SPICE Version 2G User's Guide
(10 Aug 1981)
A.Vladimirescu, Kaihe Zhang,
A.R.Newton, D.O.Pederson, A.Sangiovanni-Vincentelli
Department of Electrical Engineering and Computer Sciences
University of California
Berkeley, Ca., 94720



Acknowledgement: Dr. Richard Dowell and Dr. Sally Liu  have  con-
tributed  to develop the present SPICE version.  SPICE was origi-
nally developed by Dr.  Lawrence  Nagel  and  has  been  modified
extensively by Dr. Ellis Cohen.

	SPICE is a general-purpose circuit  simulation  program  for
nonlinear  dc, nonlinear transient, and linear ac analyses.  Cir-
cuits may contain resistors, capacitors, inductors, mutual induc-
tors,  independent  voltage  and  current  sources, four types of
dependent sources, transmission lines, and the four  most  common
semiconductor devices:  diodes, BJT's, JFET's, and MOSFET's.

	SPICE has built-in models for the semiconductor devices, and
the  user need specify only the pertinent model parameter values.
The model for the BJT is based on the integral  charge  model  of
Gummel and Poon;  however, if the Gummel- Poon parameters are not
specified, the model reduces to the simpler Ebers-Moll model.  In
either  case,  charge  storage  effects, ohmic resistances, and a
current-dependent output conductance may be included.  The  diode
model  can be used for either junction diodes or Schottky barrier
diodes.  The JFET model is based on the FET model of Shichman and
Hodges. Three MOSFET models are implemented; MOS1 is described by
a square-law I-V characteristic MOS2 is an analytical model while
MOS3  is  a  semi-empirical  model.   Both  MOS2 and MOS3 include
second-order effects such as channel length modulation, subthres-
hold  conduction,  scattering limited velocity saturation, small-
size effects and charge-controlled capacitances.

          1.  TYPES OF ANALYSIS

          1.1.  DC Analysis

	The dc analysis portion of SPICE determines the dc operating
point  of  the  circuit  with  inductors  shorted  and capacitors
opened.  A dc analysis is  automatically  performed  prior  to  a
transient analysis to determine the transient initial conditions,
and prior to an ac small-signal analysis to determine the linear-
ized,  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 resis-
tance will also be computed as a part of the dc solution.  The dc
analysis  can  also  be  used  to generate dc transfer curves:  a
specified independent voltage or current source is stepped over a
user-specified  range  and the dc output variables are stored for
each sequential source value.   If  requested,  SPICE  also  will
determine  the  dc small-signal sensitivities of specified output
variables with respect to circuit parameters.   The  dc  analysis
options  are  specified  on  the .DC, .TF, .OP, and .SENS control
cards.

	If one desires to see the small-signal models for  nonlinear
devices in conjunction with a transient analysis operating point,
then the .OP card must be provided.  The dc bias conditions  will
be  identical for each case, but the more comprehensive operating
point information is not available to be printed  when  transient
initial conditions are computed.


          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 cir-
cuit.  The resultant linear  circuit  is  then  analyzed  over  a
user-specified range of frequencies.  The desired output of an ac
small- signal analysis is usually a  transfer  function  (voltage
gain,  transimpedance,  etc).   If  the  circuit  has only one ac
input, it is convenient to set  that  input  to  unity  and  zero
phase,  so  that  output  variables  have  the  same value as the
transfer function of the output  variable  with  respect  to  the
input.


     The generation of white noise by resistors and semiconductor
devices can also be simulated with the ac small-signal portion of
SPICE.  Equivalent noise source values are  determined  automati-
cally  from  the small-signal operating point of the circuit, and
the contribution of each noise source is added at a given summing
point.   The  total  output  noise level and the equivalent input
noise level are determined at each frequency point.   The  output
and  input noise levels are normalized with respect to the square
root of the noise bandwidth and have the  units  Volts/rt  Hz  or
Amps/rt  Hz.   The output noise and equivalent input noise can be
 printed or plotted in the same fashion as other output variables.
No additional input data are necessary for this analysis.


     Flicker noise sources can be simulated in the noise analysis
by including values for the parameters KF and AF on the appropri-
ate device model cards.


     The distortion characteristics of a circuit  in  the  small-
signal  mode  can  be  simulated as a part of the ac small-signal
analysis.  The analysis is performed assuming  that  one  or  two
signal frequencies are imposed at the input.


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


1.3.  Transient Analysis


     The transient analysis portion of SPICE computes  the  tran-
sient  output  variables  as  a  function  of  time  over a user-
specified time interval.  The initial  conditions  are  automati-
cally  determined  by  a  dc analysis.  All sources which are not
time dependent (for example, power supplies) are set to their  dc
value.    For  large-signal  sinusoidal  simulations,  a  Fourier
analysis of the output waveform can be specified  to  obtain  the
frequency domain Fourier coefficients.  The transient time inter-
val and the Fourier analysis options are specified on  the  .TRAN
and .FOURIER control lines.


1.4.  Analysis at Different Temperatures

     All input data for SPICE is assumed to have been measured at
27 deg C (300 deg K).  The simulation also assumes a nominal tem-
perature of 27 deg C.  The circuit can be simulated at other tem-
peratures by using a .TEMP control line.
     Temperature appears explicitly in the exponential  terms  of
the  BJT  and  diode  model  equations.   In addition, saturation
currents have a built-in temperature dependence.  The temperature
dependence  of the saturation current in the BJT models is deter-
mined by:


    IS(T1) = IS(T0)*((T1/T0)**XTI)*exp(q*EG*(T1-T0)/(k*T1*T0))

where k is Boltzmann's constant, q is the electronic  charge,  EG
is  the  energy  gap  which  is a model parameter, and XTI is the
saturation current temperature exponent (also a model  parameter,
and  usually  equal to 3).  The temperature dependence of forward
and reverse beta is according to the formula:
     beta(T1)=beta(T0)*(T1/T0)**XTB
where T1 and T0 are in degrees Kelvin, and XTB is a user-supplied
model  parameter.  Temperature effects on beta are carried out by
appropriate adjustment to the values of BF,  ISE,  BR,  and  ISC.
Temperature  dependence of the saturation current in the junction
diode model is determined by:

    IS(T1) = IS(T0)*((T1/T0)**(XTI/N))*exp(q*EG*(T1-T0)/(k*N*T1*T0))

where N is the emission coefficient, which is a model  parameter,
and  the other symbols have the same meaning as above.  Note that
for Schottky barrier diodes, the value of the saturation  current
temperature exponent, XTI, is usually 2.

      Temperature appears explicitly  in  the  value  of  junction
potential,  PHI,  for  all  the  device  models.  The temperature
dependence is determined by:

    PHI(TEMP) = k*TEMP/q*log(Na*Nd/Ni(TEMP)**2)
where k is Boltzmann's constant, q is the electronic  charge,  Na
is  the  acceptor impurity density, Nd is the donor impurity den-
sity, Ni is the intrinsic concentration, and  EG  is  the  energy
gap.

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

    UO(TEMP) = UO(TNOM)/(TEMP/TNOM)**(1.5)

The effects of temperature on resistors is modeled  by  the  for-
mula:

    value(TEMP) = value(TNOM)*(1+TC1*(TEMP-TNOM)+TC2*(TEMP-TNOM)**2))

where TEMP is the circuit temperature, TNOM is the  nominal  tem-
perature,  and  TC1  and TC2 are the first- and second-order tem-
perature coefficients.


2.  CONVERGENCE


     Both dc and transient solutions are obtained by an iterative
 process which is terminated when both of the following conditions
hold:

1)   The nonlinear branch currents converge to within a tolerance
of  0.1  percent  or  1  picoamp (1.0E-12 Amp), whichever is
larger.

2)   The node voltages converge to within a tolerance of 0.1 per-
cent or 1 microvolt (1.0E-6 Volt), whichever is larger.
     Although the algorithm used in SPICE has been  found  to  be
very  reliable, in some cases it will fail to converge to a solu-
tion.  When this failure occurs, the program will print the  node
voltages  at  the  last iteration and terminate the job.  In such
cases, the node voltages that are  printed  are  not  necessarily
correct or even close to the correct solution.
     Failure to converge in the dc analysis is usually due to  an
error in specifying circuit connections, element values, or model
parameter values.  Regenerative switching  circuits  or  circuits
with  positive  feedback  probably  will  not  converge in the dc
analysis unless the OFF option is used for some of the devices in
the feedback path, or the .NODESET card is used to force the cir-
cuit to converge to the desired state.

3.  INPUT FORMAT

     The input format for SPICE  is  of  the  free  format  type.
Fields on a card are separated by one or more blanks, a comma, an
equal (=) sign, or a left or right parenthesis;  extra spaces are
ignored.   A  card  may  be  continued  by entering a + (plus) in
column 1 of the following card;  SPICE continues  reading  begin-
ning with column 2.
     A name field must begin with a letter (A through Z) and can-
not  contain  any delimiters.  Only the first eight characters of
the name are used.
     A number field may be an integer field (12, -44), a floating
point field (3.14159), either an integer or floating point number
followed by an integer exponent (1E-14,  2.65E3),  or  either  an
integer or a floating point number followed by one of the follow-
ing scale factors:
T=1E12   G=1E9    MEG=1E6   K=1E3     MIL=25.4E-6
        M=1E-3   U=1E-6   N=1E-9    P=1E-12   F=1E-15
Letters immediately following a number that are not scale factors
are ignored, and letters immediately following a scale factor are
ignored.  Hence, 10, 10V, 10VOLTS, and  10HZ  all  represent  the
same  number,  and  M, MA, MSEC, and MMHOS all represent the same
scale factor.  Note that 1000, 1000.0, 1000HZ, 1E3, 1.0E3,  1KHZ,
and 1K all represent the same number.


4.  CIRCUIT DESCRIPTION
     The circuit to be analyzed is described to SPICE by a set of
element  cards,  which  define  the  circuit topology and element
values, and a set of control cards, which define the model param-
eters  and  the  run  controls.  The first card in the input deck
must be a title card, and the last card must be a .END card.  The
order  of  the  remaining  cards is arbitrary (except, of course,
that continuation cards must immediately follow  the  card  being
continued).
     Each element in the circuit is specified by an element  card
that  contains  the  element name, the circuit nodes to which the
element is connected, and  the  values  of  the  parameters  that
determine  the  electrical  characteristics  of the element.  The
first letter of the element name specifies the element type.  The
format for the SPICE element types is given in what follows.  The
strings  XXXXXXX,   YYYYYYY,   and   ZZZZZZZ   denote   arbitrary
alphanumeric  strings.   For  example, a resistor name must begin
with the letter R and can contain from one to  eight  characters.
Hence, R, R1, RSE, ROUT, and R3AC2ZY are valid resistor names.
     Data fields that are enclosed in lt and gt signs '<  >'  are
optional.   All  indicated punctuation (parentheses, equal signs,
etc.)  are  required.   With  respect  to  branch  voltages   and
currents,  SPICE  uniformly uses the associated reference conven-
tion (current flows in the direction of voltage drop).
     Nodes must be nonnegative integers but need not be  numbered
sequentially.   The  datum  (ground)  node must be numbered zero.
The circuit cannot contain  a  loop  of  voltage  sources  and/or
inductors  and  cannot contain a cutset of current sources and/or
capacitors.  Each node in the circuit must  have  a  dc  path  to
ground.  Every node must have at least two connections except for
transmission line  nodes  (to  permit  unterminated  transmission
lines)  and  MOSFET substrate nodes (which have two internal con-
nections anyway).

5.  TITLE CARD, COMMENT CARDS AND .END CARD

5.1.  Title Card
Examples:

POWER AMPLIFIER CIRCUIT TEST OF CAM CELL 
     This card must be the first card in  the  input  deck.   Its
contents  are printed verbatim as the heading for each section of
output.

5.2.  .END Card
Examples:

.END

     This card must always be the last card in  the  input  deck.
Note that the period is an integral part of the name.

5.3.  Comment Card
General Form:

* <any comment>

Examples:

* RF=1K      GAIN SHOULD BE 100
* MAY THE FORCE BE WITH MY CIRCUIT

     The asterisk in the first column indicates that this card is
a comment card.  Comment cards may be placed anywhere in the cir-
cuit description.

6.  ELEMENT CARDS

6.1.  Resistors
General form:

RXXXXXXX N1 N2 VALUE <TC=TC1<,TC2>>

Examples:

R1 1 2 100
RC1 12 17 1K TC=0.001,0.015

     N1 and N2 are the two element nodes.  VALUE  is  the  resis-
tance  (in  ohms)  and  may be positive or negative but not zero.
TC1 and TC2 are the (optional) temperature coefficients;  if  not
specified,  zero  is assumed for both.  The value of the resistor
as a function of temperature is given by:

value(TEMP) = value(TNOM)*(1+TC1*(TEMP-TNOM)+TC2*(TEMP-TNOM)**2))

6.2.  Capacitors and Inductors

General form:

CXXXXXXX N+ N- VALUE <IC=INCOND>
LYYYYYYY N+ N- VALUE <IC=INCOND>

Examples:

CBYP 13 0 1UF
COSC 17 23 10U IC=3V
LLINK 42 69 1UH
LSHUNT 23 51 10U IC=15.7MA

     N+ and N- are  the  positive  and  negative  element  nodes,
respectively.   VALUE  is the capacitance in Farads or the induc-
tance in Henries.
     For the capacitor, the (optional) initial condition  is  the
initial  (time-zero)  value of capacitor voltage (in Volts).  For
the inductor, the (optional) initial  condition  is  the  initial
(time-zero)  value  of inductor current (in Amps) that flows from
N+, through the inductor, to N-.  Note that  the  initial  condi-
tions (if any) apply 'only' if the UIC option is specified on the
.TRAN card.

Nonlinear capacitors and inductors can be described.

General form :

CXXXXXXX N+ N- POLY C0 C1 C2 ... <IC=INCOND>
LYYYYYYY N+ N- POLY L0 L1 L2 ... <IC=INCOND>

     C0 C1 C2 ...(and L0 L1 L2 ...) are  the  coefficients  of  a
polynomial  describing  the  element  value.  The  capacitance is
expressed as a function of the voltage across the  element  while
the inductance is a function of the current through the inductor.
The value is computed as

value=C0+C1*V+C2*V**2+...
value=L0+L1*I+L2*I**2+...

     where V is the  voltage  across  the  capacitor  and  I  the
current flowing in the inductor.

6.3.  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 induc-
tor.

6.4.  Transmission Lines (Lossless)

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  transmis-
sion  delay, TD, may be specified directly (as TD=10ns, for exam-
ple).  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  fre-
quency).   Note  that although both forms for expressing the line
length are indicated as optional, one of the two must  be  speci-
fied.

     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 Appendix A for
further clarification.)
     The (optional) initial condition specification  consists  of
the  voltage  and current at each of the transmission line ports.
Note that the initial conditions (if any) apply 'only' if the UIC
option is specified on the .TRAN card.
     One should be aware that SPICE will use  a  transient  time-
step  which  does  not  exceed  1/2 the minimum transmission line
delay.  Therefore very short transmission  lines  (compared  with
the analysis time frame) will cause long run times.

6.5.  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.
Note:  a more complete description of dependent sources as imple-
mented in SPICE is given in Appendix B.

6.6.  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).

6.7.  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, respec-
tively.  VALUE is the voltage gain.

6.8.  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.

6.9.  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 control-
ling  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).

6.10.  Independent Sources

General form:

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

Examples:

VCC 10 0 DC 6
VIN 13 2 0.001 AC 1 SIN(0 1 1MEG)
ISRC 23 21 AC 0.333 45.0 SFFM(0 1 10K 5 1K)
VMEAS 12 9

     N+ and N- are the positive and negative nodes, respectively.
Note that voltage sources need not be grounded.  Positive current
is assumed to flow from the positive node, through the source, to
the  negative  node.   A  current  source of positive value, will
force current to flow out of the N+ node, through the source, and
into the N- node.  Voltage sources, in addition to being used for
circuit excitation, are the 'ammeters' for SPICE, that  is,  zero
valued  voltage  sources may be inserted into the circuit for the
purpose of measuring current.  They  will,  of  course,  have  no
effect on circuit operation since they represent short-circuits.
DC/TRAN is the  dc  and  transient  analysis  value  of  the
source.   If  the  source value is zero both for dc and transient
analyses, this value may be omitted.   If  the  source  value  is
time-invariant (e.g., a power supply), then the value may option-
ally be preceded by the letters DC.
     ACMAG is the ac magnitude and ACPHASE is the ac phase.   The
source  is  set  to  this  value in the ac analysis.  If ACMAG is
omitted following the keyword AC, a value of  unity  is  assumed.
If ACPHASE is omitted, a value of zero is assumed.  If the source
is not an ac small-signal input, the keyword AC and the ac values
are omitted.
     Any independent source  can  be  assigned  a  time-dependent
value  for  transient  analysis.  If a source is assigned a 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 will be assumed.  (TSTEP is the printing
increment  and  TSTOP  is  the final time (see the .TRAN card for
explanation)).

1.  Pulse         PULSE(V1 V2 TD TR TF PW PER)

Examples:

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

parameters              default values         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+TF   V1
TSTOP         V1

Intermediate points are determined by linear interpolation.

2.  Sinusoidal    SIN(VO VA FREQ TD THETA)

Examples:

VIN 3 0 SIN(0 1 100MEG 1NS 1E10)

parameters                default value   units
VO     (offset)                           Volts or Amps
VA     (amplitude)                        Volts or Amps
FREQ   (frequency)        1/TSTOP         Hz
TD     (delay)            0.0             seconds
THETA  (damping factor)   0.0             1/seconds

     The shape of the waveform  is  described  by  the  following
table:
time          value
0 to TD       VO
TD to TSTOP   VO + VA*exp(-(time-TD)*THETA)*sine(twopi*FREQ*(time+TD))

3.  Exponential  EXP(V1 V2 TD1 TAU1 TD2 TAU2)

Examples:

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

parameters                  default values   units

V1   (initial value)                         Volts or Amps
V2   (pulsed value)                          Volts or Amps
TD1  (rise delay time)      0.0              seconds
TAU1 (rise time constant)   TSTEP            seconds
TD2  (fall delay time)      TD1+TSTEP        seconds
TAU2 (fall time constant)   TSTEP            seconds

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

time           value
0 to TD1       V1
TD1 to TD2     V1+(V2-V1)*(1-exp(-(time-TD1)/TAU1))
TD2 to TSTOP   V1+(V2-V1)*(1-exp(-(time-TD1)/TAU1))
+(V1-V2)*(1-exp(-(time-TD2)/TAU2))

4.  Piece-Wise Linear  PWL(T1 V1 <T2 V2 T3 V3 T4 V4 ...>)
Examples:
		  
VCLOCK 7 5 PWL(0 -7 10NS -7 11NS -3 17NS -3 18NS -7 50NS -7)

Parameters and default values

Each pair of values (Ti, Vi) specifies that the value of the source is Vi
(in Volts or Amps) at time=Ti.  The value of the source at intermediate values
of time is determined by using linear interpolation on the input values.

5.  Single-Frequency FM   SFFM(VO VA FC MDI FS)

Examples:

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

parameters                default values   units
VO  (offset)                               Volts or Amps
VA  (amplitude)                            Volts or Amps
FC  (carrier frequency)   1/TSTOP          Hz
MDI (modulation index)
FS  (signal frequency)    1/TSTOP          Hz

The shape of the waveform  is  described  by  the  following
equation:
value = VO + VA*sine((twopi*FC*time) + MDI*sine(twopi*FS*time))

7.  SEMICONDUCTOR DEVICES

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

7.1.  Junction Diodes

General form:

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

Examples:

DBRIDGE 2 10 DIODE1
DCLMP 3 7 DMOD 3.0 IC=0.2

     N+ and N- are the positive and negative nodes, respectively.
MNAME  is  the model name, AREA is the area factor, and off indi-
cates an (optional) starting  condition  on  the  device  for  dc
analysis.   If  the  area  factor  is  omitted, a value of 1.0 is
assumed.  The (optional) initial  condition  specification  using
IC=VD  is intended for use with the UIC option on the .TRAN card,
when a transient analysis is desired starting from other than the
quiescent operating point.

7.2.  Bipolar Junction Transistors (BJT's)

General form:

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

Examples:

Q23 10 24 13 QMOD IC=0.6,5.0
Q50A 11 26 4 20 MOD1

     NC, NB, and NE are the collector, base, and  emitter  nodes,
respectively.   NS is the (optional) substrate node.  If unspeci-
fied, ground is used.  MNAME is the model name, AREA is the  area
factor,  and OFF indicates an (optional) initial condition on the
device for the dc analysis.  If the area  factor  is  omitted,  a
value  of  1.0  is  assumed.   The  (optional)  initial condition
specification using IC=VBE,VCE is intended for use with  the  UIC
option  on  the  .TRAN card, when a transient analysis is desired
starting from other than the quiescent operating point.  See  the
.IC  card  description  for a better way to set transient initial
conditions.

7.3.  Junction Field-Effect Transistors (JFET's)
		  
General form:

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

Examples:

J1 7 2 3 JM1 OFF

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

7.4.  MOSFET's

General form:

MXXXXXXX ND NG NS NB MNAME <L=VAL> <W=VAL> <AD=VAL> <AS=VAL>
+ <PD=VAL> <PS=VAL> <NRD=VAL> <NRS=VAL> <OFF> <IC=VDS,VGS,VBS>

Examples:

M1 24 2 0 20 TYPE1
M31 2 17 6 10 MODM L=5U W=2U
M31 2 16 6 10 MODM 5U 2U
M1 2 9 3 0 MOD1 L=10U W=5U AD=100P AS=100P PD=40U PS=40U
M1 2 9 3 0 MOD1 10U 5U 2P 2P

ND, NG, NS, and NB are the drain, gate, source,  and  bulk  (sub-
strate)  nodes,  respectively.  MNAME is the model name.  L and W
are the channel length and width, in meters.  AD and AS  are  the
areas  of  the  drain  and source diffusions, in sq-meters.  Note
that the suffix U specifies microns (1E-6  m)  and  P  sq-microns
(1E-12  sq-m).  If  any  of  L,  W,  AD, or AS are not specified,
default values are used.  The user may specify the values  to  be
used  for these default parameters on the .OPTIONS card.  The use
of defaults simplifies input deck preparation,  as  well  as  the
editing  required if device geometries are to be changed.  PD and
PS are the perimeters of  the  drain  and  source  junctions,  in
meters.   NRD  and NRS designate the equivalent number of squares
of the drain and source diffusions;  these  values  multiply  the
sheet resistance RSH specified on the .MODEL card for an accurate
representation of the parasitic series drain  and  source  resis-
tance 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 specif-
ication using IC=VDS,VGS,VBS is intended for  use  with  the  UIC
option  on  the  .TRAN card, when a transient analysis is desired
starting from other than the quiescent operating point.  See  the
.IC  card  for  a better and more convenient way to specify tran-
sient initial conditions.

7.5.  .MODEL Card

General form:

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

Examples:

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

     The .MODEL card specifies a set  of  model  parameters  that
will  be  used  by one or more devices.  MNAME is the model name,
and type is one of the following seven types:

NPN    NPN BJT model
PNP    PNP BJT model
D      diode model
NJF    N-channel JFET model
PJF    P-channel JFET model
NMOS   N-channel MOSFET model
PMOS   P-channel MOSFET model

     Parameter values are  defined  by  appending  the  parameter
name,  as  given  below for each model type, followed by an equal
sign and the parameter value.   Model  parameters  that  are  not
given  a  value  are  assigned the default values given below for
each model type.

7.6.  Diode Model

     The dc characteristics of the diode are  determined  by  the
parameters  IS  and  N.   An  ohmic  resistance, RS, is included.
Charge storage effects are modeled by a transit time, TT,  and  a
nonlinear  depletion layer capacitance which is determined by the
parameters CJO, VJ, and M.  The  temperature  dependence  of  the
saturation  current  is  defined by the parameters EG, the energy
and XTI, the saturation current  temperature  exponent.   Reverse
breakdown  is  modeled  by an exponential increase in the reverse
diode current and is determined by  the  parameters  BV  and  IBV
(both of which are positive numbers).
name   parameter                        units   default    example    area
1   IS     saturation current               A       1.0E-14    1.0E-14    *
2   RS     ohmic resistance                 Ohm     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
                                                                       0.67 Ge
9   XTI    saturation-current temp. exp     -       3.0        3.0 jn  2.0 Sbd
10   KF     flicker noise coefficient        -       0
11   AF     flicker noise exponent           -       1
12   FC     coefficient for forward-bias     -       0.5
depletion capacitance formula
13   BV     reverse breakdown voltage        V       infinite   40.0
14   IBV    current at breakdown voltage     A       1.0E-3

7.7.  BJT Models (both NPN and PNP)
		  
     The bipolar junction transistor model in SPICE is an adapta-
tion  of  the  integral  charge control model of Gummel and Poon.
This modified Gummel-Poon model extends  the  original  model  to
include  several  effects  at  high  bias levels.  The model will
automatically simplify to the simpler Ebers-Moll model when  cer-
tain  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 physi-
cal 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 characteris-
tics, 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  deter-
mined  by the energy-gap, EG, and the saturation current tempera-
ture exponent, XTI.  Additionally base current temperature depen-
dence  is modeled by the beta temperature exponent XTB in the new
model.
     The  BJT parameters used in the modified  Gummel-Poon  model
are listed below. The parameter names used in earlier versions of
SPICE2 are still accepted.
                  Modified Gummel-Poon BJT Parameters.
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    B-C leakage saturation current          A       0          1.0E-13   *
13   NC     B-C leakage emission coefficient        -       2          1.5
14   RB     zero bias base resistance               Ohms    0          100       *
15   IRB    current where base resistance
falls halfway to its min value          A       infinite   0.1       *
16   RBM    minimum base resistance
at high currents                        Ohms    RB         10        *
17   RE     emitter resistance                      Ohms    0          1         *
18   RC     collector resistance                    Ohms    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   -       1
connected to internal base node
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

7.8.  JFET Models (both N and P Channel)
		  
     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.

name     parameter                            units    default   example   area

1   VTO      threshold voltage                    V        -2.0      -2.0
2   BETA     transconductance parameter           A/V**2   1.0E-4    1.0E-3    *
3   LAMBDA   channel length modulation
parameter                            1/V      0         1.0E-4
4   RD       drain ohmic resistance               Ohm      0         100       *
5   RS       source ohmic resistance              Ohm      0         100       *
6   CGS      zero-bias G-S junction capacitance   F        0         5PF       *
7   CGD      zero-bias G-D junction capacitance   F        0         1PF       *
8   PB       gate junction potential              V        1         0.6
9   IS       gate junction saturation current     A        1.0E-14   1.0E-14   *
10   KF       flicker noise coefficient            -        0
11   AF       flicker noise exponent               -        1
12   FC       coefficient for forward-bias         -        0.5
depletion capacitance formula

7.9.  MOSFET Models (both N and P channel)
		  
     SPICE provides three MOSFET device models  which  differ  in
the  formulation  of  the I-V characteristic.  The variable LEVEL
specifies the model to be used:

LEVEL=1 ->    Shichman-Hodges
LEVEL=2 ->    MOS2 (as described in [1])
LEVEL=3 ->    MOS3, a semi-empirical model(see [1])

The dc characteristics of the MOSFET are defined  by  the  device
parameters  VTO,  KP, LAMBDA, PHI and GAMMA. These parameters are
computed by SPICE if process  parameters  (NSUB,  TOX,  ...)  are
given,  but  user-specified values always override.  VTO is posi-
tive (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 capa-
citance 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 respec-
tively, and are determined by the parameters CBD, CBS, CJ,  CJSW,
MJ,  MJSW  and  PB.   There are two built-in models of the charge
storage effects associated with the thin-oxide.  The  default  is
the piecewise linear voltage-dependent capacitance model proposed
by Meyer.  The second choice is the charge-controlled capacitance
model  of Ward and Dutton [1].  The XQC model parameter acts as a
flag and a coefficient at the same time.  As the former it causes
the  program to use Meyer's model whenever larger than 0.5 or not
specified, and the charge-controlled model  when  between  0  and
0.5.  In the latter case its value defines the share of the chan-
nel charge associated with the drain terminal in  the  saturation
region.   The  thin-oxide  charge  storage  effects  are  treated
slightly  different  for  the  LEVEL=1  model.   These   voltage-
dependent  capacitances  are included only if TOX is specified in
the input description and they are represented using Meyer's for-
mulation.
       There is some overlap among the  parameters  describing  the
junctions, e.g. the reverse current can be input either as IS (in
A) or as JS (in A/m**2). Whereas the first is an  absolute  value
the second is multiplied by AD and AS to give the reverse current
of the drain and source junctions respectively. This  methodology
has  been chosen since there is no sense in relating always junc-
tion characteristics with AD and AS entered on the  device  card;
the  areas  can  be defaulted.  The same idea applies also to the
zero-bias junction capacitances CBD and CBS (in F) on  one  hand,
and  CJ (in F/m**2) on the other.  The parasitic drain and source
series resistance can be expressed as either RD and RS (in  ohms)
or  RSH  (in ohms/sq.), the latter being multiplied by the number
of squares NRD and NRS input on the device card.

name     parameter                               units       default   example

1    LEVEL    model index                             -           1
2    VTO      zero-bias threshold voltage             V           0.0       1.0
3    KP       transconductance parameter              A/V**2      2.0E-5    3.1E-5
4    GAMMA    bulk threshold parameter                V**0.5      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                  Ohm         0.0       1.0
8    RS       source ohmic resistance                 Ohm         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        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 resisitance                       Ohm/sq.     0.0       10.0
17   CJ       zero-bias bulk junction bottom cap.
per sq-meter of junction area           F/m**2      0.0       2.0E-4
18   MJ       bulk junction bottom grading coef.      -           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 coef.    -           0.33
21   JS       bulk junction saturation current
per sq-meter of junction area           A/m**2                1.0E-8
22   TOX      oxide thickness                         meter       1.0E-7    1.0E-7
23   NSUB     substrate doping                        1/cm**3     0.0       4.0E15
24   NSS      surface state density                   1/cm**2     0.0       1.0E10
25   NFS      fast surface state density              1/cm**2     0.0       1.0E10
26   TPG      type of gate material:                  -           1.0
+1 opp. to substrate
-1 same as substrate
0  Al gate
27   XJ       metallurgical junction depth            meter       0.0       1U
28   LD       lateral diffusion                       meter       0.0       0.8U
29   UO       surface mobility                        cm**2/V-s   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 coef (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   XQC      thin-oxide capacitance model flag
and coefficient of channel charge
share attributed to drain (0-0.5)       -           1.0       0.4
36   KF       flicker noise coefficient               -           0.0       1.0E-26
37   AF       flicker noise exponent                  -           1.0       1.2
38   FC       coefficient for forward-bias
depletion capacitance formula           -           0.5
39   DELTA    width effect on threshold voltage
(MOS2 and MOS3)                         -           0.0       1.0
40   THETA    mobility modulation (MOS3 only)         1/V         0.0       0.1
41   ETA      static feedback (MOS3 only)             -           0.0       1.0
42   KAPPA    saturation field factor (MOS3 only)     -           0.2       0.5


8.  SUBCIRCUITS

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

8.1.  .SUBCKT Card

General form:

.SUBCKT subnam N1 <N2 N3 ...>

Examples:

.SUBCKT OPAMP 1 2 3 4

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

8.2.  .ENDS Card

General form:

.ENDS <SUBNAM>

Examples:

.ENDS OPAMP

     This card must be the last one for  any  subcircuit  defini-
tion.   The subcircuit name, if included, indicates which subcir-
cuit definition is being terminated;  if omitted, all subcircuits
being  defined  are  terminated.   The  name  is needed only when
nested subcircuit definitions are being made.

8.3.  Subcircuit Calls

General form:

XYYYYYYY N1 <N2 N3 ...> SUBNAM

Examples:

X1 2 4 17 3 1 MULTI

     Subcircuits are used in SPICE by specifying  pseudo-elements
beginning  with the letter X, followed by the circuit nodes to be
used in expanding the subcircuit.

9.  CONTROL CARDS

9.1.  .TEMP Card

General form:

.TEMP T1 <T2 <T3 ...>>

Examples:

.TEMP -55.0 25.0 125.0

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

9.2.  .WIDTH Card
		  
General form:

.WIDTH IN=COLNUM OUT=COLNUM

Examples:

.WIDTH IN=72 OUT=133

     COLNUM is the last column read from each line of input;  the
setting  takes effect with the next line read.  The default value
for COLNUM is 80.  The out parameter specifies the  output  print
width.   Permissible values for the output print width are 80 and
133.

9.3.  .OPTIONS Card

General form:

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

Examples:

.OPTIONS ACCT LIST NODE

     This card allows the user to reset program control and  user
options for specific simulation purposes.  Any combination of the
following options may be included, in  any  order.   'x'  (below)
represents some positive number.

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.
GMIN=x   resets the value of GMIN, the minimum conductance
         allowed by the program.  The default value is 1.0E-12.
RELTOL=x resets the relative error tolerance of the program.  The
         default value is 0.001 (0.1 percent).
ABSTOL=x resets the absolute current error tolerance of the
         program.  The default value is 1 picoamp.
VNTOL=x  resets the absolute voltage error tolerance of the
         program.  The default value is 1 microvolt.
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.
CHGTOL=x resets the charge tolerance of the program.  The default
         value is 1.0E-14.
PIVTOL=x resets the absolute minimum value for a matrix entry
         to be accepted as a pivot.  The default value is 1.0E-13.
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).
NUMDGT=x resets the number of significant digits printed for
         output variable values.  X must satisfy the relation
         0 < x < 8.  The default value is 4.  Note:  this option is
         independent of the error tolerance used by SPICE (i.e., if
         the values of options RELTOL, ABSTOL, etc., are not changed
         then one may be printing numerical 'noise' for NUMDGT > 4.
TNOM=x   resets the nominal temperature.  The default value is
         27 deg C (300 deg K).
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.
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.
ITL6=x   resets the dc iteration limit at each step of the source
         stepping method.  The default is 0 which means not to use
         this method.
CPTIME=x the maximum cpu-time in seconds allowed for this job.
LIMTIM=x resets the amount of cpu time reserved by SPICE for
         generating plots should a cpu time-limit cause job
         termination.  The default value is 2 (seconds).
LIMPTS=x resets the total number of points that can be printed
         or plotted in a dc, ac, or transient analysis.  The
         default value is 201.
LVLCOD=x if x is 2 (two), then machine code for the matrix
         solution will be generated.  Otherwise, no machine code is
         generated.  The default value is 2.  Applies only to CDC
         computers.
LVLTIM=x if x is 1 (one), the iteration timestep control is used.
         if x is 2 (two), the truncation-error timestep is used.
         The default value is 2.  If method=Gear and MAXORD>2 then
         LVLTIM is set to 2 by SPICE.
METHOD=name sets the numerical integration method used by SPICE.
            Possible names are Gear or trapezoidal.  The default is
            trapezoidal.
MAXORD=x sets the maximum order for the integration method if
         Gear's variable-order method is used.  X must be between
         2 and 6.  The default value is 2.
DEFL=x   resets the value for MOS channel length; the default
         is 100.0 micrometer.
DEFW=x   resets the value for MOS channel width; the default
         is 100.0 micrometer.
DEFAD=x  resets the value for MOS drain diffusion area; the
         default is 0.0.
DEFAS=x  resets the value for MOS source diffusion area; the
         default is 0.0.

9.4.  .OP Card

General form:

.OP

     The inclusion of this card in an input deck will force SPICE
to determine the dc operating point of the circuit with inductors
shorted and capacitors opened.  Note:  a dc analysis is automati-
cally  performed  prior  to a transient analysis to determine the
transient initial conditions, and prior  to  an  ac  small-signal
analysis  to  determine  the  linearized, small-signal models for
nonlinear devices.
SPICE performs a dc operating point  analysis  if  no  other
analyses are requested.

9.5.  .DC Card

General form:

.DC SRCNAM VSTART VSTOP VINCR [SRC2 START2 STOP2 INCR2]

Examples:

.DC VIN 0.25 5.0 0.25
.DC VDS 0 10 .5 VGS 0 5 1
.DC VCE 0 10 .25 IB 0 10U 1U

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

9.6.  .NODESET Card

General form:

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

Examples:

.NODESET V(12)=4.5 V(4)=2.23

     This card helps the program find the dc or initial transient
solution  by  making  a preliminary pass with the specified nodes
held to the given voltages.  The restriction is then released and
the  iteration continues to the true solution.  The .NODESET card
may be necessary for convergence on bistable or astable circuits.
In general, this card should not be necessary.

9.7.  .IC Card

General form:

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

Examples:

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

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

1.  When the UIC parameter is specified on the .TRAN card,  then
the  node  voltages specified on the .IC card are used to compute
the capacitor, diode, BJT, JFET, and MOSFET  initial  conditions.
This  is  equivalent  to  specifying the IC=... parameter on each
device card, but is much more convenient.  The  IC=...  parameter
can  still  be  specified  and  will take precedence over the .IC
values.  Since no dc bias (initial transient)  solution  is  com-
puted  before  the  transient  analysis,  one should take care to
specify all dc source voltages on the .IC card if they are to  be
used to compute device initial conditions.

2.  When the UIC parameter is not specified on the  .TRAN  card,
the  dc bias (initial transient) solution will be computed before
the transient analysis.  In this case, the node  voltages  speci-
fied on the .IC card will be forced to the desired initial values
during the bias solution.  During transient  analysis,  the  con-
straint on these node voltages is removed.

9.8.  .TF Card

General form:

.TF OUTVAR INSRC

Examples:

.TF V(5,3) VIN
.TF I(VLOAD) VIN

     This card defines the small-signal output and input for  the
dc  small-  signal  analysis.   OUTVAR is the small-signal output
variable and INSRC is the small-signal  input  source.   If  this
card is included, SPICE will compute the dc small-signal value of
the transfer function (output/input), input resistance, and  out-
put  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.

9.9.  .SENS Card

General form:

.SENS OV1 <OV2 ... >

Examples:

.SENS V(9) V(4,3) V(17) I(VCC)

     If a .SENS card is included in the input  deck,  SPICE  will
determine  the  dc  small-signal  sensitivities of each specified
output variable with respect to every circuit  parameter.   Note:
for large circuits, large amounts of output can be generated.

9.10.  .AC Card

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  varia-
tion,  and  NP  is  the number of points.  FSTART is the starting
frequency, and FSTOP is the final frequency.   If  this  card  is
included  in  the  deck, SPICE will perform an ac analysis of the
circuit over the specified frequency range.  Note that  in  order
for  this  analysis  to  be  meaningful, at least one independent
source must have been specified with an ac value.

9.11.  .DISTO Card

General form:

.DISTO RLOAD <INTER <SKW2 <REFPWR <SPW2>>>>

Examples:

.DISTO RL 2 0.95 1.0E-3 0.75

This card controls whether SPICE will compute the distortion
characteristic of the circuit in a small-signal mode as a part of
the  ac  small-signal  sinusoidal  steady-state  analysis.    The
analysis is performed assuming that one or two signal frequencies
are imposed at the input;  let the two  frequencies  be  f1  (the
nominal  analysis frequency) and f2 (=SKW2*f1).  The program then
computes the following distortion measures:

HD2  - the magnitude of the frequency component 2*f1 assuming that f2 is not present.
HD3  - the magnitude of the frequency component 3*f1 assuming that f2 is not present.
SIM2 - the magnitude of the frequency component f1 + f2.
DIM2 - the magnitude of the frequency component f1 - f2.
DIM3 - the magnitude of the frequency component 2*f1 - f2.

     RLOAD is the name of the output load resistor into which all
distortion  power  products  are  to  be  computed.  INTER is the
interval at which the summary printout of  the  contributions  of
all  nonlinear  devices to the total distortion is to be printed.
If omitted or set to zero, no  summary  printout  will  be  made.
REFPWR is the reference power level used in computing the distor-
tion products; if omitted, a value of 1  mW  (that  is,  dbm)  is
used.  SKW2 is the ratio of f2 to f1.  If omitted, a value of 0.9
is used (i.e., f2 = 0.9*f1).  SPW2 is the amplitude  of  f2.   If
omitted, a value of 1.0 is assumed.
      The distortion measures HD2, HD3, SIM2, DIM2, and  DIM3  may
also  be  be  printed  and/or plotted (see the description of the
.PRINT and .PLOT cards).

9.12.  .NOISE Card

General form:

.NOISE OUTV INSRC NUMS

Examples:

.NOISE V(5) VIN 10

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

9.13.  .TRAN Card

General form:

.TRAN TSTEP TSTOP <TSTART <TMAX>> <UIC>

Examples:

.TRAN 1NS 100NS
.TRAN 1NS 1000NS 500NS
.TRAN 10NS 1US UIC

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

9.14.  .FOUR Card

General form:

.FOUR FREQ OV1 <OV2 OV3 ...>

Examples:

.FOUR 100K  V(5)

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

9.15.  .PRINT Cards

General form:

.PRINT PRTYPE OV1 <OV2 ... OV8>

Examples:

.PRINT TRAN V(4) I(VIN)
.PRINT AC VM(4,2) VR(7) VP(8,3)
.PRINT DC V(2) I(VSRC) V(23,17)
.PRINT NOISE INOISE
.PRINT DISTO HD3 SIM2(DB)

     This card defines the contents of a tabular listing  of  one
to  eight  output  variables.  PRTYPE is the type of the analysis
(DC, AC, TRAN, NOISE, or DISTO) for which the  specified  outputs
are  desired. The form for voltage or current output variables is
as follows:

V(N1<,N2>)
		  
specifies the voltage difference between nodes  N1  and
N2.  If N2 (and the preceding comma) is omitted, ground
(0) is assumed.  For the ac analysis,  five  additional
outputs can be accessed by replacing the letter V by:

VR  -    real part
VI  -    imaginary part
VM  -    magnitude
VP  -    phase
VDB -    20*log10(magnitude)

I(VXXXXXXX)

specifies the current flowing in the  independent  vol-
tage  source  named  VXXXXXXX.   Positive current flows
from the positive node,  through  the  source,  to  the
negative  node.  For the ac analysis, the corresponding
replacements for the letter I may be made in  the  same
way as described for voltage outputs.

      Output variables for the noise and distortion analyses  have
a different general form from that of the other analyses, i.e.

OV<(X)>

where OV is any of  ONOISE  (output  noise),  INOISE  (equivalent
input  noise),  D2,  HD3, SIM2, DIM2, or DIM3 (see description of
distortion analysis), and X may be any of:

R  -    real part
I  -    imaginary part
M  -    magnitude (default if nothing specified)
P  -    phase
DB -    20*log10(magnitude)

thus, SIM2 (or SIM2(M)) describes the magnitude of the SIM2  dis-
tortion  measure, while HD2(R) describes the real part of the HD2
distortion measure.
     There is no limit on the number of  .PRINT  cards  for  each
type of analysis.

9.16.  .PLOT Cards

General form:

.PLOT PLTYPE OV1 <(PLO1,PHI1)> <OV2 <(PLO2,PHI2)> ... OV8>

Examples:

.PLOT DC V(4) V(5) V(1)
.PLOT TRAN V(17,5) (2,5) I(VIN) V(17) (1,9)
.PLOT AC VM(5) VM(31,24) VDB(5) VP(5)
.PLOT DISTO HD2 HD3(R) SIM2
.PLOT TRAN V(5,3) V(4) (0,5) V(7) (0,10)

     This card defines the contents of one plot of  from  one  to
eight  output variables.  PLTYPE is the type of analysis (DC, AC,
TRAN, NOISE, or  DISTO)  for  which  the  specified  outputs  are
desired.   The  syntax  for  the OVI is identical to that for the
.PRINT card, described above.
      The optional plot limits (PLO,PHI) may  be  specified  after
any of the output variables.  All output variables to the left of
a pair of plot limits (PLO,PHI) will be plotted  using  the  same
lower  and  upper plot bounds.  If plot limits are not specified,
SPICE will automatically determine the minimum and maximum values
of  all output variables being plotted and scale the plot to fit.
More than one scale will be used if the  output  variable  values
warrant  (i.e.,  mixing  output  variables  with values which are
orders-of-magnitude different still gives readable plots).
The overlap of two or more traces on any plot  is  indicated
by the letter X.
     When more than one output variable appears on the same plot,
the  first variable specified will be printed as well as plotted.
If a printout of all  variables  is  desired,  then  a  companion
.PRINT card should be included.
      There is no limit on the number of .PLOT cards specified for
each type of analysis.


10.  APPENDIX A:  EXAMPLE DATA DECKS

10.1.  Circuit 1

     The following deck determines the  dc  operating  point  and
small-signal transfer function of a simple differential pair.  In
addition, the ac small-signal response is computed over the  fre-
quency range 1Hz to 100MEGHz.

SIMPLE DIFFERENTIAL PAIR
VCC 7 0 12
VEE 8 0 -12
VIN 1 0 AC 1
RS1 1 2 1K
RS2 6 0 1K
Q1 3 2 4 MOD1
Q2 5 6 4 MOD1
RC1 7 3 10K
RC2 7 5 10K
RE 4 8 10K
.MODEL MOD1 NPN BF=50 VAF=50 IS=1.E-12 RB=100 CJC=.5PF TF=.6NS
.TF V(5) VIN
.AC DEC 10 1 100MEG
.PLOT AC VM(5) VP(5)
.PRINT AC VM(5) VP(5)
.END

10.2.  Circuit 2
The following deck computes the output characteristics of a  MOS-
FET device over the range 0-10V for VDS and 0-5V for VGS.

MOS OUTPUT CHARACTERISTICS
.OPTIONS NODE NOPAGE
VDS 3 0
VGS 2 0
M1 1 2 0 0 MOD1 L=4U W=6U AD=10P AS=10P
.MODEL MOD1 NMOS VTO=-2 NSUB=1.0E15 UO=550
* VIDS MEASURES ID, WE COULD HAVE USED VDS, BUT ID WOULD BE NEGATIVE
VIDS 3 1
.DC VDS 0 10 .5 VGS 0 5 1
.PRINT DC I(VIDS) V(2)
.PLOT DC I(VIDS)
.END

10.3.  Circuit 3

     The following deck determines the dc transfer curve and  the
transient  pulse response of a simple RTL inverter.  The input is
a pulse from 0 to 5 Volts with delay, rise, and fall times of 2ns
and a pulse width of 30ns.  The transient interval is 0 to 100ns,
with printing to be done every nanosecond.

SIMPLE RTL INVERTER
VCC 4 0 5
VIN 1 0 PULSE 0 5 2NS 2NS 2NS 30NS
RB 1 2 10K
Q1 3 2 0 Q1
RC 3 4 1K
.PLOT DC V(3)
.PLOT TRAN V(3) (0,5)
.PRINT TRAN V(3)
.MODEL Q1 NPN BF 20 RB 100 TF .1NS CJC 2PF
.DC VIN 0 5 0.1
.TRAN 1NS 100NS
.END

10.4.  Circuit 4

     The following deck simulates a four-bit binary adder,  using
several  subcircuits  to  describe  various pieces of the overall
circuit.
ADDER - 4 BIT ALL-NAND-GATE BINARY ADDER
*** SUBCIRCUIT DEFINITIONS
.SUBCKT NAND 1 2 3 4
*   NODES:  INPUT(2), OUTPUT, VCC
Q1 9 5 1 QMOD
D1CLAMP 0 1 DMOD
Q2 9 5 2 QMOD
D2CLAMP 0 2 DMOD
RB 4 5 4K
R1 4 6 1.6K
Q3 6 9 8 QMOD
R2 8 0 1K
RC 4 7 130
Q4 7 6 10 QMOD
DVBEDROP 10 3 DMOD
Q5 3 8 0 QMOD
.ENDS NAND
.SUBCKT ONEBIT 1 2 3 4 5 6
*   NODES:  INPUT(2), CARRY-IN, OUTPUT, CARRY-OUT, VCC
X1 1 2 7 6 NAND
X2 1 7 8 6 NAND
X3 2 7 9 6 NAND
X4 8 9 10 6 NAND
X5 3 10 11 6 NAND
X6 3 11 12 6 NAND
X7 10 11 13 6 NAND
X8 12 13 4 6 NAND
X9 11 7 5 6 NAND
.ENDS ONEBIT
.SUBCKT TWOBIT 1 2 3 4 5 6 7 8 9
*   NODES:  INPUT - BIT0(2) / BIT1(2), OUTPUT - BIT0 / BIT1,
*           CARRY-IN, CARRY-OUT, VCC
X1 1 2 7 5 10 9 ONEBIT
X2 3 4 10 6 8 9 ONEBIT
.ENDS TWOBIT

.SUBCKT FOURBIT 1 2 3 4 5 6 7 8 9 10 11 12 13 14 15
*   NODES:  INPUT - BIT0(2) / BIT1(2) / BIT2(2) / BIT3(2),
*           OUTPUT - BIT0 / BIT1 / BIT2 / BIT3, CARRY-IN, CARRY-OUT, VCC
X1 1 2 3 4 9 10 13 16 15 TWOBIT
X2 5 6 7 8 11 12 16 14 15 TWOBIT
.ENDS FOURBIT

*** DEFINE NOMINAL CIRCUIT

.MODEL DMOD D
.MODEL QMOD NPN(BF=75 RB=100 CJE=1PF CJC=3PF)
VCC 99 0 DC 5V
VIN1A 1 0 PULSE(0 3 0 10NS 10NS   10NS   50NS)
VIN1B 2 0 PULSE(0 3 0 10NS 10NS   20NS  100NS)
VIN2A 3 0 PULSE(0 3 0 10NS 10NS   40NS  200NS)
VIN2B 4 0 PULSE(0 3 0 10NS 10NS   80NS  400NS)
VIN3A 5 0 PULSE(0 3 0 10NS 10NS  160NS  800NS)
VIN3B 6 0 PULSE(0 3 0 10NS 10NS  320NS 1600NS)
VIN4A 7 0 PULSE(0 3 0 10NS 10NS  640NS 3200NS)
VIN4B 8 0 PULSE(0 3 0 10NS 10NS 1280NS 6400NS)
X1 1 2 3 4 5 6 7 8 9 10 11 12 0 13 99 FOURBIT
RBIT0 9 0 1K
RBIT1 10 0 1K
RBIT2 11 0 1K
RBIT3 12 0 1K
RCOUT 13 0 1K
.PLOT TRAN V(1) V(2) V(3) V(4) V(5) V(6) V(7) V(8)
.PLOT TRAN V(9) V(10) V(11) V(12) V(13)
.PRINT TRAN V(1) V(2) V(3) V(4) V(5) V(6) V(7) V(8)
.PRINT TRAN V(9) V(10) V(11) V(12) V(13)

.TRAN 1NS 6400NS

.OPTIONS ACCT LIST NODE LIMPTS=6401
.END

10.5.  Circuit 5

     The following deck simulates a  transmission-line  inverter.
Two transmission-line elements are required since two propagation
modes are excited.  In the case of a coaxial line, the first line
(T1)  models  the inner conductor with respect to the shield, and
the second line (T2) models the shield with respect to  the  out-
side world.

TRANSMISSION-LINE INVERTER
V1 1 0 PULSE(0 1 0 0.1N)
R1 1 2 50
X1 2 0 0 4 TLINE
R2 4 0 50
.SUBCKT TLINE 1 2 3 4
T1 1 2 3 4 Z0=50 TD=1.5NS
T2 2 0 4 0 Z0=100 TD=1NS
.ENDS TLINE
.TRAN 0.1NS 20NS
.PLOT TRAN V(2) V(4)
.END

11.  APPENDIX B:  NONLINEAR DEPENDENT SOURCES

     SPICE allows circuits to contain dependent  sources  charac-
terized by any of the four equations
i=f(v)          v=f(v)          i=f(i)          v=f(i)
where the functions must be polynomials, and the arguments may be
multidimensional.   The  polynomial  functions are specified by a
set of coefficients p0, p1, ..., pn.  Both the number  of  dimen-
sions  and the number of coefficients are arbitrary.  The meaning
of the coefficients depends upon the dimension of the polynomial,
as shown in the following examples:
     Suppose that the function is  one-dimensional  (that  is,  a
function  of one argument).  Then the function value fv is deter-
mined by the following expression in fa (the function argument):
fv = p0 + (p1*fa) + (p2*fa**2) + (p3*fa**3) + (p4*fa**4)
+ (p5*fa**5) + ...
Suppose now that the function is two-dimensional, with argu-
ments fa and fb.  Then the function value fv is determined by the
following expression:
fv = p0 + (p1*fa) +  (p2*fb)  +  (p3*fa**2)  +  (p4*fa*fb)  +
(p5*fb**2) +  (p6*fa**3)  +   (p7*fa**2*fb)   +   (p8*fa*fb**2)   +
(p9*fb**3) + ...
     Consider now the  case  of  a  three-dimensional  polynomial
function  with arguments fa, fb, and fc.  Then the function value
fv is determined by the following expression:
fv = p0  +  (p1*fa)  +  (p2*fb)  +  (p3*fc)  +  (p4*fa**2)  + (p5*fa*fb)
+ (p6*fa*fc) + (p7*fb**2) + (p8*fb*fc)  +  (p9*fc**2)  + (p10*fa**3)
+ (p11*fa**2*fb) + (p12*fa**2*fc) + (p13*fa*fb**2) + (p14*fa*fb*fc)
+  (p15*fa*fc**2)  +  (p16*fb**3)  +  (p17*fb**2*fc)   + (p18*fb*fc**2)
+ (p19*fc**3) + (p20*fa**4) + ...
Note:  if the polynomial is one-dimensional and exactly  one
coefficient  is specified, then SPICE assumes it to be p1 (and p0
= 0.0), in order to facilitate the  input  of  linear  controlled
sources.
For all four of the dependent sources described  below,  the
initial  condition  parameter  is  described as optional.  If not
specified, SPICE assumes 0 the initial  condition  for  dependent
sources  is  an  initial 'guess' for the value of the controlling
variable.  The program uses this initial condition to obtain  the
dc  operating  point  of the circuit.  After convergence has been
obtained, the program continues iterating  to  obtain  the  exact
value  for the controlling variable.  Hence, to reduce the compu-
tational effort for the dc operating point (or if the  polynomial
specifies  a  strong  nonlinearity),  a value fairly close to the
actual controlling variable should be specified for  the  initial
condition.

11.1.  Voltage-Controlled Current Sources

General form:

GXXXXXXX N+ N- <POLY(ND)> NC1+ NC1- ... P0 <P1 ...> <IC=...>

Examples:

G1 1 0 5 3 0 0.1M
GR 17 3 17 3 0 1M 1.5M IC=2V
GMLT 23 17 POLY(2) 3 5 1 2 0 1M 17M 3.5U IC=2.5, 1.3

    N+ and N- are the positive and negative nodes, respectively.
Current  flow  is  from the positive node, through the source, to
the negative node.  POLY(ND) only has  to  be  specified  if  the
source is multi-dimensional (one-dimensional is the default).  If
specified, ND is the number of dimensions, which  must  be  posi-
tive.   NC1+, NC1-, ... Are the positive and negative controlling
nodes, respectively.  One pair of nodes  must  be  specified  for
each   dimension.   P0,  P1,  P2,  ...,  Pn  are  the  polynomial
coefficients.  The (optional) initial condition  is  the  initial
guess  at  the  value(s)  of  the controlling voltage(s).  If not
specified, 0.0 is assumed.  The polynomial specifies  the  source
current  as a function of the controlling voltage(s).  The second
example above describes a current source with value

        I = 1E-3*V(17,3) + 1.5E-3*V(17,3)**2

note that since the source nodes are the same as the  controlling
nodes, this source actually models a nonlinear resistor.

11.2.  Voltage-Controlled Voltage Sources

General form:

    EXXXXXXX N+ N- <POLY(ND)> NC1+ NC1- ... P0 <P1 ...> <IC=...>

Examples:

     E1 3 4 21 17 10.5 2.1 1.75
    EX 17 0 POLY(3) 13 0 15 0 17 0 0 1 1 1 IC=1.5,2.0,17.35

     N+ and N- are the positive and negative nodes, respectively.
POLY(ND)  only  has  to  be  specified  if  the  source is multi-
dimensional (one-dimensional is the default).  If  specified,  ND
is the number of dimensions, which must be positive.  NC1+, NC1-,
... are the positive  and  negative  controlling  nodes,  respec-
tively.   One pair of nodes must be specified for each dimension.
P0, P1,  P2,  ...,  Pn  are  the  polynomial  coefficients.   The
(optional) initial condition is the initial guess at the value(s)
of the controlling voltage(s).  If not specified, 0.0 is assumed.
The  polynomial specifies the source voltage as a function of the
controlling voltage(s).  The second  example  above  describes  a
voltage source with value

        V = V(13,0) + V(15,0) + V(17,0)

(in other words, an ideal voltage summer).

11.3.  Current-Controlled Current Sources

General form:

FXXXXXXX N+ N- <POLY(ND)> VN1 <VN2 ...> P0 <P1 ...> <IC=...>

Examples:

F1 12 10 VCC 1MA 1.3M
FXFER 13 20 VSENS 0 1

     N+ and N- are the positive and negative nodes, respectively.
Current  flow  is  from the positive node, through the source, to
the negative node.  POLY(ND) only has  to  be  specified  if  the
source is multi-dimensional (one-dimensional is the default).  If
specified, ND is the number of dimensions, which  must  be  posi-
tive.   VN1,  VN2,  ...  are the names of voltage sources through
which the controlling current flows;  one name must be  specified
for  each  dimension.   The  direction  of  positive  controlling
current flow is from the positive node, through  the  source,  to
the  negative  node  of each voltage source.  P0, P1, P2, ..., Pn
 are the polynomial coefficients.  The (optional)  initial  condi-
tion  is  the  initial  guess  at the value(s) of the controlling
current(s) (in Amps).  If not specified,  0.0  is  assumed.   The
polynomial specifies the source current as a function of the con-
trolling current(s).  The first example above describes a current
source with value

I = 1E-3 + 1.3E-3*I(VCC)

11.4.  Current-Controlled Voltage Sources

General form:

HXXXXXXX N+ N- <POLY(ND)> VN1 <VN2 ...> P0 <P1 ...> <IC=...>

Examples:

HXY 13 20 POLY(2) VIN1 VIN2 0 0 0 0 1 IC=0.5 1.3
HR 4 17 VX 0 0 1

    N+ and N- are the positive and negative nodes, respectively.
POLY(ND)  only  has  to  be  specified  if  the  source is multi-
dimensional (one-dimensional is the default).  If  specified,  ND
is  the  number of dimensions, which must be positive.  VN1, VN2,
... are the names of voltage sources through which  the  control-
ling  current  flows;  one name must be specified for each dimen-
sion.  The direction of positive controlling current flow is from
the  positive  node,  through the source, to the negative node of
each voltage source.  P0, P1, P2,  ...,  Pn  are  the  polynomial
coefficients.   The  (optional)  initial condition is the initial
guess at the value(s) of the controlling  current(s)  (in  Amps).
If  not  specified, 0.0 is assumed.  The polynomial specifies the
source voltage as a function of the controlling current(s).   The
first example above describes a voltage source with value

        V = I(VIN1)*I(VIN2)


12.   APPENDIX  D:    ALTER  STATEMENT  AND  THE  SOURCE-STEPPING
METHOD

The ALTER statement allows SPICE to run with altered circuit
parameters.

General form:

.ALTER
ELEMENT CARDS (DEVICE CARDS, MODEL CARDS)
.ALTER (or .END CARD)

Examples:

R1 1 0 5K
VCC 3 0 10
M1 3 2 0 MOD1 L=5U W=2U
.MODEL MOD1 NMOS(VTO=1.0 KP=2.0E-5 PHI=0.6 NSUB=2.0E15 TOX=0.1U)
.ALTER
R1 1 0 3.5K
VCC 3 0 12
M1 3 2 0 MOD1 L=10U W=2U
.MODEL MOD1 NMOS(VTO=1.2 KP=2.0E-5 PHI=0.6 NSUB=5.0E15 TOX=1.5U)
.ALTER
M1 3 2 0 MOD1 L=10U W=4U
.END


     This card introduces the element(s), device(s) and  model(s)
whose  parameters  are  changed during the execution of the input
deck.  The analyses specified in the deck will start  over  again
with  the  changed  parameters.  The  .ALTER  card with the cards
defining the new parameters should be placed just before the .END
card.  The syntax for the element (device, model) cards is ident-
ical to that of the cards with the original parameters.
    There is no limit on the number of .ALTER cards and the cir-
cuit  will  be  re-analyzed as many times as the number of .ALTER
cards.  Subsequent ALTER operations employ parameters of the pre-
vious change.  No topological change of the circuit is allowed.
      The source-stepping method can enhance DC convergence.   But
it  is  slower  than  direct  use  of  the Newton-Raphson method.
Therefore it is best used as an alternative  to  achieve  conver-
gence of DC operating point when the circuit fails to converge by
using the Newton-Raphson method.  The source-stepping  method  is
used  by SPICE when the variable ITL6 in the .OPTIONS card is set
to the iteration limit at each step of the source(s).

For example,

     .OPTIONS ITL6=30

will cause SPICE to use  source-stepping  method  with  iteration
limit  30 at each step.  By default, ITL6 is 0 which means to use
the Newton-Raphson method directly.
