PSpice transistor simulation issue

Thread Starter

mat2ag

Joined Jun 20, 2018
9
I designed very simple CE amplifier with 2n2222 in PSpice. Ic is about 400mA and transistor is in linear domain but calculated g_m is far from simulated one.
g_m=Ic/Vt => g_m = 400mA/25mV = 16
ic = g_m * vbe => ic = 16 * 0.01 = 0.16 mA but ic is about 44 mA

Screen Shot 2020-05-08 at 11.29.10 PM.pngScreen Shot 2020-05-08 at 11.36.20 PM.pngScreen Shot 2020-05-08 at 11.37.45 PM.png
 

Papabravo

Joined Feb 24, 2006
13,688
I suppose that would be due to the model you are using. Why would you expect this parameter to fall in any kind of narrow range. A transistor is not a transconductance amplifier like a MOSFET. A transistor converts a small base current int a large collector/emitter current. Even if this were a MOSFET, you would not find g_m to be well controlled or even well characterized.
 

Thread Starter

mat2ag

Joined Jun 20, 2018
9
I suppose that would be due to the model you are using. Why would you expect this parameter to fall in any kind of narrow range. A transistor is not a transconductance amplifier like a MOSFET. A transistor converts a small base current int a large collector/emitter current. Even if this were a MOSFET, you would not find g_m to be well controlled or even well characterized.
Dear Papabravo
What do you mean of model? Hybrid Pi model is a general model which describe the behavior of transistors both mos and bjt in small signals. The variation of collector current depends to base current but here dc beta is near 80 and ac beta is near 50 (as you can see in attached images) why? if so how can predict the collector current and gain?
 

Papabravo

Joined Feb 24, 2006
13,688
Dear Papabravo
What do you mean of model? Hybrid Pi model is a general model which describe the behavior of transistors both mos and bjt in small signals. The variation of collector current depends to base current but hear dc beta is near 80 and ac beta is near 50 (as you can see in attached images) why? if so how can predict the collector current and gain?
Yes but spice does not use the hybrid-pi model to solve transistor circuits. The collector current in a CE configuration is determined by the collector/emitter resistor(s) and Vcc. The gain of an amplifier stage should not depend on poorly controlled device parameters. Also the voltage at the base is constrained to be no more than 0.6 to 0.7 volts above the emitter. Thus ist makes a poor transconductance (voltage to current) amplifier.
 

Thread Starter

mat2ag

Joined Jun 20, 2018
9
Yes but spice does not use the hybrid-pi model to solve transistor circuits. The collector current in a CE configuration is determined by the collector/emitter resistor(s) and Vcc. The gain of an amplifier stage should not depend on poorly controlled device parameters. Also the voltage at the base is constrained to be no more than 0.6 to 0.7 volts above the emitter. Thus ist makes a poor transconductance (voltage to current) amplifier.
Using the model should not affect the result. I want to predict the collector current swing by knowing the input signal. and also "The collector current in a CE configuration is determined by the collector/emitter resistor(s) and Vcc" is not correct, Ic is a function of Ib.
 

Papabravo

Joined Feb 24, 2006
13,688
Using the model should not affect the result. I want to predict the collector current swing by knowing the input signal. and also "The collector current in a CE configuration is determined by the collector/emitter resistor(s) and Vcc" is not correct, Ic is a function of Ib.
The behavior you see from a Spice program is probably due to the Gummel-Poon or similar models. The parameters selected for the spice simulation are specified for the 2N2222 and plugged into the model. The "beta" certainly is a factor in the gain of an amplifier, but as you know it is not controlled very well from part to part and can vary over a wide range. Therefore a good designer will have the actual gain of the amplifier depend on parts whose value can be controlled with very tight tolerances. These parts would be resistors. In the case of the CE amplifier it is Rc and Re an d whetehr Re is bypassed that controls the gain.
 

Thread Starter

mat2ag

Joined Jun 20, 2018
9
The behavior you see from a Spice program is probably due to the Gummel-Poon or similar models. The parameters selected for the spice simulation are specified for the 2N2222 and plugged into the model. The "beta" certainly is a factor in the gain of an amplifier, but as you know it is not controlled very well from part to part and can vary over a wide range. Therefore a good designer will have the actual gain of the amplifier depend on parts whose value can be controlled with very tight tolerances. These parts would be resistors. In the case of the CE amplifier it is Rc and Re an d whetehr Re is bypassed that controls the gain.
You are right. But I want to extend the design and calculations to RF PA which resistors can not be used as gain controllers.
 

Papabravo

Joined Feb 24, 2006
13,688
You are right. But I want to extend the design and calculations to RF PA which resistors can not be used as gain controllers.
Right. So generally an RF amplifier will operate in Class C. What that means is the the transistor will conduct for less than 1/2 of the cycle. It actually spends most of its time in cutoff. Scroll down to the discussion of Class C. One of the tricky things is that while the transistor is in conduction mode there is almost a DC short across the power supply.

https://www.electronics-tutorials.ws/amplifier/amplifier-classes.html
 

Bordodynov

Joined May 20, 2015
2,589
First of all. You made a mistake. The current should be 0.16A!
Second. Your formula doesn't take into account the parasitic ohmic resistance of the emitter. At these currents, it greatly reduces the steepness of the transistor.
Tip: Calculate the power dissipated on the transistor.
 
Last edited:

Thread Starter

mat2ag

Joined Jun 20, 2018
9
Right. So generally an RF amplifier will operate in Class C. What that means is the the transistor will conduct for less than 1/2 of the cycle. It actually spends most of its time in cutoff. Scroll down to the discussion of Class C. One of the tricky things is that while the transistor is in conduction mode there is almost a DC short across the power supply.

https://www.electronics-tutorials.ws/amplifier/amplifier-classes.html
class C amplifiers should be used as tuned amplifier and are not applicable in all cases.
 

Thread Starter

mat2ag

Joined Jun 20, 2018
9
First of all. You made a mistake. The current should be 0.16 Ah!
Second. Your formula doesn't take into account the parasitic ohmic resistance of the emitter. At these currents, it greatly reduces the steepness of the transistor.
Tip: Calculate the power dissipated on the transistor.
At first you are right. The current is 160mA. But would you explain second item. I mean that how emitter resistance affect the problem?
 

Papabravo

Joined Feb 24, 2006
13,688
You may or may not be aware that most RF Power amplifiers are Class C. It is precisely because they use tuned circuits that they are used in this application. I know for mine you have to select the band you will be operating on, and you really need an antenna with a low return loss.
 

Bordodynov

Joined May 20, 2015
2,589
I'll add it. In a real transistor, its steepness is reduced by ohmic resistance of the base body and the emitter body. On small currents they have little effect, but at high currents their bad effect is more. In spice models these are parameters rb and re.
 

Thread Starter

mat2ag

Joined Jun 20, 2018
9
I'll add it. In a real transistor, its steepness is reduced by ohmic resistance of the base body and the emitter body. On small currents they have little effect, but at high currents their bad effect is more. In spice models these are parameters rb and re.
Would you explain HOW? As PSpice ref. manual said (page 209-Bipolar transistor equations for DC current)
Ic = collector current = area·(Ibe1/Kqb - Ibc1/Kqb - Ibc1/BR - Ibc2), Where I can not find any trace of rb and re in it, however simulated current is about 1/4 of calculated one which I think it is far from the effect of sub ohmic resistance of emitter or base.
 

Bordodynov

Joined May 20, 2015
2,589
I don't use Pspice. Could you publish the spice parameters of the 2N2222A transistor that you used. I did not learn from the tutorials that you are using now (and I do not want to learn) and still I am successfully calculating and designing the circuits. With this model, I will clearly show the effects of the parameters I have specified.
 

Thread Starter

mat2ag

Joined Jun 20, 2018
9
I don't use Pspice. Could you publish the spice parameters of the 2N2222A transistor that you used. I did not learn from the tutorials that you are using now (and I do not want to learn) and still I am successfully calculating and designing the circuits. With this model, I will clearly show the effects of the parameters I have specified.
.model Q2N2222 NPN(Is=14.34f Xti=3 Eg=1.11 Vaf=74.03 Bf=255.9 Ne=1.307
+ Ise=14.34f Ikf=.2847 Xtb=1.5 Br=6.092 Nc=2 Isc=0 Ikr=0 Rc=1
+ Cjc=7.306p Mjc=.3416 Vjc=.75 Fc=.5 Cje=22.01p Mje=.377 Vje=.75
+ Tr=46.91n Tf=411.1p Itf=.6 Vtf=1.7 Xtf=3 Rb=10)
 

Bordodynov

Joined May 20, 2015
2,589
.model Q2N2222 NPN(Is=14.34f Xti=3 Eg=1.11 Vaf=74.03 Bf=255.9 Ne=1.307
+ Ise=14.34f Ikf=.2847 Xtb=1.5 Br=6.092 Nc=2 Isc=0 Ikr=0 Rc=1
+ Cjc=7.306p Mjc=.3416 Vjc=.75 Fc=.5 Cje=22.01p Mje=.377 Vje=.75
+ Tr=46.91n Tf=411.1p Itf=.6 Vtf=1.7 Xtf=3 Rb=10)
In fact, your calculation uses a different model! In order to adjust the working point, I set the temperature to 0.5 degrees Celsius. The bottom picture for the case of transistor model without base resistance is Rb=0.2020-05-12_11-24-11.png
 
Last edited:
Top