How to get the Noise figure (NF) in Hspice?

noise figure spice

I have hspice post-simulation netlist for LNA from cadence, but donot know how to get noise figure? Seems that hspice donot support the Nf ananlysis.
Another question, the S-parameters S21 and S12 are the same, why??

thank you all.

nf noise figure

Hi
Actually to get the NF in the Hspice is not a direct way, for example if you want to know the noise figure of LNA at frequency = 2.4GHz you have to do the following steps

1) Check the input resistance ex Rs vin g 50 , because the NF is the total output noise with respect to the input noise which is generated by Source resistance (usually 50 ohm )
2) In your simulation file *.sp write

.AC DEC 10 400MEG 4G
.NOISE v(out) Vin 1

3) After the simulation finish, check the results in *.lis file , and search for the value of “resistor squared noise voltage (sq v/hz )” for element Rs at the frequency 2.4GHz, and divide this value over the total output noise voltage (sq v/hz ) where u can find under the frequency 2.4GHz for example if
Resistor squared noise voltage = 8.778e-18(sq v/hz )
The total output noise voltage=6.069e-18(sq v/hz )
The NF = 8.778e-18(sq v/hz )/ 6.069e-18(sq v/hz )=1.446=1.6dB

Added after 8 minutes:

Hi
Usually S12=S21 when the circuit is passive element like spiral inductor , and if your circuit is an active circuit that mean there is short connection between your input and output or your circuit not work

spice noise figure

Hi shahroury, could I ask about your Hspice snytax
Rs vin g 50
what's the g point? is it the ground? or connect to the LNA?
You method seems double caculate the souce noise.

figure noise en hspice

Rs is the source resistance connecte between Vin and gate(g) of the first transistor , I just wrote it to emphasis that when you want to calculate NF you have not to forget the source resistance , if it is still not cleared , feel free to tell me ,I can sent an example file to you

noise figure in spice

shahroury, thank you for your kindness.

But I get a new question,
If you get NF by this way, how do you get the S11 when what you are simulating is an LNA?
I try your method today, but the result is quite different from using the
.net command of Hspice. And there seems to be many noise results for noise of rs, headed by different nummbers, such as
0:rs, 3:rs, 13:rs.
From the value it seems I should choose the first one. But why are there others?