Example of Large-Signal S-Parameter Simulation

The following figure illustrates the setup for a large-signal S-parameter (LSSP) simulation of a BJT. Power sources drive all ports in this example.

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

Large-signal S-parameter simulation example in ADS

1. From the Simulation-LSSP palette, select a P_1Tone component and place it at the input of the circuit. Edit the component and set the following values:
   • Num = 1
   • P = dbmtow((10),0)
   • Freq = LSSP_freq
2. Select another P_1Tone power source and place it at the output of the circuit. The values are the same as for the input source, except here Num = 2.

   Note The values in the Num parameter on the sources and terminations should reflect the placement of the ports in the circuit, so that the S-parameter data is meaningful. The number of the input (source) should be set to Num=1, and that of the output (load) to Num=2.

3. Select and place an LSSP simulation component on the schematic, edit it, and select the Freq tab to set the following parameters:
   • Frequency = LSSP_freq
   • Order[1] = 3
     Click Add. Make sure that 1 LSSP_freq 3 is the only line that appears in the list of fundamental frequencies. (If LSSP_freq appears as the second fundamental in the frequency list, select the line above it and click Cut.)
4. Select the Sweep tab. Ensure that Start/Stop is selected and Sweep Type is Linear, then set the following values:
   • Start = 0
   • Stop = 100
   • Step = 1
5. Select the Ports tab. In the Frequency field, at the right of the dialog box, enter LSSP_freq and click Add. This establishes the frequency at port 1, where the large-signal S-parameter will be measured. It does not have to be the same value as the fundamental frequency, it can be a harmonic.
   For example, a port may have harmonics present at 0 Hz, 1 MHz, 99 MHz, 100 MHz, and 101 MHz. You can then specify your interest in the 99 MHz component by entering 99 MHz here. On the schematic, this appears as LSSP_FreqAtPort[n]. In this example, it would appear as LSSP_FreqAtPort[2]=99 MHz.
6. To set the frequency for port 2, click Add again. You should see two entries in the Port Frequency list box, each set to LSSP_freq.
7. Click OK to accept changes and close the dialog box.
8. From the Data Items palette, select VarEqn. Place and edit the component to define the variable LSSP_freq and set its value. Select the default equation (X=1.0). In the Variable Value field at the right, enter 1.0 GHz.
9. Click OK to accept changes and close the dialog box.
10. Since the fundamental is set to a single frequency, you can use a ParamSweep component to sweep a frequency range. Return to Simulation-LSSP, select and place a ParamSweep component, and edit it. Select the Sweep tab and set the following values:
    • Parameter to sweep = LSSP_freq
    • Sweep Type = Linear
    • Enable Start/Stop
    • Start = 1 GHz
    • Stop = 10 GHz
    • Step-size = 0.1 GHz
11. Click Simulations and set Simulation 1 to HB1. Click OK.
12. Launch the simulation, and when it is finished, display the results. LSSP data items may identified with an HB prefix. The following plot displays S(1,2).