The Designer's Guide Community Forum https://designers-guide.org/forum/YaBB.pl Simulators >> Circuit Simulators >> noise simulation concept https://designers-guide.org/forum/YaBB.pl?num=1215093196 Message started by nathanee on Jul 3rd, 2008, 6:53am

Title: noise simulation concept Post by nathanee on Jul 3rd, 2008, 6:53am Hi, there, Please help to clarify the following concept about noise and simulation method. 1. Thermal, flicker, and KT/C noise CAN NOT be simulated by using spectre/hspice transient method. 2. Thermal, flicker, and KT/C noise CAN be simulated by using spectre/hspice ac method. 3. Thermal, flicker, and KT/C noise CAN be simulated by using spectreRF. Thanks in advance. BR, -nathan

Title: Re: noise simulation concept Post by pancho_hideboo on Jul 3rd, 2008, 6:26pm I can't find any design issue in your post. Your question is not design issue but simple feature of specific vendor's EDA tool.   Please post to "The Designer's Guide Community Forum ≫ Simulators ≫ RF Simulators". nathanee wrote on Jul 3rd, 2008, 6:53am: Please help to clarify the following concept about noise and simulation method. What do you mean by "concept" ? nathanee wrote on Jul 3rd, 2008, 6:53am: 1. Thermal, flicker, and KT/C noise CAN NOT be simulated by using spectre/hspice transient method. Apart from accuracy, you can evaluate these noise using transient noise analysis in Spectre. I don't think HSPICE supports transient noise analysis. So you can't evaluate these noise using HSPICE's transient analysis. nathanee wrote on Jul 3rd, 2008, 6:53am: 2. Thermal, flicker, and KT/C noise CAN be simulated by using spectre/hspice ac method. For time invariant circuit, you can evaluate thermal and flicker noise using AC noise analysis in both Spectre and HSPICE. But you can't evaluate KT/C noise directly using Spectre's AC analysis. On the other hand you can evaluate KT/C noise using HSPICE's combination analysis of ".AC", ".Noise", and ".SAMPLE" analysis, although it is not accurate evaluation. nathanee wrote on Jul 3rd, 2008, 6:53am: 3. Thermal, flicker, and KT/C noise CAN be simulated by using spectreRF. Yes, for periodically time varied circuit, you can evaluate these noise using Shooting Newton Method in both SpectreRF and HSPICE RF.

Title: Re: noise simulation concept Post by daisy on Jul 18th, 2008, 3:35am Hi! In my opinion,when thermal noise 4KTR passes through a rc circuit,the output noise equals KT/C,so we call it KTC noise.I'm not sure whether it is correct or there is another kind of noise called KTC noise like thermal noise and flicker noise? And I also have another question.What does the frequency mean in flicker noise?If I want to compute the output noise of  the circuit, should I integrate the psd of the filcker noise in the bandwidth or from 0 to infinity?I found it is hard to get the result if I integrate in the bandwidth. Thank you for your explanation! daisy pancho_hideboo wrote on Jul 3rd, 2008, 6:26pm: I can't find any design issue in your post. Your question is not design issue but simple feature of specific vendor's EDA tool.   Please post to "The Designer's Guide Community Forum ≫ Simulators ≫ RF Simulators". nathanee wrote on Jul 3rd, 2008, 6:53am: Please help to clarify the following concept about noise and simulation method. What do you mean by "concept" ? nathanee wrote on Jul 3rd, 2008, 6:53am: 1. Thermal, flicker, and KT/C noise CAN NOT be simulated by using spectre/hspice transient method. Apart from accuracy, you can evaluate these noise using transient noise analysis in Spectre. I don't think HSPICE supports transient noise analysis. So you can't evaluate these noise using HSPICE's transient analysis. nathanee wrote on Jul 3rd, 2008, 6:53am: 2. Thermal, flicker, and KT/C noise CAN be simulated by using spectre/hspice ac method. For time invariant circuit, you can evaluate thermal and flicker noise using AC noise analysis in both Spectre and HSPICE. But you can't evaluate KT/C noise directly using Spectre's AC analysis. On the other hand you can evaluate KT/C noise using HSPICE's combination analysis of ".AC", ".Noise", and ".SAMPLE" analysis, although it is not accurate evaluation. nathanee wrote on Jul 3rd, 2008, 6:53am: 3. Thermal, flicker, and KT/C noise CAN be simulated by using spectreRF. Yes, for periodically time varied circuit, you can evaluate these noise using Shooting Newton Method in both SpectreRF and HSPICE RF.

Title: Re: noise simulation concept Post by pancho_hideboo on Jul 18th, 2008, 5:48pm daisy wrote on Jul 18th, 2008, 3:35am: In my opinion,when thermal noise 4KTR passes through a rc circuit,the output noise equals KT/C,so we call it KTC noise. This is no more than thermal noise from resistor in time invariant circuit. But generally term of "kT/C noise" is used for sampled, switched or chopped noise, e.g. noises seen in switched capacitor filter circuit. daisy wrote on Jul 18th, 2008, 3:35am: And I also have another question.What does the frequency mean in flicker noise?If I want to compute the output noise of  the circuit, should I integrate the psd of the filcker noise in the bandwidth or from 0 to infinity?I found it is hard to get the result if I integrate in the bandwidth. I can't understand your question. What do you want to know ? Maybe you don't understand flicker noise correctly.

Title: Re: noise simulation concept Post by daisy on Jul 18th, 2008, 6:31pm Hi! Thank you for your answer! 1.Yes,I mean in a switched capacitor circuit,the switched mos works in the linearity region,so its thermal noise equals 4KTR,where R equals 1/gds,and it results a noise value KT/C in a capacitor which is parallelly connected to the mosfet.Is it right? 2.What I want to know is as follows:in flicker noise formula K/CoxWLf,what does the frequency mean?Does it mean any frequency within the circuit bandwidth?If it is,if I want to get the total flicker noise at the output node,should I integrate the PSD formula in the range of the bandwidth? Thank you for your explanation! daisy pancho_hideboo wrote on Jul 18th, 2008, 5:48pm: daisy wrote on Jul 18th, 2008, 3:35am: In my opinion,when thermal noise 4KTR passes through a rc circuit,the output noise equals KT/C,so we call it KTC noise. This is no more than thermal noise from resistor. But generally term of "kT/C noise" is used for switched or chopped noise, e.g. in switched capacitor filter circuit. daisy wrote on Jul 18th, 2008, 3:35am: And I also have another question.What does the frequency mean in flicker noise?If I want to compute the output noise of  the circuit, should I integrate the psd of the filcker noise in the bandwidth or from 0 to infinity?I found it is hard to get the result if I integrate in the bandwidth. I can't understand your question. What do you want to know ? Maybe you don't understand flicker noise correctly.

Title: Re: noise simulation concept Post by pancho_hideboo on Jul 18th, 2008, 6:52pm daisy wrote on Jul 18th, 2008, 6:31pm: 1.Yes,I mean in a switched capacitor circuit,the switched mos works in the linearity region,so its thermal noise equals 4KTR,where R equals 1/gds,and it results a noise value KT/C in a capacitor which is parallelly connected to the mosfet.Is it right? I don't know what test circuit you assume. Do you assume a time invariant condition and no noise other than gds ? If so,  right. daisy wrote on Jul 18th, 2008, 6:31pm: 2.What I want to know is as follows:in flicker noise formula K/CoxWLf,what does the frequency mean? It means operation frequency, that is analysis frequency. daisy wrote on Jul 18th, 2008, 6:31pm: Does it mean any frequency within the circuit bandwidth?If it is,if I want to get the total flicker noise at the output node,should I integrate the PSD formula in the range of the bandwidth? Do you understand noise holding in periodically time varied circuit ? You should integrate noise over bandwidth you have interest. See http://www.designers-guide.org/Forum/YaBB.pl?num=1211952319 http://www.designers-guide.org/Forum/YaBB.pl?num=1207830622 http://www.designers-guide.org/Forum/YaBB.pl?num=1059089369

The Designer's Guide Community Forum » Powered by YaBB 2.2.2! YaBB © 2000-2008. All Rights Reserved.