Electrical – How do I extract Spice IV parameters from an LED datasheet? – Luminus Devices

Spice uses three parameters to define a forward IV diode characteristic. Using Spice nomenclature, these are

IS - Reverse leakage current
N - Emission coefficient (also called the ideality factor in other fields)
RS - Series resistance

These correspond to the Shockley diode equation (+ a series term) with some caveats. (1) Spice uses numerical methods and there are hidden parameters that aid convergence. (2) Spice parameters that define other diode characteristics (such as pulse response or reverse bias operation) are decoupled and the models are generally simplistic. (3) Spice was developed when silicon and germanium diffused homojunctions and Schottky diodes were the only devices in existence. The default values used in Spice still reflect these types of devices.

The IS and N values used in a model definition determines the diode turn-on voltage level and the shape of the “knee” of the IV curve. The series resistance determines the slope of the IV curve in higher injection.

These three parameters can be extracted from the IV curves in an LED datasheet. We will show an example of this process for the Luminus SST-10-UV component.

First, we need to digitize the IV plot above. This can be done using the methods in a previous article, “Data Analysis - Digitize and Interpolate a Plot”. Doing that for the 385 nm curve generates the tabular data below (note that the axes are swapped). There is no particular need to interpolate these data.

We will use methods explained in a number of previous articles and in the interest of brevity we just reference them below.

Electrical – Can I simulate a set of LED IV curves that have a single Vf bin?

Electrical – Can I calculate LED lumens with Spice?

Electrical - What is Current Hogging in Series Parallel Designs?

Electrical - How do I sweep an LED IV curve in Spice?

Electrical - How do I insert a diode file into LTspice

The first step in extracting the Spice parameters for these data is to put the tabular data in Spice so that we can match with our diode model. This can be done with a “G” element which is a voltage controlled current source that accepts a tabular definition of the transfer function.

The figure below shows a prototype model where we have inserted a voltage source, a default LED, and a voltage controlled current source with a three-point table definition. Note the polarity of the voltage nodes in G1 match the voltage source. Spice has two definitions for this type of source, and we used “g2” in the component insertion menu. This figure is an intermediate step showing results immediately after creating a model with simple default elements.

The tabular data is entered in the Component Attribute Editor in the Value field. The editor is opened by right clicking on the G1 symbol.

The figure below shows the result after the following steps,

Add a diode model to the schematic that has IS, N, RS values we can modify. Here we used the values for a blue LED as a starting point.
Plot the desired IV data using the G component
Change the sweep voltage to match the data

What we want to do is modify the three Spice parameters to match the data defined in the table. We need a higher voltage (IS and N) and will tweak the series resistance to have the correct slope. Change the model by right clicking on the numbers and then run the model to see the change in the plot pane.

After five tries, we generate this set of parameters which fits the data at the low and high defined points.

The largest divergence is at 0.6 A, and we add two points to our data table to get a better-defined tabulated curve to compare between the data and the model.

Final result. The diode model “ .model LED-1 D IS=1.0E-21 N=2.7 RS = 0.15 “ has a good fit to the data digitized from the datasheet plot. This LTSpice file is in the downloads section below.

Comments

There are analytical methods to directly calculate these values from as few as three data points. We have found that we end up tweaking these results and it is easier to start with a known curve shape and iteratively run the model to find a solution.
For LEDs, N usually ranges from 2 – 10. Lower N values have sharper “knees” in the IV curve and less curvature in the forward bias section of the IV characteristic. When in doubt, use N between 2 and 3 as a starting point.
All of these parameters interact with each other, and it takes some experience to know what to change. The leakage current has a strong effect on turn-on voltage, the N parameter has a strong effect on curvature, and the RS term has a strong effect on the slope in forward bias. A large shift in one value generally requires also adjusting the others to get back to the target zone.
The ability to plot a reference curve in Spice is a powerful technique for many applications. We have used a “G” model for a voltage controlled current source, but there are other models for other input-output combinations that work similarly.
This model applies to the forward bias curve of the LED. Spice automatically uses default values for a small homojunction silicon diode if a parameter is not included in the model in use. This can lead to erroneous results in time domain modeling. We will provide guidance on how to estimate other parameters in a future article. At this time the best thing to do is copy them from a model for a similar device.
We used digitized data for this example. You can also measure the IV curves for an LED on a heatsink with a benchtop power supply. Measuring a number of your binned LEDs will give you a good idea of the range of parameters that could be employed in loops or Monte Carlo simulations; both of which are supported by Spice engines.
This method can be generalized to LED circuits and if you have (for example) a large series parallel configuration, you can measure the entire circuit and get a good fit to use as a load in a system model.

Useful Spice Resources

LTspice Simulator | Analog Devices

LTspice: Adding Third-Party Models | Analog Devices

LTwiki-Wiki for LTspice

LTspice Annotated and Expanded Help* - LTwiki-Wiki for LTspice

Simon Bramble | Analog Circuit Design | LTspice Tutorials

LTspice groups.io Group (Hendrik Jan Zwerver has contributed material similar to this article in this user group with more theory and a calculator)

https://electronics.stackexchange.com/questions/9510/how-do-i-model-an-led-with-spice/9543#9543

Related articles