Chapter 7 - Using The spice Circuit Simulation Program
“Garbage in, garbage out.”
SPICE is a very reliable piece of software, but it does have its little quirks that take some getting used to. By “quirk” I mean a demand placed upon the user to write the source file in a particular way in order for it to work without giving error messages. I do not mean any kind of fault with SPICE which would produce erroneous or misleading results: that would be more properly referred to as a “bug.” Speaking of bugs, SPICE has a few of them as well.
Some (or all) of these quirks may be unique to SPICE version 2g6, which is the only version I’ve used extensively. They may have been fixed in later versions.
SPICE demands that the source file begins with something other than the first “card” in the circuit description “deck.” This first character in the source file can be a linefeed, title line, or a comment: there just has to be something there before the first component-specifying line of the file. If not, SPICE will refuse to do an analysis at all, claiming that there is a serious error (such as improper node connections) in the “deck.”
SPICE demands that the .end line at the end of the source file not be terminated with a linefeed or carriage return character. In other words, when you finish typing “.end” you should not hit the [Enter] key on your keyboard. The cursor on your text editor should stop immediately to the right of the “d” after the “.end” and go no further. Failure to heed this quirk will result in a “missing .end card” error message at the end of the analysis output. The actual circuit analysis is not affected by this error, so I normally ignore the message. However, if you’re looking to receive a “perfect” output, you must pay heed to this idiosyncrasy.
You are given much freedom in numbering circuit nodes, but you must have a node 0 somewhere in your netlist in order for SPICE to work. Node 0 is the default node for circuit ground, and it is the point of reference for all voltages specified at single node locations.
When simple DC analysis is performed by SPICE, the output will contain a listing of voltages at all non-zero nodes in the circuit. The point of reference (ground) for all these voltage readings is node 0. For example:
node voltage node voltage ( 1) 15.0000 ( 2) 0.6522
In this analysis, there is a DC voltage of 15 volts between node 1 and ground (node 0), and a DC voltage of 0.6522 volts between node 2 and ground (node 0). In both these cases, the voltage polarity is negative at node 0 with reference to the other node (in other words, both nodes 1 and 2 are positive with respect to node 0).
SPICE cannot handle open circuits of any kind. If your netlist specifies a circuit with an open voltage source, for example, SPICE will refuse to perform an analysis. A prime example of this type of error is found when “connecting” a voltage source to the input of a voltage-dependent source (used to simulate an operational amplifier). SPICE needs to see a complete path for current, so I usually tie a high-value resistor (call it rbogus!) across the voltage source to act as a minimal load.
SPICE cannot handle certain uninterrupted loops of components in a circuit, namely voltage sources and inductors. The following loops will cause SPICE to abort analysis:
netlist l1 2 4 10m l2 2 4 50m l3 2 4 25m
netlist v1 1 0 dc 12 l1 1 0 150m
netlist c1 5 6 33u c2 6 7 47u
The reason SPICE can’t handle these conditions stems from the way it performs DC analysis: by treating all inductors as shorts and all capacitors as opens. Since short-circuits (0 Ω) and open circuits (infinite resistance) either contain or generate mathematical infinitudes, a computer simply cannot deal with them, and so SPICE will discontinue analysis if any of these conditions occur.
In order to make these component configurations acceptable to SPICE, you must insert resistors of appropriate values into the appropriate places, eliminating the respective short-circuits and open-circuits. If a series resistor is required, choose a very low resistance value. Conversely, if a parallel resistor is required, choose a very high resistance value. For example:
To fix the parallel inductor problem, insert a very low-value resistor in series with each offending inductor.
original netlist l1 2 4 10m l2 2 4 50m l3 2 4 25m
fixed netlist rbogus1 2 3 1e-12 rbogus2 2 5 1e-12 l1 3 4 10m l2 2 4 50m l3 5 4 25m
The extremely low-resistance resistors Rbogus1 and Rbogus2 (each one with a mere 1 pico-ohm of resistance) “break up” the direct parallel connections that existed between L1, L2, and L3. It is important to choose very low resistances here so that circuit operation is not substantially impacted by the “fix.”
To fix the voltage source / inductor loop, insert a very low-value resistor in series with the two components.
original netlist v1 1 0 dc 12 l1 1 0 150m
fixed netlist v1 1 0 dc 12 l1 2 0 150m rbogus 1 2 1e-12
As in the previous example with parallel inductors, it is important to make the correction resistor (Rbogus) very low in resistance, so as to not substantially impact circuit operation.
To fix the series capacitor circuit, one of the capacitors must have a resistor shunting across it. SPICE requires a DC current path to each capacitor for analysis.
original netlist c1 5 6 33u c2 6 7 47u
fixed netlist c1 5 6 33u c2 6 7 47u rbogus 6 7 9e12
The Rbogus value of 9 Tera-ohms provides a DC current path to C1 (and around C2) without substantially impacting the circuit’s operation.
Although printing or plotting of voltage is quite easy in SPICE, the output of current values is a bit more difficult. Voltage measurements are specified by declaring the appropriate circuit nodes. For example, if we desire to know the voltage across a capacitor whose leads connect between nodes 4 and 7, we might make out .print statement look like this:
c1 4 7 22u .print ac v(4,7)
However, if we wanted to have SPICE measure the current through that capacitor, it wouldn’t be quite so easy. Currents in SPICE must be specified in relation to a voltage source, not any arbitrary component. For example:
c1 4 7 22u vinput 6 4 ac 1 sin .print ac i(vinput)
This .print card instructs SPICE to print the current through voltage source Vinput, which happens to be the same as the current through our capacitor between nodes 4 and 7. But what if there is no such voltage source in our circuit to reference for current measurement? One solution is to insert a shunt resistor into the circuit and measure voltage across it. In this case, I have chosen a shunt resistance value of 1 Ω to produce 1 volt per amp of current through C1:
c1 4 7 22u rshunt 6 4 1 .print ac v(6,4)
However, the insertion of an extra resistance into our circuit large enough to drop a meaningful voltage for the intended range of current might adversely affect things. A better solution for SPICE is this, although one would never seek such a current measurement solution in real life:
c1 4 7 22u vbogus 6 4 dc 0 .print ac i(vbogus)
Inserting a “bogus” DC voltage source of zero volts doesn’t affect circuit operation at all, yet it provides a convenient place for SPICE to take a current measurement. Interestingly enough, it doesn’t matter that Vbogus is a DC source when we’re looking to measure AC current! The fact that SPICE will output an AC current reading is determined by the “ac” specification in the .print card and nothing more.
It should also be noted that the way SPICE assigns a polarity to current measurements is a bit odd. Take the following circuit as an example:
example v1 1 0 r1 1 2 5k r2 2 0 5k .dc v1 10 10 1 .print dc i(v1) .end
With 10 volts total voltage and 10 kΩ total resistance, you might expect SPICE to tell you there’s going to be 1 mA (1e-03) of current through voltage source V1, but in actuality, SPICE will output a figure of negative 1 mA (-1e-03)! SPICE regards current out of the negative end of a DC voltage source (the normal direction) to be a negative value of current rather than a positive value of current. There are times I’ll throw in a “bogus” voltage source in a DC circuit like this simply to get SPICE to output a positive current value:
example v1 1 0 r1 1 2 5k r2 2 3 5k vbogus 3 0 dc 0 .dc v1 10 10 1 .print dc i(vbogus) .end
Notice how Vbogus is positioned so that the circuit current will enter its positive side (node 3) and exit its negative side (node 0). This orientation will ensure a positive output figure for circuit current.
When performing a Fourier (frequency-domain) analysis on a waveform, I have found it necessary to either print or plot the waveform using the .print or .plot cards, respectively. If you don’t print or plot it, SPICE will pause for a moment during analysis and then abort the job after outputting the “initial transient solution.”
Also, when analyzing a square wave produced by the “pulse” source function, you must give the waveform some finite rise and fall time, or else the Fourier analysis results will be incorrect. For some reason, a perfect square wave with zero rise/fall time produces significant levels of even harmonics according to SPICE’s Fourier analysis option, which is not true for real square waves.
Published under the terms and conditions of the Design Science License