Wow, that's a nifty test case, only 2 elements and you get an assertion failure.  Send it in to tech support!

At this moment, my hypothesis is that my problem arises from a model file that is not sufficiently compatible with the simulator.

This is my netlist. I cannot include the model file here.

// Generated for: spectre
// Generated on: May 24 17:08:40 2006
// Design library name: adc
// Design cell name: testtnoise
// Design view name: schematic
simulator lang=spectre
global 0
include "/misc/icetux6/cadappl/ictools/cadence_ic/5.1.41.USR2/tools/dfII/samples/artist/
ahdlLib/quantity.spectre"
include "/misc/icetux6/cadappl/iclibs/CMOS090/PcCMOS090T6M1TPTP/3.1/lib/CMOS090T6M1T/../
../tools/models/LP_50A/mm11/spectre/c1/include_nominal.scs"

// Library name: adc
// Cell name: testtnoise
// View name: schematic
MN0 (net09 net016 0 0) nsvt w=0.12 l=0.1 nfing=1 mult=1 srcefirst=1 \
       mismatch=1
V0 (net016 0) vsource dc=1 type=dc
V1 (net11 0) vsource dc=1.2 type=dc
R1 (net11 net09) resistor r=1K
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \
   tnom=27 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
tran tran stop=10n errpreset=moderate noiseseed=1 noisefmax=10G \
   noisescale=1 write="spectre.ic" writefinal="spectre.fc" \
   annotate=status 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

Bernd,

  You are correct, in general it is best to let Cadence support deal
with the issue.

Michiel,

  Are the units of length and width correct? If I remember correctly
since the units of scale are set to 1, the gate length is 0.1m and the
gate width is 0.12m. Extremely large device sizes can cause the
simulator to fail. If updating l and w does not fix the issue, then
it would be best to contact Cadence support.

                                                         Best Regards,

                                                            Sheldon

Michiel -
I think Sheldon is correct, that the netlist as you provided specifies the dimensions in meters, not um.

Could you try changing it to
MN0 (net09 net016 0 0) nsvt w=0.12e-6 l=0.1e-6

Also, from the path you showed, models/LP_50A/mm11: does this use Mos Model 11 from Philips?


I still think you should send this in to Cadence support, because the assertion failure indicates some serious problem down in the code -- possibly with the SimKit code from Philips that is used to evaluate the MM11 model.

Michiel wrote on May 31^st, 2006, 10:21am:


OK, perhaps the model card is set up to convert to um.

Quote:


Can you figure out which MOS11 it uses?  The possibilities are mos1100, mos1100e, mos1101e, mos1101et, mos1102e, mos1102, ... mos11021t.

I just set up a test case with mos11011
model nsvt mos11011
which then uses the default parameters for the model, and I didn't see any problems.

If you can copy the model file to your local directory, you might try deleting half of the parameters and then seeing if it still errors out.  Or deleting the noise parameters (ponfa, plnfa, ...) and seeing if that is the issue.

With mos11021, the noise parameter nfa is computed from ponfa, pwnfa, plnfa, pwlnfa.  I wonder if it ends up having a negative value after the scaling rules are applied.

In my simulator, I get a warning that the value is outside the range, and nfa is clipped to zero.  If nfa is not clipped, you might get a negative number in a square root.