How to make a capacitance variable with voltage in LTpice?

[Flyback]

Hi,
How to make a capacitance variable with voltage in LTpice?

You presumably do a .param {capacitance} = (V(aaa) - V(bbb)) * 10nF
?
But that doesnt work

 

[Papabravo]

The value of a parameter must be known before the simulation begins. A parameter can be .step'ped, but each step is a new simulation. You may find some happiness in defining a capacitor in terms of charge. Check the LTspice Help file.

C. Capacitor ​

There is also a general nonlinear capacitor available. Instead of specifying the capacitance, one writes an expression for the charge.​

​

LTspice will compile this expression and symbolically differentiate it with respect to all the variables, finding the partial derivative's that correspond to capacitances.​

​

Syntax: Cnnn n1 n2 Q=<expression> [ic=<value>] [m=<value>]​

​

There is a special variable, x, that means the voltage across the device. Therefore, a 100pF constant capacitance can be written as​

​

Cnnn n1 n2 Q=100p*x​

 

[Tony Stewart]

If you want a real part there are a couple of "Varicap" diodes in the library > diode> type>Varactor.

All diodes have max capacitance at 0V and decrease with reverse voltage in a logarithmic fashion. Varactor diodes are more precisely controlled for this attribute and specified by the C ratio and value at two voltages.

A high resistor value is used for biasing and large C is used in series when used to block the DC.

Generally the bigger the current rating or smaller Rs, or bigger power rating, the bigger the C(0V) capacitance.

 

[eTech]

Hi,
How to make a capacitance variable with voltage in LTpice?

You presumably do a .param {capacitance} = (V(aaa) - V(bbb)) * 10nF
?
But that doesnt work

Specify Q=10n*X for the value attribute

 

[Roff]

https://www.pspice.com/sites/default/files/PSpice%20App%20Note_Modeling%20Voltage-Controlled%20Resistors%20and%20Capacitors%20in%20PSpice.pdf