Am 17.02.2018 um 04:22 schrieb Phil Hobbs:> On 02/16/2018 01:19 PM, Jim Thompson wrote:>> <http://www.analog-innovations.com/SED/PSpice_Noise_Calculation.pdf> >> >> Note that the individual contributions from each noise source, >> resistor, device noise, whatever, are tabulated in the .OUT file, >> where it'd be a piece-a-cake to spot the extra noise... had you >> included the termination in your simulation in the first place ;-)In LTspice you can get the contribution of any component you like in the plot of noise over frequency. No need to study the chain printer output.>> >> Oooooops! LTspice doesn't have a .OUT file!! Nor does it have a .NET >> file. Sonofa gun! > > It does have netfiles, and stuff you print gets put in the log file. > > But none of that works if the model doesn't include the noise correctly. > For instance, the ADA4898 model from AD overestimates the 1/f noise by > some orders of magnitude, which is irritating. The 4899 model is much > more realistic, but that one is ten times as fast and only runs on +-5V.A few weeks ago I downloaded a new 4898 model that is much better than the one I used b4. cheers, Gerhard
BJT base current 1/f noise
Started by ●February 10, 2018
Reply by ●February 17, 20182018-02-17
Reply by ●February 17, 20182018-02-17
Am 17.02.2018 um 09:21 schrieb Kevin Aylward:> -----Original Message----- From: Jim Thompson>>> I have a noise report in SS where I order the noise of each component >>> and >>> state its % to the total. >In LTspice just plot onoise(R1) / gain to get it scaled to the input> Oscillator phase noise is somewhat bizarre. It acts like FM capture > effect. You can have a noise plot, find and eliminate a dominant noise > noise, yet still have the "improved" topology have an essentially > overlaid new phase plot. A new noise source just pops up as the > dominant, and the noise don't change.Oscillator phase noise is not bizarre at all. It is just that Spice cannot handle nonlinear noise analysis. Harmonic balance analysis is missing. Spice calculates noise in the linearized circuit at the operating point. But oscillators are inherently nonlinear since they need a limiting mechanism or they would go super nova after some time. (Or not oscillate at all.) During each part of the oscillation cycle the OP is different, gain is different, contributions are different. So you need a harmonic balance simulator, as available in ADS or in Microwave Office and the models for it. I also cannot simulate the noise behavior of my chopper amplifier. In what state of the input switches should it be analyzed? :-( cheers, Gerhard
Reply by ●February 17, 20182018-02-17
Gerhard Hoffmann wrote:> Spice calculates noise in the linearized circuit at the operating > point. But oscillators are inherently nonlinear since they need > a limiting mechanism or they would go super nova after some time. > (Or not oscillate at all.)I thought that it was referred to as 'resonance'.
Reply by ●February 17, 20182018-02-17
"Gerhard Hoffmann" wrote in message news:feqqa1F21heU1@mid.individual.net... Am 17.02.2018 um 09:21 schrieb Kevin Aylward:> -----Original Message----- From: Jim Thompson>>> I have a noise report in SS where I order the noise of each component >>> and >>> state its % to the total. >>In LTspice just plot onoise(R1) / gain to get it scaled to the inputMissed the point. I said an *ordered* *list*, for example Component Noise Report at Frequency = 10Hz "Rank" "Ref Des" "Noise (V/sqrtHz)" "Contribution" 1 qn1 1.80771u 63.7807 % 2 qn1_1f 1.80249u 63.096 % 3 qn2 485.026n 3.1778 % 4 qn2_1f 434.741n 2.54486 % 5 r3 341.859n 1.56584 % 6 qn4 328.451n 1.44454 % 7 qn4_1f 248.531n 824.51m % 8 qn2_rb 201.111n 539.12m % 9 qn4_rb 200.766n 537.269m % 10 qn3 182.546n 443.968m % 11 qn3_1f 161.473n 347.213m % 12 qn1_ib 104.411n 145.027m % 13 qn3_rb 76.5087n 77.8453m % 14 qn1_rb 76.4419n 77.7093m % 15 qn4_ic 73.1846n 71.2255m % 16 qn2_ic 70.1976n 65.5281m % 17 qn1_ic 45.3065n 27.2912m % 18 qn3_ic 35.6833n 16.928m % 19 qn2_ib 25.1827n 8.43072m % 20 qn2_re 15.5829n 3.22808m % 21 qn4_re 15.5567n 3.21723m % 22 qn4_ib 14.3964n 2.75519m % 23 qn3_ib 9.35346n 1.16302m % 24 r2 8.44238n 947.487u % 25 qn3_re 5.92827n 467.194u % 26 qn1_re 5.92339n 466.425u % 27 r4 3.89178n 201.344u % 28 r5 1.86634n 46.3044u % 29 r1 286.521p 1.09132u % 30 qn4_rc 9.83235p 1.28516n % 31 qn2_rc 8.91246p 1.05593n % 32 qn1_rc 4.05183p 218.248p % 33 qn3_rc 3.51699p 164.435p % Total Output Noise 1.93939u>> Oscillator phase noise is somewhat bizarre. It acts like FM capture >> effect. You can have a noise plot, find and eliminate a dominant noise >> noise, yet still have the "improved" topology have an essentially >> overlaid new phase plot. A new noise source just pops up as the dominant, >> and the noise don't change.>Oscillator phase noise is not bizarre at all.Yes it is, when compared to amplitude noise. Some of us have actually done 10,000s of phases simulations over the last 10 years...and produced product to boot...> It is just that Spice >cannot handle nonlinear noise analysis. Harmonic balance analysis >is missing.>Spice calculates noise in the linearized circuit at the operating >point. But oscillators are inherently nonlinear since they need >a limiting mechanism or they would go super nova after some time. >(Or not oscillate at all.)>During each part of the oscillation cycle the OP is different, >gain is different, contributions are different. >So you need a harmonic balance simulator, as available in ADS >or in Microwave Office and the models for it.Granpas.. Suck eggs.....teach....don't... http://www.kevinaylward.co.uk/ee/phasenoise/phasenoise.html and you typically, need something like Shooting Method when the system is highly non-linear. -- Kevin Aylward http://www.anasoft.co.uk - SuperSpice http://www.kevinaylward.co.uk/ee/index.html
Reply by ●February 17, 20182018-02-17
On 02/17/2018 08:50 AM, Gerhard Hoffmann wrote:> Am 17.02.2018 um 09:21 schrieb Kevin Aylward: >> -----Original Message----- From: Jim Thompson > >>>> I have a noise report in SS where I order the noise of each >>>> component and state its % to the total. >> > > In LTspice just plot onoise(R1) / gain to get it scaled to the input > > >> Oscillator phase noise is somewhat bizarre. It acts like FM >> capture effect. You can have a noise plot, find and eliminate a >> dominant noise noise, yet still have the "improved" topology have >> an essentially overlaid new phase plot. A new noise source just >> pops up as the dominant, and the noise don't change. > > Oscillator phase noise is not bizarre at all. It is just that Spice > cannot handle nonlinear noise analysis. Harmonic balance analysis is > missing. > > Spice calculates noise in the linearized circuit at the operating > point. But oscillators are inherently nonlinear since they need a > limiting mechanism or they would go super nova after some time. (Or > not oscillate at all.) > > During each part of the oscillation cycle the OP is different, gain > is different, contributions are different. > > So you need a harmonic balance simulator, as available in ADS or in > Microwave Office and the models for it. > > I also cannot simulate the noise behavior of my chopper amplifier. In > what state of the input switches should it be analyzed? :-( >Good oscillators generally have ALC, though, so the self-limiting behaviour isn't such an issue with simulations (at least outside the ALC bandwidth). Cheers Phil Hobbs -- Dr Philip C D Hobbs Principal Consultant ElectroOptical Innovations LLC / Hobbs ElectroOptics Optics, Electro-optics, Photonics, Analog Electronics Briarcliff Manor NY 10510 http://electrooptical.net https://hobbs-eo.com
Reply by ●February 17, 20182018-02-17
On 02/17/2018 08:13 AM, Gerhard Hoffmann wrote:> Am 17.02.2018 um 04:22 schrieb Phil Hobbs: >> On 02/16/2018 01:19 PM, Jim Thompson wrote: > >>> <http://www.analog-innovations.com/SED/PSpice_Noise_Calculation.pdf> >>> >>> Note that the individual contributions from each noise source, >>> resistor, device noise, whatever, are tabulated in the .OUT file, >>> where it'd be a piece-a-cake to spot the extra noise... had you >>> included the termination in your simulation in the first place ;-) > > In LTspice you can get the contribution of any component you like > in the plot of noise over frequency. No need to study the chain printer > output.Sure. I do that commonly. I just wish that "gain" were the same as V(onoise)/inoise, which it isn't--the units come out scrambled so you get multiple vertical axes that autoscale independently. Thus I'm always plotting stuff like V(Q1)*V(onoise)/inoise and shot noise limits as 1A*sqrt(3.2e-19*1u/1Hz) to get the units to come out right, because LTspice's plotting code is too stupid to know that 1V/1A = 1 ohm.> >>> >>> Oooooops! LTspice doesn't have a .OUT file!! Nor does it have a .NET >>> file. Sonofa gun! >> >> It does have netfiles, and stuff you print gets put in the log file. >> >> But none of that works if the model doesn't include the noise >> correctly. For instance, the ADA4898 model from AD overestimates the >> 1/f noise by some orders of magnitude, which is irritating. The 4899 >> model is much more realistic, but that one is ten times as fast and >> only runs on +-5V. > > A few weeks ago I downloaded a new 4898 model that is much better > than the one I used b4.Where did you get it? Could you shoot me a copy? Cheers Phil Hobbs -- Dr Philip C D Hobbs Principal Consultant ElectroOptical Innovations LLC / Hobbs ElectroOptics Optics, Electro-optics, Photonics, Analog Electronics Briarcliff Manor NY 10510 http://electrooptical.net https://hobbs-eo.com
Reply by ●February 17, 20182018-02-17
On 02/17/2018 10:31 AM, Kevin Aylward wrote:> "Gerhard Hoffmann" wrote in message > news:feqqa1F21heU1@mid.individual.net... > > Am 17.02.2018 um 09:21 schrieb Kevin Aylward: >> -----Original Message----- From: Jim Thompson > >>>> I have a noise report in SS where I order the noise of each >>>> component and >>>> state its % to the total. >> > >> In LTspice just plot onoise(R1) / gain to get it scaled to the input > > > Missed the point. > > I said an *ordered* *list*, for example > > Component Noise Report at Frequency = 10Hz > > "Rank" "Ref Des" "Noise (V/sqrtHz)" "Contribution" > > 1 qn1 1.80771u 63.7807 % > 2 qn1_1f 1.80249u 63.096 % > 3 qn2 485.026n 3.1778 % > 4 qn2_1f 434.741n 2.54486 % > 5 r3 341.859n 1.56584 % > 6 qn4 328.451n 1.44454 % > 7 qn4_1f 248.531n 824.51m % > 8 qn2_rb 201.111n 539.12m % > 9 qn4_rb 200.766n 537.269m % > 10 qn3 182.546n 443.968m % > 11 qn3_1f 161.473n 347.213m % > 12 qn1_ib 104.411n 145.027m % > 13 qn3_rb 76.5087n 77.8453m % > 14 qn1_rb 76.4419n 77.7093m % > 15 qn4_ic 73.1846n 71.2255m % > 16 qn2_ic 70.1976n 65.5281m % > 17 qn1_ic 45.3065n 27.2912m % > 18 qn3_ic 35.6833n 16.928m % > 19 qn2_ib 25.1827n 8.43072m % > 20 qn2_re 15.5829n 3.22808m % > 21 qn4_re 15.5567n 3.21723m % > 22 qn4_ib 14.3964n 2.75519m % > 23 qn3_ib 9.35346n 1.16302m % > 24 r2 8.44238n 947.487u % > 25 qn3_re 5.92827n 467.194u % > 26 qn1_re 5.92339n 466.425u % > 27 r4 3.89178n 201.344u % > 28 r5 1.86634n 46.3044u % > 29 r1 286.521p 1.09132u % > 30 qn4_rc 9.83235p 1.28516n % > 31 qn2_rc 8.91246p 1.05593n % > 32 qn1_rc 4.05183p 218.248p % > 33 qn3_rc 3.51699p 164.435p % > > Total Output Noise 1.93939u >Does it work for subcircuits? One irritation in LTspice is that you can't readily plot the noise contribution of op amps or even of transistors if their models include parasitics (and so have to be subcircuits). Cheers Phil Hobbs -- Dr Philip C D Hobbs Principal Consultant ElectroOptical Innovations LLC / Hobbs ElectroOptics Optics, Electro-optics, Photonics, Analog Electronics Briarcliff Manor NY 10510 http://electrooptical.net https://hobbs-eo.com
Reply by ●February 17, 20182018-02-17
On 02/17/2018 11:03 AM, Phil Hobbs wrote:> On 02/17/2018 08:13 AM, Gerhard Hoffmann wrote: >> Am 17.02.2018 um 04:22 schrieb Phil Hobbs: >>> On 02/16/2018 01:19 PM, Jim Thompson wrote: >> >>>> <http://www.analog-innovations.com/SED/PSpice_Noise_Calculation.pdf> >>>> >>>> Note that the individual contributions from each noise source, >>>> resistor, device noise, whatever, are tabulated in the .OUT file, >>>> where it'd be a piece-a-cake to spot the extra noise... had you >>>> included the termination in your simulation in the first place ;-) >> >> In LTspice you can get the contribution of any component you like >> in the plot of noise over frequency. No need to study the chain printer >> output. > > Sure. I do that commonly. I just wish that "gain" were the same as > V(onoise)/inoise, which it isn't--the units come out scrambled so you > get multiple vertical axes that autoscale independently. > > Thus I'm always plotting stuff like >(wrong way up)> V(Q1)*inoise/V(onoise) > > and shot noise limits as > > 1A*sqrt(3.2e-19*1u/1Hz) > > to get the units to come out right, because LTspice's plotting code is > too stupid to know that 1V/1A = 1 ohm.Cheers Phil Hobbs -- Dr Philip C D Hobbs Principal Consultant ElectroOptical Innovations LLC / Hobbs ElectroOptics Optics, Electro-optics, Photonics, Analog Electronics Briarcliff Manor NY 10510 http://electrooptical.net https://hobbs-eo.com
Reply by ●February 17, 20182018-02-17
On Fri, 16 Feb 2018 22:22:41 -0500, Phil Hobbs <pcdhSpamMeSenseless@electrooptical.net> wrote:>On 02/16/2018 01:19 PM, Jim Thompson wrote:[snip]>> >> Oooooops! LTspice doesn't have a .OUT file!! Nor does it have a .NET >> file. Sonofa gun! > >It does have netfiles, and stuff you print gets put in the log file. >[snip] Can you show me how that works? I haven't been able to figure that out. Maybe a *.asc example that prints out a noise report? ...Jim Thompson -- | James E.Thompson | mens | | Analog Innovations | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | STV, Queen Creek, AZ 85142 Skype: skypeanalog | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | It's what you learn, after you know it all, that counts.
Reply by ●February 17, 20182018-02-17
On 02/17/2018 11:53 AM, Jim Thompson wrote:> On Fri, 16 Feb 2018 22:22:41 -0500, Phil Hobbs > <pcdhSpamMeSenseless@electrooptical.net> wrote: > >> On 02/16/2018 01:19 PM, Jim Thompson wrote: > > [snip] >>> >>> Oooooops! LTspice doesn't have a .OUT file!! Nor does it have a .NET >>> file. Sonofa gun! >> >> It does have netfiles, and stuff you print gets put in the log file. >> > [snip] > > Can you show me how that works? I haven't been able to figure that > out.View -> SPICE netlist> > Maybe a *.asc example that prints out a noise report?http://ltwiki.org/index.php?title=MEASURE_Evaluate_User_Defined_Electrical_Quantities Cheers Phil Hobbs -- Dr Philip C D Hobbs Principal Consultant ElectroOptical Innovations LLC / Hobbs ElectroOptics Optics, Electro-optics, Photonics, Analog Electronics Briarcliff Manor NY 10510 http://electrooptical.net https://hobbs-eo.com
