NF-Verstärker in SPICE

Beispiel in File nf-verstaerker.cir:

*Einfacher NF-Verstaerker
V1 in 0 AC 1 sin(0 1m 1e3) DC 0
VBATT ubatt 0 15

R1 in 1 10k
C1 1 basis 1u

R2 basis 0 330k
R3 basis ubatt 1.4MEG
R4 collector ubatt 40K
R5 emitter 0 5K
C5 emitter 0 100U

Q1 collector basis emitter BC107A
.model BC107A   NPN(Is=7.049f Xti=3 Eg=1.11 Vaf=116.3 Bf=375.5 Ise=7.049f
+ Ne=1.281 Ikf=4.589 Nk=.5 Xtb=1.5 Br=2.611 Isc=121.7p Nc=1.865
+ Ikr=5.313 Rc=1.464 Cjc=5.38p Mjc=.329 Vjc=.6218 Fc=.5 Cje=11.5p
+ Mje=.2717 Vje=.5 Tr=10n Tf=451p Itf=6.194 Xtf=17.43 Vtf=10)
+ VCEO=40 ICRATING=100M)

C2 collector out 220N
RV out 0 100K

.AC DEC 100 10 1e5
*.TRAN 10u 10m

.end

Aufruf des Simulators:
ngspice verstaerker.cir
ngspice -> run

Plots: (Alternativ, Analyse in Netzliste entsprechend auskommentieren.
Ausgabeplot für die AC-Analyse:

ngspice -> plot db(ac.v(out))

Ausgabeplot für die Transientenanalyse:

ngspice -> plot tran.v(out)