Description

Noise analysis lets you measure the noise contributions of resistors and semiconductor devices by plotting the Noise Spectral Density, which is the noise measured in Volts squared per Hertz (V²/Hz). Capacitors, inductors and controlled sources are treated as noise free.

The following noise measurements can be made:

Setup

Noise analysis is set up on the Noise Analysis Setup page of the Analyses Setup dialog (after the dialog appears, click the Noise Analysis entry in the Analyses/Options list). An example setup for this analysis type is shown in the image below:

Parameters

• Noise Source - an independent voltage source in the circuit which is to be used as an input reference for the noise calculations.
• Start Frequency - the initial frequency for the range over which to perform the noise calculations (in Hz).
• Stop Frequency - the final frequency for the range over which to perform the noise calculations (in Hz).
• Sweep Type - defines how the test points are distributed over the defined frequency range. The following three types are available:
  Linear - evenly spaced test points on a linear scale.
  Decade - evenly spaced test points per decade of a log₁₀ scale.
  Octave - evenly spaced test points per octave of a log₂ scale.
• Test Points - defines the number of points over the defined frequency range at which noise calculations will be performed.
• Points Per Summary - allows you to control which noise measurement is performed. Setting this parameter to 0 will cause input and output noise to be measured only. Setting to a 1 will measure the noise contribution of each component in the circuit.
• Output Node - the node in the circuit at which the total output noise is to be measured.
• Reference Node - the node in the circuit used as a reference for calculating the total output noise at the desired Output Node. By default, this parameter is set to 0 (GND). If set to any other node, the total output noise is calculated as:

V(Output Node) -V(Reference Node)

• Total Test Points (non-editable) - shows the total number of test points in the frequency sweep range, calculated from the initial value for Test Points and the chosen Sweep Type.

Notes

The Start Frequency must be greater than zero.

The independent voltage source specified in the Noise Source parameter must be an ac source in order for the simulation to proceed.

Data is saved for all signals in the Available Signals list, on the General Setup page of the Analyses Setup dialog.

The simulation results are displayed on the Noise Spectral Density tab of the Waveform Analysis window.

Examples

Consider the circuit in the image above, where a Noise analysis is defined with the following parameter values:

• Noise Source = Vin
• Start Frequency = 1.000k
• Stop Frequency = 1.000meg
• Sweep Type = Linear
• Test Points = 1000
• Points Per Summary = 0
• Output Node = Output
• Reference Node = 0 (GND)
• Total Test Points = 1000

The entry in the SPICE netlist will be:

*Selected Circuit Analyses:
.NOISE V(OUTPUT) Vin LIN 1000 1000 1E6 

Running the simulation will yield the output waveforms shown in the following image:

The top waveform shows the total output noise (NO) measured at the specified output node, in this case Output. The bottom waveform shows the amount of noise that would have to be injected at the input (NI) to obtain the measured output noise at this node.

If the Points Per Summary parameter had been set to 1 instead of 0, the output noise contribution of each applicable component in the circuit would have been measured and the corresponding waveforms for each made available in the Sim Data panel, ready for use in the Waveform Analysis window.