Stats

  • Locked Locked
  • Replies 7
  • Subscribers 125
  • Views 15453
  • 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

Why OCEAN script produce different analysis result from ADE?

datao

Hi,

I uses a scripts to analyze phase noise of a VCO at different control voltage. I found some data points are significantly different from ADE produced. Then I saved script in ADE and load the script in ocean. The phase noise calculated with ocean script is -80. But at ADE, it is -100. Anyone can tell me how to solve this problem? Thanks! The save script is attached as below. The frequency calculated are consisten, but phase noise are different from ocean script.

 

 ocnWaveformTool( 'wavescan )
fp=outfile(sprintf(nil "%s/tmp.csv" resultPATH) "a")
fprintf(fp "vc ts cf wc freq amp vcom phasenoise\n")

simulator( 'spectre )
design(     "/users/dtgong/simulation/testLCVCO/spectre/schematic/netlist/netlist")
resultsDir( "/users/dtgong/simulation/testLCVCO/spectre/schematic" )
modelFile(
    '("/home/dtgong/peregrine/PSC_Release_3.8.1/Rel_3.8.1/gc/models/psa/spectre/modellib.scs" "Nominal")
)
analysis('tran ?stop "200n"  ?errpreset "conservative"  )
analysis('pnoise ?sweeptype "relative"  ?relharmnum "1"  ?start "10K"  
        ?stop "100M"  ?maxsideband "7"  ?p "/vp0"  ?n "/vn0"  
        ?oprobe ""  ?iprobe ""  ?refsideband ""  ?ppv ""  )
analysis('pss ?fund "5.0G"  ?harms "7"  ?errpreset "conservative"  
        ?tstab "500n"  ?p "/vp0"  ?n "/vn0"  ?ppv ""  )
desVar(      "wc" 30u    )
desVar(      "wb" 10u    )
desVar(      "cf" 220p    )
desVar(      "r" 10    )
desVar(      "global_use_preLPE" 1    )
desVar(      "vc" 1.1    )
desVar(      "cl" 60f    )
envOption(
    'autoDisplay  nil
)
save( 'i "/I0/I0/R0/MINUS" "/I0/I0/L0/PLUS" "/I0/I0/L1/PLUS" )
converge( 'ic "/vn0" "0.01" )
temp( 27 )
run()
selectResult( 'tran )
;plot(getData("/vp0") getData("/vn0") getData("/I0/vb") getData("/I0/I0/R0/MINUS") getData("/I0/I0/L0/PLUS") getData("/I0/I0/L1/PLUS") getData("/I0/I0/vtail") )
freq = frequency(clip((VT("/vp0") - VT("/vn0")) 1e-08 4e-08))
;plot( freq ?expr '( "freq" ) )
Phase\ Noise\;\ dBc\/Hz\,\ Relative\ Harmonic\ \=\ 1 = phaseNoise(1 "pss_fd" ?result "pnoise")
;plot( Phase\ Noise\;\ dBc\/Hz\,\ Relative\ Harmonic\ \=\ 1 ?expr '( "Phase Noise; dBc/Hz, Relative Harmonic = 1" ) )
ph_1M = value(phaseNoise(1 "pss_fd" ?result "pnoise") 1000000.0)
;plot( ph_1M ?expr '( "ph_1M" ) )
;freq0 = (freq (VT("/vp0") - VT("/vn0")) "rising" ?xName "time" ?mode "auto" ?threshold 0.0 ?histoDisplay nil ?noOfHistoBins nil)
;plot( freq0 ?expr '( "freq0" ) )
fprintf(fp "%.3fGHz %f\n"  freq*1e-9 ph_1M)
close(fp)

 

Thanks a lot,

 

Datao

 

Parents

  • Hi Datao,

    When you hit the run button the second time, spectre will be re-running from what is in memory. It's possible that you have multiple operating points and your circuit is converging on a different solution after the first run.

    In order to find out the spectre version - this will appear at the top of the spectre output log, and also "spectre -W" will tell you from the UNIX command line - but I'd check the log file.

    You can also try setting "rebuildmatrix=yes" on the Simulator->Options->Analog form (if it's not on the form, type it in the additional parameters field). That said, if there is more than one operating point, maybe you need to investigate that. Perhaps you can check if the PSS simulation is finding the same oscillation frequency the first and second time you run it in ADE? It should tell you at the end of the PSS simulation what the final oscillation frequency is (and you can get this on the direct plot form too) - maybe it's converged on a different solution for the oscillation frequency?

    Regards,

    Andrew.

Reply

  • Hi Datao,

    When you hit the run button the second time, spectre will be re-running from what is in memory. It's possible that you have multiple operating points and your circuit is converging on a different solution after the first run.

    In order to find out the spectre version - this will appear at the top of the spectre output log, and also "spectre -W" will tell you from the UNIX command line - but I'd check the log file.

    You can also try setting "rebuildmatrix=yes" on the Simulator->Options->Analog form (if it's not on the form, type it in the additional parameters field). That said, if there is more than one operating point, maybe you need to investigate that. Perhaps you can check if the PSS simulation is finding the same oscillation frequency the first and second time you run it in ADE? It should tell you at the end of the PSS simulation what the final oscillation frequency is (and you can get this on the direct plot form too) - maybe it's converged on a different solution for the oscillation frequency?

    Regards,

    Andrew.

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.