Examples of DC Simulation

There are two examples that describe how to set up and run a DC simulation in ADS:

Simulating a BJT in ADS

The following figure illustrates the setup for a DC simulation of a BJT. This simulation calculates a single DC operating point.

Note
This design, DC1.dsn, is in the Examples directory under Tutorial/SimModels_prj. The results are in DC1.dds.


Setup for a single-point DC bias simulation

To perform a single-point DC simulation:

  1. Place the BJT instance and model on the schematic.
  2. From the Sources-Freq Domain palette, select V_DC. Place the DC voltage source on the schematic to provide the collector voltage and modify the voltage as needed.
    Note
    Ensure that sources are connected either by wires or by means of a named connection (Insert > Wire/Pin Label).
  3. From the Sources-Freq Domain palette, select I_DC. Place the source on the schematic to provide base current and modify the current as needed.
  4. From the Probe Components palette, select I_Probe. Place this current probe in an appropriate location in the circuit.
  5. From the Simulation-DC palette, select and place the DC simulation component on the schematic.
  6. Simulate. When the simulation is finished, you can immediately exercise the following DC simulation options:
    • For a direct representation of currents and voltages at all nodes on the schematic, choose Simulate > Annotate DC Solution.
    • For the details of the device, choose Simulate > Detailed Device Operating Point or Brief Device Operating Point, then click the device when the crosshairs appear.
    • Choose Simulate > Clear DC Annotation to remove the annotation.
  7. In the Data Display, the data from the simulation is presented as a list of DC currents and voltages:

Sweeping Parameters in ADS

By performing a DC swept bias or a swept variable simulation, you can check the operating point of the circuit against a swept parameter such as temperature or bias supply voltage. The resulting data can be plotted to resemble the appearance of a curve tracer.

The following figure illustrates a setup for performing an idealized, swept DC bias simulation of a MOSFET. Vdd and Vgg are swept across a range of voltages. The result is a family of curves representing drain current versus drain voltage, for varying values of gate voltage.

Note
This design, DC2.dsn, is in the Examples directory under Tutorial/SimModels_prj. The results are in DC2.dds.


Example setup for a swept DC simulation
Note
This example uses a referenced model. The parameter cells refers to the extraction parameter known as binning and reflects the electrical characteristics of this particular model. The number of cells has been referenced in a VarEqn component.

To perform an idealized, swept DC bias simulation:

  1. Place the MOSFET instance and model on the schematic.
  2. From the Sources-Freq Domain palette, select V_DC. Place this V_DC component (SRC1) between the base of the device and ground. Edit this component and define Vdc = Vgg1, rather than a numerical value.
  3. Place another V_DC component (SRC2) between the drain of the device and ground. Open this component and define Vdc = Vdd1, rather than a numerical value.
    This makes it possible to sweep these values. Any swept parameter must be initialized by means of an equation, as will be demonstrated later.
  4. From the Probe Components palette, select I_Probe. Place the probe between the drain and SRC2, and rename it if you like (in this case, it has been called Probe1).
  5. From the Simulation-DC palette, select and place the DC simulation component on the schematic.
  6. Edit the DC component by selecting the Sweep tab and modifying the sweep parameters as follows:
    • Parameter to sweep = Vdd1. This appears as SweepVar on the schematic if this parameter is displayed on the schematic.
      Note
      Variables entered in this field will appear in quotes on the schematic. If you enter a variable directly on the schematic (in this case, as the right-hand side of the SweepVar statement of the DC component), you must surround the variable with double quotes. This applies to the other user-defined variables shown in subsequent steps.
    • Start = 0
    • Stop = 6
    • Step = 0.1
  7. Click OK to accept changes and close the dialog box.
  8. Choose Simulation-DC palette, select Prm Swp (ParamSweep). Place this component on the schematic and edit it as follows:
    • On the Sweep tab:
      • Parameter to sweep = Vgg1
      • Start = 2
      • Stop = 3
      • Step = 0.25
    • On the Simulations tab:
      • Simulation 1 = DC1. This appears as SimInstanceName[1] on the schematic if this parameter is displayed on the schematic.
  9. Click OK to accept changes and close the dialog box.
  10. Choose the Data Items palette, select Var eqn (Variables and equations). Place this component on the schematic and enter the following equations:
    • Vdd1 = 4
    • Vgg1 = 2.5
  11. Click OK to accept changes and close the dialog box.
  12. Simulate. When the simulation is finished, plot the probe current (Probe1.i). The resulting family of curves representing drain current versus drain voltage, for varying values of gate voltage, is shown next:
 

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

Contents
Additional Resources