Try this

.MODEL TIP31C NPN(IS=1.62181E-13 ISE=1.75416E-11 ISC=4.36516E-14 XTI=3 BF=83.6 BR=20.607 IKF=6.98433 IKR=0.997156 XTB=1.5301 +VAF=110.5 VAR=159.374 VJE=0.636 VJC=0.408 RE=0.56 RC=0.96 RB=164.793 RBM=0.100291 IRB=1.24287E-7 CJE=4.77E-10 CJC=7.29E-11 +XCJC=0.589205 FC=0.5 NF=0.9899 NR=0.989511 NE=1.95 NC=1.014 MJE=0.327 MJC=0.339 TF=2.3733E-8 TR=1.0000E-8 ITF=1 VTF=10 XTF=10 EG=1.1605 VCEO=100 ICRATING=3 MFG=TEXAS)

.MODEL TIP32C PNP(IS=6.77594E-13 ISE=1.31133E-11 ISC=1.31133E-11 XTI=3 BF=198.8 BR=25.4966 IKF=0.891251 IKR=0.410482 XTB=1.2648 +VAF=77.429 VAR=70.9603 VJE=0.59 VJC=0.5 RE=0.06 RC=0.16 RB=161.0 RBM=3.097 IRB=3.548134E-5 CJE=2.7E-10 CJC=1.07E-10 +XCJC=0.589205 +FC=0.5 NF=1.001 NR=1.004 NE=1.98 NC=1.12 MJE=0.319 MJC=0.352 TF=2.3733E-8 TR=1.0000E-8 ITF=1 VTF=10 XTF=10 +EG=1.0863 VCEO=100 ICRATING=3 MFG=TEXAS)

And can you show us your model?

 

Here are my models:

.MODEL TIP31 npn
+IS=1e-09 BF=3656.16 NF=1.23899 VAF=10
+IKF=0.0333653 ISE=1e-08 NE=2.29374 BR=0.1
+NR=1.5 VAR=100 IKR=0.333653 ISC=1e-08
+NC=1.75728 RB=6.15083 IRB=100 RBM=0.00113049
+RE=0.0001 RC=0.0491489 XTB=50 XTI=1
+EG=1.05 CJE=3.26475e-10 VJE=0.446174 MJE=0.464221
+TF=2.06218e-09 XTF=15.0842 VTF=25.7317 ITF=0.001
+CJC=3.07593e-10 VJC=0.775484 MJC=0.476498 XCJC=0.750493
+FC=0.796407 CJS=0 VJS=0.75 MJS=0.5
+TR=9.57121e-06 PTF=0 KF=0 AF=1 Vceo=60 Icrating=3
* Model generated on Feb 8, 2004
* Model format: PSpice

.MODEL TIP32 pnp
+IS=1e-09 BF=134.366 NF=1.29961 VAF=10
+IKF=0.742988 ISE=1e-16 NE=1.40014 BR=0.1
+NR=1.46599 VAR=100 IKR=3.21978 ISC=1e-16
+NC=2.71657 RB=7.44433 IRB=2.41268 RBM=0.218936
+RE=0.0152284 RC=0.0761421 XTB=0.1 XTI=1
+EG=1.05 CJE=3.26474e-10 VJE=0.446178 MJE=0.464223
+TF=1e-08 XTF=3.50642 VTF=8.2848 ITF=0.0305862
+CJC=3.07595e-10 VJC=0.77548 MJC=0.476497 XCJC=0.799334
+FC=0.8 CJS=0 VJS=0.75 MJS=0.5
+TR=9.57121e-06 PTF=0 KF=0 AF=1 Vceo=40 Icrating=3

 

Simulations of circuits have many errors. Look at my last schematic, it works perfectly with the output transistors always turned off.

 

Simulations of circuits have many errors. Look at my last schematic, it works perfectly with the output transistors always turned off.

I don't follow.
How are they "always turned off"?
Does that mean the real circuit wouldn't?

 

I don't follow.
How are they "always turned off"?
Does that mean the real circuit wouldn't?

My last schematic has the base-emitter of each output transistor accidently shorted but it simulates perfectly.
Simulations operate fine with transistors grossly overpowered.
Simulations show transistors with "typical" spec's that are much higher than the "minimum" spec's that you might buy.

An example is my version of the amplifier but with tiny low power transistors instead of proper power transistors. It survives the damage.

 

Try this


And can you show us your model?

Here are the models that I have:
.MODEL TIP31C NPN(IS=1.62181E-13 ISE=1.75416E-11 ISC=4.36516E-14 XTI=3 BF=25 BR=20.607 IKF=6.98433 IKR=0.997156 XTB=1.5301 +VAF=110.5 VAR=159.374 VJE=0.636 VJC=0.408 RE=0.56 RC=0.96 RB=164.793 RBM=0.100291 IRB=1.24287E-7 CJE=4.77E-10 CJC=7.29E-11 +XCJC=0.589205 FC=0.5 NF=0.9899 NR=0.989511 NE=1.95 NC=1.014 MJE=0.327 MJC=0.339 TF=2.3733E-8 TR=1.0000E-8 ITF=1 VTF=10 XTF=10 EG=1.1605 VCEO=100 ICRATING=3 MFG=TEXAS)

.MODEL TIP32C PNP(IS=6.77594E-13 ISE=1.31133E-11 ISC=1.31133E-11 XTI=3 BF=25 BR=25.4966 IKF=0.891251 IKR=0.410482 XTB=1.2648 +VAF=77.429 VAR=70.9603 VJE=0.59 VJC=0.5 RE=0.06 RC=0.16 RB=161.0 RBM=3.097 IRB=3.548134E-5 CJE=2.7E-10 CJC=1.07E-10 +XCJC=0.589205 +FC=0.5 NF=1.001 NR=1.004 NE=1.98 NC=1.12 MJE=0.319 MJC=0.352 TF=2.3733E-8 TR=1.0000E-8 ITF=1 VTF=10 XTF=10 +EG=1.0863 VCEO=100 ICRATING=3 MFG=TEXAS)

David

 

Here are my models:

.MODEL TIP31 npn
+IS=1e-09 BF=3656.16 NF=1.23899 VAF=10
+IKF=0.0333653 ISE=1e-08 NE=2.29374 BR=0.1
+NR=1.5 VAR=100 IKR=0.333653 ISC=1e-08
+NC=1.75728 RB=6.15083 IRB=100 RBM=0.00113049
+RE=0.0001 RC=0.0491489 XTB=50 XTI=1
+EG=1.05 CJE=3.26475e-10 VJE=0.446174 MJE=0.464221
+TF=2.06218e-09 XTF=15.0842 VTF=25.7317 ITF=0.001
+CJC=3.07593e-10 VJC=0.775484 MJC=0.476498 XCJC=0.750493
+FC=0.796407 CJS=0 VJS=0.75 MJS=0.5
+TR=9.57121e-06 PTF=0 KF=0 AF=1 Vceo=60 Icrating=3
* Model generated on Feb 8, 2004
* Model format: PSpice

.MODEL TIP32 pnp
+IS=1e-09 BF=134.366 NF=1.29961 VAF=10
+IKF=0.742988 ISE=1e-16 NE=1.40014 BR=0.1
+NR=1.46599 VAR=100 IKR=3.21978 ISC=1e-16
+NC=2.71657 RB=7.44433 IRB=2.41268 RBM=0.218936
+RE=0.0152284 RC=0.0761421 XTB=0.1 XTI=1
+EG=1.05 CJE=3.26474e-10 VJE=0.446178 MJE=0.464223
+TF=1e-08 XTF=3.50642 VTF=8.2848 ITF=0.0305862
+CJC=3.07595e-10 VJC=0.77548 MJC=0.476497 XCJC=0.799334
+FC=0.8 CJS=0 VJS=0.75 MJS=0.5
+TR=9.57121e-06 PTF=0 KF=0 AF=1 Vceo=40 Icrating=3

Aren't the DC betas too high?

 

Tried all sorts of fixes, I cannot make my sim plot as bad as yours.?
Will keep trying.


EDIT:
Lets try a different power transistor, the B139 and BD140 are in the LTS models.
Run this and see what we get.

Hi Eric:

I ran that file on my pc and ended up with this

 

Aren't the DC betas too high?

Certainly for the TIP31.

 

You want to see only the waveform (which needs only the "tran" command) but you are messing it up with the "op", "ac" and "four" commands.
I changed the "tran" command so that the simulation starts after a delay for the input capacitor to charge and to show a little more than two cycles.
Your input capacitor still has a value much too high which causes a delay before it charges enough for the circuit to work. Use 1uF instead of 100uF.
Do it like this:

 

Hi Eric:

I ran that file on my pc and ended up with this

Try with this

* BD139C - created April 13, 2011 copyright Cordell Audio
.MODEL BD139C npn
+IS=150e-15 BF=260 VAF=99
+IKF=1.2 ISE=70e-15 NE=1.2 NF=1.0
+RB=5 RC=0.01 RE=0.08
+CJE=293e-12 MJE=0.33 VJE=0.67
+CJC=49e-12 MJC=0.39 VJC=0.52 FC=0.5
+TF=585e-12 XTF=10000 VTF=35 ITF=20
+TR=10e-9 BR=78 IKR=0.14
+EG=1.21 XTB=1.14 XTI=3 NC=1.45
+ISC=19e-12 NR=1.0 VAR=7.5 IRB=0.03
+RBM=0.001 XCJC=0.53 mfg=CA041311
*
*
* BD140C - created April 13, 2011 copyright Cordell Audio
.MODEL BD140C pnp
+IS=120e-15 BF=113 VAF=140
+IKF=1.5 ISE=1000e-15 NE=1.5 NF=1
+RB=5 RC=0.01 RE=0.1
+CJE=220e-12 MJE=0.35 VJE=0.7
+CJC=68e-12 MJC=0.35 VJC=0.6 XCJC=0.5 FC=0.5
+TF=320e-12 XTF=10000 VTF=35 ITF=20
+TR=100e-9 BR=25 IKR=0.1
+EG=1.2 XTB=1.5 XTI=3 NC=1.4
+ISC=7e-12 NR=1.0 VAR=8 IRB=0.01 RBM=0.01 mfg=CA041311
*
*

This is w very good model. More here:
http://www.cordellaudio.com/book/spice_models.shtml

Here are the models that I have:

It looks like you modified the model I give you. And you set very low current gain.

I also plot the each model's current gain (β) for Ib from 1mA to 50mA

And the result are:



So no surprise why you are getting a different result than others.

I also found this when you can read how the designing process looks like.
http://www.kennethkuhn.com/students/ee351/power_amplifier1.pdf