There is a strong difference in the results in the Qspice and LTspice programs when calculating the simplest circuit!


By default, LTspice, as any other SPICE, treats all diodes as snap diodes, i.e., diodes that instantly switch off once the stored charge depletes. This is utterly unrealistic.

Diodes have two charge storage mechanism: junction and diffusion capacitance. Cjo and m describe the junction capacitance. With the diode off, the more you reverse bias the diode, the farther the electrons and holes move from each other and the less junction capacitance. It’s the mechanism of a varactor diode.

But when the diode is forward biased, there are electrons and holes in the junction looking for each other to annihilate to effect the current through the junction. Those carriers make the diffusion capacitance. The more forward current through the diode, the more charge in the junction; hence the parameter that describes this charge has the units of time an is called TT. TT multiplied by the forward current is the charge in the junction that must be removed for the diode to stop conducting. A diode can be made to make this turn off extremely quick, causing an almost instantaneous stop in the current flow. These very special diodes are called snap diodes and are used in instrumentation to make exceeding fast pulses. For example, one can differentiate that abrupt stop in current to make a pulse just 100ps wide.

But most diodes are not snap diodes, even though SPICE treats all diodes as perfect snap diodes. You’ll never get a 1N4007 to turn off in 1ps as it will in most SPICE versions.

There have been a number of suggested ways to fix this shortcoming in SPICE. I use the parameter VP, which dampens the turn off. VP does not default to zero in QSPICE. If you want to duplicate the erroneous result of a standard SPICE in QSPICE, add VP=0 to your diode model.