LTSpice LED simulation question - Page 1
Forum section: electronics / beginners

author: Lucky-Luka
author_rank: Unknown
timestamp: December 29, 2021, 04:08:27 pm
content: Hi allI just wanted to simulate a 5mm green LED connected to a DC source.I expected to see more than 2V at the A point of the circuit but it looks like it's more or less 0.7V which is the typical forward voltage of a diode.Where i am going wrong?Thanks

author: ledtester
author_rank: Super Contributor
timestamp: December 29, 2021, 05:04:07 pm
content: Have a look at this stackexchange question:https://electronics.stackexchange.com/questions/9510/how-do-i-model-an-led-with-spiceIt references the original Spice, but the diode parameters all look the same so LTSpice is probably using the same model.

author: Ian.M
author_rank: Super Contributor
timestamp: December 29, 2021, 06:04:37 pm
content: Good answer, but if you just want quick and dirty models for generic small LEDs, you may find these I collected from various sources helpful:Code:*Typ IR LED from optocoupler: Vf=1.2V @10mA.model LED0 D (IS=1p N=1.999644 RS=0 BV=6 IBV=10u+ CJO=10p EG=1.424 TT=500n)*Typ RED GaAs LED: Vf=1.7V Vr=4V If=40mA trr=3uS.MODEL LED1 D (IS=93.2P RS=42M N=3.73 BV=4 IBV=10U+ CJO=2.97P VJ=.75 M=.333 TT=4.32U)*Typ RED,GREEN,YELLOW,AMBER GaAs LED: Vf=2.1V Vr=4V If=40mA trr=3uS.MODEL LED2 D (IS=93.1P RS=42M N=4.61 BV=4 IBV=10U+ CJO=2.97P VJ=.75 M=.333 TT=4.32U)*Typ BLUE SiC LED: Vf=3.4V Vr=5V If=40mA trr=3uS.MODEL LED3 D (IS=93.1P RS=42M N=7.47 BV=5 IBV=30U+ CJO=2.97P VJ=.75 M=.333 TT=4.32U)*Typ small White LED: Vf=3.2V Vr=5V If=35mA.MODEL LED4 AKO:NSSWS108T

author: Zero999
author_rank: Super Contributor
timestamp: December 31, 2021, 02:05:06 pm
content: I've never bothered. I just model it by connecting several silicon diodes in series and parallel, if necessary. This can be done by setting value2 to n=x for diodes in series, or m=x for diodes in parallel, where x is the number of components. It's not perfect, but good enough for most applications.

author: Ian.M
author_rank: Super Contributor
timestamp: December 31, 2021, 02:36:22 pm
content: Yep, that will work for a quick&dirty sim, but its very little extra effort to paste a suitable LED model directly on the .asc schematic and use it. Generally if you are simulating a LED, you are doing something tricky with it so desire better accuracy, otherwise a 'back of an envelope' dropper resistor calculation is good enough.Here's a test jig sim of your 'LED' and my models swept from 0 to 30mA.

author: Zero999
author_rank: Super Contributor
timestamp: January 02, 2022, 06:35:11 pm
content: My LED model looks close enough to LED2, the standard green, yellow, amber one. If you measured a selection real LEDs, you'll probably find there's a greater difference between them, than my model vs yours.

author: Ian.M
author_rank: Super Contributor
timestamp: January 02, 2022, 06:47:17 pm
content: Yep, and there's no significant overhead in using a diode with n=3, as its just a constant multiplier applied to some of the diode model parameters when compiling the matrix. Note that LTspice will quite happily accept non-integer and even fractional n if you want to tune the Vf of your diode moer precisely.

author: not1xor1
author_rank: Frequent Contributor
timestamp: January 03, 2022, 08:12:04 am
content: QTLP690C, part of the LTSpice default pack, provides a reasonable model of a small red LED (Imax = 30mA). The Vf vs I simulation is a bit different regarding the datasheet, but still acceptable IMHO.