anyone know anything about transistor model creation?

[kiki_barrios]

Go to tools, component wizard, follow the steps.

When you get to the symbol ( click copy from DB), locate in the master Database the transistor symbol you want to use, -next-

when you get to the step 5 ( click on model maker), select BJT for bipolar transistor model, now look carefully to the data sheet of your

transistor and copy all the important parameters and click ok, And voila, you alredy have your So hard to find Spice model. Update

the model name and click next.

Step 7 click on + of the database you want to save your component in, choose transistors, Click on add family button, coose a name you like and finish.

I hope this solve your problem,

Good luck

[lacy]

Thanks for your information. I have been there done that. The BJT Model makers ask for a bunch of information that isn't necessarily listed in the text parameters on the the Datsheet, but is contained in the curve data charts. These charts are not easy to read and the values on the graph can be interpreted 5 different ways. This doesn't help when trying to create an accurate model of a component.

If you have a different way of creating models in this manner, please let us know how you do it. Maybe we are missing some information concerning this that you may know that can help the rest of us.

Thanks for any info in advance.

[kiki_barrios]

**************************************
*      Model Generated by MODPEX     *
*Copyright(c) Symmetry Design Systems*
*         All Rights Reserved        *
*    UNPUBLISHED LICENSED SOFTWARE   *
*   Contains Proprietary Information *
*      Which is The Property of      *
*     SYMMETRY OR ITS LICENSORS      *
*    Modeling services provided by   *
* Interface Technologies www.i-t.com *
**************************************
.MODEL 2n3055 npn
+IS=2.37426e-14 BF=129.119 NF=0.85 VAF=31.1252
+IKF=0.990922 ISE=2.47498e-10 NE=1.89002 BR=1.01252
+NR=0.924456 VAR=254.624 IKR=2.70227 ISC=2.47498e-10
+NC=2.90624 RB=3.66609 IRB=0.1 RBM=0.1
+RE=0.000352673 RC=0.0764459 XTB=1.34801 XTI=1.07207
+EG=1.206 CJE=9.03089e-08 VJE=0.513954 MJE=0.59999
+TF=1e-08 XTF=1.36696 VTF=1.02605 ITF=0.987296
+CJC=5e-10 VJC=0.400243 MJC=0.410238 XCJC=0.803124
+FC=0.661216 CJS=0 VJS=0.75 MJS=0.5
+TR=1e-07 PTF=0 KF=0 AF=1
* Model generated on Jan 24, 2004
* Model format: SPICE3

[kiki_barrios]

Try that,mapping 1-collector 2-base 3-emitter.

q%p %tC %tB %tE %m

or  click on show table, is easier.

[EMC Guy]

This is a link to a very useful excel tool for modeling any transistor from its datasheet

 http://www.analogservices.com/excel.htm

[yyao]

To address one of your original questions, "q%p %tB %tC %tE %m" is the model template tells Multisim how to connect the a BJT. Multisim replaces %p with the RefDes and %C, %B, %E with the nets connected to the respective pins on the transistor and %m with the model name. However, you don't need to worry this at all because the Component Wizard creates this line for you.

I still think that the easiest way to create models is by using the component wizard. I hope these pointers will help you.

• When you come to step 3 of the Component Wizard, click on Copy from DB. Select any NPN transistor symbol such as the 2N2222.
• Since you already have the SPICE model, there is no need to use Model Maker in step 6. Paste your model into the Model Data box and remove any comments. The first line that you paste into the Model Data box must begin with .MODEL.
• If you have mixed up pin assignments, you may have misconfigured step 7. The symbol pin representing the collector must map to model pin #1, base with 2 and emitter with 3.

I have tried the Component Wizard and have been able to create the transistors based on your given models and they seem to simulate fine. I hope this helps. If you are confused about a particular step of this process, please let us know.

Message Edited by yyao on 02-02-2009 01:00 PM