The AWR® Microwave Office® program makes transient analysis with AWR® APLAC®, and SpectreTM available within the AWR Design Environment® suite. Transient analysis offers an alternative method of nonlinear analysis that complements harmonic balance. You can simply choose a transient simulator for the nonlinear measurement you need. The program performs any translations necessary for running the transient analysis with the selected simulator, reads in the results after the analysis is complete, and calculates the measurement from the results.
This section provides a general description of transient analysis that typically applies to all transient simulators. For detailed information about the operation of the transient simulator that you use, see its documentation.
Transient analysis always begins at time=0, and assumes that only the DC sources were connected to the circuit prior to that time. With the entire circuit properly biased by the DC supplies, the time-varying stimuli are switched on at time=0, and the response of the circuit to them is calculated, time point by time point. The simulation continues for the specified length of time, using step sizes that are determined by the simulator. Transient simulators start with the largest possible time steps, and reduce the size of the steps if they have difficulty converging. For example, if voltages, currents, or charges change too drastically between time-points t and t+delta, a smaller delta is attempted for the new time point.
Transient analysis saves node voltages and branch currents (and capacitor charges, if specified) at each time point in the analysis, so measurements like Vtime and Itime are extracted directly from the raw analysis results. Smaller time steps in transient analysis improve measurement accuracy. Transient simulators automatically take smaller steps when transient events occur. When measuring time domain and transient effects such as rise and fall time, or overshoot, the time domain resolution of the results is clearly indicated in the graph by the waveform of the time domain measurement. Tightening the accuracy requirements specified in the transient simulator options forces the simulator to be more conservative (take smaller time steps) during transient events. There are also simulator options that set maximum limits on step size. Frequency domain measurements such as Pcomp and Vharm (and others that are dependent on them, like PAE and IPn) are calculated from Fourier transforms of the transient analysis results. Accurate frequency domain measurements from transient simulations require at least one period of well-resolved, steady-state time domain results. These terms are further described:
The full set of frequency domain measurements are available for transient simulation of circuits that do not oscillate; for these, the period is a function of the input stimulus frequency(ies). The period T is the smallest value that is an integer multiple of every stimulus period. Another way to describe the period is T=1/F0 where F0 is the largest frequency such that every stimulus frequency is an integer multiple of it; i.e. FSi=Ni*F0, where FSi are stimulus frequencies and Ni are integers. For transient simulation of oscillating circuits, there is a set of FFT-based frequency domain measurements (for example, Vfft and Pspec), and the period is determined from the results. For more information, see the Help associated with these measurements.
Steady state is reached when the behavior of the circuit is identical from
one period to the next. Note that circuits can contain elements with very
large time constants, relative to the frequency of operation, so it may be
difficult to notice the difference between periods. See the
Basic_Transient.emp project in the AWR Microwave Office
/Examples directory for an example.
For frequency domain measurements, the maximum step size is typically 1/(25*FH), where FH is the highest significant harmonic frequency. Note that harmonic balance analysis is much better suited for measuring harmonic components, because it has a greater dynamic range (lower noise floor) than transient analysis.
Transient simulators save every voltage and current at every time point and every node (by default), so if a large circuit is analyzed for a very long time with a very small time step, it can generate a great deal of data. This is common in oscillator simulation where you don't know how long the oscillator will take to start up. Every node is saved by default, so you can probe around a circuit after simulation is complete to see data at each node with no new simulation required. In such cases, you should restrict the amount of data saved, because large data files take longer to process when calculating and displaying the measurements. In extreme cases, the data file size can use up all of the available memory.
There are three ways to reduce the amount of data saved: reduce the length of the simulated time over which data is saved, save fewer time points to reduce the "length" of the data, and/or reduce the number of variables that are saved (the "width" of the data).
The Circuit Options dialog box APLAC Sim tab provides an option that offers two ways of controlling the length of the data. The simulated time and maximum step size can be set, either by specifying the number of periods and using the harmonic balance settings, or by specifying the start and stop times, and the step size. As previously stated, all transient simulations start at time=0, so the start time is the time at which data begins to be saved. Data from previous time points is not recorded. This can reduce the data file size considerably, by excluding undesired transient effects in the early part of the analysis. Each transient simulator may treat the step value slightly differently; for example, one may use the specified step size as the maximum and another may save simulation results only at those steps. Generally, however, increasing the step size reduces resolution, and reduces the data saved. The individual options for each simulator allow greater control over the resolution of the saved data.
You can use the Save currents and Save voltages options on the Circuit Options dialog box APLAC Sim tab to reduce the width of the data (such as saving results at only ports or probes).
Nonlinear simulations are difficult for circuits containing loops consisting of inductors and voltage sources (inductor loops), or cutsets of capacitors and/or current sources only (capacitor cutsets). An inductor loop that is not obvious can result when short lossless transmission lines are modeled using LC Pi lumped subcircuits.
Each node in the circuit should have a DC path to ground. Many model translations add a 1 GOhm resistor to ground to avoid violating this rule, but there are other means. For example, if a set of elements is separated from the rest of the circuit (and ground) but not disabled, it creates a set of nodes with "No DC path to ground".
Some transient simulators issue errors in a AWR Microwave Office message window if any of these requirements are not satisfied. You can double-click an error message to identify one of the schematic elements in the offending loop or cutset.
AC sources (ports, voltage and current sources) are set up by default to run with both harmonic balance and transient simulators. Many of the sources will have a tone parameter (it may be a secondary parameter) that is only used by harmonic balance. When harmonic balance runs, it must determine all the frequencies that must be simulated. With combinations of several sources, determining these frequencies can take a significant amount of time and memory. Many sources can be set up to only run with transient simulators by setting the tone number to 0. The AC_V, AC_I, and PORT_SRC elements have specific modes for transient only. See “Dynamic AC Current Source: AC_I”, “Dynamic AC Voltage Source: AC_V”, and “Dynamic Source Port: PORT_SRC” for more details. If you are always running transient simulations, you can set all tone settings to 0 to simplify setting up your sources.
For historical reasons, not all sources will have a tone parameter. For example, the simplest AC source is the ACCS element which is hard-coded to be a tone 1 source. The ACCS2 is identical except hard-coded to be tone 2. However, there is an ACCSN source where you can specify the tone required. The most generic sources are the AC_V, AC_I, and PORT_SRC elements since they can be configured for any signal type and any tone number. However, if you want to use other sources, the following is a list of all sources with a settable tone number.
Note that the convergence to a steady state is fastest if the zero time value of the periodic stimulus is equal to its average value. Most transient simulators use a standard formula for sinusoidal sources, V(t)=Asin(ωt+φ), which means sources with φ≠0 include an offset at t=0 that may take a long time to dissipate. By default, AWR Microwave Office software translates this phase into a delay, so that the phase relationships between sources are maintained, but the initial value for all sinusoidal sources is their average value. To change this default behavior, choose Options > Default Circuit Options to display the Circuit Options dialog box. Click the tab corresponding to your transient simulator, and in the Transient Options section under Result Collection, clear the Use delay for angle check box.
At RF and microwave frequencies, accurate models are needed for both active devices (FETs, BJTs, diodes) and distributed devices such as transmission lines with discontinuities, couplers, baluns, and vias. These distributed elements must be modeled properly; simplified lumped element network models are not adequate for realistic simulation results.
For purely linear, frequency domain models, harmonic balance simulation is equivalent to Fourier analysis, and provides the most accurate reference solution. It is traditionally used to establish accuracy of the transient simulations with non-trivial models, such as frequency-dependent distributed models. At the same time, transient simulations are the reference, as harmonic balance simulations become difficult with complex input waveforms and large numbers of nonlinear models (FETs, bipolar transistors, diodes). Due to the attributes of each simulation type, comparison of transient and harmonic balance simulation results may help establish model accuracy, and gain confidence in model quality.
While harmonic balance simulations calculate the steady state of the circuit being simulated, and transient simulations follow the transient process, there are two conditions under which the results of these simulations can be expected to agree:
Transient simulations run to steady state
Pseudo-transient simulations performed in harmonic balance with a large time period (small fundamental frequency).
In the first condition, transient simulations are run long enough for the transients to die out so that the steady state is reached. Since the stimuli are periodic, the simulation length should be equal to an integer number of periods (nT). The convergence to steady state is monitored by comparing the results for period number n-1 and period n. If the results are sufficiently close (within the specified tolerance), the simulation is deemed to converge to the steady state, otherwise n must be increased.
In the second condition, simulations with pulse voltage sources (more generally, functions with finite support) are performed. The period for harmonic balance simulations is chosen sufficiently large enough to allow the transient process to complete within that period. To accurately model fast rise/fall time with such a large artificial period, a large number of harmonics must be chosen.
A typical test circuit involves a pulse voltage source with Tr=Tf=0.1ns (or 0.05 ns), a pulse width of 2 ns, and a period of 10 ns (fundamental frequency of f=0.1 Ghz). For the first tone, 4096 harmonics are used, and a 0 setting is used for all other tones. This large number of harmonics ensures that the Fourier series for the expansion of the voltage source converged within six decimal places of accuracy to the exact function. You can use a smaller number of harmonics (resulting in lower accuracy) but it should be several hundred at minimum. The transient process has to finish in the 8 ns between the end of the falling edge of the pulse and the beginning of the rising edge of the following pulse.
Note that with the first method the transient simulations take a long time, while with the second method the harmonic balance simulations take a long time.
All models intended for use in transient simulations must be causal (having a response that does not appear before the stimulus).
For models specified as the frequency-dependent admittance matrix Y(ω), the causality requirement can be expressed as:
In this expression,
P.V. represents the Cauchy principal
value of the integral. It is well known that the imaginary part of Y(w) should be an
odd function and equal to zero at zero frequency, and that the real part Re[Y(w)]
should be an even function. If the real part is constant as a function of frequency,
the imaginary part is required to be exactly zero.
Non-causal models are not translated into transient simulators unless a causality correction is possible. If a circuit contains such a model, an error message displays and the transient simulation is not performed.
Although harmonic balance simulations are possible with negative resistances, capacitances, and inductances, transient simulations of such circuits almost certainly diverge. This is not a fault of the transient simulator or the model translation, but a reflection of the fact that the solution of circuit equations with negative R, L, C is quite often a function that tends to infinity. Of course, negative R, L, and C are unphysical ("do not exist"). The negative slope of dV/dI of a V-I curve of a device is not the same as negative R.
Non-causal lumped models (for example, frequency-independent complex admittance ADMIT, frequency-independent complex impedance IMPED, and QHYB) are not translated into transient simulators. You should replace these models with causal models for transient simulations. For example, a frequency-dependent complex impedance model (ZFREQ) is causal if the real and imaginary parts are specified correctly, and you can use it for transient simulations.
Some software that matches circuit parameters of fixed topology subcircuits to the frequency-dependent S- or Y-parameters as a function of frequency may end up with subcircuits containing negative R, L, and C. This match is of no use in transient simulations. AWR Microwave Office software contains code that takes the S- or Y- parameters of a device and produces subcircuits suitable for transient simulations.
Several lumped models in the AWR Microwave Office program are causal for particular values of parameters. For example, the controlled sources (VCVS, VCCS, CCVS, CCCS) with frequency roll-off of the coefficient
are causal, provided A=0 or π. In this case, you can use them in transient simulations for these parameter values, and an error message displays for the parameter values that violate the causality condition (A≠0 or π, in this example). The code also rejects the case of A=π and you must set A=0 and change the sign of M if A=π is desired.
AWR Microwave Office software can perform accurate transient simulations with transmission line models that have frequency-dependent parameters.
There are several controls for transient simulations with transmission lines. You can choose an option to perform an accurate simulation of transmission lines (all or individually), or use various approximations. Choose Options > Default Circuit Options and click the APLAC Sim tab on the Circuit Options dialog box to access the SPICE Model Extraction options.
For the most accurate simulation results, select Level 3 - Distributed or Level 4 - Most accurate available.
All of the other transmission line modeling options are approximations that may be adequate in some cases but are generally less accurate and inadequate in other cases. These options are useful for preliminary work such as layout verification or determining the correct bias condition for transistors.
If you select Level 3 - Distributed or Level 4 - Most accurate available, the R,L,C,G, Table Generation options become relevant.
You can easily verify the accuracy of transient simulations with transmission line models by setting up a small linear circuit and comparing transient results to harmonic balance results according to the second condition discussed in “Multi-rate (Nonlinear) Harmonic Balance Analysis”. If you plan to use approximate transmission line models, you should study the effect of these approximations by setting up a small test circuit and comparing the result of the approximations to the accurate result.
NOTE: Transient simulations with transmission lines of negative length (or with negative delay) are impossible, as such models are non-causal. Some transmission line models issue an error message to this effect if transient simulations are attempted.
There is one more causality requirement for transient simulation of transmission line models. The characteristic admittance Yo and the characteristic impedance Zo=Yo-1 need to be causal functions of frequency such that the Hilbert transform or the real part is equal to the imaginary part. This condition is violated for several AWR Microwave Office models such as MCLIN (coupled microstrip line). In this case, transient simulations are performed not for the original model but for the model corrected for causality. In these cases you see disagreement between harmonic balance and transient simulations. Furthermore, in some rare cases a divergence of transient simulations with non-causal transmission line models may occur.
Short transmission lines have the effect of restricting the time step of transient simulations such that the time step cannot exceed the propagation delay of the fastest mode of the transmission line. Recognizing this, the translation uses a lumped approximation (RLC-Pi circuit) for transmission lines with electrical length less than MaxDelayFraction of the period of the MaxFrequency (maximum frequency of interest).
The AWR Microwave Office program supports accurate transient simulations with behavioral lumped filter models (located in General > Filters group in the Element Browser). Lowpass, highpass, bandpass, and bandstop filters of Butterworth, Elliptic, Chebyshev, and Bessel type are supported. In addition, an accurate translation is available for the Distributed Lowpass Butterworth Filter.
Transient simulations with realistic Q-factor of the filter are easier (for example, converge faster) than those with nearly infinite Q (such as Q=1012).
Translation of the filter models uses the exact 2 x 2 admittance matrix Y(s) that is represented by four VCCSs with frequency-dependent transconductance. No fitting of any kind takes place in obtaining equivalent models for the lumped filters. No additional circuit nodes are created for behavioral filter models, thus resulting in efficient transient simulations.
HB simulations are possible with sources specified as discontinuous (zero rise or fall time), such as a rectangular pulse or a saw-tooth signal. Nevertheless, transient simulations with discontinuities in the stimuli are not advised. They may work for lumped circuits, but not for distributed circuits. If you specify zero rise or fall time of a source, it is replaced with 1/Maximum Frequency, where Maximum Frequency is the maximum frequency used for extraction of transmission line models, and a related warning message displays. Any other positive value you specify is accepted as is. You can set Maximum frequency in the R,L,C,G Table Generation section of the Circuit Options dialog box APLAC Sim tab.
You may want to obtain the unit step response of a circuit. In this case it is necessary to choose a non-zero rise time that is sufficiently small so the result is close enough to the unit step response, yet large enough to avoid convergence problems. The exact value depends on the specific circuit, and is usually established by trial and error. An initial value of "Tr=1/ Maximum Frequency" is recommended for this trial and error procedure.
The following models with frequency-dependent Q factor in the form of
are translated for transient analysis with the simplifying assumption a=1: CAPQ, INDQ, PLCQ, SLCQ, CHIPCAP, CHIPCAP2.
The capacitor models from Dielectric Laboratories, Inc., (BOARDCAP, CHIPCAP, DICAP, GAPCAP, and MULTCAP) are modeled as a linear capacitor unless you select Level 4 - Most accurate available as the SPICE model extraction option, in which case a rational approximation is used.
The AWR Microwave Office program supports transient simulation of models specified by their S-, Y-, or Z-parameters as a function of frequency (for example, Touchstone format .sNp files). You can choose two fundamental methods to perform transient simulations with these models:
rational approximation with subsequent equivalent circuit generation (default)
numerical convolution (with four different settings which may work best in a particular case).
For successful simulation, the following requirements must be satisfied:
The device model must be causal. Solutions of Maxwell equations are causal, so if the model is obtained using a field solver with sufficiently accurate settings, it should be causal. Multiple publications deal with the subject of testing causality of experimental data (also referred to a Kramers-Kronig relation).
The number of frequency samples must be sufficient to resolve the resonances in the frequency range of interest. This is easily judged by plotting the frequency dependence in X-Y plot. You should plot the frequency dependence of the matrix elements of the short-circuit admittance matrix Y, as this is the matrix that forms the stamp for modified nodal analysis.
The number of frequency samples should be sufficient for the linear system of equations to be over-determined. Generally, this means no less than 50 frequency points, however it can be less for very simple frequency-dependence. If the numerical convolution is used, the required number of frequency samples is even greater. In this case, the simulator code interpolates linearly between the frequency samples, and the results should still be sufficiently accurate.
The value at DC is very desirable. It is usually easy to calculate-- no field solver is needed.
Transient simulation of these devices is controlled in the Element Options dialog box on the Model Options tab. Right-click the subcircuit in the schematic and choose Properties to display the Element Options dialog box, then click the Model Options tab. See “Element Options Dialog Box: (Subcircuit) Model Options Tab” for more information.
Three groups of options are available: use of rational approximation of the Y matrix, rational approximation of the S matrix directly, or use of numerical convolution implemented in the transient simulator itself. In case of rational approximation to either the Y or S matrix, the passivity of the generated approximation is enforced, and an equivalent circuit for the simulator is generated using Voltage Controlled Current Sources with the s-dependence in a form that is supported by the simulator. The aim of the models is accurate but efficient transient simulation; adding the fewest sources and internal nodes. The availability of advanced frequency domain controlled sources in some simulators makes the usage of VCCS far superior to generating the equivalent circuit with R, L, C, K elements.
Testing has demonstrated that in the majority of cases the rational approximation yields a more accurate transient simulation, and a far superior simulation performance for long transient simulations than the convolution.
If rational approximation is selected, the code first checks the passivity of the model specified by the Touchstone file or an EM structure. Passivity in this context refers to the N-port absorbing active power delivered to it at all the frequencies given in the Touchstone file or EM structure. The lack of passivity means that the N-port has an internal power source and is capable of delivering active power to the rest of the circuit. Formally the passivity test is equivalent to establishing the positive-definiteness of the matrix G=Re Y at all frequencies of interest. The same passivity criterion can be expressed in terms of the scattering matrix S, and states that eigenvalues of the matrix A=U-SHS should be non-negative. In this expression, U is the identity (unit) matrix, and the superscript "H" denotes Hermitian-conjugate of the matrix. A Linear/PASSIVE measurement is available to help you determine at which frequencies the model is non-passive, and the magnitude of passivity violation.
If the passivity check is enabled and finds the model to be non-passive, the code switches to use of direct numerical convolution. There are three possible reasons for the lack of passivity in the model:
A systematic error in the measurements or EM simulation if the N-port represents a linear passive device, such as a portion of interconnect, or a coupler
Numerical errors in EM simulations and unavoidable random measurement errors
The model represents an N-port device that has an internal power source (for example an amplifier described by its S-parameters). In this case, S-parameter description is a rough approximation that may or may not be adequate for a particular transient simulation. In the amplifier example, the model amplifier is linear regardless of the magnitude of the input signal, while in practice the linearity can be reasonably assumed only for a particular range of the amplitudes.
A small passivity violation can still occur for the model that is intended to be passive (such as interconnect), due to the numerical errors of EM simulations or experimental errors. You can override (skip) passivity checks by selecting a Make passiveoption. If the results were obtained from EM simulations, you should check the results by using PASSIVE measurements. If the passivity violation is found to be small, AWR® recommends overriding the passivity check by using the corresponding setting. If the passivity violation is found to be large, you should review the EM simulation settings or experimental setup for systematic errors.
Testing has shown that Advanced Band Synthesis of the Sonnet EM solver often yields small passivity violations as previously described. In such cases you can override the passivity check by selecting the Make passiveoption.
Using the rational approximation approach (the code developed by AWR) is recommended for transient simulations of passive devices specified by frequency-dependent S-parameters. The following are the advantages of the rational approximation approach:
Results of transient simulations are often much more accurate than those of numerical convolution.
Fewer data samples are needed (still resonances need to be resolved). The non-uniform grid of frequency points is handled well, and is recommended (more points near the resonances to resolve them, and fewer points where the Y or S matrix varies slowly).
After an initial cost of obtaining the rational approximations, the simulations are much faster. The CPU time-scales linearly with the length of transient simulations (not quadratically as is the case for numerical convolution).
To use the rational approximation approach, select an option under Fitting to Y Parameters or Fitting to S Parameters. You cannot use this approach for active devices. If the lack of passivity is detected, the code automatically switches to the usage of numerical convolution, but you can override passivity checks by selecting Make passiveoptions that skip them.
Typically, for models that correspond to interconnect, it is beneficial to fit directly to S parameters using one of the Fitting to S parameters options. If the EM simulations were performed with ideal conductors (zero resistivity), fitting to S parameters is strongly recommended. Fitting to Y parameters does not work well. Fitting to S parameters is also recommended for large N-ports (number of ports N>4), and N-ports with large electrical length (delay between ports).
When fitting to S parameters, passivity of the resulting rational approximation can be enforced either from f=0 (DC) to the maximum frequency given for the model (for the Use Convolution if not passive options and Make passive in band option, or for the entire frequency axes Make passive everywhere option). Normally, it is sufficient to enforce passivity for the frequency range of interest, as the power content outside that frequency range is negligible. However, on rare occasions you might encounter transient simulations diverging with the diagnostic "Internal time step too small in transient simulations". If this occurs, you should select Make passive everywhere under Fit to S Parameters to fix the problem. Note that using Make passive everywhere increases the time necessary to construct the rational approximation, and may cause a slight decrease in the accuracy of approximation.
Fitting to Y parameters may provide more accurate results of transient simulations for small N-ports with significant coupling, such as spiral inductors. This setting works well if the f=0 (DC) result is available, and may also require a number of low frequency data points to be provided, as Y matrix exhibits fast variation as a function of frequency near DC. Most available EM solvers cannot perform simulation at f=0 (DC), and there is a practical limit on the minimum frequency fmin at which the EM simulations can be performed (fmin=1 MHz for EMSight). Extrapolation to DC from the lowest available frequency works better for S parameters than for Y parameters due to more smooth frequency variation. Fitting to Y parameters is the method of choice for the optimal distribution of frequency samples; however, in less than ideal situations, fitting to S parameters is often preferable. For historic reasons, fitting to Y parameters remains the default.
The passivity criterion used are very strict, and it is common to override a passivity check that is intended to prevent using rational approximation with devices that are active by intent, and to alert a user if there are large passivity violations for the devices that are passive by intent (such as interconnect). Unlike small passivity violations (see the Help for the Linear > PASSIVE measurement for guidelines on which passivity violations are considered "small" and "large"), significant passivity violations indicate a serious problem with EM simulations or measurements and disqualify the results from being used.
The rational approximation approach involves obtaining the rational approximation for the given frequency-dependence of Y matrix in the form of
with the same set of poles for all matrix elements where
A'i is complex conjugate of
Ai. The fitting proceeds in two stages. First the common
set of poles is determined, and then the residues
Ai for each matrix element
are found. 
This form assures causality and stability (as all poles are selected such that Re pi<0). Furthermore, the passivity condition expressed as positive-definiteness of G=Re Y is enforced for all frequencies in the file.
When fitting to Y matrix, the code starts with NP=20 pairs of complex conjugate poles, and may reduce the number of poles for simple frequency dependencies. Fitting of the rational approximation in the form (1) requires that the system of equations be overdetermined. If the number of frequency samples is insufficient, a warning message displays and the number of pole pairs is reduced. The success of fitting in this case is not guaranteed and you are encouraged to provide more frequency samples. Obtaining more frequency samples by interpolation between the available samples is not advised as it does not provide any new useful information. A rational approximation in form (1), even with the reduced number of poles, is a far superior way to interpolate frequency dependencies than linear or even spline interpolation.
For the S matrix approximation, the approximation is obtained for each matrix element individually, with each having its own set of poles. The number of poles to use is determined dynamically, based on the complexity of the dependence to be approximated, and the quality of the obtained approximation. The code can automatically increase the order of approximation if needed, or decrease it to avoid "overfitting". As a result, rational approximation of S matrix requires fewer frequency samples, and takes less time. Since this approach involves fitting each matrix element individually, fitting to S matrix works well for large N-ports.
When simulating the propagation of digital signals through distributed devices ("pulses propagating through interconnect"), you may need to override the default Use HB settings on the APLAC Sim tab of the Circuit Options dialog box, and specify the transient time step explicitly. Transient simulators usually use variable time steps with sophisticated time step control, but an unreasonable starting value in Step time can still yield poor results, or even divergence.
The optimal setting for the transient time step Step time varies depending on the circuit, but general guidelines can be provided. If Tr is the rise time, and Tf is the fall time of the pulse, a reasonable setting for Step time ranges from 0.1 min(Tr, Tf) to 0.01 min (Tr, Tf). You can often get good results with a relatively large time step of about 0.1 min(Tr, Tf).
If Use HB settings is selected in this example, the initial step is determined as 1/(4 f0 Nh), where f0 is the fundamental frequency, and Nh is the number of harmonics specified on the APLAC Sim tab. For a reasonable case, for the period T= 4 ns, Nh=5 (default setting in a new project), the result is f0=0.25 GHz. The time step would be 0.2 ns, which is unsatisfactory.
Since Tr=0.1 ns, you can reasonably assume that providing the frequency response from f=0 (DC, or as close to DC as possible, for example, 1 MHz) up to fM=1/Tr=10 GHz is sufficient with high accuracy. Nevertheless, it is wise to provide results for the N-port parameters (S or Y parameters) from 0 to 2 fM. Note that some out-of-band frequency samples are needed to ensure passivity of the generated rational approximation. Generally, if the range of interest is from 0 to fM, provide the samples from 0 to approximately 2fM, with more coarse grid for f > fM.
For SPECTRE, the AWR Design Environment software uses a consistent circuit description, regardless of the analysis type: linear, AC, or transient. Models are always translated (if necessary) so they can be simulated with SPECTRE transient simulator. This provides an excellent opportunity to compare the behavior of a distributed AWR model in the simulator of choice, to its original implementation in the AWR simulators. For example, you can plot the port parameters (or other linear measurement) using the default and SPECTRE linear simulators, on the same graph, and compare the two to see the impact of the rational approximation on the model.
When an analysis is run that includes an APLAC measurement, an APLAC netlist is
created in the application data folder in the default location:
Environment\15.0\temp\"Project_Name"\"Schematic_Name"\. You can access
these netlists by clicking the respective link in the Status Window upon simulation
completion. When the analysis is complete, results files are also written to the same
directory. Note that these files are overwritten with each analysis, so you must move
them to a different location if you want to save files from a specific analysis.
 For information on the optimal approach for determining the common set of poles, see B. Gustavsen: "Computer code for rational approximation of frequency-dependent admittance matrices", IEEE Trans. on Power Delivery, vol. 17. no. 3, pp. 1093-1098, October 2002.