Forums

Does the noise density function increase if an OpAmp goes into slew rate limit?

Started by RobertMacy May 28, 2014
On Fri, 06 Jun 2014 07:31:54 -0700, RobertMacy
<robert.a.macy@gmail.com> wrote:

>On Fri, 30 May 2014 16:35:45 -0700, Jim Thompson ><To-Email-Use-The-Envelope-Icon@on-my-web-site.com> wrote: > >>> ..snip.... >> I have no idea... you're supposed to elucidate me >:-} >> >> ...Jim Thompson > >Didn't see any comment to yesterday's posting, showing preliminary >modleing of slew rate limiting effects. > >Also, I have the subckt model AND the discrete model all done to send to >you. just found your teaching aid .pdf with the mask photo, didn't see >the CAP yet, but at least have the pin out now, so can do a 'complete' >MC1530 subckt model including the lead/lag terminals. > >Do those 'minimum size' NPNs really act like the 3904 model? seems their >areas would have to affect the model's terms in some way.
I'm sure I have the models from that era... somewhere ;-) When I find them, I'll drop them in. I just tossed that together to get you something to play with. How does your transient simulation demonstrate noise? ...Jim Thompson -- | James E.Thompson | mens | | Analog Innovations | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | San Tan Valley, AZ 85142 Skype: skypeanalog | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | I love to cook with wine. Sometimes I even put it in the food.
On Fri, 06 Jun 2014 07:34:09 -0700, Jim Thompson  
<To-Email-Use-The-Envelope-Icon@on-my-web-site.com> wrote:

>> ...snip... > I'm sure I have the models from that era... somewhere ;-) When I find > them, I'll drop them in. I just tossed that together to get you > something to play with. > > How does your transient simulation demonstrate noise? > > ...Jim Thompson
yeah, I can just drop in new .model statement, so was worth playing with the 3904 stuff. You must not have seen, [prelim ONLY - 'walk before run' model represented the noise from only four resistors: Rinput, Rfdbk, R8 and R11] The spectrum for these results was 1kHz to 10MHz. MC1530 configured as a simple inverter 10k input, 10k feedback, GND the IN+ terminal, power with +/-6 Vdc, drive with sine at 400kHz. with only 2mVpk drive [could have used zero, but didn't], the noise is around 14nV/rtHz, fairly close to the 21nV from full blown, plus has a 'spike' at the high end caused by loop-gain effects. The spike is much lower than the full-blown because most of the full-blown spike must come from NPN's Now drive the MC1530 into slew rate limit using 2Vpk, 400kHz, the output is very triangular at around 1.5Vpks and the noise comes up approx 10dB, 3 times. That's also what happened with the OpAmp model. What is different is that above the loop gain cutoff, approx 2-3MHz, the noise stayed the same, only the low frequency part comes up, which makes sense, since noise in that higher band is outside loop gain anyway. in the OpAmp version I had to place the noise sources at the 'input' so above loop gain the noise at the output was simply not reasonable. For example, going into slew rate limit the noise above loop-gain simply disappears. But with the MC1530 'discrete' model where the noise sources are 'inside' you get closer to reality simulation, and the noise above loop-gain simply stays constant. For some reason, during slew rate limit the noise density function does NOT stay flat in the low end. There is a slight increase near the low end and a slight increase near 400kHz. I'll look more closely to see if true. but hate to spend too much more time when the model only has noise from four resistors, not any of the NPN's
On Fri, 06 Jun 2014 08:04:47 -0700, RobertMacy
<robert.a.macy@gmail.com> wrote:

>On Fri, 06 Jun 2014 07:34:09 -0700, Jim Thompson ><To-Email-Use-The-Envelope-Icon@on-my-web-site.com> wrote: > >>> ...snip... >> I'm sure I have the models from that era... somewhere ;-) When I find >> them, I'll drop them in. I just tossed that together to get you >> something to play with. >> >> How does your transient simulation demonstrate noise? >> >> ...Jim Thompson > >yeah, I can just drop in new .model statement, so was worth playing with >the 3904 stuff. > >You must not have seen, >[prelim ONLY - 'walk before run' model represented the noise from only >four resistors: Rinput, Rfdbk, R8 and R11] >The spectrum for these results was 1kHz to 10MHz. > >MC1530 configured as a simple inverter 10k input, 10k feedback, GND the >IN+ terminal, power with +/-6 Vdc, drive with sine at 400kHz. > >with only 2mVpk drive [could have used zero, but didn't], the noise is >around 14nV/rtHz, fairly close to the 21nV from full blown, plus has a >'spike' at the high end caused by loop-gain effects. The spike is much >lower than the full-blown because most of the full-blown spike must come > from NPN's > >Now drive the MC1530 into slew rate limit using 2Vpk, 400kHz, the output >is very triangular at around 1.5Vpks and the noise comes up approx 10dB, 3 >times. > >That's also what happened with the OpAmp model. > >What is different is that above the loop gain cutoff, approx 2-3MHz, the >noise stayed the same, only the low frequency part comes up, which makes >sense, since noise in that higher band is outside loop gain anyway. > >in the OpAmp version I had to place the noise sources at the 'input' so >above loop gain the noise at the output was simply not reasonable. For >example, going into slew rate limit the noise above loop-gain simply >disappears. But with the MC1530 'discrete' model where the noise sources >are 'inside' you get closer to reality simulation, and the noise above >loop-gain simply stays constant. > >For some reason, during slew rate limit the noise density function does >NOT stay flat in the low end. There is a slight increase near the low end >and a slight increase near 400kHz. I'll look more closely to see if true. >but hate to spend too much more time when the model only has noise from >four resistors, not any of the NPN's
The question is... How do you _see_ this noise in a transient analysis? ...Jim Thompson -- | James E.Thompson | mens | | Analog Innovations | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | San Tan Valley, AZ 85142 Skype: skypeanalog | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | I love to cook with wine. Sometimes I even put it in the food.
"RobertMacy"  wrote in message news:op.xgkq2kzo2cx0wh@ajm...

>Trying to sort out circuit simulation artifact from something that may be >real.
>Does the noise come up [because of the inability of the OpAmp to reduce] >when the OpAmp is driven too fast at too large a signal level?
>Circuit is a simple LT1028 in an 'inverting' configuration with power of >+/-12Vdc. GNDed non-inverting input. Rinput = 1k. Rfdbk = 1k. Cfdbk = >20pF. Load is a simple 10k in parallel with 10pF. VERY simple inverter.
>The drive is a sinusoid 1MHz of 7Vpk, which the LT1028 can't keep up with, >making the output a 'triangular' signal around 2 Vpk.
>Now I wish to consider noise: Using LTspice I get an 'expected' noise >density function over the range of ?? to 1MHz that seems reasonable for >the LT1028. With almost no input voltage and doing what I call .tranoise >analyses, where .tran and .noise analyses are combined, I get >approximately the same noise density function. HOWEVER, when the above >sinewave is applied which obviously overdrives the LT1028, the noise >density function increases around 10dB.
>Thus, my question. In real-life should I expect the noise density function >from an overdriven OpAmp to increase?
In general, yes. A key idea is "parametric amplification". This is a technique well known and used for probably 80 years. For example, a non-linear capacitor fed with a H.F. sine wave pump signal can be used to amplify another L.F signal. This is typically used to generate "noiseless" amplification of the LF signal, i.e. the capacitor does not generate noise. In the case here, the L.F signal would actually be the noise getting amplified by the input signal. The math of the signal amplification is the same math used here http://www.kevinaylward.co.uk/ee/tapebias/tapebias.xht Its a big issue for low noise oscillators and r.f. Anytime the system is non-linear there may well be effectively, amplified noise. The overall issues can be quite complicated to understand. Another example of the complexity of the problem is here: By Ken Kundert -Spectre writer http://www.designers-guide.org/Theory/puzzle.pdf Exactly how are you observing this effect anyway? It typically needs an R.F simulator with Periodic Steady State Noise (PSSN) or a spice with a Transient Noise feature. I note somewhere in this thread you say something about combined tran and noise runs. What is actually done? Kevin Aylward B.Sc. www.kevinaylward.co.uk www.anasoft.co.uk - SuperSpice
"Phil Hobbs"  wrote in message 
news:8u-dnUhMA422pxrOnZ2dnUVZ_oWdnZ2d@supernews.com...

> >> Did not mean to mislead, I'm not selecting OpAmps here, Instead I'm >> looking for interactions between non-linear operation and noise. Need to >> verify what I found is real and not a simulation artifact. Again. PSpice >> and LTspice have .noise and .tran analysis, but those analyses are >> woefully lacking if you're trying to understand anything non-linear, >> like mixers, multipliers, OpAmps overdriven, etc. That's where my >> .tranoise analysis gives much better understanding. The time waveform >> plots look just like a scope trace complete with fuzz and meandering >> [1/f noise] and the spectrum noise floor actually tells you something. >> Plus, you can find all the bumps and dragging around noise that did not >> show up using 'separate' analysis techniques. Plus, the 'new' FFT >> displays do not contain artifacts from the spice fft processing. They're >> much cleaner so more useful clear down to the noise floor. >
>If you believe SPICE down to that accuracy level.
I do. The right model truly match reality, time after time.
> It's asking a lot of a crappy macromodel,
Different issue. A good model well get good results with the right tools.
>for sure. Unless I'm very much mistaken, it would be a lot faster and >cheaper to make a couple of boards and have a look.
Spice and Spice model based simulations at the device level, are pretty much, engineering perfect, even for non-linear noise effects. It cost money though. Just this last week I have yet another asic come back where the simulations of phase noise for a complicated oscillator system come nuts on. Its Spectre R.F PSS Noise, but it still uses the same spice BSim3 and VBIC models used in Spice. This Software deals with all the complicated interaction of mixing up 1/f noise, non-linear buffer stages and VCF modulation and gets within a db or so over the range of -60 dBc to -170 dBc phase noise, due to device noise. Its actually stunning that the right mathematics means that chips can be designed first time correctly purely in the virtual world. Its just a fact. Simulations work, and its faster and cheaper than spinning test chips :-) Non-linear phase noise analysis: http://www.kevinaylward.co.uk/ee/phasenoise/A-Demir.pdf Kevin Aylward B.Sc. www.kevinaylward.co.uk www.anasoft.co.uk - SuperSpice
On Fri, 6 Jun 2014 20:05:51 +0100, "Kevin Aylward"
<ExtractkevinRemove@kevinaylward.co.uk> wrote:

>"Phil Hobbs" wrote in message >news:8u-dnUhMA422pxrOnZ2dnUVZ_oWdnZ2d@supernews.com... > >> >>> Did not mean to mislead, I'm not selecting OpAmps here, Instead I'm >>> looking for interactions between non-linear operation and noise. Need to >>> verify what I found is real and not a simulation artifact. Again. PSpice >>> and LTspice have .noise and .tran analysis, but those analyses are >>> woefully lacking if you're trying to understand anything non-linear, >>> like mixers, multipliers, OpAmps overdriven, etc. That's where my >>> .tranoise analysis gives much better understanding. The time waveform >>> plots look just like a scope trace complete with fuzz and meandering >>> [1/f noise] and the spectrum noise floor actually tells you something. >>> Plus, you can find all the bumps and dragging around noise that did not >>> show up using 'separate' analysis techniques. Plus, the 'new' FFT >>> displays do not contain artifacts from the spice fft processing. They're >>> much cleaner so more useful clear down to the noise floor. >> > >>If you believe SPICE down to that accuracy level. > >I do. The right model truly match reality, time after time. > >> It's asking a lot of a crappy macromodel, > >Different issue. A good model well get good results with the right tools. > >>for sure. Unless I'm very much mistaken, it would be a lot faster and >>cheaper to make a couple of boards and have a look. > >Spice and Spice model based simulations at the device level, are pretty >much, engineering perfect, even for non-linear noise effects. It cost money >though. > >Just this last week I have yet another asic come back where the simulations >of phase noise for a complicated oscillator system come nuts on. Its Spectre >R.F PSS Noise, but it still uses the same spice BSim3 and VBIC models used >in Spice. This Software deals with all the complicated interaction of mixing >up 1/f noise, non-linear buffer stages and VCF modulation and gets within a >db or so over the range of -60 dBc to -170 dBc phase noise, due to device >noise. Its actually stunning that the right mathematics means that chips can >be designed first time correctly purely in the virtual world. Its just a >fact. Simulations work, and its faster and cheaper than spinning test chips >:-) > >Non-linear phase noise analysis: > >http://www.kevinaylward.co.uk/ee/phasenoise/A-Demir.pdf > > >Kevin Aylward B.Sc. >www.kevinaylward.co.uk >www.anasoft.co.uk - SuperSpice
Lot of nay-sayers here, but I've not had a chip come out of foundry in many years that didn't perfectly match the simulations. Now I know of some people having problems... you know the type... they design oscillators that require a kick-start and every circuit function requires an OpAmp (that's a not-so-subtle back-handed slap at some losers lurking here... they know who they are >:-} ...Jim Thompson -- | James E.Thompson | mens | | Analog Innovations | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | San Tan Valley, AZ 85142 Skype: skypeanalog | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | I love to cook with wine. Sometimes I even put it in the food.
On 6/6/2014 3:31 PM, Jim Thompson wrote:
> On Fri, 6 Jun 2014 20:05:51 +0100, "Kevin Aylward" > <ExtractkevinRemove@kevinaylward.co.uk> wrote: > >> "Phil Hobbs" wrote in message >> news:8u-dnUhMA422pxrOnZ2dnUVZ_oWdnZ2d@supernews.com... >> >>> >>>> Did not mean to mislead, I'm not selecting OpAmps here, Instead I'm >>>> looking for interactions between non-linear operation and noise. Need to >>>> verify what I found is real and not a simulation artifact. Again. PSpice >>>> and LTspice have .noise and .tran analysis, but those analyses are >>>> woefully lacking if you're trying to understand anything non-linear, >>>> like mixers, multipliers, OpAmps overdriven, etc. That's where my >>>> .tranoise analysis gives much better understanding. The time waveform >>>> plots look just like a scope trace complete with fuzz and meandering >>>> [1/f noise] and the spectrum noise floor actually tells you something. >>>> Plus, you can find all the bumps and dragging around noise that did not >>>> show up using 'separate' analysis techniques. Plus, the 'new' FFT >>>> displays do not contain artifacts from the spice fft processing. They're >>>> much cleaner so more useful clear down to the noise floor. >>> >> >>> If you believe SPICE down to that accuracy level. >> >> I do. The right model truly match reality, time after time. >> >>> It's asking a lot of a crappy macromodel, >> >> Different issue. A good model well get good results with the right tools. >> >>> for sure. Unless I'm very much mistaken, it would be a lot faster and >>> cheaper to make a couple of boards and have a look. >> >> Spice and Spice model based simulations at the device level, are pretty >> much, engineering perfect, even for non-linear noise effects. It cost money >> though. >> >> Just this last week I have yet another asic come back where the simulations >> of phase noise for a complicated oscillator system come nuts on. Its Spectre >> R.F PSS Noise, but it still uses the same spice BSim3 and VBIC models used >> in Spice. This Software deals with all the complicated interaction of mixing >> up 1/f noise, non-linear buffer stages and VCF modulation and gets within a >> db or so over the range of -60 dBc to -170 dBc phase noise, due to device >> noise. Its actually stunning that the right mathematics means that chips can >> be designed first time correctly purely in the virtual world. Its just a >> fact. Simulations work, and its faster and cheaper than spinning test chips >> :-) >> >> Non-linear phase noise analysis: >> >> http://www.kevinaylward.co.uk/ee/phasenoise/A-Demir.pdf >> >> >> Kevin Aylward B.Sc. >> www.kevinaylward.co.uk >> www.anasoft.co.uk - SuperSpice > > Lot of nay-sayers here, but I've not had a chip come out of foundry in > many years that didn't perfectly match the simulations. > > Now I know of some people having problems... you know the type... they > design oscillators that require a kick-start and every circuit > function requires an OpAmp (that's a not-so-subtle back-handed slap at > some losers lurking here... they know who they are >:-} >
I believe that mathematics can model reality very closely in many instances, given a sufficiently good understanding of the parts and the physics involved. A foundry whose whole business depends on simulations matching reality is highly motivated to produce models that do. The board-level world is quite different. Cheers Phil Hobbs -- Dr Philip C D Hobbs Principal Consultant ElectroOptical Innovations LLC Optics, Electro-optics, Photonics, Analog Electronics 160 North State Road #203 Briarcliff Manor NY 10510 hobbs at electrooptical dot net http://electrooptical.net
On Fri, 06 Jun 2014 15:45:49 -0400, Phil Hobbs
<hobbs@electrooptical.net> wrote:

>On 6/6/2014 3:31 PM, Jim Thompson wrote:
[snip]
>> >> Lot of nay-sayers here, but I've not had a chip come out of foundry in >> many years that didn't perfectly match the simulations. >> >> Now I know of some people having problems... you know the type... they >> design oscillators that require a kick-start and every circuit >> function requires an OpAmp (that's a not-so-subtle back-handed slap at >> some losers lurking here... they know who they are >:-} >> > >I believe that mathematics can model reality very closely in many >instances, given a sufficiently good understanding of the parts and the >physics involved. > >A foundry whose whole business depends on simulations matching reality >is highly motivated to produce models that do. > >The board-level world is quite different. > >Cheers > >Phil Hobbs
Indeed, board-level models tend to be crap... I'm trying to remedy that. For that matter, the Spice models for many discrete devices, particularly power MOSFET's can be notoriously bad. ...Jim Thompson -- | James E.Thompson | mens | | Analog Innovations | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | San Tan Valley, AZ 85142 Skype: skypeanalog | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | I love to cook with wine. Sometimes I even put it in the food.
On Fri, 06 Jun 2014 12:31:28 -0700, Jim Thompson
<To-Email-Use-The-Envelope-Icon@On-My-Web-Site.com> wrote:

>On Fri, 6 Jun 2014 20:05:51 +0100, "Kevin Aylward" ><ExtractkevinRemove@kevinaylward.co.uk> wrote: > >>"Phil Hobbs" wrote in message >>news:8u-dnUhMA422pxrOnZ2dnUVZ_oWdnZ2d@supernews.com... >> >>> >>>> Did not mean to mislead, I'm not selecting OpAmps here, Instead I'm >>>> looking for interactions between non-linear operation and noise. Need to >>>> verify what I found is real and not a simulation artifact. Again. PSpice >>>> and LTspice have .noise and .tran analysis, but those analyses are >>>> woefully lacking if you're trying to understand anything non-linear, >>>> like mixers, multipliers, OpAmps overdriven, etc. That's where my >>>> .tranoise analysis gives much better understanding. The time waveform >>>> plots look just like a scope trace complete with fuzz and meandering >>>> [1/f noise] and the spectrum noise floor actually tells you something. >>>> Plus, you can find all the bumps and dragging around noise that did not >>>> show up using 'separate' analysis techniques. Plus, the 'new' FFT >>>> displays do not contain artifacts from the spice fft processing. They're >>>> much cleaner so more useful clear down to the noise floor. >>> >> >>>If you believe SPICE down to that accuracy level. >> >>I do. The right model truly match reality, time after time. >> >>> It's asking a lot of a crappy macromodel, >> >>Different issue. A good model well get good results with the right tools. >> >>>for sure. Unless I'm very much mistaken, it would be a lot faster and >>>cheaper to make a couple of boards and have a look. >> >>Spice and Spice model based simulations at the device level, are pretty >>much, engineering perfect, even for non-linear noise effects. It cost money >>though. >> >>Just this last week I have yet another asic come back where the simulations >>of phase noise for a complicated oscillator system come nuts on. Its Spectre >>R.F PSS Noise, but it still uses the same spice BSim3 and VBIC models used >>in Spice. This Software deals with all the complicated interaction of mixing >>up 1/f noise, non-linear buffer stages and VCF modulation and gets within a >>db or so over the range of -60 dBc to -170 dBc phase noise, due to device >>noise. Its actually stunning that the right mathematics means that chips can >>be designed first time correctly purely in the virtual world. Its just a >>fact. Simulations work, and its faster and cheaper than spinning test chips >>:-) >> >>Non-linear phase noise analysis: >> >>http://www.kevinaylward.co.uk/ee/phasenoise/A-Demir.pdf >> >> >>Kevin Aylward B.Sc. >>www.kevinaylward.co.uk >>www.anasoft.co.uk - SuperSpice > >Lot of nay-sayers here, but I've not had a chip come out of foundry in >many years that didn't perfectly match the simulations.
Oh, good grief! You're talking apples and orangutans. Foundry models are very good. They have to be or the foundry has no customers. OTOH, board-level models invariably suck. Some are good enough to show you that something you know works, works. I've seen none that work even in corner (or basket) case situations. It's rare to see one that even models the power supply.
>Now I know of some people having problems... you know the type... they >design oscillators that require a kick-start and every circuit >function requires an OpAmp (that's a not-so-subtle back-handed slap at >some losers lurking here... they know who they are >:-} > > ...Jim Thompson
On Fri, 06 Jun 2014 18:59:00 -0400, krw@attt.bizz wrote:

>On Fri, 06 Jun 2014 12:31:28 -0700, Jim Thompson ><To-Email-Use-The-Envelope-Icon@On-My-Web-Site.com> wrote:
[snip]
>> >>Lot of nay-sayers here, but I've not had a chip come out of foundry in >>many years that didn't perfectly match the simulations. > >Oh, good grief! You're talking apples and orangutans. Foundry models >are very good. They have to be or the foundry has no customers. OTOH, >board-level models invariably suck. Some are good enough to show you >that something you know works, works. I've seen none that work even >in corner (or basket) case situations. It's rare to see one that even >models the power supply. >
[snip] You're late to the discussion... as usual >:-} ...Jim Thompson -- | James E.Thompson | mens | | Analog Innovations | et | | Analog/Mixed-Signal ASIC's and Discrete Systems | manus | | San Tan Valley, AZ 85142 Skype: skypeanalog | | | Voice:(480)460-2350 Fax: Available upon request | Brass Rat | | E-mail Icon at http://www.analog-innovations.com | 1962 | I love to cook with wine. Sometimes I even put it in the food.