Several types of circuit elements exhibit hysteretic behavior. Unfortunately, Spice simulation programs typically don't include an easy method to model such effects. For example, a simple neon light flasher is difficult to simulate with Spice without including hysteresis in the model for the neon bulb.
A neon flasher operates by charging through an RC, which determines the flash rate (Fig. 1). The bulb looks like an open circuit until the ionizing potential is reached. Once this has occurred, the bulb discharges and can be modeled as a simple linear resistor. However, the bulb acts as a resistor until the current through it falls below a holding level, even though the voltage across it drops below the ionizing potential. Modeling this behavior requires a resistor with hysteresis.
The heart of the resistor model consists of a comparator with hysteresis. The comparator may be modeled either by a Spice macromodel, or by building up a comparator from discrete elements. Figure 2 depicts a hysteretic comparator that implements the behavior required by the neon bulb model. The switching transistor is included to switch RH in and out of the circuit at the appropriate times, thus simulating the desired hysteresis.
Operation of this circuit is as follows: Until the input voltage to the comparator exceeds 65 V, the output remains high. This keeps RH switched out of the circuit. Once the input voltage exceeds 65 V, the output of the comparator goes low, switching in RH. The output remains low until the comparator input falls below the hysteresis level of the comparator (that is, 10 V).
Consider a neon bulb with the following parameters: VON = 65 V; RON = 1k; ROFF = 10M; hysteresis = 55 V (the bulb remains on until the voltage across it drops below 10 V).
The period of the charge/discharge cycle of the bulb then can be computed approximately by solving the following for t:
VBULB(t) = VIN (1 − e-t/t)
Thus, t = 1.28t and the flash rate is approximately 1/t.
The Spice transient simulation of the neon flasher is shown in Figure 3. The Spice macromodel developed for the resistor can be employed when simulating other application circuits that require a resistance with a prescribed amount of hysteresis.