Thermistor modelling

There are two basic types of thermistors:

NTC (resistance decreases as temperature rises - "negative temperature coefficient")
PTC (resistance increases as temperature rises - "positive temperature coefficient").

Resistance changes over temperature are usually not linear in a NTC thermistor. Manufacturers often characterises NTCs using Steinhart–Hart equation. Its simplified version is below:

A NTC thermistor has a nominal resistance of R₀ at temperature T₀. Resistance at temperature T is R(T). Every NTC also has a special property β, which is measured and given by NTC thermistor manufacturer (we usually find it in product datasheet, for example this one).

At first, we will create a subcircuit that will model our NTC thermistor. For this subcircuit the temperature will be one of the input parameters. Rememeber - we have to calculate the NTC resistance using a formula. We learned in previous session, how to tell SpiceOpus to calculate the parameter value, instead of interpret it (we use curly brackets, for ex.: "r={...}").
We will do some nasty tricks in this subckt, that will help us fully model our NTC at the end. The first one is this: we will not use element R to model the resistivity, but rather use a special element, called "nonlinear controlled source". As the name tells, we can use an expression to model a node voltage (or branch current). The following line encodes a nonlinear controled source (has to start with b, that will simulate resistance (its numerical value) between nodes r and 0.

	br r 0 v={r0}*exp({b}/({temp}+273) - {b}/(25+273))

Once we have a numerical value of thermistor resistivity, we can read it from the node r, with v(r,0). Now, if we want to include this thermistor subcircuit to another circuit, it has to look like a two-pole element from the outside. Another thing - some circuit will apply some voltage between the thermistor terminals - this means, our thermistor has to "produce" electrical current, that applies to applied voltage (considering, of course, parameters e.g.: temperature). So, we need to place a current source between the thermistor terminals. You can of course use a nonlinear controled source you just learned about, like this (current is voltage vs. resistance):

	bl 2 n i=v(p,n)/v(r)

Now your netlist probably looks something like this:

	.subckt ntc p n param: temp=25 b=3988 r0=4700
	vi p 2 dc=0
	bl 2 n i=v(p,n)/v(r)
	br r 0 v={r0}*exp({b}/({temp}+273) - {b}/(25+273))
	.ends

Now you are able to model just anything in Spice, as long as you have an equation for it.

Thermistor self-heating

Power dissipation of the NTC causes the same element to heat-itself-up (!) - so its resistance changes again! We improve the model in such manner, that input parameter temp is no-longer needed, but is calculated during the transient analysis. The self-heating part is a circuit which models the temperature change (the temperature is represented by the node T voltage!). The current in this circuit actually represents dissipated power (v(p,n)*i(Vi)). The independent voltage source represents the initial temperature (25 degrees C). There are also thermal resistance and thermal capacity, which are properties of NTC body and environment. Using this configuration we will model changes in NTC resistance during time, when pulses are applied to the NTC.