Envelope Simulation Parameters
ADS provides access to envelope simulation parameters enabling you to define aspects of the simulation listed in the following table:
| Tab Name | Description | For details, see... |
|---|---|---|
| Env Setup | Sets parameters related to time and frequency, and status level. | Setting Frequencies |
| Env Params | Selects an integration mode and sweep offset, turns on all model noise, and sets device-fitting parameters. | Defining Envelope Simulation Parameters |
| Initial Guess | Sets parameters related to initial guess, including automated transient assisted harmonic balance (TAHB), harmonic balance assisted harmonic balance (HBAHB), initial guess from a data file, and initial guess for parameter sweep. It also allows the user to save the final solution in a data file. TAHB provides a transient initial guess for the underlying harmonic balance simulation at the first time point of a circuit envelope simulation. |
In Harmonic Balance Simulation, see Setting Up the Initial Guess. For additional information about using TAHB and HBAHB, see Transient Assisted Harmonic Balance and Harmonic Balance Assisted Harmonic Balance. |
| Oscillator | Sets parameters for analyzing oscillators. | Enabling Oscillator Analysis |
| Fast Cosim | Enables the Fast Cosimulation mode and sets related parameters. | Enabling Fast Cosim |
| Params | Sets device operating point levels and FFT oversampling. | Defining HB Simulation Parameters |
| Solver | Choose between an automatic selection, or a Direct or Krylov solver. The Auto Select mode is the default and recommended choice. | In Harmonic Balance Simulation, see Selecting a Harmonic Balance Solver Technique. |
| Noise † | Parameters related to noise simulation, including sweeps, input and output ports, and the nonlinear noise controllers to be simulated. | In Harmonic Balance Simulation, see Selecting Nonlinear Noise Analysis. |
| Small-Sig † | Sets parameters related to small-signal/large-signal simulation to achieve faster simulations when some signal sources are much smaller than others, and are assumed not to exercise circuit nonlinearities. | In Harmonic Balance Simulation, see Setting Up Small-Signal Simulations. |
| Output | Selectively save simulation data to a dataset. | Selectively Saving and Controlling Simulation Data |
| Display | Control the visibility of simulation parameters on the Schematic. | Displaying Simulation Parameters on the Schematic |
† Small-Signal and Noise analysis are performed only after the last Envelope time points, so that the Envelope sweep is allowed to get to a desired operating point, and then perform the standard small signal or noise characterization at that point.
Setting Frequencies
The Env Setup tab involves parameters related to time and frequency, and status levels. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.
| Setup Dialog Name | Parameter Name | Description |
|---|---|---|
| Times | Stop time | Stop | The time the analysis stops. |
| Time step | Step | Sets the fixed time step that the simulator uses to calculate the time-varying envelopes. |
| Note: The parameter Time step defines the maximum allowed bandwidth (±0.5 /Time step) of the modulation envelope. Because of the nature of the time-domain integration algorithms, the analysis bandwidth (1/Time step) should be at least twice as large as the modulation bandwidth to achieve accurate simulations at the maximum modulation frequencies. Stop time simply defines the maximum duration of the swept time simulation. An analysis starts at time = 0, so the total number of simulation time points that are stored is equal to 1+(Stop time/Time step). At each time point, the envelope values of all of the analysis frequencies, including DC, are saved. | ||
| Fundamental Frequencies | Edit | Edit the Frequency and Order fields, then use the buttons to Add the frequency to the list displayed under Select. | Frequency | Freq[n] | The frequency of the fundamental(s). Change 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 by typing over the entry in the field. |
| Select | Contains the list of fundamental frequencies. Use the Edit field to add fundamental frequencies to this window. - Add - Enables you to add an item. - Cut - Enables you to delete an item. - Paste - Enables you to take an item that has been cut and place it in a different order. |
|
| Maximum mixing order | MaxOrder | The maximum mixing order of the intermodulation terms in the simulation. The combined order is the sum of the individual frequency orders that are added or subtracted to make up the frequency list. For example, assume there are two fundamentals and Order (see below) is 3. If Maximum mixing order is 0 or 1, no mixing products are simulated. The frequency list consists of the fundamental and the first, second, and third harmonics of each source. If Maximum mixing order is 2, the sum and difference frequencies are added to the list. If Maximum mixing order is 3, the second harmonic of one source can mix with the fundamental of the others, and so on. |
| Levels | Enables you to set the level of detail in the simulation status report. | Status level | StatusLevel | Prints information about the simulation in the Status/Summary part of the Message Window. A value of 0 causes no or minimal information to be reported, depending on the simulation engine. Higher values print more detail. 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. Note: To view a report of the simulator's progress in the Status/Summary window while the simulation is running, set Status level to 3. |
Defining Envelope Simulation Parameters
The Env Params tab involves selecting an integration mode and sweep offset, turns on all model noise, and sets device-fitting parameters. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.
| Setup Dialog Name | Parameter Name | Description |
|---|---|---|
| Env Params | Integration | EnvIntegOrder | Displays the integration options. | Backward Euler | EnvIntegOrder=1 | Invokes the backward-Euler integration algorithm. |
| Trapezoidal | EnvIntegOrder=2 | Invokes the trapezoidal integration algorithm. Integrates between time points by assuming they are connected by line segments |
| Gear's | UseGear | Invokes second-order Gear's method. |
| Sweep offset | SweepOffset | Delays the output of the swept data until the SweepOffset value is reached. It also offsets that value to 0. For example, a sweep to 1 msec with a SweepOffset of 0.6 msec will result in output data with a time axis of 0 to 0.4 msec. This is one reason why this parameter is not called a TimeStart value, as in Transient. The SweepOffset value does not change the start time of transient simulation. Transient simulation begins at time = 0 regardless. |
| Turn on all noise | EnvNoise | Includes in the simulation the noise in devices such as resistors, lossy transmission lines, diodes, transistors, etc. This adds independent, white, Gaussian noise at all of the envelope frequencies. Explicit noise sources, such as V_Noise, I_NoiseBD, OSCwPhNoise Amplifier, etc., also add their noise contribution. Full nonlinear circuit equations are applied to the resulting composite signal, so that no small-signal assumptions have to be made about the relative size of the noise, and voltages are added to the simulation. The noise will be complex for non-baseband envelope frequencies, generating both amplitude- and phase-equivalent noise. The noise is generated by a random number generator. It will produce a different sequence of random numbers each time the simulation is run. If a repeatable sequence is required, it can be obtained by setting the simulator variable _randseed_ to an integer value with a schematic equation. For example, __randseed=12345 (two underscores precede randseed). |
| Device Fitting | There are several ways to control the linear device, time-domain modeling required by the circuit envelope simulator when analyzing a modulation envelope. Most built-in elements now have an Laplace or a transmission line approximation. This parameter is used only with respect to dataset devices or generic linear devices whose frequency response cannot be represented as a rational polynomial of the form e-sT(P(s)/Q(s)) where s is the Laplace variable, T is time delay, and P and Q are the numerator and denominator polynomials, respectively. For linear elements a model must be generated that reflects the envelope frequency response around each of the analysis frequencies. The first three parameters in this area are used in a pole/zero fit of the frequency response around each carrier frequency. The remaining options are used when a valid or sufficiently accurate pole/zero fit cannot be obtained. |
Bandwidth fraction | EnvBandwidth | Determines what fraction of the envelope bandwidth to use to determine the fit. The initial value provided for Bandwidth fraction is 1.0. The default value for Bandwidth fraction when the value is left blank is 0.1, so that only the frequency values that lie between ±0.5 x BandwidthFraction/Timestep around each carrier frequency are used to determine the fit. If greater accuracy is required at the edges of the envelope bandwidth, this number can be increased. However, the simulator will then typically require a higher order and a more time-consuming fit to be generated and then used during the simulation. Also, the integration algorithms cannot maintain 100% accuracy out to the edges of the envelope bandwidth. A Bandwidth fraction value of 0.0 will effectively disable this pole/zero fitting, and just the constant value will be used. This will result in the fastest simulation, but any transient effects from these models will not be included. The Relative tolerance and Absolute tolerance parameters (see below) can also be set to help determine how accurate a fit is desired. |
| Relative tolerance | EnvRelTrunc | Sets a relative truncation factor for envelope fitting. |
| Absolute tolerance | EnvAbsTrunc | Sets an absolute truncation factor for envelope fitting. |
| Warn when poor fit | EnvWarnPoorFit | Causes a warning message to appear when an envelope fit is poor. | Use fit when poor | EnvUsePoorFit | Instructs the simulator to use poor fits instead of constant values. |
| Skip fit at baseband | EnvSkipDC_Fit | Instructs the simulator not to use pole/zero fitting at the baseband (DC) envelope. Note: If an external frequency-domain-device is supplied (such as an n-port data device using a dataset of S-parameter measurements read from an instrument), and that device does not accurately represent the low-frequency or DC response, then a good pole/zero fit may not be obtained. Three of the above parameters determine what to do in these cases. Skip fit at baseband can be used to disable the fitting process at just the DC (baseband) frequencies. Warn when poor fit can be used to disable the output of these warnings. Use fit when poor then determines whether to use these poor fits in the simulation or to replace them with the constant, center frequency value. However, there is a potential risk associated with using poor fits, in that the simulation may generate incorrect, possibly unstable results. |
Setting Up the Initial Guess
This enables automated transient assisted harmonic balance (TAHB) and harmonic balance assisted harmonic balance (HBAHB). TAHB provides a transient initial guess for the underlying harmonic balance simulation at the first time point of a circuit envelope simulation.
In the Harmonic Balance Simulation documentation, see Setting Up the Initial Guess. For additional information about using TAHB and HBAHB, see Transient Assisted Harmonic Balance and Harmonic Balance Assisted Harmonic Balance.
Enabling Oscillator Analysis
The Oscillator tab involves setting up parameters to analyze oscillators. The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.
| Setup Dialog Name | Parameter Name | Description |
|---|---|---|
| Enable Oscillator Analysis | OscPortName | This causes a normal harmonic balance simulation to be performed prior to the first time step. This is used to determine and set the analysis frequency to the steady-state oscillator frequency. Select this option to simulate a circuit containing an oscillator. |
| Method | The Use Oscport method should be selected if the circuit contains an OscPort or OscPort2. The Specify Nodes method (OscProbe) should be selected if the circuit is an oscillator and does not contain an OscPort or OscPort2. | |
| Specify Oscillator Nodes The following parameters are available only when selected Method is Specify Nodes. |
Node Plus | OscNodePlus | This is the required name of a named node in the oscillator. Recommended nodes are those at the input or output of the active device, or in the resonator. Hierarchical node names are permitted. |
| Node Minus | OscNodeMinus | This second node name should only be specified for a differential (balanced) oscillator. Leave it blank for single-ended oscillators. Node Plus and Node Minus should be chosen symmetrically. Hierarchical node names are permitted. |
| Fundamental Index | OscFundIndex | Specifies which of the fundamental frequencies is to be treated as the unknown oscillator frequency which the simulator will solve for. The default value of 1 means that Freq[1] is the unknown. |
| Harmonic Number | OscHarmNum | Specifies which harmonic of the fundamental frequency is to be used for the oscillator. Normally this parameter stays at its default setting of 1. If an oscillator followed by a frequency divider is to be analyzed, this parameter should be set to the frequency divider ratio. |
| Octaves to Search | OscOctSrch | Is used in the initial frequency search during oscillator analysis. This many octaves are searched, centered around the frequency specified by the user on the Freq tab. To skip the initial frequency search, provide a good initial guess of the frequency on the Freq tab and set this parameter to zero. |
| Steps per Octave | OscOctStep | Specifies the number of steps per octave used in the initial frequency search. A high-Q oscillator may require a much larger value, such as 1000, in order for the search to find the phase shift at resonance. |
| Calculate oscillator startup transient | ResetOsc | This option resets the oscillator voltage solution to zero so that the transient buildup can be simulated. If this option is not selected, the time-domain solution begins at the steady-state solution, the transient buildup time is skipped, and the oscillator can immediately start responding to any external modulation. Note: The OscPort, if present, is used only for this initial simulation. It is disabled once the actual envelope simulation starts. |
Enabling Fast Cosim
These parameters enable and control the Fast Cosimulation mode and are only applicable when the Envelope controller is being used in a Ptolemy cosimulation. Fast Cosim parameters are used with Wireless Test Bench (WTB) cosimulation. This mode is also known as Automatic Verification Modeling (AVM). The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.
| Setup Dialog Name | Parameter Name | Description | Enable Fast Cosim | ABM_Mode | This enables the Fast Cosimulation mode to be used for the Analog/RF subcircuit. If Fast Cosim is not possible for this subcircuit, then a warning will be output and regular Circuit Envelope Cosimulation will be performed. |
|---|---|---|
| Characterization | Build Model | ABM_ReUseData= ABM_ReUseData=no |
Selecting this activates the Set Characterization parameters button, and tells the simulator to use characterization parameter values to build a new model for this Analog/RF subcircuit. This new characterization is saved in a dataset named after the subcircuit name. To open the Characterization Options dialog and change the characterization parameter values, click the Set Characterization parameters button. |
| Use previous data | ABM_ReUseData=yes | Selecting this tells the simulator to re-use any previous characterization that was done for this Analog/RF subcircuit. This characterization is saved in a dataset named after the subcircuit name. This eliminates any overhead time associated with the characterization, but it is then the responsibility of the user to make sure that nothing significant enough has changed (including carrier frequency, time step, bias voltages, temperature, optimization variables, etc.) since the last characterization. |
| Characterization Options - Click Set Characterization parameters to access the dialog box with these options. | Max Input Power | ABM_MaxPower | This specifies the maximum input power to this Analog/RF subcircuit that will be used during the Fast Cosim characterization phase. Excessively high values will take longer to characterize due to potentially more difficult circuit convergence. If the input power during the cosimulation exceeds this value, a warning will be generated since the Fast Cosim results will no longer be accurate. |
| Min Mumber of Amplitude Points | ABM_AmpPts | This sets the number of linear amplitude points between 0 and the full scale value defined by the Max Input Power. Depending on how much variation there is in the output vs. input amplitude characterization, more amplitude points may be needed to achieve optimum accuracy at a cost of additional characterization time. Due to the continuation nature of the swept amplitude harmonic balance characterization when not using Krylov modes, the cost of additional amplitude points is usually small. In addition to these linear spaced points, the characterization adds an additional power point every 6 dB down to a value 100 dB below the Max Input Power. |
| Perform Phase Sweep | ABM_PerformPhaseSweep | Select to enable phase sweep using value set for ABM_PhasePts. Enabling this may significantly increase the number of simulations required for characterization and may impact performance. Default is off. When selected ABM_PerformPhaseSweep=yes. |
| Number of Phase pts. | ABM_PhasePts | Any value greater than 0 will enable the characterization to be done as a function of both amplitude and phase. This specifies the number of phase points to be used at each amplitude point. Since this will now be a two dimensional sweep and so will be slower, it should only be used when required, such as with IQ demodulators where the output is a nonlinear function of the input phase. IQ Modems that are linear with phase, but nonlinear with amplitude, do not require phase characterization. Just identify the I/Q pair with the correct polarity in the Node Names section. If number of points entered is greater than 0 and less than 4, the simulator will change the value to 4 during the simulation. |
| Number of Frequency pts. | ABM_FreqPts | This sets the minimum number of small signal frequency points that are used to characterize the Analog/RF subcircuit. The actual number of points is increased to the next highest power of 2 value. These points are spaced between ±0.5/TimeStep, where TimeStep is the Step time defined in the Envelope controller. The maximum impulse duration for this frequency response characterization is determined by this frequency spacing. So the number of frequency points should be greater than the maximum impulse response time of the circuit around the carrier frequency plus any additional Delay specified in the Implementation block, both normalized by the Circuit Envelope TimeStep value. |
| Noise Characterization | Use the same frequencies as for Small-signal Frequency Response | ABM_NoiseLogScale=no | This is the default mode for noise characterization. Noise simulation is performed at the same frequencies as used for small-signal response around the frequency carrier. Default is selected. When selected ABM_NoiseLogScale=no. |
| Use independent log sweep | ABM_NoiseLogScale=yes | Select to enable independent log sweep and set values for parameters ABM_NoiseLogStartFreq and ABM_NoiseLogPtsPerDec. Default is unselected (ABM_NoiseLogScale=no). This feature is particularly beneficial in the characterization of 1/f noise, speeding up the characterization phase significantly. |
| Log Sweep Start Frequency | ABM_NoiseLogStartFreq | If Use independent log sweep is selected this parameter establishes the beginning of the frequency sweep. It must be greater than 0. |
| Number of Points per Decade | ABM_NoiseLogPtsPerDec | If Use independent log sweep is selected this parameter establishes the number of points per decade in the logarithmic frequency sweep. The highest frequency in the sweep is determined automatically from the envelope bandwidth. |
| Model Simulation | Apply frequency compensation | ABM_FreqComp | This specifies whether or not a frequency compensation filter is to be created for use in the Fast Cosim mode. In addition, the user can specify whether this filter is best placed on the input or the output of the nonlinear block. If the modulation is sufficiently narrow that there is not significant frequency response over the envelope bandwidth, then None should be selected. If the frequency response is primarily due to input filtering or transistor bandwidth limitations, then an Input frequency compensation should perform the best. Similarly, if the dominant filtering is at the output of Analog/RF subcircuit, such as the channel filter, then an Output frequency compensation should be used. Default is off (ABM_FreqComp=None). When selected, ABM_FreqComp=Input|Output depending on value set for Place filter at. |
| Add delay | ABM_AddDelay | Enables the ABM_Delay parameter and uses the value set for it. Default is off. When selected ABM_AddDelay=yes. |
| Delay | ABM_Delay | This adds additional transit delay to all the outputs of the Analog/RF subcircuit. In cases where this absolute delay is not critical to the overall system simulation, adding additional delay permits more accurate impulse implementation of the frequency response. This delay should not exceed half the impulse length, as determined by the frequency response characterization. |
| Verification | Stop Time | ABM_VTime | If this verification stop time is not zero, then both the normal Envelope cosimulation and the Fast Cosim results are computed. The RMS error between these two results is computed and output after this verification time has ended. This gives an indication as to how well the Fast Cosim is matching the Circuit Envelope results. |
| Accept Tolerance | ABM_VTol | If the Verification Stop Time has been set, then the resultant RMS error must be less than this value or else the Fast Cosim will be turned off and just the normal Envelope cosimulation results will be used for the remainder of the Ptolemy simulation. The stop time must be large enough to account for turn-on delays of filters and to give a sufficiently representative sample of the normal input signal. |
| Node Names | Active Input | ABM_ActiveInputNode | When multiple cosimulation inputs exists, only one (or one I/Q pair) can be active. Enter the node name of the active input here. Do not use any node name in the subcircuit input, but use the node name defined at the higher circuit level. If this is an I/Q pair input, then just use either the I or Q node name. Any non-active inputs will be monitored for activity and a warning generated if they are not truly static during a Ptolemy sweep. |
| IQ Pair | ABM_IQ_Nodes[n] | If multiple inputs or outputs correspond to an IQ pair, one pair can be defined here. Enter the I node name and the Q node name, as defined in the higher circuit level, separated by a space. If more than one IQ pair exists, use the Other = parameter in the Display tab, and use ABM_IQ_Nodes="<I node> <Q node>". Note that for IQ Modems that are linear with respect to phase, phase characterization is not required if the I/Q pair is properly identified here. |
Defining HB Simulation Parameters
Defining the HB simulation parameters consists of the following basic parts:
- Specifying the amount of device operating-point information to save.
- Specifying the FFT oversampling ratio.
The following table describes the parameter details. Names listed in the Parameter Name column are used in netlists and on schematics.
| Setup Dialog Name | Parameter Name | Description |
|---|---|---|
| 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 Env analysis (from multiple Env controllers), the device operating point data for all Env 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. |
| FFT | Fundamental Oversample | FundOversample | Sets the FFT oversampling ratio. Higher levels increase the accuracy of the solution by reducing the FFT aliasing error and improving convergence. Memory and speed are affected less when the direct harmonic balance method is used than when the Krylov option is used. |
| More... | Oversample[n] | Displays a small dialog box. To increase simulation accuracy, enter in the field an integer representing a ratio by which the simulator will oversample each fundamental. |
Selecting a Solver
Use the Solver parameters to select a convergence mode and solver type. These are the same parameters used to set up the solver for harmonic balance simulations. In the Harmonic Balance Simulation documentation, see Selecting a Harmonic Balance Solver Technique.
Selecting Noise Analysis
Use the Noise parameters to set up noise analysis including sweeps, input and output ports, and the nonlinear noise controllers to be simulated. These are the same parameters used to set up noise controllers for harmonic balance simulations. In the Harmonic Balance Simulation, see Selecting Nonlinear Noise Analysis.
Setting Up Small-Signal Simulations
Use the Small-Signal parameters to use a large-signal/small-signal method to achieve faster simulations when some signal sources are much smaller than others, and are assumed not to exercise circuit nonlinearities.
Small-Signal and Noise analysis are performed only after the last Envelope time points, so that the Envelope sweep is allowed to get to a desired operating point, and then perform the standard small signal or noise characterization at that point.
These are the same parameters used to set up small-signal simulations for harmonic balance. In the Harmonic Balance Simulation documentation, see Setting Up Small-Signal Simulations.
Privacy
Statement 
|
Terms of Use |
Legal |
Contact Us |
© Agilent 2000-2008
