how to simulate the variation(just like CORNERS for the MOS) of capacitor in HSPICE?

[allennlowaton]

Good day EDA fellows,

I would like to ask on how to simulate the process variation of the MIMcapacitor.
In MOS, we have the corner simulation but I don't know about the capacitors.
Thank you.

 

[amwygah]

It also have corner for capacitors. for example: max_capacitor tt_capacitor min_capacitor

 

[allennlowaton]

thanks amwygah..
But I don't know how to do it in HSPICE...

 

[amwygah]

you need firstly to confirm that such corner exit in your model library .
If they are there, then you can just put them together like this:

.LIB 'XXX.LIB' TT
.LIB 'XXX.LIB' max_capacitor

you can try it.

 

[dick_freebird]

In the days before CAD was a specialty, we used to just embed
"k" variables in the model files and run nested loops to shotgun
the process corners.

LOOP kmim FROM 0.8 TO 1.2 BY 0.2
LOOP krpoly FROM 0.8 TO 1.2 BY 0.2
LOOP kvtn FROM 0.8 TO 1.2 BY 0.2
LOOP kvtp FROM 0.8 TO 1.2 BY 0.2
LOOP ktox FROM 0.8 TO 1.2 BY 0.2
{run your sim}
{crunch your data}
{spit it out}
ENDLOOP
ENDLOOP
ENDLOOP
ENDLOOP
ENDLOOP

Your syntax surelay varies, as may the willingness of your
simulator to support a command language. But it's doable
with shell scripts too.

 

[Teddy]

if you have netlist for Hspice there will be a call for the model libraty i.e. models_TT or so.
If you found that you have corner models for MOSFETs it probably is something like models_SS no?
So if you have models for min and max capacitors you just call the correct models for the caps.
If you do not have corner models for the caps - copy the section for mim cap Typical model and change the mim value +/-20% - that will be close enough to real corner spread, rename this block and use it in your model call.