On Wed, 28 May 2014 02:41:37 -0700, <jurb6006@gmail.com> wrote:> ...snip... > I dunno anymore, should I just... > > ?...continue to bite your tongue? yeah, good idea. Did you notice the significance in your point got lost in the typos and gramatical errors. Perhaps, try again and elaborate a bit, and of course, epithets deleted, they didn't add much.
Simulating Power Bandwidth
Started by ●May 24, 2014
Reply by ●May 28, 20142014-05-28
Reply by ●May 28, 20142014-05-28
In article <op.xgksy1ym2cx0wh@ajm>, robert.a.macy@gmail.com says...> > On Wed, 28 May 2014 01:17:09 -0700, Tim Williams <tmoranwms@charter.net> > wrote: > > > "RobertMacy" <robert.a.macy@gmail.com> wrote in message > > news:op.xgjnprcs2cx0wh@ajm... > >> The 'bobbling' is exacerbated at crossovers. I just ran the LT1028 with > >> 7 > >> Vpk at 1MHz and found some WILD current transients at crossovers from > >> both supplies. All the 'bobbling' stopped when I forced the step size > >> small enough to not have the error estimations, etc. interact with the > >> approximation processes in the solver. > > > > I don't get "bobbling" in my simulations. Did you neglect to change the > > integration method from TRAP to GEAR? :) > > > > Tim > > > > Neglect?! spit! sputter! what the heck is that?! Again, and as usual, > can't find any reference in the manual. > > Thanks, found it as > .options method=gear > or something like that, but no explanation of the impact of selecting that > non-default value. > > Will try it. Has to make it faster than forcing the step size to be 50 > times smaller. > > Exactly where is a good description for all these options?If that don't work, you could also try the crank and at last resort then block and tackle method. I am sure there must be some hidden hacks like that somewhere in the software switches. Jamie
Reply by ●May 28, 20142014-05-28
On Wed, 28 May 2014 01:17:09 -0700, Tim Williams <tmoranwms@charter.net> wrote:> "RobertMacy" <robert.a.macy@gmail.com> wrote in message > news:op.xgjnprcs2cx0wh@ajm... >> The 'bobbling' is exacerbated at crossovers. I just ran the LT1028 with >> 7 >> Vpk at 1MHz and found some WILD current transients at crossovers from >> both supplies. All the 'bobbling' stopped when I forced the step size >> small enough to not have the error estimations, etc. interact with the >> approximation processes in the solver. > > I don't get "bobbling" in my simulations. Did you neglect to change the > integration method from TRAP to GEAR? :) > > Tim >doesn't make much difference. if the maximum step size is not set well, the output voltage 'bobbles' pretty much the same whether TRAP or GEAR only thing that stops the bobbling is to make the max step size 1/100th of what you'd normally 'like' to set it at.
Reply by ●May 28, 20142014-05-28
On Wed, 28 May 2014 10:18:34 -0700, RobertMacy <robert.a.macy@gmail.com> wrote:>On Wed, 28 May 2014 01:17:09 -0700, Tim Williams <tmoranwms@charter.net> >wrote: > >> "RobertMacy" <robert.a.macy@gmail.com> wrote in message >> news:op.xgjnprcs2cx0wh@ajm... >>> The 'bobbling' is exacerbated at crossovers. I just ran the LT1028 with >>> 7 >>> Vpk at 1MHz and found some WILD current transients at crossovers from >>> both supplies. All the 'bobbling' stopped when I forced the step size >>> small enough to not have the error estimations, etc. interact with the >>> approximation processes in the solver. >> >> I don't get "bobbling" in my simulations. Did you neglect to change the >> integration method from TRAP to GEAR? :) >> >> Tim >> > > >doesn't make much difference. if the maximum step size is not set well, >the output voltage 'bobbles' pretty much the same whether TRAP or GEAR > >only thing that stops the bobbling is to make the max step size 1/100th of >what you'd normally 'like' to set it at."Speed kills"... in a simulator you can trade accuracy for speed. I tend to use a max timestep equal to 1/(32*Fmax). "Patience is a virtue" >:-} ...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.
Reply by ●May 28, 20142014-05-28
On Wed, 28 May 2014 02:41:37 -0700 (PDT), jurb6006@gmail.com wrote:>I can hold my tpnue no longer. How the fuck can an accomp;lished engineer like you not get this. It is so fucng simple. > >the bandwidth of an amp is what is it, but the power bandwidth is what the output stae (and its asociates) cn deliver. > >I mean like come on, you are not talking some fuckin weirdo ass shit here. > >I dunno anymore, should I just... > >?Ladies and gents, the tirade above is why I blanket killfile gmail/google posters, then whitelist any good guys (takes fewer filters than killfiling the majority of gmail/google posters by their individual names >:-} Clearly this jerk-off didn't even read my post, nor does he have a clue what power bandwidth really is. Nor how power bandwidth is related to slew-rate. Nor how to measure it in the lab. Nor how you could replicate that lab setup as a performance analysis in a simulator... which was what my post was all about. I've been designing OpAmp chips for more than 50 years ...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.
Reply by ●May 28, 20142014-05-28
On Wed, 28 May 2014 10:26:48 -0700, Jim Thompson <To-Email-Use-The-Envelope-Icon@on-my-web-site.com> wrote:>> ...snip... > "Speed kills"... in a simulator you can trade accuracy for speed. I > tend to use a max timestep equal to 1/(32*Fmax). > > "Patience is a virtue" >:-} > > ...Jim ThompsonI don't know what Mike Engelhardt did inside that LTspice but it is a 'screamer'! for example, using the built-in models with graphics is usually ten times faster than using the same models, but spelling them out, in a *.cir old style entry. Mike said the noise modeling inside ALL the Linear OpAmps in the LTspice library are accurate! Which appeared to be true on the ones I checked. Even had the 1/f contributions in there! Only downside is the noise values are 'typical' ;)
Reply by ●May 28, 20142014-05-28
On Wed, 28 May 2014 10:34:48 -0700, Jim Thompson <To-Email-Use-The-Envelope-Icon@on-my-web-site.com> wrote:>> ...snip....incomprehensible tirade > ,,,snip....righteous indignation > ...Jim ThompsonYou must have missed the "Do not feed the trolls" sign? ;)
Reply by ●May 28, 20142014-05-28
On Wed, 28 May 2014 10:45:53 -0700, RobertMacy <robert.a.macy@gmail.com> wrote:>On Wed, 28 May 2014 10:34:48 -0700, Jim Thompson ><To-Email-Use-The-Envelope-Icon@on-my-web-site.com> wrote: > >>> ...snip....incomprehensible tirade >> ,,,snip....righteous indignation >> ...Jim Thompson > >You must have missed the "Do not feed the trolls" sign? ;)Every once in a while they make me want to swat them like flies. ...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.
Reply by ●May 28, 20142014-05-28
"RobertMacy" <robert.a.macy@gmail.com> wrote in message news:op.xgksy1ym2cx0wh@ajm...> Exactly where is a good description for all these options?...Let alone how to use them? Stuff like GEAR is well documented by most SPICE descriptions, and computational solvers in general; it's their word for Runge-Kutta of order MAXORD. Note that TRAP (trapezoidal, i.e. Newton's Method, more or less) is essentially RK1. I very rarely use TRAP in my simulations because the settling is poor and erratic (the result is a distinctive alternation, every other timestep, of a given variable about its ideal value -- it looks like triangles when zoomed), particularly for nonlinear (switching) circuits. Occasionally, I find RK4 (GEAR, MAXORD = 4) beneficial: the average timestep is calculated much more slowly (more derivatives to compute), but the worst-cases are much better -- it's not digging as deep (constantly redoing a bad calculation at progressively smaller timesteps) or as often, around strongly nonlinear events (such as switching edges), so the overall simulation can run faster (and more stable -- less likely to get stuck on a randomly too-small timestep). I don't believe I've ever seen GEAR2 produce "bobbling" results; either it settles asyptotically, or the oscillation is really there (as evidenced by finding a smooth sinusoidal oscillation after setting smaller RELTOL and/or max. timestep to enhance detail). As for "how to use", judging by the dearth of instructions or even useful documentation on most SPICE settings, I can only assume three things: 1. Don't touch that, you'll screw it up! Use the default settings! If it starts throwing errors, the circuit /must/ be impossible! 2. Play with all of them and see what works. Life is a journey, or something. 3. I know what works, but I'm not going to tell you. Against the apparent collective wisdom of all three, I dare suggest these, which seem to work well enough (these are in Multisim, which is your basic XSPICE backend): http://seventransistorlabs.com/Images/SimSettings1.png http://seventransistorlabs.com/Images/SimSettings2.png http://seventransistorlabs.com/Images/SimSettings3.png but not all are available in LTSpice, so YMMV. The most obscure setting of them all seems to be pivot (PIVREL, PIVTOL). It's purely a computational thing, and of the few references I can find to it, the only sentiment is "does nothing, leave it alone". Yet I've had more than a few failing circuits fixed by setting a more strict (larger) value, like as shown. I dare someone to explain that. Tim -- Seven Transistor Labs Electrical Engineering Consultation Website: http://seventransistorlabs.com
Reply by ●May 28, 20142014-05-28
On Wed, 28 May 2014 12:38:06 -0700, Tim Williams <tmoranwms@charter.net> wrote:> ...with gret regret having to snip to keep Aioe happy...> 1. Don't touch that, you'll screw it up! Use the default settings! If > it > starts throwing errors, the circuit /must/ be impossible! > 2. Play with all of them and see what works. Life is a journey, or > something. > 3. I know what works, but I'm not going to tell you.LOL!> ...snip some great URL'sI purchased from MicroSim their PSpice manual. It's in storage and I have no access. But I do remember excellent explanations for what is going on. to the point of being able to make a great deal of decent models.> The most obscure setting of them all seems to be pivot (PIVREL, PIVTOL). > It's purely a computational thing, and of the few references I can find > to > it, the only sentiment is "does nothing, leave it alone". Yet I've had > more than a few failing circuits fixed by setting a more strict (larger) > value, like as shown. I dare someone to explain that. > > Tim >Thanks for the great suggestions, will try them. Sadly, while at University I seemd to have missed three important areas: Maxwell's equations, which I need to use constantly; noise, although took some great courses at Stanford from Robert Geray and T. Kailath, which now live and breathe noise everyday; and numerical analysis, which was best described by moving hand over forehead loudly declaring 'whoosh' and now every day fight battles with simple things like truncation errors, convergence issues, and accumulation truncation errors, ad nauseum. And now, the 'nuances' of spice kernel. sigh.[if that was even the correct word]
