LTspice error with varistor model and impulse current test

Question

I'm trying to use the TDK varistor spice models in LTspice and there are some things that don't add up. In the figure below you can see the actual equivalent circuit of the TDK model. I know that I can import the model library (and I did that) but I figured that it would be interesting to trouble shoot the model by actually drawing the schematic to allow better flexibility if I want to make some changes.

In figure above you can see that the MOV model is conected to an RLC circuit which is used to produce impulse currents.

There are some cases in which the simulation breaks an error message of the type "Time step too small" allow with "Trouble with node 6" appears.

The problem arises only arises when the impulse current is an underdamped wave and I suspect that the error ocurrs when the current passes through the zero crossing.

Any idea on what could it be?

Answer 1

PWR, LOG and LIMIT functions are all very poor choices for a nonlinear integration engine like SPICE.

How SPICE works is, to prepare the node voltages and currents of the next timestep, the impedances and rates at the current timestep are calculated, then substituted into the node equations. Rates are determined by taking symbolic derivatives of expressions (where possible; and if not, then approximating it by a sampling process, I think?), and the resulting values are used to extrapolate to the next timestep. Some accuracy and stability checks are done, and if they pass, the timestep is accepted and the process repeats. If it fails, a smaller timestep is chosen and evaluated, and so on. The overall process then repeats until the simulation is completed, terminated by the user, or a "timestep too small" error is encountered.

So, usually such an error is a sign of something going wrong -- expressions that aren't analytic or continuous at the operating conditions, for example. They don't even need to be discontinuous to throw an error: if the derivative(s) don't exist either, that can cause problems. (I would guess this is probably one of the more significant differences between flavors of SPICE engine: how to find derivatives, and finding more accurate or faster substitutes when the preferred method(s) fail.)

I can't speak much for LTSpice's stability as I don't use it much myself, but the one I am familiar with (Altium's, which is XSPICE based, plus partial PSPICE compatibility -- but only in terms of model parameters and some syntax I think, not improved numerical stability), is quite hopeless with this model.

The easiest solution I would recommend, is to substitute a somewhat better model. Last I checked, Bourns' models use a TABLE expression; which, as you might guess, is still not great for stability -- being a piecewise-linear function, the derivative is discontinuous -- but, it seems to manage. Likely LTSpice will have similar success.

I've been tempted to translate examples of either model type into a proper continuous and analytic function (whether by polynomial approximation, more specific curve fitting, or equivalent circuits -- diodes are a convenient exponential element in SPICE for example)... but so far haven't sat down and done it.

Regarding brand differences, there are very few; as far as I know, MOVs are a completely mature technology, with all makers using all (or largely) identical materials and ratings. (That said, the energy rating does seem to vary a bit between otherwise-equivalent parts; this doesn't seem a very significant difference, though.) So, I would consider another manufacturer's model of an equivalent part to also be equivalent.