Hi...

My current job is to simulate several BJTs polarizations!

Where can I get a complete model for 2N2222A??? The one iI find doesn't even has the Vce and Ic!!!

 

Hello,

I do not know much about spice, but perhaps the models on this page might help:
http://www.onsemi.com/PowerSolutions/supportDoc.do?type=models&category=797

Bertus

 

Where can I get a complete model for 2N2222A??? The one iI find doesn't even has the Vce and Ic!!!

What did you mean by saying "complete model".
And why you looking Vce and Ic in the "model"? Pspice models don't have Ic and Vce.
Simulation software based on BJT "model" calculated Vce and Ic for a given circuit with transistor.

 

Those specs are really different from these ones:

.MODEL Q2n2222a npn
+IS=3.88184e-14 BF=929.846 NF=1.10496 VAF=16.5003
+IKF=0.019539 ISE=1.0168e-11 NE=1.94752 BR=48.4545
+NR=1.07004 VAR=40.538 IKR=0.19539 ISC=1.0168e-11
+NC=4 RB=0.1 IRB=0.1 RBM=0.1
+RE=0.0001 RC=0.426673 XTB=0.1 XTI=1
+EG=1.05 CJE=2.23677e-11 VJE=0.582701 MJE=0.63466
+TF=4.06711e-10 XTF=3.92912 VTF=17712.6 ITF=0.4334
+CJC=2.23943e-11 VJC=0.576146 MJC=0.632796 XCJC=1
+FC=0.170253 CJS=0 VJS=0.75 MJS=0.5
+TR=1e-07 PTF=0 KF=0 AF=1

The one I found is pretty different

.MODEL 2n2222a  NPN (IS=2.20f NF=1.00 BF=240 VAF=114
+ IKF=0.293 ISE=2.73p NE=2.00 BR=4.00 NR=1.00
+ VAR=24.0 IKR=0.600 RE=0.194 RB=0.777 RC=77.7m
+ XTB=1.5 CJE=24.9p VJE=1.10 MJE=0.500 CJC=12.4p VJC=0.300
+ MJC=0.300 TF=371p TR=64.0n EG=1.12 )

 

Those specs are really different from these ones:

.MODEL Q2n2222a npn
+IS=3.88184e-14 BF=929.846 NF=1.10496 VAF=16.5003
+IKF=0.019539 ISE=1.0168e-11 NE=1.94752 BR=48.4545
+NR=1.07004 VAR=40.538 IKR=0.19539 ISC=1.0168e-11
+NC=4 RB=0.1 IRB=0.1 RBM=0.1
+RE=0.0001 RC=0.426673 XTB=0.1 XTI=1
+EG=1.05 CJE=2.23677e-11 VJE=0.582701 MJE=0.63466
+TF=4.06711e-10 XTF=3.92912 VTF=17712.6 ITF=0.4334
+CJC=2.23943e-11 VJC=0.576146 MJC=0.632796 XCJC=1
+FC=0.170253 CJS=0 VJS=0.75 MJS=0.5
+TR=1e-07 PTF=0 KF=0 AF=1

The one I found is pretty different

.MODEL 2n2222a  NPN (IS=2.20f NF=1.00 BF=240 VAF=114
+ IKF=0.293 ISE=2.73p NE=2.00 BR=4.00 NR=1.00
+ VAR=24.0 IKR=0.600 RE=0.194 RB=0.777 RC=77.7m
+ XTB=1.5 CJE=24.9p VJE=1.10 MJE=0.500 CJC=12.4p VJC=0.300
+ MJC=0.300 TF=371p TR=64.0n EG=1.12 )

So what? They just a simulation models, create to help as predict the performance of a real world circuit. Some models will have greater accurate some will have less accurate. And these models represent the behavior of a typical BJT. But don't forget that typical BJT don't exist.
Look at data sheet
http://www.eng.yale.edu/ee-labs/morse/compo/datasheets/2n2222.pdf
And notice for example how Hfe can varies widely among 2n2222.
Any given 2n2222 may have Hfe between 75 and 300 for Ic = 1mA.

 

Ok, I know that there are no such thing as 2 bjts with the exact same settings, but those 2 examples I gave are too much different. The hFE in the first is of 240 and in the other is over 900...

And one has more settings than the other... I need one that has all the details so I don't miss anything!

 

And one has more settings than the other... I need one that has all the details so I don't miss anything!

hi Psy,

Dont forget LTSpice has limitations on the details it can work with, some Spice and PSpice parameters are not recognised by LTS and it will report errors.

 

but those 2 examples I gave are too much different. The hFE in the first is of 240 and in the other is over 900...

But this BF parameter has almost nothing to do with the Hfe that transistor will have in simulation.
See the simulation result

Hfe VS Ic for Q2n2222a

As you can see Hfe never reach 930

And Hfe vs Ic for 2n2222a model

Also read this
http://people.rit.edu/lffeee/Lab_BJT_Intro.pdf (from page 13)

 

Ok, so what is the parameter that I need to change when the teacher asks to change the gain?

 

You change the BF= value, but would not recommend doing that unless you understand what impact that will have on the remainder of the calculations.

E

 

You change the BF= value, but would not recommend doing that unless you understand what impact that will have on the remainder of the calculations.

E

So, how am i supposed to check the impact that β has in the bjt? Our teacher is asking us to change the β and check what is the difference between those different values!

 

So, how am i supposed to check the impact that β has in the bjt? Our teacher is asking us to change the β and check what is the difference between those different values!

hi Psy,

Then that is what I would do.

Its always a good idea to follow your tutors directives to get your answers, if you think that he could be missing something, add your findings as a footnote to your answers.

Try say 100 thru 500 in 100 steps, plot the gains.

If you wanted to know the effect on the other parameters, you could run for example, AC Analysis, check if the gain bandwidth changes etc.

 

Ok, let me go step by step or it will be confusing to me!

I'm using the follwoing .model:

.MODEL 2N2222A  NPN (IS=2.20f NF=1.00 BF=240 VAF=114
+ Icrating=800m Vceo=30
+ IKF=0.293 ISE=2.73p NE=2.00 BR=4.00 NR=1.00
+ VAR=24.0 IKR=0.600 RE=0.194 RB=0.777 RC=77.7m
+ XTB=1.5 CJE=24.9p VJE=1.10 MJE=0.500 CJC=12.4p VJC=0.300
+ MJC=0.300 TF=371p TR=64.0n EG=1.12 mfg=PsyTronics)

The teacher is asking us to test the attached circuit (fixed polarization).

Then he asks us the what we call the PFR whis is the Rest Fuction Point, but I don't know who you call it in English...

So, I think something is wrong because i can't get the correct Ic.

I'm using some equations to get the Vce and Ic which are:

Vcc = Rb.Ib + Vbe (1)
Vcc = Rc.Ic + Vce (2)
Ic=β.Ib (3)

The PFR is (Vce;Ic), so I've calculated Ib from the 1st equation by:

15 = 720kΩ*Ib + 0.7 <=> Ib=19.86μA

Then I calculated Ic from the 3rd equation with the β from LTSpice bjt model by:

Ic = 240*19.86μA = 4.77mA

Finally i got Vce from the 2nd equation by:

15 = 2.2kΩ*4.77mA + Vce <=> Vce = 4.51V

But ploting Ic(Vce) I'm not getting these values. For a Vce of 4.51V I have an Ic of 3.85V...

What am i missing?


PS: And also, if I plot Ic/Ib, I can't get the 240 that LTSpice has in the .model! The best I get is 197 for β. Is this normal?

 

Then he asks us the what we call the PFR whis is the Rest Fuction Point, but I don't know who you call it in English...

PFR = DC bias point or DC operating point or quiescent point.

I'm using some equations to get the Vce and Ic which are:

Vcc = Rb.Ib + Vbe (1)
Vcc = Rc.Ic + Vce (2)
Ic=β.Ib (3)

Your equation 1 and 2 are wrong.

And for this circuit we need only two equation

Vcc = (Ib + Ic)*Rc + Rb*Ib + Vbe (1)
And
Ic = β*Ib (2)

If we solve it for Ib we have

Ib = (Vcc - Vbe)/((β+1)*Rc + Rb)

And if we assume Vbe = 0.7V and β = 240

We have Ib = 11.438μA and Ic = 2.745mA and Vce = Vcc - (Ib + Ic)*Rc = 8.9V

The simulation result are

Ic = 2.4mA and Vce = 9.67V

And that's all we can do for this simple circuit.
And it is impossible to get the same result in our hand calculation as we get from LTspice. Why?

Because as you may know, transistors are nonlinear device and this is why equation describe transistor are also nonlinear. Normally, it is impossible to find analytical solution for this type of a circuits. We can use numerical method or use iteration method. But we often use hand calculation. And in this case we are force to assume some transistors parameters needed for calculation. And this is why we almost always assume Vbe value between 0.6V...0.7V. We have the same situation with other BJT parameters for example Hfe or Vce_saturation voltage
So in our hand calculation use simplified BJT model. We simply assume that Ic = β*Ib and we assume that Vbe = constant, which is not true in real world. But simulation software use full nonlinear model.
And this is why it's almost impossible to get the same result as we get in LTspice.

PS: And also, if I plot Ic/Ib, I can't get the 240 that LTSpice has in the .model! The best I get is 197 for β. Is this normal?

Read again post 8.

 

Something's wrong here!!!

In the previous post I built the wrong circuit for the fixed polarization.

Things should came out like they are now!


Edit;

Sir Jony130, I'm sorry for the mess... Looks like even with the correct circuit running, my calculations are not ok...

The equations I posted before were wrong for the 1st circuit I posted because I made a mistake building it!
But now the circuit is correct for fixed polarization!

But somehow, LTSpice doesn't gives me close results!

 

Something's wrong here!!!

In the previous post I built the wrong circuit for the fixed polarization.

Things should came out like they are now!

So what? This doesn't change the fact that still it is not possible to obtain the same results in LTspice and in hand calculations without cheating.

 

How can I calculate the new DC bias point when we change the temp for, let's say 100ºC???

 

And one other question.

I have calculated 3 DC bias points in the last 3 questions for the same BJT. The original one, then with β=100 and then with Temp = 100ºC.

Now he wants us to plot the 3 Ic(Vce) curves and also draw the Charge Line (Vce = 0 and Ic = 0)

Can I do this in LTSpice?

 

I have calculated 3 DC bias points in the last 3 questions for the same BJT. The original one, then with β=100 and then with Temp = 100ºC.

Watch this video.
https://www.youtube.com/watch?v=eRtO3EZK_Cc
Or
Try this method

Now he wants us to plot the 3 Ic(Vce) curves and also draw the Charge Line (Vce = 0 and Ic = 0)

Do you mean load line ?
http://en.wikipedia.org/wiki/Load_line_(electronics)

 

I don't know if what I called the Charge Line is what you posted from wikipedia, but I can try to explain better.

What I mean is that line where we know all DC Bias points will lay.

Something like this:

Edit;

Jony130, I can't make your .asc files run on my LTSpice!