how to use parametric Analysis in hspice?(help!!!)

hspice parametric analysis

I am the beginner of hspice simulator.These is a common-source circuit.
It's hspice netlist as follows:

*common source
*circuit*
m1 d1 g1 0 b1 nmos1 l=2u w=80u
rd vdd d1 1k

.model nmos1 nmos level=3
*source*
Vdd vdd 0 dc 5v
vsin g1 0 sin(1.8v 10mv 1k 0 0 0)
*analysis*
.tran 1u 2ms
.dc vsin 0 5 1m

.probe v(d1)
.end

I want to know how does the variety of rd affect the output of v(d1).But how to use parametric sweeping on rd with hspice?

parametric analysis in spice

hbchens said:

I am the beginner of hspice simulator.These is a common-source circuit.
It's hspice netlist as follows:

*common source
*circuit*
m1 d1 g1 0 b1 nmos1 l=2u w=80u
rd vdd d1 1k

.model nmos1 nmos level=3
*source*
Vdd vdd 0 dc 5v
vsin g1 0 sin(1.8v 10mv 1k 0 0 0)
*analysis*
.tran 1u 2ms
.dc vsin 0 5 1m

.probe v(d1)
.end

I want to know how does the variety of rd affect the output of v(d1).But how to use parametric sweeping on rd with hspice?

Click to expand...

try this
.param r_val=1k
rd vdd d1 r_val
.tran 1u 2m sweep r_val 1k 5k 1k $linear sweep
.dc vsin 0 5 1m sweep r_val dec 3 1k 100k $r_val=1k,10k,100k

hope this help

hspice parametric

To wpchan05:
thank you for your help!have followed your method,i get the right curve that include the tran and dc curve.But i find little problem in the lis file: “**warning** unknown analysis mode: .. line ignored ”。
I don't know if this problem is important?

The full output lis file does as follows:
* hspice.ini
*
* use ascii only for initial pc hspice release
*
.option post = 2
.param r_val=1k
*circuit*
m1 d1 g1 0 0 nmos1 l=2u w=80u
rd vdd d1 r_val

.model nmos1 nmos level=3
*source*
vdd vdd 0 dc 5v
vsin g1 0 sin(1.8v 10mv 1k 0 0 0)
*analysis*
.tran 1u 2ms sweep r_val 1k 5k 1k $linear sweep
.dc vsin 0 5 1m sweep r_val dec 3 1k 100k $r_val=1k,10k,100k


.probe

**warning** unknown analysis mode: .. line ignored

.end
1 ****** HSPICE X-2005.09 (20050729) 13:35:12 10/12/2006 pcnt
******
*common source
****** mos model parameters tnom= 25.000 temp= 25.000
******
***************************************************************************
*** common model parameters model name: 0:nmos1 model type:nmos ***
***************************************************************************
names values units names values units names values units
----- ------ ----- ----- ------ ----- ----- ------ -----

1*** geometry parameters ***
ld= 0. meters lmlt= 1.00 wd= 0. meters
wmlt= 1.00 xl= 0. meters xw= 0. meters
lref= 0. meters wref= 0. meters lref= 0. meters
wref= 0. meters xlref= 0. meters xwref= 0. meters
lmin= 0. meters wmin= 0. meters lmax= 0. meters
wmax= 0. meters

2*** threshold voltage parameters ***
vto= 133.88m volts nss= 0. 1/cm**2 tpg= 1.00
phi= 579.84m volts gamma= 527.63m v**0.5 bulk= gnd
ngate= 0. cm**3 nsub= 1.0e+15 1/cm**3 delvto= 0. volts

3*** gate overlap capacitance parameters ***
cgbo= 0. f/meter cgdo= 0. f/meter cgso= 0. f/meter
meto= 0. meters

4*** gate capacitance parameters ***
capop= 2.00 cf1= 0. volts cf2= 100.00m volts
cf3= 1.00 volts cf4= 50.00 cf5= 666.67m
cf6= 500.00 xqc= 500.00m tox= 100.00n meters
cox= 345.31u f/m**2

5*** diffusion parasitic parameters ***
acm= 0. is= 10.00f amps js= 0. a/m**2
jsw= 0. amp/m nds= 1.00 cbd= 0. farad
cbs= 0. farad cj= 101.85u f/m**2 cjsw= 0. f/m
cjgate= 0. f/m mj= 500.00m mjsw= 330.00m
pb= 800.00m volts php= 800.00m volts tt= 0. secs
hdif= 0. meters ldif= 0. meters rd= 0. ohms
rs= 0. ohms rsh= 0. ohms/sq fc= 0.
alpha= 0. vcr= 0. volts iirat= 0.
rdc= 0. ohms rsc= 0. ohms n= 1.00
vnds= -1.00 volts

6*** temperature effect parameters ***
tlev= 0. tlevc= 0. eg= 1.11 ev
gap1= 702.00u ev/deg gap2= 1.11k deg xti= 0.
bex= -1.50 tcv= 0. v/deg k trd= 0. /deg
trs= 0. /deg cta= 0. /deg ctp= 0. /deg

7*** noise parameters ***
kf= 0. af= 1.00 nlev= 2.00
gdsnoi= 1.00

*** level 3 model parameters ***

delta= 0. eta= 0. kappa= 200.00m /v
nfs= 0. 1/cm**2 theta= 0. /v vmax= 0. m/sec
xj= 0. meters uo= 600.00 cm**2/vs kp= 20.72u a/v**2
deriv= 1.00
Opening plot unit= 79
file=c:\hspice\csource.sw0

**warning** negative-mos conductance = 0:m1 iter= 2
vds,vgs,vbs = 2.32 2.83 0.00
gm,gds,gmbs,ids= -2.020E-05 2.243E-03 0.00 2.676E-03

***** job concluded

***** job concluded

***** job concluded

***** job concluded

***** job concluded

***** job concluded

*** parameter r_val = 1.000E+03 ***

Opening plot unit= 79
file=c:\hspice\csource.tr0


***** job concluded

*** parameter r_val = 2.000E+03 ***


***** job concluded

*** parameter r_val = 3.000E+03 ***


***** job concluded

*** parameter r_val = 4.000E+03 ***


***** job concluded

*** parameter r_val = 5.000E+03 ***


***** job concluded
1 ****** HSPICE X-2005.09 (20050729) 13:35:12 10/12/2006 pcnt
******
*common source
****** job statistics summary tnom= 25.000 temp= 25.000
******

total memory used 234 kbytes

# nodes = 4 # elements= 4
# diodes= 0 # bjts = 0 # jfets = 0 # mosfets = 1 # va device = 0

analysis time # points tot. iter conv.iter

op point 0.02 1 25
dc sweep 2.22 35007 70038
transient 0.57 10005 4030 2015 rev= 0
readin 0.01
errchk 0.00
setup 0.02
output 0.00
total cpu time 3.50 seconds
job started at 13:35:12 10/12/2006
job ended at 13:35:16 10/12/2006


Init: hspice initialization file: C:\eda\synopsys\Hspice_X-2005.09\hspice.ini
lic: Release hspice token(s)

thank you again for your help!

.param hspice

the warning message may come from the missing function call in your .option statement. Try putting the following staement to see if the warning can be handled

.option probe

I also think that as long as you get the curves, you should not worry so much at this moment.

hspice parameteric analysis

To wpchan05:
The problem have been solved with your help.
I really appreciate your help!