VCO Performance Simulations: Difference between revisions

From VLSI
Jump to navigation Jump to search
← Older edit
No edit summary
 
(17 intermediate revisions by the same user not shown)
Line 1: Line 1:
The following tutorial assumes that you have a voltage controlled oscillator (VCO) already designed and you now wish to find various performance criteria such as phase noise, tuning range, etc.
The following tutorial assumes that you have a voltage controlled oscillator (VCO) with differential outputs already designed and you now wish to find various performance criteria such as phase noise, tuning range, etc.


==Phase Noise==
=Phase Noise=
* Make sure that your tuning voltage is set such that your VCO oscillates at the desired frequency.
* Make sure that your tuning voltage is set such that your VCO oscillates at the desired frequency.
* From the Analog Design Environment click "Choose Analysis ..." and choose "pss"
* From the Analog Design Environment (ADE) click '''Choose Analysis ...''' and choose '''pss'''
**In the "Fundamental Tones" section make sure "Beat Frequency" is selected and enter your best guess as to what the frequency of oscillation should be (i.e., enter your desired operating frequency). Make sure that "Auto Calculate" is NOT selected.
**In the '''Fundamental Tones''' section make sure '''Beat Frequency''' is selected and enter your best guess as to what the frequency of oscillation should be (i.e., enter your desired operating frequency). Make sure that '''Auto Calculate''' is NOT selected.
**In "Output harmonics" select "Number of harmonics" and enter 10.
**In '''Output harmonics''' select '''Number of harmonics''' and enter 10.
**Under "Accuracy Defaults (errpreset)" select "conservative" and enter the required stabilization time under "Additional Time for Stabilization (tstab)" that you obtained from a transient simulation.
**Under '''Accuracy Defaults (errpreset)''' select '''conservative''' and enter the required stabilization time under '''Additional Time for Stabilization (tstab)'''.
***tstab is obtained from a transient simulation. It is the time that it takes for the output of your oscillator to settle to a steady state (in terms of amplitude and frequency).
***''tstab'' is obtained from a transient simulation. It is the time that it takes for the output of your oscillator to settle to a steady state (in terms of amplitude and frequency).
**Select '''Oscillator''' and then select one of the differential outputs for '''Oscillator node''' and the other differential output for the '''Reference node'''.
**Click '''Apply'''
 
*Nose select '''pnoise''' analysis in the '''Choosing Analysis''' window
**Set the '''Sweeptype''' to '''relative'''
**Enter 1 for the '''Relative Harmonic'''
**Select '''Start-Stop''' and enter 1 kHz and 100 MHz for the '''Start''' and '''Stop''' frequencies, respectively
**Set the '''Sweep Type''' to '''Logarithmic''' and set the '''Points Per Decade''' to 201
**Under '''Sidebands''' select '''Maximum sideband''' and enter 30
**Set the '''Output''' to '''voltage''' and select one of the differential outputs for the '''Positive Output Node''' and the other differential output for the '''Negative Output Node'''
**Set the '''Input Source''' to none
**Leave the '''Noise Type''' to sources
**Click '''OK'''
 
*To plot the output, in the ADE Window click '''Results -> Direct Plot -> Main Form ...'''
**Under '''Analysis''' select '''pnoise'''
**Under '''Function''' select '''Phase Noise'''
**Click Plot
 
=Tuning Range=
*Set your tuning voltage sources to be controlled by a variable (e.g., vtune)
*In the ADE window click on '''Choose Analysis ...'''
**Select '''tran'''
**Set the '''Stop Time''' to an appropriate value that ensures that the output of your VCO has settled and that at least 3/4 of the ''total'' simulation time consists of oscillation with a stable output.
** Set the '''Accuracy Defaults (errpreste)''' to '''conservative'''
**Click '''OK'''
 
*In the ADE window click '''Tools -> Parametric Analysis'''
**Enter the variable name for the control voltage under '''Variable Name'''
**Set the '''From''' and '''To''' values so that the control voltage is swept from o to Vdd
**Set the '''Total Steps''' to 10
**Click '''Analysis -> Start'''
 
*To plot the results open up the calculator
**In the calculator (under the ''tran'' tab) click '''vt''' and then select one of the differential outputs of the VCO on the schematic
**In the special functions of the calculator click '''frequency'''
**Click the plot button in the calculator
 
=Phase Noise vs. Tuning Voltage=
*Set your tuning voltage source to be controlled by a variable (e.g., vtune)
*Use the setup for '''pss''' analysis from the ''Phase Noise'' simulation above
*Configure the '''pnoise''' the same as above too, except select '''Single-Point''' under '''Output Frequency Sweep Range (Hz)''' and enter the offset frequency that you are interested in (e.g., 100 kHz or 1 MHz)
**Everything else should be the same as in the ''Phase Noise'' simulation above
*In the ADE window click '''Tools -> Parametric Analysis'''
**Enter the variable name for the control voltage under '''Variable Name'''
**Set the '''From''' and '''To''' values so that the control voltage is swept from o to Vdd
**Set the '''Total Steps''' to 10
**Click '''Analysis -> Start'''
*To plot the results, in the ADE click '''Results -> Direct Plot -> Main Form ...'''
**Under '''Analysis''' select '''pnoise'''
**Under '''Function''' select '''Phase Noise'''
**Click '''Plot'''
 
=Amplitude vs. Tuning Voltage=
*Set your tuning voltage source to be controlled by a variable (e.g., vtune)
*In the '''Analog Design Environment''' click on '''Choose Analysis ...'''
**Select '''tran'''
**Set the '''Stop Time''' to a time such that the output of the VCO has settled and steady-state oscillation makes up for at least 1/2 of the ''total'' simulation time
**Set the '''Accuracy Defaults (errpreset)''' to '''conservative'''
**Click '''OK'''
*In the ADE window click '''Tools -> Parametric Analysis'''
**Enter the variable name for the control voltage under '''Variable Name'''
**Set the '''From''' and '''To''' values so that the control voltage is swept from o to Vdd
**Set the '''Total Steps''' to 10
**Click '''Analysis -> Start'''
*To plot the results, open up the calculator
**In the calculator, under the ''tran'' tab, click '''vt''' and select one of the VCO's differential outputs on the schematic
**In the calculator click on the special function '''ymax'''
**Click '''vt''' again and now select the other differential output on the schematic
**In the calculator click on the special function '''ymin'''
**Now click the subtract button ('-')
**Click the plot button in the calculator

Latest revision as of 16:53, 17 March 2010

The following tutorial assumes that you have a voltage controlled oscillator (VCO) with differential outputs already designed and you now wish to find various performance criteria such as phase noise, tuning range, etc.

Phase Noise

  • Make sure that your tuning voltage is set such that your VCO oscillates at the desired frequency.
  • From the Analog Design Environment (ADE) click Choose Analysis ... and choose pss
    • In the Fundamental Tones section make sure Beat Frequency is selected and enter your best guess as to what the frequency of oscillation should be (i.e., enter your desired operating frequency). Make sure that Auto Calculate is NOT selected.
    • In Output harmonics select Number of harmonics and enter 10.
    • Under Accuracy Defaults (errpreset) select conservative and enter the required stabilization time under Additional Time for Stabilization (tstab).
      • tstab is obtained from a transient simulation. It is the time that it takes for the output of your oscillator to settle to a steady state (in terms of amplitude and frequency).
    • Select Oscillator and then select one of the differential outputs for Oscillator node and the other differential output for the Reference node.
    • Click Apply
  • Nose select pnoise analysis in the Choosing Analysis window
    • Set the Sweeptype to relative
    • Enter 1 for the Relative Harmonic
    • Select Start-Stop and enter 1 kHz and 100 MHz for the Start and Stop frequencies, respectively
    • Set the Sweep Type to Logarithmic and set the Points Per Decade to 201
    • Under Sidebands select Maximum sideband and enter 30
    • Set the Output to voltage and select one of the differential outputs for the Positive Output Node and the other differential output for the Negative Output Node
    • Set the Input Source to none
    • Leave the Noise Type to sources
    • Click OK
  • To plot the output, in the ADE Window click Results -> Direct Plot -> Main Form ...
    • Under Analysis select pnoise
    • Under Function select Phase Noise
    • Click Plot

Tuning Range

  • Set your tuning voltage sources to be controlled by a variable (e.g., vtune)
  • In the ADE window click on Choose Analysis ...
    • Select tran
    • Set the Stop Time to an appropriate value that ensures that the output of your VCO has settled and that at least 3/4 of the total simulation time consists of oscillation with a stable output.
    • Set the Accuracy Defaults (errpreste) to conservative
    • Click OK
  • In the ADE window click Tools -> Parametric Analysis
    • Enter the variable name for the control voltage under Variable Name
    • Set the From and To values so that the control voltage is swept from o to Vdd
    • Set the Total Steps to 10
    • Click Analysis -> Start
  • To plot the results open up the calculator
    • In the calculator (under the tran tab) click vt and then select one of the differential outputs of the VCO on the schematic
    • In the special functions of the calculator click frequency
    • Click the plot button in the calculator

Phase Noise vs. Tuning Voltage

  • Set your tuning voltage source to be controlled by a variable (e.g., vtune)
  • Use the setup for pss analysis from the Phase Noise simulation above
  • Configure the pnoise the same as above too, except select Single-Point under Output Frequency Sweep Range (Hz) and enter the offset frequency that you are interested in (e.g., 100 kHz or 1 MHz)
    • Everything else should be the same as in the Phase Noise simulation above
  • In the ADE window click Tools -> Parametric Analysis
    • Enter the variable name for the control voltage under Variable Name
    • Set the From and To values so that the control voltage is swept from o to Vdd
    • Set the Total Steps to 10
    • Click Analysis -> Start
  • To plot the results, in the ADE click Results -> Direct Plot -> Main Form ...
    • Under Analysis select pnoise
    • Under Function select Phase Noise
    • Click Plot

Amplitude vs. Tuning Voltage

  • Set your tuning voltage source to be controlled by a variable (e.g., vtune)
  • In the Analog Design Environment click on Choose Analysis ...
    • Select tran
    • Set the Stop Time to a time such that the output of the VCO has settled and steady-state oscillation makes up for at least 1/2 of the total simulation time
    • Set the Accuracy Defaults (errpreset) to conservative
    • Click OK
  • In the ADE window click Tools -> Parametric Analysis
    • Enter the variable name for the control voltage under Variable Name
    • Set the From and To values so that the control voltage is swept from o to Vdd
    • Set the Total Steps to 10
    • Click Analysis -> Start
  • To plot the results, open up the calculator
    • In the calculator, under the tran tab, click vt and select one of the VCO's differential outputs on the schematic
    • In the calculator click on the special function ymax
    • Click vt again and now select the other differential output on the schematic
    • In the calculator click on the special function ymin
    • Now click the subtract button ('-')
    • Click the plot button in the calculator
Retrieved from "https://wikis.ece.iastate.edu/vlsi/index.php?title=VCO_Performance_Simulations&oldid=112"