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

#### Heroz

Joined May 29, 2022
31
I'm studying about bjt transistors and I have a question in fixed bias circuit below : When I analyzed this circuit first I calculated DC response but I didn't do that I measure DC response when V2 is 0 found that :

Ib=15.7uA , Ic = 3.73 mA.

And I calculated r'e :

( IE approximate to Ic )
= 26mV/IE.
= 6.67 ohm.

And I find voltage gain from :
A. = (Rc//RL)/r'e
= 4761/6.67
= 713
And I checked in Multisim found that it's not same as I calculated in Multisim they equal to 365 ( How I measure gain is Vout/Vin).
Where is my wrong why it's not same ?
Thank you ( sorry my English is not good )

#### dl324

Joined Mar 30, 2015
15,458
Welcome to AAC!

For starters, you have the transistor biased to saturate. Is this schoolwork?

EDIT: I missed the k multiplier on the base resistor...

Last edited:

#### Papabravo

Joined Feb 24, 2006
19,592
It is hard to know the source of the discrepancy. As you know the models used in a simulator are "supposed" to be an average representation of devices you might see in the wild. Unfortunately, there is no central authority that certifies the accuracy or suitability of simulation models. As we speak, I have 15 different models for the TIP31C NPN power transistor. Four of them are useful and the rest are just trash. Also, 26 mV is an estimate for the value of the thermal temperature:

$$V_{T}=kT/q$$

In practice the value can be in a range from 25 mV to 52 mV depending on the transistor's junction temperature.

It is good that you are asking these questions and keeping an eye on the results that you are seeing. I would suggest that the purpose of simulation is understanding, and NOT design verification. Your next step should be to test your simulation model to see how close you can get to the characteristics that are represented in the datasheet and then change the model to get results closer to what you see in practice.

ETA: 1875 kΩ = 1.875 MegΩ! I have to ask if that was your actual intention.
Oh, and please tell me that you're not trying to make an amplifier with the emitter connected to GROUND. Actually, it would have been good to show the whole schematic and not just a fragment. That's not going to work very well for you with those king of gain numbers. The base should be near Vcc/2 and you need an emitter resistor if you want to make an amplifier.

Last edited:

#### WBahn

Joined Mar 31, 2012
27,893
When I duplicated the schematic in LTSpice, I got an overall gain across the load of 535. I got a collector current of 3.47 mA, which is pretty close to yours and indicates that the default LTSpice model for the 2n2222 has about the same beta as yours. Your beta appears to be about 238 and mine is about 221.

In general, biasing a BJT this way is NOT a good way to do it -- it is way too sensitive to variations in beta. The data sheet shows that, at these collector currents, the beta can vary anywhere from 50 to 300. A value of beta puts your quiescent collector voltage at 26 V and while a beta of 300 drops it all the way down to 6.5 V. You want to use a voltage divider with a low enough Thevenin equivalent resistance to hold the base at the voltage you want and then use an emitter resistor to set the collector current to the desired value. This results in the circuit being largely independent of beta. If you need more gain that Rc/Re, bypass the emitter resistor with a capacitor.

You might check to see if Multisim has default values for the ESR of those caps, since 100 uF is getting up there.

• Papabravo

#### MrChips

Joined Oct 2, 2009
27,686
• Papabravo

#### Heroz

Joined May 29, 2022
31
It is hard to know the source of the discrepancy. As you know the models used in a simulator are "supposed" to be an average representation of devices you might see in the wild. Unfortunately, there is no central authority that certifies the accuracy or suitability of simulation models. As we speak, I have 15 different models for the TIP31C NPN power transistor. Four of them are useful and the rest are just trash. Also, 26 mV is an estimate for the value of the thermal temperature:

$$V_{T}=kT/q$$

In practice the value can be in a range from 25 mV to 52 mV depending on the transistor's junction temperature.

It is good that you are asking these questions and keeping an eye on the results that you are seeing. I would suggest that the purpose of simulation is understanding, and NOT design verification. Your next step should be to test your simulation model to see how close you can get to the characteristics that are represented in the datasheet and then change the model to get results closer to what you see in practice.

ETA: 1875 kΩ = 1.875 MegΩ! I have to ask if that was your actual intention.
Oh, and please tell me that you're not trying to make an amplifier with the emitter connected to GROUND. Actually, it would have been good to show the whole schematic and not just a fragment. That's not going to work very well for you with those king of gain numbers. The base should be near Vcc/2 and you need an emitter resistor if you want to make an amplifier.
I have a question How does you measure voltage gain in Multisim ?

#### Papabravo

Joined Feb 24, 2006
19,592
I have a question How does you measure voltage gain in Multisim ?
I am not familiar with Multisim, but if you have the means to extract the peak-to-peak value of an AC waveform, you obtain those values and take the ratio. Is there a quicker better faster way to do it? Probably.

#### Heroz

Joined May 29, 2022
31
Welcome to AAC!

For starters, you have the transistor biased to saturate. Is this schoolwork?

EDIT: I missed the k multiplier on the base resistor...
Yes, In my school work is to find voltage gain by A = (Rc//RL)/r'e
but when I checked in my sim it's not match my calculation.

#### Papabravo

Joined Feb 24, 2006
19,592
Yes, In my school work is to find voltage gain by A = (Rc//RL)/r'e
but when I checked in my sim it's not match my calculation.
There is no a priori reason why the two should match. In order for that to happen both methods would need to use the same set of assumptions and we're not sure what assumptions the simulator is making. We do know the values of Rc and RL, but we don't know what value of r'e the simulator is using. The value of r'e depends on the value of

$$V_{T}$$

You could try changing the temperature of the simulation to see the effect.

#### Heroz

Joined May 29, 2022
31
It is hard to know the source of the discrepancy. As you know the models used in a simulator are "supposed" to be an average representation of devices you might see in the wild. Unfortunately, there is no central authority that certifies the accuracy or suitability of simulation models. As we speak, I have 15 different models for the TIP31C NPN power transistor. Four of them are useful and the rest are just trash. Also, 26 mV is an estimate for the value of the thermal temperature:

$$V_{T}=kT/q$$

In practice the value can be in a range from 25 mV to 52 mV depending on the transistor's junction temperature.

It is good that you are asking these questions and keeping an eye on the results that you are seeing. I would suggest that the purpose of simulation is understanding, and NOT design verification. Your next step should be to test your simulation model to see how close you can get to the characteristics that are represented in the datasheet and then change the model to get results closer to what you see in practice.

ETA: 1875 kΩ = 1.875 MegΩ! I have to ask if that was your actual intention.
Oh, and please tell me that you're not trying to make an amplifier with the emitter connected to GROUND. Actually, it would have been good to show the whole schematic and not just a fragment. That's not going to work very well for you with those king of gain numbers. The base should be near Vcc/2 and you need an emitter resistor if you want to make an amplifier.
Thank you .This is my school work and they want me to calculated voltage gain .
I calculated by A = (Rc//RL)/r'e.
I have one doubt. So it means that my model not match to spice model right? therefore my result not math.

#### Papabravo

Joined Feb 24, 2006
19,592
Thank you .This is my school work and they want me to calculated voltage gain .
I calculated by A = (Rc//RL)/r'e.
I have one doubt. So it means that my model not match to spice model right? therefore my result not math.
That is essentially what I am saying. If you and the simulator, make different assumptions you should expect different results.

#### WBahn

Joined Mar 31, 2012
27,893
Show a screenshot of the actual output waveform you got. It seems strange that your measured gain is almost exactly half what was expected.

#### WBahn

Joined Mar 31, 2012
27,893
There is no a priori reason why the two should match. In order for that to happen both methods would need to use the same set of assumptions and we're not sure what assumptions the simulator is making. We do know the values of Rc and RL, but we don't know what value of r'e the simulator is using. The value of r'e depends on the value of

$$V_{T}$$

You could try changing the temperature of the simulation to see the effect.
It's worth checking (or better, worth explicitly setting) the temperature. But nearly all simulators default to a temperature of 300 K (basically 27° C) and I'm pretty sure this is true for MultiSim, as well.

While you're at it, label the transistor base and collector nodes and take screenshots of those voltages, as well. And you might pull off the load resistor and output capacitor for now, just to eliminate as many variables as possible.

#### WBahn

Joined Mar 31, 2012
27,893
You might try downloading and installing LTSpice. The learning curve to run a simulation like this is pretty short. I have found that LTSpice does a pretty good job of matching what I expect for the limited use I have made of it thus far. I only used MultiSim very briefly many years ago, and I was not impressed by the quality of its built-in models. That may or may not be at play here.

#### Heroz

Joined May 29, 2022
31
You might try downloading and installing LTSpice. The learning curve to run a simulation like this is pretty short. I have found that LTSpice does a pretty good job of matching what I expect for the limited use I have made of it thus far. I only used MultiSim very briefly many years ago, and I was not impressed by the quality of its built-in models. That may or may not be at play here.
Here Vbe and Vce drop : Does my output waveform match your output ? In practical it should be 535 right? So my calculation can predicts voltage gain right but more percentage error .

Last edited:

#### WBahn

Joined Mar 31, 2012
27,893
Here Vbe and Vce drop :

View attachment 279130

Does my output waveform match your output ? In practical it should be 535 right? So my calculation can predicts voltage gain right but more percentage error .
My Vb is 685.5 mV and my Vc is 12.671 V. These differences are consistent with the previously identified difference that your beta is 238 and mine is 221, both of which are well within the realm of reasonable values for this transistor at room temperature.

What I'm interested in is seeing the AC waveform in the full circuit at key points of the base, the collector, and the load (the 100 kΩ load).

How long are you running the simulation for? It could be that you are not letting the circuit reach sinusoidal steady state. It's going to take quite a few cycles for those caps to reach that point. Let it run for a few seconds and take your measurements after at least a second has elapsed.

#### LvW

Joined Jun 13, 2013
1,586
Quote Heroz:
"In my school work is to find voltage gain by A = (Rc//RL)/r'e
but when I checked in my sim it's not match my calculation. "

As mentioned already, the gain formula

A=-(Rc||RL)/re=-gm(Rc||RL)

is an often used simplified expression, which neglects some additional effects which are covered in the models used in circuit simualors. (The influence of rce=1/hoe is only one example).
More than that, if we compare the simulation result with the above simplified expression we must not over-estimate the influence of B (resp. β) tolerances. By doing this, we have the β-model in mind (current-control) which does not give the correct view on the transistors working principle.
In fact, we have a voltage divider circuit (between R1 and the DC resistance of the B-E path) which creates the necessary voltage Vbe between base and emitter.
It is this voltage Vbe which is used in the Ebers-Moll equations (Gummel-Poon-model) which are the core of the BJT models in simulators.
Hence, no surprise that all the simplified equations we are using (Ic=B*Ib; gm=Ic/VT; A=-gm*(Rc||RL)...) are not in "good"accordance with the simulation results.

It is to be mentioned that the shown circuit does not contain negative signal feedback . It practice, we always use negative feedback - and the discreapency between simulation and (simplified) formulas wil be much smaller. This happens because negative feedback reduces the influence of the active device (and its tolerances, uncertainties) on the circuits gain.

Last edited:

#### WBahn

Joined Mar 31, 2012
27,893
I got to wondering if the discrepancy might be due to the small-signal output resistance of the transistor, so I swept Vc from 0 V to 30 V and, between 3 V and 30 V the collector current increased by 0.837 mA, making for an output resistance of about 32 kΩ. When this is put in parallel with Rc and Rload, it brings the effective value of the numerator from to 4762 Ω to 4330 Ω, which is a reduction of 9%. This would bring my anticipated gain down from 669 to 609. I lose another 3% in the voltage divider between the input capacitor and r_pi, bringing me down to 590. I'd love to account for the remaining difference between that and the 535 I got from my simulation, but in truth it's close enough that I satisfied that the simulation results are within reasonable agreement with my hand calculations.

• ericgibbs