The dc analysis portion of SPICE (.DC) determines the dc operating point of the circuit with inductors shorted and capacitors opened. The dc analysis options are specified on the .DC, .TF, and .OP control lines. A dc analysis is automatically performed prior to a transient analysis to determine the transient initial conditions, and prior to an ac small-signal analysis to determine the linearized, small-signal models for nonlinear devices. If requested, the dc small-signal value of a transfer function (ratio of output variable to input source), input resistance, and output resistance is also computed as a part of the dc solution. The dc analysis can also be used to generate dc transfer curves: a specified independent voltage or current source is stepped over a user-specified range and the dc output variables are stored for each sequential source value.
.DC: DC Transfer Function
General form:
.DC SRCNAM VSTART VSTOP VINCR [ SRC2 START2 STOP2 INCR2 ]
Examples:
.DC VIN 0.25 5.0 0.25
.DC VDS 0 10 .5 VGS 0 5 1
.DC VCE 0 10 .25 IB 0 10U 1U
The inclusion of this line in an input file directs SPICE to perform a dc analysis of the circuit. The DC line defines the dc transfer curve source and sweep limits (again with capacitors open and inductors shorted). SRCNAM is the name of an independent voltage or current source. VSTART, VSTOP, and VINCR are the starting, final, and incrementing values respectively. The first example causes the value of the voltage source VIN to be swept from 0.25 volts to 5.0 volts in increments of 0.25 volts. A second source (SRC2) may optionally be specified with associated sweep parameters. In this case, the first source is swept over its range for each value of the second source. This option can be useful for obtaining semiconductor device output characteristics.
The ac small-signal portion of SPICE (.AC) computes the ac output variables as a function of frequency. The program first computes the dc operating point of the circuit and determines linearized, small-signal models for all of the nonlinear devices in the circuit. The resultant linear circuit is then analyzed over a user-specified range of frequencies. The desired output of an ac small- signal analysis is usually a transfer function (voltage gain, transimpedance, etc). If the circuit has only one ac input, it is convenient to set that input to unity and zero phase, so that output variables have the same value as the transfer function of the output variable with respect to the input.
.AC: Small-Signal AC Analysis
General form:
.AC DEC ND FSTART FSTOP
.AC OCT NO FSTART FSTOP
.AC LIN NP FSTART FSTOP
Examples:
.AC DEC 10 1 10K
.AC DEC 10 1K 100MEG
.AC LIN 100 1 100HZ
DEC stands for decade variation, and ND is the number of points per decade. OCT stands for octave variation, and NO is the number of points per octave. LIN stands for linear variation, and NP is the number of points. FSTART is the starting frequency, and FSTOP is the final frequency. If this line is included in the input file, SPICE performs an AC analysis of the circuit over the specified frequency range. Note that in order for this analysis to be meaningful, at least one independent source must have been specified with an ac value.
The transient analysis portion of SPICE (.TRAN) computes the transient output variables as a function of time over a user-specified time interval. The initial conditions are automatically determined by a dc analysis. All sources which are not time dependent (for example, power supplies) are set to their dc value. The transient time interval is specified on a .TRAN control line.
.TRAN: Transient Analysis
General form:
.TRAN TSTEP TSTOP [ [ TSTART ] TMAX ]
Examples:
.TRAN 1NS 100NS
.TRAN 1NS 1000NS 500NS
.TRAN 10NS 1US
The inclusion of this line in an input file directs SPICE to perfom a transient analysis of the circuit. TSTEP is the printing or plotting increment for line-printer output. For use with the post-processor, TSTEP is the suggested computing increment. TSTOP is the final time, and TSTART is the initial time. If TSTART is omitted, it is assumed to be zero. The transient analysis always begins at time zero. In the interval <zero, TSTART>, the circuit is analyzed (to reach a steady state), but no outputs are stored. In the interval <TSTART, TSTOP>, the circuit is analyzed and outputs are stored. TMAX is the maximum step-size that SPICE uses; for default, the program chooses either TSTEP or (TSTOP-TSTART)/50.0, whichever is smaller. TMAX is useful when one wishes to guarantee a computing interval which is smaller than the printer increment, TSTEP.
[Note: The original Berkeley code had a bug so it actually chooses the larger of either TSTEP or (TSTOP-TSTART)/50.0 so I suggest you set TMAX explicitly unless you have a patched version. Another reason for doing this is that certain circuits, particularly those involving sinusoidal oscillation, fool the integrator into increasing the timestep too much. For circuits which use short pulses, TMAX should be no more than about 50 times the shortest feature of interest. There is also an internal lower limit 1e-9*TMAX imposed on TSTEP and non-convergent circuits may give 'Timestep too short' messages indicating this limit has been hit. CDHW.]
UIC (use initial conditions) is an optional keyword which indicates that the user does not want SPICE to solve for the quiescent operating point before beginning the transient analysis. If this keyword is specified, SPICE uses the values specified using IC=... on the various elements as the initial transient condition and proceeds with the analysis. If the .IC control line has been specified, then the node voltages on the .IC line are used to compute the initial conditions for the devices. Look at the description on the .IC control line for its interpretation when UIC is not specified
The pole-zero analysis portion of SPICE (.PZ) computes the poles and/or zeros in the small-signal ac transfer function. The program first computes the dc operating point and then determines the linearized, small-signal models for all the nonlinear devices in the circuit. This circuit is then used to find the poles and zeros of the transfer function.
Two types of transfer functions are allowed : one of the form (output voltage)/(input voltage) and the other of the form (output voltage)/(input current). These two types of transfer functions cover all the cases and one can find the poles/zeros of functions like input/output impedance and voltage gain. The input and output ports are specified as two pairs of nodes.
The pole-zero analysis works with resistors, capacitors, inductors, linear-controlled sources, independent sources, BJTs, MOSFETs, JFETs and diodes. Transmission lines are not supported.
The method used in the analysis is a sub-optimal numerical search. For large circuits it may take a considerable time or fail to find all poles and zeros. For some circuits, the method becomes "lost" and finds an excessive number of poles or zeros.
.PZ: Pole-Zero Analysis
General form:
.PZ NODE1 NODE2 NODE3 NODE4 { CUR | VOL } { POL | ZER | PZ }Examples:
.PZ 1 0 3 0 CUR POL
.PZ 2 3 5 0 VOL ZER
.PZ 4 1 4 1 CUR PZ
The inclusion of this line in an input file directs SPICE to perform a pole-zero analysis. CUR stands for a transfer function of the type (output voltage)/(input current) while VOL stands for a transfer function of the type (output voltage)/(input voltage). POL stands for pole analysis only, ZER for zero analysis only and PZ for both. This feature is provided mainly because if there is a nonconvergence in finding poles or zeros, then, at least the other can be found. Finally, NODE1 and NODE2 are the two input nodes and NODE3 and NODE4 are the two output nodes. Thus, there is complete freedom regarding the output and input ports and the type of transfer function.
In interactive mode, the command syntax is the same except that the first field is PZ instead of .PZ. To print the results, one should use the command 'print all'.
The distortion analysis portion of SPICE (.DISTO) computes steady-state harmonic and intermodulation products for small input signal magnitudes. If signals of a single frequency are specified as the input to the circuit, the complex values of the second and third harmonics are determined at every point in the circuit. If there are signals of two frequencies input to the circuit, the analysis finds out the complex values of the circuit variables at the sum and difference of the input frequencies, and at the difference of the smaller frequency from the second harmonic of the larger frequency.
Distortion analysis is supported for the following nonlinear devices: diodes (DIO), BJT, JFET, MOSFETs (levels 1, 2, 3, 4/BSIM1, 5/BSIM2, and 6) and MESFETS. All linear devices are automatically supported by distortion analysis. If there are switches present in the circuit, the analysis continues to be accurate provided the switches do not change state under the small excitations used for distortion calculations.
Spice3 will calculate (.SENS) either the DC operating-point sensitivity or the AC small-signal sensitivity of an output variable with respect to all circuit variables, including model parameters. Spice calculates the difference in an output variable (either a node voltage or a branch current) by perturbing each parameter of each device independently. Since the method is a numerical approximation, the results may demonstrate second order affects in highly sensitive parameters, or may fail to show very low but non-zero sensitivity. Further, since each variable is perturb by a small fraction of its value, zero-valued parameters are not analyized (this has the benefit of reducing what is usually a very large amount of data).
The noise analysis portion of SPICE (.NOISE) does analysis device-generated noise for the given circuit. When provided with an input source and an output port, the analysis calculates the noise contributions of each device (and each noise generator within the device) to the output port voltage. It also calculates the input noise to the circuit, equivalent to the output noise referred to the specified input source. This is done for every frequency point in a specified range - the calculated value of the noise corresponds to the spectral density of the circuit variable viewed as a stationary gaussian stochastic process.
After calculating the spectral densities, noise analysis integrates these values over the specified frequency range to arrive at the total noise voltage/current (over this frequency range). This calculated value corresponds to the variance of the circuit variable viewed as a stationary gaussian process.
.NOISE: Noise Analysis
General form:
.NOISE V(OUTPUT [ , REF ] ) SRC [ DEC | LIN | OCT ] PTS FSTART FSTOP
+ [ PTS_PER_SUMMARY ]
Examples:
.NOISE V(5) VIN DEC 10 1kHZ 100Mhz
.NOISE V(5,3) V1 OCT 8 1.0 1.0e6 1
The Noise line does a noise analysis of the circuit. OUTPUT is the node at which the total output noise is desired; if REF is specified, then the noise voltage V(OUTPUT) - V(REF) is calculated. By default, REF is assumed to be ground. SRC is the name of an independent source to which input noise is referred. PTS, FSTART and FSTOP are .AC type parameters that specify the frequency range over which plots are desired. PTS_PER_SUMMARY is an optional integer; if specified, the noise contributions of each noise generator is produced every PTS_PER_SUMMARY frequency points.
The .NOISE control line produces two plots - one for the Noise Spectral Density curves and one for the total Integrated Noise over the specified frequency range. All noise voltages/currents are in squared units (V2/Hz and A2/Hz for spectral density, V2 and A2 for integrated noise).
All input data for SPICE is assumed to have been measured at a nominal temperature of 27°C, which can be changed by use of the TNOM parameter on the .OPTIONS control line. This value can further be overridden for any device which models temperature effects by specifying the TNOM parameter on the model itself. The circuit simulation is performed at a temperature of 27°C, unless overridden by a TEMP parameter on the .OPTIONS control line. Individual instances may further override the circuit temperature through the specification of a TEMP parameter on the instance.
Temperature dependent support is provided for resistors, diodes, JFETs, BJTs, and level 1, 2, and 3 MOSFETs. BSIM (levels 4 and 5) MOSFETs have an alternate temperature dependency scheme which adjusts all of the model parameters before input to SPICE. For details of the BSIM temperature adjustment.
Temperature appears explicitly in the exponential terms of the BJT and diode model equations. In addition, saturation currents have a built-in temperature dependence. The temperature dependence of the saturation current in the BJT models is determined by:
XTI
|T | | E q(T T )|
1 g 1 0
I (T ) = I (T ) |--| exp|-----------|
S 1 S 0
|T | |k (T - T )|
0 1 0
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:
XTB
|T |
1
B(T ) = B(T ) |--|
1 0
|T |
0
where T1 and TT0 are in 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 (spice model parameters BF, ISE, BR, and ISC, respectively).
Temperature dependence of the saturation current in the junction diode model is determined by:
XTI
---
N
|T | | E q(T T ) |
1 g 1 0
I (T ) = I (T ) |--| exp|-------------|
S 1 S 0
|T | |N k (T - T )|
0 1 0
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, U (in spice PHI), for all the device models. The temperature dependence is determined by:
| N N |
a d
kT |------ |
U(T) = -- log 2
q e |N (T) |
i
where k is Boltzmann's constant, q is the electronic charge, Na is the acceptor impurity density, Nd is the donor impurity density, Ni is the intrinsic carrier concentration, and Eg is the energy gap.
Temperature appears explicitly in the value of surface mobility, M0 (or UO), for the MOSFET model. The temperature dependence is determined by:
M (T )
0 0
M (T) = -------
0 1.5
| T|
|--|
|T |
0
The effects of temperature on resistors is modeled by the formula:
R(T) = R(T0 ) [1 + TC1 (T - T0 ) + TC2 (T - T0)2 ]
where T is the circuit temperature, T0 is the nominal temperature, and TC1 and TC2 are the first- and second-order temperature coefficients.
