EDN Access -- 06.09.94 Spice plots noise figure

Design Ideas: June 9, 1994

Spice plots noise figure

Michael A Wyatt ,
SSAVD Honeywell Inc, Clearwater, FL

The waveform-manipulation capabilities of modern Spice-based simulators, such as MicroSim Corp's PSpice, make it easy to plot complex functions, such as noise figure. The traditional definition of "noise figure" is "the amount of signal-to-noise degradation a circuit causes." Another definition is "the total-output-noise power divided by the output-noise power due to the source impedance, expressed in decibels." Spice computes the total-output-noise voltage, e_onoise, as the root-sum-square voltage of all network noise sources referenced to the output, which corresponds to the equation

where e_nk is the kth noise contributor and G_k is the associated kth gain. Spice also computes the equivalent input noise e_inoise, which would produce the same output noise voltage with a noise-free amplifier as

where G_amp is the amplifier gain. Because noise power is proportional to noise voltage squared, you can replace eonoise with e_inoisex G_amp to compute noise figure for equal input and output impedances as

where k is Boltzmann's constant (1.38x10^-23 J/K) and T is temperature in Kelvin (298K at room temperature).

Consider the RF amplifier in Fig 1a. Spice computes the total root-sum-square output noise voltage and references it to the input source V_in. Spice can then use this noise voltage V_inoise with Eq 3 to display noise figure. For example, entering the equation into PSpice's Probe feature produces Fig 1b, a graph of the RF amplifier's noise figure vs frequency. This convenient display is typical of RF semiconductor manufacturers' data sheets, and you can use it to investigate circuit, bias point, and component influences on noise figure. (DI #1440)