| School of Physics |
|
| Physics Home | Study here | Our Teaching | Our Research | Our Centres | News | Work here | EMPS |
Back to top
SPICE 3 User's Manual - Section 3
3 CIRCUIT ELEMENTS AND MODELSData 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).3.1 ELEMENTARY DEVICES3.1.1 ResistorsGeneral form:3.1.2 Semiconductor ResistorsGeneral form:3.1.3 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:
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
L - NARROW
R = RSH ----------
W - NARROW
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 Z 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:
2
R(T) = R(T ) [1 + TC1 (T - T ) + TC2 (T-T ) ]
0 0 0
3.1.4 CapacitorsGeneral form: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. 3.1.5 Semiconductor CapacitorsGeneral form:3.1.6 Semiconductor Capacitor Model (C)The capacitor model contains process information that may be used to compute the capacitance from strictly geometric information.
The capacitor has a capacitance computed as CAP = CJ (LENGTH - NARROW) (WIDTH - NARROW) + 2 CJSW (LENGTH + WIDTH - 2 NARROW) 3.1.7 InductorsGeneral form: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. 3.1.8 Coupled (Mutual) InductorsGeneral form:LYYYYYYY and LZZZZZZZ are the names of the two coupled inductors, and VALUE is the coefficient of coupling, K, which must be in the range −1 ≤ K ≤ +1. Using the 'dot' convention, place a 'dot' on the first node of each inductor. 3.1.9 SwitchesGeneral form:3.1.10 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:
*(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. 3.2 VOLTAGE AND CURRENT SOURCES3.2.1 Independent SourcesGeneral form: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)). 3.2.1.1. PulseGeneral form:
A single pulse so specified is described by the following table:
Intermediate points are determined by linear interpolation. 3.2.1.2 SinusoidalGeneral form:
The shape of the waveform is described by the following table:
3.2.1.3 ExponentialGeneral form:
The shape of the waveform is described by the following table:
3.2.1.4 Piece-Wise LinearGeneral form: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. 3.2.1.5 Single-Frequency FMGeneral form:
The shape of the waveform is described by the following equation: V(t)=VO+VA.sin(2πFC.t+MDI.sin[2πFS.t]) 3.2.2 Linear Dependent SourcesSPICE allows circuits to contain linear dependent sources characterized by any of the four equations:
where g, e, f, and h are constants representing transconductance, voltage gain, current gain, and transresistance, respectively. 3.2.2.1 Linear Voltage-Controlled Current SourcesGeneral form: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). 3.2.2.2 Linear Voltage-Controlled Voltage SourcesGeneral form: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. 3.2.2.3 Linear Current-Controlled Current SourcesGeneral form: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. 3.2.2.4 Linear Current-Controlled Voltage SourcesGeneral form:3.2.3 Non-linear Dependent SourcesGeneral form: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. [Note: The SPICE3 non-linear sources are not compatible with the poly() syntax used in SPICE2. Appendix C is included to facilitate conversion of old source. CDHW.] [Note: Appendix D describes several bugs affecting these devices. CDHW.] 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:
The function "u()" is the unit step function, with a value of one for arguments greater than zero and a value of zero for arguments less than or equal to zero. The function uramp(x) 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 or equal to 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:
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). Nonlinear resistors, capacitors, and inductors may be synthesized with the nonlinear dependent source. Nonlinear resistors are obvious. Nonlinear 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: 3.3 TRANSMISSION LINES[Note: The transmission line elements are not easy to use in non-trivial cases. The significance of the statement "this element models only one propagating mode" is that a length of coaxial cable has two modes (inner-shield and shield-ground), but even a simple pair of wires also has two modes (differential and common). The example file 'ltra_3.cir' shows what is required to simulate a pair of wires, and refer to [8] for the details of the calculations required. It seems that only the transmission of the voltage and current between N1 and N3 is represented by these elements, N2 and N4 are merely these nodes' respective current mirrors. CDHW.] 3.3.1 Lossless Transmission LinesGeneral form: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 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. 3.3.2 Lossy Transmission LinesGeneral form:3.3.3 Lossy Transmission Line Model (LTRA)[Note: Consider using the TXL and CPL device models distributed with KSPICE which are for modeling a single lossy transmission line and a coupled multiconductor line system, respectively. These device models can effectively replace the LTRA model of SPICE3. CDHW.] 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. [Note: Running an .AC analysis on the LTRA model only seems to give the correct results in cases when LEN=1.0 . This is always possible provided L, C, etc. are entered as the inductance of the whole line. CDHW.]
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. 3.3.4 Uniform Distributed RC Lines (Lossy)General form:3.3.5 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 subcicuit 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:
2
| R C |(K-1)| |
_ _ 2
log|F 2 J L |-----| |
max
| L L | K | |
N = ------------------------------
log K
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.
3.4 TRANSISTORS AND DIODESThe 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 con- trol line for a detailed explanation of initial conditions. 3.4.1 Junction DiodesGeneral form:3.4.2 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).
3.4.3 Bipolar Junction Transistors (BJTs)General form: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. 3.4.4 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.
3.4.5 Junction Field-Effect Transistors (JFETs)General form:3.4.6 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].
3.4.7 MOSFETsGeneral form:3.4.8 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:
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:
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
P P
L W
P = P + ---------- + ----------
0
L W
effective effective
is used to evaluate the parameter for the actual device specified with
L = L - DL
effective input
and
W = W - DW
effective input
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:
XPART = 0 selects a 40/60 drain/source charge partition in saturation, while XPART=1 selects a 0/100 drain/source charge partition. [Note: Al Davis reported 'In the BSIM1 model, the parameter "xpart" behaves randomly. To fix, .. in the file "b1mpar.c" line 290, change "iValue" to "rValue".' CDHW.] 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. 3.4.9 MESFETsGeneral form:3.4.10 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:
3
2
B (V -V ) | | V | | 3
gs T ds _
I = --------------- |1 - |1-A---| |(1 + L V ) for 0 < V <
d ds ds
1 + b(V - V ) | | 3 | | A
gs T
2
B (V -V ) 3
gs T _
I = ---------------(1 + L V ) for V >
d ds ds
1 + b(V - V ) A
gs T
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.
|
