Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

PSpice transistor simulation issue

Status
Not open for further replies.
Can you post a copy of the used 2N2222A model? It's apparently different from the Ltspice model.
 

Can you post a copy of the used 2N2222A model? It's apparently different from the Ltspice model.

In PSpice when I right click on 2n2222 and select "edit PSpice model" it shows 2 models and I think it uses second one:
1.
.model Q2N2222A 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)
* National pid=19 case=TO18
* 88-09-07 bam creation

2.
Screen Shot 2020-05-16 at 12.19.10 AM.png

- - - Updated - - -

Can you post a copy of the used 2N2222A model? It's apparently different from the Ltspice model.

I also test LTspice with this model and result it very near PSpice.
Screen Shot 2020-05-16 at 12.52.32 AM.png
 

I think the source of problem is here but I don't know why?
We know that Ic = Is*exp(Vbe/Vt) but by this equation Ic = 14.34e-15 * exp(0.878/0258) = 3.5A which to far from reality.
.
 

The graphs in the datasheet for your 2N222A and your simulator both guess that you have transistor with "typical" spec's. But then all transistors you buy with spec's less than typical but still pass the written minimum spec's will not work. Is that a good or a bad way to design a circuit? I always design so that every passing transistor works perfectly, not just some transistors. Also, your biasing with only one resistor to the rail will not work with a transistor with low or high but passing hFE.

The written spec's say that with a collector current of 500mA and a 50mA base current then some of them have a terrible saturation voltage loss of 1V but a typical one needs less base current and still works much better.

You overloaded a 2N3904 transistor with too much current and too much heating and you said that the simulator said it was fine. You used 290mA but the datasheet says "Absolute maximum collector current= 200mA" and your heating was 290mA x 4V= 1.16W nut the datasheet says "Absolute maximum dissipation= 625mW". Your simulator cannot smell the smoke and does not care about overloads.
 

The graphs in the datasheet for your 2N222A and your simulator both guess that you have transistor with "typical" spec's. But then all transistors you buy with spec's less than typical but still pass the written minimum spec's will not work. Is that a good or a bad way to design a circuit? I always design so that every passing transistor works perfectly, not just some transistors. Also, your biasing with only one resistor to the rail will not work with a transistor with low or high but passing hFE.

The written spec's say that with a collector current of 500mA and a 50mA base current then some of them have a terrible saturation voltage loss of 1V but a typical one needs less base current and still works much better.

You overloaded a 2N3904 transistor with too much current and too much heating and you said that the simulator said it was fine. You used 290mA but the datasheet says "Absolute maximum collector current= 200mA" and your heating was 290mA x 4V= 1.16W nut the datasheet says "Absolute maximum dissipation= 625mW". Your simulator cannot smell the smoke and does not care about overloads.

Dear friend
I used 2n2222 transistor not 2n3904 and maximum current of 2n2222 is about 800mA and here it passes about 400mA and Vce>2 so it is not in saturation region. Also I know that single resistor bias is not good, but here it is not the case. My question is although the transisto is not saturated, hybrid pi model relations did not work at all.
 

You find different spec's and different models because your 2N2222A in a metal case(!) is VERY old (58 years old). The transistor in your simulation is a little better than "typical" and is close to saturation. If you buy some then a few will be in saturation.
Its maximum allowed collector current is 800mA but its spec's and graphs show that a typical one works poorly above 300mA.

Your circuit is unreal with such a high amount of heating. Your transistor is heating with 410mA x 2.2V= 900mW but its absolute maximum allowed dissipation (in a room that is not warm) is only 500mW.
If your 2N2222A transistor has a little lower current gain than typical so that it conducts 250mA then in your circuit the collector voltage will be 6V and the transistor will smoke and burn with 3 times (!) the maximum allowed dissipation. But your simulator cannot see or smell the smoke.

Basically, if you need a power transistor then use a power transistor. And bias it correctly.
 

You find different spec's and different models because your 2N2222A in a metal case(!) is VERY old (58 years old). The transistor in your simulation is a little better than "typical" and is close to saturation. If you buy some then a few will be in saturation.
Its maximum allowed collector current is 800mA but its spec's and graphs show that a typical one works poorly above 300mA.

Your circuit is unreal with such a high amount of heating. Your transistor is heating with 410mA x 2.2V= 900mW but its absolute maximum allowed dissipation (in a room that is not warm) is only 500mW.
If your 2N2222A transistor has a little lower current gain than typical so that it conducts 250mA then in your circuit the collector voltage will be 6V and the transistor will smoke and burn with 3 times (!) the maximum allowed dissipation. But your simulator cannot see or smell the smoke.

Basically, if you need a power transistor then use a power transistor. And bias it correctly.

There is no real transistor and everything is in simulator. Its bias is correct since it is in power amplifier mode. Problem is that in simulation nothing works correctly (in real world I don't know what will happen). Smoking is not my consideration here and also simulator can check for it but now it is not the case. At last I use this transistor since all parameter is known, this setup is also done with some power transistors and there is no meaningful difference.
 

The Mororola datasheet for the 2N2222A also has most of its spec's the same for the 2N2219A that is in a larger metal case. Years ago a heatsink was made for the 2N2219A.
 

In PSpice when I right click on 2n2222 and select "edit PSpice model" it shows 2 models and I think it uses second one:
1.
.model Q2N2222A 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)
* National pid=19 case=TO18
* 88-09-07 bam creation

2.
View attachment 159391

- - - Updated - - -



I also test LTspice with this model and result it very near PSpice.
View attachment 159392

I will correct my last post. With same model PSpice and LTspice have the exact same result.
 

Thanks for reporting. I have no doubts that the simulation result corresponds exactly to the transistor behaviour described by the model. The question is how the model differs from the simplified equations you are using for comparison.
 

Thanks for reporting. I have no doubts that the simulation result corresponds exactly to the transistor behaviour described by the model. The question is how the model differs from the simplified equations you are using for comparison.

Nice, Exactly that's right.
 

There are several parameters that affect the transconductance of a bipolar transistor. Many of them are already pointed out:

--- Re emitter series resistance (RE = 0 in your model then no reduction)

--- Rb base series resistance. In your model RB = 10 then a quite high reduction is expected since it is in series with the input resistance of bjt (Rpi). We know that Rpi = beta/gm = 255/16 = 16 ohm (I used the gm you calculated). So the actual Vbe seen by the transistor is 16/26 = 0.6*Vbe

--- VA early voltage (reduction of roughly 1+Vce/VAF, in your case 1+2.2/74 = 1.03 negligible)

--- NF diffusion factor that is a multiplier of Vth (1 in your case, then non reduction)

--- IKF high injection knee. When Ic is exceeding this value the gain starts compress (in your case IKF = 285mA while Ic = 400mA that means strong compression)

Just to try you can modify the model removing IKF (IKF=0 that means infinite) and RB=0 then change the biasing base resistor in order to have the same Q point of before and see if now Ic = gm*Vbe
Be careful the input voltage (now 10m) will not be too high, I'll try with 1m.
 
  • Like
Reactions: mat2ag

    mat2ag

    Points: 2
    Helpful Answer Positive Rating
There are several parameters that affect the transconductance of a bipolar transistor. Many of them are already pointed out:

--- Re emitter series resistance (RE = 0 in your model then no reduction)

--- Rb base series resistance. In your model RB = 10 then a quite high reduction is expected since it is in series with the input resistance of bjt (Rpi). We know that Rpi = beta/gm = 255/16 = 16 ohm (I used the gm you calculated). So the actual Vbe seen by the transistor is 16/26 = 0.6*Vbe

--- VA early voltage (reduction of roughly 1+Vce/VAF, in your case 1+2.2/74 = 1.03 negligible)

--- NF diffusion factor that is a multiplier of Vth (1 in your case, then non reduction)

--- IKF high injection knee. When Ic is exceeding this value the gain starts compress (in your case IKF = 285mA while Ic = 400mA that means strong compression)

Just to try you can modify the model removing IKF (IKF=0 that means infinite) and RB=0 then change the biasing base resistor in order to have the same Q point of before and see if now Ic = gm*Vbe
Be careful the input voltage (now 10m) will not be too high, I'll try with 1m.

Dear friend
your reply is right. By setting ikf=0, rb=0 and vin=1mv, then
gm = IC/Vt = 410.8/25.8=15.9
ic = gm*vbe = 15.9*0.001=15.9mA and by calculating from graph ic=(424mA-397mA)/2=13.5mA
Screen Shot 2020-05-20 at 1.50.46 AM.png

But now one question is remained, I have never seen IKF in data sheets. How can measure or calculate this such important parameter?
 

IKF is a parameter that indicates when the gain starts to decrease. In any case to correctly model a part (diodes, bjt, mos, etc.) I suggest to use the model parameter estimator you can find often embedded in the simulator.
 

The simple answer is, most datasheets don't have detailed data necessary to extract the questioned SPICE model parameters.
 

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top