spectre_model_file

hello sir,

thanks for your reply,as u asked about the model file i have written
them below which are added during my spectre simulation.and the
warnings that i got are also added for your kind perusal.

MODEL FILE:

nmos: level=3 nsub=7.16e+16 tox=200 uo=511 xj=0.5u rsh=236 theta
=61.28m
+lmlt=1 xl=-0.05u ld=0.1u wmlt=1 xw=0.8u wo=0.45u vto=0.815 delta=1.24
gamma=0.681 eta=19.25m
+wic=1 nfs=3.10e+11 vmax=160k kappa=0 tlev=1 bex=-1.6 tcv=-1.2m
capop=2 acm=2 cj=350u
+mj=0.43 cjsw=450p mjsw=0.43 pb=0.675 cgdo=310p cgso=310p js=2u

pmos: level=3 nsub=1.00e+18 tox=200 uo=156.7 xj=0.1u rsh=207
+theta =0.1132 lmlt=1 xl=0.098u ld=0.1u wmlt=1 xw=0.78u wo=0.45u
vto=-1.05
+delta=0.734 gamma=0.671 eta=50m
+wic=1 nfs=1.00e+10 vmax=500k kappa=20 tlev=1 bex=-1.6 tcv=1.7m
cj=540u
+mj=0.51 cjsw=760p mjsw=0.51 pb=0.7 cgdo=300p cgso=300p js=10u


WARNINGS:

Warning from spectre during circuit read-in.
`itin': `lmlt' is not a valid parameter for `mos3' models.
`itin': `wmlt' is not a valid parameter for `mos3' models.
`itin': `wo' is not a valid parameter for `mos3' models.
`itin': `wic' is not a valid parameter for `mos3' models.
`itin': `capop' is not a valid parameter for `mos3' models.
`itin': `acm' is not a valid parameter for `mos3' models.
`itip': `lmlt' is not a valid parameter for `mos3' models.
`itip': `wmlt' is not a valid parameter for `mos3' models.
`itip': `wo' is not a valid parameter for `mos3' models.
`itip': `wic' is not a valid parameter for `mos3' models.

Sir, itin and itip are the model name that i have given to the
transistors nmos and pmos respectively in my schematic.i think mos3
models are the executables within spectre,in which the above
parameters are not defined.

kindly help me to get rid of the warnings.

regards

selvakumar

 

Selvakumar:
Your model file was not in spectre format. I put it in spectre format
as follows:
1. create model.l and copy your model into it
2. make sure the first line is empty
3. change nmos: to .model nmos nmos
change pmos: to .model pmos pmos
4. spp -convert <model.l> model.scs

The resulting file is:

//
simulator lang=spectre insensitive=yes
model nmos mos3 type=n
+ nsub=7.16e+16 tox=200 uo=511
+ xj=0.5u rsh=236 theta=61.28m
+ lmlt=1 xl=-0.05u ld=0.1u
+ wmlt=1 xw=0.8u wo=0.45u
+ vto=0.815 delta=1.24 gamma=0.681
+ eta=19.25m wic=1 nfs=3.10e+11
+ vmax=160K kappa=0 tlev=1
+ bex=-1.6 tcv=-1.2m capop=2
+ acm=2 cj=350u mj=0.43
+ cjsw=450p mjsw=0.43 pb=0.675
+ cgdo=310p cgso=310p js=2u

model pmos mos3 type=p
+ nsub=1.00e+18 tox=200 uo=156.7
+ xj=0.1u rsh=207 theta=0.1132
+ lmlt=1 xl=0.098u ld=0.1u
+ wmlt=1 xw=0.78u wo=0.45u
+ vto=-1.05 delta=0.734 gamma=0.671
+ eta=50m wic=1 nfs=1.00e+10
+ vmax=500K kappa=20 tlev=1
+ bex=-1.6 tcv=1.7m cj=540u
+ mj=0.51 cjsw=760p mjsw=0.51
+ pb=0.7 cgdo=300p cgso=300p
+ js=10u

This will still give the messages as the parameters mentioned in the
warnings are not valid spectre MOS3 parameters. From what I can tell,
they are valid bsim3 parameters minus acm which is a hspice parameter.
Please do a search for device models on sourcelink.cadence.com. I
think you have an hspice bsim3 model. Please do a search for hspice
level 49 also. There is a compatibility page on hspice 49 to spectre
bsim3.