[SOLVED] difference between equivalent input noise and input referred noise

Hai,
Can anybody tell me the difference between total equivalent input noise and total input referred noise? How to calculate these two quantities with cadence tool ? How the tool calculates theses two quantities ? How to calculate these two quantities theoretically? What is the relationship of these quantities with frequency ? (I want to measure these two parameters for a preamplifier with two inputs and two outputs )

Equivalent noise simply represents a noise source (current, voltage, or resistor) at the input, output, or any other terminal of a noiseless circuit, which replaces the existing (real) noise at the respective otherwise open terminal of the real circuit.

Hence the equivalent input noise is identical (or equivalent) to the input noise of the open input circuit (meaning: no other noise sources present than that/those from the circuit itself); accordingly the same is valid for the open (no load) output, or any other open terminal of the circuit.

Sir,
While doing noise analysis of a preamplifier in cadence i came across these two quantities. Initially i thought that that these two are the same. But the cadence tool gives different values for these two(Also with different units). Unit of total equivalent input noise is volts per square root of hertz, Unit of total input referred noise is volts square as per the cadence tool. When i searched in the book i just got confused. Can you tell me how to calculate these two quantities theoretically? Is there any relationship between these two?
Thanks for the reply

I don't use Cadence but it sounds like one of those is really noise "power" and the other is noise "voltage". So they could both be expressing the same thing in different ways. Noise power would need an impedance - probably 50 ohms.

Keith

Use noise analysis in spectre. In the noise analysis setup window, choose your input voltage source as your input noise source. Run the analysis and then go to
Results>direct plot>noise, you will be able to display the input referred noise in v^2/Hz or V/sqrt(Hz)

Under your analysis select noise. Change everything into voltage. If you wan to measure input referred noise voltage. To measure current you would need a port connected to it.
First of under noise analysis. Select the range of frequencies you wan. Select the output node by clicking select go to your schematic and select the node. It would be automatically updated. The second node select it to point to ground which is /gnd! in cadence analog design environment.
For the input source change it to voltage. A warning will be given cos the Noise figure is calculated based on current. Don't worry about that.
Remember the input source is to inform the simulator where is the input so that it can calculate the input referred noise.
Run your simulation. Nothing came out. Hehe go to result direct plot, You can see equivalent input/output voltage or squared input/output voltage.

This is basically not enough. Pin point the noisy components. Go to result print Noise summary. Select the type of output either in terms of V squared or sqrt at the right up upper side of the form. Select integrated noise meaning the noise at certain frequency. Under filter select the devices you wish to see. Under truncate and sort select by number then choose to top 30 to allow you to see the top 30 contributor of noise. Select apply and wait a while. The printout will have all the information, how much each component contributes and the total output / input referred noise is available.

One more thing. If your device model is BSIM3v3 please take note that the gate resistance thermal noise is not modelled. Trust only 50% of the result