Interactive User Guide

 

 

1.           INTRODUCTION

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, lossless and lossy transmission lines (two separate implementations), switches, uniform distributed RC lines, and the five most common semiconductor devices: diodes, BJTs, JFETs, MESFETs, and MOSFETs.

The SPICE3 version is based directly on SPICE 2G.6. While SPICE3 is being developed to include new features, it continues to support those capabilities and models which remain in extensive use in the SPICE2 program.

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. Six MOSFET models are implemented: MOS1 is described by a square-law I-V characteristic, MOS2 [1] is an analytical model, while MOS3 [1] is a semi-empirical model; MOS6 [2] is a simple analytic model accurate in the short-channel region; MOS4 [3, 4] and MOS5 [5] are the BSIM (Berkeley Short-channel IGFET Model) and BSIM2. MOS2, MOS3, and MOS4 include second-order effects such as channel-length modulation, subthreshold conduction, scattering-limited velocity saturation, small-size effects, and charge-controlled capacitances.

1.1.  TYPES OF ANALYSIS

1.1.1.            DC Analysis

The dc analysis portion of SPICE determines the dc operating point of the circuit with inductors shorted and capacitors opened. The dc analysis options are specified on the .DC, .TF, and .OP control lines. 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 is also 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.

1.1.2.            AC Small-Signal Analysis

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.

1.1.3.            Transient Analysis

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. The transient time interval is specified on a .TRAN control line.

1.1.4.            Pole-Zero Analysis

The pole-zero analysis portion of SPICE computes the poles and/or zeros in the small-signal ac transfer function. The program first computes the dc operating point and then determines the linearized, small-signal models for all the nonlinear devices in the circuit. This circuit is then used to find the poles and zeros of the transfer function.

Two types of transfer functions are allowed : one of the form (output voltage)/(input voltage) and the other of the form (output voltage)/(input current). These two types of transfer functions cover all the cases and one can find the poles/zeros of functions like input/output impedance and voltage gain. The input and output ports are specified as two pairs of nodes.

The pole-zero analysis works with resistors, capacitors, inductors, linear-controlled sources, independent sources, BJTs, MOSFETs, JFETs and diodes. Transmission lines are not supported.

The method used in the analysis is a sub-optimal numerical search. For large circuits it may take a considerable time or fail to find all poles and zeros. For some circuits, the method becomes "lost" and finds an excessive number of poles or zeros.

1.1.5.            Small-Signal Distortion Analysis

The distortion analysis portion of SPICE computes steady-state harmonic and intermodulation products for small input signal magnitudes. If signals of a single frequency are specified as the input to the circuit, the complex values of the second and third harmonics are determined at every point in the circuit. If there are signals of two frequencies input to the circuit, the analysis finds out the complex values of the circuit variables at the sum and difference of the input frequencies, and at the difference of the smaller frequency from the second harmonic of the larger frequency.

Distortion analysis is supported for the following nonlinear devices: diodes (DIO), BJT, JFET, MOSFETs (levels 1, 2, 3, 4/BSIM1, 5/BSIM2, and 6) and MESFETS. All linear devices are automatically supported by distortion analysis. If there are switches present in the circuit, the analysis continues to be accurate provided the switches do not change state under the small excitations used for distortion calculations.

1.1.6.            Sensitivity Analysis

Spice3 will calculate either the DC operating-point sensitivity or the AC small-signal sensitivity of an output variable with respect to all circuit variables, including model parameters. Spice calculates the difference in an output variable (either a node voltage or a branch current) by perturbing each parameter of each device independently. Since the method is a numerical approximation, the results may demonstrate second order affects in highly sensitive parameters, or may fail to show very low but non-zero sensitivity. Further, since each variable is perturb by a small fraction of its value, zero-valued parameters are not analyized (this has the benefit of reducing what is usually a very large amount of data).

1.1.7.            Noise Analysis

The noise analysis portion of SPICE does analysis device-generated noise for the given circuit. When provided with an input source and an output port, the analysis calculates the noise contributions of each device (and each noise generator within the device) to the output port voltage. It also calculates the input noise to the circuit, equivalent to the output noise referred to the specified input source. This is done for every frequency point in a specified range - the calculated value of the noise corresponds to the spectral density of the circuit variable viewed as a stationary gaussian stochastic process.

After calculating the spectral densities, noise analysis integrates these values over the specified frequency range to arrive at the total noise voltage/current (over this frequency range). This calculated value corresponds to the variance of the circuit variable viewed as a stationary gaussian process.

1.2.  ANALYSIS AT DIFFERENT TEMPERATURES

All input data for SPICE is assumed to have been measured at a nominal temperature of 27 C, which can be changed by use of the TNOM parameter on the .OPTION control line. This value can further be overridden for any device which models temperature effects by specifying the TNOM parameter on the model itself. The circuit simulation is performed at a temperature of 27 C, unless overridden by a TEMP parameter on the .OPTION control line. Individual instances may further override the circuit temperature through the specification of a TEMP parameter on the instance.

Temperature dependent support is provided for resistors, diodes, JFETs, BJTs, and level 1, 2, and 3 MOSFETs. BSIM (levels 4 and 5) MOSFETs have an alternate temperature dependency scheme which adjusts all of the model parameters before input to SPICE. For details of the BSIM temperature adjustment, see [6] and [7].

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:

where k is Boltzmann's constant, q is the electronic charge, E_g 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:

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 _F, I_SE, _R, and I_SC (spice model parameters BF, ISE, BR, and ISC, respectively).

Temperature dependence of the saturation current in the junction diode model is determined by:

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,  (in spice PHI), for all the device models. The temperature dependence is determined by:

where k is Boltzmann's constant, q is the electronic charge, N_a is the acceptor impurity density, N_d is the donor impurity density, N_i is the intrinsic carrier concentration, and E_g is the energy gap.

Temperature appears explicitly in the value of surface mobility, ₀ (or UO), for the MOSFET model. The temperature dependence is determined by:  

The effects of temperature on resistors is modeled by the formula:

where T is the circuit temperature, T₀ is the nominal temperature, and TC₁ and TC₂ are the first- and second-order temperature coefficients.

2.           CIRCUIT DESCRIPTION

GENERAL STRUCTURE AND CONVENTIONS

The circuit to be analyzed is described to SPICE by a set of element lines, which define the circuit topology and element values, and a set of control lines, which define the model parameters and the run controls. The first line in the input file must be the title, and the last line must be ".END". The order of the remaining lines is arbitrary (except, of course, that continuation lines must immediately follow the line being continued).

Each element in the circuit is specified by an element line 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 one or more characters. Hence, R, R1, RSE, ROUT, and R3AC2ZY are valid resistor names. Details of each type of device are supplied in a following section.

Fields on a line are separated by one or more blanks, a comma, an equal ('=') sign, or a left or right parenthesis; extra spaces are ignored. A line may be continued by entering a '+' (plus) in column 1 of the following line; SPICE continues reading beginning with column 2.

A name field must begin with a letter (A through Z) and cannot contain any delimiters.

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 = 10¹² G = 10⁹ Meg = 10⁶ K = 10³ mil = 25.4 10^-6

m = 10^-3 u = 10^-6 n = 10^-9 p = 10^-12 f = 10^-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.

Nodes names may be arbitrary character strings. The datum (ground) node must be named '0'. Note the difference in SPICE3 where the nodes are treated as character strings and not evaluated as numbers, thus '0' and '00' are distinct nodes in SPICE3 but not in SPICE2. The circuit cannot contain a loop of voltage sources and/or inductors and cannot contain a cut-set 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).

TITLE LINE, COMMENT LINES AND .END LINE

Title Line

Examples:

POWER AMPLIFIER CIRCUIT

TEST OF CAM CELL

The title line must be the first in the input file. Its contents are printed verbatim as the heading for each section of output.

.End line

Examples:

.END

The "End" line must always be the last in the input file. Note that the period is an integral part of the name.

Comments

General Form:

* &ltany; comment>

Examples:

* RF=1K Gain should be 100

* Check open-loop gain and phase margin

The asterisk in the first column indicates that this line is a comment line. Comment lines may be placed anywhere in the circuit description. Note that SPICE3 also considers any line with leading white space to be a comment.

DEVICE MODELS

General form:

.MODEL MNAME TYPE(PNAME1=PVAL1 PNAME2=PVAL2 ... )

Examples:

.MODEL MOD1 NPN (BF=50 IS=1E-13 VBF=50)

Most simple circuit elements typically require only a few parameter values. However, some devices (semiconductor devices in particular) that are included in SPICE require many parameter values. Often, many devices in a circuit 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 line and assigned a unique model name. The device element lines in SPICE then refer to the model name.

For these more complex device types, each device element line 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 some devices: geometric factors and an initial condition (see the following section on Transistors and Diodes for more details).

MNAME in the above is the model name, and type is one of the following fifteen types:

 

R 

Semiconductor resistor model 

C 

Semiconductor capacitor model 

SW 

Voltage controlled switch 

CSW 

Current controlled switch 

URC 

Uniform distributed RC model 

LTRA 

Lossy transmission line model 

D 

Diode model 

NPN 

NPN BJT model 

PNP 

PNP BJT model 

NJF 

N-channel JFET model 

PJF 

P-channel JFET model 

NMOS 

N-channel MOSFET model 

PMOS 

P-channel MOSFET model 

NMF 

N-channel MESFET model 

PMF 

P-channel MESFET model 

 

Parameter values are defined by appending the parameter name 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. Models, model parameters, and default values are listed in the next section along with the description of device element lines.

SUBCIRCUITS

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 file by a grouping of element lines; 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 //*(AA.

.SUBCKT

General form:

.SUBCKT subnam N1 <N2; N3 ...>

Examples:

.SUBCKT OPAMP 1 2 3 4

A circuit definition is begun with a .SUBCKT line. SUBNAM is the subcircuit name, and N1, N2, ... are the external nodes, which cannot be zero. The group of element lines which immediately follow the .SUBCKT line define the subcircuit. The last line in a subcircuit definition is the .ENDS line (see below). Control lines 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 line are strictly local, with the exception of 0 (ground) which is always global.

.ENDS

General form:

.ENDS <SUBNAM;>

Examples:

.ENDS OPAMP

The "Ends" line 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.

Subcircuit Calls

General form:

XYYYYYYY N1 <N2; N3 ...> SUBNA

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.

COMBINING FILES: .INCLUDE LINES

General form:

.INCLUDE filename

Examples:

.INCLUDE /users/spice/common/wattmeter.cir

Frequently, portions of circuit descriptions will be reused in several input files, particularly with common models and subcircuits. In any spice input file, the ".include" line may be used to copy some other file as if that second file appeared in place of the ".include" line in the original file. There is no restriction on the file name imposed by spice beyond those imposed by the local operating system.

3.           ANALYSES AND OUTPUT CONTROL

The following command lines are for specifying analyses or plots within the circuit description file. Parallel commands exist in the interactive command interpreter (detailed in the following section). Specifying analyses and plots (or tables) in the input file is useful for batch runs. Batch mode is entered when either the -b option is given or when the default input source is redirected from a file. In batch mode, the analyses specified by the control lines in the input file (e.g. ".ac", ".tran", etc.) are immediately executed (unless ".control" lines exists; see the section on the interactive command interpretor). If the -r rawfile option is given then all data generated is written to a Spice3 rawfile. The rawfile may be read by either the interactive mode of Spice3 or by nutmeg; see the previous section for details. In this case, the .SAVE line (see below) may be used to record the value of internal device variables (see Appendix B).

If a rawfile is not specified, then output plots (in "line-printer" form) and tables can be printed according to the .PRINT, .PLOT, and .FOUR control lines, described next. .PLOT, .PRINT, and .FOUR lines are meant for compatibility with Spice2.

SIMULATOR VARIABLES (.OPTIONS)

Various parameters of the simulations available in Spice3 can be altered to control the accuracy, speed, or default values for some devices. These parameters may be changed via the "set" command (described later in the section on the interactive front-end) or via the ".OPTIONS" line:

General form:

.OPTIONS OPT1 OPT2 ... (or OPT=OPTVAL ...)
 

Examples:

.OPTIONS RELTOL=.005 TRTOL=8

The options line allows the user to reset program control and user options for specific simulation purposes. Additional options for Nutmeg may be specified as well and take effect when Nutmeg reads the input file. Options specified to Nutmeg via the 'set' command are also passed on to SPICE3 as if specified on a .OPTIONS line. See the following section on the interactive command interpreter for the parameters which may be set with a .OPTIONS line and the format of the 'set' 'command. Any combination of the following options may be included, in any order. 'x' (below) represents some positive number.

option 

effect 

ABSTOL=x 

resets the absolute current error tolerance of the program. 
The default value is 1 picoamp. 

BADMOS3 

Use the older version of the MOS3 model with the "kappa" discontinuity. 

CHGTOL=x 

resets the charge tolerance of the program. The default value is 1.0e-14. 

DEFAD=x 

resets the charge tolerance of the program. The default value is 1.0e-14. 

DEFAS=x 

resets the value for MOS source diffusion area; the default is 0.0. 

DEFL=x 

resets the value for MOS source diffusion area; the default is 0.0. 

DEFW=x 

resets the value for MOS channel width; the default is 100.0 micrometer 

GMIN=x 

resets the value of GMIN, the minimum conductance allowed by the program. The default value is 1.0e-12. 

ITL1=x 

resets the dc iteration limit. The default is 100. 

ITL2=x 

resets the dc transfer curve iteration limit. The default is 50. 

ITL3=x 

resets the lower transient analysis iteration limit. the default value is 4. (Note: not implemented in Spice3). 

ITL4=x 

resets the transient analysis timepoint iteration limit. the default is 10. 

ITL5=x 

resets the transient analysis total iteration limit. the default is 5000. Set ITL5=0 to omit this test. (Note: not implemented in Spice3). 

KEEPOPINFO 

Retain the operating point information when either an 
AC, Distortion, or Pole-Zero analysis is run. 
This is particularly useful if the circuit is large 
and you do not want to run a (redundant) ".OP" analysis. 

METHOD=name 

ets the numerical integration method used by SPICE. 
Possible names are "Gear" or "trapezoidal" (or just "trap"). 
The default is trapezoidal. 

PIVREL=x 

resets the relative ratio between the largest column entry and an acceptable pivot value. The default value is 1.0e-3. 
In the numerical pivoting algorithm the allowed minimum pivot value is determined by 
EPSREL=AMAX1(PIVREL*MAXVAL, PIVTOL) 
where MAXVAL is the maximum element in the column where a pivot is sought (partial pivoting). 

PIVTOL=x 

resets the absolute minimum value for a matrix entry to be accepted as a pivot. The default value is 1.0e-13. 

RELTOL=x 

resets the relative error tolerance of the program. The default value is 0.001 (0.1%). 

TEMP=x 

Resets the operating temperature of the circuit. The default value is 27 deg C (300 deg K). TEMP can be overridden by a temperature specification on any temperature dependent instance. 

TNOM=x 

resets the nominal temperature at which device parameters are measured. The default value is 27 deg C (300 deg K). TNOM can be overridden by a specification on any temperature dependent device model. 

TRTOL=x 

resets the transient error tolerance. The default value is 7.0. This parameter is an estimate of the factor by which SPICE overestimates the actual truncation error. 

TRYTOCOMPACT 

Applicable only to the LTRA model. When specified, the simulator tries to condense LTRA transmission lines' past history of input voltages and currents. 

VNTOL=x 

resets the absolute voltage error tolerance of the program. The default value is 1 microvolt. 

In addition, the following options have the listed effect when operating in spice2 emulation mode:   

option 

effect 

ACCT 

causes accounting and run time statistics to be printed 

LIST 

causes the summary listing of the input data to be printed 

NOMOD 

suppresses the printout of the model parameters 

NOPAGE 

suppresses page ejects 

NODE 

causes the printing of the node table. 

OPTS 

causes the option values to be printed. 

 

INITIAL CONDITIONS

.NODESET: Specify Initial Node Voltage Guesses

General form:

.NODESET V(NODNUM)=VAL V(NODNUM)=VAL ...

Examples:

.NODESET V(12)=4.5 V(4)=2.23
 
The Nodeset line 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 line may be necessary for convergence on bistable or a-stable circuits. In general, this line should not be necessary.

.IC: Set Initial Conditions

General form:

.IC V(NODNUM)=VAL V(NODNUM)=VAL ...

Examples:

.IC V(11)=5 V(4)=-5 V(2)=2.2

The IC line is for setting transient initial conditions. It has two different interpretations, depending on whether the UIC parameter is specified on the .TRAN control line. Also, one should not confuse this line with the .NODESET line. The .NODESET line is only to help dc convergence, and does not affect final bias solution (except for multi-stable circuits). The two interpretations of this line are as follows:

1. When the UIC parameter is specified on the .TRAN line, then the node voltages specified on the .IC control line are used to compute the capacitor, diode, BJT, JFET, and MOSFET initial conditions. This is equivalent to specifying the IC=... parameter on each device line, but is much more convenient. The IC=... parameter can still be specified and takes 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 control line if they are to be used to compute device initial conditions.

2. When the UIC parameter is not specified on the .TRAN control line, the dc bias (initial transient) solution is computed before the transient analysis. In this case, the node voltages specified on the .IC control line is forced to the desired initial values during the bias solution. During transient analysis, the constraint on these node voltages is removed. This is the preferred method since it allows SPICE to compute a consistent dc solution.

ANALYSES

.AC: Small-Signal AC Analysis

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 line is included in the input file, SPICE performs 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.

.DC: DC Transfer Function

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
 

The DC line defines the dc transfer curve source and sweep limits (again with capacitors open and inductors shorted). 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 causes 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 is 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 circuit description in Appendix A.

.DISTO: Distortion Analysis

General form:

.DISTO DEC ND FSTART FSTOP &ltF2OVERF1;>

.DISTO OCT NO FSTART FSTOP &ltF2OVERF1;>

.DISTO LIN NP FSTART FSTOP &ltF2OVERF1;>
 

Examples:

.DISTO DEC 10 1kHz 100Mhz

.DISTO DEC 10 1kHz 100Mhz 0.9
 
The Disto line does a small-signal distortion analysis of the circuit. A multi-dimensional Volterra series analysis is done using multi-dimensional Taylor series to represent the nonlinearities at the operating point. Terms of up to third order are used in the series expansions.

If the optional parameter F2OVERF1 is not specified, .DISTO does a harmonic analysis - i.e., it analyses distortion in the circuit using only a single input frequency F1, which is swept as specified by arguments of the .DISTO command exactly as in the .AC command. Inputs at this frequency may be present at more than one input source, and their magnitudes and phases are specified by the arguments of the DISTOF1 keyword in the input file lines for the input sources (see the description for independent sources). (The arguments of the DISTOF2 keyword are not relevant in this case). The analysis produces information about the A.C. values of all node voltages and branch currents at the harmonic frequencies 2 F1 and 3 F1, vs. the input frequency F1 as it is swept. (A value of 1 (as a complex distortion output) signifies cos( 2  (2 F1) t) at 2 F1 and cos (2  (3 F1) t ) at 3 F1, using the convention that 1 at the input fundamental frequency is equivalent to cos( 2  F1 t ).) The distortion component desired (2 F1 or 3 F1) can be selected using commands in nutmeg, and then printed or plotted. (Normally, one is interested primarily in the magnitude of the harmonic components, so the magnitude of the AC distortion value is looked at). It should be noted that these are the A.C. values of the actual harmonic components, and are not equal to HD2 and HD3. To obtain HD2 and HD3, one must divide by the corresponding A.C. values at F1, obtained from an .AC line. This division can be done using nutmeg commands.

If the optional F2OVERF1 parameter is specified, it should be a real number between (and not equal to) 0.0 and 1.0; in this case, .DISTO does a spectral analysis. It considers the circuit with sinusoidal inputs at two different frequencies F1 and F2. F1 is swept according to the .DISTO control line options exactly as in the .AC control line. F2 is kept fixed at a single frequency as F1 sweeps - the value at which it is kept fixed is equal to F2OVERF1 times FSTART. Each independent source in the circuit may potentially have two (superimposed) sinusoidal inputs for distortion, at the frequencies F1 and F2. The magnitude and phase of the F1 component are specified by the arguments of the DISTOF1 keyword in the source's input line (see the description of independent sources); the magnitude and phase of the F2 component are specified by the arguments of the DISTOF2 keyword. The analysis produces plots of all node voltages/branch currents at the intermodulation product frequencies F1 + F2, F1 - F2, and (2 F1) - F2, vs the swept frequency F1. The IM product of interest may be selected using the setplot command, and displayed with the print and plot commands. It is to be noted as in the harmonic analysis case, the results are the actual AC voltages and currents at the intermodulation frequencies, and need to be normalized with respect to .AC values to obtain the IM parameters.

If the DISTOF1 or DISTOF2 keywords are missing from the description of an independent source, then that source is assumed to have no input at the corresponding frequency. The default values of the magnitude and phase are 1.0 and 0.0 respectively. The phase should be specified in degrees.

It should be carefully noted that the number F2OVERF1 should ideally be an irrational number, and that since this is not possible in practice, efforts should be made to keep the denominator in its fractional representation as large as possible, certainly above 3, for accurate results (i.e., if F2OVERF1 is represented as a fraction A/B, where A and B are integers with no common factors, B should be as large as possible; note that A < B because F2OVERF1 is constrained to be < 1). To illustrate why, consider the cases where F2OVERF1 is 49/100 and 1/2. In a spectral analysis, the outputs produced are at F1 + F2, F1 - F2 and 2 F1 - F2. In the latter case, F1 - F2 = F2, so the result at the F1-F2 component is erroneous because there is the strong fundamental F2 component at the same frequency. Also, F1 + F2 = 2 F1 - F2 in the latter case, and each result is erroneous individually. This problem is not there in the case where F2OVERF1 = 49/100, because F1-F2 = 51/100 F1 < > 49/100 F1 = F2. In this case, there are two very closely spaced frequency components at F2 and F1 - F2. One of the advantages of the Volterra series technique is that it computes distortions at mix frequencies expressed symbolically (i.e. n F1  m F2), therefore one is able to obtain the strengths of distortion components accurately even if the separation between them is very small, as opposed to transient analysis for example. The disadvantage is of course that if two of the mix frequencies coincide, the results are not merged together and presented (though this could presumably be done as a postprocessing step). Currently, the interested user should keep track of the mix frequencies himself or herself and add the distortions at coinciding mix frequencies together should it be necessary.

.NOISE: Noise Analysis

General form:

.NOISE V(OUTPUT <,REF>) SRC ( DEC | LIN | OCT ) PTS FSTART FSTOP
+ &ltPTS;_PER_SUMMARY>
 

Examples:

.NOISE V(5) VIN DEC 10 1kHZ 100Mhz

.NOISE V(5,3) V1 OCT 8 1.0 1.0e6 1
 
The Noise line does a noise analysis of the circuit. OUTPUT is the node at which the total output noise is desired; if REF is specified, then the noise voltage V(OUTPUT) - V(REF) is calculated. By default, REF is assumed to be ground. SRC is the name of an independent source to which input noise is referred. PTS, FSTART and FSTOP are .AC type parameters that specify the frequency range over which plots are desired. PTS_PER_SUMMARY is an optional integer; if specified, the noise contributions of each noise generator is produced every PTS_PER_SUMMARY frequency points.

The .NOISE control line produces two plots - one for the Noise Spectral Density curves and one for the total Integrated Noise over the specified frequency range. All noise voltages/currents are in squared units V²/Hz and A²/Hz for spectral density, V² and A² for integrated noise).

.OP: Operating Point Analysis

General form:

.OP
 
The inclusion of this line in an input file directs 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, Noise, and Pole-Zero analysis to determine the linearized, small-signal models for nonlinear devices (see the KEEPOPINFO variable above).

.PZ: Pole-Zero Analysis

General form:

.PZ NODE1 NODE2 NODE3 NODE4 CUR POL

.PZ NODE1 NODE2 NODE3 NODE4 CUR ZER

.PZ NODE1 NODE2 NODE3 NODE4 CUR PZ

.PZ NODE1 NODE2 NODE3 NODE4 VOL POL

.PZ NODE1 NODE2 NODE3 NODE4 VOL ZER

.PZ NODE1 NODE2 NODE3 NODE4 VOL PZ
 

Examples:

.PZ 1 0 3 0 CUR POL

.PZ 2 3 5 0 VOL ZER

.PZ 4 1 4 1 CUR PZ
 
CUR stands for a transfer function of the type (output voltage)/(input current) while VOL stands for a transfer function of the type (output voltage)/(input voltage). POL stands for pole analysis only, ZER for zero analysis only and PZ for both. This feature is provided mainly because if there is a nonconvergence in finding poles or zeros, then, at least the other can be found. Finally, NODE1 and NODE2 are the two input nodes and NODE3 and NODE4 are the two output nodes. Thus, there is complete freedom regarding the output and input ports and the type of transfer function.

In interactive mode, the command syntax is the same except that the first field is PZ instead of .PZ. To print the results, one should use the command 'print all'.

.SENS: DC or Small-Signal AC Sensitivity Analysis

General form:

.SENS OUTVAR

.SENS OUTVAR AC DEC ND FSTART FSTOP

.SENS OUTVAR AC OCT NO FSTART FSTOP

.SENS OUTVAR AC LIN NP FSTART FSTOP
 

Examples:

.SENS V(1,OUT)

.SENS V(OUT) AC DEC 10 100 100k

.SENS I(VTEST)
 
The sensitivity of OUTVAR to all non-zero device parameters is calculated when the SENS analysis is specified. OUTVAR is a circuit variable (node voltage or voltage-source branch current). The first form calculates sensitivity of the DC operating-point value of OUTVAR. The second form calculates sensitivity of the AC values of OUTVAR. The parameters listed for AC sensitivity are the same as in an AC analysis (see ".AC" above). The output values are in dimensions of change in output per unit change of input (as opposed to percent change in output or per percent change of input).

.TF: Transfer Function Analysis

General form:

.TF OUTVAR INSRC
 

Examples:

.TF V(5, 3) VIN

.TF I(VLOAD) VIN
 
The TF line 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 line is included, SPICE computes 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.

.TRAN: Transient Analysis

General form:

.TRAN TSTEP TSTOP &ltTSTART; &ltTMAX;>>
 

Examples:

.TRAN 1NS 100NS

.TRAN 1NS 1000NS 500NS

.TRAN 10NS 1US
 
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 &ltzero;, TSTART>, the circuit is analyzed (to reach a steady state), but no outputs are stored. In the interval &ltTSTART;, TSTOP>, the circuit is analyzed and outputs are stored. TMAX is the maximum stepsize that SPICE uses; 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 control line has been specified, then the node voltages on the .IC line are used to compute the initial conditions for the devices. Look at the description on the .IC control line for its interpretation when UIC is not specified.

BATCH OUTPUT

.SAVE Lines

General form:

.SAVE vector vector vector ...
 

Examples:

.SAVE i(vin) input output

.SAVE @m1[id]
 
The vectors listed on the .SAVE line are recorded in the rawfile for use later with spice3 or nutmeg (nutmeg is just the data-analysis half of spice3, without the ability to simulate). The standard vector names are accepted. If no .SAVE line is given, then the default set of vectors are saved (node voltages and voltage source branch currents). If .SAVE lines are given, only those vectors specified are saved. For more discussion on internal device data, see Appendix B. See also the section on the interactive command interpretor for information on how to use the rawfile.

.PRINT Lines

General form:

.PRINT PRTYPE OV1 &ltOV2; ... OV8>
 

Examples:

.PRINT TRAN V(4) I(VIN)

.PRINT DC V(2) I(VSRC) V(23, 17)

.PRINT AC VM(4, 2) VR(7) VP(8, 3)
 
The Print line 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 the same as given in the previous section for the print command; Spice2 restricts the output variable to the following forms (though this restriction is not enforced by Spice3):

V(N1<,N2>)

specifies the voltage difference between nodes N1 and N2. If N2 (and the preceding comma) is omitted, ground (0) is assumed. See the print command in the previous section for more details. For compatibility with spice2, the following five additional values can be accessed for the ac analysis by replacing the "V" in V(N1,N2) with:

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.

There is no limit on the number of .PRINT lines for each type of analysis.

.PLOT Lines

General form:

.PLOT PLTYPE OV1 <(PLO1, PHI1)> &ltOV2; <(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)

The Plot line 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 line and for the plot command in the interactive mode.

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 is printed as well as plotted. If a printout of all variables is desired, then a companion .PRINT line should be included.

There is no limit on the number of .PLOT lines specified for each type of analysis.

.FOUR: Fourier Analysis of Transient Analysis Output

General form:

.FOUR FREQ OV1 &ltOV2; OV3 ...>
 

Examples:

.FOUR 100K V(5)
 
The Four (or Fourier) line 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 &ltTSTOP-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 harmonics are determined. For maximum accuracy, TMAX (see the .TRAN line) should be set to period/100.0 (or less for very high-Q circuits).

4.           CIRCUIT ELEMENTS AND MODELS

Data fields that are enclosed in less-than and greater-than signs ('< >') are optional. All indicated punctuation (parentheses, equal signs, etc.) is optional but indicate the presence of any delimiter. Further, future implementations may require the punctuation as stated. A consistent style adhering to the punctuation shown here makes the input easier to understand. With respect to branch voltages and currents, SPICE uniformly uses the associated reference convention (current flows in the direction of voltage drop).

ELEMENTARY DEVICES

Resistors

General form:

RXXXXXXX N1 N2 VALUE

Examples:

R1 1 2 100

RC1 12 17 1K

N1 and N2 are the two element nodes. VALUE is the resistance (in ohms) and may be positive or negative but not zero.

Semiconductor Resistors

General form:

RXXXXXXX N1 N2 <VALUE> <MNAME> <L=LENGTH> <W=WIDTH> <TEMP=T>

Examples:

RLOAD 2 10 10K

RMOD 3 7 RMODEL L=10u W=1u

This is the more general form of the resistor presented in section 6.1, and allows the modeling of temperature effects and for the calculation of the actual resistance value from strictly geometric information and the specifications of the process. If VALUE is specified, it overrides the geometric information and defines the resistance. If MNAME is specified, then the resistance may be calculated from the process information in the model MNAME and the given LENGTH and WIDTH. If VALUE is not specified, then MNAME and LENGTH must be specified. If WIDTH is not specified, then it is taken from the default width given in the model. The (optional) TEMP value is the temperature at which this device is to operate, and overrides the temperature specification on the .OPTION control line.

Semiconductor Resistor Model (R)

The resistor model consists of process-related device data that allow the resistance to be calculated from geometric information and to be corrected for temperature. The parameters available are:
 

name

parameter

units

default

example

TC1 

first order temperature coeff. 

/ C 

0.0 

- 

TC2 

second order temperature coeff. 

/ C² 

0.0 

- 

RSH 

sheet resistance 

/q 

- 

50 

DEFW 

default width 

meters 

1.e-6 

2.e-6 

NARROW 

narrowing due to side etching 

meters 

0.0 

1.e-7 

TNOM 

parameter measurement temperature 

C 

27 

50 

 
The sheet resistance is used with the narrowing parameter and L and W from the resistor device to determine the nominal resistance by the formula

DEFW is used to supply a default value for W if one is not specified for the device. If either RSH or L is not specified, then the standard default resistance value of 1k  is used. TNOM is used to override the circuit-wide value given on the .OPTIONS control line where the parameters of this model have been measured at a different temperature. After the nominal resistance is calculated, it is adjusted for temperature by the formula:

Capacitors

General form:

CXXXXXXX N+ N- VALUE <IC=INCOND>

Examples:

CBYP 13 0 1UF

COSC 17 23 10U IC=3V

N+ and N- are the positive and negative element nodes, respectively. VALUE is the capacitance in Farads.

The (optional) initial condition is the initial (time-zero) value of capacitor voltage (in Volts). Note that the initial conditions (if any) apply 'only' if the UIC option is specified on the .TRAN control line.

Semiconductor Capacitors

General form:

CXXXXXXX N1 N2 <VALUE> <MNAME> <L=LENGTH> <W=WIDTH> <IC=VAL>

Examples:

CLOAD 2 10 10P

CMOD 3 7 CMODEL L=10u W=1u

This is the more general form of the Capacitor presented in section 6.2, and allows for the calculation of the actual capacitance value from strictly geometric information and the specifications of the process. If VALUE is specified, it defines the capacitance. If MNAME is specified, then the capacitance is calculated from the process information in the model MNAME and the given LENGTH and WIDTH. If VALUE is not specified, then MNAME and LENGTH must be specified. If WIDTH is not specified, then it is taken from the default width given in the model. Either VALUE or MNAME, LENGTH, and WIDTH may be specified, but not both sets.

Semiconductor Capacitor Model (C)

The capacitor model contains process information that may be used to compute the capacitance from strictly geometric information.
 

name

parameter

units

default

example

CJ 

junction bottom capacitance 

F/meters² 

- 

5.e-5 

CJSW 

junction sidewall capacitance 

F/meters 

- 

2.e-11 

DEFW 

default device width 

meters 

1.e-6 

2.e-6 

NARROW 

narrowing due to side etching 

meters 

0.0 

1.e-7 

 
The capacitor has a capacitance computed as

Inductors

General form:

LYYYYYYY N+ N- VALUE <IC=INCOND>

Examples:

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 inductance in Henries.

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 analysis line.

Coupled (Mutual) Inductors

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.

Switches

General form:

SXXXXXXX N+ N- NC+ NC- MODEL <ON><OFF>

WYYYYYYY N+ N- VNAM MODEL <ON><OFF>

Examples:

s1 1 2 3 4 switch1 ONs2 5 6 3 0 sm2 off

Switch1 1 2 10 0 smodel1

w1 1 2 vclock switchmod1

W2 3 0 vramp sm1 ON

wreset 5 6 vclck lossyswitch OFF

Nodes 1 and 2 are the nodes between which the switch terminals are connected. The model name is mandatory while the initial conditions are optional. For the voltage controlled switch, nodes 3 and 4 are the positive and negative controlling nodes respectively. For the current controlled switch, the controlling current is that through the specified voltage source. The direction of positive controlling current flow is from the positive node, through the source, to the negative node.

Switch Model (SW/CSW)

The switch model allows an almost ideal switch to be described in SPICE. The switch is not quite ideal, in that the resistance can not change from 0 to infinity, but must always have a finite positive value. By proper selection of the on and off resistances, they can be effectively zero and infinity in comparison to other circuit elements. The parameters available are:
 

name

parameter

units

default

switch

VT 

threshold voltage 

Volts 

0.0 

S 

IT 

threshold current 

Amps 

0.0 

W 

VH 

hysteresis voltage 

Volts 

0.0 

S 

IH 

hysteresis current 

Amps 

0.0 

W 

RON 

on resistance 

 

1.0 

both 

ROFF 

off resistance 

 

1/GMIN* 

both 

 
*(See the .OPTIONS control line for a description of GMIN, its default value results in an off-resistance of 1.0e+12 ohms.)

The use of an ideal element that is highly nonlinear such as a switch can cause large discontinuities to occur in the circuit node voltages. A rapid change such as that associated with a switch changing state can cause numerical roundoff or tolerance problems leading to erroneous results or timestep difficulties. The user of switches can improve the situation by taking the following steps:

First, it is wise to set ideal switch impedances just high or low enough to be negligible with respect to other circuit elements. Using switch impedances that are close to "ideal" in all cases aggravates the problem of discontinuities mentioned above. Of course, when modeling real devices such as MOSFETS, the on resistance should be adjusted to a realistic level depending on the size of the device being modeled.

If a wide range of ON to OFF resistance must be used in the switches (ROFF/RON >1e;+12), then the tolerance on errors allowed during transient analysis should be decreased by using the .OPTIONS control line and specifying TRTOL to be less than the default value of 7.0. When switches are placed around capacitors, then the option CHGTOL should also be reduced. Suggested values for these two options are 1.0 and 1e-16 respectively. These changes inform SPICE3 to be more careful around the switch points so that no errors are made due to the rapid change in the circuit.

VOLTAGE AND CURRENT SOURCES

Independent Sources

General form:

VXXXXXXX N+ N- <DC<> DC/TRAN VALUE> <AC <ACMAG <ACPHASE>>>

+ <DISTOF1 <F1MAG <F1PHASE>>> <DISTOF2 <F2MAG <F2PHASE>>>

IYYYYYYY N+ N- <<DC> DC/TRAN VALUE> <AC <ACMAG <ACPHASE>>>

+ <DISTOF1 <F1MAG <F1PHASE>>> <DISTOF2 <F2MAG <F2PHASE>>>

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

VCARRIER 1 0 DISTOF1 0.1 -90.0

VMODULATOR 2 0 DISTOF2 0.01

IIN1 1 5 AC 1 DISTOF1 DISTOF2 0.001

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 forces 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 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.

DISTOF1 and DISTOF2 are the keywords that specify that the independent source has distortion inputs at the frequencies F1 and F2 respectively (see the description of the .DISTO control line). The keywords may be followed by an optional magnitude and phase. The default values of the magnitude and phase are 1.0 and 0.0 respectively.

Any independent source can be assigned a time-dependent value for transient analysis. If a source is assigned a time-dependent 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 are assumed. (TSTEP is the printing increment and TSTOP is the final time (see the .TRAN control line for explanation)).

Pulse

General form:

PULSE(V1 V2 TD TR TF PW PER)

Examples:

VIN 3 0 PULSE(-1 1 2NS 2NS 2NS 50NS 100NS)

 

parameter

default value

units 

V1 (initial value)

 

Volts or Amps

V2 (pulsed value)

 

Volts or Amps

TD (delay time)

0.0 

seconds

TR (rise time)

TSTEP

seconds

TF (fall time)

TSTEP

seconds

PW (pulse width)

TSTOP

seconds

PER(period)

TSTOP

seconds

 
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 V2

V1

TSTOP

V1

 
Intermediate points are determined by linear interpolation.

Sinusoidal

General form:

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

 

Exponential

General Form:

EXP(V1 V2 TD1 TAU1 TD2 TAU2)

Examples:

VIN 3 0 EXP(-4 -1 2NS 30NS 60NS 40NS)

 

parameter

default value

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 

TSTEP

seconds

  The shape of the waveform is described by the following table:
   

time 

value 

0 to TD1

V1 

TD1 to TD2

 

TD2 to TSTOP

 

 

Piece-Wise Linear

General Form:

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)

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.

Single-Frequency FM

General Form:

SFFM(VO VA FC MDI FS)

Examples:

V1 12 0 SFFM(0 1M 20K 5 1K)

 

parameter

default value

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:

Linear Dependent Sources

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.

Linear Voltage-Controlled Current Sources

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).

Linear Voltage-Controlled Voltage Sources

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.

Linear Current-Controlled Current Sources

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.

Linear Current-Controlled Voltage Sources

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).

Non-linear Dependent Sources

General form:

BXXXXXXX N+ N- <I=EXPR> <V=EXPR>
 

Examples:

B1 0 1 I=cos(v(1))+sin(v(2))

B1 0 1 V=ln(cos(log(v(1,2)^2)))-v(3)^4+v(2)^v(1)

B1 3 4 I=17

B1 3 4 V=exp(pi^i(vdd))
 

N+ is the positive node, and N- is the negative node. The values of the V and I parameters determine the voltages and currents across and through the device, respectively. If I is given then the device is a current source, and if V is given the device is a voltage source. One and only one of these parameters must be given.

The small-signal AC behavior of the nonlinear source is a linear dependent source (or sources) with a proportionality constant equal to the derivative (or derivatives) of the source at the DC operating point.

The expressions given for V and I may be any function of voltages and currents through voltage sources in the system. The following functions of real variables are defined:
 

abs

asinh 

cosh 

sin 

acos 

atan 

exp 

sinh 

acosh 

atanh 

ln 

sqrt 

asin 

cos 

log 

tan 

The function "u" is the unit step function, with a value of one for arguments greater than one and a value of zero for arguments less than zero. The function "uramp" is the integral of the unit step: for an input x, the value is zero if x is less than zero, or if x is greater than zero the value is x. These two functions are useful in sythesizing piece-wise non-linear functions, though convergence may be adversely affected.

The following standard operators are defined:
 

+ - * / ^ unary -

If the argument of log, ln, or sqrt becomes less than zero, the absolute value of the argument is used. If a divisor becomes zero or the argument of log or ln becomes zero, an error will result. Other problems may occur when the argument for a function in a partial derivative enters a region where that function is undefined.

To get time into the expression you can integrate the current from a constant current source with a capacitor and use the resulting voltage (don't forget to set the initial voltage across the capacitor). Non-linear resistors, capacitors, and inductors may be synthesized with the nonlinear dependent source. Non-linear resistors are obvious. Non-linear capacitors and inductors are implemented with their linear counterparts by a change of variables implemented with the nonlinear dependent source. The following subcircuit will implement a nonlinear capacitor:

.Subckt nlcap pos neg

* Bx: calculate f(input voltage)

Bx 1 0 v = f(v(pos,neg))

* Cx: linear capacitance

Cx 2 0 1

* Vx: Ammeter to measure current into the capacitor

Vx 2 1 DC 0Volts

* Drive the current through Cx back into the circuit

Fx pos neg Vx 1

.ends

Non-linear inductors are similar.

TRANSMISSION LINES

Lossless Transmission Lines

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 transmission-line elements are required. (see the example in //*(AA 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 control line.

Note that a lossy transmission line (see below) with zero loss may be more accurate than than the lossless transmission line due to implementation details.

Lossy Transmission Lines

General form:

OXXXXXXX N1 N2 N3 N4 MNAME
 

Examples:

O23 1 0 2 0 LOSSYMOD

OCONNECT 10 5 20 5 INTERCONNECT
 

This is a two-port convolution model for single-conductor lossy transmission lines. N1 and N2 are the nodes at port 1; N3 and N4 are the nodes at port 2. Note that a lossy transmission line with zero loss may be more accurate than than the lossless transmission line due to implementation details.

Lossy Transmission Line Model (lTRA)

The uniform RLC/RC/LC/RG transmission line model (referred to as the LTRA model henceforth) models a uniform constant-parameter distributed transmission line. The RC and LC cases may also be modeled using the URC and TRA models; however, the newer LTRA model is usually faster and more accurate than the others. The operation of the LTRA model is based on the convolution of the transmission line's impulse responses with its inputs (see [8]).

The LTRA model takes a number of parameters, some of which must be given and some of which are optional.
 

name 

parameter 

units/type 

default 

example 

R 

resistance/length

 

0.0 

0.2 

L 

inductance/length

henrys/unit

0.0 

9.13e-9

G 

conductance/length

mhos/unit 

0.0 

0.0 

C 

capacitance/length

farads/unit 

0.0 

3.65e-12

LEN 

lenght of line 

 

no default 

1.0 

REL 

breakpoint control 

arbitrary unit 

1 

0.5 

ABS 

breakpoint control 

 

1 

5 

NOSTEPLIMIT 

don't limit timestep to less than line delay

flag 

not set 

set 

NOCONTROL

don't do complex timestep control 

flag 

not set 

set 

LININTERP

use lineair interpolation 

flag 

not set 

set 

MIXEDINTERP

use lineair when quadratic seems bad 

 

not set 

set 

COMPACTREL

special reltol for history compaction 

flag 

RELTOL 

1.0e-3

COMPACTABS

special abstol for history compaction 

 

ABSTOL 

1.0e-9

TRUNCNR

use Newton-Raphson method for timestep control 

flag 

not set 

set 

TRUNCDONTCUT

don't limit timestep to keep impulse-response errors low 

flag 

not set 

set 

The following types of lines have been implemented so far: RLC (uniform transmission line with series loss only), RC (uniform RC line), LC (lossless transmission line), and RG (distributed series resistance and parallel conductance only). Any other combination will yield erroneous results and should not be tried. The length LEN of the line must be specified.

NOSTEPLIMIT is a flag that will remove the default restriction of limiting time-steps to less than the line delay in the RLC case. NOCONTROL is a flag that prevents the default limiting of the time-step based on convolution error criteria in the RLC and RC cases. This speeds up simulation but may in some cases reduce the accuracy of results. LININTERP is a flag that, when specified, will use linear interpolation instead of the default quadratic interpolation for calculating delayed signals. MIXEDINTERP is a flag that, when specified, uses a metric for judging whether quadratic interpolation is not applicable and if so uses linear interpolation; otherwise it uses the default quadratic interpolation. TRUNCDONTCUT is a flag that removes the default cutting of the time-step to limit errors in the actual calculation of impulse-response related quantities. COMPACTREL and COMPACTABS are quantities that control the compaction of the past history of values stored for convolution. Larger values of these lower accuracy but usually increase simulation speed. These are to be used with the TRYTOCOMPACT option, described in the .OPTIONS section. TRUNCNR is a flag that turns on the use of Newton-Raphson iterations to determine an appropriate timestep in the timestep control routines. The default is a trial and error procedure by cutting the previous timestep in half. REL and ABS are quantities that control the setting of breakpoints.

The option most worth experimenting with for increasing the speed of simulation is REL. The default value of 1 is usually safe from the point of view of accuracy but occasionally increases computation time. A value greater than 2 eliminates all breakpoints and may be worth trying depending on the nature of the rest of the circuit, keeping in mind that it might not be safe from the viewpoint of accuracy. Breakpoints may usually be entirely eliminated if it is expected the circuit will not display sharp discontinuities. Values between 0 and 1 are usually not required but may be used for setting many breakpoints.

COMPACTREL may also be experimented with when the option TRYTOCOMPACT is specified in a .OPTIONS card. The legal range is between 0 and 1. Larger values usually decrease the accuracy of the simulation but in some cases improve speed. If TRYTOCOMPACT is not specified on a .OPTIONS card, history compaction is not attempted and accuracy is high. NOCONTROL, TRUNCDONTCUT and NOSTEPLIMIT also tend to increase speed at the expense of accuracy.

Uniform Distributed RC Lines (lossy)

General form:

UXXXXXXX N1 N2 N3 MNAME L=LEN <N=LUMPS>
 

Examples:

U1 1 2 0 URCMOD L=50U

URC2 1 12 2 UMODL l=1MIL N=6

N1 and N2 are the two element nodes the RC line connects, while N3 is the node to which the capacitances are connected. MNAME is the model name, LEN is the length of the RC line in meters. LUMPS, if specified, is the number of lumped segments to use in modeling the RC line (see the model description for the action taken if this parameter is omitted).

Uniform Distributed RC Model (URC)

The URC model is derived from a model proposed by L. Gertzberrg in 1974. The model is accomplished by a subcircuit type expansion of the URC line into a network of lumped RC segments with internally generated nodes. The RC segments are in a geometric progression, increasing toward the middle of the URC line, with K as a proportionality constant. The number of lumped segments used, if not specified for the URC line device, is determined by the following formula:

The URC line is made up strictly of resistor and capacitor segments unless the ISPERL parameter is given a non-zero value, in which case the capacitors are replaced with reverse biased diodes with a zero-bias junction capacitance equivalent to the capacitance replaced, and with a saturation current of ISPERL amps per meter of transmission line and an optional series resistance equivalent to RSPERL ohms per meter. 

 

name 

parameter 

units 

default 

example 

area 

1 

K 

Propagation Constant

- 

2.0 

1.2 

- 

2 

FMAX 

Maximum Frequency of interest

Hz 

1.0G 

6.5Meg 

- 

3 

RPERL 

Resistance per unit length

 

1000 

10 

- 

4 

CPERL 

Capacitance per unit length

F/m 

1.0e-15

1pF 

- 

5 

ISPERL 

Saturation Current per unit length

A/m 

0 

- 

- 

6 

RSPERL 

Diode Resistance per unit length

 

0 

- 

- 

TRANSISTORS AND DIODES

The area factor used on the diode, BJT, JFET, and MESFET devices 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 line.

Two different forms of initial conditions may be specified for some 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 still obtains the correct solution (assuming the solutions converge) but more iterations are required since the program must independently converge to two separate solutions. The .NODESET control line 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 control line and the .TRAN control line for a detailed explanation of initial conditions.

Junction Diodes

General form:

DXXXXXXX N+ N- MNAME <AREA>> <OFF> <IC=VD> <TEMP>

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 control line, when a transient analysis is desired starting from other than the quiescent operating point. The (optional) TEMP value is the temperature at which this device is to operate, and overrides the temperature specification on the .OPTION control line.

Diode Model (D)

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. The nominal temperature at which these parameters were measured is TNOM, which defaults to the circuit-wide value specified on the .OPTIONS control line. 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).

 

name 

parameter 

units 

default 

example 

area 

1 

IS 

saturation current

A 

1.0e-14

1.0e-14

* 

2 

RS 

ohmic resistance

 

0 

10 

* 

3 

N 

emission coefficient

- 

1 

1.0 

 

4 

TT 

transit-time

sec 

0 

0.1ns 

 

5 

CJO 

zero-bias junction capacitance

F 

0 

2pF 

* 

6 

VJ 

junction potential

V 

1 

0.6 

 

7 

M 

grading coefficient

- 

0.5 

0.5 

 

8 

EG 

activation energy

eV 

1.11 

1.11 Si 
0.69 Sbd 
0.67Ge 

 

9 

XTI 

saturation-current temp. exp

- 

3.0 

3.0jn 
2.0Sbd 

 

10 

KF 

flicker noise coefficient

- 

0 

 

 

11 

AF 

flicker noise exponent

- 

1 

 

 

12 

FC 

coefficient for forward-bais depletion capacitance formula

- 

0.5 

 

 

13 

BV 

reverse breakdown voltage

V 

infinite 

40.0 

 

14 

IBV 

current at breakdown voltage

A 

1.0e-3 

 

 

15 

TNOM 

parameter measurement temperature

C

27 

50 

 

Bipolar Junction Transistors (BJTs)

General form:

QXXXXXXX NC NB NE <NS> MNAME <AREA> <OFF> <IC=VBE, VCE> <TEMP=T>

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 control line, when a transient analysis is desired starting from other than the quiescent operating point. See the .IC control line description for a better way to set transient initial conditions. The (optional) TEMP value is the temperature at which this device is to operate, and overrides the temperature specification on the .OPTION control line.

BJT Models (NPN/PNP)

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 automatically simplifies 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 determined 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 values specified are assumed to have been measured at the temperature TNOM, which can be specified on the .OPTIONS control line or overridden by a specification on the .MODEL line.

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

 

name 

parameter 

units 

default 

example 

area 

1 

IS 

transport saturation current

A 

1.0e-16 

1.0e-15

* 

2 

BF 

ideal maximum forward beta

- 

100 

100 

 

3 

NF 

forward current emission coefficient

- 

1.0 

1 

 

4 

VAF 

forward Early voltage

V 

infinite 

200 

 

5 

IKF 

corner for forward beta high current roll-off

A 

infinite 

0.01 

* 

6 

ISE 

B-E leakage saturation current

A 

0 

1.0e-13

* 

7 

NE 

B-E leakage emission coefficient

- 

1.5 

2 

 

8 

BR 

ideal maximum reverse beta 

- 

1 

0.1 

 

9 

NR 

reverse current emission coefficient

- 

1 

1 

 

10 

VAR 

reverse Early voltage

V 

infinite 

200 

 

11 

IKR 

corner for reverse beta high current roll-off

A 

infinite 

0.01 

* 

12 

ISC 

leakage saturation current

A 

0 

 

8 

13 

NC 

leakage emission coefficient

- 

2 

1.5 

 

14 

RB 

zero bias base resistance

 

0 

100 

* 

15 

IRB 

current where base resistance falls halfway to its min value

A 

infinte 

0.1 

* 

16 

RBM 

minimum base resistance at high currents

 

RB 

10 

* 

17 

RE 

emitter resistance

 

0 

1 

* 

18 

RC 

collector resistance 

 

0 

10 

* 

19 

CJE 

B-E zero-bias depletion capacitance

F 

0 

2pF 

* 

20 

VJE 

B-E built-in potential

V 

0.75 

0.6 

 

21 

MJE 

B-E junction exponential factor 

- 

0.33 

0.33 

 

22 

TF 

ideal forward transit time 

sec 

0 

0.1ns 

 

23 

XTF

coefficient for bias dependence of TF 

- 

0 

 

 

24 

VTF 

voltage describing VBC 
dependence of TF 

V 

infinite 

 

 

25 

ITF 

high-current parameter 
for effect on TF 

A 

0 

 

* 

26 

PTF 

excess phase at freq=1.0/(TF*2PI) Hz 

deg 

0 

 

 

27 

CJC 

B-C zero-bias depletion capacitance 

F 

0 

2pF 

* 

28 

VJC 

B-C built-in potential 

V 

0.75 

0.5 

 

29 

MJC 

B-C junction exponential factor 

- 

0.33 

0.5 

 

30 

XCJC 

fraction of B-C depletion capacitance 
connected to internal base node 

- 

1 

 

 

31 

TR 

ideal reverse transit time 

sec 

0 

10ns 

 

32 

CJS 

zero-bias collector-substrate capacitance 

F 

0 

2pF 

* 

33 

VJS 

substrate junction built-in potential 

V 

0.75 

 

 

34 

MJS 

substrate junction exponential factor 

- 

0 

0.5 

 

35 

XTB 

forward and reverse beta 
temperature exponent 

- 

0 

 

 

36 

EG

energy gap for temperature 
effect on IS 

eV 

1.11 

 

 

37 

XTI

temperature exponent for effect on IS 

- 

3 

 

 

38 

KF 

flicker-noise coefficient 

- 

0 

 

 

39 

AF 

flicker-noise exponent 

- 

1 

 

 

40 

FC 

coefficient for forward-bias 
depletion capacitance formula 

- 

0.5 

 

 

41 

TNOM 

Parameter measurement temperature 

C 

27 

50 

 

 

Junction Field-Effect Transistors (JFETs)

General form:

JXXXXXXX ND NG NS MNAME <AREA> <OFF> <IC=VDS, VGS> <TEMP>

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 control line, when a transient analysis is desired starting from other than the quiescent operating point. See the .IC control line for a better way to set initial conditions. The (optional) TEMP value is the temperature at which this device is to operate, and overrides the temperature specification on the .OPTION control line.

JFET Models (NJF/PJF)

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.

Note that in Spice3f and later, a fitting parameter B has been added. For details, see [9].

 

name

parameter

units

default

example

area

1 

VTO 

threshold voltage (V_T0)

V 

-2.0 

-2.0 

 

2 

BETA 

transconductance parameter ( ) transconductance parameter

A/V²

1.0e-4

1.0e-3 

* 

3 

LAMBDA 

channel-length modulation  
parameter ( ) 

1/V 

0 

1.0e-4

 

4 

RD 

drain ohmic resistance

 

0 

100 

* 

5 

RS 

source ohmic resistance

 

0 

100 

* 

6 

CGS 

zero-bias G-S junction capacitance (C_gs)

F 

0 

5pF 

* 

7 

CGD 

zero-bias G-D junction capacitance (C_gs)

F 

0 

1pF 

* 

8 

PB 

gate junction potential 

V 

1 

0.6 

 

9 

IS 

gate junction saturation current (I_S)

A 

1.0e-14

1.0e-14

* 

10 

B 

doping tail parameter 

- 

1 

1.1 

 

11 

KF 

flicker noise coefficient

- 

0 

 

 

12 

AF 

flicker noise exponent

- 

1 

 

 

13 

FC 

coefficient for forward-bias

- 

0.5 

 

 

14 

TNOM 

parameter measurement temperature

C

27 

50 

 

 

MOSFETs

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> <TEMP=T>

Examples:

M1 24 2 0 20 TYPE1

M31 2 17 6 10 MODM L=5U W=2U

M1 2 9 3 0 MOD1 L=10U W=5U AD=100P AS=100P PD=40U PS=40U

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 m². Note that the suffix U specifies microns (1e-6 m) and P sq-microns (1e-12 m²). If any of L, W, AD, or AS are not specified, default values are used. The use of defaults simplifies input file 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 control line 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 control line, when a transient analysis is desired starting from other than the quiescent operating point. See the .IC control line for a better and more convenient way to specify transient initial conditions. The (optional) TEMP value is the temperature at which this device is to operate, and overrides the temperature specification on the .OPTION control line. The temperature specification is ONLY valid for level 1, 2, 3, and 6 MOSFETs, not for level 4 or 5 (BSIM) devices.

MOSFET Models (NMOS/PMOS)

SPICE provides four 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])
LEVEL=4 -> BSIM (as described in [3])
LEVEL=5 -> new BSIM (BSIM2; as described in [5])
LEVEL=6 -> MOS6 (as described in [2])The dc characteristics of the level 1 through level 3 MOSFETs 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. Charge storage effects are modeled by the piecewise linear voltages-dependent capacitance model proposed by Meyer. The thin-oxide charge-storage effects are treated slightly different for the LEVEL=1 model. These voltage-dependent 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/m²). 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 line; 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/m²) 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 line.

A discontinuity in the MOS level 3 model with respect to the KAPPA parameter has been detected (see [10]). The supplied fix has been implemented in Spice3f2 and later. Since this fix may affect parameter fitting, the option "BADMOS3" may be set to use the old implementation (see the section on simulation variables and the ".OPTIONS" line).

SPICE level 1, 2, 3 and 6 parameters:

 

name

parameter

units

default

example

1 

LEVEL 

model 

index 

- 

1 

2 

VTO 

zero-bias threshold voltage (V_T0) 

V 

0.0 

1.0 

3 

KP 

transconductance parameter 

A/V² 

2.0e-5 

3.1e-5 

4 

GAMMA 

bulk threshold parameter ( ) 

V^1/2 

0.0 

0.37 

5 

PHI 

surface potential () 

V 

0.6 

0.65 

6 

LAMBDA 

channel-length modulation 
(MOS1 and MOS2 only) ( ) 

1/V 

0.0 

0.02 

7 

RD 

drain ohmic resistance 

 

0.0 

1.0 

8 

RS 

source ohmic resistance 

 

0.0 

1.0 

9 

CBD 

zero-bias B-D junction capacitance 

F 

0.0 

20fF 

10 

CBS 

zero-bias B-S junction capacitance 

F 

0.0 

20fF 

11 

IS 

bulk junction saturation current (I_S) 

A 

1.0e-14 

1.0e-15 

12 

PB 

bulk junction potential 

V 

0.8 

0.87 

13 

CGSO 

gate-source overlap capacitance 
per meter channel width 

F/m 

0.0 

4.0e-11 

14 

CGDO

gate-drain overlap capacitance 
per meter channel width 

F/m 

0.0 

4.0e-11 

15 

CGBO

gate-bulk overlap capacitance 
per meter channel length 

F/m 

0.0 

2.0e-10 

16 

RSH

drain and source diffusion 
sheet resistance 

/q 

0.0 

10.0 

17 

CJ 

zero-bias bulk junction bottom cap. 
per sq-meter of junction area 

F/m² 

0.0 

2.0e-4 

18 

MJ 

bulk junction bottom grading coeff. 

- 

0.5 

0.5 

19 

CJSW 

zero-bias bulk junction sidewall cap. 
per meter of junction perimeter 

F/m 

0.0 

1.0e-9 

20 

MJSW 

bulk junction sidewall grading coeff. 

- 

0.50(level1) 
0.33(level2,3) 

 

21 

JS 

bulk junction saturation current 
per sq-meter of junction area 

A/m² 

 

1.0e-8 

22 

TOX 

oxide thickness 

meter 

1.0e-7 

1.0e-7 

23 

NSUB 

substrate doping 

1/cm³ 

0.0 

4.0e15 

24 

NSS 

surface state density 

1/cm² 

0.0 

1.0e10 

25 

NFS 

fast surface state density 

1/cm² 

0.0 

1.0e10 

26 

TPG 

type of gate material: 
+1 opp. to substrate 
-1 same as substrate 
0 Al gate 

- 

1.0 

 

27 

XJ 

metallurgical junction depth 

meter 

0.0 

1  

28 

LD 

lateral diffusion 

meter 

0.0 

0.8  

29 

UO 

surface mobility 

cm²/Vs 

600 

700 

30 

UCRIT 

critical field for mobility 
degradation (MOS2 only) 

V/cm 

1.0e4 

1.0e4 

31 

UEXP 

critical field exponent in 
mobility degradation (MOS2 only) 

- 

0.0 

0.1 

32 

UTRA 

transverse field coeff. (mobility) 
(deleted for MOS2) 

- 

0.0 

0.3 

33 

VMAX 

maximum drift velocity of carriers 

m/s 

0.0 

5.0e4 

34 

NEFF 

total channel-charge (fixed and 
mobile) coefficient (MOS2 only) 

- 

1.0 

5.0 

35 

KF 

flicker noise coefficient 

- 

0.0 

1.0e-26 

36 

AF 

flicker noise exponent 

- 

1.0 

1.2 

37 

FC 

coefficient for forward-bias 
depletion capacitance formula 

- 

0.5 

 

38 

DELTA 

width effect on threshold voltage 
(MOS2 and MOS3) 

- 

0.0 

1.0 

39 

THETA 

mobility modulation (MOS3 only) 

1/V 

0.0 

0.1 

40 

ETA 

static feedback (MOS3 only) 

- 

0.0 

1.0 

41 

KAPPA 

saturation field factor (MOS3 only) 

- 

0.2 

0.5 

42 

TNOM 

parameter measurement temperature 

C 

27 

50 

The level 4 and level 5 (BSIM1 and BSIM2) parameters are all values obtained from process characterization, and can be generated automatically. J. Pierret [4] describes a means of generating a 'process' file, and the program Proc2Mod provided with SPICE3 converts this file into a sequence of BSIM1 ".MODEL" lines suitable for inclusion in a SPICE input file. Parameters marked below with an * in the l/w column also have corresponding parameters with a length and width dependency. For example, VFB is the basic parameter with units of Volts, and LVFB and WVFB also exist and have units of Volt- meter The formula

is used to evaluate the parameter for the actual device specified with

and

Note that unlike the other models in SPICE, the BSIM model is designed for use with a process characterization system that provides all the parameters, thus there are no defaults for the parameters, and leaving one out is considered an error. For an example set of parameters and the format of a process file, see the SPICE2 implementation notes[3].

For more information on BSIM2, see reference [5].
 

SPICE BSIM (level 4) parameters:

name

parameter

units

l/w

VFB 

flat-band voltage 

V 

* 

PHI 

surface inversion potential 

V 

* 

K1 

body effect coefficient 

V^1/2 

* 

K2 

drain/source depletion charge-sharing coefficient 

- 

* 

ETA 

zero-bias drain-induced barrier-lowering coefficient 

- 

* 

MUZ 

zero-bias mobility 

cm²/V-s 

 

DL 

shortening of channel 

m 

 

DW 

narrowing of channel 

m 

 

U0 

zero-bias transverse-field mobility degradation coefficient 

V^-1 

* 

U1 

zero-bias velocity saturation coefficient 

m/V 

* 

X2MZ 

sens. of mobility to substrate bias at v_ds=0 

cm²/V²-s 

* 

X2E 

sens. of drain-induced barrier lowering effect to substrate bias 

V^-1 

* 

X3E 

sens. of drain-induced barrier lowering effect to drain bias at V_ds=V_dd 

V^-1 

* 

X2U0 

sens. of transverse field mobility degradation effect to substrate bias 

V^-2 

* 

X2U1 

sens. of velocity saturation effect to substrate bias 

mV^-2 

* 

MUS 

mobility at zero substrate bias and at V_ds=V_dd 

cm²/V²-s 

 

X2MS 

sens. of mobility to substrate bias at V_ds=V_dd 

cm²/V²-s 

* 

X3MS 

sens. of mobility to drain bias at V_ds=V_dd 

cm²/V²-s 

* 

X3U1 

sens. of velocity saturation effect on drain bias at V_ds=V_dd 

mV^-2 

* 

TOX 

gate oxide thickness 

m 

 

TEMP 

temperature at which parameters were measured 

C 

 

VDD 

measurement bias range 

V 

 

CGDO 

gate-drain overlap capacitance per meter channel width 

F/m 

 

CGSO 

gate-source overlap capacitance per meter channel width 

F/m 

 

CGBO 

gate-bulk overlap capacitance per meter channel length 

F/m 

 

XPART 

gate-oxide capacitance-charge model flag 

- 

 

N0 

zero-bias subthreshold slope coefficient 

- 

* 

NB 

sens. of subthreshold slope to substrate bias 

- 

* 

ND 

sens. of subthreshold slope to drain bias 

- 

* 

RSH 

drain and source diffusion sheet resistance 

/q 

 

JS 

source drain junction current density 

A/m² 

 

PB 

built in potential of source drain junction 

V 

 

MJ 

Grading coefficient of source drain junction 

- 

 

PBSW 

built in potential of source, drain junction sidewall 

V 

 

MJSW 

grading coefficient of source drain junction sidewall 

- 

 

CJ 

Source drain junction capacitance per unit area 

F/m² 

 

CJSW 

source drain junction sidewall capacitance per unit length 

F/m 

 

WDF 

source drain junction default width 

m 

 

DELL 

Source drain junction length reduction 

m 

 

XPART = 0 selects a 40/60 drain/source charge partition in saturation, while XPART=1 selects a 0/100 drain/source charge partition.

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 control line, when a transient analysis is desired starting from other than the quiescent operating point. See the .IC control line for a better way to set initial conditions.

MESFETs

General form:

ZXXXXXXX ND NG NS MNAME <AREA> <OFF> <IC=VDS, VGS>

Examples:

Z1 7 2 3 ZM1 OFF

MESFET Models (NMF/PMF)

The MESFET model is derived from the GaAs FET model of Statz et al. as described in [11]. The dc characteristics are defined by the parameters VTO, B, and BETA, which determine the variation of drain current with gate voltage, ALPHA, which determines saturation voltage, and LAMBDA, which determines the output conductance. The formula are given by:

Two ohmic resistances, RD and RS, are included. Charge storage is modeled by total gate charge as a function of gate-drain and gate-source voltages and is defined by the parameters CGS, CGD, and PB.
 

 

name

parameter

units

default

example

area

1 

VTO 

pinch-off voltage

V 

-2.0 

-2.0 

 

2 

BETA 

transconductance parameter

A/V² 

1.0e-4

1.0e-3

* 

3 

B 

doping tail extending parameter

1/V 

0.3 

0.3 

* 

4 

ALPHA 

saturation voltage parameter

1/V 

2 

2 

* 

5 

LAMBDA 

channel-length modulation parameter

1/V 

0 

1.0e-4

 

6 

RD 

drain ohmic resistance

 

0 

100 

* 

7 

RS 

source ohmic resistance

 

0 

100 

* 

8 

CGS 

zero-bias G-S junction capacitance

F 

0 

5pF 

* 

9 

CGD 

zero-bias G-D junction capacitance

F 

0 

1pF 

* 

10 

PB 

gate junction potential

V 

1 

0.6 

 

11 

KF 

flicker noise coefficient

- 

0 

 

 

12 

AF 

flicker noise exponent

- 

1 

 

 

13 

FC 

coefficient for forward-bias  
depletion capacitance formula 

- 

0.5 

 

 

 

5.           INTERACTIVE INTERPRETER

Spice3 consists of a simulator and a front-end for data analysis and plotting. The front-end may be run as a separate "stand-alone" program under the name Nutmeg.

Nutmeg will read in the "raw" data output file created by spice -r or with the write command in an interactive Spice3 session. Nutmeg or interactive Spice3 can plot data from a simulation on a graphics terminal or a workstation display. Most of the commands available in the interactive Spice3 front end are available in nutmeg; where this is not the case, Spice-only commands have been marked with an asterisk ("*"). Note that the raw output file is different from the data that Spice2 writes to the standard output, which may also be produced by spice3 with the "-b" command line option.

Spice and Nutmeg use the X Window System for plotting if they find the environment variable DISPLAY. Otherwise, a graphics-terminal independent interface (MFB) is used. If you are using X on a workstation, the DISPLAY variable should already be set; if you want to display graphics on a system different from the one you are running Spice3 or Nutmeg on, DISPLAY should be of the form "machine:0.0". See the appropriate documentation on the X Window Sytem for more details.

Command Synopsis

spice [ -n ] [ -t term ] [ -r rawfile] [ -b ] [ -i ] [ input file ... ]

nutmeg [ - ] [ -n ] [ -t term ] [ datafile ... ]

Options are:

·  - Don't try to load the default data file ("rawspice.raw") if no other files are given. Nutmeg only.
 

·  -n (or -N)

Don't try to source the file ".spiceinit" upon startup. Normally spice and nutmeg try to find the file in the current directory, and if it is not found then in the user's home directory.

·  -t term (or -T term)

The program is being run on a terminal with mfb name term.

·  -b (or -B)

Run in batch mode. Spice3 reads the default input source (e.g. keyboard) or reads the given input file and performs the analyses specified; output is either Spice2-like line-printer plots ("ascii plots") or a spice rawfile. See the following section for details. Note that if the input source is not a terminal (e.g. using the IO redirection notation of "<") Spice3 defaults to batch mode (-i overrides). This option is valid for Spice3 only.

·  -s (or -S)

Run in server mode. This is like batch mode, except that a temporary rawfile is used and then written to the standard output, preceded by a line with a single "@", after the simulation is done. This mode is used by the spice daemon. This option is valid for Spice3 only.

·  -i (or -I)

Run in interactive mode. This is useful if the standard input is not a terminal but interactive mode is desired. Command completion is not available unless the standard input is a terminal, however. This option is valid for Spice3 only.

·  -r rawfile (or -P rawfile)

Use rawfile as the default file into which the results of the simulation are saved. This option is valid for Spice3 only.

Further arguments to spice are taken to be Spice3 input files, which are read and saved (if running in batch mode then they are run immediately). Spice3 accepts most Spice2 input file, and output ascii plots, fourier analyses, and node printouts as specified in .plot, .four, and .print cards. If an out parameter is given on a .width card, the effect is the same as set width = .... Since Spice3 ascii plots do not use multiple ranges, however, if vectors together on a .plot card have different ranges they are not provide as much information as they would in Spice2. The output of Spice3 is also much less verbose than Spice2, in that the only data printed is that requested by the above cards.

For nutmeg, further arguments are taken to be data files in binary or ascii format (see sconvert(1)) which are loaded into nutmeg. If the file is in binary format, it may be only partially completed (useful for examining Spice2 output before the simulation is finished). One file may contain any number of data sets from different analyses.

EXPRESSIONS, FUNCTIONS, AND CONSTANTS

Spice and Nutmeg data is in the form of vectors: time, voltage, etc. Each vector has a type, and vectors can be operated on and combined algebraicly in ways consistent with their types. Vectors are normally created when a data file is read in (see the load command below), and when the initial datafile is loaded. They can also be created with the let command.

An expression is an algebraic formula involving vectors and scalars (a scalar is a vector of length 1) and the following operations:

+ - * / ^ %

% is the modulo operator, and the comma operator has two meanings: if it is present in the argument list of a user-definable function, it serves to separate the arguments. Otherwise, the term x , y is synonymous with x + j(y).

Also available are the logical operations & (and), | (or), ! (not), and the relational operations <, >, >=, <=, =, and <> (not equal). If used in an algebraic expression they work like they would in C, producing values of 0 or 1. The relational operators have the following synonyms:

gt >
lt <
ge >=
le <=
ne <>
eq //&=
and &
or |
not !

These are useful when < and > might be confused with IO redirection (which is almost always).

The following functions are available:

mag(vector) 

The magnitude of vector 

ph(vector) 

The phase of vector 

j(vector) 

i (sqrt(-1)) times vector 

real(vector) 

The real component of vector 

imag(vector) 

The imaginary part of vector 

db(vector) 

20 log10(mag(vector)) 

log(vector) 

The logarithm (base 10) of vector 

ln(vector) 

The natural logarithm (base e) of vector 

exp(vector) 

e to the vector power 

abs(vector) 

The absolute value of vector. 

sqrt(vector) 

The square root of vector. 

sin(vector) 

The sine of vector. 

cos(vector) 

The cosine of vector. 

tan(vector) 

The tangent of vector. 

atan(vector) 

The inverse tangent of vector. 

norm(vector) 

The vector normalized to 1( i.e,the largest magnitude of any componentis 1) 

rnd(vector) 

A vector with each component a random integer between 0 and the absolute value of the vectors's corresponding component. 

mean(vector) 

The result is a scalar (a length 1 vector)that is the mean of the elements of vector. 

vector(number) 

The result is a vector of length number, with elements 0, 1, ... number - 1. If number is a vector then just the first element is taken, and if it isn't an integer then the floor of the magnitude is used. 

lenght(vector) 

The length of vector. 

interpolate(plot.vector) 

The result of interpolating the named vector onto the scale of the current plot. This function uses the variable polydegree to determine the degree of interpolation. 

deriv(vector) 

Calculates the derivative of the given vector. 
This uses numeric differentiation by interpolating a polynomial and may not produce satisfactory results (particularly with iterated differentiation).The implementation only caculates the dirivative with respect to the real componant of that vector's scale. 

 

A vector may be either the name of a vector already defined or a floating-point number (a scalar). A number may be written in any format acceptable to SPICE, such as 14.6Meg or -1.231e-4. Note that you can either use scientific notation or one of the abbreviations like MEG or G, but not both. As with SPICE, a number may have trailing alphabetic characters after it.

The notation expr [num] denotes the num'th element of expr. For multi-dimensional vectors, a vector of one less dimension is returned. Also for multi-dimensional vectors, the notation expr[m][n] will return the nth element of the mth subvector. To get a subrange of a vector, use the form expr[lower, upper].

To reference vectors in a plot that is not the current plot (see the setplot command, below), the notation plotname.vecname can be used.

Either a plotname or a vector name may be the wildcard all. If the plotname is all, matching vectors from all plots are specified, and if the vector name is all, all vectors in the specified plots are referenced. Note that you may not use binary operations on expressions involving wildcards it is not obvious what all + all should denote, for instance. Thus some (contrived) examples of expressions are:

cos(TIME) + db(v(3))
sin(cos(log([1 2 3 4 5 6 7 8 9 10])))
TIME * rnd(v(9)) - 15 * cos(vin#branch) ^ [7.9e5 8]
not ((ac3.FREQ[32] & tran1.TIME[10]) gt 3)

Vector names in spice may have a name such as @name[param], where name is either the name of a device instance or model. This denotes the value of the param parameter of the device or model. See Appendix B for details of what parameters are available. The value is a vector of length 1. This function is also available with the show command, and is available with variables for convenience for command scripts.

There are a number of pre-defined constants in nutmeg. They are:

pi 

(3.14159...) 

e 

The base of natural logarithms (2.71828...) 

c 

The speed of light (299,792,500 m/sec) 

i 

The square root of -1 

kelvin 

Absolute 0 in Centigrade (-273.15  C) 

echarge 

The charge on an electron (1.6021918e-19 C) 

boltz 

Boltzman's constant (1.3806226e-23) 

planck 

Planck's constant (h = 6.626200e-34) 

These are all in MKS units. If you have another variable with a name that conflicts with one of these then it takes precedence.

COMMAND INTERPRETATION

If a word is typed as a command, and there is no built-in command with that name, the directories in the sourcepath list are searched in order for the file. If it is found, it is read in as a command file (as if it were sourced). Before it is read, however, the variables argc and argv are set to the number of words following the filename on the command line, and a list of those words respectively. After the file is finished, these variables are unset. Note that if a command file calls another, it must save its argv and argc since they are altered. Also, command files may not be re-entrant since there are no local variables. (Of course, the procedures may explicitly manipulate a stack...) This way one can write scripts analogous to shell scripts for nutmeg and Spice3.

Note that for the script to work with Spice3, it must begin with a blank line (or whatever else, since it is thrown away) and then a line with .control on it. This is an unfortunate result of the source command being used for both circuit input and command file execution. Note also that this allows the user to merely type the name of a circuit file as a command and it is automatically run. The commands are executed immediately, without running any analyses that may be spicified in the circuit (to execute the analyses before the script executes, include a "run" command in the script).

There are various command scripts installed in /usr/local/lib/spice/scripts (or whatever the path is on your machine), and the default sourcepath includes this directory, so you can use these command files (almost) like builtin commands.

COMMANDS

Ac*: Perform an AC, small-signal frequency response analysis

General Form

ac ( DEC | OCT | LIN ) N Fstart Fstop

Do an ac analysis. See the previous sections of this manual for more details.

Alias: Create an alias for a command

General Form

alias [word] [text ...]

Causes word to be aliased to text. History substitutions may be used, as in C-shell aliases.

Alter*: Change a device or model parameter

General Form

alter device value alter device parameter value [ parameter value ]

Alter changes the value for a device or a specified parameter of a device or model. The first form is used by simple devices which have one principal value (resistors, capacitors, etc.) where the second form is for more complex devices (bjt's, etc.). Model parameters can be changed with the second form if the name contains a "#".

For specifying vectors as values, start the vector with "[", followed by the values in the vector, and end with "]". Be sure to place a space between each of the values and before and after the "[" and "]".

Asciiplot: Plot values using old-style character plots

General Form

asciiplot plotargs

Produce a line printer plot of the vectors. The plot is sent to the standard output, so you can put it into a file with asciiplot args ... > file. The set options width, height, and nobreak determine the width and height of the plot, and whether there are page breaks, respectively. Note that you will have problems if you try to asciiplot something with an X-scale that isn't monotonic (i.e, something like sin(TIME) ), because asciiplot uses a simple-minded linear interpolation.

Aspice: Asynchronous spice run

General Form

aspice input-file [output-file]

Start a SPICE-3 run, and when it is finished load the resulting data. The raw data is kept in a temporary file. If output-file is specified then the diagnostic output is directed into that file, otherwise it is thrown away.

Bug: Mail a bug report

General Form

bug

Send a bug report. Please include a short summary of the problem, the version number and name of the operating system that you are running, the version of Spice that you are running, and the relevant spice input file. (If you have defined BUGADDR, the mail is delivered to there.)

Cd: Change directory

General Form

cd [directory]

Change the current working directory to directory, or to the user's home directory if none is given.

Destroy: Delete a data set

General Form

destroy [plotnames | all]

Release the memory holding the data for the specified runs.

Dc*: Perform a DC-sweep analysis

General Form

dc Source-Name Vstart Vstop Vincr [ Source2 Vstart2 Vstop2 Vincr2 ]

Do a dc transfer curve analysis. See the previous sections of this manual for more details.

Define: Define a function

General Form

define function(arg1, arg2, ...) expression

Define the user-definable function with the name function and arguments arg1, arg2, ... to be expression, which may involve the arguments. When the function is later used, the arguments it is given are substituted for the formal arguments when it is parsed. If expression is not present, any definition for function is printed, and if there are no arguments to define then all currently active definitions are printed. Note that you may have different functions defined with the same name but different arities.

Some useful definitions are:

define max(x,y) (x > y) * x + (x <= y) * y define min(x,y) (x < y) * x + (x >= y) * y

 

Delete*: Remove a trace or breakpoint

General Form

delete [ debug-number ... ]

Delete the specified breakpoints and traces. The debug numbers are those shown by the status command (unless you do status > file, in which case the debug numbers are not printed).

Diff: Compare vectors

General Form

diff plot1 plot2 [vec ...]

Compare all the vectors in the specified plots, or only the named vectors if any are given. There are different vectors in the two plots, or any values in the vectors differ significantly the difference is reported. The variable diff_abstol, diff_reltol, and diff_vntol are used to determine a significant difference.

Display: List known vectors and types

General Form

display [varname ...]

Prints a summary of currently defined vectors, or of the names specified. The vectors are sorted by name unless the variable nosort is set. The information given is the name of the vector, the length, the type of the vector, and whether it is real or complex data. Additionally, one vector is labeled [scale]. When a command such as plot is given without a vs argument, this scale is used for the X-axis. It is always the first vector in a rawfile, or the first vector defined in a new plot. If you undefine the scale (i.e, let TIME = []), one of the remaining vectors becomes the new scale (which is undetermined).

Echo: Print text

General Form

echo [text...]

Echos the given text to the screen.

Edit*: Edit the current circuit

General Form

edit [ file ]

Print the current Spice3 input file into a file, call up the editor on that file and allow the user to modify it, and then read it back in, replacing the original file. If a filename is given, then edit that file and load it, making the circuit the current one.

Fourier: Perform a fourier transform

General Form

fourier fundamental_frequency [value ...]

Does a fourier analysis of each of the given values, using the first 10 multiples of the fundamental frequency (or the first nfreqs, if that variable is set see below). The output is like that of the .four Spice3 line. The values may be any valid expression. The values are interpolated onto a fixed-space grid with the number of points given by the fourgridsize variable, or 200 if it is not set. The interpolation is of degree polydegree if that variable is set, or 1. If polydegree is 0, then no interpolation is done. This is likely to give erroneous results if the time scale is not monotonic, though.

Hardcopy: Save a plot to a file for printing

General Form

hardcopy file plotargs

Just like plot, except creates a file called file containing the plot. The file is an image in plot(5) format, and can be printed by either the plot(1) program or lpr with the -g flag.

Help: Print summaries of Spice3 commands

General Form

help [all] [command ...]

Prints help. If the argument all is given, a short description of everything you could possibly type is printed. If commands are given, descriptions of those commands are printed. Otherwise help for only a few major commands is printed.

History: Review previous commands

General Form

history [number]

Print out the history, or the last number commands typed at the keyboard. Note: in Spice3 version 3a7 and earlier, all commands (including ones read from files) were saved.

Iplot*: Incremental plot

General Form

iplot [ node ...]

Incrementally plot the values of the nodes while Spice3 runs. The iplot command can be used with the where command to find trouble spots in a transient simulation.

Jobs: List active asynchronous spice runs

General Form

jobs

Report on the asynchronous SPICE-3 jobs currently running. Nutmeg checks to see if the jobs are finished every time you execute a command. If it is done then the data is loaded and becomes available.

Let: Assign a value to a vector

General Form

let name = expr

Creates a new vector called name with the value specified by expr, an expression as described above. If expr is [] (a zero-length vector) then the vector becomes undefined. Individual elements of a vector may be modified by appending a subscript to name (ex. name[0]). If there are no arguments, let is the same as display.

Linearize*: Interpolate to a linear scale

General Form

linearize vec ...

Create a new plot with all of the vectors in the current plot, or only those mentioned if arguments are given. The new vectors are interpolated onto a linear time scale, which is determined by the values of tstep, tstart, and tstop in the currently active transient analysis. The currently loaded input file must include a transient analysis (a tran command may be run interactively before the last reset, alternately), and the current plot must be from this transient analysis. This command is needed because Spice3 doesn't output the results from a transient analysis in the same manner that Spice2 did.

Listing*: Print a listing of the current circuit

General Form

listing [logical] [physical] [deck] [expand]

If the logical argument is given, the listing is with all continuation lines collapsed into one line, and if the physical argument is given the lines are printed out as they were found in the file. The default is logical. A deck listing is just like the physical listing, except without the line numbers it recreates the input file verbatim (except that it does not preserve case). If the word expand is present, the circuit is printed with all subcircuits expanded.

Load: Load rawfile data

General Form

load [filename] ...

Loads either binary or ascii format rawfile data from the files named. The default filename is rawspice.raw, or the argument to the -r flag if there was one.

Op*: Perform an operating point analysis

General Form

op

Do an operating point analysis. See the previous sections of this manual for more details.

Plot: Plot values on the display

General Form

plot exprs [ylimit ylo yhi] [xlimit xlo xhi] [xindices xilo xihi] [xcompress comp] [xdelta xdel] [ydelta ydel] [xlog] [ylog] [loglog] [vs xname] [xlabel word] [ylabel word] [title word] [samep] [linear]

Plot the given exprs on the screen (if you are on a graphics terminal). The xlimit and ylimit arguments determine the high and low x- and y-limits of the axes, respectively. The xindices arguments determine what range of points are to be plotted everything between the xilo'th point and the xihi'th point is plotted. The xcompress argument specifies that only one out of every comp points should be plotted. If an xdelta or a ydelta parameter is present, it specifies the spacing between grid lines on the X- and Y-axis. These parameter names may be abbreviated to xl, yl, xind, xcomp, xdel, and ydel respectively.

The xname argument is an expression to use as the scale on the x-axis. If xlog or ylog are present then the X or Y scale, respectively, is logarithmic (loglog is the same as specifying both). The xlabel and ylabel arguments cause the specified labels to be used for the X and Y axes, respectively.

If samep is given, the values of the other parameters (other than xname) from the previous plot, hardcopy, or asciiplot command is used unless re-defined on the command line.

The title argument is used in the place of the plot name at the bottom of the graph.

The linear keyword is used to override a default log-scale plot (as in the output for an AC analysis).

Finally, the keyword polar to generate a polar plot. To produce a smith plot, use the keyword smith. Note that the data is transformed, so for smith plots you will see the data transformed by the function (x - 1) / (x + 1). To produce a polar plot with a smith grid but without performing the smith transform, use the keyword smithgrid.

Print: Print values

General Form

print [col] [line] expr ...

Prints the vector described by the expression expr. If the col argument is present, print the vectors named side by side. If line is given, the vectors are printed horizontally. col is the default, unless all the vectors named have a length of one, in which case line is the default. The options width, length, and nobreak are effective for this command (see asciiplot). If the expression is all, all of the vectors available are printed. Thus print col all > file prints everything in the file in SPICE2 format. The scale vector (time, frequency) is always in the first column unless the variable noprintscale is true.

Quit: Leave Spice3 or Nutmeg

General Form

quit

Quit nutmeg or spice.

Rehash: Reset internal hash tables

General Form

rehash

Recalculate the internal hash tables used when looking up UNIX commands, and make all UNIX commands in the user's PATH available for command completion. This is useless unless you have set unixcom first (see above).

Reset*: Reset an analysis

General Form

reset

Throw out any intermediate data in the circuit (e.g, after a breakpoint or after one or more analyses have been done already), and re-parse the input file. The circuit can then be re-run from it's initial state, overriding the affect of any set or alter commands. In Spice-3e and earlier versions this was done automatically by the run command.

Reshape: Alter the dimensionality or dimensions of a vector

General Form

reshape vector vector ... or reshape vector vector ... [ dimension, dimension, ... ] or reshape vector vector ... [ dimension ][ dimension ] ...

This command changes the dimensions of a vector or a set of vectors. The final dimension may be left off and it will be filled in automatically. If no dimensions are specified, then the dimensions of the first vector are copied to the other vectors. An error message of the form 'dimensions of x were inconsistent' can be ignored.

Resume*: Continue a simulation after a stop

General Form

resume

Resume a simulation after a stop or interruption (control-C).

Rspice: Remote spice submission

General Form

rspice input file

Runs a SPICE-3 remotely taking the input file as a SPICE-3 input file, or the current circuit if no argument is given. Nutmeg or Spice3 waits for the job to complete, and passes output from the remote job to the user's standard output. When the job is finished the data is loaded in as with aspice. If the variable rhost is set, nutmeg connects to this host instead of the default remote Spice3 server machine. This command uses the "rsh" command and thereby requires authentication via a ".rhosts" file or other equivalent method. Note that "rsh" refers to the "remote shell" program, which may be "remsh" on your system; to override the default name of "rsh", set the variable remote_shell. If the variable rprogram is set, then rspice uses this as the pathname to the program to run on the remote system.

Note: rspice will not acknowledge elements that have been changed via the "alter" or "altermod" commands.

Run*: Run analysis from the input file

General Form

run [rawfile]

Run the simulation as specified in the input file. If there were any of the control lines .ac, .op, .tran, or .dc, they are executed. The output is put in rawfile if it was given, in addition to being available interactively. In Spice-3e and earlier versions, the input file would be re-read and any affects of the set or alter commands would be reversed. This is no longer the affect.

Rusage: Resource usage

General Form

rusage [resource ...]

Print resource usage statistics. If any resources are given, just print the usage of that resource. Most resources require that a circuit be loaded. Currently valid resources are:

elapse 

The amount of time elapsed since the last rusage elapsed call 

faults 

Number of page faults and context switches (BSD only). 

space 

Data space used. 

time 

CPU time used so far. 

 

temp 

Operating temperature. 

tnom 

Temperature at which device parameters were measured. 

equations 

Circuit Equations 

 

time 

Total Analysis Time 

totiter 

Total iterations 

accept 

Accepted timepoints 

rejected 

Rejected timepoints 

 

loadtime 

Time spent loading the circuit matrix and RHS 

reordertime 

Matrix reordering time 

lutime 

L-U decomposition time 

solvetime 

Matrix solve time 

 

trantime 

Transient analysis time 

tranpoints 

Transient timepoints 

traniter 

Transient iterations 

trancuriters 

Transient iterations for the last time point* 

tranlutime 

Transient L-U decomposition time 

transolvetime 

Transient matrix solve time 

 

everything 

All of the above. 

* listed incorrectly as "Transient iterations per point".

Save*: Save a set of outputs

General Form

save [all | output ...] .save [all | output ...]

Save a set of outputs, discarding the rest. If a node has been mentioned in a save command, it appears in the working plot after a run has completed, or in the rawfile if spice is run in batch mode. If a node is traced or plotted (see below) it is also saved. For backward compatibility, if there are no save commands given, all outputs are saved.

When the keyword "all" appears in the save command, all default values (node voltages and voltage source currents) are saved in addition to any other values listed.

Sens*: Run a sensitivity analysis

General Form

sens output_variable sens output_variable ac ( DEC | OCT | LIN ) N Fstart Fstop

Perform a Sensitivity analysis. output_variable is either a node voltage (ex. "v(1)" or "v(A,out)") or a current through a voltage source (ex. "i(vtest)"). The first form calculates DC sensitivities, the second form calculates AC sensitivies. The output values are in dimensions of change in output per unit change of input (as opposed to percent change in output or per percent change of input).

Set: Set the value of a variable

General Form

set [word] set [word = value] ...

Set the value of word to be value, if it is present. You can set any word to be any value, numeric or string. If no value is given then the value is the boolean 'true'.

The value of word may be inserted into a command by writing $word. If a variable is set to a list of values that are enclosed in parentheses (which must be separated from their values by white space), the value of the variable is the list.

The variables used by nutmeg are listed in the following section.

Setcirc*: Change the current circuit

General Form

setcirc [circuit name]

The current circuit is the one that is used for the simulation commands below. When a circuit is loaded with the source command (see below) it becomes the current circuit.

Setplot: Switch the current set of vectors

General Form

setplot [plotname]

Set the current plot to the plot with the given name, or if no name is given, prompt the user with a menu. (Note that the plots are named as they are loaded, with names like tran1 or op2. These names are shown by the setplot and display commands and are used by diff, below.) If the "New plot" item is selected, the current plot becomes one with no vectors defined.

Note that here the word "plot" refers to a group of vectors that are the result of one SPICE run. When more than one file is loaded in, or more than one plot is present in one file, nutmeg keeps them separate and only shows you the vectors in the current plot.

Settype: Set the type of a vector

General Form

settype type vector ...

Change the type of the named vectors to type. Type names can be found in the manual page for sconvert.

Shell: Call the command interpreter

General Form

shell [ command ]

Call the operating system's command interpreter; execute the specified command or call for interactive use.

Shift: Alter a list variable

General Form

shift [varname] [number]

If varname is the name of a list variable, it is shifted to the left by number elements (i.e, the number leftmost elements are removed). The default varname is argv, and the default number is 1.

Show*: List device state

General Form

show devices [ : parameters ] , ...

Old Form

show -v @device [ [ name ] ]

The show command prints out tables summarizing the operating condition of selected devices (much like the spice2 operation point summary). If device is missing, a default set of devices are listed, if device is a single letter, devices of that type are listed; if device is a subcircuit name (beginning and ending in ":") only devices in that subcircuit are shown (end the name in a double-":" to get devices within sub-subcircuits recursively). The second and third forms may be combined ("letter:subcircuit:") or "letter:subcircuit::") to select a specific type of device from a subcircuit. A device's full name may be specified to list only that device. Finally, devices may be selected by model by using the form "#modelname" or ":subcircuit#modelname" or "letter:subcircuit#modelname".

If no parameters are specified, the values for a standard set of parameters are listed. If the list of parameters contains a "+", the default set of parameters is listed along with any other specified parameters.

For both devices and parameters, the word "all" has the obvious meaning. Note: there must be spaces separating the ":" that divides the device list from the parameter list.

The "old form" (with "-v") prints the data in a older, more verbose pre-spice3f format.

Showmod*: List model parameter values

General Form

showmod models [ : parameters ] , ...

The showmod command operates like the show command (above) but prints out model parameter values. The applicable forms for models are a single letter specifying the device type letter, "letter:subckt:", "modelname", ":subckt:modelname", or "letter:subcircuit:modelname".

Source: Read a Spice3 input file

General Form

source file

For Spice3: Read the Spice3 input file file. Nutmeg and Spice3 commands may be included in the file, and must be enclosed between the lines .control and .endc. These commands are executed immediately after the circuit is loaded, so a control line of ac ... works the same as the corresponding .ac card. The first line in any input file is considered a title line and not parsed but kept as the name of the circuit. The exception to this rule is the file .spiceinit. Thus, a Spice3 command script must begin with a blank line and then with a .control line. Also, any line beginning with the characters *# is considered a control line. This makes it possible to imbed commands in Spice3 input files that are ignored by earlier versions of Spice2

For Nutmeg: Reads commands from the file filename. Lines beginning with the character * are considered comments and ignored.

Status*: Display breakpoint information

General Form

status

Display all of the traces and breakpoints currently in effect.

Step*: Run a fixed number of timepoints

General Form

step [number]

Iterate number times, or once, and then stop.

Stop*: Set a breakpoint

General Form

stop [ after n] [ when value cond value ] ...

Set a breakpoint. The argument after n means stop after n iteration number n, and the argument when value cond value means stop when the first value is in the given relation with the second value, the possible relations being

eq or //&= equal to
ne or <> not equal to
gt or > greater than
lt or < less than
ge or >= greater than or equal to
le or <= less than or equal to

IO redirection is disabled for the stop command, since the relational operations conflict with it (it doesn't produce any output anyway). The values above may be node names in the running circuit, or real values. If more than one condition is given, e.g. stop after 4 when v(1) > 4 when v(2) < 2, the conjunction of the conditions is implied.

Tf*: Run a Transfer Function analysis

General Form

tf output_node input_source

The tf command performs a transfer function analysis, returning the transfer function (output/input), output resistance, and input resistance between the given output node and the given input source. The analysis assumes a small-signal DC (slowly varying) input.

Trace*: Trace nodes

General Form

trace [ node ...]

For every step of an analysis, the value of the node is printed. Several traces may be active at once. Tracing is not applicable for all analyses. To remove a trace, use the delete command.

Tran*: Perform a transient analysis

General Form

tran Tstep Tstop [ Tstart [ Tmax ] ] [ UIC ]

Perform a transient analysis. See the previous sections of this manual for more details.

Transpose: Swap the elements in a multi-dimensional data set

General Form

transpose vector vector ...

This command transposes a multidimensional vector. No analysis in Spice3 produces multidimensional vectors, although the DC transfer curve may be run with two varying sources. You must use the "reshape" command to reform the one-dimensional vectors into two dimensional vectors. In addition, the default scale is incorrect for plotting. You must plot versus the vector corresponding to the second source, but you must also refer only to the first segment of this second source vector. For example (circuit to produce the tranfer characteristic of a MOS transistor):

spice3 > dc vgg 0 5 1 vdd 0 5 1

spice3 > plot i(vdd)

          spice3 > reshape all [6,6]

spice3 > transpose i(vdd) v(drain)

spice3 > plot i(vdd) vs v(drain)[0]

Unalias: Retract an alias

General Form

unalias [word ...]

Removes any aliases present for the words.

Undefine: Retract a definition

General Form

undefine function

Definitions for the named user-defined functions are deleted.

Unset: Clear a variable

General Form

unset [word ...]

Clear the value of the specified variable(s) (word).

Version: Print the version of Spice

General Form

version [version id]

Print out the version of nutmeg that is running. If there are arguments, it checks to make sure that the arguments match the current version of SPICE. (This is mainly used as a Command: line in rawfiles.)

Where: Identify troublesome node or device

General Form

where

When performing a transient or operating point analysis, the name of the last node or device to cause non-convergence is saved. The where command prints out this information so that you can examine the circuit and either correct the problem or make a bug report. You may do this either in the middle of a run or after the simulator has given up on the analysis. For transient simulation, the iplot command can be used to monitor the progress of the analysis. When the analysis slows down severly or hangs, interrupt the simulator (with control-C) and issue the where command. Note that only one node or device is printed; there may be problems with more than one node.

Write: Write data to a file

General Form

write [file] [exprs]

Writes out the expressions to file.

First vectors are grouped together by plots, and written out as such (i.e, if the expression list contained three vectors from one plot and two from another, then two plots are written, one with three vectors and one with two). Additionally, if the scale for a vector isn't present, it is automatically written out as well.

The default format is ascii, but this can be changed with the set filetype command. The default filename is rawspice.raw, or the argument to the -r flag on the command line, if there was one, and the default expression list is all.

Xgraph: use the xgraph(1) program for plotting.

General Form

xgraph file [exprs] [plot options]

The spice3/nutmeg xgraph command plots data like the plot command but via xgraph, a popular X11 plotting program.

If file is either "temp" or "tmp" a temporary file is used to hold the data while being plotted. For available plot options, see the plot command. All options except for polar or smith plots are supported.

CONTROL STRUCTURES

While End

General Form

while condition statement ... end

While condition, an arbitrary algebraic expression, is true, execute the statements.

Repeat End

General Form

repeat [number] statement ... end

Execute the statements number times, or forever if no argument is given.

Dowhile End

General Form

dowhile condition statement ... end

The same as while, except that the condition is tested after the statements are executed.

Foreach End

General Form

foreach var value ... statement ... end

The statements are executed once for each of the values, each time with the variable var set to the current one. (var can be accessed by the $var notation see below).

If Then Else

General Form

if condition statement ... else statement ... end

If the condition is non-zero then the first set of statements are executed, otherwise the second set. The else and the second set of statements may be omitted.

Label

General Form

label word

If a statement of the form goto word is encountered, control is transferred to this point, otherwise this is a no-op.

Goto

General Form

goto word

If a statement of the form label word is present in the block or an enclosing block, control is transferred there. Note that if the label is at the top level, it must be before the goto statement (i.e, a forward goto may occur only within a block).

Continue

General Form

continue

If there is a while, dowhile, or foreach block enclosing this statement, control passes to the test, or in the case of foreach, the next value is taken. Otherwise an error results.

Break

General Form

break

If there is a while, dowhile, or foreach block enclosing this statement, control passes out of the block. Otherwise an error results.

Of course, control structures may be nested. When a block is entered and the input is the terminal, the prompt becomes a number of >'s corresponding to the number of blocks the user has entered. The current control structures may be examined with the debugging command cdump.

VARIABLES

The operation of both Nutmeg and Spice3 may be affected by setting variables with the "set" command. In addition to the variables mentioned below, the set command in Spice3 also affect the behaviour of the simulator via the options previously described under the section on ".OPTIONS".

The variables meaningful to nutmeg which may be altered by the set command are:
 
 

diff_abstol 

he absolute tolerance used by the diff command. 

appendwrite 

Append to the file when a write command is issued, if one already exists. 

colorN 

These variables determine the colors used, if X is being run on a color display.IN may be between 0 and 15. Color 0 is the background, color 1 is the grid and text color, and colors 2 through 15 are used in order for vectors plotted. The value of the color variables should be names of colors, which may be found in the file /usr/lib/rgb.txt. 

combplot 

Plot vectors by drawing a vertical line from each point to the X-axis, as opposed to joining the points.Note that this option is subsumed in the plottype option, below. 

cpdebug 

Print cshpar debugging information (must be complied with the -DCPDEBUG flag). Unsupported in the current release 

debug 

If set then a lot of debugging information is printed (must be compiled with the -DFTEDEBUG flag).Unsupported in the current release. 

device 

The name (/dev/tty??) of the graphics device.If this variable isn't set then the user's terminal is used.To do plotting onanother monitor you probably have to set both the device and term variables.(If device is set to the name of a file, nutmeg dumps the graphics control codes into this file -- this is useful for saving plots.) 

echo 

Print out each command before it is executed. 

filetype 

This can be either ascii or binary, and determines what format rawfiles are. The default is ascii. 

fourgridsize 

How many points to use for interpolating into when doing fourier analysis. 

gridsize 

If this variable is set to an integer, this number is used as the number of equally spaced points to use for the Y-axis when plotting. Otherwise the current scale is used (which may not have equally spaced points). If the current scale isn't strictly monotonic, then this option has no effect. 

hcopydev 

If this is set, when the hardcopy command is run the resulting file is automatically printed on the printer named hcopydev with the command lpr -Phcopydev -g file. 

hcopyfont 

This variable specifies the font name for hardcopy output plots. The value is device dependent. 

hcopyfontsize 

This is a scaling factor for the font used in hardcopy plots. 

hcopydevtype 

This variable specifies the type of the printer output to use in the hardcopy command. If hcopydevtype is not set, plot (5) format is assumed. The standard distribution currently recognizes postscript as an alternative output format. When used in conjunction with hcopydev, hcopydevtype should specify a format supported by 
the printer. 

hcopyfontsize 

This is a scaling factor for the font used in hardcopy plots. 

hcopydevtype 

This variable specifies the type of the printer output to use in the hardcopy command. If hcopydevtype is not set, plot (5) format is assumed. The standard distribution currently recognizes postscript as an alternative output format. When used in conjunction with hcopydev, hcopydevtype should specify a format supported by 
the printer. 

height 

The length of the page for asciiplot and print col. 

history 

The number of events to save in the history list. 

lprplot5 

This is a printf(3s) style format string used to specify the command to use for sending plot(5)-style plots to a printer or plotter. The first parameter supplied is the printer name, the second parameter supplied is a file name containing the plot. Both parameters are strings. It is trivial to cause Spice3 to abort by supplying a unreasonable format string. 

lprps 

This is a printf(3s) style format string used to specify the command to use for sending PostScript plots to a printer or plotter. The first parameter supplied is the printer name, the second parameter 
supplied is a file name containing the plot. Both parameters are strings. It is trivial to cause Spice3 to abort by supplying a unreasonable format 
string. 

nfreqs 

The number of frequencies to compute in the fourier command. (Defaults to 10.) 

nobreak 

Don't have asciiplot and print col break between pages. 

noasciiplotvalue 

Don't print the first vector plotted to the left when doing an asciiplot. 

noclobber 

Don't overwrite existing files when doing IO redirection. 

noglob 

Don't expand the global characters `*', `?', `[', `and `]'. This is the default. 

nogrid 

Don't plot a grid when graphing curves (but do label the axes). 

nomoremode 

If nomoremode is not set, whenever a large amount of data is being printed to the screen (e.g, the print or asciiplot commands), the output is stopped every screenful and continues when a carriage return is typed. If nomoremode is set then data scrolls off the screen without check. 

nonomatch 

If noglob is unset and a global expression cannot be matched, use the global characters literally instead of complaining. 

nosort 

Don't have display sort the variable names. 

noprintscale 

Don't print the scale in the leftmost column when a print col command is given. 

numdgt 

The number of digits to print when printing tables of data (fourier, print col). The default precision is 6 digits. On the VAX, approximately 16 decimal digits are available using double precision, so numdgt should not be more than 16. If the number is negative, one fewer digit is printed to ensure constant widths in tables. 

plottype 

This should be one of normal, comb, or point:chars. normal, the default, causes points to be plotted as parts of connected lines. comb causes a comb plot to be done (see the description of the combplot variable above). point causes each point to be plotted separately - the chars are a list of characters that are used for each vector plotted. If they are omitted then a default set is used. 

polydegree 

The degree of the polynomial that the plot command should fit to the data. If polydegree is N, then nutmeg fits a degree N polynomial to every set of N points and draw 10 intermediate points in between each endpoint. If the points aren't monotonic, then it tries rotating the curve and reducing the degree until a fit is achieved. 

polysteps 

The number of points to interpolate between every pair of points available when doing curve fitting. 
The default is 10. 

program 

The name of the current program (argv[0]) 

prompt 

The prompt, with the character `!' replaced by the current event number. 

rawfile 

The default name for rawfiles created. 

diff_reltol 

The relative tolerance used by the diff command. 

remote_shell 

Overrides the name used for generating rspice runs (default is "rsh"). 

rhost 

The machine to use for remote SPICE-3 runs, instead of the default one (see the description of the rspice command, below). 

rprogram 

The name of the remote program to use in the rspice command. 

slowplot 

Stop between each graph plotted and wait for the user to type return before continuing. 

sourcepath 

A list of the directories to search when a source command is given. The default is the current directory and the standard spice library (/usr/local/lib/spice, or whatever LIBPATH is #defined to in the Spice3 source. 

spicepath 

The program to use for the aspice command. The default is /cad/bin/spice. 

term 

The mfb name of the current terminal. 

  

units 

If this is degrees, then all the trig functions will use degrees instead of radians. 

unixcom 

If a command isn't defined, try to execute it as a UNIX command. Setting this option has the effect of giving a rehash command, below. This is useful for people who want to use nutmeg as a login shell. 

verbose 

Be verbose. This is midway between echo and debug / cpdebug. 

diff_vntol 

The absolute voltage tolerance used by the diff command. 

 

width 

The width of the page for asciiplot and print col. 

x11lineararcs 

Some X11 implementations have poor arc drawing. If you set this option, Spice3 will plot using an approximation to the curve using straight lines. 

xbrushheight 

The height of the brush to use if X is being run. 

xbrushwidth 

The width of the brush to use if X is being run. 

xfont 

The name of the X font to use when plotting data and entering labels. The plot may not look good if this is a variable-width font. 

 

 

There are several set variables that Spice3 uses but Nutmeg does not. They are:

editor 

The editor to use for the edit command. 

modelcard 

The name of the model card (normally .model). 

noaskquit 

Do not check to make sure that there are no circuits suspended and no plots unsaved. Normally Spice-3 warns the user when he tries to quit if this is the case. 

nobjthack 

Assume that BJTs have 4 nodes. 

noparse 

Don't attempt to parse input files when they are read in (useful for debugging). Of course, they cannot be run if they are not parsed. 

nosubckt 

Don't expand subcircuits 

renumber 

Renumber input lines when an input file has .include's. 

subend 

The card to end subcircuits (normally .ends). 

subinvoke 

The prefix to invoke subcircuits (normally x). 

substart 

The card to begin subcircuits (normally .subckt). 

 

MISCELLANEOUS

If there are subcircuits in the input file, Spice3 expands instances of them. A subcircuit is delimited by the cards .subckt and .ends, or whatever the value of the variables substart and subend is, respectively. An instance of a subcircuit is created by specifying a device with type 'x' ' the device line is written

xname node1 node2 ... subcktname

where the nodes are the node names that replace the formal parameters on the .subckt line. All nodes that are not formal parameters are prepended with the name given to the instance and a ':', as are the names of the devices in the subcircuit. If there are several nested subcircuits, node and device names look like subckt1:subckt2:...:name. If the variable subinvoke is set, then it is used as the prefix that specifies instances of subcircuits, instead of 'x'.

Nutmeg occasionally checks to see if it is getting close to running out of space, and warns the user if this is the case. (This is more likely to be useful with the SPICE front end.)

C-shell type quoting with "" and '', and backquote substitution may be used. Within single quotes, no further substitution (like history substitution) is done, and within double quotes, the words are kept together but further substitution is done. Any text between backquotes is replaced by the result of executing the text as a command to the shell.

Tenex-style ('set filec' in the 4.3 C-shell) command, filename, and keyword completion is possible: If EOF (control-D) is typed after the first character on the line, a list of the commands or possible arguments is printed (If it is alone on the line it exits nutmeg). If escape is typed, then nutmeg trys to complete what the user has already typed. To get a list of all commands, the user should type &ltspace;> ^D.

The values of variables may be used in commands by writing $varname where the value of the variable is to appear. The special variables $$ and $< refer to the process ID of the program and a line of input which is read from the terminal when the variable is evaluated, respectively. If a variable has a name of the form $&word;, then word is considered a vector (see above), and its value is taken to be the value of the variable. If $foo is a valid variable, and is of type list, then the expression $foo[low-high] represents a range of elements. Either the upper index or the lower may be left out, and the reverse of a list may be obtained with $foo[len-0]. Also, the notation $?foo evaluates to 1 if the variable foo is defined, 0 otherwise, and $#foo evaluates to the number of elements in foo if it is a list, 1 if it is a number or string, and 0 if it is a boolean variable.

History substitutions, similar to C-shell history substitutions, are also available see the C-shell manual page for all of the details.

The characters ~, {, and } have the same effects as they do in the C-Shell, i.e., home directory and alternative expansion. It is possible to use the wildcard characters *, ?, [, and ] also, but only if you unset noglob first. This makes them rather useless for typing algebraic expressions, so you should set noglob again after you are done with wildcard expansion. Note that the pattern [^abc] matchs all characters except a, b, and c.

IO redirection is available the symbols >, >>, >&, >>&, and < have the same effects as in the C-shell.

You may type multiple commands on one line, separated by semicolons.

If you want to use a different mfbcap file than the default (usually ~cad/lib/mfbcap), you have to set the environment variable SPICE_MFBCAP before you start nutmeg or spice. The -m option and the mfbcap variable no longer work.

If X is being used, the cursor may be positioned at any point on the screen when the window is up and characters typed at the keyboard are added to the window at that point. The window may then be sent to a printer using the xpr(1) program.

Nutmeg can be run under VAX/VMS, as well as several other operating systems. Some features like command completion, expansion of *, ?, and [], backquote substitution, the shell command, and so forth do not work.

On some systems you have to respond to the -more- prompt during plot with a carriage return instead of any key as you can do on UNIX.

BUGS

The label entry facilities are primitive. You must be careful to type slowly when entering labels -- nutmeg checks for input once every second, and can get confused if characters arrive faster.

If you redefine colors after creating a plot window with X, and then cause the window to be redrawn, it does not redraw in the correct colors.

When defining aliases like

alias pdb plot db( '!:1' - '!:2' )

you must be careful to quote the argument list substitutions in this manner. If you quote the whole argument it might not work properly.

In a user-defined function, the arguments cannot be part of a name that uses the plot.vec syntax. For example:

define check(v(1)) cos(tran1.v(1))

does not work.

If you type plot all all, or otherwise use a wildcard reference for one plot twice in a command, the effect is unpredictable.

The asciiplot command doesn't deal with log scales or the delta keywords.

Often the names of terminals recognized by MFB are different from those in /etc/termcap. Thus you may have to reset your terminal type with the command

set term = termname

where termname is the name in the mfbcap file.

The hardcopy command is useless on VMS and other systems without the plot command, unless the user has a program that understands plot(5) format.

Spice3 recognizes all the notations used in SPICE2 .plot cards, and translates vp(1) into ph(v(1)), and so forth. However, if there are spaces in these names it won't work. Hence v(1, 2) and (-.5, .5) aren't recognized.

BJTs can have either 3 or 4 nodes, which makes it difficult for the subcircuit expansion routines to decide what to rename. If the fourth parameter has been declared as a model name, then it is assumed that there are 3 nodes, otherwise it is considered a node. To disable this, you can set the variable "nobjthack" which forces BJTs to have 4 nodes (for the purposes of subcircuit expansion, at least).

The @name[param] notation might not work with trace, iplot, etc. yet.