eldo_user

Setting Up An Analysis
Transient Noise Analysis
Transient Noise Analysis
In most analog design applications, knowledge of noise levels generated by the circuit is of
great importance. In all traditional SPICE-like simulators, noise computation is only available
in AC analysis. In this case the circuit is assumed to have a fixed bias (DC operating point), and
noise simulation can only be applied to circuits working under small signal conditions. For this
reason, many applications cannot be simulated and their noise performance is unknown until
physical measurement is possible on the manufactured design. The only other method available
to obtain this important information is to perform tedious hand calculations (when possible).
The objective of a noise simulation is to see the effect of the physical noise generated by the
different devices on the characteristics of an electrical circuit. Three different noise analyses are
available inside Eldo: .NOISE, .SSTNOISE, and .NOISETRAN.
.NOISE and .SSTNOISE are similar in the sense that the effect of the noise sources is treated as
linear (meaning that doubling the noise amplitude will double the effect). To compute the
contribution from the different noise sources the circuit is linearized around its operation point
(can be DC OP for .NOISE analysis or large signal Steady-State OP for .SSTNOISE analysis).
The contributions from the individual noise sources are computed by multiplying the noise
Power Spectral Density (PSD) by the corresponding transfer functions (or harmonic transfer
functions) between the noise source and the specified circuit output.
• Noise and signal are handled separately.
• Noise is considered as small and noise effects are considered as linear.
• It is possible to see the individual contributions from all the different noise sources.
.NOISETRAN analysis is very different from .NOISE or .SSTNOISE analyses. It is a true noise
simulation, similar to what actually happens in reality when an electrical circuit is running.
There is no simplification, no linearization, and no assumption. Noise is handled as any other
electrical signal during a transient simulation. There is no separation between noise and other
signals, and no separation between the noise sources.
Transient noise simulation can be applied to all types of circuit without restriction. To perform
transient noise analysis, physical noise of electrical devices is emulated by time-dependent
current sources. The frequency characteristics of these sources are referred to the noise models
of the noisy components. The method used is simple, fast and does not disturb the simulated
behavior of the circuit because the noise signals introduced are continuous and fully
deterministic.
Tip
See “.NOISETRAN” in the Eldo Reference Manual.
Simulation results from transient noise analysis include:
Eldo® User's Manual, 15.3 241