Now, I understand that the simulator does not make the engineer. But being able to use a simulator is definitely beneficial. My question is below, but first I need to give a little introduction:

I am an aspiring electrical engineer, and am not working in the power electronics/power supply field yet. In the mean time, I build things and try my best to keep current.

It seems like the majority of power electronics job descriptions require that you be well versed in SPICE simulators (PSPICE, ICAPS, etc). I have the demo versions of PSPICE and ICAPS, and have really been impressed with ICAPS.

Intusoft offers a Power Supply Designer package that includes ICAPS with a Magnetics Designer software which looks very interesting. I am thinking of buying the full Power Supply Designer package for my home PC (yes, my home PC) so that I can hopefully master the whole SPICE thing before any job interviews in the future, and use this software on the future job site (and off the job site if traveling or what not).

My question to you all in the field is this: is this overkill on my part? Is this a good investment, or am I crazy?

The schematic capture process is mostly straight forward as you probably have experience in this already.... Pretty much all the same for OrCAD, DX designer, Altium..ect.. The tough part is getting a complex schematic to run and avoid convergence issues... That's when you use all the tricks and work-arounds... and that takes a bit of time to accumulate that experience..
Also you need to develop models that you can verify and trust and re-use...
Detailed modeling can be time consuming ...
Get all the CAD software experience you can, but I wouldn't put all my eggs in only that one basket...

I agree with Chris in not putting all of your eggs in one basket if you are tight on money. If they have not changed the program I found I could enter schematics twice as fast with ICAPS than any other schematic capture program and I could easily grab all or part of their object orientated schematic and place it in Microsoft's products including their high end drawing program if I wanted to make a presentation slide for management.
On the other hand LTSpice and TI's SPICE programs are free and give you practice. All simulations lie when the models are not correct and most if not all models are not exact (sometimes for good reasons, approximations run faster). It is good to learn what you can an cannot use a simulation program for.

Simulation programs can be very useful but you need to learn their weaknesses or where they will mislead you and how to solve convergence problems. For instance a reasonable model of a switching circuit will show overshoot (good) but it will not likely show the correct magnitude unless you have used an circuit analyzer to help generate very accurate models of the circuit parasitics. But with poor models you can investigate the effects of snubbers etc. remembering that the real values of the snubber probably are not correct because the models of the parasitics were not correct.

Jay
I have several Simulators" on my desktop, LT Spice, I Spice, Beigebag Spice, TINA, etc... I have found over the course of years building Power Systems that ISpice was the best compromise if I had none of the others. That and Mathcad are my "go to " programs when I analyze a system.
Soinds like you've had the same experiance wrt ISpice. BTW, I advise signing up for the support, well worth it.

Hello everybody!

I greatly appreciate the comments and suggestions. I ended up renting to own the Power Suply Designer package from Intusoft, so paying for it will be easier. Intusoft was nice enough to accomodate me.

I will also look into LTspice a little more...a free simulator can't hurt. I used it once, and I found it was really slow for what I needed to do.

From reading the comments, it sounds like using multiple simulators is the way to go for alot of people. I think I put a really big egg in one basket with buying the full-fledged ICAPS, but I am still going to probably end up using multiple simulators.

On a slightly different note, has anyone ever heard of PSIM? Definitely a little mickey mouse in some respects, but really powerful in others. Does anybody know if it is used in industry? Just curious.

Again, thank you all for taking the time to offer your suggestions and advice.

Jay, I would respectfully suggest that you look at simulation performance benchmarks of standard test circuits. LTspice wins most (by the way, LTspice was perhaps the first SPICE type simulator to make full use of the I7 and other multi-threaded, multi-cored processors).

Slow performance is most often caused by less than optimum user input (sometimes a simulator that is advanced enough to keep running - rather than just give up - seems slow because it is still going in spite of ill-formed input). For me, simulation speed is only very rarely even on my radar screen of issues during the design process. Generally, LTspice is blisteringly fast.

Dave: I realize my comment above sounded really stupid. I was trying to thank you for giving me tips on how to better use LTspice, but sort of in the wrong context! It kind of looks like I was mocking you, when in reality I was trying to say thanks. My excuse is that I was holding my extremely cute 7 month year old daughter while trying to type.

Anyways, odds are I was probably doing something wrong in LTspice when I first used it. Still going to download it and give it another shot with your awesome tips.

I would have to respectfully disagree about LTspice.....LTspice is not taken seriously in any places I have worked... There are a ton of problems with the accuracy of the IC models... The LT Field Apps will even admit to take the results with a grain of salt... Many of the pins are "dummy pins" that have no effect on the IC... .... Does not allow any deep modeling of the IC's .... I can run a bunch of test on LTspice that will show erroneous results.... Tell your boss you are sending your SMPS to deep space because LTspice says it's good and watch how fast you get thrown out the front door :)

Chris,

You give the impression that you would throw out the baby because you think the bathwater is dirty. Yes, LTspice's public IC models are macro models. And, yes, some of the models omit the functionality of seldom used pins (the synch pin on several ICs comes to mind). And, yes, for their typical customer, who is likely designing commercial consumer products, this is a very good thing (because LTC macro models run very fast while accurately capturing most behaviors important to a commercial consumer products designer).

Do these models include radiation effects, worst case variations, space level temperature sensitivities and other characteristics critically important to space products design? No, but, frankly, who cares? (What percentage of their IC sales do you suppose goes into space?)

LTC no doubt has device level LTspice models for all of their ICs, as LTspice is the tool with which they design their ICs in the first place, but these models probably would run an order of magnitude (or more) slower than the macro models and would not be appropriate for design of most board level commercial products. Such models might be very appropriate for space products and perhaps you might be able to get access if you were a good customer of theirs who had signed an ironclad nondisclosure agreement, but of course LTC will generally be reluctant to reveal the inner details of their proprietary IC designs.

But all this macro model "bathwater" is irrelevant to an assessment of LTspice as a simulation tool. If we leave out the macro models (which I think actually are excellent for their intended purpose) and focus on the basic simulation tool, then LTspice is a great choice for serious development work. It has all sorts of unique features useful for nonlinear circuit design (an alternate solver with >1000x the numerical dynamic range, full use of a PC platform's multiple threads and cores, a native VDMOS power MOSFET device model with integral nonlinear interelectrode capacitances, inductors and capacitors with extensive built in parasitics available that don't cost any extra nodes, a good set of very fast digital and analog behavioral devices, behavioral inductors, capacitors and resistors, and standard behavioral sources, too, of course). This list is by no means exhaustive.

When I did space products work some years ago, we had several simulation tools available, but my first choice was LTspice because of its speed, robustness and powerful tool set. That it was free was not a consideration. Among other things, I used it for worst case, Monte Carlo and sensitivity analyses (LTspice include all the necessary hooks for these tasks, but it does not have a corresponding fully developed user interface to hold your hand through the process). LTspice produces a range of output formats, so that very professional graphics were a snap to incorporate into Word or Power Point reports.

Most recently I have used LTspice to design every circuit section in a multi-kilowatt PV-to-battery charge controller. No standard control ICs were used in the power circuit design, which is a resonant transition, critical conduction mode buck based design with four synchronize, evenly staggered phases. LTspice simulated the complete design, including my novel phase locking circuitry and all four power stages, all with full closed loop feedback as I swept both line and load. It also does a great job of simulating solar arrays with partial shading and of simulating various maximum power point tracking schemes. And, unlike its occasionally thick-headed operator, LTspice has never proven to be a stumbling block in the design process.

Lots of good discussion here. I also recommend LTspice as a very good SPICE package at an unbeatable price.

I would also suggest you try out some of the piecewise linear time domain solvers for power electronics. My favorite is SIMPLIS and there is a free, but limited version, available that will show you the advantages of this approach. For a low cost PWL time domain solver take a look at NL5 by Alexei Smirnov. PLECS, as I understand it, is another PWL time domain solver although to me it seems more oriented to systems analysis than to circuit analysis.

I don't have a problem with the LTspice engine ...It is good in that respect... The problem is the LT IC models are not very accurate ... I get more predictable results when I create my own IC models myself..

Hi everybody, I personally have been using PSIM and I have limited experience with LTSpice. It depends on what you need to do; PSIM is closer to ideal behavior and I the models are very simplified: a diode is either on or off (you can add the threshold, but it is constant), mosfet have Rds_on and diode threshold and so on. When analyzing circuits from concept point of view, I think is great. If you need more details, there is a database of device models that include all the parasitic parameters. I have recently seen briefly PLECS and seems very good as well.

Hello Marco!

It is good to hear from a PSIM user. I found the DEMO version to be very fast and very user friendly. To me it seems geared towards using ideal switches, but pretty much most converter systems are initially analyzed assuming ideal switches anyways. PSIM seems powerful in that it allows the engineer to gain understanding of complex converter systems with ease. Plus, it's affordable, which is a huge plus. Also sounds like you have the option of adding more model complexity, which is another plus.

Mr. White and Dr. Ray: I will take a look at SIMPLIS, NL5, PLECS and 4-5-6..thank you both for pointing those out to me. I must say that 4-5-6 looks impressive.

Anyways, thanks everybody for sharing your simulator advice and suggestions.

@Bob

Thanks for the NL5 suggestion. I had forgotten about this software and hadn't looked into it for some time prior to their latest number bump to the NL5 version. They make it clear that the software uses only ideal switches and that it doesn't have to calculate any middle points to track the transitions between switch state changes. But it is not clear how it decides exactly at what moment it should make those transitions (however, their website is generally very informative, pleasant and well worth a visit).

From the suite of benchmark results that they make available (which show less than a 2x improvement over LTspice, the nearest performer of the SPICE family of simulators tested) I would guess that it, like SPICE, notices that it has overshot the time point for a transition, throws away the point, cuts the trial time step in half (or whatever the setting) and tries again, repeating this process until the transition has been temporally pinned down to within the time tolerance accuracy window.

If this is the method used, it would be slower (but more general purpose) than a predictive type simulator that uses an a priori knowledge of the shape of the trajectory to the impending transition point to precalculate the exact step size required to get there (for example, I would assume 4-5-6 is of this type).

Anyway, I could not find any link to download the NL5 test suite, but it is not likely that the LTspice code was fully optimized to run with ideal switches, thus leading to an inadvertent unfair performance comparison (LTspice contains nonstandard model extensions to its ideal switches and contains special state-change sensing devices that, if correctly utilized, would likely make it behave more like NL5 and less like generic SPICE, which would be more of an apples-to-apples comparison).

LTspice has a rich feature set of extensions to generic SPICE, which gives it a great versatility in behavior as appropriate to the accuracy/speed tradeoff level required for the particular simulation, but these extensions are only available to those who have bothered to learn first that they exist and then how to best make use of them. In this regard, LTspice does not do a lot of proactive hand-holding (the necessary information is usually available in Help and/or some of the other resources, but one must make the effort to go find it, and not many users, even the true engineer-types, take the time to do this).

I must add that everyone has their favorites and mine is SiMetrix. The free version with generous node size will give you two simulation engines, SPICE and SIMPLIS for those fast PWL control loop problems. Also, the full version enables the scripting feature which enables automation and customization of everything. I haven't found a better general purpose simulator.

Well, with 5+ years of experience in Power electronics in the higher education field, mostly as teaching assistant, lab owner and senior project supervisor for undergraduates, I never used any Spice based simulation software. I only use PLECS for preliminary design (because of it's excellent text book like results) and Psim for finalizing the project and testing it with little more real world results. Some of my students do prefer Pspice over Psim at first, but, after wasting time troubleshooting convergence related problems, they end up ditching spice for Psim.

Don't forget in all this simulator talk - there is only one system simulator that counts, the hardware prototype. Regardless of which software you use, and they all have merits, something will be missing from the model that shows up in the hardware to cause trouble.

It is becoming harder these days to convince managers that prototypes must still be built, and every behavior still cannot be predicted accurately for power devices and circuits without iteration back and forth between hardware and simulation.

LTSpice is a great package in that it's free. It is also very versatile and easy to use.

PSIM is good for looking at open loop power systems with reduced models, but last time I checked, it doesn't have a proper convergence algorithm and aggressive control loops don't work well.

Simplis if a great tool if you can afford it. It is quite remarkable how they have managed to get the small signal to work so well.

POWER 4-5-6 is the fastest, and also the only one that actively designs the power circuit, magnetics, and control loop for you so you are immediately simulating closed loop systems. I use this upfront on every design to get decent circuit values, then move on to a general purpose simulator to add more details if I need to before building hardware.

to all -

I downloaded the node-limited free trial version of SIMPLIS and was able to use it to simulate a simple boost test circuit. Learning its human interface has been a challenge, but I am *extremely* impressed with its powerful ability to be able to simulate the ac response (loopgain) of a SMPS circuit directly from the transient model. One does not have to know anything about how to generate averaged models and the like. This is actually easy to do in LTspice once the technique and underlying theory is understood, but with SIMPLIS, the exact same schematic can be used for both transient and small signal analyses, so there is zero chance of making a mistake while generating an assumed "equivalent" ac translation.

Schematic capture, editing and manipulation in SIMPLIS is very different than in LTspice (editing is more like the standard Microsoft interface with regard to the detailed order of the editing actions, whereas LTspice is more like using an RPN calculator) and SMIPLIS doesn't seem to have redefinable hotkeys, but I'd say that it is probably equally as good as schematic capture in LTspice. Plotting results and manipulating the graphical output is another story, however. There, I'd give LTspice the clear edge as it has powerful waveform math that is easy to use and edit after-the-fact (SIMPLIS seems to require deleting and replotting waveforms to "edit" them).

I overlaid the output data from SIMPLIS and the LTspice ac equivalent model and the results produce a clear visual demonstration of why the time domain frequency analyzer loopgain response from SIMPLIS is better than any averaged approximation. The LTspice averaged model attempts to be realistic up to half the switching frequency (any mismatch beyond that is unimportant to compensation design), but it fails to agree precisely with SIMPLIS.

The two curves are essentially the same at low frequencies (the small difference at very low frequency is probably due to mismatch in PWM IC models), but at near half the switching frequency the phase really does not match well. This is due to the second order LCR approximation to the Zero Order Hold like response of the real PWM model - it is impossible to get a perfect match. Making approximate averaged models is a tricky business and it is much safer just to get the response from the switched model.

All is not lost with the averaged model however, as in spite of the slight mismatch, it still can be used to predict the onset of subharmonic oscillations quite well. But considering accuracy, ease of use and inherent immunity to modeling errors, SIMPLIS is a clear winner here.

A few additional comments about SIMPLIS v. LTspice -

SIMPLIS is indeed very fast, but LTspice is generally fast enough when it comes to SMPS transient simulations (even for very complex complete system level sims). However, when it comes to generating Bode plots from the full time domain model, SIMPLIS is superb and head and shoulders above LTspice. I routinely run small-signal ac, low frequency averaged SMPS approximations with little trouble in LTspice, but it is much easier (and safer for the less capable user) to just use one unified model for both ac and transient analyses. Averaged models do not capture the zero-order-hold, sinX/X type response of a sampled data system (which SIMPLIS does flawlessly, very quickly and with little user effort).

Some years ago, I wrote a DFT frequency response analyzer module for LTspice which uses some of its custom behavioral devices to perform a point-by-point DFT loopgain analysis within a transient run. While it runs and produces the expected results, it runs at least 1000x slower than SIMPLIS and suffers numerical noise/dynamic range issues, rendering it mostly useless for practical design.

Averaged models are fine for those knowledgeable enough to generate them, but this process can be challenging and error prone when working with nonstandard designs (e.g., constant on-time control, fully resonant convertors, free-running boundary-mode control, etc.). For working with such designs, SIMPLIS would be ideal, I would think.