2
\$\begingroup\$

I'm trying to simulate an LED circuit but I am getting a large difference in results from the simulation vs calculations done using the datasheet information. In this case both the spice model and the datasheet info are direct from the manufacturer. Given the large difference in results, I'm wondering which information I should base my design off of.

In this case the datasheet shows a typical Vf of 2.1v, the spice model seems to be using a Vf of 2.134v. I'm wiring 4 of these LEDs in series with a target of 18mA. Assuming a 9v source if I use a 33.3333ohm resistor (or resistor combination) based on the 2.1Vf of the datasheet I get a simulation result of 13.9mA instead of the expected 18mA.

Should I base the resistance off of the datasheet and ignore the simulation in this case, or should I base things more off of the simulation results? I'm asking since if I'm wrong either the LEDs will be too dim, or they will blow out.

I'm attaching the specific simulation and Datasheet in this example here as well. I'm using a SML-P12WTT86R model LED from ROHM Semiconductor.

The datasheet is here.

Here is what I got from the spice simulation using ROHM's spice model. enter image description here

\$\endgroup\$
  • \$\begingroup\$ If a 1% parameter difference makes enough of a difference to care about, your design is probably not robust enough. \$\endgroup\$ – Scott Seidman Apr 8 at 1:29
4
\$\begingroup\$

Always follow the datasheet. I strongly recommend looking up some of Mike Engelhardt's videos or attend one of his seminars (Arrow sponsors a lot of them). While you're not using LTSpice, Mike has a very deep understanding of Spice simulation, the good, the bad, and the ugly. The reality is most Spice models are made by people that don't really understand them (aka. interns) and can't be trusted a large percent of the time.

\$\endgroup\$
  • \$\begingroup\$ Notice the datasheet value is also only a "typical", not a maximum or minimum. \$\endgroup\$ – The Photon Apr 7 at 14:58
  • \$\begingroup\$ @ThePhoton Didn't even look at the datasheet, I just know I've seen a lot of crappy Spice models over the years. \$\endgroup\$ – Matt Young Apr 7 at 14:59
  • 1
    \$\begingroup\$ These days, SPICE models are more likely to be generated by specialized modeling consultants than by interns. The real problem isn't that the person making the model doesn't understand modeling, it's that they can't anticipate every use case that customers will try to apply the device to. \$\endgroup\$ – The Photon Apr 7 at 15:05
  • 1
    \$\begingroup\$ It may also be that the samples of the part that were used to extract the SPICE model actually had a \$V_f\$ of 2.134 V at 18 mA, but on the datasheet they rounded this to 2.1 V because they know it will vary by more than a few 10's of mV due to process. \$\endgroup\$ – The Photon Apr 7 at 20:20
  • 1
    \$\begingroup\$ @MattYoung. I had a chance to briefly speak with Mike Engelhardt. His main gripe with most Spice models is that they follow a Boyle model (analog.com/media/en/technical-documentation/application-notes/…). The problem with this model is that it typically produces incorrect power draw numbers and hides higher order effects that the designer does not show. Mike told me for LT they focus on more detailed simulation that takes advantage of stronger modern processors and should provide better resutls. \$\endgroup\$ – EasyOhm Apr 7 at 20:44
10
\$\begingroup\$

In this case the datasheet shows a typical Vf of 2.1v, the spice model seems to be using a Vf of 2.134v.

If your circuit works for \$V_f\$ of 2.1 V, but fails for 2.134 V, then you need to get a new circuit.

The forward voltage will vary due to manufacturing variations and junction temperature. And the variation will be more than 35 mV over realistic operating conditions.

Also, keep in mind that the datasheet value is for an ambient temperature of 25 C, while SPICE is probably (unless you've added an option to specify otherwise) simulating a junction temperature of 25 C. That means the datasheet value reflects a higher junction temperature than the SPICE model. And forward voltage does typically drop with increasing temperature so it's conceivable both models are correct.

Assuming a 9v source if I use a 33.3333ohm resistor (or resistor combination) based on the 2.1Vf of the datasheet I get a simulation result of 13.9mA instead of the expected 18mA. ... I'm asking since if I'm wrong either the LEDs will be too dim, or they will blow out.

If this application requires the brightness to be controlled so carefully that the difference between 13.9 and 18 mA makes a difference, you should use a constant current LED driver instead of a simple resistive current limiter.

But in most applications, users won't notice the difference in brightness due to this kind of current change. So you just live with some brightness variability to save cost. Modern LEDs are visibly lit even with 1 mA forward current so whether at 13.9 or 18 mA they will be quite bright.

You could also reduce the variability by designing your resistive limiting circuit with more voltage overhead. Either use a higher voltage source (12 V maybe) and a larger resistor, or place 2 strings of 2 LEDs in parallel, so you have roughly 5 V overhead instead of just 1. The trade-off here is of course more power wasted in the resistors.

\$\endgroup\$
  • \$\begingroup\$ Well when using small # of LEDs in the series the closer the results get to what I’d have expected from the data sheet. Thanks for all of the input. Here and below. \$\endgroup\$ – CyF Apr 7 at 21:50

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.