Earlier this year, we presented a series of LTSpice simulations with temperature control provided by NTC thermistor SPICE models driven by a voltage: Old-School Analog Temperature Control Circuits Solved with Modern LTSpice Thermistor Dynamic Models, Part one, Old-School Analog Temperature Control Circuits Solved with Modern LT spice Thermistor Dynamic Models, Part 2, and Old-School Analog Temperature Control Circuits Solved With Modern LTSpice Thermistor Dynamic Models, Part 3.
At that time, the SPICE models were successfully included in classical temperature regulating circuits.
In this new article series, we will proceed further in this research area and present new application cases, taking advantage of recent developments in thermal SPICE modelling for devices like light emitting diodes (LEDs) and thermoelectric Peltier elements. In the meantime, we will continue to combine these models with some MacroModel test fixtures from LTSpice IV.
In the first part of the series, we are going to present the principles of LED current control using an LT34743 , which is a step-down 1A current driver, and a Vishay surface-mount NTC thermistor. The LED thermal SPICE model is similar to the thermal models presented in the first series of articles1 , completed by the SPICE model principles developed in Practical Lighting Design With LEDs 2 . The whole schematic is detailed in Figure 1. In fact, it’s an extension of the PWM-sourced LTspice LT3474 MacroModel test fixture3 , with several new features.
The thermal modelling of the LED (including the heatsink) is made with a resistor R6 and a capacitor C4, to which the power dissipated in the LED is applied (the B1 analog behavior model source), as well as a voltage source V4 equivalent to the ambient temperature. The voltage at the node THERM represents the LED system’s temperature and is sensed by a thermistor (a 22 k Ω surface-mount Vishay NTC). This thermistor is a part of a resistor network4 connected to the ADJ pin of the LT3474, and will tune down the pulse current into the LED.
To complete the LED modelling, we use two other analog behavior sources:
- B2: a negative voltage source representing the decrease in forward voltage of 3mV/o C in series with the LED
- B3: models the optical output of the LED (as defined in Practical Lighting Design With LEDs2 , but not directly used in the thermal simulation of this article)
Now a simulation of a 2 kHz PWM source in the circuit of Figure 1 is performed with a ratio (real time / computation time) of 50 μ s/s, and it could take as long as 24 hours for a device like an LED to reach a steady state after a few seconds of real time. For memory, most simulations should have a practical duration of a few seconds for computation. That is what makes simulation interesting before testing hardware. If you need to spend hours staring at your computer’s screen (for one simulation), the whole thing would not make sense anymore.
Getting results within a reasonable time frame was accomplished as follows: instead of fixing the initial temperature of the LED system at 25o C and waiting forever, I swept the initial temperature of the LED through a given temperature range (25o C to 100o C). After 2 ms of switching on the PWM source, we looked to see if this temperature was still increasing, remained stable, or eventually decreased. The temperature’s initial rate of change after 2 ms is represented in Figure 2.
For an initial temperature of 25o C, the pulsed current amplitude is 1 A and the LED begins to warm up (Figure 2: green curve of lower pane). When the fixed initial temperature rises (35o C in blue, then 45o C in red, etc.), the current is progressively tuned down and the initial temperature slope decreases.
Around 65o C (curve in magenta), the temperature remains flat after 2 ms. Above 65o C, the LED begins to cool down, leading to a re-increasing of the current. Therefore, we know that we have detected an equilibrium point there, which we can determine precisely by measuring this initial temperature rate of rise, extracting it from the “SPICE Log File,” and plotting it on Figure 3. We measure the RMS value of the current in the LED as well.
We see that a zero rate of temperature rise is reached for a temperature of 70o C. At this temperature, the current into the LED reaches a minimum. This is thus the steady state of the system.
How can we apply the principles of this simulation in the real world? In practice, the thermal parameters of the LED and the heatsink must be adapted. Therefore, the user will need some preliminary measurements. It is possible to apply a standard current of 1 A DC, for example, and to measure the speed of temperature rise. This will give the response time (R6C4 constant) of the LED system. The power dissipated divided by the temperature increase during this 1 A application will give the dissipation coefficient.
Then the user can fix the maximum temperature/power at which the LED can work and adapt the fixed resistor/thermistor network in order to achieve this goal. Figure 4 shows that it’s possible to adapt the steady state of one defined LED from 40o C to 70o C by changing the value of R3.
higher pane: Irms in LED / lower pane: Temperature increase (mK/s) both in function of initial LED temperature (sup>oC)
In a similar way, the user will now be able to study the influence of the other fixed resistors, the ambient tolerance, and more before finalizing the design.
To see a demo video of this simulation, please visit this link.
LTspice is a registered trademark of Analog Devices, Inc.
- Old-School Analog Temperature Control Circuits Solved with Modern LT spice Thermistor Dynamic Models, Part 2
- Practical Lighting Design with LEDs 1st Edition by Ron Lenk (Author), Carol Lenk (Author) ISBN-13: 978-0470612798
- Linear Technology : LT3474 Step Down 1A LED DRIVER, web, Aug 2017
- Analog Circuit Design Volume Three: Design Note Collection by Bob Dobkin (Author), John Hamburger (Author) ISBN-13 :978-0128000014