First of all, I want to emphasize the word “nearly” in the slightly provocative title of this article. No SPICE model can be better than the real measurements performed on electronic components, which are sometimes patiently gathered over the course of weeks and years. Yet when modelling is done correctly and completely — taking all the phenomena characterized by these measurements into account — its use can save time and simplify experimentation. Sometimes, modelling also allows for the interpolation of characteristics for intermediary part numbers between two extremes. In a nutshell, SPICE models can be used to present these measurements in a velvet case.
But I digress. The reference components for this article are Vishay’s VY1 / VY2 series ceramic capacitors1 . These are highly non-linear capacitors, whose capacitance value is dependent on both temperature and the applied voltage. The temperature dependence of the capacitance value is determined by the material used to manufacture the device. For the neophytes in electronic ceramics, these materials seem to have Star Wars -esque names like X5R, S3L, Y5U, and U2J. 3PO is not one of them, though!!!
The temperature and electrical field sensitivity for the Y5U material is reprinted as an example in Figures 1 (temperature) and 2 (voltage). Y5U is a Class 2 material per EIA RS-1982 , operating between -30 o C (first digit: Y) and +85 o C (last digit: U), and the maximum capacitance variation is defined by the middle digit: 5 (+22 % / -56 %).
If we want to produce realistic models for such elements, we also need to take two other figures into account: the leakage current (dependent on the applied voltage, as represented in Figure 3) and the impedance vs. frequency relationship (the self-resonance frequency is inversely proportional to that capacitance value, as shown in Figure 4).
With such non-linear variations, SPICE is the ideal software for this type of device. Most of the time, SPICE techniques for complex devices involve analog behavior sources (also called arbitrary behavior sources) and are ideal for reproducing such relationships. Several examples of such technique can be found in the application note “Modeling Voltage-Controlled Resistors and Capacitors in PSpice.”3
The LTspice schematics principle for such a temperature- / voltage-dependent device is represented in Figure 5.
Aside from the equivalent series resistance (ESR) and inductance (ESL), the ceramic capacitor behavior is modeled via two current sources.
The first current source is named Bfunct. Its current must be capacitive and thus made proportional to a small sense capacitive current passing through capacity (C1), connected to a source (Ecopy) derived from the voltage applied to the model. This current is also proportional to the nominal capacitance value (Cnom, 25 o C, 0 V) and to a function that is both voltage- and temperature-dependent. Then comes the Bleakage source, which represents the leakage current and is also dependent upon the applied voltage.
Once the model is created, we can proceed to the virtual capacitance measurement for different DC voltages and temperatures. In Figure 6, we apply a 1 kHz AC voltage on top of a DC voltage, and measure the SPICE capacitance value by analyzing the AC current variation compared to the DC leakage current:
Cspice = (Imax – Ileakage) / (Vmax 2 π f), where Vmax = 5 V, f = 1 kHz, Imax is the maximum swing current into the capacitor, and Ileakage is the current corresponding to the VDC voltage.
SPICE simulation measurements can be directly compared to the real physical measurements (voltage at node CY5Umeas).
Figure 7 below shows a direct comparison in the LTspice log file between the measurements Cy5um and the SPICE computations (which allows for implementing the maximum and minimal tolerances). One can hardly see the differences between the SPICE simulation results and the original datasheet curve.
The variations in the capacitance for five different ceramic materials as a function of the temperature can also be reproduced (see Figure 8; the points are the experimental measurements).
We can even reproduce the self-resonance graphs of Figure 4 for all our models by performing a frequency sweep small signal AC simulation (circuit in Figure 9 and results in Figure 10).
So, we come back to the question in this article’s title: Are SPICE models for ceramic capacitors nearly better than the real thing?
Having seen the impressive results in Figures 7, 8, and 10, I’ll rest my case stating that this question has now become completely rhetorical.