# Spice transient vs AC models

In process of designing an electronic or a mechatronic system, we take into account AC analysis and Transient analysis of that system. In my case, I want to design a speed and position control system for a DC motor. I went through the theoretical analysis of my system by taking into account:

• The electrical and mechanical characteristics of of the motor.
• I have designed a theoretical controller for each: "Inner current control loop", "Inner speed control loop" and "Position control loop".
• I have simulated my system using Matlab and I got a satisfactory result.

Now I want to simulate my system using component models, by using any well known electronic simulators like: LTSpice, Simetrix/Simplis. but when I come to component selection, specially Gate Driver ICs or Motor Driver ICs I do not find SPICE models of these components.

If I search on the internet, I am surprised to find that most companies provide transient rather than average models.

See the example in the following link: https://www.ti.com/product/DRV8701#design-development

Texas instruments provides three different Transient models but no one AC model.

My questions:

• Why it is easy to find a Transient SPICE model rather than AC model?
• Why companies do not provide AC models of their components to allow designers to incorporate these components in AC analysis of the whole system?
• How can I take advantage of the transient models to validate my simulation work for implementation?
• The model is just a mathematical representation of the component (i.e. an equation). With a good model, you can obtain either transient or AC behavior. I will suggest you to start with simulating a simple RC model. Run both transient analysis and AC analysis. The same model works. That will help you understand the process. Granted, you won't always find an exact model but you can always approximate. Commented Apr 29, 2023 at 20:08
• Even if you don't end up using LTspice, this is a good read: ltwiki.org/files/LTspiceHelp.chm/html/Bode.htm Also, LTspice 17.1 now includes built-in FRA analysis: ez.analog.com/design-tools-and-calculators/ltspice/w/faqs-docs/… Commented Apr 30, 2023 at 8:12

Consider what you are asking for: you desire an average AC model, but the device in question has 20-some pins on it. Which pins are you expecting a model through? Under what mode/condition (driver, PWM current limiter) shall it be linearized or averaged? How many combinations of pins should they model for reasonable completeness across all end users that desire this type of model? And how many people will actually make use of such models, when a reasonably complete* transient model is provided instead? (That is, even if such a model is reasonable and meaningful, it might still not be worth crafting because too few people will make use of it to justify the expense.)

*Assumption.

And, what are you really asking for? -- A PWM cycle-averaged model of a gate/motor driver is just a buffer, give or take some phase shift due to propagation delay, and some gain factor due to modulator gain (if applicable). Besides the current limiting function, these components are trivial in such a model; were you expecting more?

Also be careful about what kind of "AC" models you are asking for. SPICE does not require models specific to this, because it performs linearization on the system automatically, using a small-signal steady-state assumption. Note that a switching circuit has approximately zero gain under this method (i.e., consider the gain of a logic gate where its input voltage is below the logic threshold), so you will be disappointed with the results from this analysis, if you use device models. (So, you are correct, with respect to your assumption that transient models will not work as-is for AC/average purposes.)

AC Analysis is only applicable to passive and analog circuits, where bias (operating point) is easily calculated from the circuit as given, and the small-signal frequency response is desired.

In contrast, as you move from simplified average models towards a practical PCB design, you must consider transient conditions within a switching cycle (peak current flows and voltage drops due to stray inductance from the layout and other component strays), cycle-to-cycle variations (e.g. ripple current, for purposes of dimensioning supply components), and quasi-steady-state conditions (e.g. heat dissipation of devices, for component selection and thermal design purposes). Few things which your average or AC model

The only duty you have at this later [implementation] stage, with respect to the earlier (average) model, is to show that they still exhibit the same averaged dynamics. Which I think you will find is a much simpler task than all the other considerations the transient models bring, and ultimately the whole design.

I'm also assuming this is in academic context, or perhaps a high-reliability design context, given the emphasis on modeling. In contrast, much practical engineering is done on assumptions and testing. If you are in fact doing the latter, I would suggest not worrying about it, and concentrate on solving implementation issues (with or without simulation).

Finally, keep in mind what you stand to learn / develop from a given model. If I understand your meaning correctly, then about all you're going to find from your average model is just the compensation components for the respective control loops. That's, at most, 9 PID parameters total across your three loops (or equivalent R and C component values if analog, or perhaps more parameters if more complex controllers are chosen). Whereas the complete design might involve, what, 50 or 100 components, or more? So the average model can only helping you with say 10% of the overall design -- a small part of the whole. And, you can assume those values will have to be chosen somehow, and just leave them as placeholders -- deferring choice of values until final modeling, or even "tune" them in testing.

• I understand from your answer that AC analysis (AC models) are just a starting point in the design process, and the whole work and focus are in the transient analysis of the whole system. On that I can make some assumptions on the gain and phase shift of the IC, and once the controller's components are sellected I have to focus on the transient analysis of the whole system and ajust the controller if necessary !! Commented May 1, 2023 at 4:27

As an example - let us consider the model for a transistor.

• There are pure ac models - based on h- or y- or z-parameters. These are linear models which are valid for small signals and a given DC operational point only. There are some simulation programs which are based on such simplified models - in most cases symbolic programs.

• On the other hand, the task of all SPICE based programs is circuit simulation that is not restricted to small signals only. More than that, supply voltages and all corresponding DC voltages and DC currents are an essential part of the circuits behaviour. Therefore, SPICE based simulation programs, of course, must contain corresponding large signal models (which, of course, can be used for small-signal operation).

• There is also an extension to the method in the first point, where a piecewise-linear model is constructed. This is what SIMPLIS does, and it's what eventually led the questioner to ask the current question at hand. Commented Apr 30, 2023 at 18:15