Although different SPICE-based simulators may include various enhancements to the basic version from the University of California at Berkeley, most use a similar approach in describing circuits. This approach involves capturing the information present in a circuit schematic in the form of a text file that follows a defined format. This format requires the assignment of alphanumeric identifiers to each circuit node, the assignment of component identifiers to each circuit device, and the definition of the significant parameters for each device. For example, the circuit description below shows the equivalent input file for the circuit shown in Fig. 26.1.

Examples for control of a behavioral resistor:

Small Signal Amplifier
*
* This circuit simulates a simple small signal amplifier.
*
Vin          Input 0                    0 SIN(0 .1 500Hz)
R_source     Input Amp_In               100
C1           Amp_In 0                   1uF
R_Amp_Input  Amp_In 0                   1MEG
E1           (Amp_Out 0) (Amp_In 0)    -10
R_Load       Amp_Out 0                  1000

.Tran 1.0u 0.01
.end

Figure 26.1: Example Circuit 1

This file exhibits many of the most important properties common to all SPICE circuit description files including the following:

• The first line of the file is always interpreted as the title of the circuit. The title may consist of any text string.
• Lines that provide user comments, but no circuit information, are begun by an asterisk.
• A circuit device is specified by a device name, followed by the node(s) to which it is connected, and then by any required parameter information.
• The first character of a device name tells the simulator what kind of device it is (e.g. R = resistor, C = capacitor, E = voltage controlled voltage source).
• Nodes may be labeled with any alphanumeric identifier. The only specific labeling requirement is that 0 must be used for ground.
• A line that begins with a dot is a `control directive' Control directives are used most frequently for specifying the type of analysis the simulator is to carry out.
• An .end statement must be included at the end of the file.
• With the exception of the Title and .end statements, the order in which the circuit file is defined is arbitrary.
• All identifiers are case insensitive - the identifier `npn' is equivalent to `NPN' and to `nPn'.
• Spaces and parenthesis are treated as white space.
• Long lines may be continued on a succeeding line by beginning the next line with a `+' in the first column.

In this example, the title of the circuit is `Small Signal Amplifier'. Three comment lines are included before the actual circuit description begins. The first device in the circuit is voltage source Vin, which is connected between node Input and `0' (ground). The parameters after the nodes specify that the source has an initial value of 0, a wave shape of SIN, and a DC offset, amplitude, and frequency of 0, .1, and 500 respectively. The next device in the circuit is resistor R_Source, which is connected between nodes Input and Amp_In, with a value of 100 Ohms. The remaining device lines in the file are interpreted similarly.

The control directive that begins with .tran specifies that the simulator should carry out a simulation using the Transient analysis mode. In this example, the parameters to the transient analysis control directive specify that the maximum time-step allowed is 1 microsecond and that the circuit should be simulated for 0.01 seconds of circuit time.

Other control cards are used for other analysis modes. For example, if a frequency response plot is desired, perhaps to determine the effect of the capacitor in the circuit, the following statement will instruct the simulator to perform a frequency analysis from 100 Hz to 10 MHz in decade intervals with ten points per decade.

.ac dec 10 100 10meg

To determine the quiescent operating point of the circuit, the following statement may be inserted in the file.

.op

A fourth analysis type supported by ngspice is swept DC analysis. An example control statement for the analysis mode is

.dc Vin -0.1 0.2 .05

This statement specifies a DC sweep that varies the source Vin from -100 millivolts to +200 millivolts in steps of 50 millivolts.