vsource voltage level always 1V, val0 & val1 missing in netlist

Hi Marten,

From "spectre -h vsource":

Pulse waveform parameters:
6       val0=0 V          Zero value used in pulse and exponential waveforms.
7       val1=1 V          One value used in pulse and exponential waveforms.

You have not specified val0 and val1 (the low and high voltages) and so the defaults are being used. The dc value only affects a dc analysis, not the transient analysis. If dc is not specified, then the time=0 value is used for any DC analysis.

Regards,

Andrew.

Hi Andrew,

thanks for your reply. Since I want to run a dc and a transient analysis in the same testbench, I do have specified the voltage 0 and voltage 1 inside the testbench schematic:

And this is an excerpt of the generated netlist:

I0 (A B OUT 0 gnds! vdd! vdds!) NAND2_X1
V5 (A 0) vsource dc=300m type=dc delay=0 period=5u rise=10n fall=10n \
        width=2.5u
V1 (B 0) vsource dc=300m type=pulse delay=-1.25u period=5u rise=10n \
        fall=10n width=2.5u
C0 (OUT 0) capacitor c=4f ic=0
V3 (vdd! 0) vsource dc=v_vdd type=dc
V2 (vdds! gnds!) vsource dc=v_vdds type=dc
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \
    tnom=25 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 \
    digits=5 cols=80 pivrel=1e-3 sensfile="../psf/sens.output" \
    checklimitdest=psf
dc dc dev=V1 param=dc start=0 stop=300m step=0.001 write="spectre.dc" \
    oppoint=rawfile maxiters=150 maxsteps=10000 annotate=status
tran tran stop=5u write="spectre.ic" writefinal="spectre.fc" \
    annotate=status save=all maxiters=5
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
saveOptions options save=allpub subcktprobelvl=2

So why is V1 generated without val0, val1?

I suspect you're using an analogLib which isn't from Cadence. The vsource component in our analogLib doesn't have parameters v1E or v2E - maybe this is for another simulator (Eldo?).

Can you check the path to your analogLib - perhaps you can change to use a Cadence-supplied version.

Alternatively, you might be able to use Options->Tool Filter to ensure that parameters relevant for spectre rather than the other simulator are shown?

Regards,

Andrew.

Hey Andrew,

thanks a lot! Our cds.lib sourced some other .lib-Files, that redefined the analogLib and used ELDOs libs instead.
 I fixed this and now simulation is running as expected, thank you.

Cheers,

Marten