# Why does voltage gain of fixed bias transistors not as same I calculated ?

#### Jony130

Joined Feb 17, 2009
5,440
To be able to answer this question I extract 2N2222 BJT's model from Multisim.
.MODEL 2N2222_Multisim npn
+IS=1.87573e-15 BF=153.575 NF=0.897646 VAF=10
+IKF=0.410821 ISE=3.0484e-09 NE=4 BR=0.1
+NR=1.00903 VAR=1.92063 IKR=4.10821 ISC=1.94183e-12
+NC=3.92423 RB=8.70248 IRB=0.1 RBM=0.1
+RE=0.111394 RC=0.556972 XTB=1.76761 XTI=1
+EG=1.05 CJE=1.67272e-11 VJE=0.83191 MJE=0.23
+TF=3.573e-10 XTF=0.941617 VTF=9.22508 ITF=0.0107017
+CJC=9.98785e-12 VJC=0.760687 MJC=0.345235 XCJC=0.9
+FC=0.49264 CJS=0 VJS=0.75 MJS=0.5
+TR=3.55487e-06 PTF=0 KF=0 AF=1
And if we do this, we see that Early's voltage (VAF) has a very low-value VAF = 10V. Thus, the transistor output resistance (ro) will be extremely low.

ro ≈ (11.3V + 10V)/3.73mA ≈ 5.7kΩ

Therefore the voltage gain will be around

Av ≈ (Rc||RL||ro)/re ≈ (5kΩ||5.7kΩ||100kΩ)/6.9Ω ≈ 2.6kΩ/6.9Ω ≈ 376V/V

#### MrChips

Joined Oct 2, 2009
28,151
I simulated the circuit on CircuitMaker 2000.

With, R1 = 1875kΩ
VB = 0.613V
VC = 20.70V
Av = -320

With R1 = 1300kΩ
VB = 0.625V
VC = 15.76V
Av = -480

With R1 = 620kΩ connected to transistor collector
VB = 0.626V
VC = 15.12V
Av = -480

#### WBahn

Joined Mar 31, 2012
28,185
To be able to answer this question I extract 2N2222 BJT's model from Multisim.

And if we do this, we see that Early's voltage (VAF) has a very low-value VAF = 10V. Thus, the transistor output resistance (ro) will be extremely low.

ro ≈ (11.3V + 10V)/3.73mA ≈ 5.7kΩ

Therefore the voltage gain will be around

Av ≈ (Rc||RL||ro)/re ≈ (5kΩ||5.7kΩ||100kΩ)/6.9Ω ≈ 2.6kΩ/6.9Ω ≈ 376V/V
That is pretty low. Based on my sim of LTSpice's model, I got an early voltage of 98 V (I'm going to guess that if I go dig up the model file it will be 100 V).

I would say that this mystery is solved (although I don't know why my sim results are still off by ~10% from the hand calculations).

#### LvW

Joined Jun 13, 2013
1,622
Yes - an output resistance rce of app 6 kOhm is too low. This can`t be true.

#### Jony130

Joined Feb 17, 2009
5,440
I would say that this mystery is solved (although I don't know why my sim results are still off by ~10% from the hand calculations).
I think that the situation is using |Vbc| voltage instead of Vce when calculating ro. Also, the re will be slightly different and the β/(β + 1) factor.
And LTspice shows that the gain is 367 V/V

#### Papabravo

Joined Feb 24, 2006
19,869
To be able to answer this question I extract 2N2222 BJT's model from Multisim.

And if we do this, we see that Early's voltage (VAF) has a very low-value VAF = 10V. Thus, the transistor output resistance (ro) will be extremely low.

ro ≈ (11.3V + 10V)/3.73mA ≈ 5.7kΩ

Therefore the voltage gain will be around

Av ≈ (Rc||RL||ro)/re ≈ (5kΩ||5.7kΩ||100kΩ)/6.9Ω ≈ 2.6kΩ/6.9Ω ≈ 376V/V
That is an oversight you could drive a truck through. Good catch @Jony130

#### WBahn

Joined Mar 31, 2012
28,185
I think that the situation is using |Vbc| voltage instead of Vce when calculating ro. Also, the re will be slightly different and the β/(β + 1) factor.
And LTspice shows that the gain is 367 V/V
My simulation using LTSpice got a gain of 535. I wonder what we are doing differently.

#### LvW

Joined Jun 13, 2013
1,622
My simulation using LTSpice got a gain of 535. I wonder what we are doing differently.
To complete the picture, here are my simulation results (PSpice) measured for 10kHz:

1.) 2N2222 model from Zetex: A=-554.75 (ac) and A=-548.5 (TRAN, 1mV)
2.) Q2N2222 model : A=-467,5 (ac) and A=-461 (TRAN, 1mV)

#### Heroz

Joined May 29, 2022
31
To complete the picture, here are my simulation results (PSpice) measured for 10kHz:

1.) 2N2222 model from Zetex: A=-554.75 (ac) and A=-548.5 (TRAN, 1mV)
2.) Q2N2222 model : A=-467,5 (ac) and A=-461 (TRAN, 1mV)
I have a question. Which model is true ?

#### LvW

Joined Jun 13, 2013
1,622
I have a question. Which model is true ?
That is a very good question.
Simple answer: No model is "true". But the question remains: Which model comes as close as possible to reality?
I am afraid that even this qiestion cannot be answered.
I think, instead we must ask for a certain parameter (bandwidth, Early effect,..).
However, with respect to tolerances of the real device, even such a specific question is hard to answer.

#### Heroz

Joined May 29, 2022
31
That is a very good question.
Simple answer: No model is "true". But the question remains: Which model comes as close as possible to reality?
I am afraid that even this qiestion cannot be answered.
I think, instead we must ask for a certain parameter (bandwidth, Early effect,..).
However, with respect to tolerances of the real device, even such a specific question is hard to answer.
So model don't give an exact value right? But to design we use this to predict and give as close as possible to reality and to predict we need to choose suitable model for each situation.

#### ericgibbs

Joined Jan 29, 2010
17,174
hi Hero,
There is a spread in the parameters for most semiconductor devices, this is mainly due to manufacturing.
I use the typical values from the device's datasheet, other users choose the lowest parameter listings.
E

#### Heroz

Joined May 29, 2022
31
I think that the situation is using |Vbc| voltage instead of Vce when calculating ro. Also, the re will be slightly different and the β/(β + 1) factor.
And LTspice shows that the gain is 367 V/V
Sorry . I'm still not understand your gain in LTspice is 367 ? But I tried to simulate in LTspice it's 535 . What is different?

Last edited:

#### Papabravo

Joined Feb 24, 2006
19,869
Sorry . I'm still not understand your gain in LTspice is 367 ? But I tried to simulate in LTspice it's 535 . What is different?
That is still a hard question to answer, because we are not there looking over your shoulder. We already know ther are numerous different models in the wild for the same component. As I mentioned before there is no central authority that will adjudicate the accuracy or suitability of any model. As a designer your only defense is to know what you are working with and to use simulation to enhance your understanding and NOT for design verification. Depending on simulation for design verification is the road to perdition. The same is true of real devices in that you must assume that no two devices selected at random will have the same parameters. In some case they won't even be close. What you do is make sure that your design is not sensitive to the actual device parameters.

#### LvW

Joined Jun 13, 2013
1,622
So model don't give an exact value right? But to design we use this to predict and give as close as possible to reality and to predict we need to choose suitable model for each situation.
Heroz - there is one important aspect which you must know for not to be too pessimistic:
Fortunately, there is the method of negative feedback which remarkably reduces the influence of parameter tolerances and other uncertainties of the active device.
This method is usd, therefore, in all practical realizations.
Either we add a resistor between the emitter and ground (current-controlled voltage feedback) or the upper resistor of the bias voltage divider is not connected to the supply but to the collector node (voltage-controlled current feedback).

#### Heroz

Joined May 29, 2022
31
Thank you everyone for answer me.
Now I'm understand .

#### Jony130

Joined Feb 17, 2009
5,440
Sorry . I'm still not understand your gain in LTspice is 367 ? But I tried to simulate in LTspice it's 535 . What is different?
Because LTspcie is using the "correct" value for Early voltage. And I used the "corrupted" Multisim model. But in Mulitsim you can use a "better" model, try to use 2N2222A instead of 2N2222.
See my LTspice file with the "corrupted" model

My simulation using LTSpice got a gain of 535. I wonder what we are doing differently.
Try to use this model:

.MODEL 2N2222_Multisim npn
+IS=1.87573e-15 BF=153.575 NF=0.897646 VAF=10
+IKF=0.410821 ISE=3.0484e-09 NE=4 BR=0.1
+NR=1.00903 VAR=1.92063 IKR=4.10821 ISC=1.94183e-12
+NC=3.92423 RB=8.70248 IRB=0.1 RBM=0.1
+RE=0.111394 RC=0.556972 XTB=1.76761 XTI=1
+EG=1.05 CJE=1.67272e-11 VJE=0.83191 MJE=0.23
+TF=3.573e-10 XTF=0.941617 VTF=9.22508 ITF=0.0107017
+CJC=9.98785e-12 VJC=0.760687 MJC=0.345235 XCJC=0.9
+FC=0.49264 CJS=0 VJS=0.75 MJS=0.5
+TR=3.55487e-06 PTF=0 KF=0 AF=1

#### Attachments

• 1.9 KB Views: 0

#### LvW

Joined Jun 13, 2013
1,622
Because LTspcie is using the "correct" value for Early voltage. And I used the "corrupted" Multisim model. But in Mulitsim you can use a "better" model, try to use 2N2222A instead of 2N2222.
See my LTspice file with the "corrupted" model
Hi Jony - just for your information:
In PSpice there are two models with different Vaf values:
2N2222A: Vaf=74.03
2N2222A/ZTX (from Zetex): Vaf=104.

#### ericgibbs

Joined Jan 29, 2010
17,174
hi,
This is the Vaf that LTS shows for those types, Ic ~ 3.5mA.
E

Last edited:

#### MrChips

Joined Oct 2, 2009
28,151
Interesting. I redid the simulation on CircuitMaker 2000 using 2N2222A instead of 2N2222.

With 2N2222
With, R1 = 1875kΩ
VB = 0.613V
VC = 20.70V
Av = -320

With R1 = 1300kΩ
VB = 0.625V
VC = 15.76V
Av = -480

With R1 = 620kΩ connected to transistor collector
VB = 0.626V
VC = 15.12V
Av = -480

With 2N2222A
With, R1 = 1875kΩ
VB = 0.629V
VC = 14.68V
Av = -506

With R1 = 1300kΩ
VB = 0.639V
VC = 8.58V
Av = -662

With R1 = 620kΩ connected to transistor collector
VB = 0.633V
VC = 12.07V
Av = -550