2021: A Simulation Odyssey for Thermistors, Part 3

Let’s say you’ve built a new SPICE model – including all the voltage dependency and self-heating temperature effects – of a nonlinear component. Your model mimics the real characteristics of the component in simulations with DC voltage sources1. During large physical time transient simulations involving AC sources, however, you’ve noticed that the finalization time can be relatively long. As a tenacious engineer, you are exercising patience. But after ten minutes or more, patience starts to run out. Even worse, your progress can be impeded with pop-up messages like the one depicted in Figure 1.

Figure 1. A pop-up message indicates that the simulation has been interrupted.

You can then try a number of possible solutions2,3, but alas, the computation time only seems to increase while accuracy evaporates. At some point, you must face the fact that it’s time for a model reboot.

Now, it may be easier to state what a reboot should be for a superhero movie character than a SPICE model. My advice: rethink your model and simplify it. In doing so, combine as many characteristics as possible into continuous and derivable behavioral sources. And while you’re at it, you could take this opportunity to add new exciting features that will encourage users to look at it with a more considering eye.

The original positive temperature coefficient (PTC) model ( was built on the following equivalent circuit (Figure 2), which physically describes what a PTC is with its parallel voltage dependency:

Figure 2. An equivalent circuit of a PTC thermistor includes a voltage-dependent resistor (VDR) and a positive temperature coefficient (PTC).

The following equations apply to this circuit:

where: K and β are the VDR parameters (both dependent on the temperature  )

  • IVDR is the fraction of total current flowing through the VDR
  • R (TPTC) is the resistance temperature curve of the PTC (without VDR effect)
  • IPTC is the fraction of current that flows through the PTC
  • CTH and DTH are the thermal capacity and the dissipation coefficient of the PTC, respectively

Equations 1 to 3 are the electrical laws ruling the component. Equation 4 is the heat balance of the component.

Without entering into the details of transposing Equations 1 to 4 into the classical E, G, and H SPICE sources, we then have to deal with eleven behavioral sources, all interacting with each other.

After simplification, we reduce the model description to two equations:

The new model will not contain the VDR physical parameters of Equation 1, and the pure fitting function F of Equation 5 will be established on the basis of experimental measurements like the ones in Figure 34.


Figure 3. The apparent PTC resistance ratio is plotted as a function of the applied pulsed voltage.

The new symbol of this reboot model can be seen in Figure 4, as opposed to the models published in Ref. 2. The new feature is a pin indicating the internal temperature of the PTC (T5 node), which, we hope, will be very useful to designers.

Instead of leaving this temperature node hanging in the air, the LTspice symbol editor allowed for a cosmetic operation consisting of building a little internal thermometer, showing that it’s there that the component temperature can be measured.

Figure 4. A basic LTspice transient simulation will allow for reproducing the measured characteristics.

The next question: is the simplified model as valid as the former when evaluating the basic properties? To find out, we have to compare them in the same simulation conditions.

In this first transient simulation (Fig. 4), we apply a non-heating voltage pulse onto the PTCEL13R501RBE at very low and high voltage, and we let the SPICE error log file compute and represent graphically the instantaneous resistance vs temperature in Fig. 2.

The obtained curves are compared to the same measurements performed on the same simulation but using the classical models, which are exact replications of the physical measurements.

Now we see in Figure 5 that if the results of resistance for the reboot and normal models are identical in the 0 V condition over the whole temperature range, they only coincide for a 700 V pulse (orange and red curves) as long as the temperature does not exceed 170 °C. This inconvenience is fortunately not important for PTC protection; designers are mainly interested in what happens under, around, or just above the switch temperature, i.e. 140 °C. Above this temperature, the PTC resistance will be driven fully to very high ohmic values, the current circuit will decrease fast, and the PTC temperature is not likely to increase further. Reproducing everything that happens above 170 °C can easily be considered as a nice but not indispensable performance.

Figure 5. A comparison of the simulated results of old and new models, together with the measured PTC characteristics.

Let’s verify now how effective these models are in transient simulations with AC sources which is now possible in a reasonable time with our new models.

0 comments on “2021: A Simulation Odyssey for Thermistors, Part 3

Leave a Reply

This site uses Akismet to reduce spam. Learn how your comment data is processed.