Spice has features that enable parametric studies. You can name parameters inside of LED models and loop through a maximum of three levels of variation. The advantages of using Spice are conceptual simplicity for circuit layout and extreme speed in solving linear systems. Here we will show an example of how to calculate a large number of spice models that all fall in the same voltage bin.
These collected models can be used to simulate a set of loads in a more realistic way in complex Spice models compared to using a single diode model for everything. An example of this type of application can be found in the Luminus Help Center article “Electrical - What is Current Hogging in Series Parallel Designs?”.
The figures below show four variational cases for a small GaN LED model that is Vf binned near 3 V at 60 mA. The parameter being varied is N, the diode ideality factor and the values of IS and RS are adjusted so that the diode forward voltage at 60 mA is in a voltage bin near 3 V.
The “.step param <var_name> list var1, var2, var3, …” directive is used to loop through named variables in the LED model definition. Variables are indicated by using braces “{var_name}”. You can also put mathematical and logical expressions in braces, but these Spice features are not used in the article.
The ideality factor, N, has a strong effect on the shape of the IV curve. The technical slang for this is “soft nose” and “sharp nose”. The Case 1 IV curve above has the sharpest nose, and the Case 4 curve has the softest nose. The loops used in this study produce 18 case results which can be viewed using the <view> <step legend> item on the plot right click menu. You can also use <view> <select steps> to subset the plot and produce a more user-friendly list of the parameters.
There are an infinite number of solutions to these constraints. We suggest using N values ranging from ~1.5 to ~5 to simulate the behavior of this type of diode. LEDs can and do have N values well above 2, the junction recombination leakage dominated value for high bandgap materials. The reasons for this are complex and will be discussed in a future article.
The curves above were manually generated. Spice is capable of logic but fully automating this process within Spice is pretty complex. Spice engines can be run as a process in Python where much more complex strategies can be employed.
The iterative manual procedure for a target of 3 V at 60 mA is as follows:
- Pick a value of N
- Change IS to get close to 3 V
- Change RS to tweak in the results
Here we use explicit lists of values to determine the ranges that give tight groupings. The .step directive is versatile, and a number of other strategies could be employed.
*This article was inspired by a circuit file (Alter_LE_CG_P3AQ.asc) uploaded to the LTspice users' group.
Useful Spice Resources
LTspice Simulator | Analog Devices
LTspice: Adding Third-Party Models | Analog Devices
LTspice Annotated and Expanded Help* - LTwiki-Wiki for LTspice
Simon Bramble | Analog Circuit Design | LTspice Tutorials
Related Luminus Help Center Articles
Electrical – How do I extract Spice IV parameters from an LED datasheet?
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
Electrical - Can I add reference lines to Spice plot panes?
Data Analysis - Using Python to run LTspice as a remote process.
--------------------------------------------------------------------------------------------------------------------
Luminus Website https://www.luminus.com/
Luminus Product Information (datasheets): https://www.luminus.com/products
Luminus Design Support (ray files, calculators, ecosystem items: [power supplies, lenses, heatsinks]): https://www.luminus.com/resources
Luminus Product Information sorted by Applications: https://www.luminus.com/applications
Where to buy Samples of Luminus LEDs: https://www.luminus.com/contact/wheretobuy.
Comments
0 comments
Please sign in to leave a comment.