Stats

  • Locked Locked
  • Replies 27
  • Subscribers 127
  • Views 32402
  • 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

  • Hello, Andrew

    Thanks a lot. I may want to see how this will be fixed in the future.

    Regards,

  •  Hi Andrew,

         as you said above, i have tried but i failed to sample the certain port capacitance to a  file, in fact , i want to sample the output node capacitance versus time, i had a careful study of the "captab" and "info" function, but i didn't find any parameter which can let the user to specify a node, now i just can sample the whole circuit nodes capacitance versus, but i care only about the output node, do you have any suggestion?

    regards,

    zhenfu

  •  You can't output the captab just for one node. If you're asking how to save it to an ASCII file, you can create an include file myCaptab.scs

    mycaptab info what=captab where=file 

    and then reference this file from the Setup->Model Libraries. You can add any other captab related options (see "spectre -h info")). Then don't turn on captab on the DC analysis form (you can if you like, but it will add a second captab output which will generate a rawfile). You can reference mycaptab in the infonames  field on transient if you want it to run just at a certain time, see my previous post on this.

    Andrew.

  •  Hi Andrew,

         thanks for your reply, as you said we can't save the capacitance only for one node, so commonly, how people to monitor the node capacitance's changes versus time during the transient simulation? in another word, how can i know a node capacitance when i performed a transient simulation except the captab function? do you have some idea?

    regards,

    zhenfu

  • So why is the infotimes approach that I've suggested not OK - is that not enough granularity for you? You should be able to plot it from the results browser (I think) if you use the original approach I suggested.

    Andrew
  • Hi Andrew, sorry for asking the same question again, but i can't still solve my problem. i have enabled the captab in DC analysis, and i also follow your instruction to add the additional parameters in the transient analysis option form, but i met an conflict error when i try to do the simulation, so i want to make sure about some points, 1, just enable the captab in dc analysis? 2,do not enable the captab in transient analysis, but add the additional parameters 3,perform both analysis at the same time? regards, zfeng

  • Zfeng,

    You should just be able to do the steps I mention here. You need to enable the captab in the DC analysis, and then fill in the additional parameters field on the transient analysis as I mentioned in step 2 of the reply I linked to.

    You didn't say what the "conflict error" was, so it's hard to know what your problem actually is.

    Kind Regards,

    Andrew.

     

  • Hi Andrew, here is the error: Error found by spectre during hierarchy flattening. tran: Component analysis name expected for parameter `infoname'. name conflict: value `capInfo_dc' of type `scalar instance' encountered. Expected value is of type `scalar analysis'. by the way, i didn't find the capInfo_dc in the results, regards, zfeng

  • Please post the bottom part of your input.scs when you're getting this error (everything from the bottom of the circuit onwards - i.e. all the options and analysis statements).

    Andrew.

  • Hi Andrew,

         here is the analysis statements:

        simulatorOptions options reltol=100e-6 vabstol=1e-6 iabstol=1e-12 temp=27 \
        tnom=27 homotopy=all limit=delta scalem=1.0 scale=1.0 \
        compatible=spice2 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 digits=5 \
        cols=80 pivrel=1e-3 ckptclock=1800 sensfile="../psf/sens.output" \
        checklimitdest=psf
    dcOp dc write="spectre.dc" save=all maxiters=150 maxsteps=10000 \
        annotate=status
    capInfo_dc info what=captab where=logfile threshold=0.0 detail=node \
        sort=name
    dcOpInfo info what=oppoint where=rawfile
    tran tran stop=30m errpreset=conservative step=1n ic=dc write="spectre.ic" \
        writefinal="spectre.fc" annotate=status save=all oppoint=rawfile \
        maxiters=5 infoname="capInfo_dc" infotimes=[3m 7m 11m]
    finalTimeOP info what=oppoint where=rawfile
    modelParameter info what=models where=rawfile
    element info what=inst where=rawfile
    outputParameter info what=output where=rawfile
    designParamVals info what=parameters where=rawfile
    primitives info what=primitives where=rawfile
    subckts info what=subckts  where=rawfile
    save MCOLUMNAMP:d MCOLUMNAMP:g Pixel0.MSELECT:d Pixel0.MSELECT:s
    saveOptions options save=all currents=selected 

    could you see it clearly now?

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.