Ngspice Tutorial

Predicting the behavior of an electronic circuit using simulation tools enables us to run experiments, explore a larger set of alternatives, and verify results quickly and inexpensively.

Most modern circuit simulators are based on the SPICE (Simulation Program with Integrated Circuit Emphasis) simulator, developed at UC Berkeley, and first presented in 1973. In this tutorial, we will use ngspice, and just like the original Berkeley SPICE, it is open source.

Classes Using this Tutorial

• EE 220 Analog Integrated Circuits

Installing ngspice

ngspice is available for Linux, MacOS, and Windows machines. Visit the ngspice download page for specific installation instructions. The user manual is available here.

Our First Circuit

Let's simulate the circuit in Fig. 1 using ngspice. Note that we labeled every device (Q1, Vbe, and Vce), as well as labeled every unique node (b1, c1, and 0).

Figure 1: Our first circuit.

First, we need to describe the circuit using a "SPICE deck". In the 1970's, punched cards were used, and hence the reference to a "deck" of cards. Now, this just refers to a text file containing a description of our circuit. Since our description will contain circuit elements and nodes (or "nets"), this file is also commonly known as a "netlist".

This is the netlist for the circuit in Figure 1:

* Transistor Characteristic Curves
* LPA 2020-04-16
 
.include 2N2222A.lib
.options savecurrents
 
Q1  c1 b1 0     Q2n2222a
Vbe b1 0        dc 0
Vce c1 0        dc 0.2
 
.control
 
dc Vbe 500m 750m 1m
 
wrdata circuit1.dat @Q1[ic]
 
.endc
 
.end

Parts of a Netlist

The first line of a SPICE netlist is treated as the circuit title or description, and is always ignored by the simulator. Comments, like the one in line 2, are preceeded by an asterisk, (*).

SPICE “dot commands” are commands that provide directives to the simulator. These are the commands in lines 4, 5, 11, 17, and 19.

• The .include <filename> command includes other files, such as those that contain model information. In this case, .include 2N2222A.lib (line 4) adds the model file for a transistor, the 2N2222A NPN BJT.
• The .options savecurrents (line 5) command tells the simulator to save the current data, since by default, only voltage data is saved.
• The .control and .endc encapsulate the control statements, which specify which analyses will be performed by the simulator.
• The .end command signifies the end of the netlist file.