Supernodes and KCL

Question

Lets talk about Colpitts oscillator again (or the very basic circuit theory if you want). Suppose I modeled circuit as on the schematics below

I am interested in systematic ways of obtaining circuit state-space equations with no ad hoc computations. Modified nodal analysis works fine but for obvious reasons I am iterested in ODEs rather than DAEs. In this simplified circuit there is proper tree (blue edges) and (red) co-tree.

To formulate state equations I need to write KCL for each capacitor and its selected node or supernode (see 19.3 in the link).

Situation is straightforward if I choose \$+\$node \$+v_{C_{\mathrm{b}}^{\mathrm{d}}}\$. Then we are left with \begin{equation} \frac{\mathrm{d}v_{C_{\mathrm{b}}^{\mathrm{d}}}}{\mathrm{d}t} + i_{R_c} - \alpha_{\mathrm{F}}i_{\mathrm{E}} - i_{R_b} = 0 \end{equation}

Problem. Suppose, that I choose + node of \$v_{C_{\mathrm{g}}}\$. As I understand, I should make something called supernode. By definition, supernode is the set of all braneches of the tree incident with the node. In this case it is \$v_{C_{\mathrm{b}}^{\mathrm{g}}}\$. Does it mean, that each time I must go along path of tree until I reach node, where there are only co-tree braneches?

For this example, does it mean, that \begin{equation} \frac{\mathrm{d}v_{C_g}}{\mathrm{d}t} + (1 + \alpha_{\mathrm{F}})i_{\mathrm{E}} + i_{R_{\mathrm{b}}} + i_{L}= 0 \end{equation}

Edit. I ended up with the equation below (with simplified notation \$C_g^b = C_1\$ and \$C_d^b = C_2\$)

\begin{align} \begin{bmatrix} 0 & -\frac{1}{L} & 0 & \frac{1}{L} & 0 \\ \frac{1}{C_g} & -\frac{1}{C_g R_B} & -\frac{1}{C_g R_B} & \frac{1}{C_g R_B} & \frac{1}{C_g R_B}\\ 0 & -\frac{1}{C_{g}^{b}R_B} & -\frac{1}{C_{g}^{b}R_B} & \frac{1}{C_{g}^{b}R_B} & \frac{1}{C_{g}^{b}R_B}\\ -\frac{1}{C_d} & \frac{1}{C_d R_B} & \frac{1}{C_d R_B} & -\frac{1}{C_d R_B} - \frac{1}{C_{d}^{b}R_C} & -\frac{1}{C_d R_B} - \frac{1}{C_{d}^{b}R_C}\\ 0 & \frac{1}{C_d R_B} & \frac{1}{C_d R_B} & -\frac{1}{C_d R_B} - \frac{1}{C_{d}^{b}R_C} & -\frac{1}{C_d R_B} - \frac{1}{C_{d}^{b}R_C} \end{bmatrix} \begin{bmatrix} i_L\\ v_g\\ v_1\\ v_d\\ v_2 \end{bmatrix} + \begin{bmatrix} 0\\ \frac{\alpha - 1}{C_g}\\ \frac{\alpha - 1}{C_g^b}\\ -\frac{\alpha}{C_d}\\ -\frac{\alpha}{C_d^b} \end{bmatrix}\frac{I_s}{\alpha}\left(\mathrm{exp}\,\left(\frac{v_g + v_1}{V_T}\right) - 1\right) + \begin{bmatrix} 0\\ 0\\ 0\\ \frac{1}{R_C C_d}\\ \frac{1}{R_C C_d^b} \end{bmatrix}\overline{U} \end{align}

If I choose \$ C_d = 2C_g\$, Runge-Kutta 45 integration converges with no additional scaling. Using stiff ODE solver implemented in Matlab, I can get all trajectories with values in ranges \$I_s = 10^{-13}\$ while \$C_g = 10^{-12}\$, \$R_b = 10^{5}\$ etc. But when I consider a situation where \$ C_d = C_g\$, integration is immediately singular from the beginning. I also check the process step by step using Euler explicit integration and it clearly showed that the current \$i_E\$ is growing extremely fast after few steps. Is something wrong with the circuit then? For \$\alpha = 0.99\$ and values \$R_c = 400\mathrm{k}\$, \$R_b = 4\mathrm{k}\$, \$C_d = C_g = 25\mathrm{pF}\$, \$L = 125\mathrm{nH}\$, both \$C_{\mathrm{block}} = 10\mathrm{nF}\$, \$\overline{U} = 5-10\mathrm{V}\$ it seems ok. Also simulation with NPN in LTSPICE worked fine. Is my simplified Ebers-Moll model misused?

Answer 1

Do you really expect the integration to NOT blow up in your formulation? Thinking about it, I would suspect if you choose initial conditions where locally the oscillation criteria is fulfilled then naïve integration of these equations will simply result it the emitter current blowing up.

So as I see it, you need to implement what happens in the real world, i.e you will need some form of additional non-linearity/limiting for what would represent the limited supply voltage/current compliance, this will interact with the diode non linearity and give you stable limit cycles.

Spice for example does something similar with such devices, when it is attempting to converge it limits the slope of the exponential which is what also happens with real devices.

Answer 2

Is my simplified Ebers-Moll model misused?

Yes, you can't use an exponential in a linear model or a set of linear equations unless you check for stability, this is the subject of books and courses (if your really want to go this route, they cover the topic of stability and state space systems in many mutivariable controls classes).

The best route is to linearize the diode about the operating point. This is how spice works. It finds an operating point then creates a linear model about that point, then solves it with a solver, it then advances the timestep and then does it all over again.

The last problem with the whole simulation/circuit model is it also uses ideal sources and there are no parasitics of the components (most real world components have all three R L and C components. For example an SMT resistor will have a few pfs of capacitance in parallel and some inductance from the pads, wires and traces also have inductance and resistance) which will make the behavior differ vastly from a circuit (especially at high frequencies) built in the real world (like on a PCB).