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 smallsignal 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 frequency range and the noise and distortion analysis parameters are specified on the .AC, .NOISE, and .DISTO control lines.

The transient analysis portion of SPICE computes the transient output variables as a function of time over a userspecified 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)**XT)*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:
1) The nonlinear branch currents converge to within a tolerance
of 0.1 percent or 1 picoamp (1.0E-12 Amp), whichever is larger.
2) The node voltages converge to within a tolerance of 0.1 per
cent or 1 microvolt (1.0E-6 Volt), whichever is larger.
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 + (plus) in column 1 of the following card; SPICE continues reading beginning with column 2. 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 CELL
This 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:
* <any comment>
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.

General form:
RXXXXXXX N1 N2 VALUE <TC=TC1<,TC2>>
Examples:
R1 1 2 100
RC1 12 17 1K TC=0.001,0.015
N1 and N2 are the two element nodes. VALUE is the resistance (in ohms) and may be positive or negative but not zero. TC1 and TC2 are the (optional) temperature coefficients; if not specified, zero is assumed for both. The value of the resistor as a function of temperature is given by:
value(TEMP) = value(TNOM)*(1+TC1*(TEMP-TNOM)+TC2*(TEMP-TNOM)**2))

General form:
CXXXXXXX N+ N- VALUE <IC=INCOND>
LYYYYYYY N+ N- VALUE <IC=INCOND>
Examples:
CBYP 13 0 1UF
COSC 17 23 10U IC=3V
LLINK 42 69 1UH
LSHUNT 23 51 10U IC=15.7MA
N+ and N- are the positive and negative element nodes, respectively. VALUE is the capacitance in Farads or the inductance in Henries.
For the capacitor, the (optional) initial condition is the initial (time-zero) value of capacitor voltage (in Volts). For the inductor, the (optional) initial condition is the initial (time-zero) value of inductor current (in Amps) that flows from N+, through the inductor, to N-. Note that the initial conditions (if any) apply 'only' if the UIC option is specified on the .TRAN card.
Nonlinear capacitors and inductors can be described.
General form :
CXXXXXXX N+ N- POLY C0 C1 C2 ... <IC=INCOND>
LYYYYYYY N+ N- POLY L0 L1 L2 ... <IC=INCOND>
C0 C1 C2 ...(and L0 L1 L2 ...) are the coefficients of a polynomial describing the element value. The capacitance is expressed as a function of the voltage across the element while the inductance is a function of the current through the inductor. The value is computed as
value=C0+C1*V+C2*V**2+...
value=L0+L1*I+L2*I**2+...
where V is the voltage across the capacitor and I the current flowing in the inductor.

General form:
KXXXXXXX LYYYYYYY LZZZZZZZ VALUE
Examples:
K43 LAA LBB 0.999
KXFRMR L1 L2 0.87
LYYYYYYY and LZZZZZZZ are the names of the two coupled inductors, and VALUE is the coefficient of coupling, K, which must be greater than 0 and less than or equal to 1. Using the 'dot' convention, place a 'dot' on the first node of each inductor.

General form:
TXXXXXXX N1 N2 N3 N4 Z0=VALUE <TD=VALUE> <F=FREQ <NL=NRMLEN>> <IC=V1,I1,V2,I2>
Examples:
T1 1 0 2 0 Z0=50 TD=10NS
N1 and N2 are the nodes at port 1; N3 and N4 are the nodes at port 2. Z0 is the characteristic impedance. The length of the line may be expressed in either of two forms. The transmission delay, TD, may be specified directly (as TD=10ns, for example). Alternatively, a frequency F may be given, together with NL, the normalized electrical length of the transmission line with respect to the wavelength in the line at the frequency F. If a frequency is specified but NL is omitted, 0.25 is assumed (that is, the frequency is assumed to be the quarter-wave frequency). Note that although both forms for expressing the line length are indicated as optional, one of the two must be specified.
Note that this element models only one propagating mode. If all four nodes are distinct in the actual circuit, then two modes may be excited. To simulate such a situation, two transmissionline elements are required. (see the example in Appendix A for further clarification.) The (optional) initial condition specification consists of the voltage and current at each of the transmission line ports. Note that the initial conditions (if any) apply 'only' if the UIC option is specified on the .TRAN card.
One should be aware that SPICE will use a transient timestep which does not exceed 1/2 the minimum transmission line delay. Therefore very short transmission lines (compared with the analysis time frame) will cause long run times.

SPICE allows circuits to contain linear dependent sources characterized by any of the four equations
i=g*v
v=e*v
i=f*i
v=h*i
where g, e, f, and h are constants representing transconductance, voltage gain, current gain, and transresistance, respectively. Note: a more complete description of dependent sources as implemented in SPICE is given in Appendix B.

General form:
GXXXXXXX N+ N- NC+ NC- VALUE
Examples:
G1 2 0 5 0 0.1MMHO
N+ and N- are the positive and negative nodes, respectively. Current flow is from the positive node, through the source, to the negative node. NC+ and NC- are the positive and negative controlling nodes, respectively. VALUE is the transconductance (in mhos).

General form: EXXXXXXX N+ N- NC+ NC- VALUE
Examples: E1 2 3 14 1 2.0
N+ is the positive node, and N- is the negative node. NC+ and NC- are the positive and negative controlling nodes, respectively. VALUE is the voltage gain.

General form:
FXXXXXXX N+ N- VNAM VALUE
Examples:
F1 13 5 VSENS 5
N+ and N- are the positive and negative nodes, respectively. Current flow is from the positive node, through the source, to the negative node. VNAM is the name of a voltage source through which the controlling current flows. The direction of positive controlling current flow is from the positive node, through the source, to the negative node of VNAM. VALUE is the current gain.

General form:
HXXXXXXX N+ N- VNAM VALUE
Examples:
HX 5 17 VZ 0.5K
N+ and N- are the positive and negative nodes, respectively. VNAM is the name of a voltage source through which the controlling current flows. The direction of positive controlling current flow is from the positive node, through the source, to the negative node of VNAM. VALUE is the transresistance (in ohms).

General form:
VXXXXXXX N+ N- <<DC> DC/TRAN VALUE> <AC <ACMAG <ACPHASE>>>
IYYYYYYY N+ N- <<DC> DC/TRAN VALUE> <AC <ACMAG <ACPHASE>>>
Examples: VCC 10 0 DC 6
VIN 13 2 0.001 AC 1 SIN(0 1 1MEG)
ISRC 23 21 AC 0.333 45.0 SFFM(0 1 10K 5 1K)
VMEAS 12 9
N+ and N- are the positive and negative nodes, respectively. Note that voltage sources need not be grounded. Positive current is assumed to flow from the positive node, through the source, to the negative node. A current source of positive value, will force current to flow out of the N+ node, through the source, and into the N- node. Voltage sources, in addition to being used for circuit excitation, are the 'ammeters' for SPICE, that is, zero valued voltage sources may be inserted into the circuit for the purpose of measuring current. They will, of course, have no effect on circuit operation since they represent short-circuits.
DC/TRAN is the dc and transient analysis value of the source. If the source value is zero both for dc and transient analyses, this value may be omitted. If the source value is time-invariant (e.g., a power supply), then the value may optionally be preceded by the letters DC.
ACMAG is the ac magnitude and ACPHASE is the ac phase. The source is set to this value in the ac analysis. If ACMAG is omitted following the keyword AC, a value of unity is assumed. If ACPHASE is omitted, a value of zero is assumed. If the source is not an ac small-signal input, the keyword AC and the ac values are omitted.
Any independent source can be assigned a time-dependent value for transient analysis. If a source is assigned a timedependent value, the time-zero value is used for dc analysis. There are five independent source functions: pulse, exponential, sinusoidal, piece-wise linear, and single-frequency FM. If parameters other than source values are omitted or set to zero, the default values shown will be assumed. (TSTEP is the printing increment and TSTOP is the final time (see the .TRAN card for explanation)).

1. Pulse
PULSE(V1 V2 TD TR TF PW PER)
Examples:
VIN 3 0 PULSE(-1 1 2NS 2NS 2NS 50NS 100NS)

A single pulse so specified is described by the following table:
time value
0 V1
TD V1
TD+TR V2
TD+TR+PW V2
TD+TR+PW+TF V1
TSTOP V1
Intermediate points are determined by linear interpolation

.
2. Sinusoidal
SIN(VO VA FREQ TD THETA)
Examples:
VIN 3 0 SIN(0 1 100MEG 1NS 1E10)
parameters default value units
VO (offset) Volts or Amps
VA (amplitude) Volts or Amps
FREQ (frequency) 1/TSTOP Hz
TD (delay) 0.0 seconds
THETA (damping factor) 0.0 1/seconds
The shape of the waveform is described by the following table:
time value
0 to TD VO
TD to TSTOP VO + VA*exp(-(time-TD)*THETA)*sine(twopi*FREQ*(time+TD))

3. Exponential
EXP(V1 V2 TD1 TAU1 TD2 TAU2)
Examples:
VIN 3 0 EXP(-4 -1 2NS 30NS 60NS 40NS)
parameters default values units
V1 (initial value) Volts or Amps
V2 (pulsed value) Volts or Amps
TD1 (rise delay time) 0.0 seconds
TAU1 (rise time constant) TSTEP seconds
TD2 (fall delay time) TD1+TSTEP seconds
TAU2 (fall time constant) TSTEP seconds
The shape of the waveform is described by the following table:
time value
0 to TD1 V1
TD1 to TD2 V1+(V2-V1)*(1-exp(-(time-TD1)/TAU1))
TD2 to TSTOP V1+(V2-V1)*(1-exp(-(time-TD1)/TAU1))
+(V1-V2)*(1-exp(-(time-TD2)/TAU2))

4. Piece-Wise Linear
PWL(T1 V1 <T2 V2 T3 V3 T4 V4 ...>)
Examples:
VCLOCK 7 5 PWL(0 -7 10NS -7 11NS -3 17NS -3 18NS -7 50NS -7)
Parameters and default values
Each pair of values (Ti, Vi) specifies that the value of the source is Vi (in Volts or Amps) at time=Ti. The value of the source at intermediate values of time is determined by using linear interpolation on the input values.

5. Single-Frequency
FM SFFM(VO VA FC MDI FS)
Examples:
V1 12 0 SFFM(0 1M 20K 5 1K)
parameters default values units
VO (offset) Volts or Amps
VA (amplitude) Volts or Amps
FC (carrier frequency) 1/TSTOP Hz
MDI (modulation index)
FS (signal frequency) 1/TSTOP Hz
The shape of the waveform is described by the following equation:
value = VO + VA*sine((twopi*FC*time) + MDI*sine(twopi*FS*time))

The elements that have been described to this point typically require only a few parameter values to specify completely the electrical characteristics of the element. However, the models for the four semiconductor devices that are included in the SPICE program require many parameter values. Moreover, many devices in a circuit often are defined by the same set of device model parameters. For these reasons, a set of device model parameters is defined on a separate .MODEL card and assigned a unique model name. The device element cards in SPICE then reference the model name. This scheme alleviates the need to specify all of the model parameters on each device element card. Each device element card contains the device name, the nodes to which the device is connected, and the device model name. In addition, other optional parameters may be specified for each device: geometric factors and an initial condition.
The area factor used on the diode, BJT and JFET device card determines the number of equivalent parallel devices of a specified model. The affected parameters are marked with an asterisk under the heading 'area' in the model descriptions below. Several geometric factors associated with the channel and the drain and source diffusions can be specified on the MOSFET device card.
Two different forms of initial conditions may be specified for devices. The first form is included to improve the dc convergence for circuits that contain more than one stable state. If a device is specified OFF, the dc operating point is determined with the terminal voltages for that device set to zero. After convergence is obtained, the program continues to iterate to obtain the exact value for the terminal voltages. If a circuit has more than one dc stable state, the OFF option can be used to force the solution to correspond to a desired state. If a device is specified OFF when in reality the device is conducting, the program will still obtain the correct solution (assuming the solutions converge) but more iterations will be required since the program must independently converge to two separate solutions. The .NODESET card serves a similar purpose as the OFF option. The .NODESET option is easier to apply and is the preferred means to aid convergence. The second form of initial conditions are specified for use with the transient analysis. These are true 'initial conditions' as opposed to the convergence aids above. See the description of the .IC card and the .TRAN card for a detailed explanation of initial conditions.

General form:
DXXXXXXX N+ N- MNAME <AREA> <OFF> <IC=VD>
Examples:
DBRIDGE 2 10 DIODE1
DCLMP 3 7 DMOD 3.0 IC=0.2
N+ and N- are the positive and negative nodes, respectively. MNAME is the model name, AREA is the area factor, and off indicates an (optional) starting condition on the device for dc analysis. If the area factor is omitted, a value of 1.0 is assumed. The (optional) initial condition specification using IC=VD is intended for use with the UIC option on the .TRAN card, when a transient analysis is desired starting from other than the quiescent operating point.

General form:
QXXXXXXX NC NB NE <NS> MNAME <AREA> <OFF> <IC=VBE,VCE>
Examples:
Q23 10 24 13 QMOD IC=0.6,5.0
Q50A 11 26 4 20 MOD1
NC, NB, and NE are the collector, base, and emitter nodes, respectively. NS is the (optional) substrate node. If unspecified, ground is used. MNAME is the model name, AREA is the area factor, and OFF indicates an (optional) initial condition on the device for the dc analysis. If the area factor is omitted, a value of 1.0 is assumed. The (optional) initial condition specification using IC=VBE,VCE is intended for use with the UIC option on the .TRAN card, when a transient analysis is desired starting from other than the quiescent operating point. See the .IC card description for a better way to set transient initial conditions.

General form:
JXXXXXXX ND NG NS MNAME <AREA> <OFF> <IC=VDS,VGS>
Examples:
J1 7 2 3 JM1 OFF
ND, NG, and NS are the drain, gate, and source nodes, respectively. MNAME is the model name, AREA is the area factor, and OFF indicates an (optional) initial condition on the device for dc analysis. If the area factor is omitted, a value of 1.0 is assumed. The (optional) initial condition specification, using IC=VDS,VGS is intended for use with the UIC option on the .TRAN card, when a transient analysis is desired starting from other than the quiescent operating point (see the .IC card for a better way to set initial conditions).

General form:
MXXXXXXX ND NG NS NB MNAME <L=VAL> <W=VAL> <AD=VAL> <AS=VAL>
+ <PD=VAL> <PS=VAL> <NRD=VAL> <NRS=VAL> <OFF> <IC=VDS,VGS,VBS>
Examples:
M1 24 2 0 20 TYPE1
M31 2 17 6 10 MODM L=5U W=2U
M31 2 16 6 10 MODM 5U 2U
M1 2 9 3 0 MOD1 L=10U W=5U AD=100P AS=100P PD=40U PS=40U
M1 2 9 3 0 MOD1 10U 5U 2P 2P
ND, NG, NS, and NB are the drain, gate, source, and bulk (substrate) nodes, respectively. MNAME is the model name. L and W are the channel length and width, in meters. AD and AS are the areas of the drain and source diffusions, in sq-meters. Note that the suffix U specifies microns (1E-6 m) and P sq-microns (1E-12 sq-m). If any of L, W, AD, or AS are not specified, default values are used. The user may specify the values to be used for these default parameters on the .OPTIONS card. The use of defaults simplifies input deck preparation, as well as the editing required if device geometries are to be changed. PD and PS are the perimeters of the drain and source junctions, in meters. NRD and NRS designate the equivalent number of squares of the drain and source diffusions; these values multiply the sheet resistance RSH specified on the .MODEL card for an accurate representation of the parasitic series drain and source resistance of each transistor. PD and PS default to 0.0 while NRD and NRS to 1.0. OFF indicates an (optional) initial condition on the device for dc analysis. The (optional) initial condition specification using IC=VDS,VGS,VBS is intended for use with the UIC option on the .TRAN card, when a transient analysis is desired starting from other than the quiescent operating point. See the .IC card for a better and more convenient way to specify transient initial conditions.

General form:
.MODEL MNAME TYPE(PNAME1=PVAL1 PNAME2=PVAL2 ... )
Examples:
.MODEL MOD1 NPN BF=50 IS=1E-13 VBF=50
The .MODEL card specifies a set of model parameters that will be used by one or more devices. MNAME is the model name, and type is one of the following seven types:
NPN NPN BJT model
PNP PNP BJT model
D diode model
NJF N-channel JFET model
PJF P-channel JFET model
NMOS N-channel MOSFET model
PMOS P-channel MOSFET model
Parameter values are defined by appending the parameter name, as given below for each model type, followed by an equal sign and the parameter value. Model parameters that are not given a value are assigned the default values given below for each model type.

The dc characteristics of the diode are determined by the parameters IS and N. An ohmic resistance, RS, is included. Charge storage effects are modeled by a transit time, TT, and a nonlinear depletion layer capacitance which is determined by the parameters CJO, VJ, and M. The temperature dependence of the saturation current is defined by the parameters EG, the energy and XTI, the saturation current temperature exponent. Reverse breakdown is modeled by an exponential increase in the reverse diode current and is determined by the parameters BV and IBV (both of which are positive numbers).

The bipolar junction transistor model in SPICE is an adaptation of the integral charge control model of Gummel and Poon. This modified Gummel-Poon model extends the original model to include several effects at high bias levels. The model will automatically simplify to the simpler Ebers-Moll model when certain parameters are not specified. The parameter names used in the modified Gummel-Poon model have been chosen to be more easily understood by the program user, and to reflect better both physical and circuit design thinking. The dc model is defined by the parameters IS, BF, NF, ISE, IKF, and NE which determine the forward current gain characteristics, IS, BR, NR, ISC, IKR, and NC which determine the reverse current gain characteristics, and VAF and VAR which determine the output conductance for forward and reverse regions. Three ohmic resistances RB, RC, and RE are included, where RB can be high current dependent. Base charge storage is modeled by forward and reverse transit times, TF and TR, the forward transit time TF being bias dependent if desired, and nonlinear depletion layer capacitances which are determined by CJE, VJE, and MJE for the B-E junction , CJC, VJC, and MJC for the B-C junction and CJS, VJS, and MJS for the C-S (Collector-Substrate) junction. The temperature dependence of the saturation current, IS, is detemined by the energy-gap, EG, and the saturation current temperature exponent, XTI. Additionally base current temperature dependence is modeled by the beta temperature exponent XTB in the new model.
The BJT parameters used in the modified Gummel-Poon model are listed below. The parameter names used in earlier versions of SPICE2 are still accepted.

Modified Gummel-Poon BJT Parameters.

The JFET model is derived from the FET model of Shichman and Hodges. The dc characteristics are defined by the parameters VTO and BETA, which determine the variation of drain current with gate voltage, LAMBDA, which determines the output conductance, and IS, the saturation current of the two gate junctions. Two ohmic resistances, RD and RS, are included. Charge storage is modeled by nonlinear depletion layer capacitances for both gate junctions which vary as the -1/2 power of junction voltage and are defined by the parameters CGS, CGD, and PB.

SPICE provides three MOSFET device models which differ in the formulation of the I-V characteristic. The variable LEVEL specifies the model to be used:
LEVEL=1 -> Shichman-Hodges
LEVEL=2 -> MOS2 (as described in [1])
LEVEL=3 -> MOS3, a semi-empirical model(see [1])
The dc characteristics of the MOSFET are defined by the device parameters VTO, KP, LAMBDA, PHI and GAMMA. These parameters are computed by SPICE if process parameters (NSUB, TOX, ...) are given, but user-specified values always override. VTO is positive (negative) for enhancement mode and negative (positive) for depletion mode N-channel (P-channel) devices. Charge storage is modeled by three constant capacitors, CGSO, CGDO, and CGBO which represent overlap capacitances, by the nonlinear thin-oxide capacitance which is distributed among the gate, source, drain, and bulk regions, and by the nonlinear depletion-layer capacitances for both substrate junctions divided into bottom and periphery, which vary as the MJ and MJSW power of junction voltage respectively, and are determined by the parameters CBD, CBS, CJ, CJSW, MJ, MJSW and PB. There are two built-in models of the charge storage effects associated with the thin-oxide. The default is the piecewise linear voltage-dependent capacitance model proposed by Meyer. The second choice is the charge-controlled capacitance model of Ward and Dutton [1]. The XQC model parameter acts as a flag and a coefficient at the same time. As the former it causes the program to use Meyer's model whenever larger than 0.5 or not specified, and the charge-controlled model when between 0 and 0.5. In the latter case its value defines the share of the channel charge associated with the drain terminal in the saturation region. The thin-oxide charge storage effects are treated slightly different for the LEVEL=1 model. These voltagedependent capacitances are included only if TOX is specified in the input description and they are represented using Meyer's formulation.
There is some overlap among the parameters describing the junctions, e.g. the reverse current can be input either as IS (in A) or as JS (in A/m**2). Whereas the first is an absolute value the second is multiplied by AD and AS to give the reverse current of the drain and source junctions respectively. This methodology has been chosen since there is no sense in relating always junction characteristics with AD and AS entered on the device card; the areas can be defaulted. The same idea applies also to the zero-bias junction capacitances CBD and CBS (in F) on one hand, and CJ (in F/m**2) on the other. The parasitic drain and source series resistance can be expressed as either RD and RS (in ohms) or RSH (in ohms/sq.), the latter being multiplied by the number of squares NRD and NRS input on the device card.

A subcircuit that consists of SPICE elements can be defined and referenced in a fashion similar to device models. The subcircuit is defined in the input deck by a grouping of element cards; the program then automatically inserts the group of elements wherever the subcircuit is referenced. There is no limit on the size or complexity of subcircuits, and subcircuits may contain other subcircuits. An example of subcircuit usage is given in Appendix A.

General form:
.SUBCKT subnam N1 <N2 N3 ...>
Examples:
.SUBCKT OPAMP 1 2 3 4
A circuit definition is begun with a .SUBCKT card. SUBNAM is the subcircuit name, and N1, N2, ... are the external nodes, which cannot be zero. The group of element cards which immediately follow the .SUBCKT card define the subcircuit. The last card in a subcircuit definition is the .ENDS card (see below). Control cards may not appear within a subcircuit definition; however, subcircuit definitions may contain anything else, including other subcircuit definitions, device models, and subcircuit calls (see below). Note that any device models or subcircuit definitions included as part of a subcircuit definition are strictly local (i.e., such models and definitions are not known outside the subcircuit definition). Also, any element nodes not included on the .SUBCKT card are strictly local, with the exception of 0 (ground) which is always global.

General form:
.ENDS <SUBNAM>
Examples:
.ENDS OPAMP
This card must be the last one for any subcircuit definition. The subcircuit name, if included, indicates which subcircuit definition is being terminated; if omitted, all subcircuits being defined are terminated. The name is needed only when nested subcircuit definitions are being made.

General form:
XYYYYYYY N1 <N2 N3 ...> SUBNAM
Examples:
X1 2 4 17 3 1 MULTI
Subcircuits are used in SPICE by specifying pseudo-elements beginning with the letter X, followed by the circuit nodes to be used in expanding the subcircuit.

General form:
.TEMP T1 <T2 <T3 ...>>
Examples:
.TEMP -55.0 25.0 125.0
This card specifies the temperatures at which the circuit is to be simulated. T1, T2, ... Are the different temperatures, in degrees C. Temperatures less than -223.0 deg C are ignored. Model data are specified at TNOM degrees (see the .OPTIONS card for TNOM); if the .TEMP card is omitted, the simulation will also be performed at a temperature equal to TNOM.

General form:
.WIDTH IN=COLNUM OUT=COLNUM
Examples:
.WIDTH IN=72 OUT=133
COLNUM is the last column read from each line of input; the setting takes effect with the next line read. The default value for COLNUM is 80. The out parameter specifies the output print width. Permissible values for the output print width are 80 and

General form:
.OPTIONS OPT1 OPT2 ... (or OPT=OPTVAL ...)
Examples:
.OPTIONS ACCT LIST NODE
This card allows the user to reset program control and user options for specific simulation purposes. Any combination of the following options may be included, in any order. 'x' (below) represents some positive number.

General form:
.OP
The inclusion of this card in an input deck will force SPICE to determine the dc operating point of the circuit with inductors shorted and capacitors opened. Note: 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. SPICE performs a dc operating point analysis if no other analyses are requested.

General form:
.DC SRCNAM VSTART VSTOP VINCR [SRC2 START2 STOP2 INCR2]
Examples:
.DC VIN 0.25 5.0 0.25
.DC VDS 0 10 .5 VGS 0 5 1
.DC VCE 0 10 .25 IB 0 10U 1U
This card defines the dc transfer curve source and sweep limits. SRCNAM is the name of an independent voltage or current source. VSTART, VSTOP, and VINCR are the starting, final, and incrementing values respectively. The first example will cause the value of the voltage source VIN to be swept from 0.25 Volts to 5.0 Volts in increments of 0.25 Volts. A second source (SRC2) may optionally be specified with associated sweep parameters. In this case, the first source will be swept over its range for each value of the second source. This option can be useful for obtaining semiconductor device output characteristics. See the second example data deck in that section of the guide.

General form:
.NODESET V(NODNUM)=VAL V(NODNUM)=VAL ...
Examples:
.NODESET V(12)=4.5 V(4)=2.23
This card helps the program find the dc or initial transient solution by making a preliminary pass with the specified nodes held to the given voltages. The restriction is then released and the iteration continues to the true solution. The .NODESET card may be necessary for convergence on bistable or astable circuits. In general, this card should not be necessary.

General form:
.IC V(NODNUM)=VAL V(NODNUM)=VAL ...
Examples:
.IC V(11)=5 V(4)=-5 V(2)=2.2
This card is for setting transient initial conditions. It has two different interpretations, depending on whether the UIC parameter is specified on the .TRAN card. Also, one should not confuse this card with the .NODESET card. The .NODESET card is only to help dc convergence, and does not affect final bias solution (except for multi-stable circuits). The two interpretations of this card are as follows:
1. When the UIC parameter is specified on the .TRAN card, then the node voltages specified on the .IC card are used to compute the capacitor, diode, BJT, JFET, and MOSFET initial conditions. This is equivalent to specifying the IC=... parameter on each device card, but is much more convenient. The IC=... parameter can still be specified and will take precedence over the .IC values. Since no dc bias (initial transient) solution is computed before the transient analysis, one should take care to specify all dc source voltages on the .IC card if they are to be used to compute device initial conditions.
2. When the UIC parameter is not specified on the .TRAN card, the dc bias (initial transient) solution will be computed before the transient analysis. In this case, the node voltages specified on the .IC card will be forced to the desired initial values during the bias solution. During transient analysis, the constraint on these node voltages is removed.

General form:
.TF OUTVAR INSRC
Examples:
.TF V(5,3) VIN
.TF I(VLOAD) VIN
This card defines the small-signal output and input for the dc small- signal analysis. OUTVAR is the small-signal output variable and INSRC is the small-signal input source. If this card is included, SPICE will compute the dc small-signal value of the transfer function (output/input), input resistance, and output resistance. For the first example, SPICE would compute the ratio of V(5,3) to VIN, the small-signal input resistance at VIN, and the small-signal output resistance measured across nodes 5 and 3.

General form:
.SENS OV1 <OV2 ... >
Examples:
.SENS V(9) V(4,3) V(17) I(VCC)
If a .SENS card is included in the input deck, SPICE will determine the dc small-signal sensitivities of each specified output variable with respect to every circuit parameter. Note: for large circuits, large amounts of output can be generated.

General form:
.AC DEC ND FSTART FSTOP
.AC OCT NO FSTART FSTOP
.AC LIN NP FSTART FSTOP
Examples:
.AC DEC 10 1 10K
.AC DEC 10 1K 100MEG
.AC LIN 100 1 100HZ
DEC stands for decade variation, and ND is the number of points per decade. OCT stands for octave variation, and NO is the number of points per octave. LIN stands for linear variation, and NP is the number of points. FSTART is the starting frequency, and FSTOP is the final frequency. If this card is included in the deck, SPICE will perform an ac analysis of the circuit over the specified frequency range. Note that in order for this analysis to be meaningful, at least one independent source must have been specified with an ac value.

General form:
.DISTO RLOAD <INTER <SKW2 <REFPWR <SPW2>>>>
Examples:
.DISTO RL 2 0.95 1.0E-3 0.75
This card controls whether SPICE will compute the distortion characteristic of the circuit in a small-signal mode as a part of the ac small-signal sinusoidal steady-state analysis. The analysis is performed assuming that one or two signal frequencies are imposed at the input; let the two frequencies be f1 (the nominal analysis frequency) and f2 (=SKW2*f1). The program then computes the following distortion measures:
HD2 - the magnitude of the frequency component 2*f1 assuming
that f2 is not present.
HD3 - the magnitude of the frequency component 3*f1 assuming
that f2 is not present.
SIM2 - the magnitude of the frequency component f1 + f2.
DIM2 - the magnitude of the frequency component f1 - f2.
DIM3 - the magnitude of the frequency component 2*f1 - f2.
RLOAD is the name of the output load resistor into which all distortion power products are to be computed. INTER is the interval at which the summary printout of the contributions of all nonlinear devices to the total distortion is to be printed. If omitted or set to zero, no summary printout will be made. REFPWR is the reference power level used in computing the distortion products; if omitted, a value of 1 mW (that is, dbm) is used. SKW2 is the ratio of f2 to f1. If omitted, a value of 0.9 is used (i.e., f2 = 0.9*f1). SPW2 is the amplitude of f2. If omitted, a value of 1.0 is assumed. The distortion measures HD2, HD3, SIM2, DIM2, and DIM3 may also be be printed and/or plotted (see the description of the .PRINT and .PLOT cards).

General form:
.NOISE OUTV INSRC NUMS
Examples:
.NOISE V(5) VIN 10
This card controls the noise analysis of the circuit. The noise analysis is performed in conjunction with the ac analysis
(see .AC card). OUTV is an output voltage which defines the summing point. INSRC is the name of the independent voltage or current source which is the noise input reference. NUMS is the summary interval. SPICE will compute the equivalent output noise at the specified output as well as the equivalent input noise at the specified input. In addition, the contributions of every noise generator in the circuit will be printed at every NUMS frequency points (the summary interval). If NUMS is zero, no summary printout will be made.
The output noise and the equivalent input noise may also be printed and/or plotted (see the description of the .PRINT and .PLOT cards).

General form:
.TRAN TSTEP TSTOP <TSTART <TMAX>> <UIC>
Examples:
.TRAN 1NS 100NS
.TRAN 1NS 1000NS 500NS
.TRAN 10NS 1US UIC
TSTEP is the printing or plotting increment for line-printer output. For use with the post-processor, TSTEP is the suggested computing increment. TSTOP is the final time, and TSTART is the initial time. If TSTART is omitted, it is assumed to be zero. The transient analysis always begins at time zero. In the interval <zero, TSTART>, the circuit is analyzed (to reach a steady state), but no outputs are stored. In the interval <TSTART, TSTOP>, the circuit is analyzed and outputs are stored. TMAX is the maximum stepsize that SPICE will use (for default, the program chooses either TSTEP or (TSTOP-TSTART)/50.0, whichever is smaller. TMAX is useful when one wishes to guarantee a computing interval which is smaller than the printer increment, TSTEP.
UIC (use initial conditions) is an optional keyword which indicates that the user does not want SPICE to solve for the quiescent operating point before beginning the transient analysis. If this keyword is specified, SPICE uses the values specified using IC=... on the various elements as the initial transient condition and proceeds with the analysis. If the .IC card has been specified, then the node voltages on the .IC card are used to compute the intitial conditions for the devices. Look at the description on the .IC card for its interpretation when UIC is not specified.

General form:
.FOUR FREQ OV1 <OV2 OV3 ...>
Examples:
.FOUR 100K V(5)
This card controls whether SPICE performs a Fourier analysis as a part of the transient analysis. FREQ is the fundamental frequency, and OV1, ..., are the output variables for which the analysis is desired. The Fourier analysis is performed over the interval <TSTOP-period, TSTOP>, where TSTOP is the final time specified for the transient analysis, and period is one period of the fundamental frequency. The dc component and the first nine components are determined. For maximum accuracy, TMAX (see the .TRAN card) should be set to period/100.0 (or less for very high-Q circuits).

General form:
 .PRINT PRTYPE OV1 <OV2 ... OV8>
Examples: .
PRINT TRAN V(4) I(VIN)
.PRINT AC VM(4,2) VR(7) VP(8,3)
.PRINT DC V(2) I(VSRC) V(23,17)
.PRINT NOISE INOISE
.PRINT DISTO HD3 SIM2(DB)
This card defines the contents of a tabular listing of one to eight output variables. PRTYPE is the type of the analysis (DC, AC, TRAN, NOISE, or DISTO) for which the specified outputs are desired. The form for voltage or current output variables is as follows: V(N1<,N2>)specifies the voltage difference between nodes N1 and N2. If N2 (and the preceding comma) is omitted, ground (0) is assumed. For the ac analysis, five additional outputs can be accessed by replacing the letter V by:
VR - real part
VI - imaginary part
VM - magnitude
VP - phase
VDB - 20*log10(magnitude)
I(VXXXXXXX) specifies the current flowing in the independent voltage source named VXXXXXXX. Positive current flows from the positive node, through the source, to the negative node. For the ac analysis, the corresponding replacements for the letter I may be made in the same way as described for voltage outputs.
Output variables for the noise and distortion analyses have a different general form from that of the other analyses, i.e.
OV<(X)> where OV is any of ONOISE (output noise), INOISE (equivalent input noise), D2, HD3, SIM2, DIM2, or DIM3 (see description of distortion analysis), and X may be any of:
R - real part
I - imaginary part
M - magnitude (default if nothing specified)
P - phase
DB - 20log10(magnitude)
thus, SIM2 (or SIM2(M)) describes the magnitude of the SIM2 distortion measure, while HD2(R) describes the real part of the HD2 distortion measure. There is no limit on the number of .PRINT cards for each type of analysis.

General form:
.PLOT PLTYPE OV1 <(PLO1,PHI1)> <OV2 <(PLO2,PHI2)> ... OV8>
Examples: .
.PLOT DC V(4) V(5) V(1)
.PLOT TRAN V(17,5) (2,5) I(VIN) V(17) (1,9)
.PLOT AC VM(5) VM(31,24) VDB(5) VP(5)
.PLOT DISTO HD2 HD3(R) SIM2
.PLOT TRAN V(5,3) V(4) (0,5) V(7) (0,10)
This card defines the contents of one plot of from one to eight output variables. PLTYPE is the type of analysis (DC, AC, TRAN, NOISE, or DISTO) for which the specified outputs are desired. The syntax for the OVI is identical to that for the .PRINT card, described above.
The optional plot limits (PLO,PHI) may be specified after any of the output variables. All output variables to the left of a pair of plot limits (PLO,PHI) will be plotted using the same lower and upper plot bounds. If plot limits are not specified, SPICE will automatically determine the minimum and maximum values of all output variables being plotted and scale the plot to fit. More than one scale will be used if the output variable values warrant (i.e., mixing output variables with values which are orders-of-magnitude different still gives readable plots).
The overlap of two or more traces on any plot is indicated by the letter X.
When more than one output variable appears on the same plot, the first variable specified will be printed as well as plotted. If a printout of all variables is desired, then a companion .PRINT card should be included.
There is no limit on the number of .PLOT cards specified for each type of analysis.

The following deck determines the dc operating point and small-signal transfer function of a simple differential pair. In addition, the ac small-signal response is computed over the fre- quency range 1Hz to 100MegHz.
SIMPLE DIFFERENTIAL PAIR
VCC 7 0 12
VEE 8 0 -12
VIN 1 0 AC 1
RS1 1 2 1K
RS2 6 0 1K
Q1 3 2 4 MOD1
Q2 5 6 4 MOD1
RC1 7 3 10K
RC2 7 5 10K
RE 4 8 10K
.MODEL MOD1 NPN BF=50 VAF=50 IS=1.E-12 RB=100 CJC=.5PF TF=.6NS
.TF V(5) VIN
.AC DEC 10 1 100MEG
.PLOT AC VM(5) VP(5)
.PRINT AC VM(5) VP(5)
.END

The following deck computes the output characteristics of a MOS- FET device over the range 0-10V for VDS and 0-5V for VGS.
MOS OUTPUT CHARACTERISTICS
.OPTIONS NODE NOPAGE
VDS 3 0
VGS 2 0
M1 1 2 0 0 MOD1 L=4U W=6U AD=10P AS=10P
.MODEL MOD1 NMOS VTO=-2 NSUB=1.0E15 UO=550
* VIDS MEASURES ID, WE COULD HAVE USED VDS, BUT ID WOULD BE NEGATIVE
VIDS 3 1
.DC VDS 0 10 .5 VGS 0 5 1
.PRINT DC I(VIDS) V(2)
.PLOT DC I(VIDS)
.END

The following deck determines the dc transfer curve and the transient pulse response of a simple RTL inverter. The input is a pulse from 0 to 5 Volts with delay, rise, and fall times of 2ns and a pulse width of 30ns. The transient interval is 0 to 100ns, with printing to be done every nanosecond.
SIMPLE RTL INVERTER
VCC 4 0 5
VIN 1 0 PULSE 0 5 2NS 2NS 2NS 30NS
RB 1 2 10K
Q1 3 2 0 Q1
RC 3 4 1K
.PLOT DC V(3)
.PLOT TRAN V(3) (0,5)
.PRINT TRAN V(3)
.MODEL Q1 NPN BF 20 RB 100 TF .1NS CJC 2PF
.DC VIN 0 5 0.1
.TRAN 1NS 100NS
.END

The following deck simulates a four-bit binary adder, using several subcircuits to describe various pieces of the overall circuit.
ADDER - 4 BIT ALL-NAND-GATE BINARY ADDER
*** SUBCIRCUIT DEFINITIONS
.SUBCKT NAND 1 2 3 4
* NODES: INPUT(2), OUTPUT, VCC
Q1 9 5 1 QMOD
D1CLAMP 0 1 DMOD
Q2 9 5 2 QMOD
D2CLAMP 0 2 DMOD
RB 4 5 4K
R1 4 6 1.6K
Q3 6 9 8 QMOD
R2 8 0 1K
RC 4 7 130
Q4 7 6 10 QMOD
DVBEDROP 10 3 DMOD
Q5 3 8 0 QMOD
.ENDS NAND
.SUBCKT ONEBIT 1 2 3 4 5 6
* NODES: INPUT(2), CARRY-IN, OUTPUT, CARRY-OUT, VCC
X1 1 2 7 6 NAND
X2 1 7 8 6 NAND
X3 2 7 9 6 NAND
X4 8 9 10 6 NAND
X5 3 10 11 6 NAND
X6 3 11 12 6 NAND
X7 10 11 13 6 NAND
X8 12 13 4 6 NAND
X9 11 7 5 6 NAND
.ENDS ONEBIT
.SUBCKT TWOBIT 1 2 3 4 5 6 7 8 9
* NODES: INPUT - BIT0(2) / BIT1(2), OUTPUT - BIT0 / BIT1,
* CARRY-IN, CARRY-OUT, VCC
X1 1 2 7 5 10 9 ONEBIT
X2 3 4 10 6 8 9 ONEBIT
.ENDS TWOBIT
.SUBCKT FOURBIT 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15
* NODES: INPUT - BIT0(2) / BIT1(2) / BIT2(2) / BIT3(2),
* OUTPUT - BIT0 / BIT1 / BIT2 / BIT3, CARRY-IN, CARRY-OUT, VCC
X1 1 2 3 4 9 10 13 16 15 TWOBIT
X2 5 6 7 8 11 12 16 14 15 TWOBIT
.ENDS FOURBIT
*** DEFINE NOMINAL CIRCUIT
.MODEL DMOD D
.MODEL QMOD NPN(BF=75 RB=100 CJE=1PF CJC=3PF)
VCC 99 0 DC 5V
VIN1A 1 0 PULSE(0 3 0 10NS 10NS 10NS 50NS)
VIN1B 2 0 PULSE(0 3 0 10NS 10NS 20NS 100NS)
VIN2A 3 0 PULSE(0 3 10NS 10NS 40NS 200NS)
VIN2B 4 0 PULSE(0 3 0 10NS 10NS 80NS 400NS)
VIN3A 5 0 PULSE(0 3 0 10NS 10NS 160NS 800NS)
VIN3B 6 0 PULSE(0 3 0 10NS 10NS 320NS 1600NS)
VIN4A 7 0 PULSE(0 3 0 10NS 10NS 640NS 3200NS)
VIN4B 8 0 PULSE(0 3 0 10NS 10NS 1280NS 6400NS)
X1 1 2 3 4 5 6 7 8 9 10 11 12 0 13 99
RBIT0 9 0 1K
RBIT1 10 0 1K
RBIT2 11 0 1K
RBIT3 12 0 1K
RCOUT 13 0 1K
.PLOT TRAN V(1) V(2) V(3) V(4) V(5) V(6) V(7) V(8)
.PLOT TRAN V(9) V(10) V(11) V(12) V(13)
.PRINT TRAN V(1) V(2) V(3) V(4) V(5) V(6) V(7) V(8)
.PRINT TRAN V(9) V(10) V(11) V(12) V(13)
*** (FOR THOSE WITH MONEY (AND MEMORY) TO BURN)
.TRAN 1NS 6400NS
.OPTIONS ACCT LIST NODE LIMPTS=6401
.END

The following deck simulates a transmission-line inverter. Two transmission-line elements are required since two propagation modes are excited. In the case of a coaxial line, the first line (T1) models the inner conductor with respect to the shield, and the second line (T2) models the shield with respect to the out- side world.
TRANSMISSION-LINE INVERTER
V1 1 0 PULSE(0 1 0 0.1N)
R1 1 2 50
X1 2 0 0 4 TLINE
R2 4 0 50
.SUBCKT TLINE 1 2 3 4
T1 1 2 3 4 Z0=50 TD=1.5NS
T2 2 0 4 0 Z0=100 TD=1NS
.ENDS TLINE
.TRAN 0.1NS 20NS
.PLOT TRAN V(2) V(4)
.END

SPICE allows circuits to contain dependent sources charac terized by any of the four equations
i=f(v)
v=f(v)
i=f(i)
v=f(i)
where the functions must be polynomials, and the arguments may be multidimensional. The polynomial functions are specified by a set of coefficients p0, p1, ..., pn. Both the number of dimen sions and the number of coefficients are arbitrary. The meaning of the coefficients depends upon the dimension of the polynomial, as shown in the following examples:
Suppose that the function is one-dimensional (that is, a function of one argument). Then the function value fv is deter mined by the following expression in fa (the function argument):
fv = p0 + (p1*fa) + (p2*fa2) + (p3*fa3) + (p4*fa4) + (p5*fa5) + ...
Suppose now that the function is two-dimensional, with argu ments fa and fb. Then the function value fv is determined by the following expression:
fv = p0 + (p1*fa) + (p2*fb) + (p3*fa**2) + (p4*fa*fb) + (p5*fb**2) + (p6*fa**3) + (p7*fa**2*fb) + (p8*fa*fb**2) + (p9*fb**3) + ...
Consider now the case of a three-dimensional polynomial function with arguments fa, fb, and fc. Then the function value fv is determined by the following expression:
fv = p0 + (p1*fa) + (p2*fb) + (p3*fc) + (p4*fa**2) + (p5*fa*fb)
+ (p6*fa*fc) + (p7*fb**2) + (p8*fb*fc) + (p9*fc**2) + (p10*fa**3)
+ (p11*fa**2*fb) + (p12*fa**2*fc) + (p13*fa*fb**2) + (p14*fa*fb*fc)
+ (p15*fa*fc**2) + (p16*fb**3) + (p17*fb**2*fc) + (p18*fb*fc**2)
+ (p19*fc**3) + (p20*fa**4) + ...
Note: if the polynomial is one-dimensional and exactly one coefficient is specified, then SPICE assumes io be p1 (and p0 = 0.0), in order to facilitate the input of linear controlled sources.
For all four of the dependent sources described below, the initial condition parameter is described as optional. If not specified, SPICE assumes 0 the initial condition for dependent sources is an initial 'guess' for the value of the controlling variable. The program uses this initial condition to obtain the dc operating point of the circuit. After convergence has been obtained, the program continues iterating to obtain the exact value for the controlling variable. Hence, to reduce the compu tational effort for the dc operating point (or if the polynomial specifies a strong nonlinearity), a value fairly close to the actual controlling variable should be specified for the initial condition.

General form
GXXXXXXX N+ N- <POLY(ND)> NC1+ NC1- ... P0 <P1 ...> <IC=...>
Examples
G1 1 0 5 3 0 0.1M
GR 17 3 17 3 0 1M 1.5M IC=2V
GMLT 23 17 POLY(2) 3 5 1 2 0 1M 17M 3.5U IC=2.5, 1.3
N+ and N- are the positive and negative nodes, respectively. Current flow is from the positive node, through the source, to the negative node. POLY(ND) only has to be specified if the source is multi-dimensional (one-dimensional is the default). If specified, ND is the number of dimensions, which must be posi tive. NC1+, NC1-, ... Are the positive and negative controlling nodes, respectively. One pair of nodes must be specified for each dimension. P0, P1, P2, ..., Pn are the polynomial coefficients. The (optional) initial condition is the initial guess at the value(s) of the controlling voltage(s). If not specified, 0.0 is assumed. The polynomial specifies the source current as a function of the controlling voltage(s). The second example above describes a current source with value I = 1E-3*V(17,3) + 1.5E-3*V(17,3)**2 note that since the source nodes are the same as the controlling nodes, this source actually models a nonlinear resistor.

General form
EXXXXXXX N+ N- <POLY(ND)> NC1+ NC1- ... P0 <P1 ...> <IC=...>
Examples
E1 3 4 21 17 10.5 2.1 1.75
EX 17 0 POLY(3) 13 0 15 0 17 0 0 1 1 1 IC=1.5,2.0,17.35
N+ and N- are the positive and negative nodes, respectively. POLY(ND) only has to be specified if the source is multi dimensional (one-dimensional is the default). If specified, ND is the number of dimensions, which must be positive. NC1+, NC1-, ... are the positive and negative controlling nodes, respec tively. One pair of nodes must be specified for each dimension. P0, P1, P2, ..., Pn are the polynomial coefficients. The (optional) initial condition is the initial guess at the value(s) of the controlling voltage(s). If not specified, 0.0 is assumed. The polynomial specifies the source voltage as a function of the controlling voltage(s). The second example above describes a voltage source with value
V = V(13,0) + V(15,0) + V(17,0)
(in other words, an ideal voltage summer).

General form
FXXXXXXX N+ N- <POLY(ND)> VN1 <VN2 ...> P0 <P1 ...> <IC=...>
Examples
F1 12 10 VCC 1MA 1.3M
FXFER 13 20 VSENS 0 1
N+ and N- are the positive and negative nodes, respectively. Current flow is from the positive node, through the source, to the negative node. POLY(ND) only has to be specified if the source is multi-dimensional (one-dimensional is the default). If specified, ND is the number of dimensions, which must be posi tive. VN1, VN2, ... are the names of voltage sources through which the controlling current flows; one name must be specified for each dimension. The direction of positive controlling current flow is from the positive node, through the source, to the negative node of each voltage source. P0, P1, P2, ..., Pn are the polynomial coefficients. The (optional) initial condi tion is the initial guess at the value(s) of the controlling current(s) (in Amps). If not specified, 0.0 is assumed. The polynomial specifies the source current as a function of the con trolling current(s). The first example above describes a current source with value
I = 1E-3 + 1.3E-3*I(VCC)

General form
HXXXXXXX N+ N- <POLY(ND)> VN1 <VN2 ...> P0 <P1 ...> <IC=...>
Examples
HXY 13 20 POLY(2) VIN1 VIN2 0 0 0 0 1 IC=0.5 1.3
HR 4 17 VX 0 0 1
N+ and N- are the positive and negative nodes, respectively. POLY(ND) only has to be specified if the source is multi dimensional (one-dimensional is the default). If specified, ND is the number of dimensions, which must be positive. VN1, VN2, ... are the names of voltage sources through which the control ling current flows; one name must be specified for each dimen sion. The direction of positive controlling current flow is from the positive node, through the source, to the negative node of each voltage source. P0, P1, P2, ..., Pn are the polynomial coefficients. The (optional) initial condition is the initial guess at the value(s) of the controlling current(s) (in Amps). If not specified, 0.0 is assumed. The polynomial specifies the source voltage as a function of the controlling current(s). The first example above describes a voltage source with value
V = I(VIN1)*I(VIN2)