DC Analysis
AC Analysis
Transient Analysis
Analysis at Different Temperatures
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.
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.
The transient analysis portion of SPICE computes the transient output variables as a function of time over a user specified time interval. The initial conditions are automatically determined by a dc analysis. All sources which are not time dependent (for example, power supplies) are set to their dc value. For large-signal sinusoidal simulations, a Fourier analysis of the output waveform can be specified to obtain the frequency domain Fourier coefficients. The transient time interval and the Fourier analysis options are specified on the .TRAN and .FOURIER control lines.
All input data for SPICE is assumed to have been measured at 27 deg C (300 deg K). The simulation also assumes a nominal temperature of 27 deg C. The circuit can be simulated at other temperatures by using a .TEMP control line.
Temperature appears explicitly in the exponential terms of the BJT and diode model equations. In addition, saturation currents have a built-in temperature dependence. The temperature dependence of the saturation current in the BJT models is 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 formula:
value(TEMP) = value(TNOM)*(1+TC1*(TEMP-TNOM)+TC2*(TEMP-TNOM)**2))
where TEMP is the circuit temperature, TNOM is the nominal temperature, and TC1 and TC2 are the first- and second-order temperature coefficients.