1
\$\begingroup\$

A real capacitor can be modeled using a series RLC equivalent circuit. However, there are still discrepancies between the two. I've generated a waveform from the lab and I've modelled the equivalent series RLC. Why are there discrepancies between the two circuits and how can I generate a model that more closely resembles the lab generated waveform?

The first image is the lab-generated waveform for the voltage across a 2.2uF capacitor, second image is the simulated waveform resulting from the series RLC equivalent. Both have 200k Hz, 10Vp-p square wave input Lab generated waveform Simulated readings from modelled series RLC circuit

\$\endgroup\$
  • 2
    \$\begingroup\$ You need to model the test equipment as well. \$\endgroup\$ – Ignacio Vazquez-Abrams Oct 30 '16 at 19:42
  • \$\begingroup\$ Looks like saturated input of amplifier before the ADC :) Sometimes the clip the signal. Seriously, what were you simulating and modeling? Even the units seem very different \$\endgroup\$ – Gregory Kornblum Oct 30 '16 at 19:47
  • \$\begingroup\$ Is that the only way to get a better model? \$\endgroup\$ – Alura Oct 30 '16 at 19:47
  • \$\begingroup\$ @GregoryKornblum The first graph is just the voltage across a 2.2uF capacitor with an input of a 200k Hz 10Vp-p square wave, then the second is the simulation on LTspice. The units don't look different to me, both have a peak to peak amplitude of about 205mV and a period of about 5us \$\endgroup\$ – Alura Oct 30 '16 at 19:51
  • 1
    \$\begingroup\$ The biggest difference between the two looks to be that the inductive "spike" is narrower in simulation than in real life. That could be caused by the measurement system bandwidth, or additional parasitic components such as a capacitance in parallel with R or L. But I wouldn't worry about it, barring more information about your application, your simulation is good enough. The goal of simulation is usually to capture the reproducible and important behavior of a circuit, not the exact parasitics of a specific single capacitor. \$\endgroup\$ – Evan Oct 30 '16 at 20:46
1
\$\begingroup\$

If we had an FFT amplitude and phase, one could get a perfect passive model of all the elements, knowing that the source is 50Ω and thus the transfer function.

The signal has the following characteristics from which a model can be generated.

  • Slew rate dV/dt= 200mV/1us or dt/dV=5us/V (*)
  • ΔVin=10Vpp thus with 50Ω source
  • ΔIc=10V/50Ω=200mA
  • Vpp= 200mV but asymptotic slopes of Vout project to 222 mVpp thus
    • fundamental dt/dV becomes 4.5us/V (*)

Since C=Ic dt/dV = 200mA * 4.5us/V = **0.9 uF and not 2.2 uF**

However with a simulator you can model the waveform and adjust the parameters. From this I get RLC1= 0.6uF+ 20nH + 50mΩ and RLC2 = 0.8uF + 0nH + 300mΩ (in //)

enter image description here

It is either Rs=100 Ohm source and 1.8uF or 50 Ohm source and 0.9uF with an ESR=50mΩ approx with about 20nH of ESL and many other RLC smaller networks shunting the RL network.

schematic

simulate this circuit – Schematic created using CircuitLab

This is also why C(f), ESR and ESL changes value with sine frequency due to reactance model. But SRF and PRF will give a better model and a scatttering s22 plot is the best from the OEM.

\$\endgroup\$
0
\$\begingroup\$

There are non-linear equations that can be used to model most things more accurately.

https://www.ema-eda.com/sites/ema/files/resources/files/nonlinear-capacitor-model.pdf

http://www.designers-guide.org/modeling/varactors.pdf

When you start with the fundamental equations describing the ideal non-linear capacitor, such as the ones listed above, you can then add various things like noise, hysteresis, non-linear resistance, non-linear inductance, RF characteristics, etc. Each addition gives you more accuracy but also requires more input parameters to describe those characteristics.

My guess as to why the curves are different is the non-linear capacitor includes some of these effects. Most likely the noise and inductive effects as these are more commonly modeled.

Also, the measurement of these introduces errors. There are quantization errors in the ADC, loading effects due to the probes, etc. RF effects being picked up, etc. The list goes on and on. The main thing to get out of is actually that the graphs are pretty close. The main differences seem to be "noise". In 99.9% of all electronics, you'll be ok making the assumption that capacitors are ideal/linear(within the SOR).

I would point out that these non-linear effects are generally not required and not desirable to model. 1. They slow down analysis significantly and are not always stable. 2. They don't add much to the precision of the analysis. 3. Actual components are more variable so one never will be completely accurate. 4. Most components function quite close to the linear model but vastly different to the non-linear model. (e.g., because of noise, no two components ever function exactly the same) 5. Measurement of actual components require using real measurement devices. These devices are also inaccurate so they add to the inaccuracies. The linear model and some of the non-linear models are derived from first principles(math + physics) and hence are "true" and can be relied on.

\$\endgroup\$
0
\$\begingroup\$

You can model dielectric absorption as a string of RC circuits in parallel with an ideal capacitor.

enter image description here

\$\endgroup\$

Your Answer

By clicking “Post Your Answer”, you agree to our terms of service, privacy policy and cookie policy

Not the answer you're looking for? Browse other questions tagged or ask your own question.