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 31st, 2004, 12:45pm |
Title: How to Calculate Noise Figure using spectre RF Post by Iamalearner on Mar 31st, 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 31st, 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 1st, 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 1st, 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 2nd, 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 2nd, 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 3rd, 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 3rd, 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 4th, 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 5th, 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 7th, 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 7th, 2005, 7:23am It appears to be a mistake. It should use a simple noise analysis rather than a pnoise analysis. -Ken |
The Designer's Guide Community Forum » Powered by YaBB 2.2.2! YaBB © 2000-2008. All Rights Reserved. |