Mixer Performance Simulations

Conversion Gain

• You must first instance ports for the RF, LO, and IF ports of the mixer (analogLib -> Sources -> Independent -> port). If your mixer requires differential inputs/outputs then refer to the separate tutorial on how to drive differential signals.
• Edit the properties of the RF port
  • Set the Resistance to 50 Ω and the Port number to 1
  • Set the Source type to dc
  • Click OK
• Edit the properties of the LO port
  • Set the Resistance to 50 Ω
  • Set the Port number to 2
  • Set the Source type to sine
  • Fill in the flo for the Frequency name 1
  • Frequency 1 should be either 2.2 GHz (for low-side injection) or 2.6 GHz (for high-side injection)
    • This is the frequency of the local oscillator signal
  • Fill in Amplitude 1 (Vpk) with the amplitude of your LO signal
  • Click OK
• Edit the IF port
  • Set the Resistance to 50 Ω and the Port number to 3
  • Set the Source type to dc
  • Click OK
• In the Analog Design Environment, enable the pss analysis
  • Verify that only flo is displated in the Fundamental tones section
  • Select Beat Frequency and click Auto Calculated
  • Select Number of harmonics under Output harmonics and fill in the value of 0
    • This number of ourput harmonics is required by the pxf analysis that we will use to perform the conversion gain simulation
  • Set the Accuracy Defaults (errpreset) to conservative
  • Set the Additional Time for Stabalizatoin (tstab) to a time larger that the settling time of your system
    • Run a short tran simulation to find the time when all of the voltages in your mixer have settled and there is no "ringing"
  • Click OK
• In the Analog Design Environment, select pxf analysis (pxf stands for periodic transfer function)
  • Set Sweep type to default
  • Under Output Frequency Sweep Range (Hz) select Start-Stop
  • Set Start to 1 MHz and Stop to 400 MHz
• Set the Sweep Type to Linear
  • Select Number of Steps and set the value to 1000
  • Set Sidebands to Maximum Sideband and enter the value 3
  • Under Output select probe and then selct the IF port
  • Click OK
• Run the simulation
• To view the results for the conversion gain simulatoin click Results -> Direct Plot -> Main Form ...
  • Set the Analysis to pxf
  • Set the Function to Voltage Gain
  • Set Sweep to sideband
  • Select sidebands -1 and 1 (hold down the ctrl key to select multiple sidebands)
    • This is the sideband that provides us the conversion gain of our RF frequency of interest
  • Set Modifier to dB20
  • Click on the RF port in the schematic