Transient Simulation Parameters

ADS provides access to Transient simulation parameters enabling you to define aspects of the simulation listed in the following table:

Tab Name Description For details, see...
Time Setup Sets parameters related to time and frequency. Defining the Time Setup
Integration Selects an integration mode and sweep offset, turns on source and resistor noise, and sets device-fitting parameters. Options for oscillator analysis are also available. Setting the Integration Method
Convolution Sets parameters related to convolution analysis setup.
Includes access to advanced convolution options.		 Setting Up Convolution Analysis
Convergence Sets parameters related to achieving convergence. Setting Up the Convergence
Options Sets parameters related to simulation reporting levels and saving operating point level data. Setting Up Optional Parameters
Noise Sets noise bandwidth and scale. Defining the Noise Parameters
Freq Sets parameters for the fundamental frequencies which are used for computing an initial guess for a harmonic balance simulation. This approach is called Transient-Assisted Harmonic Balance (TAHB). Setting the Fundamental Frequencies
Output Selectively save simulation data to a dataset. For details, see Selectively Saving and Controlling Simulation Data.
Display Control the visibility of simulation parameters on the schematic. For details, see Displaying Simulation Parameters on the Schematic.

Using Transient Parameters in ADS

When using this controller, here are tips about preparing your design for simulation:

Setting Initial Conditions with InitCond Components

There are two elements for setting initial conditions in a transient simulation InitCond and InitCondbyName. InitCond and InitCondByName are used to provide an initial DC value for transient analysis only. These elements attach the specified voltage source with a series resistor to the specified node(s) to force a value. The DC solution for the entire circuit is then calculated. This DC solution is then used as the starting state for the transient analysis.

Defining the Time Setup

Following is information on the parameters related to time and frequency. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Transient Simulation Time Setup Parameters
Setup Dialog Name Parameter Name Description
Output Times
  Start time StartTime The time at which the simulator begins outputting time-point results. This enables control over large amounts of output data.
Stop time StopTime The time at which the simulator stops outputting time-point results. Must be long enough if steady state is needed. You must specify this parameter.
Max time step MaxTimeStep The largest time step to be taken in the simulation. You must specify this parameter.
Min time step MinTimeStep The smallest time step to be taken in the simulation. Generally the default value is satisfactory.
Limit timestep for Transmission Line LimitStepForTL Where transmission lines are involved, setting this option further limits the time step to half of the shortest transmission line's delay time.

Setting the Integration Method

Following is information on setting up the Integration portion of the simulation. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Transient Simulation Integration Parameters  
Setup Dialog Name Parameter Name Description
Time step control method TimeStepControl  
  Fixed Fixed Selects a fixed time-step method. The simulation is performed with a uniform, constant time step that is specified by Max time step (under the Time Setup tab). It is quicker than the other methods. However, it is not as robust, because it cannot select a smaller time step when convergence problems are encountered.
Iteration Count Iteration Count Uses the number of Newton-Raphson iterations that were needed to converge at a time point as a measure of the rate of change of the circuit. If the number of iterations is less than an internal threshold, the time step is doubled; if the number is greater than Max iterations per time step, the time step is scaled by a factor of Integration coefficient mu divided by 8 (see below). This method has a minimal computational overhead, but does not take into account the true rate of change of circuit variables. Use this if no energy storage component is present and the Local truncation error is not checked.
Trunc Error Trunc Error Default. Uses the current estimate of local truncation error to determine an appropriate time step. Although it takes longer than Iteration count, it sets a meaningful error bound on computed output values.
Local truncation error over-est factor TruncTol A value against which the simulation's error tolerance is compared. In transient analysis each time step is computed by means of the truncation-error estimate method. If the error is within acceptable limits, the results are stored and analysis continues at the next time point. Otherwise, the analysis is repeated at a smaller time step. Increase this value to relax local truncation error convergence tolerance without relaxing the Newton iteration convergence tolerance.
Charge accuracy ChargeTol The minimum charge value used to determine the charge tolerance when computing the local truncation error. Default = 1e-14.
Integration IntegMethod  
  Trapezoidal Trapezoidal Default. Integrates between time points by assuming they are connected by line segments. The local truncation error is then related to the difference between the areas determined by the present and previous time points.
Gear's Gear's Integrates by assuming that the time points are connected by a polynomial curve. The order of the polynomial is controlled by the Max Gear order parameter. Lower-order polynomials tend to create greater truncation error, while higher-order polynomials can become unstable.
Max Gear order MaxGearOrder Determines the maximum order of the polynomial when Gear's method is used. The default is 2. This is available only when Gear's is selected.
Integration coefficient mu Mu A coefficient that determines the degree of mixing of the trapezoidal (mu = 0.5) and backward-Euler (mu = 0.0) methods when the trapezoidal method is used. This is available only when Trapezoidal is selected. The valid range for mu is: 0.0 <= mu <= 0.5.
Caution: Do not set mu to 1.0; this results in a divide-by-zero condition.
The integration order at each timestep is output to the dataset as the variable tranorder. This data is used by the fs() function in the data display server to do accurate interpolation of the data when an FFT is required. For the default trapezoidal integration, this will normally have a value of 2, except at source-induced breakpoints where it will be 1.

Setting Up Convolution Analysis

Following is information on setting up the Convolution portion of the simulation. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Note
It is recommended that the Convolution parameters are left at their default settings.
Transient Simulation Convolution Parameters
Setup Dialog Name Parameter Name Description
Tolerance - Sets the tolerance for relative and absolute truncation factors for the impulse response: ImpRelTrunc and ImpAbsTrunc. Values are set depending on the option selected for Tolerance. Auto is the default. ImpRelTrunc default value is 1e-4. ImpAbsTrunc default value is 1e-7, and it controls how small the impulse must be before it is considered zero.
  Relax   When selected, impulse response truncation factors are set to the following:
ImpRelTrunc = 1e-2
ImpAbsTrunc = 1e-5
Auto   Default setting. Default values are used for ImpRelTrunc=1e-4, and ImpAbsTrunc=1e-7.
Strict   When selected, impulse response truncation factors are set to the following:
ImpRelTrunc = 1e-6
ImpAbsTrunc = 1e-8
Enforce Passivity ImpEnforcePassivity Default setting is off (unselected). When selected, this option enforces passivity for linear frequency domain components which are simulated using discrete mode convolution. Similarly, if EnforcePassivity=yes in a SnP component, passivity will be enforced in that particular device. The EnforcePassivity setting of SnP component overwrites the ImpEnforcePassivity setting of the transient controller in an individual device.
Advanced   Click Advanced on the Convolution tab to set these parameters. For parameter descriptions, see Defining Advanced Convolution Parameters


Defining Advanced Convolution Parameters

Use the following parameters for additional control of convolution simulations.

Advanced Convolution Options
Setup Dialog Name Parameter Name Description
Use approximate models when available ImpApprox Causes the simulator to bypass impulse-based convolution (when that option is available to you). Instead, it uses models that, although somewhat less accurate, can provide faster simulations. These approximations neglect effects such as frequency-dependent loss and dispersion, but include the basic delay and impedance. These models are the default, if no convolution license is available. Default setting is unselected.
Approximate short transmission lines ShortTL_Delay Specifies a limit on the time delay below which transmission lines will be approximated instead of modeled as a delay line. This enables you to analyze very short transmission lines with a Laplace transform approximation. Also, it does not require the simulator to take the very small time steps normally associated with short transmission lines. Only single, two terminal, transmission lines (like MLIN and TLIN, but not MCLIN and TLIN4) can be approximated this way.
Max Frequency ImpMaxFreq The maximum frequency to which a frequency-domain device is evaluated to obtain its impulse response. By default, the program chooses this value according to signal source bandwidth. You do not normally need to set this, unless it is necessary to increase it to model the high frequency components due to circuit nonlinearity.
Delta Frequency ImpDeltaFreq The frequency interval between samples in the evaluation of frequency-domain-defined devices.
Save Impulse Spectrum ImpSaveSpectrum Saves the impulse response, its FFT, and the original spectrum to a dataset when discrete mode convolution is used in transient analysis. The default value is no (unselected). The information added to the dataset uses names similar to those shown here where CMP1 is the component name:
CMP1_FFT_IMP: FFT of final impulse response used in convolution.
CMP1_IMP: Final impulse response used in convolution.
CMP1_OR: Original spectrum.
CMP1_S0: Exists only if passivity is enforced. Spectrum after causality but before passivity correction.


Backward Compatibility for Convolution

Due to the improved convolution simulation algorithm in ADS 2008 the parameters listed in the following table that were available in previous releases are obsolete. Parameters for Convolution Mode and Tolerance will be handled in ADS 2008 as described here:


Convolution Parameters Obsoleted in ADS 2008
Setup Dialog Name Parameter Name
Max impulse sample points ImpMaxPts
Convolution interpolation order ImpInerpOrder
Convolution mode ImpMode
  Discrete Discrete
PWL Continuous PWL Continuous
Smoothing window type ImpWindow
  Rectangle Rectangle
Hanning Hanning
Non-causal fcn imp response length ImpNoncausalLength


Setting Up the Convergence

Following is information on setting up the Tran Convergence portion of the simulation. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Transient Simulation Convergence Parameters
Setup Dialog Name Parameter Name Description
Use user-specified initial conditions UseInitCond Instructs the simulator to use user-specified initial conditions to compute the initial charges and fluxes in the circuit. The simulator will skip time=0 dc analysis.
When this option is enabled, the simulator uses the currents specified in the InitCond field of the inductors and the branch voltages specified in the InitCond field of the capacitors, as well as the node voltages specified in both the Simulation-Transient InitCond and Simulation-Transient InitCondByName components to compute the initial charges and fluxes in the circuit. The voltage given in the capacitor's InitCond field will take precedence over the voltage given in the Simulation-Transient InitCond and Simulation-Transient InitCondByName components if there is a conflict.
When the option is disabled and the Simulation-Transient InitCond and/or Simulation-Transient InitCondByName components are placed on the schematic, the simulator will start the transient analysis with a DC analysis at time=0 and try to force those node voltages identified in the Simulation-Transient InitCond and/or Simulation-Transient InitCondByName components to be close to the voltages specified. The values, if any, given in the InitCond field of the capacitors and inductors, however, will not be used.
Connect all nodes to GND via GMIN during initial DC analysis LoadGminDC Useful in conditions where open circuits would result in a singular matrix error (where the diagonal term is missing). When selected, this option instructs the simulator to insert a resistor valued at 1e12 ohms between any node and ground, whether at the circuit or the device level. ("GMIN" stands for minimum conductance.) This allows you to still obtain useful results.
Perform KCL check for convergence CheckKCL Checks to verify how closely Kirchoff's Current Law is satisfied at each node. This also depends on how the current tolerances are set (under the Convergence tab of the Options component). This option is selected by default, but may help convergence if not performed.
Check only delta voltage for convergence CheckOnlyDeltaV Looks for only the voltage difference between two consecutive iterations. This less-stringent check saves both time and memory. This option is selected by default.
Check for strange behavior at every timestep OverloadAlert Looks for inordinate device currents or voltages and returns a warning message when it finds any for devices or models which support the Overload Alert and have their limit values specified. Although this can be slower, it is useful where out-of-bounds conditions are suspected.
Skip device evaluation if volt chg are small between iters DeviceBypass Instructs the simulator to bypass the full evaluation of a device if it finds small voltage changes between iterations. This can improve simulation time in digital circuits containing many devices. "Small" voltage change is defined by voltage tolerances set under the Convergence tab of the Options component. This may increase analysis speed for digital circuits.
Max iterations per time step MaxIters The maximum number of iterations allowed for each time step.
Max iterations @ initial DC MaxItersDC The maximum number of iterations allowed during DC analysis, before the stepping of the source begins.
IV_RelTol IV_RelTol This is the transient relative voltage and current tolerance. The default is 1e-3. When simulation options are included in the simulation (using the Options controller), and there are other simulation controllers besides transient in an ADS design, use this parameter to set specific relative tolerances to be used for transient only. The value of IV_RelTol will be used for both current and voltage relative tolerance for transient. The IV_RelTol parameter makes it possible to have relative tolerances specifically for transient.

Setting Up Optional Parameters

Following is information on setting up the Tran Options portion of the simulation. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Transient Simulation Options
Setup Dialog Name Parameter Name Description
Levels   Select the degree of simulation information to be reported.
  Status level StatusLevel Prints information about the simulation in the Status/Summary part of the Message Window.
- 0 reports little or no information, depending on the simulation engine.
- 1 and 2 yield more detail.
- Use 3 and 4 sparingly since they increase process size and simulation times considerably.
The type of information printed may include the sum of the current errors at each circuit node, whether convergence is achieved, resource usage, and where the dataset is saved. The amount and type of information depends on the status level value and the type of simulation.
Device operating point level DevOpPtLevel Enables you to save all the device operating-point information to the dataset. If this simulation performs more than one Transient analysis (from multiple Transient controllers), the device operating point data for all Transient analyses will be saved, not just the last one. Default setting is None.
  None None No information is saved.
Brief Brief Saves device currents, power, and some linearized device parameters.
Detailed Detailed Saves the operating point values which include the device's currents, power, voltages, and linearized device parameters.
Output solutions
  Output all internal time points OutputAllPoints Causes the simulator to save simulation results at all internal timepoints; this option is on by default. Deselecting this option causes results to be saved at least as often as the Max timestep option but some of the intermediate points will be suppressed. For simulations that take many small timesteps due to automatic timestep control, but whose output is still well-sampled at Max timestep, this can make the resulting datasets smaller and make the post-processing of the data faster.

Defining the Noise Parameters

Following is information on setting up the Tran Noise portion of the simulation. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Transient Simulation Noise Parameters
Setup Dialog Name Parameter Name Description
Noise bandwidth NoiseBandwidth Enables the generation of pseudorandom noise at each timestep. NoiseBandwidth controls the bandwidth of the generated noise and must be less than or equal to 1/(2*MaxTimeStep). If this parameter is not specified or is zero, no noise is generated.
Noise scale NoiseScale A multiplicative scaling applied to all generated noise.

Setting the Fundamental Frequencies

Following is information on setting up the frequency portion of the simulation. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.

Transient Simulation Frequency Parameters
Setup Dialog Name Parameter Name Description
Fundamental Frequencies
  Edit   Edit the Frequency and Order fields, then click Add to add the frequency to the list in the Select area.
  Frequency Freq[n] The frequency of the fundamental(s). Change value by typing over the entry in the field. Select the units (None, Hz, kHz, MHz, GHz) from the drop-down list.
Order Order[n] The maximum order (harmonic number) of the fundamental(s) that will be considered. Change value by typing over the entry in the field.
Select   Contains the list of fundamental frequencies and their orders. Use the Edit area to add fundamental frequencies to this window.
- Add - Adds a frequency to the list.
- Cut - Removes selected frequency from the list.
- Paste - Enables you to move an item cut from the list to a new position.
Maximum mixing order MaxOrder Determines how many mixing products are to be transformed for the multi-tone harmonic balance simulation. A mixing term, or mixing product, is a combination of two or more fundamentals or their successive harmonics. Mixing products will occur when there are multiple frequencies in a circuit.
For example, consider having a simulation with Freq[1]=f1, Order[1]=4, Freq[2]=f2, Order[2]=5, and MaxOrder=3. The mixing products that are to be transformed are f1-f2, 2f1-f2, f1-2f2, f1+f2, 2f1+f2, and f1+2f2.
If Maximum order is 0 or 1, no mixing products are simulated. If the MaxOrder is not given, then it will be set to the largest order of the fundamental.
Compute HB Solution
  Write Initial Guess for HB HB_Sol Check this box to generate a transient initial guess for a harmonic balance simulation.
File HB_OutFile Enter the name of the file for the transient initial guess. Be sure to use the file name when running the harmonic balance simulation. If no file name is entered (and Write Initial Guess for HB has been selected), then the name of the design will be used as the default name.
Apply Window HB_Window Applies a window to the time domain data. This window helps to minimize the spectral leakage when multiple frequency tones are present. The window type is a Blackman window. For multi-tone applications, it is recommended to enable the Apply Window option.
Detect steady state SteadyState When enabled, causes the transient simulator to determine if the circuit reaches steady state. If steady state is reached, then the time value and frequency of oscillation (if simulating an oscillator) will be reported. At least one frequency and order pair (Freq[1] and Order[1]) must be specified when selecting this parameter. For a transient assisted harmonic balance simulation, enable SteadyState for the simulator to generate a transient initial guess (which captures the steady state portion of the waveform) for later use in the harmonic balance simulation. The simulator will stop when a steady state has been reached and transform just the last period of the solution. Thus, the transient simulation may end earlier than the StopTime when steady state is reached.
 

Privacy Statement  | Terms of Use  | Legal | Contact Us  | © Agilent 2000-2008 

Contents
Additional Resources