1
\$\begingroup\$

I'm looking for appropriate models to model magnetic components, mostly transformers and perhaps for chokes as well, for use in LTspice.

I've heard briefly of some models, like Jiles-Atherton-model (JA) and John-Chan-model. At LTwiki non of these models feels very appealing. Maybe the JA-model can be used in a late simulation of a design, but before that the sim-time do not feel any appealing at all, so i'm trying to find something more appropriate.

In "Switch-mode power supplies" by Basso, there is a model presented that I think is pretty suitable, that can model saturation, hysterical losses and "frequency losses" and also plot Flux and the magnetizing force, however it doesn't work to just take the subckt to LTspice, the syntax isn't the same.

I've also found some other literature that reminds of the one in "switch-mode power supplies", perhaps some of them are exactly the same just described a bit differently. 1,2 and some in 3 and 4 look very much the same. However non seem to be direct "copy paste" compatible with LTspice.

1http://www.intusoft.com/articles/satcore.pdf

2http://www.ti.com/lit/ml/slup109/slup109.pdf

3Transfromer modeling,beigbag

4SPICE Modeling of Magnetic Components by Sanders

5Non-Linear Saturable Kool Mu Core Model, aeng

6Spice3 Compatible core model, at aeng

Before deciding which model or models to implements in LTspice, I need to know what the pros and cons of the models are? and are there any more relevant ones that I've missed?

Best regards

\$\endgroup\$
4
  • \$\begingroup\$ I think some chan model is the most used for ltspice, but it isn't really very suitable for modeling accurate real life transformer behavior. \$\endgroup\$
    – PlasmaHH
    Commented Aug 29, 2017 at 15:22
  • \$\begingroup\$ SPICE is a "Simulation Program with Integrated Circuit Emphasis"...so it's not surprising it's a bit crap at dealing with transformers. \$\endgroup\$
    – The Photon
    Commented Aug 29, 2017 at 15:41
  • \$\begingroup\$ If you are planning on using off the shelf components, then Wurth provides (scarily) accurate simulation models for LTSpice. \$\endgroup\$ Commented Dec 21, 2017 at 15:01
  • \$\begingroup\$ Also consider value of poweresim.com \$\endgroup\$ Commented Dec 30, 2019 at 7:07

3 Answers 3

2
\$\begingroup\$

I made models of transformer components (windings and linear and non-linear core models) from which transformers are easily constructed. See https://yadi.sk/d/GwFHUX_w3PgL6h it is My packaged folder with models and examples and https://yadi.sk/i/yhWPb4Io3PgLBc it is information about UPdate. Example LTspiceXVII\examples\Bordodynov\TRANSFORMS\ I have a transformer of winding Winding_RC or WINDING_LCR (Just Winding not use.) The library is Volodin with the same symbol name (valvol.lib). (There is a swap on the diagram) and the Core. The hubs are not linear (nonlinear) or linear. Non-linear Core, Coreja. Coreja-Model Jiles-Atherton. Parameters can be taken from files magmod.txt. Linear Core Two: Corelin_al, the parameter is AL, i.e., induction for one spiral (turn) and The CORELIN_A_Lm parameter is the Section area, length of the average magnetic line and effective magnetic permeability. Use linear lines before using non-linear Core. And the most important thing. All elements must have a shared point (Connected via wires ). But you can also post the coils and the core. The main thing to do is to pin one name to the PIN. For this, there is a third pin in the winding. One pin on the core. The simplest transformer consisting of a primary, a secondary, and a core can just move together to pines fit (connected). I prefer to use TR1, TR2, etc. The coress allow for the loss of the eddy. For this, there is a boundary frequency of Fe (Feddy). WINDING_RC has the parameters of Rser and Cpars and the number of coils. WINDING_LCR is the additional inductiveness of the scattering. I prefer not to clutter the diagram. Parameters other than the number of coils are not visible, but when they get into the symbol and then the Tick will be Visible. You can get the dissipation power of the core (non-linear) in the normal way using ALT.

\$\endgroup\$
2
  • 2
    \$\begingroup\$ Welcome to EE.SE. Your post is a difficult read. Try editing to add some paragraphs (enter x 2) and maybe some bullet points. \$\endgroup\$
    – Transistor
    Commented Dec 21, 2017 at 11:21
  • \$\begingroup\$ I suspect the language barrier to be the cause, most likely an online translator was used (with some adjustments?). \$\endgroup\$ Commented Dec 23, 2017 at 7:53
2
\$\begingroup\$

I haven't worked extensively with nonlinear cores but, to my knowledge, there are three models, as you mention:

  • The Chan core. It's based on tanh() curves and is native to LTspice, therefore it will simulate very fast, if not the fastest, but when the BH loop is made square, like a ferrite's, and it's saturated hard, it can have some glitches, despite the underlying tanh(). I have also heard it said that the curves cannot be modelled very accurately, but the area can be. The parameters to configure are simple and readily available in any datasheet: Br, Bs, and Hc, for the magnetic properties, A (area), Lm (magnetic length), and Lg (gap length) for the physical properties, and N as the number of turns.

  • The Jiles-Atherton core. It's based on heavy math and polynomial approximations, and its implementation (at least, in LTspice, that I know of) is based on a heavy behavioural approach involving some discontinuous functions such as uramp() and sgn(). This makes it run very slow compared to the Chan core, but the curves can be approximated to better match a particular core. The parameters are more difficult to tune since they involve a direct connection to the magnetic properties.

  • A generic SPICE approach, incorporating anti-parallel diodes to model the nonlinearity. This has been a long-standing approach, it can run very fast, but the curves will always be hourglass-shaped, no matter what, and it requires a bit of tinkering since the diodes are the ones that set the curves, and their parameters have little to do with magnetics. There are approaches to some cooked-up formulas, but they, too, require adjustments.

As for recommendations, that's very much a function of what you need more: if you need speed, then it's the Chan core or the SPICE approach, though I'd favour the Chan core for the simplicity and directness of the parameters. If you need accuracy, then Jiles-Atherton is a better choice, but you need to know the properties of the magnetic core. It also needs more patience and, most probably, more care in designing the driving circuit such that it is as derivative-friendly as possible.

\$\endgroup\$
0
\$\begingroup\$

In the need for fast simulation and stable convergence for switching applications I've developed a very simple model, featured by monotonic and smooth function:

At least in my cases it fits super well to iron, nanocrystalline, ferrite cores, etc.

The only thing is that for the simplicity I have not added hysteresis (yet). Particularly my application required stable convergence in deep saturation.

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service and acknowledge you have read our privacy policy.

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