S-Parameter Simulation >Chapter 1: S-Parameter Simulation
Print version of this Book (PDF file)
prevnext

Examples (ADS only)

This section contains examples for:

These examples give detailed descriptions for setting up and running S-parameter simulations.

Simulating an Amplifier

Figure 1-1 illustrates an example setup for performing a basic S-parameter simulation of an amplifier.


Note    This design, SP1.dsn,is in the Examples directory under Tutorial/SimModels_prj. The results are in SP1.dds.

Figure 1-1. Example setup for a basic S-parameter simulation

To perform a basic S-parameter simulation:

  1. From the Simulation-S_Param palette, select a Term component for each port of the component or circuit to be simulated. You can edit the impedances as required, although the default value of 50 ohms is generally sufficient. Ensure that the terminations are properly connected to the component or circuit under test.

  2. Ensure that the number of the input Term component is set to Num = 1, and that of the output Term component to Num = 2.


Note    By default, the Term component provides a noise contribution (Noise = yes), but is inactive unless noise contributions are requested. Also, ensure that the number of each Term component (as defined by the component's Num parameter) is appropriate to the location of the component in the circuit, to ensure that the S-parameter data is meaningful.

  1. From the Simulation-S_Param palette, select SP. Place this component on the schematic and select the Frequency tab. Ensure that Start/Stop is selected, then set the following parameters:

      • Sweep Type = Linear

      • Start = 800 MHz

      • Stop = 900 MHz

      • Step-size = 1 MHz

  2. To obtain S-parameters, select the Parameters tab and ensure that S-parameters is selected. For a description of the options on the Parameters tab, click Help. To obtain Y- (admittance) and Z- (impedance) parameters, select the corresponding options.

  3. Click OK to accept changes and close the dialog box.

  4. Simulate. When the simulation is finished, plot S(2,1) in the Data Display. The following is a plot of the gain (S21) versus frequency.

Calculating Group Delay

By measuring the transit time, with respect to frequency, of a signal through the device under test, group delay is a useful measure of phase distortion in components such as amplifiers and filters.

To calculate group delay, you enable the Group delay option and, if desired, set the group delay aperture. These options are under the Parameters tab. The results appear in the Data Display variables list under delay.

For more information, refer to Group Delay.

To calculate group delay:

  1. Proceed as in Simulating an Amplifier, setting frequencies and sweep parameters as needed.

  2. Edit the S-Parameters component, select the Parameters tab, and enable Group delay.

  3. Group delay aperture is an option that is found on network analyzers and behaves similarly here. The simulator sets the frequency aperture to 0.01% of the current frequency. To override the default frequency aperture, enable Group delay aperture and edit the value as needed.

  4. Click OK to accept changes and close the dialog box.

  5. Simulate. When the simulation is finished, plot the group delay data items, identified by the prefix delay. This is the absolute group delay, in seconds.


Hint    If the group delay data appears noisy, increase the value in the Group delay aperture field. If the results appear inaccurate, decrease the value. Generally, adjusting this value by a factor of 10 (in the appropriate direction) improves noisy or inaccurate results.

For an example of group delay data, refer to the topic "Obtaining Group Delay Data" in the chapter "Using Circuit Simulators for RF System Analysis" in the Using Circuit Simulators documentation.

Simulating Linear Noise

Options for simulating linear noise are available from the Noise tab of the S-Parameters simulation component. For more information about how noise is calculated, refer to Noise Analysis.

To simulate linear noise:

  1. Proceed as in Simulating an Amplifier, setting frequencies and sweep parameters as needed.

  2. Edit the S-parameter Simulation component and select the Noise tab. Then select the Calculate noise option.

  3. In the Edit field, enter the names of the nodes at which you want noise data to be reported.


Note    It is not necessary to name nodes if only noise figure is desired.

  1. Use the Mode popup menu to sort the noise contributors (nodes) that are reported.

  2. Either accept the default values for Dynamic range to display and Bandwidth, or edit these as required. The defaults are generally sufficient.

  3. Click OK to accept changes and close the dialog box.

  4. Simulate. When the simulation is finished, plot the noise data items. These are noise figure, identified as nf[port_number], and the equivalent input noise temperature, identified as te[port_number].

Adjusting Noise Temperature

The IEEE definition of noise figure states that it should be measured at the standard noise temperature of 290 K (16.85°C). Advanced Design System uses this definition and value of the standard noise temperature in its calculation of noise figure. For a passive circuit, if the simulation temperature is not equal to this value, the noise figure will not be the same as the loss in decibels. The simulation temperature defaults to 25°C. It can be changed by adding an Options item to the design and changing the simulation temperature there to 16.85°C.

Analyzing a Frequency Translating Network

To simulate the effects of frequency translation (also known as frequency conversion) in circuits employing mixers, the S-parameter simulator uses the same algorithm as the AC simulation component. This option causes the simulator to consider the frequency not only of the input fundamental, but also the frequency of the resulting translations. A simple model is used to calculate the reference frequencies at each node.

Selecting the Calculate noise option (under the Noise tab) will result in frequency conversion data for nonlinear noise.

For more conversion information, refer to S-Parameter Frequency Conversion.

To analyze a frequency translating network:

  1. Proceed as in Simulating an Amplifier.

  2. Insert passive ports at locations where you want to obtain S-parameters.

  3. Set frequencies and sweep parameters as needed.

  4. Use a large-signal voltage or current source, such as V_1Tone or I_1Tone as the driving signal that causes the frequency translation (not a large-signal port source, such as a P_1Tone).

  5. Select the Parameters tab, then select Enable AC frequency conversion.

  6. In the field labeled S-parameter freq. conv. port, enter 1.


Note    The frequency conversion port must be the number of the input port.

  1. To calculate frequency conversion data for nonlinear noise, select the Noise tab and enable Calculate noise.

Eliminating Unwanted Effects

It is sometimes helpful to reduce the contribution of other components in an analysis of a circuit involving, for example, amplifiers. The DC_Block component functions as an open during the DC part of the simulation (which is conducted automatically), while the DC_Feed component functions as an open during the S-parameter simulation. This eliminates the loss that would otherwise be experienced with the Term and the bias resistors in the circuit. Figure 1-2 illustrates the use of the DC_Block component in an example circuit.


Note    This design, Amp_wBothMatches.dsn, is in the Examples directory under MW_Ckts/LNA_prj.

Figure 1-2. DC_Block and DC_Feed components in a circuit

To eliminate the effects of port and bias resistances:

  1. From the Lumped Elements palette, select the DC_Block and DC_Feed components (as appropriate) and place them in the circuit as follows:

      • Place the DC_Block component (represented by a capacitor) between the ports and the device under test.

      • Place the DC_Feed components (represented by an inductor, not shown in this design) between the pins of the device under test and any bias resistors.


prevnext