Differences

This shows you the differences between two versions of the page.

--- simulating_a_time-varying_capacitor_in_spice [2024/09/08 17:14] – removed bm
+++ simulating_a_time-varying_capacitor_in_spice [2024/09/10 11:51] (current) – bm
@@ Line 1: / Line 1: @@
+=====Simulating a time-varying capacitor in Spice=====
+The relationship between the voltage $v_C$ over and the current $i_C$ through a capacitor is determined by its capacitance $C$:
+$$ i_C(t)=C\frac{dv_C(t)}{dt}$$
+However, this current-voltage relationship is not valid when the capacitor is varying in time. For a time variant capacitor, the equation modifies to:
+$$ i_C(t)=\frac{d}{dt}[C(t).v_C(t)]=C(t)\frac{dv_C(t)}{dt}+v_C(t)\frac{dC(t)}{dt}$$
+Rearranging this equation gives an expression for the voltage over the capacitor:
+$$ v_C(t)=\frac{1}{C(t)}[C(0)v_C(0)+\int_0^t i_C(t) dt] $$
+valid if $C(t)\neq 0$ at //any// time.
+We will use this expression to simulate a time-varying capacitor in LT Spice. Notice the limitation that $C(t)\neq 0$ at //any// time.
+Suppose we want we simulate a sinusoidal value in function of time with a certain offset: $C(t)$= 5 nF + 3 nF.sin(2π.100 kHz.t). In order to realize this, we have to introduce a custom component in SPICE with the following subcircuit:
+<code>
+.subckt capacitor + - params: VC0=0
+.func C(time) {5n+3n*sin(2*pi*100k*time)}
+hvolt + - value={(sdt(I(hvolt))+VC0*C(0))/C(time)}
+.ends
+</code>
+Current Dependent Voltage Source
+The voltage over the capacitor (see equation above) is modeled via a current dependent voltage source ''hvolt''. The integral is realized via the ''sdt'' function in SPICE. The initial value at time t=0 of the capacitor must be given as parameter.
+First, we save the code for this subcircuit into a .txt-file and, for example, place this file in the same folder as your SPICE circuit file.
+Next, open the text file in LT Spice, right click on the first word ".subckt", and select "Create symbol".
+The program asks you if you wish to automatically create a symbol. Click "yes". A .asy file is created which contains your custom time-varying capacitor, typically in the folder 'C:Users\YourUserName\AppData\Local\LTspice\lib\sym\AutoGenerated'
+To use the time-varying capacitor in a circuit, click "component" (F2) and insert the custom capacitor by searching "capacitor" in the window.
+Plotting the value of the capacitance in SPICE in function of time is not straightforward. Let us just check some individual times: we compare the value of the current through and voltage over the capacitor (i) in the case of the time-varying capacitor at time $t_i$ (after the transition period), and (ii) in the case of a static capacitor with value $C(t_i)$.
+Case (i): We apply a high frequency source in order to create an envelope facilitating comparison between both cases.
+{{:simulating_a_time-varying_capacitor_in_spice-1.png|}}
+At a certain time, e.g., t=50µs, the value of the capacitor equals $C$(50µs)=  5 nF + 3 nF.sin(2π.100 kHz.50µs)=5 nF.
+If we then zoom in at the simulation at t=50µs, we find the peak value of voltage over and current through the inductor.
+Case (ii): We compare this value with a static inductor of 5 nF:
+{{:simulating_a_time-varying_capacitor_in_spice-2.png|}}
+We find that both the current and voltage correspond to case (i).
+We do the same for a lot of other values of time, and always find a correspondence between both cases. This is not a rigid proof, but it gives us sufficient confidence that the capacitor was modeled correctly in SPICE.
+----
+**References**
+  * Biolek, D., Kolka, Z., & Biolkova, V. (2007). Modeling time-varying storage components in PSpice. In Proc. Electronic Devices and Systems IMAPS CS International Conference EDS (Vol. 2007, pp. 39-44).