>Take it up with Berkeley... the method has never changed... all these >years.And (AFAIK) all the copies and rewrites do it too. It's still a wart--numerical methods have come a long way since 1970, except in circuit design.>It's not like "over and over" is a big deal... noise/AC analysis >occurs about as fast as you can blink.With discrete circuits, usually so. However, lots of IC models *cough* TI op amps *cough* have ugly convergence issues even with ".savebias internal", so waiting needlessly for that 50 times is annoying. Cheers Phil Hobbs
LT Spice noise analysis
Started by ●February 27, 2017
Reply by ●March 1, 20172017-03-01
Reply by ●March 1, 20172017-03-01
On Wed, 1 Mar 2017 06:26:23 -0800 (PST), pcdhobbs@gmail.com wrote:>>Take it up with Berkeley... the method has never changed... all these >>years. > >And (AFAIK) all the copies and rewrites do it too. It's still a wart--numerical methods have come a long way since 1970, except in circuit design. > >>It's not like "over and over" is a big deal... noise/AC analysis >>occurs about as fast as you can blink. > >With discrete circuits, usually so. However, lots of IC models *cough* TI op amps *cough* have ugly convergence issues even with ".savebias internal", so waiting needlessly for that 50 times is annoying. > > >Cheers > >Phil HobbsTake it up with TI and LTspice... LTspice had a lot of convergence issues with analog parts that other simulators don't. (Also, You should read up on that important tool .STEP. You should be able to do component stepping within a single run... minimizing the bias recalculation.) ...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 | Thinking outside the box... producing elegant solutions.
Reply by ●March 1, 20172017-03-01
On Wed, 1 Mar 2017 06:00:12 -0800 (PST), pcdhobbs@gmail.com wrote:>>But LT Spice doesn't calculate input referred noise. > >Sure it does--INOISE is just V(ONOISE)/GAIN.I can do that. How do I get Spice to do that? And GAIN is not a number, it's a function of frequency. My circuit is a transconductance amp, so GAIN is in ohms. -- John Larkin Highland Technology, Inc lunatic fringe electronics
Reply by ●March 1, 20172017-03-01
On 03/01/2017 09:58 AM, Jim Thompson wrote:> On Wed, 1 Mar 2017 06:26:23 -0800 (PST), pcdhobbs@gmail.com wrote: > >>> Take it up with Berkeley... the method has never changed... all >>> these years. >> >> And (AFAIK) all the copies and rewrites do it too. It's still a >> wart--numerical methods have come a long way since 1970, except in >> circuit design. >> >>> It's not like "over and over" is a big deal... noise/AC analysis >>> occurs about as fast as you can blink. >> >> With discrete circuits, usually so. However, lots of IC models >> *cough* TI op amps *cough* have ugly convergence issues even with >> ".savebias internal", so waiting needlessly for that 50 times is >> annoying.> > Take it up with TI and LTspice... LTspice had a lot of convergence > issues with analog parts that other simulators don't.Nah, ragging you is way more entertaining. I recall your having trouble with the OPA140 in PSPICE as well. And of course LTspice's price is right.> > (Also, You should read up on that important tool .STEP. You should > be able to do component stepping within a single run... minimizing > the bias recalculation.)I use .step fairly often, but in LTspice it doesn't fix the bias issues. Changing resistors or voltages makes the bias different on each run. Using .step to flip switches (nice infinitely differentiable ones) to connect INOISE to different places in the circuit shouldn't make the bias move, but for some reason with models like TI's OPA140 LTspice doesn't skip the entire bias calculation even with .savebias internal. (Super nice op amp, super crappy model.) 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
Reply by ●March 1, 20172017-03-01
On 03/01/2017 10:18 AM, John Larkin wrote:> On Wed, 1 Mar 2017 06:00:12 -0800 (PST), pcdhobbs@gmail.com wrote: > >>> But LT Spice doesn't calculate input referred noise. >> >> Sure it does--INOISE is just V(ONOISE)/GAIN. > > I can do that. How do I get Spice to do that? > > And GAIN is not a number, it's a function of frequency. > > My circuit is a transconductance amp, so GAIN is in ohms. > >Select the plot window, go ctl-A and type "inoise" into the dialogue box. 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
Reply by ●March 1, 20172017-03-01
On Wed, 1 Mar 2017 10:30:54 -0500, Phil Hobbs <pcdhSpamMeSenseless@electrooptical.net> wrote:>On 03/01/2017 10:18 AM, John Larkin wrote: >> On Wed, 1 Mar 2017 06:00:12 -0800 (PST), pcdhobbs@gmail.com wrote: >> >>>> But LT Spice doesn't calculate input referred noise. >>> >>> Sure it does--INOISE is just V(ONOISE)/GAIN. >> >> I can do that. How do I get Spice to do that? >> >> And GAIN is not a number, it's a function of frequency. >> >> My circuit is a transconductance amp, so GAIN is in ohms. >> >> > >Select the plot window, go ctl-A and type "inoise" into the dialogue box. > >Cheers > >Phil HobbsOK, tried that. It shows V(inoise) as bigger than V(onoise), both in units of volts; my named input is a current source. The circuit has a gain of 3, 150 ohms Gm, so that makes no sense. Hey, this is fun. I went to "edit simulation command" for noise and entered V(AMP) as the output and I(Ipd) as the input. That made the thing go bezerk and made nonsense out of the sim parameters. Yes, it should have been V(AMP) and Ipd. This is what it did to my setup: https://dl.dropboxusercontent.com/u/53724080/Spice/Noise_Sim.jpg This is the second time I managed to tie LT Spice in knots by entering an incorrect expression. Last time, I crashed it with mismatched parentheses, and Mike fixed it. I can name a power supply as the input noise source, and it calculates my output noise as usual. If I then do the ctrl/A thing, I get a very weird input noise graph, a huge noise floor and a giant spike about 16 MHz. I think I'll ignore the input noise thing. I have to name some source to get it to run, but apparently I can name anything. The calculated output noise does seem to make sense. -- John Larkin Highland Technology, Inc lunatic fringe electronics
Reply by ●March 1, 20172017-03-01
On Wed, 1 Mar 2017 10:20:09 -0500, Phil Hobbs <pcdhSpamMeSenseless@electrooptical.net> wrote:>On 03/01/2017 09:58 AM, Jim Thompson wrote: >> On Wed, 1 Mar 2017 06:26:23 -0800 (PST), pcdhobbs@gmail.com wrote: >> >>>> Take it up with Berkeley... the method has never changed... all >>>> these years. >>> >>> And (AFAIK) all the copies and rewrites do it too. It's still a >>> wart--numerical methods have come a long way since 1970, except in >>> circuit design. >>> >>>> It's not like "over and over" is a big deal... noise/AC analysis >>>> occurs about as fast as you can blink. >>> >>> With discrete circuits, usually so. However, lots of IC models >>> *cough* TI op amps *cough* have ugly convergence issues even with >>> ".savebias internal", so waiting needlessly for that 50 times is >>> annoying. > >> >> Take it up with TI and LTspice... LTspice had a lot of convergence >> issues with analog parts that other simulators don't. > >Nah, ragging you is way more entertaining. > >I recall your having trouble with the OPA140 in PSPICE as well. And of >course LTspice's price is right. > >> >> (Also, You should read up on that important tool .STEP. You should >> be able to do component stepping within a single run... minimizing >> the bias recalculation.) > >I use .step fairly often, but in LTspice it doesn't fix the bias issues. > Changing resistors or voltages makes the bias different on each run. > >Using .step to flip switches (nice infinitely differentiable ones) to >connect INOISE to different places in the circuit shouldn't make the >bias move, but for some reason with models like TI's OPA140 LTspice >doesn't skip the entire bias calculation even with .savebias internal. >(Super nice op amp, super crappy model.) > >Cheers > >Phil HobbsThat is nice. TI is doing good linears lately. My fave gumdrop is now OPA197. Cheaper than LM7301 and better. -- John Larkin Highland Technology, Inc lunatic fringe electronics
Reply by ●March 1, 20172017-03-01
On 03/01/2017 11:47 AM, John Larkin wrote:> On Wed, 1 Mar 2017 10:30:54 -0500, Phil Hobbs > <pcdhSpamMeSenseless@electrooptical.net> wrote: > >> On 03/01/2017 10:18 AM, John Larkin wrote: >>> On Wed, 1 Mar 2017 06:00:12 -0800 (PST), pcdhobbs@gmail.com wrote: >>> >>>>> But LT Spice doesn't calculate input referred noise. >>>> >>>> Sure it does--INOISE is just V(ONOISE)/GAIN. >>> >>> I can do that. How do I get Spice to do that? >>> >>> And GAIN is not a number, it's a function of frequency. >>> >>> My circuit is a transconductance amp, so GAIN is in ohms. >>> >>> >> >> Select the plot window, go ctl-A and type "inoise" into the dialogue box. >> >> Cheers >> >> Phil Hobbs > > OK, tried that. It shows V(inoise) as bigger than V(onoise), both in > units of volts; my named input is a current source. The circuit has a > gain of 3, 150 ohms Gm, so that makes no sense. > > Hey, this is fun. I went to "edit simulation command" for noise and > entered > > V(AMP) as the output and > > I(Ipd) as the input. > > That made the thing go bezerk and made nonsense out of the sim > parameters. Yes, it should have been V(AMP) and Ipd.Sure, the parser isn't very smart--it bumps you down to the next field when it gets confused.> > This is what it did to my setup: > > https://dl.dropboxusercontent.com/u/53724080/Spice/Noise_Sim.jpg > > This is the second time I managed to tie LT Spice in knots by entering > an incorrect expression. Last time, I crashed it with mismatched > parentheses, and Mike fixed it. > > > I can name a power supply as the input noise source, and it calculates > my output noise as usual. If I then do the ctrl/A thing, I get a very > weird input noise graph, a huge noise floor and a giant spike about 16 > MHz.There's probably a null in the transfer function. I nearly always have to change the vertical scale or do something like min(inoise, 100f) in the plot expression (that prevents the autoranging from screwing up the display when you re-run the sim).> > I think I'll ignore the input noise thing. I have to name some source > to get it to run, but apparently I can name anything. The calculated > output noise does seem to make sense.I usually inoise in preference to onoise, because onoise is much harder to relate to the fundamental physics, which is what I usually care about. Inoise works fine. Another nice thing is that LTspice does the right thing when you add noise contributions. For instance, in a front end with two parallelled JFETs Q1 and Q2, you can plot V(Q1)+V(Q2) and it comes out sqrt(2) times larger than just V(Q1) instead of doubled. 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
Reply by ●March 1, 20172017-03-01
On 03/01/2017 11:54 AM, John Larkin wrote:> On Wed, 1 Mar 2017 10:20:09 -0500, Phil Hobbs > <pcdhSpamMeSenseless@electrooptical.net> wrote: > >> On 03/01/2017 09:58 AM, Jim Thompson wrote: >>> On Wed, 1 Mar 2017 06:26:23 -0800 (PST), pcdhobbs@gmail.com wrote: >>> >>>>> Take it up with Berkeley... the method has never changed... all >>>>> these years. >>>> >>>> And (AFAIK) all the copies and rewrites do it too. It's still a >>>> wart--numerical methods have come a long way since 1970, except in >>>> circuit design. >>>> >>>>> It's not like "over and over" is a big deal... noise/AC analysis >>>>> occurs about as fast as you can blink. >>>> >>>> With discrete circuits, usually so. However, lots of IC models >>>> *cough* TI op amps *cough* have ugly convergence issues even with >>>> ".savebias internal", so waiting needlessly for that 50 times is >>>> annoying. >> >>> >>> Take it up with TI and LTspice... LTspice had a lot of convergence >>> issues with analog parts that other simulators don't. >> >> Nah, ragging you is way more entertaining. >> >> I recall your having trouble with the OPA140 in PSPICE as well. And of >> course LTspice's price is right. >> >>> >>> (Also, You should read up on that important tool .STEP. You should >>> be able to do component stepping within a single run... minimizing >>> the bias recalculation.) >> >> I use .step fairly often, but in LTspice it doesn't fix the bias issues. >> Changing resistors or voltages makes the bias different on each run. >> >> Using .step to flip switches (nice infinitely differentiable ones) to >> connect INOISE to different places in the circuit shouldn't make the >> bias move, but for some reason with models like TI's OPA140 LTspice >> doesn't skip the entire bias calculation even with .savebias internal. >> (Super nice op amp, super crappy model.) >> >> Cheers >> >> Phil Hobbs > > That is nice. TI is doing good linears lately. > > My fave gumdrop is now OPA197. Cheaper than LM7301 and better. > >Nice. 36V CMOS RRIO, reasonable noise, 70 cents. Drift fairly putrid, but not out of line. 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
Reply by ●March 1, 20172017-03-01
On Wed, 1 Mar 2017 10:20:09 -0500, Phil Hobbs <pcdhSpamMeSenseless@electrooptical.net> wrote:>On 03/01/2017 09:58 AM, Jim Thompson wrote: >> On Wed, 1 Mar 2017 06:26:23 -0800 (PST), pcdhobbs@gmail.com wrote: >> >>>> Take it up with Berkeley... the method has never changed... all >>>> these years. >>> >>> And (AFAIK) all the copies and rewrites do it too. It's still a >>> wart--numerical methods have come a long way since 1970, except in >>> circuit design. >>> >>>> It's not like "over and over" is a big deal... noise/AC analysis >>>> occurs about as fast as you can blink. >>> >>> With discrete circuits, usually so. However, lots of IC models >>> *cough* TI op amps *cough* have ugly convergence issues even with >>> ".savebias internal", so waiting needlessly for that 50 times is >>> annoying. > >> >> Take it up with TI and LTspice... LTspice had a lot of convergence >> issues with analog parts that other simulators don't. > >Nah, ragging you is way more entertaining.I know >:-}> >I recall your having trouble with the OPA140 in PSPICE as well. And of >course LTspice's price is right.I know how to model such creatures now, but have very little time to "play"... suddenly got busy :-)> >> >> (Also, You should read up on that important tool .STEP. You should >> be able to do component stepping within a single run... minimizing >> the bias recalculation.) > >I use .step fairly often, but in LTspice it doesn't fix the bias issues. > Changing resistors or voltages makes the bias different on each run. > >Using .step to flip switches (nice infinitely differentiable ones) to >connect INOISE to different places in the circuit shouldn't make the >bias move, but for some reason with models like TI's OPA140 LTspice >doesn't skip the entire bias calculation even with .savebias internal. >(Super nice op amp, super crappy model.) > >Cheers > >Phil HobbsFace it, LTspice is not that wonderful for lots of analog stuff. But I'm back into painful land... having to use Cadence Virtuoso for a customer... almost as bad a schematic entry as LTspice :-( ...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 | Thinking outside the box... producing elegant solutions.
