Content

SPICE Analog Behavioral Modeling of Variable Passives (Part 2)

April 1, 2005

In part two of this three part article, PET outlines a technique to model variable capacitors.

For the PDF version of this article, click here. Click to read part I and part III of this article.

In part one of this article (see “SPICE Analog Behavioral Modeling of Variable Passives,” March 2005, Power Electronics Technology), a method for modeling a variable resistor within SPICE was described. Here in part two, a similar technique is applied to model variable capacitors.

As we did in the previous article with the resistor, a capacitor can be portrayed by a voltage source obeying the following law:

In other words, if we integrate the current flowing into our equivalent subcircuit capacitor and multiply it by the inverse of a control voltage V, we obtain a capacitor of value C = V. Unfortunately, there is no integral primitive in SPICE since it involves the variable t, which is continuously varying. Therefore, why not capitalize on the equation and force the subcircuit current into a 1-F capacitor? By observing the resulting voltage over this 1-F capacitor, we have integrated I_c(t). Fig. 1 shows how we can build the subcircuit.

In Fig. 1, the dummy source V routes the current into the 1-F capacitor, which develops the integrated voltage on the “int” node. Then, once multiplied by the inverse of the CTRL node voltage, it mimics our variable capacitor. Fig. 2 shows an actual test circuit used to verify the validity of our Spice model. Fig. 3 displays voltages and currents obtained from both the real capacitor and the variable one modelled in Spice. There is no difference between plots.

Below are the models in both IsSpice and PSpice:

IsSpice

.SUBCKT VARICAP 1 2 CTRL

R1 1 3 1u

VC 3 4

BC 4 2 V=(1/v(ctrl))*v(int)

BINT 0 INT I=I(VC)

CINT INT 0 1

.ENDS

PSpice

.SUBCKT VARICAP 1 2 CTRL

R1 1 3 1u

VC 3 4

EC 4 2 Value = { (1/v(ctrl))*v(int) |

GINT 0 INT Value = { I(VC) |

CINT INT 0 1

.ENDS

Tests also were run in ac analysis where the model confirmed its accuracy in the frequency domain.

About the Author

Christophe Basso

Christophe Basso is a Technical Fellow at ON Semiconductor in Toulouse, France, where he leads an application team dedicated to developing new offline PWM controller specifications. He has originated numerous integrated circuits among which the NCP120X series has set new standards for low standby power converters.

Further to his 2008 book “Switch-Mode Power Supplies: SPICE Simulations and Practical Designs”, published by McGraw-Hill, he released in 2012 a new title with Artech House, “Designing Control Loops for Linear and Switching Power Supplies: a Tutorial Guide”. His new book is dedicated to Fast Analytical Techniques and was recently published by Wiley in the IEEE-press imprint under the title “Linear Circuit Transfer Function: An Introduction to Fast Analytical Techniques”.Christophe has over 20 years of power supply industry experience. He holds 17 patents on power conversion and often publishes papers in conferences and trade magazines including How2Power and PET. Prior to joining ON Semiconductor in 1999, Christophe was an application engineer at Motorola Semiconductor in Toulouse. Before 1997, he worked as a power supply designer at the European Synchrotron Radiation Facility in Grenoble, France, for 10 years. He holds a BSEE equivalent from the Montpellier University (France) and a MSEE from the Institut National Polytechnique of Toulouse (France). He is an IEEE Senior Member.