Here's a simple example - just put this together for one of my colleagues:

Code:

// Generated for: spectre
// Generated on: Mar 29 11:31:59 2004
// Design library name: mynoise
// Design cell name: test
// Design view name: schematic
simulator lang=spectre
global 0
parameters vg=1 vd=2
include "rfModels.scs"

// Library name: mynoise
// Cell name: test
// View name: schematic
V1 (net1 0) vsource dc=vd type=dc
V0 (net3 0) vsource dc=vg type=dc
M0 (net1 net3 0 net1) nmos301 w=10u l=1u
simulatorOptions options reltol=1e-3 vabstol=1e-6 iabstol=1e-12 temp=27 \
    tnom=27 scalem=1.0 scale=1.0 gmin=1e-12 rforce=1 maxnotes=5 maxwarns=5 \
    digits=5 cols=80 pivrel=1e-3 ckptclock=1800 \
    sensfile="../psf/sens.output"
noise noise start=1 stop=1G dec=10 oprobe=V1 annotate=status
modelParameter info what=models where=rawfile
element info what=inst where=rawfile
outputParameter info what=output where=rawfile
designParamVals info what=parameters where=rawfile
saveOptions options save=allpub
 

The rfModels.scs is:
Code:

// rf models
model nmos301 mos3  type=n   \
 vto=0.725  uo=585.0  tox=23.5n  nsub=3.27e+16 \
 nfs=3.5e+11  vmax=1.6e+05  eta=0.012  kappa=0.13  theta=0.080 \
 delta=2.62  xj=0.08u    rsh=533.0 \
 ld=0.250u  cgdo=2.1e-10  cgso=2.1e-10  af=1.0  kf=2.5e-28 \
 cj=4.4e-04  mj=0.370  cjsw=3.4e-10  mjsw=0.220  pb=1.100
 

Note that the models themselves need to have flicker noise enabled (the above simple mos3 model does, because it has af, kf defined).

Essentially you can wire up the device how you want; I'm measuring the noise through id in the V1 voltage source. Because I'm measuring it with a probe of a voltage source, the output will be in A/sqrt(Hz) (or A**2/Hz).

Regards,

Andrew.