LCSC, looking for spice modals - Page 1
Forum section: electronics / projects

author: Geoff
author_rank: Contributor
timestamp: August 07, 2024, 10:35:17 am
content: LCSChas a lot of nice MOSFETs, but I would like to pick from those that have spice modals available.I have tried searching for the manufacturer's website, but no luck when it comes to these lesser known brands.Is there another, better way, or place to search for their spice modals?

author: robzy
author_rank: Regular Contributor
timestamp: August 07, 2024, 01:09:00 pm
content: Coincidentally I have the exact same question at the moment.I am looking at using some Alpha & Omega semiconductor MOSFETs, but A&O don't have any spice models available.My solution was to go to Digikey, and choose something kinda-sorta-ish similar and use that SPICE model.

author: tggzzz
author_rank: Super Contributor
timestamp: August 07, 2024, 04:43:22 pm
content: Be very aware that the quality of Spice MOSFET models is, um, variable.Starting point:https://www.eevblog.com/forum/beginners/please-help-understanding-relative-permiivity/msg5586663/#msg5586663

author: selcuk
author_rank: Frequent Contributor
timestamp: August 07, 2024, 06:12:48 pm
content: Some 3rd party model libraries for SPICE simulators are available online. You can check them for various parts. This one was shared recently:https://www.eevblog.com/forum/eda/ltspice-v17-1-x-how-to-add-custom-library

author: T3sl4co1l
author_rank: Super Contributor
timestamp: August 07, 2024, 06:36:44 pm
content: Hah... no.FWIW, probably the best models today are by Infineon, at least of relevant parts -- I haven't looked in a while, but last I did, there were at least a few that had, almost no, if any, SPICE primitives in them, instead cooking up pretty much the whole thing as behavioral equivalents, tons of functions, TABLEs and POLYs -- which also run quite slow, but give accurate results at least. By "relevant", I mean, read the model yourself -- if it's some old MODPEX output (e.g. classic IR parts), uses MOS primitives (especially of low LEVEL), those are just kind of whatever -- they're usuallynot badfor older MOSFETs (low to modest doping grading coefficients; maybe even for semi-modern (single gate) trench parts, typical in low to medium voltage ratings), but the real elephant in the room is high voltage types (>200V or so), for which SuperJunction (SJ) technology is now ubiquitous, and the Coss and Crss curves arewild, something SPICE itself has trouble even implementing.I might even be remembering IGBT models (which are even more remote from SPICE primitive transistors); it's been a while since I needed to model anything like this in such detail.And not to say Infineon is the only one, but again, it's been a while, so I don't have a comprehensive look at what kinds of models are offered by who.Anyway, models are mostly from major manufacturers, and validity varies; I would say the older models and parts (legacy, like HEXFETs and whatnot -- their switching performance is almost an order of magnitude out of date now, but there's still plenty of applications where that's more than enough, and plenty of applications where the linear performance and wider SOA* is desirable and switching is ~irrelevant) are good enough, and highly complex models may representmoderndevices well enough; but beware the gap inbetween. And then, for manufacturers that just don't produce (or release) such modeling data, you're never going to get a model for their devices; just use the closest equivalent that fits, or test it yourself.*Modern datasheets of IRFxxx(x) don't usually give DC SOA curve for some reason, but they have in the past (e.g. 80s-90s IR databooks). That doesn't mean modern ones still do -- but in my limited experience, they do tend to test well for such applications. So if word-of-mouth is good enough for you -- or preferably a test-approval selection process -- they're worth looking at.It may be worth understanding that SPICE isn't too useful for a lot of things these days -- I would say it's most useful for learning how things work, what kind of behavior to expect, but then to build and test the real thing to get the most subtle details, like overall conduction + switching losses in a converter. There are even aspects that may not be modeled at all (e.g. SJ hysteresis loss). SPICE is at its best when doing analog/mixed simulations of complicated (difficult to build and revise), but tractable (not combinatorially infeasible to explore internal state, or design variations), circuits. It was born of the 70s IC boom, when CPUs (in IC form) were just coming out, PNPs were still lateral, and computers were mainframe time shares. It's at its strongest when developing circuits like the uA741, dozens of transistors in an integrated circuit; it's at its worst when tasked with myriad variations, or narrow margins and errors which accumulate only slowly over time (like switching converter losses).So, given that learning interest, perhaps -- SPICE is still useful for that, and, you can see given the state of industry support and device complexity, it's unfortunately hard to play with these devices in a learning context. That still leaves everything else, like for converter design, you can test lots of permutations, device ratings, circuit/layout strays, snubbers, etc., and develop a feel for all of that, all using classic/old devices and models. Arguably, doing it with modern, complicated devices might be a more difficult learning experience anyway, you don't get a feel for how fundamental one or another aspect is -- if it's been modeled correctly at all -- but, such is life, and learning about this can be done from many angles. Just beware there is more out there than what you've seen, and be open to researching those things on their own basis.For sake of argument, here's a real measured example illustrating how SPICE itself might fail -- not that such a system isimpossible to express, mind -- but the amount of detail required to do so, is far from worthwhile to code. Consider the following circuit using SJ MOSFETs:https://www.seventransistorlabs.com/Images/SJ_Test5.pngQ2 turns on, discharging Q3 Coss through R9. Waveforms recorded for a series of Q3 samples (identical PN/date, just different parts from the same tube, and yeah approved distributor and all that, nothing suspicious):https://www.seventransistorlabs.com/Images/SJ_Test7.pngYes, that's a curvebouncing upward, showing negative incremental capacitance, and in a way that I cannot attribute to mere breadboard setup or other measurement error -- it's really doing loops on the discharge curve, it's nuts! (This is probably a side effect of the multi-epitaxy SJ process, being less uniform than the deep-trench-and-backfill process.) How the heck would you even model this? Simple, you don't, almost no one needs to know that this is even an effect that exists -- but so too, it goes to show just how alien these parts are, compared to textbook examples.Hm, regarding distributors and stuff -- the supply chain itself is still a big deal, always pay attention to that -- but there's no need to be similarly skeptical ofmanufacturers. Taiwanese and even Chinese parts these days are doing everything the brand names are doing. SJ-capable fabs have disseminated widely. I've seen some no-name MOSFETs that undercut major brand names modestly in price, with no compromise in performance -- they seem to do what the datasheet claims, at least within the bounds of what I'd tested them at.Tim

author: Nominal Animal
author_rank: Super Contributor
timestamp: August 07, 2024, 07:11:44 pm
content: Quote from: T3sl4co1l on August 07, 2024, 06:36:44 pmCan confirm.I'm a hobbyist, although I do have some formal education in electronics circuits and stuff (physicist), but just not enough practical experience.To compensate, I read a lot of datasheets (they're easy when you're used to peer-reviewed articles) and examine the circuit I intend to use –– like PWM'd LED backlight for a display module –– in spice, specifically KiCad and ngspice nowadays. Designing a converter is still outside my skill range, but I can adapt those in datasheets or suggested by TI Webench. What I do in spice is experiment with the parameters to see how robust the circuit seems to be, whether varying resistor and capacitor and inductor values and voltage somewhat will still produce the desired results or not, and how large those changes are. Plus, I get an idea as to what kind of operating range I can expect in real life, when I create the circuit in practice.Because my designs are 99% public domain / CC0-1.0 and one-offs, I tend to overengineer them so that if I need to adjust something a bit, I don't have to do a redesign or respin the board.I like JLCPCB, but prefer to buy components off Mouser. One reason is that it is easier to find SPICE models. (That's how I ended up using NXP NX138AK's instead of say BSS138's N-MOSFETs for small signal stuff: slightly faster, otherwise very similar, and a set of 100 in SOT-23 (hand-solderable and even dead-buggable without any board directly to wires) only costs about 5.30€.)Quote from: T3sl4co1l on August 07, 2024, 06:36:44 pmYup. A corollary is that for some ideas I want to explore, I sometimes start with an ideal component model (especially for stuff like diodes and inductors) before recomposing the entire spice simulation with actual components. It helps getting an idea of how the ideal situation and real world differ, and what kind of effects one can expect.And I do agree: no simulation or theory can replace experimenting with real-world circuits. With the prototype PCB manufacturing prices today, it's definitely worth doing, especially if you can make modular boards like say an efficient DC-DC switcher from 5V to 3.3V @ 700mA with low ripple for use in digital circuits powered from an USB power bank or wall wart.

author: TimNJ
author_rank: Super Contributor
timestamp: August 07, 2024, 10:15:30 pm
content: Agree that the Infineon models seem to generally be the "best", at least, they seem to behave closest to what I'd expect. Whatever part you are looking at, I'd try to find something in the same ballpark from Infineon. In addition to matching up typical datasheet parameters, I'd make sure that the technologies are the same too. e.g. If you are looking at VDMOS or LDMOS part on LCSC, don't pick a super-junction model from Infineon.

author: Geoff
author_rank: Contributor
timestamp: August 08, 2024, 01:02:18 am
content: Thank you for your reply.My use of spice is more akin to a jumped up calculator. Like, did I get my RC timing right. And making a guess as to when the photo transistor will turn on, if I use an opaque cover.Playing with spice does give me a better understanding than I probably need, also it's good practise if I really need spice for something, and it's fun.But it would be even better if I could find the spice modals for those nice cheap parts.