SPICE Models for Ceramic Capacitors … (Nearly) Better Than the Real Thing?

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 %).

Figure 1

Figure 2

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).

Figure 3

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.

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 6

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.

Figure 7

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).

Figure 8

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).

Figure 9

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.


1) VY1 Series and VY2 Series

2) EIA-198-1-F standard, published by: Electronic Components Industry Association (ECIA), 2002

3) Modeling voltage-controlled resistors and capacitors in PSpice

2 comments on “SPICE Models for Ceramic Capacitors … (Nearly) Better Than the Real Thing?

  1. Doug.Leeper
    November 14, 2018

    It would be nice to see the common DC Bias (drop in capacitance when DC is on the capacitor), value drop in the model.

    Also lacking from most models is how the caps reduce in value as they age.

    The difficult thing, is as they have pushed to high C*V values in a given size, they have gone to 5um ceramic layers, and the DC Bias you see in a particular series, like X7R, can vary *quite* a bit between suppliers. Some at 50% of the DC rating drop by 80% of their value, others only 20%.  Each has different “doping” of the ceramic with various elements.

    Conversely, Reliabilty would be good to see in a model.  If you dig down to an individual datasheet for a specific part, instead of just the family series sheet, you will see that instead of the standard 200% to 300% applied voltage for the Reliability- Durability or also called Long Term High Operating Temp. So, basically- like with an X5R you put 200% to 300% of it's working voltage on it and run it at the characteristics maximum temp, so X5R you would use 85 degrees C, for 1000 hours, and you have to pass a number of parameters.

    However, all the vendors have had to drop the overvoltage value, many are down to 100% of the working voltage for this test.  And there are some that are intended for Mobile applications, that not only do this, but then have a chart, and depending on your voltage and temp, you will only get a 3 year life out of the part before 1% will fail.

    Anyhow it would be nice to see some of this in the models.

    One needs to really dig down in the datasheets for the parts these days, lots of cutting corners to worship at the Altar of BOM.  The devil is always in the details….

  2. Alain Stas
    November 15, 2018

    Hello Doug

    In fact, during the simulation, the user can measure the current passing into and the voltage across the capacitors.

    Also the tolerances tolCmin and tolCmax are independently tunable.These are respectively the minimal and maximal tolerances on the capacitor. So if at 0 Hrs you have a tolerance of +/-10% , you can indicate tolCmin= -10 and tolCmax=+10 (if you don't, it's already implemented into the modelsanyway) . But for a drift between -5% and -10 % during the lifetime, then it will be worth to perform the simulation while writing tolCmin =-20 and tolCmax = +5 or any other limits given by the manufacturer.

    By the way the models presented in this article will be uploaded on the Vishay website soon but they are availble on simple mail request at

    I like your last sentence: the devil is always in the details…….Thanks for your reaction.

Leave a Reply

This site uses Akismet to reduce spam. Learn how your comment data is processed.