Noise simulation in Cadence

You cannot measure noise with a transistor as the output. You can measure the output noise at a node, or probing a port (in which case it gives the noise voltage across the port, but can then exclude the noise in the load when computing noise figure), or probing a resistor or a voltage source/iprobe, in which case it will measure the output noise current.

So, you can measure the noise voltage at a suitable point, and then look at the noise contributions from the transistor (either with the results->print->noise summary, or with the results browser).

Regards,

Andrew.

 Thank you so much Andrew! It helps a lot! However, I'm still not very sure what to probe if I want to measure the output noise current. You mentioned "a voltage source/iprobe", then what is 'iprobe'?

My test circuit is shown below. I want to test the thermal current noise "ID^2" of the NMOS transistor. Do you mean that I can just set up "probe the \VD" in the noise simulation setup (probe the voltage souece VD)? 

I did probe the "VD" and it gave me a current plot, in the "result browser", there are some parameters which I want to confirm:

fn: flicker current noise?

id: thermal current noise?

igb/igd/igs: current noise from gate to bulk/drain/souece?

Am I right with those? Thank you very much! I'm very appreciate for your correcting.

Best Regards,

Ethan

Hi Ethan,

I deleted your last append (after you figured out how to make an attachment; note that you can attach in any reply, using the Options tab). Pasted images don't work. I probably should add this to the forum guidelines as it comes up so often!

iprobe is a component in analogLib (which corresponds to iprobe in spectre - see "spectre -h iprobe"). In effect this is similar to a zero-volt source, and is an efficient way of measuring currents. You'd place one in your schematic. However, since you already have voltage sources, you can measure it via those.

Unfortunately the noise output parameters are still not documented (there's a request for this - so feel free to contact customer support and add to the list of customers requesting this). fn is indeed flicker noise, the r* parameters are thermal noise for the drain, source etc resistors. The i* are shot noise from the current in the drain, source, etc. There's a bit more information in this solution.

What you are seeing in the results however is the contribution of those noise sources to the output noise (measured as a current, through the VD source). So the noise is output-referred, and is not the magnitude of the noise at the source.

Some explanation of this can be found in another solution (this one written by me).

Kind Regards,

Andrew.

 Thanks a lot Andrew! Now it works, I get all the data I want! BIG THANK YOU for your detailed help and time! Thank you very much!

Andrew,

I was wondering how do you plot flicker and thermal noise envelope during transition in an inverter ? 

It's mentioned on slide 36 of the following designer's community document (http://www.designers-guide.org/Theory/cyclo-preso.pdf)

I tried using noise analyses in ADE-L but  I think I'm going wrong with my intentions to see effect of sweeping input from 0v to 1v of inverter on flicker and thermal noise generated at the output of inverter.