View source for Mixer Performance Simulations

==Conversion Gain==
*You must first instance ports for the RF, LO, and IF ports of the mixer (<code>analogLib -> Sources -> Independent -> port</code>). 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 <code>Results -> Direct Plot -> Main Form ...</code>
**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

==LO Feed Through==
*You must first instance ports for the RF, LO, and IF ports of the mixer (<code>analogLib -> Sources -> Independent -> port</code>). 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 '''sine'''
**Enter '''frf''' for the '''Frequency name 1'''
**Enter 2.4 GHz for '''Frequency 1'''
**Enter '''prf''' for Amplitude 1 (dBm)'''
**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 both '''frf''' and '''flo''' are displated in the '''Fundamental tones''' section
**Select '''Beat Frequency''' and click '''Auto Calculated'''
***The beat frequency should be 200 MHz (your IF frequency)
**Select '''Number of harmonics''' under '''Output harmonics''' and fill in the value of 15
**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
*Run the simulatoin
*To view the results for the conversion gain simulatoin click <code>Results -> Direct Plot -> Main Form ...</code>
**Set the '''Analysis''' to '''pss'''
**Set the '''Function''' to '''Voltage'''
**Choose '''Differential Nets''' under the '''Select''' optoin if you have a differential output
**Set '''Sweep''' to '''spectrum'''
**Set '''Signal Level''' to '''Peak'''
**Choose '''dB20''' for the '''Modifier'''
**Select the IF output nets on the schematic to plot the result
**Place a marker on the harmonic that appears at you LO frequency (2.2 GHz for low-side injection or 2.6 GHz for high-side injection)and read the value

==Noise Figure==
*You must first instance ports for the RF, LO, and IF ports of the mixer (<code>analogLib -> Sources -> Independent -> port</code>). If your mixer requires differential inputs/outputs then refer to the separate tutorial on how to drive differential signals.
*This simulation does not require an IF port so remove the IF port (and accompanying balun circuitry if you have a differential IF signal)
*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
*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
**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 the pnoise analysis
**The '''PSS Beat Frequency (Hz)''' should read 2.2G (2.6G if you are using high-side injection)
**Set '''Output Frequency Sweep Range (Hz)''' to '''Start-Stop'''
**Set '''Start''' to '''1 MHz''' and '''Stop''' to '''1 GHz'''
**Set '''Sweep Type''' to '''Logarithmic'''
**Use 100 points per decade
**Under '''sidebands''' select '''Maximum sideband''' and set it to 30
**Under '''Output''', select '''voltage''' and select the appropriate node for the IF on your schematic
**For the '''Input Source''' select '''port''' and select the RF port
**For '''Reference side-band''' select '''Enter in field''' and enter -1
**Click OK
*Run the Simulation
*To view the results for the conversion gain simulatoin click <code>Results -> Direct Plot -> Main Form ...</code>
**Set the '''Analysis''' to '''pnoise'''
**Set the '''Function''' to '''Noise Figure'''
**Click '''Plot'''

==Linearity using IIP3==
*You must first instance ports for the RF, LO, and IF ports of the mixer (<code>analogLib -> Sources -> Independent -> port</code>). 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 '''sine'''
**Enter '''frf''' for the '''Frequency name 1'''
**Enter 2.4 GHz for '''Frequency 1'''
**Enter '''prf''' for Amplitude 1 (dBm)'''
**Click on '''Display small signal params''' and enter '''prf''' in the '''PAC magnitude (dBm)''' field
**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 both '''frf''' and '''flo''' are 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 2
**Set the '''Accuracy Defaults (errpreset)''' to '''conservative'''
**Select '''Sweep''' and make sure that '''Variable''' is selected and enter '''prf''' for '''Variable Name'''
**Under '''Sweep Range''' select '''Start-Stop'''
**Set '''Start''' to -25 and '''Stop''' to +5
**Set '''Sweep Type''' to '''Linear'''
**Set '''Step Size''' to 5
**Click OK
*In the Analog Design Environment enable the '''pac''' analysis
**Under '''Input Frequency Sweep Range (Hz)''' chosse '''Single-Point'''
**Set '''Freq''' to 2.402 GHz
**Under '''Sidebands''' select '''Array of indicies'''
**Enter -11 -13 (with a space between) in the '''Additional indicies''' field
***These numbers correspond to the harmonic of the beat frequency that corresponds to the fundamental and IM3 components
**Clic OK
*Run the Simulation
*To view the simulation results
**Click <code>Results -> Direct Plot -> Main Form ...</code>
**Under '''Analysis''' select '''pac'''
**Under '''Function''' select '''IPN Curves'''
**For '''Circuit Input Power''' select '''Variable Sweep ("prf")'''
**Enter -20 for '''Input Power Extrapolation Point (dBm)'''
**Under '''1st Order Harmonic''' select '''-11 202M'''
***This is our downconverted fundamental component assuming low-side injection (2.402 GHz - 2.2 GHz = 202 MHz)
**Under '''3rd Order Harmonic''' select -13 198M
***This is our downconverted IM3 component assuming low-side injection ([2*2.4 GHz - 2.402 GHz] - 2.2 GHz = 198 MHz)
**Select the IF port on your schematic