BJT SPICE Models, reality-check

[klewis]

Originally Posted by keantoken

That was interesting. In the VAS, you are applying positive feedback instead of negative feedback (your image is wrong it seems). Try this.

I used different models, so you'll have to change them back.

- keantoken

Keantoken,

Thanks for the help. I got it to run in what I would describe as a static state - no input signal. So, how do I inject the sine wave into the model to get THD?

Ken

[keantoken]

Pretend the - side of the voltage amplifier is the input side of an LTP, so attach the input cource to it. Treat this voltage source as a VAS also, thus Cdom as C1. This gives proper compensation, whereas the old 1u cap actually did the opposite of compensation. I'm not sure how this schematic came about but it has some major errors.

- keantoken

[klewis]

Originally Posted by keantoken

Pretend the - side of the voltage amplifier is the input side of an LTP, so attach the input cource to it. Treat this voltage source as a VAS also, thus Cdom as C1. This gives proper compensation, whereas the old 1u cap actually did the opposite of compensation. I'm not sure how this schematic came about but it has some major errors.

- keantoken

It came from here
On Semi ThermalTrak

post 519.

Thanks again for the help.

Ken

[klewis]

Keantoken,

It works great, thanks. Back to topic, do you have better models for the MJL3281/1302, MJE15033/32?

Ken

[keantoken]

These are models made by AndyC. The 4793/1837 are the drivers I usually simulate with, models also courtesy of Andy. These are all I have.

.MODEL mjl3281a_x npn IS=9.8145e-12 BF=438.0 NF=1.00 VAF=38 IKF=19.0 ISE=1.0e-12 NE=1.1237388682 BR=4.98985 NR=1.09511 VAR=4.32026 IKR=4.37516 ISC=3.25e-13 NC=3.96875 RB=3.997 RE=0.00 RC=0.06 XTB=0.115253 XTI=1.03146 EG=1.11986 CJE=1.144e-08 VJE=0.468574 MJE=0.34957 TF=2.6769e-9 XTF=7500 VTF=3.0 ITF=1000 CJC=1.093685e-9 VJC=0.623643 MJC=0.482111 XCJC=0.959922 FC=0.1 CJS=0 VJS=0.75 MJS=0.5 TR=1e-07 PTF=0 KF=0 AF=1 Vceo=200 Icrating=15 mfg=OnSemiconductor
.MODEL mjl1302a_x pnp IS=9.8145e-12 BF=122.925 NF=1.00 VAF=40 IKF=19 ISE=9.18577762370362E-07 NE=5.0 BR=4.98985 NR=1.09511 VAR=4.32026 IKR=4.37516 ISC=3.25e-13 NC=3.96875 RB=3.30 RE=0.00 RC=0.06 XTB=0.115253 XTI=1.03146 EG=1.11986 CJE=1.561e-08 VJE=0.781803 MJE=0.433868 TF=3.257e-9 XTF=1000 VTF=2.0 ITF=260 CJC=2.346838e-9 VJC=0.27876 MJC=0.411324 XCJC=0.959922 FC=0.1 CJS=0 VJS=0.75 MJS=0.5 TR=1e-07 PTF=0 KF=0 AF=1 Vceo=200 Icrating=15 mfg=OnSemiconductor
.MODEL Q2SA1837_x PNP ( IS=2.39372559E-10 NF=1.304015937 BF=300 VAF=273 IKF=2.087725944 NK=0.94719458 ISE=1.46829699E-11 NE=1.526663542 BR=4 NR=1 VAR=20 IKR=1.05 RE=0 RB=1.8 RC=1.65 CJE=4.7407E-10 VJE=1.1 MJE=0.5 CJC=8.6700E-11 VJC=0.3 MJC=0.3 TF=1.642191E-09 FC=0.5 ITF=1.076260106 XTF=5.868994022 TR=1.38U)
.MODEL Q2SC4793_x NPN ( IS=1.8E-09 NF=1.43 BF=146.38 VAF=273 IKF=2.6 NK=0.95 ISE=6.286997E-10 NE=2.223629 BR=4 NR=1 VAR=20 IKR=1.05 RE=0 RB=1.7 RC=1.25 CJE=5.96964E-10 VJE=1.1 MJE=0.5 CJC=5.78E-11 VJC=0.3 MJC=0.3 TF=1.22678E-09 FC=0.5 ITF=10 XTF=99.52253015 TR=983N)

- keantoken

[tiefbassuebertr]

an interesting thread
in this case this thread could be of interest:
Transistor modeling - how do I generate P-Spice Parameter ?

[klewis]

keantoken,

Happy new year a day early...

I'm trying to make my own models. Following Andy_C's instructions, I was able to plot hFE vs Ic, but can't figure out what expressions to use for the following:

1. Plotting Vbe vs Ic

2. Plotting B (Beta) vs Ic

3. Plotting fT at Ic = 100mA and 300mA

I'm sure you can help... the spice circuit setup is attached.

Thanks,

Ken L

[keantoken]

For Vbe vs. Ic, just click at the Q's emitter. Left-click on the bottom ruler in the trace window and deselect the logarithmic option (for other graphs the X axis is usually logarithmic, but not for Vbe).

Hfe and Beta are the same in andy's article if I'm correct, and it worked for me usually.

Now for Ft, set up a .ac analysis, right-click on I1 to give it the desired current, and then plot Hfe (Ic/Ib). Ft will be, if I'm correct, the point where Hfe crosses zero.

I can give a file to test Vcesat as well.

What is your aim though with the MJD models? I think I checked and they are surprisingly accurate compared to the throw-away models one usually encounters. (not to say there's nothing more to be desired...) And BTW you may be interested in the BD787/788 which are very similar, in fact they could be the same die, I had a hard time trying to find the difference.

This can get tricky since Andy doesn't describe the relationships simply between IKF, ISE, NE... Just so you know, I have some experience here and can help if necessary. (there are a few things I can't figure out myself though, which makes me wonder how on earth I managed to finish my 5769/5771 models...)

And by the way, I generally use the _k signature on my models to distinguish between them and the old models. It might be confusing if we use the same signature, if it matters.

And I ask you put finished model here, so other people can access them:

Spice Models - diyAudio Contributions - diyAudio

- keantoken

[klewis]

Originally Posted by keantoken

For Vbe vs. Ic, just click at the Q's emitter. Left-click on the bottom ruler in the trace window and deselect the logarithmic option (for other graphs the X axis is usually logarithmic, but not for Vbe).

Hfe and Beta are the same in andy's article if I'm correct, and it worked for me usually.

Now for Ft, set up a .ac analysis, right-click on I1 to give it the desired current, and then plot Hfe (Ic/Ib). Ft will be, if I'm correct, the point where Hfe crosses zero.

I can give a file to test Vcesat as well.

What is your aim though with the MJD models? I think I checked and they are surprisingly accurate compared to the throw-away models one usually encounters. (not to say there's nothing more to be desired...) And BTW you may be interested in the BD787/788 which are very similar, in fact they could be the same die, I had a hard time trying to find the difference.

This can get tricky since Andy doesn't describe the relationships simply between IKF, ISE, NE... Just so you know, I have some experience here and can help if necessary. (there are a few things I can't figure out myself though, which makes me wonder how on earth I managed to finish my 5769/5771 models...)

And by the way, I generally use the _k signature on my models to distinguish between them and the old models. It might be confusing if we use the same signature, if it matters.

And I ask you put finished model here, so other people can access them:

Spice Models - diyAudio Contributions - diyAudio

- keantoken

I think my model is way, way off, but, I'll get there... I couldn't figure out your instructions... could you make plt files, save them and send them back?

I've attached the sim files with the one plt file I have - the hFE vs Collector current.

If I every have a model worth sharing, I'll append it with either KL or K3

Thanks

Ken L

[klewis]

And now the file