circuit modeling with multisim/circuitmaker

I use both multisim 9 student and circuitmaker 2000 student. I am
wondering why I get vastly different DC operating point results given
an exact duplicate transistor biasing scheme for each program? Not
being an engineer and coming from a strictly hobbiest point of
reference I'm at a loss to explain what's going on. The circuit is a
simple base-bias arrangement.

 

[Helmut Sennewald]

<tsal4@hotmail.com> schrieb im Newsbeitrag
news:1177863204.494645.14050@o5g2000hsb.googlegroups.com...

I use both multisim 9 student and circuitmaker 2000 student. I am
wondering why I get vastly different DC operating point results given
an exact duplicate transistor biasing scheme for each program? Not
being an engineer and coming from a strictly hobbiest point of
reference I'm at a loss to explain what's going on. The circuit is a
simple base-bias arrangement.

Hello,

I guess that each program has a different model definition for the
same transistor. The most important parameter for the DC-
bias point is the current gain B. If this is the case, you should
consider other resistor values for the bias point to achieve
less sensitvity regarding the current gain.
Real transistors will also have a lot of tolerance regarding this
parameter, e.g. B=50 to 200 @Ic=5mA.

You can send me your files for checking.
I think I have all these student versions on a harddisk.

Best regards,
Helmut

PS:
We had a discussion about other simulators over the last
days in this group. "Free electronics simulation software"
The following new simulator is advertised as free with unlmited
circuit size. It looks like this is a refreshed circuitmaker program.
Crcuitmaker-users shouldn't have a problem to run their
existing circuits with this simulator. Try your circuit with
this simulator too.
www.CircuitLogix.com


I personally use LTspice.
http://www.linear.com/designtools/software/switchercad.jsp
http://tech.groups.yahoo.com/group/LTspice/

 

This is the multisim 9 netlist:

rR1 1 3 1.100e+004

rR2 1 2 1.00e+002

qQ1 2 3 0 2N3904__BJT_NPN__1

VV1 1 0 dc 10 ac 0 0
+ distof1 0 0
+ distof2 0 0


..MODEL 2N3904__BJT_NPN__1 NPN(Is=6.734f Xti=3 Eg=1.11 Vaf=74.03
Bf=416.4 Ne=1.259
+ Ise=6.734f Ikf=66.78m Xtb=1.5 Br=.7371 Nc=2 Isc=0
Ikr=0 Rc=1
+ Cjc=3.638p Mjc=.3085 Vjc=.75 Fc=.5 Cje=4.493p Mje=.
2593 Vje=.75
+ Tr=239.5n Tf=301.2p Itf=.4 Vtf=4 Xtf=2 Rb=10)

This is the circuitmaker 2000 netlist:

Q1 Q1_1 Q1_2 0 Q2N3904
V1 V1_1 0 DC 10V
R2 Q1_1 V1_1 100
R1 Q1_2 V1_1 11k
..SAVE V1_1 Q1_2 Q1_1 @q1[p] @q1[ic] @q1[ib] @q1[ie] @v1[p] v1#branch
@v1[z]
..SAVE @r2[p] @r2 @r1[p] @r1

* Selected Circuit Analyses :
..OP
..TRAN 20n 5u 0 20n

* Models/Subcircuits Used:

*2N3904 Si 625mW 40V 200mA 300MHz pkg:TO-92B 1,2,3
..MODEL Q2N3904 NPN(IS=1.4E-14 BF=300 VAF=100 IKF=0.025 ISE=3E-13
+ BR=7.5 RC=2.4 CJE=4.5E-12 TF=4E-10 CJC=3.5E-12 TR=2.1E-8 XTB=1.5
KF=9E-16 )
..END

I do notice some differences in the transistor model variables but I
wouldn't know what they were or how they would effect the results.
The circuitmaker results match much more closely with what I would
expect (based on the transistor data sheet specs).

 

[Helmut Sennewald]

<tsal4@hotmail.com> schrieb im Newsbeitrag
news:1177937564.473528.16140@u30g2000hsc.googlegroups.com...

This is the multisim 9 netlist:

rR1 1 3 1.100e+004

rR2 1 2 1.00e+002

qQ1 2 3 0 2N3904__BJT_NPN__1

VV1 1 0 dc 10 ac 0 0
+ distof1 0 0
+ distof2 0 0


.MODEL 2N3904__BJT_NPN__1 NPN(Is=6.734f Xti=3 Eg=1.11 Vaf=74.03
Bf=416.4 Ne=1.259
+ Ise=6.734f Ikf=66.78m Xtb=1.5 Br=.7371 Nc=2 Isc=0
Ikr=0 Rc=1
+ Cjc=3.638p Mjc=.3085 Vjc=.75 Fc=.5 Cje=4.493p Mje=.
2593 Vje=.75
+ Tr=239.5n Tf=301.2p Itf=.4 Vtf=4 Xtf=2 Rb=10)

This is the circuitmaker 2000 netlist:

Q1 Q1_1 Q1_2 0 Q2N3904
V1 V1_1 0 DC 10V
R2 Q1_1 V1_1 100
R1 Q1_2 V1_1 11k
.SAVE V1_1 Q1_2 Q1_1 @q1[p] @q1[ic] @q1[ib] @q1[ie] @v1[p] v1#branch
@v1[z]
.SAVE @r2[p] @r2 @r1[p] @r1

* Selected Circuit Analyses :
.OP
.TRAN 20n 5u 0 20n

* Models/Subcircuits Used:

*2N3904 Si 625mW 40V 200mA 300MHz pkg:TO-92B 1,2,3
.MODEL Q2N3904 NPN(IS=1.4E-14 BF=300 VAF=100 IKF=0.025 ISE=3E-13
+ BR=7.5 RC=2.4 CJE=4.5E-12 TF=4E-10 CJC=3.5E-12 TR=2.1E-8 XTB=1.5
KF=9E-16 )
.END

I do notice some differences in the transistor model variables but I
wouldn't know what they were or how they would effect the results.
The circuitmaker results match much more closely with what I would
expect (based on the transistor data sheet specs).

Hello,

The curves shown in the datasheet are only typical values.
You have to design with the min/max values in the specification.

I simulated your circuit with the models above and with the model from
LTspice.
All three models give roughly one Volt difference in V(2). I simply guess
that
the three models are provided from three different manufacturers of the
2N3904.
This is not a simlator problem! It's a model issue only.

The most important parameter is BF and around them IKF and ISE.
I recommend to look in any SPICE manual about the bipolar transistor
for more details.

Best regards,
Helmut