NOISE ANALYSIS
Overview
The SPICE simulator engine can model the thermal noise generated in resistors and semiconductor devices. The individual contributions of noise are summed together at a voltage probe in the circuit for a range of frequencies. The noise voltage, normalised with respect to the square root of the noise bandwidth, can then be plotted against frequency. Traces on a noise graph always have units of V/√Hz.
Two types of noise figure are computed, Output Noise and Equivalent Input Noise. The computation of the latter enables comparison of the noise with the input signal, or input noise, since it represents the level of noise at the input that would be required to create the actual noise at the output, taking into account the circuit gain at a particular frequency.
Placing a probe on the left axis displays output noise, whilst equivalent input noise can be displayed by dragging the probe onto the right axis.
Noise analysis tends to produce extremely small values (of the order of nanovolts). For this reason, there is the option to display them in dBs. The 0dB reference is 1V/√Hz.
Correct modelling of noise for circuits involving IC macro models is not guaranteed in any way, because these models may well use linear controlled sources to model basic device behaviour only.
Method of calculation
The operating point of the circuit is computed in the normal way, and then the circuit model is modified to correctly sum the noise contributions. All generators except the input reference are ignored in noise analysis (except during computation of the operating point) and so do not have to be removed before the analysis. The PROSPICE engine will compute the thermal noise for every net carrying a voltage probe, including those associated with generators and tapes, as it has no way of knowing which probes you wish to look at after the analysis. Noise currents are not supported, and the PROSPICE engine will ignore any current probes.
A separate simulation run is performed for each probed net, so the simulation time is roughly proportional to the number of distinct nets you have probed. Several probes on the same net cost nothing extra, because they share a single run.
Using Noise Graphs
When using noise analysis, it is important to remember that the effects of noise pick-up from external electric or magnetic fields are not modelled. In many situations where noise is critical the noise picked up in the input leads will dominate the noise performance of the system.
If you have partitioned the circuit using tapes, you must be aware that only the current partition is considered by the PROSPICE simulator engine. A noise figure taken in isolation is still useful, but the tapes must be removed to see the equivalent noise of the entire circuit. See Tapes and Partitioning.
The frequency range of the analysis is set on the Edit Noise Graph dialogue form by Start frequency and Stop frequency, which default to 10Hz and 1MHz. As with a frequency graph, Interval chooses whether the range is divided into DECADES, OCTAVES or LINEAR steps, and No. Steps/Interval sets how many points are computed within each interval.
Noise Contributions in the Simulation Log
In order to determine the source of noise in the circuit, the individual noise voltages can be entered into the simulation log. Each probed net is considered in turn, and the noise contribution for each component given. The values are square-rooted before they are printed, so they are reported in volts rather than as squared quantities, and they are printed at every frequency step of the analysis. If you have a large number of probes, or a wide frequency range, there may well be a great deal of result data printed.
Two options in the Options group of the dialogue form control this. Log total contributions reports the integrated noise contribution of each component and is enabled by default. Log spectral contributions reports the per-component contribution at each frequency, in V/√Hz, and is disabled by default because of the volume of data it produces.
To analyse the noise in a circuit:
- Place a Noise graph, and edit it to set the frequency range of interest, and the input reference generator.
- Add the voltage probes at the circuit outputs, or other points of interest, to the graph. See Adding Traces To A Graph.
- Press the space bar to invoke the PROSPICE simulator engine.
- If the noise level needs to be reduced, examine the simulation log (CTRL+V) to determine the source of the noise.
See Also: