A.Vladimirescu, K.Zhang, A.R.Newton, D.O.Pederson Department of Electrical Engineering and Computer Sciences University of CaliforniaBerkeley, Ca., 94720 Acknowledgement: Dr. Richard Dowell and Dr. Sally Liu have contributed to develop the present SPICE version. SPICE was originally developed by Dr. Lawrence Nagel and has been modified extensively by Dr. Ellis Cohen.
SPICE is a general-purpose circuit simulation program for nonlinear dc, nonlinear transient, and linear ac analyses. Circuits may contain resistors, capacitors, inductors, mutual inductors, independent voltage and current sources, four types of dependent sources, transmission lines, and the four most common semiconductor devices: diodes, BJT's, JFET's, and MOSFET's.
SPICE has built-in models for the semiconductor devices, and the user need specify only the pertinent model parameter values. The model for the BJT is based on the integral charge model of Gummel and Poon; however, if the Gummel-Poon parameters are not specified, the model reduces to the simpler Ebers-Moll model. In either case, charge storage effects, ohmic resistances, and a current-dependent output conductance may be included. The diode model can be used for either junction diodes or Schottky barrier diodes. The JFET model is based on the FET model of Shichman and Hodges. Three MOSFET models are implemented; MOS1 is described by a square-law I-V characteristic MOS2 is an analytical model while MOS3 is a semi-empirical model. Both MOS2 and MOS3 include second-order effects such as channel length modulation, subthreshold conduction, scattering limited velocity saturation, smallsize effects and charge-controlled capacitances.
The dc analysis portion of SPICE determines the dc operating point of the circuit with inductors shorted and capacitors opened. A dc analysis is automatically performed prior to a transient analysis to determine the transient initial conditions, and prior to an ac small-signal analysis to determine the linearized, small-signal models for nonlinear devices. If requested, the dc small-signal value of a transfer function (ratio of output variable to input source), input resistance, and output resistance will also be computed as a part of the dc solution. The dc analysis can also be used to generate dc transfer curves: a specified independent voltage or current source is stepped over a user-specified range and the dc output variables are stored for each sequential source value. If requested, SPICE also will determine the dc small-signal sensitivities of specified output variables with respect to circuit parameters. The dc analysis options are specified on the .DC, .TF, .OP, and .SENS control cards. If one desires to see the small-signal models for nonlinear devices in conjunction with a transient analysis operating point, then the .OP card must be provided. The dc bias conditions will be identical for each case, but the more comprehensive operating point information is not available to be printed when transient initial conditions are computed.
The ac small-signal portion of SPICE computes the ac output variables as a function of frequency. The program first computes the dc operating point of the circuit and determines linearized, small-signal models for all of the nonlinear devices in the circuit. The resultant linear circuit is then analyzed over a user-specified range of frequencies. The desired output of an ac small- signal analysis is usually a transfer function (voltage gain, transimpedance, etc). If the circuit has only one ac input, it is convenient to set that input to unity and zero phase, so that output variables have the same value as the transfer function of the output variable with respect to the input. The generation of white noise by resistors and semiconductor devices can also be simulated with the ac small-signal portion of SPICE. Equivalent noise source values are determined automatically from the small-signal operating point of the circuit, and the contribution of each noise source is added at a given summing point. The total output noise level and the equivalent input noise level are determined at each frequency point. The output and input noise levels are normalized with respect to the square root of the noise bandwidth and have the units Volts/rt Hz or Amps/rt Hz. The output noise and equivalent input noise can be printed or plotted in the same fashion as other output variables. No additional input data are necessary for this analysis.
Flicker noise sources can be simulated in the noise analysis by including values for the parameters KF and AF on the appropriate device model cards.
The distortion characteristics of a circuit in the small signal mode can be simulated as a part of the ac small-signal analysis. The analysis is performed assuming that one or two signal frequencies are imposed at the input.
The transient analysis portion of SPICE computes the transient output variables as a function of time over a user specified time interval. The initial conditions are automatically determined by a dc analysis. All sources which are not time dependent (for example, power supplies) are set to their dc value. For large-signal sinusoidal simulations, a Fourier analysis of the output waveform can be specified to obtain the frequency domain Fourier coefficients. The transient time interval and the Fourier analysis options are specified on the .TRAN and .FOURIER control lines.
All input data for SPICE is assumed to have been measured at 27 deg C (300 deg K). The simulation also assumes a nominal temperature of 27 deg C. The circuit can be simulated at other temperatures by using a .TEMP control line. Temperature appears explicitly in the exponential terms of the BJT and diode model equations. In addition, saturation currents have a built-in temperature dependence. The temperature dependence of the saturation current in the BJT models is determined by:
IS(T1) = IS(T0)*((T1/T0)**XTI)*exp(q*EG*(T1-T0)/(k*T1*T0))
where k is Boltzmann's constant, q is the electronic charge, EG is the energy gap which is a model parameter, and XTI is the saturation current temperature exponent (also a model parameter, and usually equal to 3). The temperature dependence of forward and reverse beta is according to the formula:
beta(T1)=beta(T0)*(T1/T0)**XTB
where T1 and T0 are in degrees Kelvin, and XTB is a user-supplied model parameter. Temperature effects on beta are carried out by appropriate adjustment to the values of BF, ISE, BR, and ISC. Temperature dependence of the saturation current in the junction diode model is determined by:
IS(T1) = IS(T0)*((T1/T0)**(XTI/N))*exp(q*EG*(T1-T0)/(k*N*T1*T0))
where N is the emission coefficient, which is a model parameter, and the other symbols have the same meaning as above. Note that for Schottky barrier diodes, the value of the saturation current temperature exponent, XTI, is usually 2. Temperature appears explicitly in the value of junction potential, PHI, for all the device models. The temperature dependence is determined by:
PHI(TEMP) = k*TEMP/q*log(Na*Nd/Ni(TEMP)**2)
where k is Boltzmann's constant, q is the electronic charge, Na is the acceptor impurity density, Nd is the donor impurity density, Ni is the intrinsic concentration, and EG is the energy gap. Temperature appears explicitly in the value of surface mobility, UO, for the MOSFET model. The temperature dependence is determined by:
UO(TEMP) = UO(TNOM)/(TEMP/TNOM)**(1.5)
The effects of temperature on resistors is modeled by the formula:
value(TEMP) = value(TNOM)*(1+TC1*(TEMP-TNOM)+TC2*(TEMP-TNOM)**2))
where TEMP is the circuit temperature, TNOM is the nominal temperature, and TC1 and TC2 are the first- and second-order temperature coefficients.
Both dc and transient solutions are obtained by an iterative process which is terminated when both of the following conditions hold:
Although the algorithm used in SPICE has been found to be very reliable, in some cases it will fail to converge to a solution. When this failure occurs, the program will print the node voltages at the last iteration and terminate the job. In such cases, the node voltages that are printed are not necessarily correct or even close to the correct solution. Failure to converge in the dc analysis is usually due to an error in specifying circuit connections, element values, or model parameter values. Regenerative switching circuits or circuits with positive feedback probably will not converge in the dc analysis unless the OFF option is used for some of the devices in the feedback path, or the .NODESET card is used to force the circuit to converge to the desired state.
The input format for SPICE is of the free format type. Fields on a card are separated by one or more blanks, a comma, an equal (=) sign, or a left or right parenthesis; extra spaces are ignored. A card may be continued by entering a ; (semicolon) as the last character of the card; SPICE continues reading the command on the next card.
A name field must begin with a letter (A through Z) and cannot contain any delimiters. Only the first eight characters of the name are used.
A number field may be an integer field (12, -44), a floating point field (3.14159), either an integer or floating point number followed by an integer exponent (1E-14, 2.65E3), or either an integer or a floating point number followed by one of the following scale factors:
T=1E12 G=1E9 MEG=1E6 K=1E3 MIL=25.4E-6 M=1E-3 U=1E-6 N=1E-9 P=1E-12 F=1E-15
Letters immediately following a number that are not scale factors are ignored, and letters immediately following a scale factor are ignored. Hence, 10, 10V, 10VOLTS, and 10HZ all represent the same number, and M, MA, MSEC, and MMHOS all represent the same scale factor. Note that 1000, 1000.0, 1000HZ, 1E3, 1.0E3, 1KHZ, and 1K all represent the same number.
The circuit to be analyzed is described to SPICE by a set of element cards, which define the circuit topology and element values, and a set of control cards, which define the model parameters and the run controls. The first card in the input deck must be a title card, and the last card must be a .END card. The order of the remaining cards is arbitrary (except, of course, that continuation cards must immediately follow the card being continued).
Each element in the circuit is specified by an element card that contains the element name, the circuit nodes to which the element is connected, and the values of the parameters that determine the electrical characteristics of the element. The first letter of the element name specifies the element type. The format for the SPICE element types is given in what follows. The strings XXXXXXX, YYYYYYY, and ZZZZZZZ denote arbitrary alphanumeric strings. For example, a resistor name must begin with the letter R and can contain from one to eight characters. Hence, R, R1, RSE, ROUT, and R3AC2ZY are valid resistor names.
Data fields that are enclosed in lt and gt signs '< >' are optional. All indicated punctuation (parentheses, equal signs, etc.) are required. With respect to branch voltages and currents, SPICE uniformly uses the associated reference convention (current flows in the direction of voltage drop).
Nodes must be nonnegative integers but need not be numbered sequentially. The datum (ground) node must be numbered zero. The circuit cannot contain a loop of voltage sources and/or inductors and cannot contain a cutset of current sources and/or capacitors. Each node in the circuit must have a dc path to ground. Every node must have at least two connections except for transmission line nodes (to permit unterminated transmission lines) and MOSFET substrate nodes (which have two internal connections anyway).
Examples:
POWER AMPLIFIER CIRCUIT TEST OF CAM CELLThis card must be the first card in the input deck. Its contents are printed verbatim as the heading for each section of output.
Examples:
.END
This card must always be the last card in the input deck. Note that the period is an integral part of the name.
General form:
*
Examples:
* RF=1K GAIN SHOULD BE 100
* MAY THE FORCE BE WITH MY CIRCUIT
The asterisk in the first column indicates that this card is a comment card. Comment cards may be placed anywhere in the circuit description.