You need both mathematical equations and simulation, often in tandem, to produce accurate worst-case analysis. You also need accurate model correlation, which often takes work, before applying tolerances.

Circuit models are the heart of worst-case circuit analysis (WCCA). For simulations to be valid, you must gather and vet models or create them yourself; you can't usually rely on the manufacturer's model. Your models must correlate to datasheets or test data, and then you need to add tolerances to those models. Your goal is to create an accurate model with the "proper" fidelity. Too much fidelity results in high costs, but models that are too simple or inaccurate can result in bogus outcomes.

Modeling was my first assignment out of college and much of the material I published while at Intusoft is still relevant today. Reference 1 includes a link for a free download I wrote some years ago on modeling diodes and BJTs.

The WCCA for analog functional blocks (power systems, linear circuits) is most optimally performed using simulation (usually SPICE or some board level simulator such as ADS). In some cases, we have reviewed WCCAs that used 100% math (Mathcad) or 100% simulation. Neither technique is optimum for all types of analyses, nor are they even appropriate. You can't easily use math to perform many nonlinear analyses like transients or frequency domain stability. On the other hand, SPICE is overkill for many steady state assessments. Most analog WCCAs are about 50-50 math vs. simulation from a methodology standpoint. Digital WCCA is a bit of a different story, there, it is commonplace for all the analysis to be simulation based and you are largely dependent on the manufacturer provided IBIS models.

SPICE is a powerful tool, but you can easily get yourself into trouble and not know it. All it takes is one incorrect parameter in a sea of models, each with its own subcircuit or model parameter set, to invalidate the simulation’s results (Ref. 2).

For most SPICE based analyses, more than half the work scope is taken up deriving a believable, supportable, and correlated nominal model. Correlation is critical. Part and circuit models must be anchored to something known, at least nominally. How can we expect to perform parametric extreme value analysis (‘EVA’) or Monte Carlo analysis using worst-case tolerances if the nominal model isn’t within the range of the band of initial tolerances? You can’t just take a nominal model from a vendor, slap tolerances onto it, and assume the results are valid for all circuit configurations and operating ranges.

**Figure 1** shows a simple test circuit for simulating MOSFET transconductance (gFS). L1 and C2 are used to “open the loop” allowing you to measure the transfer function from the gate to the output, while maintaining a closed DC loop (Ref. 3).

**Figure 2a** (left) shows the circuit simulation of a fitted model made by AEi Systems while **Figure 2b** (right) shows the breadboard measured at load currents of 30 µA, 250 µA, 1mA, 10 mA, and 50 mA for comparison to the model performance. The motivation here is that most SPICE models for FETs are not accurate for linear operation so we created one. The SPICE models are generally set up for hard switching applications and V_{GS} isn't accurate for the low operating currents. The data usually isn't in the data sheet, but that's another story.

**Figure 2. We created our own simulation (a) because many MOSFET models don't cover low operating current. (b) shows the measured performance.**

**Figure 3** shows the same gFS data from a vendor-supplied SPICE model. The difference between Fig. 3 and Fig. 2a (our model) is clear.

**Figure 3. The same simulation using the SPICE model for the IRF230 from IRF.com. Note that in this case, the model kind of portrays the gFS characteristic but doesn’t get the actual performance quite right. The MOSFET manufacturer didn’t prioritize or evaluate the gFS performance at low currents and their subcircuit topology did not model it well.**

Transients, whether for part stress assessments or to assess circuit startup/EMC performance, AC analyses like stability, or any analysis that is not monotonic with respect to the outcome vs. tolerances, usually requires some sort of simulation model.

So herein lies the problem. Most analysts rely on the component manufacturers to supply the part models, often without checking the validity of the model in their circuit application. A model needs checking for both the characteristics needed and the operating range over which the characteristics need to be accurate.

This may come as a surprise, but vendor models often lack the fidelity you need. Important characteristics aren't modeled or only modeled at certain specific operating conditions. This is not to say that the models are wrong, but that they are often not accurate under the conditions you need. In most cases, documentation is scant, buried in the netlist, or nonexistent. This is a huge problem. Models need documentation and its often inexplicably not available. Without documentation, you don't know over which operating conditions the models are good or even what characteristics the models portray. SPICE models, by their very nature, have limitations. The trick is to know them and adapt the models accordingly.

How do you know if a model is any good? You must build test circuits that emulate the data sheet's test circuits and correlate all the parameters that must be right for your simulation. Then, you must correlate the entire application circuit model to test data or practical theory of some kind. It is only at that point that you can apply tolerances and run worst-case scenarios. In **Figure 4a**, you can see the top left plot how the vendor voltage reference model did not have the output impedance modeled. Therefore, it could not be used in transient or AC analyses. In **Figure 4b**, the vendor model is first order only and not very accurate.

**Figure 4. There are two aspects to SPICE models that need to be verified. Does the model exhibit the characteristic of interest and then how accurately is the characteristic modeled over the operating conditions needed? In (a), the model didn't at all portray the output impedance. In (b), the model varied the forward voltage with current, but not very accurately.**

Knowing how to do this requires knowledge of how to model each individual part using the simulator's syntax and available constructs, what characteristics are important, and how to spot when the circuit model doesn't behave properly. The debugging can be time-consuming and frustrating. It's simply not likely you will "luck into" a usable model without extensive experience in both the application and the parts involved. This is particularly true if you are trying to perform a WCCA on a circuit that has yet to be built and you have no test data.

End-of-life or worst-case tolerance models are normally not provided, so if the model isn't encrypted, you will have to learn where the parameter "knobs" are in the netlist so that you can apply tolerances to the characteristics for which the circuit is sensitive. This is a bit of a learned art, as sub-circuits from different manufacturers for the same part type (e.g. FETs) are different.

In addition, most SPICE parameters don't directly relate to a datasheet counter-part. For instance, in a diode there are three SPICE parameters that are used to fit the diode’s forward V-I response: N, IS, and RS. So, if you're only matching a few data points, there are multiple combinations that will get you there, though some can be physically unrealizable. More importantly, if you chose the wrong set, the model may not operate correctly outside of those data points.

[Continue reading on EDN US: Nominal isn't enough]

**References**

- Hymowitz, Ober, Robson, Horita, “Definitive Handbook of Transistor Modeling”
- Ho, Sandler, Hymowitz, “SPICE models need correlation to measurements,” EDN, June 2014.
- Sandler, Hymowitz, “SPICE Model Supports LDO Regulator Designs,” Power Electronics, 2005.
- Basso, “Switch-Mode Power Supplies Spice Simulations and Practical Designs”, ASIN: B012HU9XIU, 2010.
- Sandler, “Switched-Mode Power Supply Simulation with SPICE: The Faraday Press Edition”, ISBN-13: 978-1941071847, 2018
- Sandler, “Power Integrity: Measuring, Optimizing, and Troubleshooting Power Related Parameters in Electronics Systems”, ISBN-13: 978-0071830997, 2014. Book review.

**Related articles:**