Signal Integrity

Welcome to Signal Integrity! Check out our “About” page for more info. Thanks for visiting.

In his retrospective Life of SPICE, Larry Nagel the co-author of SPICE (an acronym for "Simulation Program with Integrated Circuit Emphasis") noted:

SPICE was announced to the world … in Waterloo, Canada at the Sixteenth Midwest Symposium on Circuit Theory on April 12, 1973. The paper was presented by none other than Professor Donald O. Pederson of the University of California, Berkeley. I don’t think anyone had a clue of the impact of that paper or the computer program it described.

Well, impact it certainly had. So, in honor of SPICE’s thirty-sixth "birthday", here is the first of several interactive posts about how SPICE works. Here in part one we start simply with one time step (i.e. DC) solution of a circuit that consists of two unknown node voltages, V₁, V₂, a ground node V₀, three known ohmic conductances, G_xy = 1/R_xy (where I_xy = G_xy (V_y – V_x) and x and y are the node indices), and three known current sources.

You can solve a circuit using either Kirchhoff’s current law or voltage law or both. These laws are named after a German physicist Gustav Robert Kirchhoff (1824-87). (The ch in Kirchhoff is pronounced like the ch in the Scots word loch.) SPICE is a modified nodal solver and uses the current law: the sum of the currents into each node is zero. We’ll talk about what the ‘modified’ bit means in a future posting on ’super nodes.’ We’ll also postpone a discussion about when Kirchhoff’s laws break down for a future post (hint: Faraday’s law trumps Kirchoff’s law).

The nodes are joined by branches, so the other ingredients are the branch constitutive equations of the components that join them, for example V = IR if it’s an ohmic resisitor, V = L dI/dt for an inductor, etc. In this simple example, we have three simultaneous equations, one each from node 0, 1, and 2:

… with three unknowns, V₀, V₁, and V₂.

The same equations can be rearranged into matrix form, in this case the augmented (or indefinite) node conductance matrix relates the voltage and current vectors:

Note the ‘pattern of four’ that each conductance (e.g. G₀₁ highlighted in yellow above) impresses into the conductance matrix:

In SPICE parlance, making this ‘pattern of four’ impression is called ’stamping the matrix.’ Conveniently, this ’stamping’ generalizes for any number of nodes and two terminal components. In a future post, we’ll show how a small modification to this method allows us to ’stamp in’ a three- or four-terminal component like a voltage-controlled current source (and hence deal with transistors).

Pairs of nodes with no physical branch element connecting them have a conductance of 0. In practical circuits, the average number of non-zero conductances per node is only ~3-4, whereas the number of nodes can be quite large: hundreds, thousands, even millions. Thus, practical circuits have sparse, not full, conductance matrices: SPICE can make use of the efficiency of a sparse matrix solver.

An n+1 by n+1 augmented matrix has rank n. (In our simple example n = 2.) The normal (or definite) conductance matrix can be obtained simply by selecting a datum node (e.g. define node 0 to be 0V) and deleting its row and column. The matrix equation GV = I can then be solved for the column vector of voltages ([V₁; V₂]) by matrix inversion: V = G^-1I.

Now here’s the interactive part where we do exactly that:

Inputs:

Currents (A):

 I₀₁  I₁₂  I₂₀

Resistances (Ω):

 R₀₁  R₁₂  R₂₀

Results:

Conductances (S):

 G₀₁  G₁₂  G₂₀

Voltages (V):

 V₀  V₁  V₂

Look for a future posting on how SPICE deals with time-stepping (’transient analysis’), with reactive, four-terminal, and non-linear elements, and with shorts and voltage sources.

Here’s a link to the web page for the SPICE descendant in Agilent ADS: W2302 Transient Convolution Element