DC Small Signal Transfer Function - (Not Available in ICAP/4Rx)

The .TF function produces the DC value of the transfer function between any output node and any input source. It also acquires the input resistance looking into the circuit at the source, and the output resistance looking into the output node.

This analysis computes the small signal ratio of the output node to the input source, and the input and output impedances. Any nonlinear models, such as diodes or transistors, are first linearized based on the DC bias point, then the small signal DC analysis is carried out.

(top)

Sensitivity Analysis - (Not Available in ICAP/4Rx)

Sensitivity analysis produces the Operating Point, DC, AC, and Transient sensitivities of any output variable with respect to all circuit parameters, or, the sensitivities of any circuit parameter with respect to any output variable.

There are two sensitivity analysis approaches: traditional SPICE sensitivity and Simulation Templates. Sensitivity is useful when trying to find worst-case circuit operation. By finding the most sensitive components with respect to variation in a design, and moving their values accordingly, a circuit’s more adverse performance can be evaluated. Traditional SPICE sensitivity uses a direct approach to support sensitivity calculations for the DC and AC analyses, wherebythe DC sensitivity is calculated with respect to the DC operating point. IsSpice4 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 effects in highly sensitive components, or may fail to show very low but nonzero sensitivity. Since each variable is perturbed by a small fraction of its value, zero-valued parameters are not analyzed. The output, consisting of the sensitivity of all circuit parameters (values and model parameters) with respect to a named voltage or current, is placed in the IsSpice4 output file.

IsSpice4 supports a more powerful sensitivity analysis using scripted Simulation Templates. AC, DC, Transient, and OP related sensitivities may be obtained for large parameter perturbations using this method. In addition, this version is more flexible and allows more sorting and output options. For example, you can get the sensitivity of any circuit parameter with respect to any output measurement (maximum, minimum, or rise time for any voltage, current, power dissipation waveform, etc.) as well as the opposite; the sensitivity of any output measurement with respect to any circuit parameter. RSS, EVA and Worst Case options are also available when using Simulation Templates. This is the preferred method for sensitivity analysis.

(top)

Noise Analysis - (Not Available in ICAP/4Rx)

Noise analysis computes the integrated noise contributions for each noise generating element in the circuit over the frequency range which is specified in the SPICE Noise statement. It also calculates the level of input noise from the specified input source, which is required to generate the equivalent output noise at a specified output node.

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, the noise analysis integrates these values over the specified frequency range in order to determine the total noise voltage or total noise current. The particular output variables are defined by the Noise analysis statement.

Noise data is stored in the output file in two forms. One is for noise spectral density curves, INOISE and ONOISE, and the other is 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) to maintain consistency and prevent confusion.

Resistors have thermal noise. (Note: To remove a resistor’s thermal noise from the noise calculation, set its temperature to -273.15.) Semiconductor devices have shot, flicker, and burst noise. Capacitors, inductors, and controlled sources are noise-free. Each noise source is assumed to be statistically uncorrelated to the other noise sources in the circuit. Each noise source value is calculated independently. The total noise is the RMS sum of the individual noise contributions.

(top)

Distortion Analysis - (Not Available in ICAP/4Rx)

Distortion analysis computes the steady-state harmonic and inter-modulation products for small input signal magnitudes. Distortion analyses can be performed using linear devices and the following semiconductors; diode, BJT, JFET, MOSFET and MESFET. If there are switches present in the circuit, the analysis will continue to be accurate if the switches do not change state under small excitations, which are used for distortion calculations.

In the distortion analysis, a multidimensional Volterra series analysis is solved using a multidimensional Taylor series to represent the nonlinearities at a specific circuit operating point. Terms are used up to the third order in the series expansions. One of the advantages of the Volterra series technique is that it computes distortions at mix frequencies symbolically (i.e. n F1 ± m F2). It is possible, therefore, to obtain the strengths of distortion components accurately even if the separation between them is very small. The disadvantage is, of course, that if two of the mix frequencies coincide, the results are not merged together and presented. However, this could be done as a post-processing step in Intusoft’s IntuScope waveform processing tool. One will have to keep track of the mix frequencies and add the distortions at coinciding mix frequencies together.

(top)