Your link gives an "Access not authorized" error.

You can often find simulation models by seeding a search engine with, e.g., "TIP41C SPICE". Another source is the "LTSpice" Yahoo group at

LTspice : LTspice/SwitcherCAD III Please respect the members' time by searching the Files and old messages before posting "Can somebody send me a model for . . . ".

The quality and effectiveness of simulation models is a major topic by itself. The ones published by device manufacturers are usually OK for representing basic behavior in run-of-the-mill applications. You may also find some pretty crude models thrown together by individuals . . . . and in some situations a crude model is all you really need to investigate the behavior of a circuit. Occasionally you will find models that have been carefully crafted or modified by individuals to better represent some aspect of the physical component's behavior, or its behavior in certain situations. Bob Cordell's SPICE models are examples.

Here's what I found for the TIP4xx family:

.MODEL TIP41C NPN (IS=7.55826e-11 BF=260.542 NF=1.11221 VAF=100 IKF=0.526814 ISE=1e-08 NE=2.18072 BR=26.0542 NR=1.5 VAR=1000 IKR=3.54059 ISC=1e-08 NC=1.63849 RB=4.56157 IRB=0.1 RBM=0.1 RE=0.0162111 RC=0.0810556 XTB=0.1 XTI=1 EG=1.206 CJE=1.93296e-10 VJE=0.4 MJE=0.259503 TF=1e-08 XTF=4.06972 VTF=7.1157 ITF=0.001 CJC=1.09657e-10 VJC=0.730921 MJC=0.23 XCJC=0.803085 FC=0.8 CJS=0 VJS=0.75 MJS=0.5 TR=9.01013e-08 PTF=0 KF=0 AF=1 Vceo=100 ICrating=6 mfg=ON_Semi)

.MODEL TIP42C PNP (IS=5.65618e-10 BF=120.073 NF=1.24004 VAF=90.6071 IKF=1.46498 ISE=6.98929e-14 NE=4 BR=2.83268 NR=1.30331 VAR=27.1221 IKR=10 ISC=6.98934e-14 NC=3.78125 RB=4.71382 IRB=0.234602 RBM=0.12691 RE=0.000666374 RC=0.0927424 XTB=3.21145 XTI=1 EG=1.05 CJE=1.93221e-10 VJE=0.4 MJE=0.259369 TF=9.99163e-09 XTF=4.41941 VTF=6.53488 ITF=0.001 CJC=1.0962e-10 VJC=0.731968 MJC=0.23 XCJC=0.799902 FC=0.799995 CJS=0 VJS=0.75 MJS=0.5 TR=1e-07 PTF=0 KF=0 AF=1 Vceo=100 ICrating=6 mfg=ON_Semi)

.MODEL TIP41C NPN ( IS=290.83E-15 BF=113.55 VAF=100 IKF=1.9905 ISE=1.3946E-12 NE=1.4763 BR=.1001 VAR=100 IKR=10.010E-3 ISC=320.65E-12 NC=1.8994 NK=.58929 RB=.71129 CJE=348.44E-12 VJE=.78228 MJE=.42865 CJC=184.26E-12 VJC=.47897 MJC=.40458 TF=36.381E-9 XTF=100.32 VTF=21.563 ITF=28.791 TR=10.000E-9 Vceo=100 ICrating=6 mfg=Central_Semi)

.MODEL TIP42C PNP (Is=66.19f Xti=3 Eg=1.11 Vaf=100 Bf=137.6 Ise=862.2f Ne=1.481 Ikf=1.642 Nk=.5695 Xtb=2 Br=5.88 Isc=273.5f Nc=1.24 Ikr=3.555 Rc=79.39m Cjc=870.4p Mjc=.6481 Vjc=.75 Fc=.5 Cje=390.1p Mje=.4343 Vje=.75 Tr=235.4n Tf=23.21n Itf=71.33 Xtf=5.982 Vtf=10 Rb=.1 Vceo=100 ICrating=6 mfg=Texas_Inst)

You will probably want to check out "How to Import a Transistor Model in LTSpice" at

http://courses.ee.sun.ac.za/Electronics_365/Praktika/Using your own models in LTScpice.pdf (The associated course syllabus page at

Elektronika 365 - 2012 includes links to additional TIP4xx models.)

If you are studying this circuit as a way to learn about amplifiers (which is not a bad idea!), consider doing the following exercise, based on your observations from the circuit you first entered into LTSpice:

- Learn to do a frequency response plot using the " .AC " analysis. Measure the upper and lower cutoff frequencies for your circuit.
- Change some capacitor values, one at a time. The compensation capacitor might be a good place to start, since it's value was originally your most significant error. Increase, or decrease, its value by a factor of, say, 3 or 4. Then try a factor of 20 or 50. Or even 1000. What happens? Do you see why your original value gave the results you observed?
- Do the same experiment with the input and output coupling capacitors. How do they affect overall performance?

Dale