Hi,

Is there anyway, I can simulate transient noise for the ADI amplifier macro-models? Pspice does not allow transient noise simulation in any easy way, so to estimate p-p noise of the amplifier over certain bandwidth, usually I multiply rms noise 6-9 times, calculated through ac noise simulation. Does all the time domain voltage noise plot in datasheets come from the experiment or is there a way to derive those plots through macro-model based simulation run?

Another related question. I was trying to up-convert flicker noise part of the amplifier. Surprisingly there is no effect on the noise due to chopping. I have no idea why would that be the case since noise in amplifiers are actual modeled by active sources and so would have similar effect as the real signal. I am wondering if this is due to the pspice not being able to simulate switching circuit properly. May be I am missing something here.

Would be really helpful if somebody can answer to these questions.

Thanks

Hi Analog_sup,

Unfortunately there's not an easy answer how to display noise in a Transient Analysis in any SPICE software that I'm aware of. The Noise Analysis in SPICE is a variant of an AC Analysis, the only difference being that resistors, diodes, and transistors are replaced with their noise equivalents. If it is important for you to display the noise in transient analysis, the only way I have seen to do this is to first calculate the noise (or have SPICE do that for you) and then add an equivalent noise source to your circuit. Some simulators have noise sources built-in, but I'm not aware of one in PSpice. The only way I know how to do it in PSpice is explained here: Quick Tutorial: Adding a Random Noise Source in PSpice

For the other half of your question, yes, the time-domain noise plots in our amplifier datasheets come from measurement, not simulation. All of the "Typical Performance Characteristics" are measurement results. For the peak-to-peak noise graph, we generally have a very heavy 0.1Hz to 10Hz filter and we take a lot of gain to ensure that the amplifier noise dominates, and we record the voltage at the output of the filter.

SPICE can give a very accurate value for how much RMS noise is in your circuit, assuming the noise curves in the model match the datasheet. MS-2066 is a very good resource for amplifier noise, in which Reza explains how to use the PSpice integral function S() to calculate the total rms noise in your circuit.

As for the chopping, the problem is for the same reason you don't see noise in the transient analysis. Noise Analysis is a variant of the AC Analysis. AC analysis works by taking a dc operating point first, then it linearizes the entire circuit around that dc operating point, replaces L's and C's with energy storage models, and sweeps the frequency. So your switches will never switch during the ac analysis, chopping won't occur, and the 1/f noise will still be there.

I hope this helps.

Best regards,

Scott