Thermal - Can I use Spice to perform Luminus LED thermal modeling?

Yes you can.

We will give an example calculation using the SST-10-SB Sky Blue LED and model the time-dependent thermal response for continuous wave (CW) operation with typical system component values and then show how it can be used to model how the LED junction temperature, Tj, changes if a different component is used.

Define the thermal stack: we will use a single LED operating at the maximum rated power in a room temperature environment. The thermal stack will consist of the LED package soldered to a small MCPCB, a thermal interface material (TIM), and a small heatsink. To construct the Spice model, we need to following information:

Component	Rth (K/W)	Mass (kg)	Cp (J/kgK)	Cth (J/K)
LED package	5.3	2.5e-5	780	1.93e-2
Al-MCPCB (1 cm2)	0.3	2.7e-4	921	2.53e-1
TIM (1-cm2)	0.6	2.9e-5	710	2.04e-2
Heatsink (40 mm dia)	3.7	50e-3	921	4.61e+1

• Rth is the electrical thermal resistance of each component and can be usually be found on datasheets.
• Cth is the thermal capacitance of each component.  This value can be estimated from the mass and specific heat (Cp) of the predominant material in each component.  Cth is estimated as 
  Cth = mass * Cp 

Spice Model for CW operation

Below is the output of an LTspice model using a 5 watt CW LED power level as input [1].  The red line is Tj.  It jumps immediately to 53 C (this appears to be due to the digitization of the time tick in linear time plots. The semilog plot give better resolution for temperature rise behavior) and then slowly rises to a steady state value of 74.5 C after 1200 seconds of run time (20 minutes).  The maximum Tj rating for this LED is 115 C so this system is operating at safe levels. 

The temperatures shown below are at the interfaces, so we know that the LED has a Spice-modeled 
26.5 C temperature difference between the junction and the solder point after reaching steady state. If we use the datasheet value of 5.3 K/W and 5 W input power, we also get 26.5 C. 

Similarly, we know that the temperature difference between the bottom of the LED and the top of the heatsink is 4.5 C. which illustrates the value of using MCPCBs and TIMs in high power LED applications.

If I replace the MCPCB with a 0.7 mm thick FR-4 substrate (Run 2) by changing the PCB Rth from 0.3 to 20.4 K/W, the steady state Tj increases to about 170 C, definitely an unsafe operating temperature [2]. In this case, the LED current will need to be derated to ensure a safe operating temperature.

Thermal Circuit used in this analysis.

Run 1.  Al-based MCPCB Spice model. This output has time scaled logarithmically. The response speed of each component in the thermal system is easily seen. The LED has the fastest response and the heatsink has the slowest.  

Run 1 Al-based MCPCB Spice model output with time in a linear scale.

Case 2 FR-4 PCB circuit. The only change is the Rth_MCPCB value.

Run 2 FR-4 PCB model output with a logarithmic time scale.

Run 2 FR-4 PCB model output with a linear time scale.

Notes on SPICE modeling:

[1] The free program LTspice has good help files so we will not discuss the mechanics of creating this model.  Please note the directive statements in the lower left.  These two statements are required to perform a transient analysis.  In particular, .IC V(N003)=25, sets the initial conditions and if omitted, you will get flat lines for 1200 seconds.

[2] We are using the 2040 K-mm2/W value found on page 7 in the Texas Instruments application note, https://www.ti.com/lit/an/tida030/tida030.pdf and a 1 cm2 area to estimate the Rth value to use in the second model. 

The TI article discusses how the effective Rth value can be improved by using thermal vias in FR-4 PCBs. The small size of the 3535 LED precludes using this strategy. The TI device under discussion has room for 33 thermal vias directly under the device.

Addendum for using luminaire cooling data to estimate Cth:

The values calculated in the table above contain assumptions about the effective areas and volumes of material participating in the heat extraction process. If these assumptions are wrong, so are the analysis results. An empirical approach using an estimate for the LED and a cooling curve measurement for the balance of system (BOS) thermal path might give better results.  

Procedure: Empirical Calibration of the BOS Thermal Model

1. Identify Fixed LED Parameters

Before measuring, establish the known "constants" for the LED package.

• Thermal Resistance (Rth_LED): Use the manufacturer's datasheet value (e.g., 5.3 K/W} from the Luminus SST-10-SB data).

• Thermal Capacitance (Cth_LED): Use the mass-calculated value (1.93e-2 { J/K} as these small-scale transients are rarely captured by external thermocouples.

2. Steady-State Data Collection

Run the system under normal operating conditions until the temperature stabilizes.

• Measure T_s: Place a thermocouple at the solder point (the interface between the LED and MCPCB).

• Measure T_amb: Record the ambient air temperature.

• Calculate P_LED: Determine the actual heat power (Total Power in Watts minus Optical Power out).

• Solve for Rth_BOS:

This gives you the total resistance of the path including the MCPCB, TIM, and Heatsink.

3. Transient Cooling Measurement

Once at steady state, cut the power to the LED and record the temperature decay at the solder point (T_s).

• Sampling Rate: Ensure your logger captures at least 1 sample per second.

• Determine the Time Constant (tau): Identify the time it takes for the temperature to drop by 63.2 % of the way to ambient.

  • Calculation: T_{target} = T_{amb} + 0.368 \times (T_s - T_{amb}).

  • Find the time (t) where the measured temperature reaches T_{target}. This is your tau_{BOS}.

4. Extracting the Empirical Cth_BOS

Since you now have the measured resistance (Rth_BOS) and the measured time constant (tau_{BOS}), you can calculate the effective thermal mass:

The modified SPICE model is then:

and the program output is below where the blue line is the thermocouple position next to the LED (red line)

Addendum for using pulsed inputs:

To model a pulsed input, replace the DC Power (e.g. 5W) with a SPICE pulse definition in the current source component. There is an App that will convert duty cycle and frequency to the SPICE format.

https://subtle-far-jellyfish.anvil.app/

For a 240 Hz, 50% DC with a peak power of 5 W, the command is

PULSE( 0 5 0 4.167e-06 4.167e-06 0.002084 0.004167)

and the modified model is below. This runs slow so only the first 2000 seconds are modeled.

The output is below. The time constant of this LED is ~100 ms so there is only a small amount of temperature change due to each pulse. The system lines out at lower temperatures than the DC case above.

If we slow the pulse rate down to 0.1 Hz (50% DC), there is large temperature swing in the LED as shown below and the line out temperatures are higher.

--------------------------------------------------------------------------------------------------------------------

Luminus Website https://www.luminus.com/

Luminus Product Information (datasheets): go to the main page and select Products and then select the type of product you are interested in.

Luminus Design Support (ray files, calculators, ecosystem items: [power supplies, lenses, heatsinks]): go to the main page and select Resources & Tools and select the item you are interested in.

Luminus Product Information sorted by Applications:  go to the main page and select Applications.

Where to buy Samples of Luminus LEDs: https://www.luminus.com/contact/wheretobuy.

--------------------------------------------------------------------------------------------------------------------

Technical Support Contact Information: [e-mail]

Sales Support Contact Information: [e-mail]

Customer Service Support Contact Information: [e-mail]