Simulation Basics

This documentation provides information that applies to the Analog/RF simulation in ADS. It also contains general information about the various simulation controllers that are available in ADS. Before using this documentation, you should see Advanced Design System Quick Start and Schematic Capture and Layout to review the whole product.

For details about running an Analog/RF simulation, you should also see Preparing a Circuit for Simulation in ADS and An ADS Simulation Example, then continue with other areas of the Simulation documentation that provide details about the simulation controllers.

Simulation Types

ADS provides simulators that enable you to simulate circuits and RF systems designed for specific objectives. The following table provides brief descriptions of the available simulation controllers. See the documentation for the Analog/RF simulation controllers for complete information about each one.

Simulator	Description
DC	Fundamental to all simulations, it performs a topology check and an analysis of the DC operating point of a circuit. See DC Simulation.
AC	Obtains small-signal transfer parameters, such as voltage gain, current gain, and linear noise voltage and currents. This simulator is useful in designing passive circuits and small-signal active circuits such as low-noise amplifiers (LNAs). See AC Simulation.
S-parameter	Provides linear S-parameters, linear noise parameters, transimpedance (Z ij ), and transadmittance (Y ij ), by linearizing the circuit about the DC operating point and performing a linear small-signal analysis that treats the circuit as a multiport. Each port is turned on sequentially. S-parameters can be converted to Y- and Z-parameters. This simulator can be used to achieve many of the same design goals as the AC simulator. See S-Parameter Simulation.
Harmonic Balance	Uses nonlinear harmonic-balance techniques to find the steady-state solution in the frequency domain. This simulator is useful in designing RF amplifiers, mixers, and oscillators. A Krylov subspace technique is available to reduce memory requirements and increase the speed of solution. This option is useful in designing large RF integrated circuits or RF/IF subsystems, where a large number of devices or large numbers of harmonics and intermodulation products are involved. See Harmonic Balance Simulation.
Large-signal S-parameter (LSSP)	A type of harmonic balance simulation, it performs large-signal S-parameter analyses to represent the nonlinear behavior of items such as power amplifiers. The accompanying P2D simulator available in ADS can be used to speed up subsequent analyses. See Large-Signal S-Parameter Simulation.
P2D	Generates a .p2d file that can be used to describe the behavior of a file-based component (such as the AmplifierP2D component, available in the System-Amps & Mixers library). See P2D Simulation.
Gain Compression (XdB)	Seeks a user-defined gain-compression point at which an actual power curve deviates from an idealized linear power curve. This is useful in power amplifier design. See Gain Compression Simulation.
Circuit Envelope	Uses a combination of frequency- and time-domain analysis techniques to yield a fast and complete analysis of complex signals such as digitally modulated RF signals. It represents input waveforms as RF carriers with modulation envelopes that are described in the time domain. This is useful in designing circuits and systems involving modulators/demodulators or complex modulated signals. See Circuit Envelope Simulation.
Transient/Convolution	Solves a nonlinear circuit in the time domain, and linear components can be simulated by means of convolution or a simplified equivalent-circuit model. See Transient and Convolution Simulation.
RF System Budget Analysis	Determines the linear and nonlinear characteristics of an RF system comprising a cascade of two-port linear or nonlinear components. The RF system may also include automatic gain control (AGC) loops to control gain and set power levels at specific points in the RF system. See RF System Budget Analysis.

About Licensing

These simulators require licenses to run a simulation. Confirm that the simulator of interest is included with your purchase. ADS allows you to create a circuit, but if you do not have the correct license you will not be able to simulate it.

Common Simulation Usage

The following table describes some common design objectives and the simulators that would be appropriate to each. The simulators are listed in the order they would generally be applied.

Working with the Examples Directory

ADS includes example projects containing designs that you can open and run.

Most of the designs discussed in this manual are available in the location where you installed ADS, typically $HPEESOF_DIR/examples directory. For detailed information about locating and opening ADS example projects, see Schematic Capture and Layout. For documentation on ADS examples organized by application, see the Examples Documentation.

Briefly, here is how to get started using examples. ADS examples include projects and templates. On UNIX, these projects are read-only directories. To work with an example project, you must first make a copy in a directory for which you have write permission. Windows users should also copy these examples to preserve the integrity of the examples. For convenience in keeping track of designs, you may want to create directory names that mirror those in the examples directory.

Do not copy projects by using your operating system alone. Use these methods:

• Use the Copy Project command in the Main window to copy entire projects to your local directory.
• Copy projects as part of the software installation procedure.

This ensures that all files that are part of the project are copied.

The Simulation Process

The following list shows the basic simulation process, and the sections to see for more information:

• Create your schematic, then add current probes and wire/pin labels to identify the nodes from which you want to collect data.
• Select a simulation method, specifying parameters as necessary. The parameters you specify are based on the type of simulation you choose, the simulation options you require, and whether you're sweeping parameters, using expressions, and optimizing your design.
  Selecting Simulation Controllers
  Using the Simulator Options Component
  Sweeping Parameters
  Working with Expressions
• Select a name for the dataset. This is where the simulation data will be saved.
  Saving and Controlling Simulation Data.
• Run the simulation.
  Controlling a Simulation
• View DC data by annotating the schematic with DC solutions and by viewing brief or detailed device operating point data.
  Viewing DC Solutions
• Display additional results using the Data Display.
  Displaying Simulation Results
• Optimize and tune a design.
  Displaying Simulation Results
  For complete information, see Tuning, Optimization, and Statistical Design.

These are the basic steps. It is possible to develop very detailed, complex simulations, but the process, for the most part, remains the same. The remainder of this chapter gives an overview of these steps. If you are new to using ADS, or you use it infrequently, two wizards are available to help you with several steps in the process:

• Using the Schematic Wizard follows the standard ADS use-model to help you with design creation and setting up a simulation.
• Using the Smart Simulation Wizard requires an existing design, and helps you sequence several simulations on the same device.

These wizards provide different features which may determine which one you prefer to use. The Schematic Wizard helps you develop a design and prepares it for a simulation as if you are working directly in the design environment. The Smart Simulation Wizard requires that you already have a design available and adds a Smart Simulation module for sequencing simulations to the design. The following table presents additional differences:

Comparison of Schematic Wizard to Smart Simulation Wizard

Schematic Wizard	Smart Simulation Wizard
Sets up the initial schematic, but does not include simulation sequencing, allowing support for more application types.	Has two major features: Set up initial schematic. Simulation sequencing on a common device under test.
Uses the standard ADS use-model for schematic development.	Simulation sequencing is a non-standard use-model in ADS.
Allows selection of application categories and applies to more application types.	Simulation sequencing is limited to certain types of devices under test, and is not generally extendable to all application categories.
Provides selection by application, and includes schematics by simulation-type.	Does not include selection of simulation-type.
Assists with some schematic corrections when simulation errors appear.	Does not include error correction.

Using the Schematic Wizard

The Schematic Wizard is provided to assist new ADS users or those who use it infrequently in performing the basic steps associated with schematic creation. Two options for schematic creation are available:

• Creating a design in the schematic that can be used as a component or subnetwork in another ADS design.
• Setting up a simulation based on a desired application or simulation type. The schematic can include an existing or sample test circuit, or simply provide a simulation schematic into which a test circuit can be placed.

The Schematic Wizard guides you through a sequence of steps gathering information from you about the type of schematic you want to create. Based on your inputs, the wizard automatically creates the specified schematic components. The wizard then provides you with instructions for completing the schematic manually, and for invoking the simulator when applicable. The simulations are set up to automatically display the results after successful simulations.

Accessing the Schematic Wizard

Access to the Schematic Wizard is controlled by the Schematic Wizard and Create Initial Schematic Window preference options. You can set these options in the Main Preference dialog (in the ADS Main window: Tools > Preferences ). The Schematic Wizard automatically appears when you perform certain actions related to the Schematic window.

Note The Schematic Wizard is not available for designs manipulated through any Layout window.

Starting a New Project

When you start a new project within ADS, the Schematic Wizard will appear if you have selected both preferences Schematic Wizard and Create Initial Schematic Window.

Opening a New Schematic Window from Main

When you open a new Schematic window from the ADS Main window (using the toolbar button or Window > New Schematic ), the Schematic Wizard will appear if you have selected the Schematic Wizard preference. The wizard will not appear if the new Schematic window is requested from an existing Schematic or Layout window.

New Design

Requesting a new design from any ADS window opens the New Design dialog. This dialog also contains a Schematic Wizard option. (This option is not accessible when a new design is opened from any Layout window.) If the wizard option is selected, the Schematic Wizard will open after you click OK in the New Design dialog. The default setting for the Schematic Wizard option is controlled by its preference setting in the Main Preference dialog. If it is selected in the Main Preference dialog, it will be checked by default in the New Design dialog.

When setting the design content options, the Schematic Wizard and Schematic Design Templates cannot be used at the same time since they both place components on the Schematic. Therefore, selecting the Schematic Wizard option automatically clears any request for a Schematic Design Template. Similarly, requesting a Schematic Design Template automatically clears the Schematic Wizard option.

Simulation Error

If you run a simulation using a simulation schematic that is not properly configured, the simulator will terminate with errors. If the Schematic Wizard option is selected, the wizard will appear automatically after the simulation attempt has completed if the error occurs due to either of these reasons:

• A schematic with an S-parameter simulation controller does not contain any valid Term components.
• The simulation schematic does not contain a valid simulation controller.

You can use the Schematic Wizard to help you correct the schematic. See Correcting an S-Parameter Simulation Schematic and Correcting a Simulation Schematic with No Simulation Controller.

Schematic Wizard Start Page

When the Schematic Wizard appears, the Start page presents you with the following choices for proceeding with the schematic creation:

• Circuit Helps you create a subnetwork that can be used as a component in another ADS design. See Creating a Circuit.

• Simulation Helps you set up a simulation and place a circuit to be simulated. See Creating a Simulation Schematic.

• No help needed Dismisses the wizard.

When the Schematic Wizard is accessed by starting a new project or opening a new schematic window, this page also offers the option Do not show this dialog again. Selecting this option will turn off the Schematic Wizard preference. You can select the Schematic Wizard preference option again in the Main Preferences dialog.

Schematic Wizard Navigation

The Schematic Wizard provides a navigation bar in the upper left corner of the window. This navigation bar indicates your progress through the steps required to complete the schematic setup, with a green box next to the current step. The steps on the navigation bar change depending on the options you select in the wizard.

Use the Back and Next buttons to move back and forth through the steps. The Back button is active for all steps except for Start. The Next button remains inactive for each step until you make a valid selection. When you have completed all required steps, use the Finish button to initiate schematic creation. The final step also provides an option to have instructions appear that assist you in the remainder of the schematic creation process. This option is persistent, so the setting for this option is the default the next time the wizard is used.

Creating a Circuit

Choosing the Circuit option from the Start page enables you to create a subnetwork that can be placed in another ADS design. Creating a subnetwork involves placing and naming ports, and selecting a symbol that will represent the circuit. The steps associated with this choice are:

• Circuit Setup
• Name Ports
• Finish

Circuit Setup Step

Network ports represent the connections of a circuit to the outside world. In this step of the design, you must specify how many ports you anticipate for your circuit. For example, if designing an amplifier from a transistor and passive components, the circuit might have an input, output, and bias connection. In this case, you should request three network ports.

A symbol is used to represent a subnetwork when it is placed within another ADS design. Each connection point on the symbol will correspond to one of the subnetwork ports. ADS can automatically generate a symbol for you based on the number of ports specified, which is achieved using the Use default symbol option. However, if you want your symbol to be representative of the underlying subnetwork, use the Allow symbol selection option. You will be provided with a large set of possible symbols from which to choose.

Correctly specifying the number of ports at this stage of the process will ease the work in creating the subnetwork. However, if you later determine that you must add or remove a port from the circuit, this can be done manually. It is important, however, that the change is made to both the circuit design and the symbol in order for the subnetwork to function properly.

Naming Ports Step

Ports created in ADS assume default names of P1, P2, etc. However, to make the port designations more physically meaningful, it is possible to specify alternate names for these ports. In this phase of the process, you may either use the default names provided or type in the desired names for each port.

If you chose the Use default symbol option in the Circuit Setup step, you are given the opportunity to determine whether or not you would like instructions to appear after the wizard has completed the setup. However, if you chose the Allow symbol selection option, this option regarding supplemental instructions is not available. In this case, the instructions will be shown to help you create the custom symbol and return to the schematic view following symbol selection.

Finish Circuit Creation Step

Successful completion of the wizard leads to a starting design in which ports are placed. If you chose to allow ADS to create a default symbol for you, you will see the requested number of ports placed on the schematic. You can view the symbol that has been created for you using the View > Create/Edit Schematic Symbol menu selection. If you go to the symbol view, you can return to the schematic using the View > Create/Edit Schematic menu selection. If you chose to have supplemental instructions provided, a dialog will also appear, similar to the following figure, containing these instructions. You can move this dialog out of the way to interact with the schematic.

If you chose to create a custom symbol in the Circuit Setup step, the Symbol Generation dialog box appears with a selection of different symbols. You can scroll through these selections and choose a suitable symbol. Be sure, however, that the number of pins on the symbol matches the number of ports specified on the wizard. Once you have selected a symbol, you can return to the schematic view either using the Schematic button on the Schematic Wizard's instruction dialog or the View > Create/Edit Schematic menu selection. If you chose a symbol with a number of pins that does not match the specified number of ports, you will be warned of this problem when you return to the schematic view provided that the dialog containing the instructions is currently visible.

In either case, once you are in the schematic view, you can create the appropriate design and connect it to the ports at the proper nodes in the circuit. Once the design has been saved and provided a suitable name, it will be ready for placement in other designs.

Creating a Simulation Schematic

Choosing the Simulation option from the Schematic Wizard Start page enables you to create a schematic that will simulate the behavior of a sample or user-created circuit. Creating this schematic involves choosing the desired application, specifying the test circuit, indicating the desired simulation type, and when appropriate, specifying how a circuit should be placed in the simulation schematic. The steps associated with creating a simulation schematic are:

• Application
• Circuit
• Simulation Setup
• Finish

Application Selection Step

The first step in creating a simulation schematic is choosing the application type. A variety of different choices representing common applications are provided. If you find your intended application on the list, you can select it. If you do not see your application, the Schematic Wizard may still be able to provide assistance in creating your schematic. Simply choose the Other Application (not listed) option at the bottom of the tree.

Hint The wizard will not allow you to proceed until you have made a valid selection from the list. Top-level items in the tree structure that have sub-items beneath them are not valid selections.

Circuit Selection Step

Once you have determined the application type, you are ready to specify the circuit that will be simulated within the schematic. Three options are provided relative to the test circuit:

• Use sample design A sample circuit appropriate for the application is provided. This circuit will be copied into your project directory and connected into the simulation schematic.
• Use existing design Enables you to specify an existing ADS subnetwork (created, for example, using the Circuit option of the Schematic Wizard ) for placement within the simulation schematic. All designs in the current project will be shown. However, if you select a design that has not been properly created for use as a subnetwork, a warning will be issued and the design will be deselected. If you have a design within another project that you would like to use, you can copy it into the current project using the Copy Design from Another Project button.
• I will design my own circuit No test circuit will be placed in the simulation schematic. It is assumed that you will design your own circuit and manually connect it into the schematic created by the wizard.

The availability of each option is dependent on the selection made at prior steps.

Hint The wizard will not allow you to proceed until you have made a valid selection.

Simulation Setup Step

You are now prepared to specify the type of simulation that you would like to complete. Based on prior selections, a list of possible simulations is offered. If you could not find your desired application earlier ( Other Application ), then at this stage you are presented with a tree structure of common simulations as well as system and user-defined simulation templates. The Description area below the list of simulations helps you to choose from the different simulation options.

Hint The wizard will not allow you to proceed until you have made a valid selection.

Port Specification Step

If you chose Use existing design in the Circuit Selection step, and you have selected a valid design to use as a test circuit within your simulation schematic, the Port Specification step is added. You must use this step to indicate what each of the pins on the component refers to within the subnetwork. Based upon application/simulation selections, you will be given a list of possible designations for each port. Using the pull-down list, specify the appropriate port type. If you do not see the port type listed, you can choose either to ground the port or leave it unconnected (open circuit termination). The circuit will be placed on the schematic at this point so that you can visually inspect it to assist in the port designation.

Hint Using the Back button at this step will remove the placed circuit from the schematic.

Schematic Completion Step

Successful completion of the wizard leads to a schematic that is nearly ready for simulation. If you requested that instructions be provided in the Simulation Setup step, a dialog will appear with information to assist you in performing the specific tasks associated with completing your design, simulating the circuit, and viewing the simulation results.

Important Be sure to save the design if you want to preserve it.

If you chose to use a simulation template (obtained using the Other Application path), you must manually connect the test circuit (if specified) into the simulation schematic. Some templates may already have a test circuit included, in which case you can either use the existing test circuit or delete it and put the specified test circuit placed by the wizard in its place. Furthermore, if you chose to create your own circuit, you must do so before meaningful results can be generated by the simulation.

Each simulation schematic is associated with a display template. Once you have completed the schematic and successfully simulated a design, a display window will appear showing the results of the simulation for your circuit.

Correcting an S-Parameter Simulation Schematic

If a simulation schematic contains an S-Param simulation controller but does not include Term components, the Schematic Wizard will appear (if the preference is set). In this case, the Start page will indicate the error and give you the option of using the wizard to assist in correcting the schematic. The tasks associated with correcting an S-parameter simulation schematic are:

• Term Properties
• Finish

This page also offers the option Do not show this dialog again. Selecting this option will turn off the Schematic Wizard preference option. You can select the wizard option again in the ADS Main window: Tools > Preferences.

Term Properties Specification Step

The first step in correcting an S-parameter simulation schematic is specifying the reference impedance for the ports in the network. You can later change this value by editing the parameters of the Term components placed on the schematic.

Hint The wizard will not allow you to specify an invalid reference impedance.

Term Placement Step

You are now prepared to place your S-parameter network ports ( Term components) on the schematic. Simply click the mouse at the locations in the circuit where you would like to place a Term. The Schematic Wizard will automatically place the component for you with a ground, and the ports will be numbered in the order in which they are placed. Placing the Term components directly on a node of a circuit will result in their automatic connection to the circuit. Placing them elsewhere will require that you manually wire the Term components to the desired nodes after you have finished placing them. If the placement is not exactly what you had intended, you can manually move and rewire the Term components after completion of the placement step.

Once you have finished placing all desired terms, click Finished.

Schematic Completion Step

If you requested that instructions be provided in the Term Properties step, a dialog will appear with information to assist you in performing the specific tasks associated with completing your design and simulating the circuit. If you did not place the Term components directly on a circuit node, you will need to manually wire them to the intended nodes in the circuit.

Important Be sure to save the design if you want to preserve the changes.

Correcting a Simulation Schematic with No Simulation Controller

If a simulation schematic does not contain a simulation controller, the Schematic Wizard will appear (if the preference is set). In this case, the Start page will indicate the error and give you the option of using the wizard to assist in correcting the schematic. The tasks associated with correcting the simulation schematic are:

• Template Setup
• Finish

This page also offers the option Do not show this dialog again. Selecting this option will turn off the Schematic Wizard preference. You can select the wizard option again in the ADS Main window: Tools > Preferences.

Template Setup Step

You can now specify the type of simulation that you would like to complete. You are presented with a tree structure of common simulations as well as system and user-defined simulation templates for the design type (Analog/RF or DSP). The Description area below the list of simulations helps you to choose from the different simulation options. If you do not wish to place an entire simulation template, you can choose to place only a simulation controller by selecting the Place simulation controller only option.

Hint The wizard will not allow you to proceed until you have made a valid selection from the list. Top-level items in the tree structure that have sub-items beneath them are not valid selections.

Schematic Completion Step

If you requested that instructions be provided in the Template Setup step, a dialog will appear with information to assist you in performing the specific tasks associated with completing your design and simulating the circuit. For most templates, this will include placing the requested simulation template in the desired location on your schematic. If, however, you requested a full S-parameter simulation template, the main elements of the template will be placed at the top of your schematic and you will be given the opportunity to place the Term components on the schematic. The instructions will not appear until you have clicked Finished on the dialog that appears.

Important Be sure to save the design if you want to preserve the changes.

Using the Smart Simulation Wizard

The Smart Simulation Wizard is provided to assist new ADS users, as well as those who use it infrequently, in setting up simulations for typical microwave/RF circuits. The wizard will guide you through the process of:

• Selecting an application-specific design (or your own design)
• Selecting predefined simulation setups
• Specifying simulation settings (frequency, bias, etc.)

The wizard then configures the sources and simulation controls and begins the simulation(s). When multiple simulations-requiring different configurations-are requested, the wizard automatically reconfigures the subnetwork for the appropriate sources, terminations, and simulation controls. When the simulation is finished, simply click to display the results. Note that although basic simulation setups are provided with the various simulator licenses, additional simulation setups require specific DesignGuide licenses. These differences are identified in the wizard.

To invoke the Smart Simulation Wizard :

From the Schematic window in the project of interest, choose Simulate > Smart Simulation Wizard.

Step 1 prompts you to select one of several different application types.

Device Characterization	BJT Characterization FET Characterization MOSFET Characterization
Amplifier	Amplifier
Mixer	Single-Ended Mixer Differential Mixer
Linear Circuit	Linear 2-port Linear 4-port

Step 2 prompts you to select one of the following design types:

• A sample design provided by the Smart Simulation Wizard
• An existing ADS subnetwork design
• A new subnetwork design

Step 3 varies based on the choice made in Step 2. You are prompted to select an existing design, enter a name for a new design, or select one of the following application-specific designs.

Step 4/Step 5 varies based on your previous choices. For an existing ADS design, you are prompted to identify the port type for each port in your design (input, output, base, collector, etc.). For all design types, the wizard then describes how to view the network associated with the schematic symbol and how to access the simulation setup portion of the wizard.

When you click Finish, the top-level design appears, and you will see that it consists of two main parts: a schematic symbol representing the subnetwork to be simulated and a simulation setup symbol.

Note If working with a sample design, the top-level and subnetwork designs, as well as the related data displays, are copied to the current project. If you select an existing design from a different project (via an Included project), that design is copied to the current project.

• Schematic symbol -A schematic symbol representing the subnetwork to be simulated, is visually connected to the simulation setup symbol. Push into the symbol to view, edit, or create the subnetwork.
  When you push into most of the schematic symbols, you will notice that the subnetwork designs contain cautions against deleting or renumbering of ports.
• Simulation setup symbol -The simulation setup symbol is similar to the one shown next. Double-click (or right-click and select the first choice from the pop-up menu) to specify the simulation setup details.

Each simulation is marked with one of two icons, as shown next.

You can highlight any selected simulation (from the list box on the right) and click Show Schematic to view the design containing the simulation setup.

From the Simulation Settings tab you can specify the desired settings for the simulation parameters such as frequency, power, bias, etc. When you have selected all the desired simulations and specified the desired settings, click Simulate to proceed. The progress window appears and is dynamically updated to indicate which simulations have completed and which remain. When all simulations are complete click Display Results to view the data displays. Note that the results for each simulation are displayed on separate pages, which can be accessed individually from the Page menu.

Hint After simulating a given design once, you can display the results from the previous simulation via the pop-up menu. Position the pointer over the simulation setup symbol, click right, and select Display Data from Last Simulation.

Selecting Simulation Controllers

Simulation controllers are grouped in a number of simulation palettes accessed from the Component Palette List.

Each palette contains the specific simulation controller, plus:

• The Options component
• Components for defining sweep plans and parameter sweeps
• Node set components
• Measurements
• Frequently-used components, such as ports and sources

To use a controller, select it from the palette, position the pointer in the drawing areas of the Schematic window and click to place it.

Using the Simulator Options Component

This section discusses the details about the Options component in ADS. The Options component includes general simulation options such as convergence tolerances, warnings, and global noise temperature. An Options component can be used with any ADS simulation, and it is available from every simulation palette. The options cover the following areas:

Tab Name	Description	For details, see...
Misc	Miscellaneous options for simulation and model temperatures, topology checking, and linear and nonlinear devices.	Setting Miscellaneous Simulation Options
Convergence	Options related to voltage and current convergence tolerances.	Setting Convergence Options
Output	Sets warnings, and the saving of branch currents and node voltages.	Setting Output Options
DC Solutions	Saves DC solution to a file to re-use as an initial guess in further simulations.	Setting DC Solution Options
Display	Controls the visibility of simulation parameters on the Schematic.	Displaying Simulation Parameters on the Schematic

Setting Miscellaneous Simulation Options

Use the Misc options described in the following table to control simulation and model temperatures, topology checking, and set options for linear and nonlinear devices. In the table, names used in netlists and ADS schematics appear under Parameter Name.

Note Simulator options are commonly used in nonlinear noise analyses. The IEEE standard temperature (T0) for noise figure measurement is 290 K (16.85 degrees Celsius). This can be set by editing Simulation temperature to that value (on Misc tab).

† For more information about topology checking see DC Simulation.

Setting Convergence Options

The simulators work using an iterative method to solve the nonlinear equations. Given an initial guess x_0, it computes a new guess x_1. From that, it computes x_2. This continues until convergence is reached. When x_j is close to x_j-1, it is considered converged, and the solution stops changing. Convergence is defined as follows:

if (x_j− x_j−1 < reltol*x_j + abstol) then
converged
else
keeps iterating

If the difference between the two iterations is less than the relative tolerance times the solution plus an absolute tolerance, the convergence is effective.

Note Advanced simulation parameters are accessible with this group. However, as a result of the improvements made to the DC simulation algorithm, it is extremely unlikely that the default values need to be modified. You are strongly encouraged to leave the advanced parameters set to their default values. If you encounter a circuit for which a DC analysis does not converge using the default values, or you find it necessary to change the value of any of these parameters, please contact Agilent EEsof Technical Support. See Setting Advanced DC Convergence Options for details about these parameters.

Caution Simulator parameters saved in design files in previous releases are supported in later releases. The advanced simulation parameters saved prior to and opened in ADS 2005A are recognized and populated in the simulation setup dialog box. However, due to the improvement in robustness and speed of the default DC simulation algorithm the user-defined values are disabled, and factory-defined default values are used. Changing these default values is not recommended. However, if you find it necessary to restore the original user-defined values, you must manually enable Advanced Settings to restore them.

Use the Convergence options described in the following table to select voltage and current convergence criteria (tolerances) which apply to all analysis types. In the table, names used in netlists and ADS schematics appear under Parameter Name.

Default Preset Tolerance Values

	Relaxed	Intermediate	Strict (default)
V_RelTol	10 -3	3x10 -5	10 -6
I_RelTol	10 -3	3x10 -5	10 -6
V_AbsTol	10 -4	10 -5	10 -6
I_AbsTol	10 -8	10 -10	10 -12

Note If simulator options are not set, transient analysis uses a default value of 10 -3 for V_RelTol, and I_RelTol, while all other analysis types use the default value of 10 -6. If simulator options are set, they apply to all analysis types.

Current Relative Tolerance, Current Absolute Tolerance

These tolerances are used to satisfy Kirchhoff's Current Law (KCL) in solving for the currents at each node in the circuit. The simulator attempts to find a solution that satisfies KCL, so that the sum of the currents entering (or leaving) all circuit nodes is zero. At each iteration, it uses Current relative tolerance and Current absolute tolerance as a tolerance for the node currents. For convergence to be achieved, the currents must satisfy the following at each circuit node:

where

= Current in each branch connected to the node

= Current relative tolerance

= Current absolute tolerance

The default value for Current relative tolerance is 10 ^-6 (0.0001 percent), and the default value for Current absolute tolerance is 10 ^-12 (1 pA). For many problems, these tolerances are much tighter than they need to be. (The default value of Current relative tolerance in Berkeley SPICE 3e1 is 10 ^-3.) Relaxing these tolerances not only allows problem circuits to be solved, but it also allows them to be solved in less time.

Voltage Relative Tolerance, Voltage Absolute Tolerance

Once Kirchhoff's law is satisfied for all nodes, the simulator checks for unique solutions by calculating all node voltages. Sometimes, large changes in node voltages cause very little change in node currents. For instance, if two S-parameter blocks (that is, any 2-port, such as an amplifier or filter, for which there are measured S-parameters) are cascaded, and the reference node between the two components is not grounded, then the differential voltage between the two S-parameter blocks can have any value at all without changing the currents. The circuit then has multiple possible solutions. To find the correct solution for all node voltages, the simulator will use the Voltage relative tolerance and Voltage absolute tolerance parameters in a manner similar to the way it uses Current absolute tolerance and Current relative tolerance. For convergence, the following relationship must be satisfied for every node voltage in the circuit:

where

= Change in the node voltage solution from the previous iteration

= Node voltage found in this iteration of the solution

= Voltage relative tolerance

= Voltage absolute tolerance

The default value for both Voltage relative tolerance and Voltage absolute tolerance is 10 ^-6. Like Current absolute tolerance and Current relative tolerance, these tolerances can be loosened to help with simulation convergence and speed.

Setting Advanced DC Convergence Options

The stand-alone DC simulator's sole role is to do a DC analysis. All other simulators such as AC, S-parameter, transient, harmonic balance, and circuit envelope do an initial DC analysis as their first step. The Advanced DC Convergence options are used to control the initial DC analysis done by these simulators. For information about setting up stand-alone DC simulations, see DC Simulation.

The robustness and speed of the default DC analysis algorithm has been significantly improved in ADS 2005A. All DC analyses with factory-default settings are expected to converge to the correct solution with near-optimal speed. This means that it is extremely unlikely that either of the following advanced simulation parameters must be altered:

DC_ConvMode
MaxDeltaV

Use the options in the following table to select Advanced DC convergence options. In the table, names used in netlists and ADS schematics appear under Parameter Name.

† For more information about setting MaxDeltaV and DC_ConvMode for DC simulations, see DC Simulation.

Setting Output Options

Use the Output options described in the following table to select warnings options, as well as to determine whether branch currents and node voltages will be saved. In the table, names used in netlists and ADS schematics appear under Parameter Name.

Note These Output options available in the Options component are not the same as the Output parameters used in other simulation setup dialog boxes, such as HB, AC, etc., which are described in the section Selectively Saving and Controlling Simulation Data.

Note A resistor has threshold parameters for wPmax and wImax, for maximum power and current dissipation, respectively (all such settings begin with "w," which signifies a warning will be issued in the Simulation/Synthesis Messages window). Some components also check voltages. A BJT has eight threshold settings. All diodes, transistors, FETs, resistors, capacitors, current probes, and shorts contain threshold parameters.

Setting DC Solution Options

You can save the complete DC solution to a file and then re-use it as an initial guess in further simulations. For large circuits or those with time-consuming DC simulations, this can save a significant amount of CPU time by avoiding the needless repetition of the same or similar simulations each time. This applies to any simulation that either performs or relies on a DC solution, which includes all simulations with nonlinear elements.

For example, once a DC solution is obtained by running an AC simulation, future AC simulations at different frequencies or linear noise simulations do not have to re-simulate to get the same DC solution again. If the circuit is changed, either via a parameter change or even a topology change that will change the DC solution, this saved DC solution can still be used as an initial guess for the new DC solution. If the circuit change was not too extensive, then having a reasonable initial guess usually will still reduce the total re-simulation time. If the circuit change is so extensive that the simulation cannot converge using the supplied initial guess, then the simulator will proceed with its normal DC simulation algorithm. In this case, it would save CPU time to disable the Use Initial Guess.

If the circuit topology has changed between the time the solution file was created and when it is used as an initial guess, the simulator will still attempt to use as much of the data as possible. It will also output various messages, if desired, noting what has changed between the two versions. While this feature does not check for parameter changes, it can be a useful tool for comparing the topology of two circuits, or to identify what has changed since the solution was last saved. Items checked include the total number of equations (nodes and branches), the total number of instances and their names, and most connectivity changes.

For information on initial guess and final solution options available in the Harmonic Balance simulation controller, see Setting Up the Initial Guess.

Use the DC Solutions options in in the following table to select options for saving DC solutions. In the table, names used in netlists and ADS schematics appear under Parameter Name.

Sweeping Parameters

Most simulations are performed over a range of values instead of just a single point. You can sweep over time or frequency (depending upon the type of simulation) or you can elect to sweep over another parameter. For ADS, you can sweep one or more parameters using the following methods:

• You can set the sweep range of time, frequency, or a single other parameter (under the Sweep tab for a given simulator controller).
• You can use the ParamSweep and SweepPlan components for sweeping more than one parameter, or sweeping over more than one range of values. These components appear on all simulation palettes. For details about using on using these components, see Parameter Sweeps and Sweep Plans.

If using the Load Sharing Facility (LSF) utility, you can break up a sweep and run the simulation on multiple machines, in parallel, by selecting Parallel Hosts as the Simulation Mode ( Simulate > Simulation Setup ). Individual sweep points are run on each machine and the results are combined into a single dataset on the local machine. For details on setting up remote and local machines for remote processing, see "Using Remote Simulation" in the installation documentation for your platform:

• Windows Installation
• UNIX and Linux Installation

Optimizing a Design

You can set up nominal optimizations or statistical yields as part of a simulation. These features require a separate license. For complete information, see the Tuning, Optimization, and Statistical Design documentation.

Working with Expressions

You can add variables, functions, and conditional statements to a schematic, making your designs more flexible and versatile.

You can use these items:

• In component parameter definitions. From the component parameter editing dialog box, select the parameter and, if available, click Equation Editor. You can write an expression that defines this parameter.
• In variables. Variables can be added to a schematic using the VAR (VarEqn) component, which can be found in the Data Items palette. Once a variable is defined, it can be used in expressions within the design.

You can also add measurements to a schematic. Measurements are predefined functions that process data so that it can be presented in the Data Display. There are numerous predefined measurements under the simulation palettes, but you can also create your own using the MeasEqn component.

For more information on how to use measurements, see Measurement Expressions.

Expressions Examples

Many of the projects in the Examples directory use variables and measurements. One example that includes many variable definitions plus conditional statements is NADC_PA_Test.dsn in RF_Board/NADC_PA_prj.

Saving and Controlling Simulation Data

The results of the simulation are stored in a dataset. This dataset is then used by the Data Display for viewing results. You can select the name and location of the dataset you want to use for a simulation. The default name of the dataset is the name of the design.

Note If you accept the default dataset name and perform multiple simulations, the dataset will be overwritten each time. To collect separate datasets for each simulation, specify a unique name (for the dataset you are about to create) prior to each simulation.

To specify a dataset name prior to simulating:

1. In the Schematic window, choose Simulate > Simulation Setup.
2. In the Dataset field, enter the name of the dataset where you want simulation data to be saved. Click Browse to view existing dataset names in the current project. Click Apply or, if you are ready to run the simulation, click Simulate.

   Hint Datasets are stored in the /data subdirectory of a project. This means that you should provide unique names for the datasets that will be generated from the different designs in the same project directory.

3. Supply a name in the Data Display field, or accept the default name.
   Data Display --The name you specify here will be the title of the Data Display window that is opened, and the default filename should you choose Save As (from the Data Display window). The default name shown is based on the current design name.
   Open Data Display when simulation completes --If enabled, a Data Display window will open automatically when the simulation is complete. For details see Automatically Displaying Simulation Data.
4. Select the desired Simulation Mode:
   • To simulate on a single machine, select Single Host. Select the Single tab and select the desired Simulation Host Type, Local or Remote. If you select Remote, you can then select Specify to choose a specific server by name, or select Find Fastest and let the Load Sharing Facility (LSF) choose the most suitable remote host.
   • To break up your sweep and simulate individual parts simultaneously on remote machines, select Parallel Hosts. In the Parallel tab, select the desired Sweep Variable from the drop-down list and set the desired Start, Stop and Step values. Individual sweep points are run on each machine and the results are combined into a single dataset on the local machine.
   • To break up a signal processing BER simulation over multiple hosts, select Parallel Hosts. In the Parallel tab, check the Parallel BER check box, and specify the number of hosts to be used in the Number of Partitions field. This feature is only available when BER simulation is using one of the berMC, berMC4, or BER_FER components. For more information, see the documentation for these components in Signal Processing Components documentation.

     Note Taking advantage of the LSF utility requires the installation and configuration of that software on the necessary files/machines. For details on setting up your remote and local machines for remote processing, see "Using Remote Simulation" in the installation documentation for your platform: Windows Installation UNIX and Linux Installation

Automatically Displaying Simulation Data

When setting up your simulation ( Simulate > Simulation Setup, in the Schematic window), you can enable an automatic display of your results.

Select the Open Data Display when simulation completes option to force a Data Display window to open automatically when the simulation is complete. The data display that appears in that window depends on the simulation setup and the status of display templates:

• If you specify the name of an existing display to open, that display is opened.
• If you specify a new name, then a blank Data Display window opens.
• If one or more data display templates are associated with the current design, then the Data Display window opens and inserts each template on its own page. A data display template can be associated with a design in one of two ways:
  • By default, if your design includes a supplied schematic template, and a data display template is associated with that schematic template.
  • Explicitly, if you create your own data display template ( File > Save As Template in the Data Display window) and associate that template with your design via the DisplayTemplate component. (See the next section, Using a DisplayTemplate Component)
• If none of the above criteria are met, but you select the option, then a blank Data Display window opens.

Using a DisplayTemplate Component

The DisplayTemplate component (available from most simulation libraries) enables you to associate one or more data display templates with a given design. (If you include one of the supplied schematic templates in your design, it most likely has a data display template associated with it.)
The starting point of this procedure assumes you have already created a data display file for use as a template, by setting up the Data Display window as desired and choosing File > Save As Template.
To associate a data display template with the current design:

1. Place a DisplayTemplate component in the Schematic window.
2. Select String and Reference as the Parameter Entry Mode.
3. Enter the name of the template (the filename you supplied in the Data Display window) and click Add.

   Hint You can specify multiple templates for the same data display and subsequently access them from the Page menu).

4. When you are through specifying display templates for the current design, click OK.

Manually Displaying Simulation Data

If you do not want the Data Display window to open automatically, disable the option Open Data Display when simulation completes in the Simulation Setup dialog box.
To open a new window for displaying and manipulating data:

Choose Window > New Data Display from the Main, Schematic, or Layout windows.

To save a graph for later viewing/manipulating:

Choose File > Save.

To save a graph for use as a template:

Choose File > Save As Template.

To open a previously saved data display:

1. Choose Window > Open Data Display from the Main, Schematic, or Layout windows. In the dialog box that appears, the path is automatically set to the current project directory and the filter displays all saved graphs (*.dds).
2. Double-click the graph you want to open or select it and click OK.

For details on working with simulation data, see Data Display.

Selectively Saving and Controlling Simulation Data

The Output tab in all A/RF analysis components can be used to create an Output Plan, which controls the data that will be saved to the dataset. You can control output generated from named nodes, buses, measurement and VAR equations. By default, all named nodes up to two levels below the top level are saved. The data from all measurement equations and components with the parameter SaveCurrent set to yes is also saved. You can also control the saving of data using the hierarchy level for nodes and measurement equations or by explicitly specifying the output quantity.

Note The Output tab described in the section is used in the simulation dialog boxes, such as HB, AC, etc. It is not the same as the Output tab used in the Options component, which is described in the section Setting Output Options.

To modify the default behavior of sending data to the dataset:

1. Edit the analysis controller item, and select the Output tab.
   
   • To output all named nodes/measurement equations in the top-level design only, select the Node Voltages and/or Measurement Equations options and use zero as the Maximum Depth.
   • To output all named nodes/measurement equations in the top-level design and one or more levels in the hierarchy, select the Node Voltages and/or Measurement Equations options and set the desired Maximum Depth.

     Note When you use the Save by hierarchy options, all data from the specified levels is output-you cannot restrict it. However, you can add to it, selectively, from lower levels in the hierarchy using the Save by name section.

   • To output named nodes/measurement equations selectively, irrespective of the hierarchy, disable the Node Voltages and/or Measurement Equations options in the Save by hierarchy section and use the Save by name section to select only those nodes/equations you want to output. (Click Add/Remove to open the Edit Output Plan dialog box.)
2. If using the Save by hierarchy method, select the desired level of hierarchy and click OK.
3. If using the Save by name method (alone or in conjunction with a specified level of hierarchy), click Add/Remove.
   The Edit Output Plan dialog box appears with a list of available nodes and equations.
   

   Note Buses appear in the list box as nodes. They do not contain any indices (as they do in the design environment). Individual components of a bus cannot be output.

4. Select each individual node from the Available Outputs list that you want to send to the dataset and save for each iteration (time, frequency) for the next simulation. Click Add to move each to the Current Selection list box. Selected nodes will be stored in the parameter NodeName[i] on the schematic.
   
5. Select each individual equation you want to send to the dataset and save at the end of the next simulation. Click Add to move each to the Current Selection list box. Selected equations will be stored in the parameter SavedEquationName[i] on the schematic.
   
6. In addition, you can also select individual equations appearing in the Current Selection list box to be saved for each iteration (time, frequency) of the next simulation. Select an equation in the Current Selection list box and check the option labeled Evaluate equation at each analysis point.
   The option must be checked separately for each equation appearing in the list. The checked equation will be stored in both parameters SavedEquationName[i] and AttachedEquationName[i] on the schematic.
   

   Note A non-selected equation may still be output depending on the Maximum Depth setting, but all data will be processed at the end of all simulation iterations, requiring more memory.

   If an equation is selected for any one simulation, it will not be output for any other simulation for which it is not explicitly selected.

7. Click OK to accept all changes. The selected nodes and equations are then displayed in the Save by name section on the Output tab.
8. Make any other desired changes for this analysis and click OK.

Output Tab Fields for Simulation Controllers

Following are more detailed explanations of the dialog box fields.

Save by hierarchy. Enables you to save the data in the active hierarchical designs. To output all named nodes/measurement equations in the top-level design only, select the Node Voltages ( UseNodeNestLevel ) and/or Measurement Equations ( UseSavedEquationNestLevel ) options and use zero as the Maximum Depth ( NodeNestLevel/SavedEquationNestLevel ). To output all named nodes/measurement equations in the top-level design and one or more levels in the hierarchy, select the Node Voltages and/or Measurement Equations options and set the desired Maximum Depth. When you use the Save by hierarchy options, all data from the specified levels is output-you cannot restrict it. However, you can add to it, selectively, from lower levels in the hierarchy using the Save by name section (see next paragraph).

Save by name. Identifies the names of individual nodes and equations that you want to save to a dataset. To output named nodes/measurement equations selectively, irrespective of the hierarchy, disable the Node Voltages and/or Measurement Equations options in the Save by hierarchy section described in the preceding paragraph and use this section, along with the secondary Add/Remove dialog box (see next paragraph) to select only those nodes/equations you want to output.

Add/Remove. This button opens the Edit Output Plan dialog box, which corresponds to the node voltages and measurement equations included in the active design. In this dialog box, deselect Equations ( SavedEquationName[1], AttachedEquationName[1] ) if you want to view a shorter list while adding selections. Choose the Add button to select equations that you want to include in the data to be saved. Choose the Remove button to take equations out of the Current Selection list. The selections in this list will be reflected in the Save by name box in the controller dialog box, and will be evaluated after your analysis is finished. If you would like the selected equation to be evaluated at each analysis point, select the Evaluate equation at each analysis point option.

Displaying Simulation Parameters on the Schematic

You can reduce screen clutter by displaying on the schematic only the parameters you are interested in. Whether a parameter is displayed or not does not affect its functionality. However, some parameters must be displayed to be used.

DC Simulation Display Options

Display
Display parameter on schematic-Enables you to set the visibility of simulation parameters on the schematic. Set All-Use this option to quickly select all parameters, and then deselect those you do not want to display. Clear All-Use this option to quickly deselect all parameters, and then select only those you want to display.

Controlling a Simulation

You can select how to start and end a simulation:

• To start a simulation, choose Simulate from the Simulate menu. You can also start one by clicking the Simulate button on the tool bar or by pressing F7.
• To end a simulation before it is finished, choose Stop and Release Simulator from the Simulate menu. This will release your simulation license. To end the simulation but keep the license, choose Simulation/Synthesis > Stop Simulation from the Simulation Message window.

You can add more than one simulation component to a schematic, and specify which simulation to run (only one simulator can be active at a time):

To disable simulations that are not desired, choose Edit > Component > Deactivate/Activate and click the appropriate simulation component.

For more information about deactivating simulation controllers, as well deactivating/activating other components in your design, see
Activating, Deactivating, and Shorting Components.

If using the Load Sharing Facility (LSF) utility, you can break up a sweep and run the simulation on multiple machines, in parallel, by selecting Parallel Hosts as the Simulation Mode ( Simulate > Simulation Setup ). Individual sweep points are run on each machine and the results are combined into a single dataset on the local machine. You can also use this utility to select the fastest available machine.

For details on setting up remote and local machines for remote processing, see "Using Remote Simulation" in the installation documentation for your platform:

• Windows Installation
• UNIX and Linux Installation

Simulating from a Layout

Simulating a layout cannot be done directly from the Layout window; it involves a few steps in the Schematic window. Essentially, you must treat the design as though it were a subnetwork and place it in a higher-level design. To do this, you must create a symbol for it (in the Schematic window).

To simulate a layout:

1. From the Layout window containing the design you want to simulate (in this example, DesignB ), choose Window > Schematic.
2. In the Schematic window for DesignB, create a symbol ( View > Create/Edit Schematic Symbol ). The number of pins must equal the number of ports on the design.
3. Switch back to the Schematic view ( View > Create/Edit Schematic ) and choose File > Design Parameters and select the option labeled Simulate from Layout (SimLay).
4. Save the design.
5. From the Schematic window, create a new design (in this example, DesignA).
6. In the Schematic window for DesignA, open the Component Library and select and place an instance of DesignB.
7. Place the desired simulation control items, as well as any substrate or equation definitions, in DesignA and run the simulation from DesignA.

Viewing DC Solutions

After a simulation is finished, you can display DC node voltages and branch/pin currents on the schematic. Because a DC simulation is part of most other types of simulations as well, this feature is available for most simulations.

• To view DC solutions, from the Schematic window, choose Simulate > Annotate DC Solution. All node voltages and branch/pin currents of the last DC solution – which was obtained from either the last explicit or implicit DC analysis – are displayed on the schematic.
• To erase the solutions from the schematic, choose Simulate > Clear DC Annotation.

Viewing Device Operating Point Data

Any simulation that includes a DC analysis produces DC operating point information for most active and some passive devices in the circuit. This data includes currents, power, voltages, and linearized device parameters of the selected device. An explanation of the displayed parameters, if available, is under the model documentation in the Circuit Component manual.

To view device operating point data:

• From the Schematic window, choose Simulate > Detailed Device Operating Point. Crosshairs appear. Click the component of interest. The details appear in a separate window.
• To view a condensed list of details, choose Simulate > Brief Device Operating Point instead.
• You can save device operating point data to a dataset for viewing in the Data Display. Under the Parameters tab of most simulators, set the Device operating point level as desired.

Displaying Simulation Results

Most of the simulation results are viewed in the Data Display. You can set the Data Display so that it automatically opens when a simulation is finished:

1. Choose Simulate > Simulation Setup.
2. Select the option Open Data Display when simulation completes.
3. Specify a data display file (.dds) and it will be opened in the Data Display window when the simulation is finished.
   The simulation templates include DisplayTemplate components. If your design includes a simulation template and the automatic display option is enabled, then the Data Display window will open with the corresponding display template.
   If neither a data display file (. dds) is specified nor a template used, a blank Data Display window is opened.

Subsequent simulations of the same schematic will not open a new window, but rather bring the existing one to the foreground.

For information on how to work with the items in a Data Display window, see Data Display.

There are also ways to view DC data directly from the schematic. You can view:

• DC node solutions
• DC operating point data

Tuning

ADS tuning capability enables you to change one or more design parameter values and quickly see the effect on the output without resimulating the entire design. Multiple traces generated from various tuning trials can be overlaid in the Data Display window. This can help you find the best results and the most sensitive components or parameters more easily.

Basic tuning consists of the following steps:

1. Build the design you want to tune.
2. Set up your simulation.
3. Simulate your design and verify that your simulation operates as expected.
4. Set up, display, and analyze your results in the Data Display window.
5. Choose Simulate > Tuning or click the Tune Parameters icon (tuning fork) on the toolbar.
   When the initial analysis is complete, the Tune Parameters dialog box appears.
6. Select each parameter you want to tune by clicking it on the schematic. The Tune Parameters dialog box is updated with a new slider for each parameter selected.
7. Change the tunable parameter(s) by moving the slider(s), or clicking the up/down arrows.
8. Update your schematic with the changes.

For complete details about tuning your design, see Tuning, Optimization, and Statistical Design.

Reusing Simulation Solutions

For some types of simulations, you can save a simulation solution, reusing it as an initial guess in a later simulation. This can save time by avoiding repeating the same, or a very similar simulation, on a design. Using a simulation solution as an initial guess can help the subsequent simulation to reach a final answer faster. If you have made minor changes to the design or simulation setup, reusing solutions can reduce CPU time.

You can save and reuse these types of simulation data:

• DC solutions-You can save the complete DC solution and reuse it for any type of simulation that either performs or relies on a DC solution. For example, once a DC solution is obtained by running an AC simulation, then future AC simulations at different frequencies or linear noise simulations do not have to resimulate to get the same DC solution again. This feature is available from the DC Solutions tab of the Options component. For details, see Using the Simulator Options Component.
• Harmonic Balance solutions-You can save a harmonic balance solution and use it as an initial guess for another harmonic balance simulation, large-signal S-parameter, gain compression, or Circuit Envelope simulation. With the saved harmonic balance solution, you can later perform a nonlinear noise simulation and use the saved solution as the initial guess, removing the time required to recompute the nonlinear harmonic balance simulation. Another use would be to use the initial harmonic balance solution, then sweep a parameter to see the changes. For details, see Reusing Simulation Solutions.
• Harmonic Balance guess from a Transient simulation-Transient simulations can be set to generate a harmonic balance solution that can then be used as an initial guess for a harmonic balance simulation. For example, in circuits such as dividers, harmonic balance usually cannot directly converge on a solution since multiple mathematical, but useless, solutions exist. By first running a transient simulation and generating a harmonic balance solution file that can then be used as an initial guess, the harmonic balance simulation can converge to the desired solution. This feature is available when setting up the Harmonic Balance or Transient controller. For details, see the following documentation:
  • In Harmonic Balance Simulation, see Transient Assisted Harmonic Balance.
  • In Transient and Convolution Simulation, see Using the Steady State Detector and Transient Assisted Harmonic Balance.

Analog/RF Simulation Computations and Convergence Criteria

Analog/RF simulation computes the response of a circuit to a particular stimulus by formulating a system of circuit equations and then solving them numerically. Each simulation technology accomplishes this analysis as follows.

DC analysis

• Solves a system of nonlinear ordinary differential equations (ODEs).
• Solves for an equilibrium point.
• All time-derivatives are constant (zero).
• System of nonlinear algebraic equations.

Transient analysis

• Solves a system of nonlinear ordinary differential equations (ODEs).
• Time-derivatives replaced with a finite-difference approximation (integration method).
• Sequence of systems of nonlinear algebraic equations (one system at each timepoint).

Harmonic Balance (HB)

• Solves a system of nonlinear ordinary differential equations (ODEs).
• Steady-state method.
• Solution approximated by truncated Fourier series.
• System of nonlinear ODEs becomes a system of nonlinear algebraic equations in the frequency domain.

Solving Nonlinear Algebraic Equations

Nonlinear algebraic equations are solved using the Newton-Raphson algorithm (Newton's method) as follows.

1. Convert the problem to a sequence of systems of linear equations.
2. Quadratic convergence near the solution (error squared at each iteration).
   

Common Circuit Simulation Methods

Backward Euler

• First order method that assumes the solution waveform is linear over one time step
• One-step method (needs one previous time point solution only)
• Adapts faster to abrupt signal changes
• Stable on all stable differential equations and some unstable ones.
• Exhibits heavy numerical damping, increases loss
• Require smaller time step to maintain accuracy

Trapezoidal Rule

• Second-order method, assumes the solution waveform is quadratic over one time step
• One-step method
• May exhibit point-to-point ringing on circuits that have very small time constant comparing to time step (stiff circuit)
• Stable only on stable differential equations
• Exhibits no artificial numerical damping

Backward Difference Formulas (Gear's methods)

• Multiple order polynomial over one time step
• Only the first six orders are available in ADS
• First order method is identical to backward Euler
• Higher-order polynomials allow a larger time step without sacrificing accuracy, are efficient for smooth waveforms
• Higher order methods (order > 2) may exhibit stability problems on lightly damped circuits
• Second-order backward difference formula (Gear 2)
• Two-step method
• Stable on all stable differential equations and some unstable ones.
• Exhibit some numerical damping

Truncation Error

The error made by replacing the time derivatives with a discrete-time approximation. This error is difficult to estimate and depends on the type of circuits and the time steps.

Local Truncation Error (LTE)

The truncation error made on a single step

Global Truncation Error (GTE)

• Maximum accumulated truncation error
• The circuit with long time constant is sensitive to these errors
• Logic and bias circuits are not sensitive to these errors

Convergence Criteria

Newton's iteration is converged if the approximate solution first satisfies the Residue criteria at the end of each Newton iteration and the Update criteria once the residue criteria are satisfied.

Residue criterion

KCL satisfied to a given tolerance. This is enforced at each node and is important when impedance at a node is small.

Update criteria

Difference between the last two iterations must be small. This is important when impedance at a node is large.

Using Continuation Methods

Use continuation methods to provide a sequence of initial guesses that are sufficiently close to the solution to assure Newton's method convergence.

• Choose a natural or contrived continuation parameter which controls a modification of the circuit
• Step the continuation parameter from 0 to 1 (the original circuit configuration), using the solution from the previous step as the starting point.

As long as the solution changes continuously as a function of the continuation parameter and the steps are small enough, Newton's method will converge. Keep in mind though that the first two methods, Source and gmin stepping, will fail if the continuation path contains a limit point.

Source Stepping

Uses a fraction of the source voltages and currents applied to the circuit as the continuation parameter.

• Turn off all sources when the continuation parameter equals 0.
• Raise source levels to their final levels slowly, generating a sequence of circuit configurations.
• Use the solution from the previous configuration as an initial guess for the current configuration.

Gmin Stepping

Uses the continuation parameter to control the value of the gmin resistors

• Start with a large gmin for an easy to compute solution because nonlinear device behavior is muted by the presence of the small resistors.
• End with very small gmins for resistors that are so large that they no longer affect the circuit.
• Remove the gmins to compute the final solution.

Arc-Length Continuation

Works best for complicated continuation paths and limit points using a continuation parameter that is a function of the arc-length parameter

• Travel same distance at each step, as specified by the arc-length.
• Increase or decrease the continuation parameter along the path in each step.

Preventing Convergence Problems

Convergence problems usually arise as a result of errors in circuit connectivity or unreasonable (out of range) model or component values. Some of the steps you can take are as follows.

• Turn on the topology checker (default is on). In ADS, set the topology checker mode on the Options component's Misc tab.
• Turn on warnings.(default is no ). In ADS, set warnings on the Option component's Output tab.
• Act upon the messages in the Status window.
• Eliminate small floating resistors (or increase I_AbsTol). Any error in computed voltages for nodes with small resistors results in large error currents.
• Avoid very large and very small resistances connected to a node. Large resistances are lost during Jacobian construction due to numerical round-offs.

Clearing Highlights from Items Causing Simulation Errors

When an error occurs during simulation, a box is drawn around each item causing an error. To clear all highlights, choose the Clear Highlighting command from the View menu in the appropriate window.

Hint The color of this identifying box is the Highlight color defined through Options > Preferences > Display.