Protel99SE/LTspice with different results?

[RA]

Hello to everyone,
I have been trying to get Protel99SE to calculate the input
impedance of a simple circuit. Literally a 2n2222 with
a 10k from +5V to the collector, a 2k from the emitter
to ground and a current source from ground to the base DC 1A.
Assuming a beta of 200 the input impedance looking into
the base would be Zin = (beta + 1)*Remitter = 201*2k = 402k.
When I run the simulation I get:
Protel99SE 128.94k
LTspice 425.54k
None of them are ok, but I would pick LTspice if would have
to pick one. I'm posting here the netlist for both of them,
maybe someone can point out where I'm screwing up the whole
thing.
Thanks for taking your time and reading this.
Best regards
Reinaldo Alvares

PROTEL99SE NETLIST

*SPICE Netlist generated by Advanced Sim server on 6/2/2004 9:41:33 AM
*for: Impedance.nsx

*Schematic Netlist:
I1 0 2 1u AC 1
Q1 NetR1_2 2 NetR2_1 2N2222
R1 NetV1_1 NetR1_2 10k
R2 NetR2_1 0 2k
V1 NetV1_1 0 +5V AC 0 0

..SAVE 0 2 NetR1_2 NetR2_1 NetV1_1 I1[v] V1#branch @V1[z] @Q1[ib] @Q1[ic]
@Q1[ie]
..SAVE @R1 @R2 @I1[p] @Q1[p] @R1[p] @R2[p] @V1[p]

*PLOT AC -1 1 A=2
*PLOT OP -1 1 A=2

*Selected Circuit Analyses:
..AC LIN 100000 10 1E8
..OP

*Models and Subcircuit:
..MODEL 2N2222 NPN (IS=81.2F NF=1 BF=195 VAF=98.6 IKF=0.48 ISE=53.7P NE=2
BR=4
+ NR=1 VAR=20 IKR=0.72 RE=64.4M RB=0.258 RC=25.8M XTB=1.5 CJE=89.5P VJE=1.1
+ MJE=0.5 CJC=28.9P VJC=0.3 MJC=0.3 TF=530P TR=368N)

..END

******************** LTSpice NETLIST **************************
* C:\Program Files\LTC\SwCADIII\Draft6.asc

R1 N003 N001 10k

R2 N002 0 2k

I1 0 2 1µ AC 1

Q1 N001 2 N002 0 2N2222

V1 N003 0 5

..model NPN NPN

..model PNP PNP

..lib C:\Program Files\LTC\SwCADIII\lib\cmp\standard.bjt

..ac lin 100000 10 100Meg

..backanno

..end

******** 2N2222 Model *******

..model 2N2222 NPN(IS=1E-14 VAF=100 BF=200 IKF=0.3 XTB=1.5 BR=3 CJC=8E-12
CJE=25E-12 TR=100E-9 TF=400E-12 ITF=1 VTF=2 XTF=3 RB=10 RC=3 RE=1 Vceo=30
Icrating=800m mfg=Philips)

 

[RA]

Well, now I know why Protel99SE and LTspice were giving
different results. all was in the model for the 2N2222
transistor. When I plugged the LTspice model into the
Protel99SE netlist I got the same results!! Now the
question is: what exactly makes the Protel99SE model
behave so wrong? It must be my ignorance and I'd be
happy to understand what might be my mistake. In any
case I used the standard models coming with the software.
But the LTspice comes closer to what it should be, although
not exactly, but pretty much.
As before, thanks for any replies.
Best regards
Reinaldo Alvares

 

[Ken Smith]

to ground and a current source from ground to the base DC 1A.

1 Amp into the BASE!

 

[RA]

Thanks Ken for your reply,
However the 1 Amp into the *BASE* is nothing else
than a commodity to simplify the readings from
the AC small signal analysis chart. You see, the input
impedance Zin = Vin/Iin, if you make Iin = 1A
then for every volt you get on the base you will
have an Ohm of input impedance. Further more if
you change the current source AC to 1mA the Zin
doesn't change, you just get instead of 425kV
425V, nothing else.
Z = 425E3(V)/1(A)= 425E3 Ohms
Z = 425(V)/1E-3(A) = 425E3 Ohms
don't loose from sight that the DC bias is only 1E-6 Amp.
So, unfortunately this is not the issue why the
Protel99SE model doesn't work properly. I will have
to dig into the model and understand it well before
using it. I think, I should have done that from the
beginning :-/
Thanks anyway for trying to help.
Best regards
Reinaldo Alvares

 

[Damir]

Hello to everyone,
I have been trying to get Protel99SE to calculate the input
impedance of a simple circuit. Literally a 2n2222 with
a 10k from +5V to the collector, a 2k from the emitter
to ground and a current source from ground to the base DC 1A.
Assuming a beta of 200 the input impedance looking into
the base would be Zin = (beta + 1)*Remitter = 201*2k = 402k.
When I run the simulation I get:
Protel99SE 128.94k
LTspice 425.54k
None of them are ok, but I would pick LTspice if would have
to pick one. I'm posting here the netlist for both of them,
maybe someone can point out where I'm screwing up the whole
thing.
Thanks for taking your time and reading this.
Best regards
Reinaldo Alvares

Hello Reinaldo.
Try to simulate with 2.8kHz starting frequency in LTspice.
Best Regards,

Damir

 

[Helmut Sennewald]

Hello to everyone,
I have been trying to get Protel99SE to calculate the input
impedance of a simple circuit. Literally a 2n2222 with
a 10k from +5V to the collector, a 2k from the emitter
to ground and a current source from ground to the base DC 1A.
Assuming a beta of 200 the input impedance looking into
the base would be Zin = (beta + 1)*Remitter = 201*2k = 402k.
When I run the simulation I get:
Protel99SE 128.94k
LTspice 425.54k
None of them are ok, but I would pick LTspice if would have
to pick one. I'm posting here the netlist for both of them,
maybe someone can point out where I'm screwing up the whole
thing.

Hello Reinaldo,
it is not a question of the simulator. It's simply a
question of the transistor model. You will get the Rin=128k
with LTSPICE, if you use the 2N2222 model from Protel.
I am shure that both simulators will show exactly the same
result, if you use the same model.

You will get about 405k if you remove "ISE=53.7P" from the
Protel 2N2222 model. The PSPICE Q2N2222 has ISE=14.34f which
is 4000 times less than in the Protel model.

Best Regards,
Helmut

Remove the line "+ ISE=53.7p" from the protel model.
VJE and MJE seem to be also too high in the Protel model.

*PROTEL
..MODEL 2N2222 NPN (IS=81.2F NF=1 BF=195 VAF=98.6 IKF=0.48
+ ISE=53.7P
+ NE=2 BR=4
+ NR=1 VAR=20 IKR=0.72 RE=64.4M RB=0.258 RC=25.8M XTB=1.5
+ CJE=89.5P VJE=1.1
+ MJE=0.5 CJC=28.9P VJC=0.3 MJC=0.3 TF=530P TR=368N)


*LTSPICE
..model 2N2222 NPN(IS=1E-14 VAF=100 BF=200 IKF=0.3 XTB=1.5
+ BR=3 CJC=8E-12
+ CJE=25E-12 TR=100E-9 TF=400E-12 ITF=1 VTF=2 XTF=3
+ RB=10 RC=3 RE=1)


*PSPICE DEMO Version V10
..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)

 

[RA]

Thanks Damir,
It simulates well in LTspice, the problem actually
is the model of the transistor not the setup, not
even the simulator.
Thanks again for your time
Best regards
Reinaldo Alvares

 

[RA]

Thank you very much Helmut,
I understood the problem was in the transistor model, but
I didn't know what exactly it was. You pointed out correctly
,it was exactly as you said. When I changed the ISE value
in the Protel99SE model to 14.34f, I got the proper value.
One interesting thing I observed was that the Protel99SE
model with ISE = 14.34f gave a better result than the LTspice
model! I got 405.19kOhms which is much closer to the 402kOhms
I calculated.
One more time, thanks a lot. I will change the model in my
Protel99SE package.
Best regards
Reinaldo Alvares