  • Richard,

    Really? Which version of spectre/APS are you using? (It will be at the top of the output log from spectre).

    I'll check when I get into the office, but please let me know the version you're using too.

    Thanks,

    Andrew
  • Andrew

    The version is probably 10.1.1.218. I lost capInfo_dc when selecting APS.
    Thanks

    Richard

  • Richard,

    I've reproduced the problem - it's there in MMSIM11.1 too. I suspect it's an oversight, so I've filed CCR  972106 to address this.

    If  you want visibility of the CCR and when this will be fixed, you should log a service request with customer support for this issue, and then the AE can file a duplicate of that CCR (please reference this discussion on the forum).

    Regards,

    Andrew.

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.