How transient operating point is calculated in cadence

Bit hard to read (probably you were using Chrome, which doesn't work well with the forum).

Anyway, my guess is that you're using spectre from IC5141, not from an MMSIM stream (in other words, a really old one). If using the old front end to spectre, you need to omit the quotes from the infoname value. i.e. put infoname=capInfo_dc rather than infoname="capInfo_dc" . If you miss out the quotes, it should work in IC5141 spectre and MMSIMXX. 

Using such an old version of spectre is not a good idea... it's not been touched in years.

Andrew.

Hi Andrew,

here is the new 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

Zfeng,

I just tried this with spectre from IC5141, and the problem is that spectre does not save the results correctly (the actual data seems to be missing). I ran in IC5141 with spectre from MMSIM10.1 - and then it all worked perfectly.

So the solution is to not use an (almost) 8 year old version of the simulator, but to use something more recent.

See this picture of printing the capacitance table in IC5141.

Andrew.

Zfeng,

Use Tools->Results Browser, and then expand the tran_info-tran_info results. You'll see results of the form "net1 : net2" (where the two may be the same - depends on the captab options you chose). If you click on these and expand, you'll see three entries Fixed, Total and Variable (say), and you can then either plot these or  send to the calculator. That might generate an expression such as:

 getData("net50 : net50:Fixed" ?result "tran_info-tran_info")

If you plot this, it will be versus the timepoints in your infotimes parameter.

The above was with wavescan as the waveform tool. If you're using AWD, you'd expand tran_info-tran_info and then click on sweepVariable, which will show "time". If you then click on one of the time points, and then go to the net pair name, click on that to see Fixed/Total/Variable, and then use the Middle Mouse button and pick "Expression" - you'll end up with an expression in the calculator such as:

 pv( "net62 : net62" "Total" ?result "tran_info-tran_info" ?resultsDir "/export/home/andrewb/demos/SpectreRF/simulation/ne600/spectre/schematic" )

(You could omit the ?resultsDir if it's the current results).

Either the pv() form or the getData() form will work in either calculator/waveform tool.

Regards,

Andrew.

 Hi Andrew,

    great, thanks a lot!