0
\$\begingroup\$

I'm trying to do a simulation on Microcap 12 using vendor provided models. The devices I'm trying to use in my schematic are the following:

2SA1312 2SC3324

I add the models via component editor as per this guide suggests.

After drawing my circuit, I try starting a transient simulation and this warning appears:

Warnings

Warning unknown parameter TNOM in model 2SA1312_BJT. Warning unknown parameter TNOM in model 2SC3324_BJT.

These warning are easily fixed by opening the model and removing (or commenting) the line related to TNOM.

After doing this, transient simulation actually goes through, but a quick check on the voltage nodes shows that these transistors are simply open circuits, since the voltages shown at their terminals are simply the power rails values.

Here's a simple example with a built-in model (2n2222):

enter image description here

And here's the same circuit but different transistor (for which I imported the model):

enter image description here

Notice that the voltage on the emitter is the negative rail.

Any advice on how to try to fix this problem?

\$\endgroup\$
3
  • \$\begingroup\$ Did you simply try to remove TMON? Because MON is a nominal temperature I suspect \$\endgroup\$
    – G36
    Mar 22 at 15:02
  • \$\begingroup\$ yes, to get the simulation working I had to comment/delete the line "+ TNOM = 25" off the model files. Not sure if this was the right thing to do or if it has any effect on the simulation issue I described. \$\endgroup\$
    – Qwerty8787
    Mar 22 at 15:10
  • \$\begingroup\$ I think microcap uses "TEMP" for temperature. \$\endgroup\$
    – Andy aka
    Mar 22 at 15:17
1
\$\begingroup\$

Why don't you just copy the "model text" directly into the model tab?

See here

.MODEL 2SC3324 NPN (BF=475 BR=28 CJC=4.9687e-012 CJE=3.0625e-011 FC=0.5 IKF=0.2
+ IKR=0.004 IS=1.3e-013 ISC=1.5e-010 ISE=3.5e-014 ITF=0.1 MJC=0.1914 MJE=0.33
+ NC=1.5 NE=1.3 NK=0.5 RB=2 RC=0.02 RE=0.25 TF=3e-010 TR=10E-09 TRC1=0.05
+ VAF=200 VAR=10 VJC=0.9247 VJE=0.75 VTF=5 XTB=1.5 XTF=50 XTI=4)

And

enter image description here

"model tab"

enter image description here

\$\endgroup\$
2
  • \$\begingroup\$ sorry I didn't see your answer before posting mine. Haven't tried the "models" tab before. That seems to work as you're showing. Not sure how the pinout is dealt with in this way. Since this is a part that I use often, having it fixed right at the component editor level is ultimately best since that would allow in future to just drag and drop the same part onto new schematics. Thank you very much for your input and help! \$\endgroup\$
    – Qwerty8787
    Mar 22 at 15:57
  • \$\begingroup\$ In the model's tab, you do not have to worry about the pinout. Because the "pure" model does not contain information about the pinout (simulation assumes standard pinout). In your case, you have used a .SUBCKT and this is why you have to worry about pinout. \$\endgroup\$
    – G36
    Mar 22 at 16:04
0
\$\begingroup\$

Apologies if "answering my own question" is not the right etiquette. First time ever I actually post a question here. I played a bit more and found the solution myself. I think it's useful to leave the solution here in case someone else is in the same situation.

The issue is pin numbering. When importing the model, I used the numbering suggested by datasheet for the physical package:

  1. Base
  2. Emitter
  3. Collector

I later noticed that on the model itself, the numbering system is different:

enter image description here

Went back into Component Editor and renumbered the part as per model:

enter image description here

Running the simulation gives good results now:

enter image description here

enter image description here

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.