How to model a polynomial voltage controlled current source?

[tpoche]

I am wondering if anyone knows how to model a voltage controlled current source who's relationship is defined as a polynomial function. The function is of the form: I(V) = c1*V^6 + c2*V^5 + c3*V^4 ... In PSpice there is a component called GPOLY which performs this exact function, but I prefer Multisim and would like to use it instead. Any help would be appreciated. Thanks, Trent

[nestor-sg]

I guess there are two options you might want to try:

1.  Place >> Component... >> Master Database >> Sources >> Control Function Blocks >> NONLINEAR_DEPENDENT

With this function block, you can create a formula based on voltage inputs, however, the dependant variable can be either V or I, for your purpose I would select 'I' right?. Check out its help file for info on how to use it.

2. The second option is a combination, you will need to use two components for what I've seen. First get the VOLTAGE_CONTROLLED CURRENT SOURCE which is in the Sources >> Controlled Current Sources folder. However, by its own this component only controls current based on 'one' voltage. So, the other component we need is the POLYNOMIAL_VOLTAGE which is in the Sources >> Control Function Blocks folder. So I guess you will first use the POLYNOMIAL_VOLTAGE component to create a voltage specified by the Poly Fn of other voltages, and then add the V controlled I Source based on the resulting voltage.

I don't experience using those components, but from what I saw on the help files I guess option 1 if you learn how to use it will be more efficient...  I hope this helps...

[Maxish]

Remember that behind any simulatable component is a SPICE stamp. It is very easy to create customized component with some knowledge of SPICE. For your case, do the following:

Make an analog component (using component wizard), with one input pin and two output pins. For the model you can use:
------------
 .subckt current_poly in out1 out2

*this will shoot a current from out1 to out2 equal to the evaluation of expression. V(in) is referenced to ground.
B1 out1 out2 I={c1*v(in)^6 + c2*v(in)^5 + c3*v(in)^4 }

.ends
-----------

[_user32]

In v9/v10 you can now add in LabVIEW based instruments.

In the "LabVIEW Virtual Instruments" section of the Multisim Technical Library there

is a LabVIEW VI allowing you to create an expression/equation as a voltage source into Multisim. 

http://zone.ni.com/devzone/cda/tut/p/id/5579