UNIVERSITY of PENNSYLVANIA

DEPARTMENT OF ELECTRICAL ENGINEERING
 
 

SPICE - A Brief Overview
(URL: http://www.seas.upenn.edu/~jan/spice/spice.overview.html)

 


This document gives a brief overview of SPICE. The description is far from complete, as SPICE is a powerful circuit simulator with many capabilities. However, this document will serve as a start for students in introductory classes. For more information, please refer to the SPICE user's manual or books listed at the end of the document.

Do not print this document on the CETS printers.

  1. INTRODUCTION

    2.  

     
     
     

  2. HOW TO SPECIFY CIRCUIT TOPOLOGY AND ANALYSIS?

    3.  

     
     
     

  3. PSPICE - Getting started
  4. HSPICE

    5.  

     
     
     

  5. EXAMPLES
  6. MODELS of Selected Devices and Components
  7. MOST COMMON MISTAKES

    8.  

     
     
     

  8. WHEN SPICE DOES NOT RUN

    9.  

     
     
     

  9. REFERENCES

1. INTRODUCTION

SPICE is a powerful general purpose analog circuit simulator that is used to verify circuit designs and to predict the circuit behavior. This is of particular importance for integrated circuits. It was for this reason that SPICE was originally developed at the Electronics Research Laboratory of the University of California, Berkeley (1975), as its name implies:
 
  PSpice is a PC version of SPICE (MicroSim Corp.) and HSpice is a version (Avant!.) that runs on workstations and larger computers. PSpice is available on the PCs in the SEAS PC computing Labs and HSPICE is available on ENIAC or PENDER. A complete manual of the Avant! Star- HSPICE (pdf document) is available as well.

SPICE can do several types of circuit analyses. Here are the most important ones:
 
 

In addition, PSpice has analog and digital libraries of standard components (such as NAND, NOR, flip-flops, and other digital gates, op amps, etc). This makes it a useful tool for a wide range of analog and digital applications.

All analyses can be done at different temperatures. The default temperature is 300K.

The circuit can contain the following components:
 
 

2. HOW TO SPECIFY THE CIRCUIT TOPOLOGY AND ANALYSIS?

A SPICE input file, called source file, consists of three parts.
 
 
  1. Data statements: description of the components and the interconnections.
  2. Control statements: tells SPICE what type of analysis to perform on the circuit.
  3. Output statements: specifies what outputs are to be printed or plotted.
Although these statements may appear in any order, it is recommended that they be given in the above sequence. Two other statements are required: the title statement and the end statement. The title statement is the first line and can contain any information, while the end statement is always .END. This statement must be a line be itself, followed by a carriage return! In addition, you can insert comment statements, which must begin with an asterisk (*) and are ignored by SPICE.
 
  Format: The statements have a free format and consist of fields separated by a blank. If one wants to continue a statement to the next line, one uses a "+" sign (continuation sign) at the beginning of the next line. Numbers can be integers, or floating points. For example,
 
  One can also use the following scale factors:
 
 

T(= 1E12 or 10+12); G(= E9); MEG(= E6); K(= E3); M(= E-3); U(= E-6); N(= E-9); P(= E-12), and F(= E-15)
 
 

Both upper and lower case letters are allowed in PSpice and Hspice (SPICE uses only uppercase characters). As an example, one can specify a capacitor of 225 picofarad in the following ways:
 
 

2.1 Data Statements to Specify the Circuit Components and Topology

a. Independent DC Sources

Voltage source: Vname N1 N2 Type Value

 Current source: Iname N1 N2 Type Value
 
 

Examples: The positive current direction through the current or voltage source is from the positive (N1) node to the negative (N2) node: Voltage and Current Conventions:
  1. Spice always assigns a positive reference mark to the 1st node and uses the passive sign convention to assign the current reference.
  2. Spice uses the node-voltage analysis. It solves for the unknown node voltages and also the unknown currents through independent voltage sources. This gives us a way to find currents flowing in elements: one has to ask for the current through a voltage source. Thus one can insert an independent voltage source of zero value in series with the element in which one wants to know the current, as shown in the example below:

    3.  

     
     
     

b. Dependent Sources

Voltage controlled voltage source: Voltage controlled current source: Current controlled voltage source: Current controlled current source:

c. Resistors

d.Capacitors (C) and Inductors (L)

e. Mutual Inductors

A mutual inductance in SPICE is defined by specifying the coupling coefficient K between the two inductors. The syntax is as follows:
 
  The value of K must be larger than 0 but smaller than 1. Spice does not support perfect coupling (k=1). The above statement must always be together with the statements for the two inductors. An example is given in the figure below. The coupling coefficient K can be calculated as K=M/sqrt(L1xL2)=0.81.
 
 

The SPICE statements to define the above coupled coils are as follows.
 
 

The DOTS are always associated with the first node of the inductances (i.e. node no. 3 of L1 and no. 4 of L2). Also SPICE will assign the positive node voltage to the first node of the inductance (i.e. the DOT) and use the passive sign convention for the current direction as indicated in the figure above. For an example circuit see under the section Examples.
 
 

f. Ideal Transformer

SPICE has no model for an ideal transformer. An ideal tranformer is simulated using mutual inductances such that the transformer ratio N1/N2 = sqrt(L1/L2). Make the coupling factor K close to one (ex. K=0.99999) and choose L such that wL >> the resistance seen be the inductor. The secondary circuit needs a DC connection to ground. This can be accomplished by adding a large resistor to ground or giving the primary and secondary circuits a common node. For an example circuit see under the section Examples

g. Sinusoidal sources

If TD, THETA and PHASE are not specified, it is assumed to be zero.
 
  The last example is an undamped, undelayed sinusoid with an amplitude of 10V and frequency of 50 Hz.
 
 

To generate a cosine function, you can make use of the phase relationship between the sinusoid and cosine. Here is an example of an undelayed cosine with an amplitude of 5V and frequency of 50 Hz.
 
 

h. Piecewise linear source (PWL)

in which (Ti Vi) specifies the value Vi of the source at time Ti

 Example:

i. Pulse

V1 - initial voltage; V2 - peak voltage; TD - initial delay time; Tr - rise time; Tf - fall time; pwf - pulse-wise; and Period - period.
 
  Other sources such as polynominal controlled source, exponential source, FM-modulated source, etc. can be specified. For information on these components, check the SPICE manual.
 
 

j. Voltage- and Current-controlled Switches

Voltage Controlled: Current Controlled:
 
  The .MODEL statement allows you to specify the parameters of a variety of devices used in SPICE, such as switches, diodes, transistors. In case of a switch, we have:
 
  Example:
 
 

k. Operational Amplifiers, and other elements

An operational amplifier can be simulated in different ways. The first method is to model the amplifier by resistors, capacitors and dependent sources. As an example an ideal opamp is easily simulated using a voltage dependent voltage source. The second option uses actual transistors to model the opamp. The device library contains nonlinear models of the most common op amps. The student version of PSpice has macromodels for the linear amplifiers LM324 and uA741 which are included in the EVAL.LIB file. The professional version comes with library files of many commercial amplifiers and devices.

An example of the first approach (linear AC model) is given below for the uA741 opamp. We defined a subcircuit for the opamp.

l. Subcircuits

A subcircuit allows you to define a collection of elements as a subcircuit (e.g. an operational amplifier) and to insert this description into the overall circui (as you would do for any other element).

Defining a subcircuit

 A subcircuit is defined bu a .SUBCKT control statement, followed by the circuit description as follows:
 
 

in which SUBNAME is the subcircuit name and N1, N2, N3 are the external nodes of the subcircuit. The external nodes cannot be 0. The node numbers used inside the subcircuit are stricktly local, except for node 0 which is always global. For an example, see Operational Amplifier above.

Using a subcircuit

 The element statement for a subcircuit is similar to any other element. The format is as follows:

in which Xname refers to the element (subcircuit) being used; N1, N2, N3 are the nodes to which the external nodes of the subcircuit are being connected, and SUBNAME is the name of the subcircuit being used.

 An example of an inverting opamp circuit using the subcircuit of the the uA741 (see operational amplifiers above) is given below. The subcircuit is called x1.
 
 

m. Semiconductor Devices

Most of the elements that have been described above require only a few parameters to specify its electrical characteristics. However, the models for semiconductor devices require many parameter values. A set of device model parameters is defined in a separate .MODEL statement and assigned a unique name. This method alliaviates the need to specify all of the model parameters on each device element card. Thus a semiconductor device is specified by two command lines: an element and model statement.

The syntax for the model statement is:
 
 

MODName is the name of the model for the device. The Type refers to the type of device and can be any of the following:
 
  The parameter values specify the device characteristics as explained below.

m1. Diode

Element line: Dname N+ N- MODName
 
 

Model statement:

The element name starts with D to indicate that the element is a diode, N+ and N- are the two node numbers and MODName is the name of the model of the diode which is specified in the model line. The values one can specify include: the saturation current, IS (default=1E-14A), the emission coefficient, N (=1), the series resistance, RS (=0 ohm), junction capacitance, CJO (=0F), transit time, TT (=0sec), reverse bias breakdown voltage, BV (=infinite) and the reverse bias breakdown current, IBV (=1xE-10A). If a parameter is not specified the default value (given in parenthesis) is assumed.

 As an example, the model parameters for a 1N4148 commercial diode are as follows:
 
 

m2. Bipolar transistors

Element: Qname C B E BJT_modelName
 
 

Model statement:

in which BF is the common emitter current gain ß, IS is the saturation current and VAF is the Early voltage. If no values are specified, the default values are assumed (ß=100; IS=1E-16A, and VAF=[infinite]). Other parameters can be specified including the junction capacitances CJE (0pF) and CJC (0pF), the transit times TT (0sec) and TR (0sec), the base RB (0 Ohm), emitter RE (0 Ohm) and collector resistances RC (0 Ohm). For a complete list of the parameters please refer to one of the references. As an example, the model parameters for the 2N2222A NPN transistor is given below:
 
  Notice that the continuation sign + should be added at the beginning of a new line. A circuit example with a npn transistor can be found under the section Examples
 
 

m3. MOSFETS

Element: Mname ND NG NS &ltNB> ModName L= W=
 
 

The MOS transistor name (Mname) has to start with a M; ND, NG, NS and NB are the node numbers of the Drain, Gate, Source and Bulk terminals, respectively. ModName is the name of the transistor model (see further). L and W is the length and width of the gate (in m).

 The above paramters are usually sufficient when specifying discrete transistors. However, for integrated circuit simulations one need to specify several other parameter values related to the transistor geomtry. These are optional.
 
 

in which Model statement: in which KP=uCox and VTO is the threshold voltage. The default values are KP=20uA/V2; and the rest is equal to 0. There are several other transistor parameters that can be specified, in particular when doing simulations of integrated circuits. The general form of the .MODEL statement is as follows: LEVEL refers to the MOSFET model that describes the terminal I-V characteristics of the transistors. LEVEL 1 is the simplest Mosfet model and is in general sufficient for describing discrete transistors as is done in the EE216 and EE319 courses. However to simulate integrated circuit transistors, one need to use a more sophisticated models. LEVEL 2 includes extensive second-order models, while LEVEL 3 is a semi-empirical model that is better suited for short-channel transistors. Another model that is especially suited to model short-channel effects is called the BSIM model (LEVEL 13 in HSpice).

 For partial listing of the MOSFET MODEL parameters click here. Refer to the references for a complete list of parameters.

An example of the model parameters of the 1.2um CMOS MOSIS transistors can be found in section on Models of Selected Devices and Components later on.

m4. JFETS

Element: Jname ND NG NS ModName

ND, NG, and NS are the node numbers of the Drain, Gate, and Source terminals, respectively. ModName is the name of the transistor model
 
 

Model statement:

for the N-JFET and P-JFET respectively. A partial list of the parameters that can be specified is: VT0 (threshold voltage, -2V default for N_JFET), BETA (transconductance coefficient, 1E-4 A/V2), LAMBDA (channel length modulation, 0 /V), IS (gate p-n saturation current, 1E-14A), CGD and CGS (drain and source zero-bias junction capacitances, 0pf), RD and RS (drain and source ohmic resistances, 0 Ohm).

For an example of the model parameters of the 2N5459 N-JFET see section on Models of Selected Devices and Components later on.

2.2 Commands or Control Statements to Specify the Type of Analysis

a. .OP Statement

This statement instructs Spice to compute the DC operating points:
 
  In PSpice it is usually not necessary to specify .OP as it gives you automatically the DC node voltages. However, HSpice does not give the DC voltages unless you have specified a certain analysis type, such as for instance .TRAN, or .AC analysis (Spice automatically does a DC analysis before doing a transient or AC analysis). Thus, if you are only interested in the DC voltages in HSpice, you should specify the .OP option, or the .DC option (see further).

b. .DC Statement

This statement allows you to increment (sweep) an independent source over a certain range with a specified step. The format is as follows:
 
  in which SRC name is the name of the source you want to vary; START and STOP are the starting and ending value, respectively; and STEP is the size of the increment.
 
  When the Start and Stop values are identical (and the Step is non-zero), the .DC command produces only one value. This may be usefull in HSpice when you do not want all the DC voltages and currents to be printed (with the .OP option), but are interested in a limited number of DC voltages and currents. In the .PRINT statement (see further) you would then also specify the node voltages you like to know (ex. .DC Vs 3 3 1 and .PRINT DC V(2), V(3), I(Vmeas) ).

You can nest the DC sweep command which is often used to plot transistor characteristics, such as the Drain current ids versus the Drain-source voltage Vds for different gate voltages Vgs. This can be done as follows:
 
 

In the example above, the voltage Vds will be swept from 0 to 5V in steps of 1V for every value of Vgs.

c. .TF Statement

The .TF statement instructs PSpice to calculate the following small signal characteristics:
 
 
  1. the ratio of output variable to input variable (gain or tranfer gain)
  2. the resistance with respect to the input source
  3. the resistance with respect to the output terminals
in which OUTVAR is the name of the output variable and INSRC is the input source.
 
  The .TF statement can be used to find the Thevenin small signal equivalent resistance. (The Thevenin voltage is given by the node voltage at the open circuit terminal, as a result of the .OP statement). See also Output Statements later on.
 
 

d. .SENS Statement

This instructs PSpice to calculate the DC small-signal sensitivities of each specified output variable with respect to every circuit parameter.
 
 

e. .TRAN Statement

This statement specifies the time interval over which the transient analysis takes place, and the time increments. The format is as follows:
 
  See also Output Statements later on.

f. .IC Statement

This statement provides an alternative way to specify initial conditions of nodes (and thus over capacitors).
 
 

g. .AC Statement

This statement is used to specify the frequency (AC) analysis. The format is as follows:
 
  in which LIN stands for a linear frequency variation, DEC and OCT for a decade and octave variation respectively. NP stands for the number of points and ND and NO for the number of frequency points per decade and octave. FSTART and FSTOP are the start and stopping frequencies in Herz
 
  See also Output Statements later on. For an example circuit see under the section Examples.
 
 

h. For .NOISE, .DISTO, and .FOUR statements

Please consult the manual.
 
 

2.3 Output Statements

These statements will instruct PSpice what output to generate. If you do not specify an output statement, PSpice will always calculate the DC operating points. The two types of outputs are the prints and plots. A print is a table of data points and a plot is a graphical representation. The format is as follows:
 
  in which TYPE specifies the type of analysis to be printed or plotted and can be:
 
  The output variables are OV1, OV2 and can be voltage or currents in voltage sources. Node voltages and device currents can be specified as magnitude (M), phase (P), real (R) or imaginary (I) parts by adding the suffix to V or I as follows:
 
  Examples:
 
 
This page has been  accessed since Jan. 12, 1996.
Back to Table of Contents 
Jan Van der Spiegel
jan@ee.upenn.edu

Created Sept. 30, 1995; Updated October 15, 1995