# 2021: A Simulation Odyssey for Thermistors, Part 2

At the end of Part 1 of this article1 , it was mentioned that VHDL_AMS modeling allows designers to coordinate thermal and electrical designs. Indeed, after reading the article “Hot Topic: Electronic Thermal Design”2 , it’s clear that in a VHDL-AMS design, the heat production fluxes created by several transistors, other semiconductor elements, as well as heating elements can be directly injected into thermal RC networks modeling the heatsinks of these elements, or simply the ambient environment.

This allows for the computation of hot spots in the application and to properly design the various heat sinks.

An example of the heat production quantified devices can be seen in the off/off temperature sensing application in Figure 1 (Reference 3 provides the URL where the reader can simulate this circuit).

Figure 1 off/off temperature sensing

The resulting computed temperature (node: “achieved temp”) is then used as a feedback signal to control the heating elements via the Vishay NTCLE100 thermistor.

The computation of this heat power is built into the SystemVision Cloud VHDL AMS description models. And while it is straightforward for a fixed resistor, the computation is slightly more complicated for a transistor.

The idea of combining the didactic descriptive precision of VHDL-AMS with the speed of the best SPICE looks appealing, but who has the time? This was without counting on the fact that LTspice remains (partly) undocumented for some aspects, even after 20 years, and still divulges some secret resources. Take the circuit in Figure 2a. We would like to compute the power dissipated in the Q1 transistor. After the transient simulation, direct the mouse to Q1 and press “alt”. A green/red thermometer will appear near Q1 (Figure 2b). Left click on this and you not only get the power dissipated in Q1, you even get the formula used to perform it on the virtual oscilloscope.

Power= V(C,E) x Ic(Q1) + V(B,E) x Ib(Q1)

where

• C, E, and B nodes are the collector, emitter, and base nodes of Q1
• Ic(Q1) and Ib(Q1) are the collector and the base current of Q1, respectively
Figure 2 The same works for R2, for example. The power level for Q1 and R2 are represented in Figure 3.

Figure 3 The power level for Q1 and R2

So let’s go one step further. As it appears that LTspice offers engineers the same possibility for a coordinated thermal/electrical design as the VHDL-AMS, all we have to do now is build a thermal electronic database. Figure 4 illustrates how to do that. New devices can be easily created with the addition of a behavioral current source whose value is exactly given by the formula computed by LTspice. A heat source (in W) modelled as a current (in A) – it looks a bit awkward, but nevertheless, it works.

On the left part of Figure 4, we see the decomposed device, and on the right side, a new synthetic symbol of a thermal NPN transistor with the HEAT pin out.

Figure 4 Build a thermal electronic database

This current source (by this I mean “heat source”) can then be directly injected into a thermal RC network, which is a situation completely analog to what’s being done in SystemVision Cloud. The temperature of the system is the voltage at the node (syst) and changes exponentially from 25o C (where we have initiated it) until a high value, depending on the thermal resistance R10 (Figure 5).

Figure 5 The thermal resistance R10

As a last example, let’s examine the circuit of Figure 6, which is a temperature regulation circuit based on the Vishay VOT8125 TRIAC optocoupler. Note that the heat sink consists of a thermal resistor (o C/W) and a thermal capacitor (in J/o C) created for the occasion.

Figure 6 A temperature regulation circuit based on the Vishay VOT8125 TRIAC optocoupler

Figure 7a shows the transient variations of the heat sink and NTC temperature, with all elements having a Monte Carlo tolerance. Figure 7b shows the corresponding voltage variations, and the opamp U3 switch when V(NTC) reaches v(ref) , as well the hysteresis due to R9.

Figure 7a Transient variations of the heat sink and NTC temperature

Figure 7b The corresponding voltage variations, and the opamp U3 switch when V(NTC) reaches v(ref) , and the hysteresis due to R9

As a general conclusion, we see that SystemVision Cloud and LTspice both allow for a coordinated thermal/electrical design, in particular for thermistor-based circuits. Both achieve the same goal, albeit through different pathways.

In what concerns LTspice specifically, we started Part one of this article by mentioning that a device temperature in this software needed to be expressed in Volts sometimes, and now we end Part 2 with heat expressed as a current source. Well, engineers should be flexible nowadays, shouldn’t they? In the end, this waltz of the units would be cosmetically solved by using a trick discovered in the Reference 4. Let’s consider Figure 6 and suppose we want to display the power dissipated in the heating element U9 in W and the element temperatures in o C.

Let’s plot the trace expressions literally written as -I(V5)*1W/1A , then V(Tsystem)*1degC/1V etc. We then get the graph in Figure 8, where the power (dissipated in heat) and temperature quantities have gone back to their respective units.

Figure 8 The power (dissipated in heat) and temperature quantities have gone back to their respective units

As always, all the simulations used in this article are available – either on the SystemVision Cloud website or from the author at edesign.ntc@vishay.com

1. 2021: A Simulation Odyssey for Thermistors
2. Hot Topic: Electronic Thermal Design
3. ON/OFF temperature control (with thermistor and heated body models), SystemVision Cloud
4. LTspice : Nouvelles commandes, applications inédites, création et importation de modèles et de sous-circuits, page 85, Dunod, 2015

## 0 comments on “2021: A Simulation Odyssey for Thermistors, Part 2”

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