how to calculate noise figure

Hi Guys
I have designed a differential LNA. I get a good voltage gain of 27dB.

The Problem is that i donot know how to calculate the Noise Figure of the design using SPECRE RF!

I know how to do S-paramter simulation in SPECTRE RF but i donot know how to find Noise Figue from that.

What else does SP analysis in SPECTRE RF tell me and how?

Can anyone help me with this.?
Thanks

In the S parameter form switch on the "DO NOISE" button and you'll get the NF. Simple.
Mazz

Hi
while doing sp analysis, In the coosing analysis form for "sp" analysis

I select start-stop for Sweep Range and the range i enter is :
Start : 800 M
Stop: 5 G

But when i simulate i get the following error:

Error found by spectre at freq = 800 MHz during SP analysis `sp'.
'iprobe' or 'oprobe' did not appear in the first or the second entry in
'ports' parameter. Respecify 'ports' parameter and start again.

any idea how to solve the problem ?

NF is a ratio of input ( C/N) and output (C/N).
When you design a LNA . it is better use noise signal source.Combine it with carrier signal , and see output power.
Take noise signal as idea .So the
NF(dB)=(Pin+174dBm-10logBW)-(P1-P2)
P1 is with carrier signal,P2 is only noise signal. see at output port.

In the Analog Design Environment do the following:

1.In the Simulation window, choose Analyses - Choose.
2.In the Choosing Analyses form, click on sp for the Analysis choice.
3.Highlight Frequency for the Sweep Variable.
4.Highlight Start-Stop for the Sweep Range. Type 800M in the Start field and 5G in the Stop field.
5.In the Sweep Type cyclic field, choose Linear for the sweep type and highlight Number of Steps. Type
"whatever" in the Number of Steps field.
6.Highlight yes for Do Noise.
The form changes to let you specify values for the Output port and Input port fields.
7.To select the Output port
a.Click the Select button next to the Output port field.
b.In the Schematic window, select the output port. /PORT0 displays in the Output port field.
8.To select the Input port
a.Click the Select button next to the Input port field.
b.In the Schematic window, select the RF port.
/RF displays in the Input port field. 9.Make sure that Enabled is highlighted.
10.In the Choosing Analyses form, click OK.

Then choose Simulation - Netlist and Run

Good luck

T Zul

Hi
thanks for the reply, I seek help but for that i need to specify the problem in detail. Here is the detail ..

I have a differential LNA with output pins as out+ and out-. At the outputs I have stuck in two "psin" ports, one at each differential output.

At the input side, again i have two "psin" ports , one at each differential input.

Now I do "sp" analysis.
If I highlight "NO" in the "Do Noise" field, the sp analysis works and i am able to plot S11, S22 etc.

But the problem starts when i highlight "YES" in the "Do Noise". When i do that, It prompts me to specify the "output Port" and "input Port". Now I amstuck, since I have two output ports and two input ports. Therefore, without much knowing, I click on the "psin" port corresponding to "out+" and specify it as output port in do-noise. Similarly, I click on "psin" port corresponding to "In+" and specify it as "input port" in do-noise.

this is how the completed form looks like :
***********************************
Sweep Variable
(frequency highlighted)

Sweep range
(Start-Stop highlighted)
Start : 800M
Stop: 5G

Sweep Type
(linear selected)
Number of steps : 40

Do Noise
("yes" highlighted") and output and input ports specifiedas explained above.
*******************************************

Now when the simulation is run, I get this error :
"Error found by spectre at freq = 800 MHz during SP analysis `sp'. 'iprobe' or 'oprobe' did not appear in the first or the second entry in 'ports' parameter. Respecify 'ports' parameter and start again.

This is the problem and Any help is highly appreciated
Thankyou very much

Hi all,
While finding the noise figure of a differential LNA using SPECTRE RF, should i use "sp" analysis or "pnoise" analysis ? whats the difference?
Thanks

HI all,
I have also this problem. However, if you use pss pnoise options together you may get around this problem but I am not completly sure how?

Now I've understood better your problem.
The question is not on the simulator, but on what you're looking for.
Usually in differential amplifiers, if you're interested in differential signal only, you must use input/output baluns with proper impedance ratio.
In this way you'll have only one input port (you can set dc port instead of sine in linear analysis such as sp, ac, noise) and only one output port that you should put properly in the noise form (as T ZUL said).
Regarding pnoise (that can be used only after a pss) analysis it is for time varying steady state solutions: it is useful for example for mixers or for amplifiers to see the degradation of NF when al large (blocking) signal is applied. The simulator computes a large signal steady state solution with pss analysis and around this solution computes a small signal noise analysis (or small signal ac with pac).
If your amplifier should be in/out power matched you'd better use sp with noise enabled.
Mazz

I have a collegue of mine simulating the differential LNA and obtain -ve NF. I told him that let us file for patent for Nobel Laurette ... Balun implementation as suggested by Mazz is the solution to your problem.

T Zul