I tried to do monte carlo simulaiton in spectre. I succeeded with process variation simulation. But I failed with mismatch simulation. The simulation can complete successfully. But all the runs yield the same result without any mismatch. I am using TSMC018 CMOS design kit.

The model file is a binned model. It includes several processor corners defined like tt, ss, ff, sf, fs. I am only using the tt corner (typical case).


library tsmclib
section tt
....
parameters dvthn=0
parameters dvthp=0
...

statistics {
 mismatch {
   vary dvthn dist=gauss std=0.01
   vary dvthp dist=gauss std=0.01
 }
}

model nmos bsim3v3 {

1: lmin=xx, lmax=xx, vth0=0.4xx+dvthn,
....
2: lmin=xx, lmax=xx, vth0=0.4xx+dvthn,
...
3. lmin=xx, lmax=xx, vth0=0.4xx+dvthn,
...

}

model pnmos bsim3v3 {
...
vthp=0.4xx+dvthp
...
}

I put two identical NMOS transistors in the same schematic. Made 4 runs of monte carlo. I couldn't observe any mismatch of their operation points. The 4 runs yield identical operation points for both transistors.

Any tips will be greatly appreciated.

Thanks, paul. dvthn(p) are used for process corners. But I think it doesn't matter to use it for mismatch too. Anyway, I've tried using another parameter like vthmis and changing the equation for vth0 to be sth like

vth0=vthmis*(0.4xxx+dvthn).

But still no use.

By the way, the simulation result is the same from run to run if I choose "Mismatch Only" in monte carlo GUI window.


[quote author=Paul  link=1074804759/0#1 date=1074887862]Stephen,

the first thing you should not forget is that matching for MOS devices is size dependent, which is not the case in your file. Have a look at EVI's example in
http://www.designers-guide.com/Forum/?board=circuit;action=display;num=106670695...
Further more, I don't know your model file, but I would guess dvthn (and p) are used to calculate the corner values for VTH, so you should use a different parameter name for your mismatch simulations (again see EVI's example).

Regarding your problem, I don't know very well the detailed MC calculations performed by Spectre, but as you don't use subcircuits to interface the devices with the models, the simulator may calculate once per run the mismatch and apply the same mismatch to both devices. Does your simulation give different operating points from one run to the next?

Maybe EVI or BSIM4, doing these simulations with Spectre, can help here?

Paul [/quote]

You can also see an example of how to use inline subcircuits for mismatch analysis in Recommended Spectre Monte Carlo modeling methodology, which you can find at http://www.designers-guide.com/Modeling/.

- MM -