Simulation and Optimization Controllers

Data Flow Simulation Controller

Use the Data Flow controller to control the flow of mixed numeric and timed signals for all digital signal processing simulations within Advanced Design System. This controller works with the sink components to provide you flexibility to control the duration of the simulation globally or locally.

While you can no longer place multiple controllers on the schematic to simulate the same design with different controller parameters, you can achieve the same functionality by using single-point sweeps on the parameter you are interested in varying.

DC Simulation Controller

The DC controller provides for both single-point and swept simulations. Swept variables can be related to voltage or current source values, or to other component parameter values. By performing a DC swept bias or a swept variable simulation, you can check the operating point of the circuit against a swept parameter such as temperature or bias supply voltage.

Use the DC controller to:

• Verify the proper DC operating characteristics of the design under test.
• Determine the power consumption of your circuit.
• Verify model parameters by comparing the DC transfer characteristics (I-V curves) of the model with actual measurements.
• Display voltages and currents after a simulation.

A DC simulation is the first analysis for most other analyses. It uses a system of nonlinear ordinary differential equations (ODEs) to solve for an equilibrium point in the linear/nonlinear algebraic equations that describe a circuit once:

• Independent sources are constant valued
• Capacitors and similar items are replaced with open circuits
• Inductors and similar items are replaced with short circuits
• Time-derivatives are constant (zero)

Linear elements are replaced by their conductance at zero frequency

AC Simulation Controller

A linear AC analysis is a small-signal analysis. For this analysis the DC operating point is found first and then the nonlinear devices are linearized around that operating point. Small-signal AC simulation is also performed before a harmonic-balance (spectral) simulation to generate an initial guess at the final solution.

Use the AC controller to:

• Perform a swept-frequency or swept-variable small-signal linear A simulation.
• Obtain small-signal transfer parameters, such as voltage gain, current gain, transimpedance, transadmittance, and linear noise.

An AC simulation also offers a linear noise simulation option that can include the following noise contributions in its simulation:

• Temperature-dependent thermal noise from lossy passive elements, including those specified by data files.
• Temperature and bias-dependent noise from nonlinear devices.
• Noise from linear active devices specified by two-port data files that include noise parameters.
• Noise from noise source elements.

The noise simulation computes the noise generated by each element, and then determines how that noise affects the noise properties of the network.

S-Parameter Simulation Controller

The S-Parameter controller is used to define the signal-wave response of an n-port electrical element at a given frequency. It is a type of small-signal AC simulation that is most commonly used to characterize a passive RF component and establish the small-signal characteristics of a device at a specific bias and temperature.

Use the S-Parameter controller to:

• Obtain the scattering parameters (S-parameters) of a component or circuit, and convert the parameters to Y- or Z-parameters.
• Plot, for example, the variations in swept-frequency S-parameters with respect to another changing variable.
• Simulate group delay.
• Simulate linear noise.
• Simulate the effects of frequency conversion on small-signal
• S-parameters in a circuit employing a mixer.

S-parameter simulation normally considers only the source frequency in a noise analysis. Use the Enable AC Frequency Conversion option if you also want to consider the frequency from a mixer's upper or lower sideband.

Harmonic Balance Simulation Controller

The Harmonic Balance controller is best suited for simulating analog RF and microwave circuits. It is a frequency-domain analysis technique for simulating distortion in nonlinear circuits and systems. Within the context of high-frequency circuit and system simulation, harmonic balance offers the following benefits over conventional time-domain transient analysis:

• It captures the steady-state spectral response directly.
• Many linear models are best represented in the frequency domain at high frequencies.
• The frequency integration required for transient analysis is prohibitive in many practical cases.

Use the Harmonic Balance controller to:

• Determine the spectral content of voltages or currents.
• Compute quantities such as third-order intercept points, total harmonic distortion, and intermodulation distortion components.
• Perform power amplifier load-pull contour analyses.
• Perform nonlinear noise analysis.

Harmonic Balance enables the multitone simulation of circuits that exhibit intermodulation frequency conversion, including frequency conversion between harmonics. It is an iterative method that assumes that for a given sinusoidal excitation there exists a steady-state solution that can be approximated to a satisfactory accuracy.

Simulation Overview

Harmonic balance is a frequency-domain analysis technique for simulating distortion in nonlinear circuits and systems. It obtains the frequency-domain voltages and currents to calculate the spectral content of voltages or currents in the circuit. The harmonic balance method is iterative. It is based on the assumption that for a given sinusoidal excitation there exists a steady-state solution that can be approximated to satisfactory accuracy by means of a finite Fourier series.

The Harmonic Balance solution is approximated by truncated Fourier series and this method is inherently incapable of representing transient behavior. The time-derivative can be computed exactly with boundary conditions, v(0)=v(t), automatically satisfied for all iterates.

The truncated Fourier approximation + N circuit equations results in a residual function that is minimized.
N x M nonlinear algebraic equations are solved for the Fourier coefficients using Newton's method and the inner linear problem is solved by:

• Direct method (Gaussian elimination) for small problems
• Krylov-subspace method (e.g. GMRES) for larger problems

Nonlinear devices (transistors, diodes, etc.) in Harmonic Balance are evaluated (sampled) in the time-domain and converted to frequency-domain via the FFT.

Advantages

• Harmonic balance captures the steady-state spectral response directly while conventional transient methods need to integrate over many periods of the lowest-frequency sinusoid to reach steady state.
• Harmonic balance is faster at solving typical high-frequency problems that transient analysis can't solve accurately or can only do so at prohibitive costs.
• Harmonic balance is more accurate at solving high frequencies where many linear models are best represented in the frequency domain.

Convergence

Nonconvergence is a numerical problem encountered by the harmonic balance simulator when it cannot reach a solution, within a given tolerance, after a given number of numerical iterations. There is no one specific solution for solving convergence problems. However, consider the following guidelines:

• Increase the Order (or other harmonic controls); this is the most basic technique for solving convergence problems, if the time penalty for doing so is acceptable.
• Use the Status server window as the main tool in solving convergence problems (set StatusLevel=4). For each Newton iteration the L-1 norm of the residuals throughout the circuit is printed: a "*" indicates a full Newton step (vs. a Samanskii step).
• Convergence criteria are controlled by Voltage relative tolerance, and Current relative tolerance (in the Options component, under the Convergence tab). In general, convergence speed is improved by increasing these values, but at the expense of accuracy. Similarly, the smaller these values are, the more accurate the results but the slower the convergence.
• Newton convergence issues with Krylov methods (because linear problem solutions can only approximate) can be improved by using better preconditioners.
• Set the Oversample parameter to a value greater than 1.0, such as 2.0 or 4.0. However, remember that although this can often solve convergence problems, it does so at the cost of computer memory and simulation time. For multiple-tone harmonic balance simulations, make sure that the largest signal in the circuit is assigned to Freq[1]. The simulator's FFT algorithm is set up so that aliasing errors are much less likely to affect Freq[1] than any other tone.
• When using a direct linear solver, the blocks of the Harmonic Balance Jacobian inherit the Jacobian matrix ordering from the DC solution process. This matrix ordering can greatly affect the efficiency of the Harmonic Balance Jacobian factorization, and in some circuits show noticeable simulation slowdown. To circumvent this issue, use a DC convergence mode that hasn't changed, e.g. DC_ConvMode=3.
• For non-convergence due to tight tolerances, monitor the residuals in the Status Server window.
  • Increase I_AbsTol if the circuit is converging to within a few pA but not quite to
    I_AbsTol=1pA
  • Increase I_RelTol if the problem is with nodes associated with large currents
  • Increase I_AbsTol if the small current nodes are the issue
  • Relax voltage tolerances for failure in the Newton update criterion
• The internal circuit simulator engine in ADS (Gemini) runs from a netlist. ADS writes a netlist file (netlist.log) before invoking Gemini. The order of the components and model definitions in the netlist determine the initial Jacobian matrix ordering. This matrix ordering can affect the efficiency of the Jacobian factorization and cause either a simulation slow down or non-convergence.
• For convergence problems due to errors in the component model equations (incorrect derivatives, etc.) make sure ancient Berkeley MOSFET Level 1, 2, 3 are not the culprit and that the latest model version is used (especially BSIM3 models). Model problems can cause the Newton residual to hit a threshold (greater than the convergence criteria tolerances) and stale the convergence process or even exhibit random jumps (sudden increase in value). Set the device's Xqc parameter to a nonzero value to allow the simulator to use a charge-based model for the gate capacitance. This often enables convergence, but at the cost of extracting an extra SPICE model parameter.

Sweeps as Convergence Tools

Continuation methods provide a sequence of initial guesses that are sufficiently close to the solution to assure Newton's method convergence in Harmonic Balance. Sweeps can be used to formulate a specialized continuation method geared towards the particular circuit problem.

Sweep a circuit element that, when set to some different value, makes the circuit more linear. For instance, in an amplifier circuit there may be a resistor that can be used to lower the amplifier's gain. The simulator may be able to find a solution to the circuit under a low-gain condition. Then, if the component's value is swept toward the desired value, the simulator may be able to find a final solution. Start with a value that works, and stop with the desired value. Also, select Restart, under the Params tab. Usually, a better initial guess at each step helps the simulator to converge.

The two main ways to perform sweeps are:

• HB sweep within the HB controller. This is preferred for most sweeps, except frequency.
• Parameter sweep using a separate sweep controller.

Convergence and Samanskii Steps

The Samanskii steps can significantly speed up the solution process. However, using an approximate Jacobian, particularly for a larger number of iterations, may result in poor or even no convergence. The constant is used in two ways. First, it becomes a more absolute measure when it is smaller. It then approaches the requirement that each iteration reduces the relevant norm by one-third.

Decreasing the Samanskii constant beyond a certain point (which in turn depends on the quality of the most recent Newton step) will make no difference. However, setting the Samanskii constant to zero will effectively disable any Samanskii steps altogether.

Increasing the Samanskii constant relaxes this requirements in general, but the condition becomes more dependent on the quality of the standard most recent Newton iteration. In other words, a more rapid convergence of the Newton step would also require better convergence of the Samanskii steps.

Convergence and Arc-Length Continuation

Arc-length continuation is an extremely robust algorithm. If it fails, try all other convergence remedies first before adjusting arc-length parameters

• MaxStepRatio controls the maximum number of continuation steps (default 100)
• MaxShrinkage controls the minimum size of the arc-length step (default 1e-5)
• ArcMaxStep limits the maximum size of the arc-length step (default is 0, i.e. no limiting)
• ArcMinValue & ArcMaxValue define the allowed range for the variation of the continuation parameter

Circuit Envelope Simulation Controller

The Circuit Envelope controller is best suited for a fast and complete analysis of complex signals such as digitally modulated RF signals. It combines features of time and frequency-domain representation by permitting input waveforms to be represented in the frequency domain as RF carriers, with modulation "envelopes" that are represented in the time domain.

Circuit Envelope is highly efficient in analyzing circuits with digitally modulated signals, because the transient simulation takes place only around the carrier and its harmonics. In addition, its calculations are not made where the spectrum is empty.

• It is faster than Harmonic Balance, for a given complex signal Spice, assuming most of the frequency spectrum is empty
• It does not compromise in Signal complexity, unlike time-varying HB or Shooting Method Component accuracy, unlike Spice, Shooting Method, or DSP
• It adds physical analog/RF performance to DSP/system simulation with real-time co-simulation with ADS Ptolemy
• It is integrated in same design environment as RF, Spice, DSP, electromagnetic, instrument links, and physical design tools

Advantages over Harmonic Balance

• In Harmonic Balance, if you add nodes or more spectral frequencies, the RAM and CPU requirements increase geometrically. Krylov improved this, but it's still a limitation of Harmonic Balance because the signals are inherently periodic.
• Conversely the penalty for more spectral density in Circuit Envelope is linear: just add more time points by increasing TSTOP. The longer you simulate, the finer your resolution bandwidth.
• Doing a large number of simple 1-tone HB simulations is effectively faster and less RAM intensive than one huge HB simulation.
• With a circuit envelope simulation the amplitude and phase at each spectral frequency can vary with time, so the signal representing the harmonic is no longer limited to a constant, as it is with harmonic balance.

Limitations

1. More occupied spectrum than unoccupied spectrum.
   You're carrying more overhead with frequency-domain assumptions and harmonics than necessary. Use SPICE.
2. Everything baseband. Depends.
   • If everything linear, use AC/S-parameter (for noise or budget)
   • If everything nonlinear or digital, use SPICE.
   • If everything logic/behavioral, use PTOLEMY.
3. Occupied spectrum is relatively sparse.
   If you can do what you want using Harmonic Balance, you should. Post-processing, optimization, and yield are simpler and faster.

Simulation Process

1. Transform input signal
   
   Each modulated signal can be represented as a carrier modulated by an envelope - A(t)*ejf(t). The values of amplitude and phase of the sampled envelope are used as input signals for Harmonic Balance analyses.
2. Frequency Domain Analysis
   
   Harmonic Balance analysis is performed at each time step. This process creates a succession of spectra that characterize the response of the circuit at the different time steps.
3. Time Domain Analysis
   
   Circuit Envelope provides a complete non steady-state solution of the circuit through a Fourier series with time-varying coefficients.
4. Extract Data from Time Domain
   
   Selecting the desired harmonic spectral line (fc in this case), it is possible to analyze:
   • Amplitude vs. Time (Oscillator start up, Pulsed RF response, AGC transients)
   • Phase (f) vs. Time (t) (VCO instantaneous frequency (df/dt), PLL lock time)
   • Amplitude & Phase vs. Time (Constellation plots, EVM, BER)
5. Extract Data from Frequency Domain
   
   By applying FFT to the selected time-varying spectral line it is possible to analyze:
   • Adjacent Channel Power Ratio (ACPR)
   • Noise Power Ratio (NPR)
   • Power Added Efficiency
   • Reference frequency feedthrough in PLL
   • Higher order intermods (3rd, 5th, 7th, 9th)

Simulation Steps

Define baseband signal modulation Predefined sources Equations I & Q data vs. time data from DSP simulation Define RF carrier frequencies, time step and duration of the simulation Compute time-varying Fourier coefficients Post-process and display results

OR

Define input signal(s) with modulation - amplitude, phase, frequency, I/Q, etc. Define the time step Simulator computes Fourier coefficients versus time: Fourier transforms are computed to display frequency spectrum around any tone (if necessary)

Typical Analyses

• Intermodulation distortion.
• Amplifier spectral regrowth and adjacent channel power leakage.
• Oscillator turn-on transients and frequency output versus time in response to a transient control voltage.
• PLL transient responses.
• AGC and ALC transient responses.
• Circuit effects on signals having transient amplitude, phase, or frequency modulation.
• Amplifier harmonics in the time domain.
• Subsystems using modulation signals such as multilevel FSK, CDMA, or TDMA.
• Third-order-intercept and higher-order intercept analyses of amplifiers and mixers.
• Time-domain optimization of transient responses.

Typical Applications

Time Domain Data Extraction

Selecting the desired harmonic spectral line it is possible to analyze:

• Amplitude vs. Time
  Oscillator start up
  Pulsed RF response
  AGC transients
• Phase vs. Time
  VCO instantaneous frequency, PLL lock time
• Amplitude & phase vs. time
  Constellation plots
  EVM, BER

Frequency Domain Data Extraction

By applying FFT to the selected time-varying spectral line it is possible to analyze:

• Adjacent Channel Power Ratio (ACPR)
• Noise Power Ratio (NPR)
• Power added efficiency
• Reference frequency feedthrough in PLL
• Higher order intermods (3rd, 5th, 7th, 9th)

LSSP Simulation Controller

The large-signal S-parameter simulation controller facilitates the computation of large-signal S-parameters in nonlinear circuits.

Large-signal S-parameters are based on a harmonic balance simulation of the full nonlinear circuit. Unlike S-parameters, large signal S-parameters can change as power levels are varied because the harmonic balance simulation includes nonlinear effects such as compression.

XDB Simulation Controller

The XDB simulation controller computes the gain compression point of an amplifier or mixer. It sweeps the input power upward from a small value, stopping when the required amount of gain compression is seen at the output.

Transient/Conv. Simulation Controller

The transient and convolution simulation controllers solve a set of integro-differential equations that express the time dependence of the currents and voltages of the circuit. The result of such an analysis is nonlinear with respect to time and, possibly, a swept variable.

Use the Transient/Convolution controller to perform:

• SPICE-type transient time-domain analysis.
• Nonlinear transient analysis on circuits that include the frequency-dependent loss and dispersion effects of linear models, or Convolution analysis.

A transient analysis is performed entirely in the time-domain. It does not account for the frequency-dependent behavior of distributed elements.

A convolution analysis represents distributed elements in the frequency domain to account for their frequency-dependent behavior.

Transient Simulation and Convergence

In Transient analysis a numerical integration algorithm is employed at each time point to approximate the differential equations into algebraic equations. Integration methods are used to replace the time derivative with a discrete-time approximation

Time Step Control Characteristics

Local Truncation Error

• Estimates the LTE made on every capacitor and inductor
• Determines the time step size to ensure the largest LTE remains within the accepted tolerance
• The estimated LTE is inversely proportional to TruncTol
• The accepted tolerance depends upon the relative and truncation tolerances set for the current and voltage. It is proportional to I_RelTol x TruncTol and V_RelTol x TruncTol

Iteration-Count

• Determines the time step size based on the number of Newton iterations required for previous time point
• No direct relationship between iterations and LTE
• Effectively controlled by Max time step (for linear circuits)

Fixed

• The time step is fixed and equal to Max time step

Break Points

• Generated by built-in independent sources whenever an abrupt change in slop occurs
• Ensure that corners in waveforms are not missed
• ADS always places time points on a break point (except fixed time step)
• Backward Euler is used on time points that are the first time step after break points
• The step size is reduced when time point is close to a break point

Transient Convergence Tips

1. For initial Transient analysis, try to use I_RelTol = V_RelTol = 1e-3, and tighten these values only when higher accuracy is needed. Simulation will run much faster with these setting compared to 1e-6.
2. Transient analysis convergence problems are often caused by jumps in the solution. This most often occurs in circuits with overly simplified models that exhibit positive feedback, or when the circuit contains nodes that do not have a capacitive path to ground. Add a small capacitor from the troublesome node to ground and give a complete capacitance model when specifying the nonlinear device model parameters.
3. Generally analog circuits are sensitive to truncation error due to their relative long time constants. Use LTE time step control to ensure the accuracy of the results.
4. Backward Euler (Gear1 or Mu=0 in Trapezoidal) and Gear2 are stable for all stable and some unstable differential equations. However, trapezoidal rule are stable only on stable differential equations. Switch to Gear1 or Gear2 when trapezoidal rule fails on unstable differential equations.

Typical Convergence Problems

Capacitor model problems

• Use simplified device models that do not include capacitance model or incomplete capacitance model give a complete capacitance model when specifying nonlinear device model parameters, in junction capacitance, include both depletion (at least) and diffusion capacitances
• Discontinuous jumps in waveforms when circuit contains nodes have no capacitive path to ground add small capacitor to ground or specify Cmin
• Capacitance model does not conserve charge GaAsFET Statz's, MOSFET Meyer's capacitance models switch to charge based model
• Large floating capacitors that are similar to the small-floating resistor problem in DC (finite precision problem) check capacitance unit, use smaller capacitance
• Discontinuous capacitance models in user defined model, SDD device fix the model

Slow Transient analysis

• Make sure I_RelTol and V_RelTol are set to 1e-3 or not set at all
• Decrease these values when higher accuracy is needed

Oscillator circuit does not oscillate

• Apply a short pulse at the beginning of the simulation
• Avoid using Gear2 or backward Euler

Circuit exhibits ringing or divergence

• Reduce Mu value from 0.5 toward 0 if trapezoidal rule is used
• Use Gear1 or Gear2

Circuit does not converge at first time point

• Reduce Min time step

Convergence Hints

Add break points

Use piecewise linear source to add break points to the region where the waveform changes abruptly

Reduce max time step

Ensure enough time points for sharp edges

Increase Max iterations per time step

Increase to 50 or more to increase the possible number of Newton iterations on each time step

Increase I_AbsTol

Try 1e-10 instead of the default 1e-12

Relax TruncTol

Increase this value 10 times or more to relax LTE tolerance

Relax I_Reltol and V_Reltol

Increase to 1e-3 to relax Newton convergence tolerance as well as LTE tolerance

Try different integration methods

Switch from trapezoidal to Gear's method

Using Convolution

• Don't set any convolution parameters (let the adaptive algorithm figure it out)
• Set ImpMaxFreq first (larger than signal bandwidth)
• Set convolution parameters on component, not controller, when possible
• Don't allowed measured data to be extrapolated (either set ImpMaxFreq or provide more data)

Convolution Modeling for Time-Domain Simulation

• In time-domain simulation, simulate devices that can only be defined in the frequency domain
  • Transmission lines with dispersion
  • Devices with frequency-dependent loss
  • Measured frequency-domain data
• Convolution is the key
  • Inverse Fourier transform of frequency-domain data produces the impulse response h(t)
  • The impulse response is convolved with time-domain signal

Time and Frequency Range

• Impulse response is computed from the inverse Fourier transform of frequency-domain response frequency is uniformly sampled from 0 to some upper value
• Upper frequency sets the time-domain spacing of the impulse response
• Frequency spacing sets the length of the impulse response

Adaptive Impulse Response Calculation

• Estimate of system bandwidth is made from source frequencies and rise times - initial guess at fmax
• Build a trial impulse response with 32 timepoints
  very coarse frequency spacing
• Build a second impulse response with 64 timepoints
  less coarse frequency spacing
• Keep doubling the number of timepoints until a good impulse response is obtained
  increase fmax, decrease Df
• y11 and y12 may be sampled with different fmax and Df
• Adaptive calculation is only done if ImpDeltaFreq is not specified
  don't set ImpDeltaFreq if you don't have to

Good Impulse Responses

• Compare impulse responses with N and 2N points. The second impulse response is twice as long in time domain and has half the frequency spacing.
• An impulse is considered "good" when no appreciable energy is present in the second half of the impulse response if energy is present in the second half, implies either that the impulse is not long enough or it is noncausal
• If not good, Controller keeps doubling the length
• Controller also tries doubling the maximum frequency, giving smaller impulse timesteps
  

Interpolation

• The impulse response is sampled with a uniform timestep, but is not guaranteed to match the simulation timestep. The simulation may even be using a variable timestep.
• Interpolate the signal v(t) to match the timepoints in the impulse response
• Don't interpolate the impulse response because the Fourier transform of the interpolated impulse response would no longer match the original frequency response

Impulse Evaluation

• Signal response at time zero extends back to minus infinity
• Evaluate the integral as a sum
  

Solving an Invalid Impulse Response

This is the most commonly encountered problem during convolution. It does not necessarily imply noncausality but means that significant energy is present in the second half of the impulse response. In addition, simulation results may or may not be valid.

• Set ImpMaxFreq or ImpDeltaFreq. Set ImpMaxFreq first, typically only for measured data.
• For every component that generates this message, fix each component one at a time to simplify the design.

Viewing an Impulse Response

• In an S-parameter simulation, analyze over the given frequency spacing and maximum frequency
  inverse Fourier transform the response by plotting ts (x)
• In the time domain, apply an impulse and simulate
  plot the transient result
  the pulse risetime is used to set fmax and thus can influence the impulse response

Setting ImpMaxFreq and ImpDeltaFreq

Generally a good impulse response can be found without manually setting ImpMaxFreq and ImpDeltaFreq

• If ImpMaxFreq is set, the adaptive algorithm tries different lengths but doesn't modify fmax
• If ImpDeltaFreq is set, the adaptive algorithm is disabled and the impulse is computed from ImpDeltaFreq and ImpMaxFreq
• Set ImpMaxFreq on the component, then set ImpDeltaFreq on component if necessary, and finally, set ImpMaxFreq on the transient controller if necessary
• For transmission lines, set ImpMaxFreq to at least n/td, where td is the delay time and n is a small integer (2-3)
• For lowpass and bandpass filters, set ImpMaxFreq to at least twice the upper passband edge

Measured Data with S2P Component

• The algorithm that computes the impulse response has no special knowledge of the component it's working on and assumes data is available at any desired frequency. It has no knowledge of flow and fhigh or frequency spacing of measured data
• S2P interpolates and extrapolates data as needed
• Be sure to supply good data to prevent dangerous extrapolation extends down to DC and up to fmax
• Set ImpMaxFreq on S2P component to match frequency limits in datafile (avoid extrapolation)
• Typically there is not enough frequency-domain data in the S2P file for use in the simulation

Given a pulse with a risetime of tr, the equivalent bandwidth is 2.2/tr (0.1 ns risetime represents a 22 GHz bandwidth)

Package models typically must be measured up to 10x higher than the signal frequency to represent transmission line effects well

Solving a Noncausal Impulse Response

This is the second most commonly encountered problem during convolution. The Time-domain simulation starts at time zero and moves forward in time, computing the value of next timepoint from all previous timepoints. And the Controller deals with this by introducing a delay to force causality.

Length of delay set to ImpNoncausalLength (default=32) with timestep set by default ImpMaxFreq
Simulation results will not be accurate because of the added delay, especially if the delay is added in a critical timing or phase path.

All physically realizable devices are causal (the output is dependent only on past states and not any future states) while noncausal devices are nonphysical. Some ADS components, user-defined data or equations may be noncausal.

• Frequency-dependent real part with constant imaginary part, for example resistance as a function of frequency without any reactance
• Constant real and constant non-zero imaginary part
• Negative time delays
• INDQ, CAPQ, PLCQ, SLCQ have problems in some modes

RF Budget Controller

Use the Budget controller for budget analysis of an RF system. This RF system budget analysis enables you to determine the linear and nonlinear characteristics of an RF system comprising a cascade of two-port, two-pin linear or nonlinear components.
The Budget controller includes a large number of built-in budget measurements and improved budget noise measurements.

Use the RF Budget Controller to

• Modify simulations using tuning, parameter sweeps, optimization, yield analysis, etc.
• Include AGC loops to control gain and set power levels at specific points in the RF system.
• Select alternate budget paths.

Nominal Optimization Controller

Use the Nominal Optimization controller in combination with Goal components to satisfy predetermined performance goals. Optimizers that compare computed and desired responses and modify design parameter nominal values to bring the computed response closer to that desired can be selected from within the Nominal Optimization controller setup.

Monte Carlo Controller

Use the Monte Carlo analysis controller to randomly vary network statistical parameter values according to statistical distributions to get the overall performance variation. This process involves simulating the design over a given number of trials in which the statistical variables have values that vary randomly about their nominal values with specified probability distribution functions.

Yield Analysis Controller

Use the Yield Analysis controller in combination with a Yield Specification component to vary a set of statistical parameter values, using specified probability distributions, to determine how many possible combinations result in satisfying predetermined performance requirements. This process involves simulating the design over a given number of trials in which the statistical variables have values that vary randomly about their nominal values with specified probability distribution functions. The numbers of passing and failing trials are recorded and these numbers are used to compute an estimate of the yield.

Yield Optimization Controller

Use the Yield Optimization controller in combination with a Yield Specification component to perform multiple yield analyses with the goal of adjusting the nominal values of the statistical variables to maximize the yield estimate.

During yield optimization, each yield improvement is referred to as a design iteration.

Design of Experiments Controller

Use the Design of Experiments (DOE) controller in combination with DOE Goal components to perform an experiment and collect response data. You can then analyze the data using statistical methods. Sequential application of this methodology can be used to improve the statistical performance of a given circuit or system. Because of an inherent compromise between statistical performance prediction accuracy and the number of input variables, a screening experiment is used to identify variables that contribute significantly to performance variation. Next a refining experiment can be used to hone in on the target statistical response.