spectremdl montecarlo simulations, how to fix my errors ?

What version of spectre are you using? (Type "spectre -W" in the UNIX command line).

Your example (or a slightly modified one) works fine for me - I used your MDL script with a separate design example, with a tran statement in the same as yours. I was using MMSIM12.1 ISR10 (but also tried a recent MMSIM11.1 version too).

Andrew.

Hello Andrew,

thanks for the quick feedback.

I am using :

...> which spectre

/home/.../cadence/MMSIM10_11/tools/bin/spectre

...> spectre -W

sub-version  10.1.1.181.isr12 

I am still investigating on my way.

P. 

OK, I have a kind of workaround. I am using straight spectre and not spectremdl, as follow :

I execute : mc_script_spectremdl.sh and I get the waveform results of my montecarlo simulations :

My current issue is to get the  mc simulation runs where the below export (written in the input.scs) is greater than a value (1 for example):

export aout_b_max=oceanEval("ymax(v(\"/aout_b\" ?result \"tran\"))")

Graphically, it's easy to put a "target" and then get the yield of the mc run, but I don't know how to do it in batch. 

I have the following files : 

mc_script_spectre.sh : 

#! /bin/csh -f 

spectre input.scs +log mc_log_file.log

input.scs :

// Generated for: spectre

simulator lang=spectre

global 0

include "models.scs"

parameters ...

subckt ncx ncx

ends ncx

// End of subcircuit definition.

subckt inv A1 YN vdd vnw vpw vss

parameters wp=xxx lp=xxx pfolds=1 wn=xxx ln=xxx nfolds=1

M5 (YN A1 vdd vnw) psvtlp w=wp*10e5 l=lp*10e5 nfing=pfolds mult=1 \

        srcefirst=1 mismatch=1 lpe=0 numcos=1 numcod=1 ngcon=1

M2 (YN A1 vss vpw) nsvtlp w=wn*10e5 l=ln*10e5 nfing=nfolds mult=1 \

        srcefirst=1 mismatch=1 lpe=0 numcos=1 numcod=1 ngcon=1

ends inv

...

M0 (aout aout_b vss vpw) nsvtlp w=wndiff l=lndiff nfing=1 mult=1 \

        srcefirst=1 mismatch=1 lpe=0 numcos=1 numcod=1 ngcon=1

...

include "./_graphical_stimuli.scs"

ic aout=1 aout_b=0 

simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=70.0 \

    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 

mc1 montecarlo numruns=50 seed=12345 variations=mismatch sampling=standard \

    donominal=yes scalarfile="../monteCarlo/mcdata" \

    paramfile="../monteCarlo/mcparam" savemismatchparams=yes \

    mismatchparamfile="../monteCarlo/mismatchparam" \

    mismatchscalarfile="../monteCarlo/mismatchdata" \

    dumpdependency=mismatch \

    dependencymapfile="../monteCarlo/mismatchdependency" \

    savefamilyplots=yes savedatainseparatedir=yes {

tran tran stop=20n 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

export saout_b_max=oceanEval("ymax(v(\"/aout_b\" ?result \"tran\"))")

}

mcOptions options genmcdep=yes

saveOptions options save=allpub subcktprobelvl=2 

-------------------------------------------------------------------

 I have the expected mc1_tran.tran waveforms :

...> ls input.raw/mc1_separate/

mc1-001/ mc1-003/ mc1-005/ mc1-007/ ...

...> ls input.raw/mc1_separate/mc1-001/

logFile                         mc1_element.info                mc1_modelParameter.info         mc1_primitives.info.primitives  mc1_tran.tran

mc1_designParamVals.info        mc1_finalTimeOP.info            mc1_outputParameter.info        mc1_subckts.info.subckts

However, I would like to get the mc simulation runs where the below export (writen in the input.scs) is greater than a value (1 for example):

export aout_b_max=oceanEval("ymax(v(\"/aout_b\" ?result \"tran\"))")

I would like to write in a result file this value. I think I should specify a result file in the spectre commandline (spectre input.scs +log mc_log_file.log) ?

Then, I would like to remove the useless files to get some disk space. How can I specify that I want to keep only the transeint result files and the result file with the export value ? 

Thanks.

P. 

Regarding the spectre method (and not the spectremdl  which doesnt work for some unknown reason, cf. above), I display the input.scs from the adexl window. 

At this time, I have the line :

export aout_b_max=oceanEval("ymax(v(\"/aout_b\" ?result \"tran\"))")

which corresponds to the graphical setting I did (meaning the yield, sigma... of the montecarlo runs will be based on a comparison of this aout_b_max and a spec value (not specified in the input.scs)).

I decide to use this input.scs to launch the montecarlo simu : spectre input.scs +log mc_log_file.log

And surprise, surprise, I have the above export in error :

*Error* _ymaxMethod: can't handle _ymaxMethod(nil)

Error found by spectre during Monte Carlo analysis `mc1'.

    ERROR (SPECTRE-8003): subckts: Error evaluating ocean expression

        `aout_b_max=ymax(v("/aout_b" ?result "tran"))'.

Unsuccessfully evaluated export statements (based on return code).

Analysis `mc1' was terminated prematurely due to an error. 

In graphical mode, the montecarlo runs occur very well using this input.scs, how it comes in batch mode I have this issue ?

The input.scs file I am using :

// Generated for: spectre

// Design library name: Test

simulator lang=spectre

global 0

include "corners_SS.scs"

parameters lndiff=...

subckt ncx ncx

ends ncx

// End of subcircuit definition.

subckt inv A1 YN vdd vnw vpw vss

parameters wp=xxx lp=xxx pfolds=1 wn=xxx ln=xxx nfolds=1

M5 (YN A1 vdd vnw) psvtlp w=wp*10e5 l=lp*10e5 nfing=pfolds mult=1 \

        srcefirst=1 mismatch=1 lpe=0 numcos=1 numcod=1 ngcon=1

...

I0 (aout net33 vdd vnw vpw vss) inv wp=xxx lp=xxx pfolds=1 wn=xxx \

        ln=xxx nfolds=1

...

Rright (vdd aout) resistor r=Rright

Rleft (vdd aout_b) resistor r=Rleft

M0 (aout aout_b vss vpw) nsvtlp w=wndiff l=lndiff nfing=1 mult=1 \

        srcefirst=1 mismatch=1 lpe=0 numcos=1 numcod=1 ngcon=1

...

include "./_graphical_stimuli.scs"

ic aout=1 aout_b=0 

simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=70.0 \

    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 

mc1 montecarlo numruns=1 seed=12345 variations=mismatch sampling=standard \

    donominal=yes scalarfile="../monteCarlo/mcdata" \

    paramfile="../monteCarlo/mcparam" savemismatchparams=yes \

    mismatchparamfile="../monteCarlo/mismatchparam" \

    mismatchscalarfile="../monteCarlo/mismatchdata" \

    dumpdependency=mismatch \

    dependencymapfile="../monteCarlo/mismatchdependency" \

    savefamilyplots=yes savedatainseparatedir=yes {

tran tran stop=20n 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

export aout_b_max=oceanEval("ymax(v(\"/aout_b\" ?result \"tran\"))")

}

mcOptions options genmcdep=yes

saveOptions options save=allpub subcktprobelvl=2 

Thanks & best regards !! 

Regarding the spectre method, I have the feeling I need the amap/ directory otherwise I have the error :

 *Error* _ymaxMethod: can't handle _ymaxMethod(nil)

Error found by spectre during Monte Carlo analysis `mc1'.

    ERROR (SPECTRE-8003): subckts: Error evaluating ocean expression

        `aout_b_max=ymax(v("/aout_b" ?result "tran"))'.

Unsuccessfully evaluated export statements (based on return code).

Analysis `mc1' was terminated prematurely due to an error. 

I found that doing the simulation in the adexl simulation database (.../xxxdesign_cell_namexxx/adexl/results/data/MonteCarlo.0/2/Test:xxxdesign_cell_namexxx:1/netlist/), whereas until now I was just simulating in a remote location.

...> ls amap/

__multiplefiles_amap_format__          __simulator_information__              cmosxxx_psvtlp_SimMosfetStandard.inst  xxxdesign_cell_namexxx.inst      ncx.inst                               top_level_map.net

__new_amap_format__                    analogLib_res_hspiceD.inst             inv.inst                               xxxdesign_cell_namexxx.net       ncx.net                                top_level_map.port

__nmp_amap_format__                    cmosxxx_nsvtlp_SimMosfetStandard.inst  inv.net                                xxxdesign_cell_namexxx.port      top_level_map.inst 

How it comes I cannot simulate without an error my input.scs with the export line : export aout_b_max=oceanEval("ymax(v(\"/aout_b\" ?result \"tran\"))") if I don't have the amap/ directory ? 

To my point, I should be able to launch the commandline : spectre input.scs +log mc_log_file.log with only :

_graphical_stimuli.scs

corners_SS.scs

global_flags.scs

input.scs

netlist

stat_flags.scs 

Thanks.

P. 

I'm out of the office today (and tomorrow), but will carefully read through your various posts and give more thought out answers, but to answer this issue with the amap directory - you only need that if you use schematic names for your signals. Because your expressions are using v("/aout_b") etc - the "/" at the beginning tells it that it's a "schematic" name rather than a "netlist" name. If you omit the leading "/" it will assume it's a netlist name (so you have to use "." as the hierarchy delimiter rather than "/" too) - and then the amap dir is not needed.

More when I have a chance to respond properly

Regards,

Andrew.

Hello Andrew,

thanks it works with this syntax modification, meaning launching graphically a 3 runs mc with the

export aout_b_max=oceanEval("ymax(v(\"aout_b\" ?result \"tran\"))")

I can then move to another directory, recreate/copy the input files I need and launch the simu for one of the 3 cases and I refind the /monteCarlo/mcdata value 

such as  (for example) :

more ../monteCarlo/mcdata

0.999954 

with the following lines in the input.scs :

...

mc1 montecarlo numruns=1 seed=12345 variations=mismatch sampling=standard \

    donominal=no scalarfile="../monteCarlo/mcdata" \

    savefamilyplots=yes savedatainseparatedir=yes firstrun=2 {

tran tran stop=20n 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

export saout_b_max=oceanEval("ymax(v(\"aout_b\" ?result \"tran\"))")

} 

... 

One notice :

It seems there is a bug in the scalarfile, because when I specify :  scalarfile="../monteCarlo/mcdata", the mc run will create the monteCarlo/mcdata file in the current directory (and not the specified directory).

Next step is to be able to launch the 3 mc runs and get the information (so it means global information) :

yield/min/target/max/mean/sigma

33/300m/900m/1000m/500m/600m (example) 

Does someone know what is the option for the montecarlo simu to get (in batch) the above global information on all (here just 3) the mc runs ?

The unix architecture is :

xxxDesign_Cell_Namexxx/adexl/results/data/MonteCarlo.1/

1/   2/   3/   psf/ 

Thanks.

P.