# Why do people waste time using a SPICE .NOISE analysis for circuits with resistances with significant excess noise?

Excess noise in a resistor is the electrical noise which is in excess of the value predicted by the well-known Johnsson-Nyquist-Thermal noise formula. Excess noise is created as a voltage impressed across a resistor causes electrons to flow through the resistive material.

In some types of resistors, the increase in noise is so significant that the circuit is useless.

Even in "very good" resistors the voltage noise density can increase by 50% over the Johnson-Nyquist-Thermal formula when 1V is impressed across the resistor. More over, the voltage noise density spectrum takes on flicker (1/f) shape as the DC voltage across the resistor is increased.

To the best of my knowledge, there is no SPICE variant with a .NOISE analysis which accounts for excess noise. Is this true?

• does excess-noise exhibit a 1/F behavior? Oct 11, 2019 at 3:05
• The cited report shows that excess noise exhibits 1/f behavior when current flows the the resistor
– BHS
Oct 11, 2019 at 7:35
• I understand that spice is designed for IC circuitry, which may not have resistors with excess noise. But if you inspect any Tina Or Ltspice page hosted by a major manufacturer, you will see abundant training on using .noise for a variety of op amp circuitry.
– BHS
Oct 12, 2019 at 19:48
• Yes but excess noise is not intrinsically modeled.
– BHS
Oct 29, 2020 at 16:10

To first of all answer the title of this question, modeling noise is not a waste of time as long as the device models are reasonably good and include the dominant noise sources. 1/f noise, in particular, becomes insignificant above a certain frequency, and in many applications is not detectable beyond other noise sources (never mind not being a significant noise source).

1/f noise is not (inherently) modeled in LTSpice (or SPICE in general), and depends on the particular resistor.

To model excess noise, you could try the technique illustrated below. In this file, you can see the 1/f noise at node "noise". To use it in a circuit, place E1 in series with the resistor you want to add 1/f noise to.

In doing this, you will need to know the resistor's noise index in uV/V. Since excess noise is proportional to the resistor's DC bias, you will also need to know the DC bias of the resistor. This technique will work if the resistor's DC bias is fairly constant. Edit the VALUE2 field of E1 (laplace=1*659/sqrt(s/6.2832)), and change the 1 to the product of the DC bias and the noise index.

• Thank you for taking the time to answer the question.
– BHS
Oct 29, 2020 at 16:13
• See Motchenbacher and Connelly, Low Noise System Design, 1993, p 89 suggests a spice model which also adds excess noise
– BHS
Oct 29, 2020 at 16:14