Page tree
Skip to end of metadata
Go to start of metadata


An ADS Simulation Example

This topic is a detailed simulation example for ADS. The circuit is a simple BJT and the simulation is set up to calculate the DC operating point. The simulation process is described here in detail, and this process can be applied to more complex circuits and simulations.

Before continuing with this topic, you should be familiar with the other topics in Using Circuit Simulators, in Schematic Capture and Layout, and in the Advanced Design System Quick Start.

The DC_OP_POINT.dsn design used here is located in the Examples directory under MW_Ckts/LNA_prj . Details on working with example projects can be found in Schematic Capture and Layout.

Working through this example consists of these tasks:

Placing Circuit Sources

In many cases your circuit will contain sources. In this example, you need to select a voltage source that is appropriate for a DC simulation:

  1. From the Component Palette List, choose Sources-Time Domain .
  2. Select V_DC ( DC Voltage Source) and place this component in the Schematic window.
  3. Set the DC voltage (Vdc) to 3.0 V .

Ensuring Sources are Connected Properly

You must ensure that the sources are connected properly to the circuit. You can do this two ways:

  • Wire the source directly to your circuit.
  • Use node names ( Insert > Wire/Pin Label ) to define connections. By labeling the end of the source and a point in the circuit, the source then behaves as if connected physically to that point of the circuit. For example, named connections can be used for Vcc, Vb, and Ve.

If you are wiring components, the color of the pin changes when a successful connection is established. Wires that are simply overlaid on intervening nodes will not be connected to those nodes, and clicking on the intervening nodes after the end node is wired does not ensure that the intervening nodes are connected properly.

In addition, the endpoints of dangling wires (wires that are connected at one end only) can be moved but not edited. To move an endpoint, choose Edit > Move > Move Wire Endpoint . When crosshairs appear, select the open endpoint and move it; the wire will move with it. It is also possible, using standard copy and move commands, to move and copy dangling wires and networks of wires.

To label and share a source:

  1. Choose Insert > Wire/Pin Label and a dialog box appears.
  2. Enter a name for the node (for example, Vcc).
  3. Click the pin of the source you want to label (for example, the positive side of V_DC). The label Vcc appears at that node.
  4. Next click the pin of a node to which you want Vcc to apply (for example, one end of a resistor). The resistor node is also labeled Vcc. (Note that you must click the component pin, not a wire between components.)

    Note

    To delete a named connection, choose Edit > Wire/Pin Label > Remove Wire/Pin Label. When crosshairs appear, click the pin whose connection name you want to remove.

  5. Edit any parameters of the source as needed.

Specifying Points for Collecting Data

You must specify the points in the circuit where voltage and current values will be collected and saved in the dataset:

  • To identify points where you want voltages to be taken, use node names ( Insert > Wire/Pin Label ) or global nodes ( Insert > Global Node ). For circuit nodes that are labeled this way, voltages will be calculated during the simulation and saved to the dataset.
  • For collecting current values, insert current probes (I_Probe) in your circuit at points of interest. Current probes are found on the Probe Components palette.
  • Some components, such as the DC voltage source (V_DC) used in this example, include a SaveCurrent parameter. If this is set to yes , the current flowing through this component will be saved to the data set.

To help identify the data collected by a probe or source, you might want to change the default Instance Name to something more meaningful. For example, you can name a DC voltage source Vsupply. The current through that source will appear in the dataset as Vsupply.i .

Note

Current probes (I_Probe components) must be placed so that the arrow on the probe points in the direction of (positive) current flow. To flip a probe horizontally, choose Edit > Rotate/Mirror > Mirror About Y .

In general, voltage and current data is in phasor representation, so the voltage values at named nodes are peak voltage.

The process for labeling nodes is described in Ensuring Sources are Connected Properly.

To insert a current probe:

  1. Select the Probe Components palette.
  2. Select the I_Probe component and place it at the desired point in your schematic. (You may need to move components or rewire to do this.) Edit the probe component and change the Instance Name to something that suggests its purpose in the circuit.

For details on selectively sending data to the dataset, refer to Selectively Saving and Controlling Simulation Data.

Selecting a Simulation Type

There are a variety of simulation methods to choose from. To use a particular simulator, you must have purchased a license for it. If you do not have a license, a message will appear when you attempt to run the simulator. This may also happen if you share licenses that are already in use.

Each simulator has its own palette, which can be selected from the Component Palette List. Details for using each simulator are described in later topics.

To add a DC simulation component (for this example):

  1. Select the Simulation-DC palette.
  2. Select and place the DC component on your schematic.

Editing Simulation Parameters

There are two ways to edit simulation parameters:

  • You can edit parameters directly on the schematic. Click somewhere within the parameter value to invoke the on-screen editor, and change the value as desired. Press Return to enter data and go to the next entry. Note that by default, not all parameters are displayed on the schematic; to view/edit additional parameters, use the dialog box, as described next.
  • You can edit parameters within the dialog box. To open the dialog box, either double-click the simulation component, or select it and choose Edit > Component > Edit Component Parameters . You can also bring up the dialog box using the Edit Component Parameters icon on the toolbar.

Note

For many simulation options, the default parameters should provide satisfactory results and will not need editing.


You may find it useful to display (on the schematic) the options you have selected, to remind you of the parameters governing a simulation.

To display additional parameters on the schematic:

  1. Select the Display tab.
  2. Select each parameter you want to appear and click OK.

To exercise certain simulation options, you must first display them on the schematic, then set them equal to the desired value. For example, to send a defined power parameter RF_power to the dataset following a simulation, use the Output tab of the DC Operating Point dialog box. Refer to the section Selectively Saving and Controlling Simulation Data.

Selecting a Sweep Type and Plan

The Sweep tab enables you to identify the parameter that you want to sweep, and then specify the sweep type. You can sweep over:

  • A single point
  • A linear range
  • A logarithmic range

After you select the sweep type, you can then specify the sweep range.

You can also select a sweep plan . A sweep plan enables you to specify a sweep once and then use these settings in other places. For more information, refer to Parameter Sweeps and Sweep Plans. Note that for some simulators, these settings are found on the Freq tab.

To set the sweep values for this example:

  1. Double-click the DC component to edit it.
  2. Set the following parameters as shown here:
    • Parameter to sweep = VBE
    • Start = 0.6
    • Stop = 0.85
    • Step size = .002
    • Num. of pts. = 126

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 results combined into a single dataset on the local machine. For details on setting up remote and local machines for remote processing, see the topic Using Remote Simulation in the installation documentation for your platform.

Setting Simulation Options

An Options component can be used with any simulation. The most common use of the Options component is to set the simulation temperature, but it also enables you to specify settings for convergence tolerances, warnings and other advanced options. (For this example, an Options component is not used.)

To add an Options component:

  1. Select any simulation palette.
  2. Select and place a simulation Options component and double-click to edit it. You can set general simulation options such as temperature, DC convergence tolerances, warnings, and other settings.

For more information about each field, click the Help button at the bottom of the Options Component dialog box.

Modifying the Simulation Setup

Additional simulation setup options include:

  • Specifying a name for the dataset to which simulation data will be saved
  • Automatically displaying data when the simulation is finished
  • Selecting a different machine on which to run the simulation

To specify simulation setup options:

  1. From the Schematic window, choose Simulate > Setup . A Simulation Setup dialog box appears:
  2. The data calculated during a simulation is saved in a dataset. The default dataset name is the same as the project. Change the name as desired.
  3. By default, the Data Display will automatically launch when the simulation is complete. If the simulation results were displayed before, the same window will open if you specify its name in the Data Display field.
  4. If you use remote simulation hosts, you can specify a machine other than the local one for running the simulation. For more information on how to set up remote machines, see the installation documentation for your platform.

Starting the Simulation

There are several ways to launch a simulation:

  • Press F7 on the keyboard.
  • Click the Simulate icon on the toolbar.
  • Choose Simulate > Simulate from the Schematic window.
  • Choose Simulate from the Setup dialog box while it is open.

When the simulation begins, a status and error message window appears. When the simulation is complete, the line Simulation finished . at the bottom of the window indicates that the simulation has run successfully. The location of the dataset where the simulation data is saved is also noted.

Displaying Simulation Data

You will typically want to view most of your results in a Data Display, however you also have the option to view DC results on the schematic and view lists of device operating point details. While it is not very useful in this example-given that the DC results are reported only for the last point in a sweep – it illustrates an important feature.

Viewing the DC Solution

  1. Choose Simulate > Annotate DC Solution . DC voltages and currents appear at the pins of all the active devices and lumped elements, as shown below.

    Note

    Current is defined as positive if flowing into a device, so +13.5 mA is flowing from the emitter to ground.

    Note

    To clear the annotations, choose Simulate > Clear DC Annotation from the main menu. You will have to resimulate to annotate again.

Viewing the Detailed Device Operating Point

  1. In the same Schematic window, choose Simulate > Detailed Device Operating Point . Crosshairs appear.
  2. Place the crosshairs over a transistor and click. A detailed DC operating point listing appears.
  3. As you select other devices in a circuit, the DC operating point data for additional devices is added to the list.

For more information about the parameters that are displayed in the list, refer to the documentation for the specified component.

Viewing the Brief Device Operating Point

To view a subset of the above information that covers the most common parameters, choose Simulate > Brief Device Operating Point and select a device. The details are similar to those in the detailed list, but this list contains fewer parameters.

For details about the data that appears in the list, refer to the selected component's documentation.

Viewing More Results in the Data Display

The remainder of the simulations results can be viewed using the Data Display. For complete details on how to use the Data Display, refer to Data Display and to the Advanced Design System Quick Start. The results of this simulation are in DC_op_point.dds. In this example, collector current versus Vbe at Probe1 is displayed.

There are various options for plotting and scaling data. To edit general plot characteristics, select the Plot Options tab. This allows you to enter a title and axis label. It also allows you to deselect Auto Scale and enter a scale that zooms in on a range of interest. You can also choose between linear and log scales here, and select grid characteristics.

To edit a trace before placing it (unless you have selected the List plot type), select the parameter under Traces, then click Trace Options . Select the Trace Type , Trace Options , and Trace Expressions tabs to select, for example, trace patterns, trace colors, and fonts for labels, as well as to edit mathematical expressions for display.

  • No labels