The simulator supports the specification of voltage and current initial conditions on capacitor and inductor models, respectively. These models are not the standard ones supplied with SPICE3, but are in fact code models that can be substituted for the SPICE models when realistic initial conditions are required. For details please refer to Chapter 12. A XSPICE deck example using these models is shown below:

*

* This circuit contains a capacitor and an inductor with

* initial conditions on them. Each of the components

* has a parallel resistor so that an exponential decay

* of the initial condition occurs with a time constant of

* 1 second.

*

a1 1 0 cap

.model cap capacitor (c=1000uf ic=1)

r1 1 0 1k

*

a2 2 0 ind

.model ind inductor (l=1H ic=1)

r2 2 0 1.0

*

.control

tran 0.01 3

plot v(1) v(2)

.endc

.end