The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Design >> RF Design >> How to Calculate Noise Figure using spectre RF
https://designers-guide.org/forum/YaBB.pl?num=1080765926

Message started by Iamalearner on Mar 31^st, 2004, 12:45pm

Title: How to Calculate Noise Figure using spectre RF
Post by Iamalearner on Mar 31^st, 2004, 12:45pm

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

Title: Re: How to Calculate Noise Figure using spectre RF
Post by skt on Mar 31^st, 2004, 1:39pm

In the s-parameter results window
select NF for function, plot type and scale

see cadence spectre RF user guide fo more details. A step by step procedure is given in
Ch-6 : Simulating Low- Noise amplifiers

Title: Re: How to Calculate Noise Figure using spectre RF
Post by Iamalearner on Apr 1^st, 2004, 1:37am

Hi,

while doing sp analysis, In the choosing 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 ideas how to solve the problem?

Title: Re: How to Calculate Noise Figure using spectre RF
Post by Andrew Beckett on Apr 1^st, 2004, 1:12pm

Did you do this from the UI? If so, then it is telling you
that if you specify the input and output port for the noise
part of the sp-analysis, then those ports must appear in the
list of ports you are analysing.

In other words, on the sp Choose Analysis form, where you
specify the list of ports to compute the s-parameters between, this must contain the ports you are specifying as
your input and output ports for the noise part.

Regards,

Andrew.

Title: Re: How to Calculate Noise Figure using spectre RF
Post by Iamalearner on Apr 2^nd, 2004, 2:41pm

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

Title: Re: How to Calculate Noise Figure using spectre RF
Post by skt on Apr 2^nd, 2004, 4:05pm

try connecting the input port between vin+ and vin- and output port between vout+ and vout-.
use these ports in your sp analysis form.
Surya

Title: Re: How to Calculate Noise Figure using spectre RF
Post by Andrew Beckett on Apr 3^rd, 2004, 5:41am

Either that or use an ideal balun (there's one in rfLib) to do
a single <-> differential conversion.

Andrew.

Title: Re: How to Calculate Noise Figure using spectre RF
Post by Ken Kundert on Apr 3^rd, 2004, 1:55pm

See "Measuring S-parameters of a differential mixer" (http://www.designers-guide.com/Analysis/diff-sp.pdf).

-Ken

Title: Re: How to Calculate Noise Figure using spectre RF
Post by Iamalearner on Apr 4^th, 2004, 9:19pm

Hi all,
When i placed only one "psin" port for each of differential input and output, I was able to get Noise figure graph from "sp" analysis.

But I have another question. We can also find noise figure using pnoise analysis. How will that be different from the noise figure found using sp analysis. And for LNA, which simulation should i use, "sp" or "pnoise" ??

Thanks

Title: Re: How to Calculate Noise Figure using spectre RF
Post by Ken Kundert on Apr 5^th, 2004, 12:18am

For an LNA you should not be using pnoise (unless you are applying a large blocking tone). You should use noise.

The sp analysis is somewhat more expensive than a noise analysis. So you would use an sp analysis when you needed s-parameters or if you needed the four noise parameters (nf, min nf, etc.) otherwise you can just use noise.

-Ken

Title: Re: How to Calculate Noise Figure using spectre RF
Post by longma on Oct 7^th, 2005, 12:52am

Hello Ken,

While you said it is not suggested to use Pnoise to calcualte NF for LNA, why in SpctreRF user guide they have an example using Pnoise for NF in "simulating LNA"? what is their purpose for this example? Thanks.

Title: Re: How to Calculate Noise Figure using spectre RF
Post by Ken Kundert on Oct 7^th, 2005, 7:23am

It appears to be a mistake. It should use a simple noise analysis rather than a pnoise analysis.

-Ken