Forums

diode recovered charge

Started by John Larkin September 6, 2014
On Sat, 06 Sep 2014 12:31:46 -0700, John Larkin
<jlarkin@highlandtechnology.com> wrote:

> >I got curious about the amount of reverse-recovery charge in PN >diodes, as a function of forward current (and time of fwd bias) and >diode size/type. > >Question is, are the LT Spice diode models realistic? We'll have to >test some diodes to see. Since diode recovery for a given part number >depends a lot on the manufacturer, we should stick to sole-source >parts and tweak the Spice model to align with reality. > >The ES1D below, straight from the LT Spice diode list, seems to have a >definite step-recovery behavior, which probably isn't realistic. It >stores 115 nC when biased to 1 amp forward. The recovered charge is >not a function of ON time, also unrealistic. >
[snip] These two links seem to have reasonable subcircuit additions to model diode reverse recovery time.... <http://www.camacho.prof.ufu.br/Tesi_Gustavo_12gen2006.pdf> <http://www.intusoft.com/nlpdf/nl32.pdf> I don't have the time right now, but I'll later see if I can spin these into a parameterized subcircuit where all you have to do is fill in the blanks >:-] ...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 Thu, 11 Sep 2014 11:10:31 -0400, Phil Hobbs
<pcdhSpamMeSenseless@electrooptical.net> wrote:

>On 09/10/2014 11:51 PM, John Larkin wrote: >> On Wed, 10 Sep 2014 18:53:39 +0100, "Kevin Aylward" >> <ExtractkevinRemove@kevinaylward.co.uk> wrote: >> >>> "John Larkin" wrote in message >>> news:59eu0a521ld1frmg2596rrpbtksg65mgdj@4ax.com... >>> >>> On Tue, 9 Sep 2014 18:21:33 +0100, "Kevin Aylward" >>> <ExtractkevinRemove@kevinaylward.co.uk> wrote: >>> >>>> "Kevin Aylward" wrote in message >>>> news:wcydnUoc3IdqdZDJnZ2dnUVZ7rWdnZ2d@bt.com... >>>> >>>>> "John Larkin" wrote in message >>>>> news:du7p0ad9fmfik7f8utc9e419paiklu6uod@4ax.com... >>>> >>>>> Playing with the standard 1N914 in LT Spice, it shows no forward >>>>> recovery (ie, no turn-on delay). It does store reverse charge, but it >>>>> snaps off instantly, probably just junction capacitance limited, when >>>>> the charge is exhausted. Power diodes do that in Spice, too. >>>> >>>>>> This is interesting: >>>> >>>>>> https://dl.dropboxusercontent.com/u/53724080/Diode_TurnOn/1N914_Spice.jpg >>>> >>>>>> https://dl.dropboxusercontent.com/u/53724080/Diode_TurnOn/1N914_d.JPG >>>> >>>>>> Spice has no turn-on delay and gets the reverse charge wrong by maybe >>>>>> 3:1 or so. Could be worse, I guess. >>>> >>>>> .MODEL D1N914 d(is=100f Rs=2 CJO=10p Tt=4n Bv=100 ) >>>> >>>>> I had a play with the model values. The above gives a much better match to >>>>> your oscilloscope graph than the LTSpice version. The LTSpice graph shows >>>>> excessive delay in turn off. The CJO here is larger than stock, but gives >>>>> a >>>>> more rounded turn off like the measurement. Turn on overshoot is not >>>>> modelled. >>>> >>>>> TT is the key parameter to set diffusion capacitance. >>>> >>>> Now that I have actually checked the dc response with a data sheet, >>>> er...ahh... >>>> >>>> .MODEL D1N914 d(is=4n N=1.9 Rs=0.5 CJO=2p Tt=4n Bv=100 ) >>>> >>>> Is quite a good fit. Note the lack of the many digits of precision that are >>>> usually worthless and attempt to give the user a false sense of security. >>>> >>>> Teaser: >>>> >>>> To get N, first use any "is", from the data sheet, measure the Vbe >>>> difference difference from any decade change in current, in the lower >>>> current region. N=(delta Vbe)/60mv >>>> >>>> Why? >>>> >>>>> Then set "is" by trial and error on simulation runs of V against I at one >>>>> low current point. Set R from one high current point. >>>> >>>>> Oh... I found a tutorial on turn on time. The equation is >>>> >>>>> V = Vt.ln(1 + If/Io(1-exp(-t/tp))) >>> >>> >>> >>>> Thanks, Kevin. >>> >>>> In this particular application, I don't care about turn-on time, as I >>>> have microseconds to forward bias my diode. I do care about being able >>>> to control the amount of stored charge, and I somewhat care about the >>>> nature of the turn-off; LT Spice seems to treat diodes as SRDs, >>>> snapping off when the charge is used up. Real power diodes have softer >>>> turnoff, especially high voltage ones. >>> >>>> I have a ton of annoying stuff to do this week, so I'll have to wait >>>> for the weekend at least to play with your stuff. >>> >>>> Our potential customer is playing the increasingly common >>>> big-company-pummels-little-company game, wanting to own everything and >>>> make us do "open costing" to guarantee that we'll lose money. We may >>>> just tell them to drop dead. >>> >>>> If P.C. gets rational and lets us do this, I may just hire someone to >>>> find us a diode and make a good model of it. >>> >>> >>> It is interesting that the most basic semiconductor, is actually quite >>> complex. On the surface,it would seem that an inductor in series would model >>> the increase in voltage during turn on, which it does, but it messes up the >>> turn off waveform. It looks like it needs to be a nonlinear inductor with >>> other stuff. It will have to wait till the weekend though. >>> >>> >>> Kevin Aylward >>> www.kevinaylward.co.uk >>> www.anasoft.co.uk - SuperSpice >> >> >> Here are four cases: >> >> https://dl.dropboxusercontent.com/u/53724080/Diode_TurnOn/1N914_a.JPG >> >> https://dl.dropboxusercontent.com/u/53724080/Diode_TurnOn/1N914_b.JPG >> >> https://dl.dropboxusercontent.com/u/53724080/Diode_TurnOn/1N914_c.JPG >> >> https://dl.dropboxusercontent.com/u/53724080/Diode_TurnOn/1N914_d.JPG >> >> >> The overshoot areas are sorta similar. >> >> Even more fun is the DSRD (Grekhov drift step-recovery diode) power >> diode effect, where the time of forward bias affects the amount and >> especially the distribution of charge. We biased one diode to +48 >> volts for a couple of hundred ns, then reverse biased it at about 100 >> amps, and then it snapped, giving us a 2KV, 3 ns pulse. It wouldn't >> snap off fast if the forward bias had been DC. >> >> HP discovered, in the 1960's, that an SRD snaps off faster if the >> forward bias is only applied for a few ns. >> >> > >ISTM that it's intrinsically hard to model carrier diffusion problems in >SPICE, because SPICE is an ODE solver, and diffusion is a transport >problem. > >Transport problems require integral equations, which in general aren't >reducible to systems of ODEs. > >It's pretty reasonable that the turn-off behaviour would be a function >of how long the forward bias is applied--you want a nice sharp front >edge to the carrier distribution, so that the edge arrives back at the >contact all at once. The distribution gets flatter and flatter as time >goes on. > >Cheers > >Phil Hobbs
The miniority carries are getting in the way, you'd need software, maybe MicrowaveOffice, to model those effects that really affect microwave design. Maybe John needs a high voltage tunnel diode. Cheers
Kevin Aylward wrote:
> "John Larkin" wrote in message > news:59eu0a521ld1frmg2596rrpbtksg65mgdj@4ax.com... > > On Tue, 9 Sep 2014 18:21:33 +0100, "Kevin Aylward" > <ExtractkevinRemove@kevinaylward.co.uk> wrote: > >> "Kevin Aylward" wrote in message >> news:wcydnUoc3IdqdZDJnZ2dnUVZ7rWdnZ2d@bt.com... >> >>> "John Larkin" wrote in message >>> news:du7p0ad9fmfik7f8utc9e419paiklu6uod@4ax.com... >> >>> Playing with the standard 1N914 in LT Spice, it shows no forward >>> recovery (ie, no turn-on delay). It does store reverse charge, but it >>> snaps off instantly, probably just junction capacitance limited, when >>> the charge is exhausted. Power diodes do that in Spice, too. >> >>>> This is interesting: >> >>>> https://dl.dropboxusercontent.com/u/53724080/Diode_TurnOn/1N914_Spice.jpg >>>> >> >>>> https://dl.dropboxusercontent.com/u/53724080/Diode_TurnOn/1N914_d.JPG >> >>>> Spice has no turn-on delay and gets the reverse charge wrong by maybe >>>> 3:1 or so. Could be worse, I guess. >> >>> .MODEL D1N914 d(is=100f Rs=2 CJO=10p Tt=4n Bv=100 ) >> >>> I had a play with the model values. The above gives a much better >>> match to >>> your oscilloscope graph than the LTSpice version. The LTSpice graph >>> shows >>> excessive delay in turn off. The CJO here is larger than stock, but >>> gives a >>> more rounded turn off like the measurement. Turn on overshoot is not >>> modelled. >> >>> TT is the key parameter to set diffusion capacitance. >> >> Now that I have actually checked the dc response with a data sheet, >> er...ahh... >> >> .MODEL D1N914 d(is=4n N=1.9 Rs=0.5 CJO=2p Tt=4n Bv=100 ) >> >> Is quite a good fit. Note the lack of the many digits of precision >> that are >> usually worthless and attempt to give the user a false sense of security. >> >> Teaser: >> >> To get N, first use any "is", from the data sheet, measure the Vbe >> difference difference from any decade change in current, in the lower >> current region. N=(delta Vbe)/60mv >> >> Why? >> >>> Then set "is" by trial and error on simulation runs of V against I at >>> one >>> low current point. Set R from one high current point. >> >>> Oh... I found a tutorial on turn on time. The equation is >> >>> V = Vt.ln(1 + If/Io(1-exp(-t/tp))) > > > >> Thanks, Kevin. > >> In this particular application, I don't care about turn-on time, as I >> have microseconds to forward bias my diode. I do care about being able >> to control the amount of stored charge, and I somewhat care about the >> nature of the turn-off; LT Spice seems to treat diodes as SRDs, >> snapping off when the charge is used up. Real power diodes have softer >> turnoff, especially high voltage ones. > >> I have a ton of annoying stuff to do this week, so I'll have to wait >> for the weekend at least to play with your stuff. > >> Our potential customer is playing the increasingly common >> big-company-pummels-little-company game, wanting to own everything and >> make us do "open costing" to guarantee that we'll lose money. We may >> just tell them to drop dead. > >> If P.C. gets rational and lets us do this, I may just hire someone to >> find us a diode and make a good model of it. > > > It is interesting that the most basic semiconductor, is actually quite > complex. On the surface,it would seem that an inductor in series would > model the increase in voltage during turn on, which it does, but it > messes up the turn off waveform. It looks like it needs to be a > nonlinear inductor with other stuff. It will have to wait till the > weekend though.
* I think use of a linear inductor with nonlinear series resistor,that combo in parallel with another nonlinear resistor. That might be a simplified first cut..
> > > Kevin Aylward > www.kevinaylward.co.uk > www.anasoft.co.uk - SuperSpice
"Phil Hobbs"  wrote in message news:5411BB67.4040201@electrooptical.net...


> > The overshoot areas are sorta similar. > >> Even more fun is the DSRD (Grekhov drift step-recovery diode) power >> diode effect, where the time of forward bias affects the amount and >> especially the distribution of charge. We biased one diode to +48 >> volts for a couple of hundred ns, then reverse biased it at about 100 >> amps, and then it snapped, giving us a 2KV, 3 ns pulse. It wouldn't >> snap off fast if the forward bias had been DC. > > HP discovered, in the 1960's, that an SRD snaps off faster if the >> forward bias is only applied for a few ns. > >
>ISTM that it's intrinsically hard to model carrier diffusion problems in >SPICE, because SPICE is an ODE solver, and diffusion is a transport >problem. >Transport problems require integral equations, which in general aren't >reducible to systems of ODEs.
Sure, many integral equations cannot be solved as a differential equation, but I don't see that as being relevant to a Spice simulation being restricted to solving nonlinear ODEs. In principal, Spice does not solve the internal device equations that might be produced by an integral equation, it just takes the already solved internal device equations and solves an external set of equations. Ok, in practice, the internal equations may be transcendental, and these get solved in the wash of the external solution so that the internal equations sort of get solved by Spice, but it doesn't change the principle. Spice and reality only care about an I = f(V,t) at the device terminals, as a black box. It doesn't care how that relation was generated, be it solving a partial differential diffusion equation, or some 3D integral transport equation. The device physics don't even need to be solved at all. I=f(V,t) can be determined from running lots of measurements. Indeed, that's how individuals like Jim T,and I, that lack extensive semiconductor physics and the time, actually get somewhat reasonable models. We piss about with simulation graphs until we get a match. Kevin Aylward www.kevinaylward.co.uk www.anasoft.co.uk - SuperSpice
On Fri, 12 Sep 2014 14:24:32 +0100, "Kevin Aylward"
<ExtractkevinRemove@kevinaylward.co.uk> wrote:

>"Phil Hobbs" wrote in message news:5411BB67.4040201@electrooptical.net... > > >> >> The overshoot areas are sorta similar. >> >>> Even more fun is the DSRD (Grekhov drift step-recovery diode) power >>> diode effect, where the time of forward bias affects the amount and >>> especially the distribution of charge. We biased one diode to +48 >>> volts for a couple of hundred ns, then reverse biased it at about 100 >>> amps, and then it snapped, giving us a 2KV, 3 ns pulse. It wouldn't >>> snap off fast if the forward bias had been DC. >> >> HP discovered, in the 1960's, that an SRD snaps off faster if the >>> forward bias is only applied for a few ns. >> >> > >>ISTM that it's intrinsically hard to model carrier diffusion problems in >>SPICE, because SPICE is an ODE solver, and diffusion is a transport >>problem. >>Transport problems require integral equations, which in general aren't >>reducible to systems of ODEs. > >Sure, many integral equations cannot be solved as a differential equation, >but I don't see that as being relevant to a Spice simulation being >restricted to solving nonlinear ODEs. > >In principal, Spice does not solve the internal device equations that might >be produced by an integral equation, it just takes the already solved >internal device equations and solves an external set of equations. Ok, in >practice, the internal equations may be transcendental, and these get solved >in the wash of the external solution so that the internal equations sort of >get solved by Spice, but it doesn't change the principle. > >Spice and reality only care about an I = f(V,t) at the device terminals, as >a black box. It doesn't care how that relation was generated, be it solving >a partial differential diffusion equation, or some 3D integral transport >equation. The device physics don't even need to be solved at all. I=f(V,t) >can be determined from running lots of measurements. Indeed, that's how >individuals like Jim T,and I, that lack extensive semiconductor physics and >the time, actually get somewhat reasonable models. We piss about with >simulation graphs until we get a match. > > >Kevin Aylward >www.kevinaylward.co.uk >www.anasoft.co.uk - SuperSpice
Once upon a time (like 50 or more years ago) I had all that semiconductor physics course-work... but it promptly faded away from disuse >:-} And a whole lot of physical phenomena have direct analogs from circuit elements... easing the pain of making subcircuits that match what you can measure. Diode reverse recovery modeling actually looks to be a piece-a-cake. ...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 Thu, 11 Sep 2014 21:48:16 -0700, Robert Baer
<robertbaer@localnet.com> wrote:

>Kevin Aylward wrote:
[snip]
>> >> >> It is interesting that the most basic semiconductor, is actually quite >> complex. On the surface,it would seem that an inductor in series would >> model the increase in voltage during turn on, which it does, but it >> messes up the turn off waveform. It looks like it needs to be a >> nonlinear inductor with other stuff. It will have to wait till the >> weekend though. >> >> Kevin Aylward >> www.kevinaylward.co.uk >> www.anasoft.co.uk - SuperSpice
>* I think use of a linear inductor with nonlinear series resistor,that >combo in parallel with another nonlinear resistor. > That might be a simplified first cut..
That's sort of like a solution in a paper I ran across. But I think I've found an even better way. (The non-linear resistor scheme is better-suited to modeling the electrical behavior of B-H core behavior.) ...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 09/12/2014 09:24 AM, Kevin Aylward wrote:
> "Phil Hobbs" wrote in message news:5411BB67.4040201@electrooptical.net... > > >> >> The overshoot areas are sorta similar. >> >>> Even more fun is the DSRD (Grekhov drift step-recovery diode) power >>> diode effect, where the time of forward bias affects the amount and >>> especially the distribution of charge. We biased one diode to +48 >>> volts for a couple of hundred ns, then reverse biased it at about 100 >>> amps, and then it snapped, giving us a 2KV, 3 ns pulse. It wouldn't >>> snap off fast if the forward bias had been DC. >> >> HP discovered, in the 1960's, that an SRD snaps off faster if the >>> forward bias is only applied for a few ns. >> >> > >> ISTM that it's intrinsically hard to model carrier diffusion problems >> in SPICE, because SPICE is an ODE solver, and diffusion is a transport >> problem. >> Transport problems require integral equations, which in general aren't >> reducible to systems of ODEs. > > Sure, many integral equations cannot be solved as a differential > equation, but I don't see that as being relevant to a Spice simulation > being restricted to solving nonlinear ODEs. > > In principal, Spice does not solve the internal device equations that > might be produced by an integral equation, it just takes the already > solved internal device equations and solves an external set of > equations. Ok, in practice, the internal equations may be > transcendental, and these get solved in the wash of the external > solution so that the internal equations sort of get solved by Spice, but > it doesn't change the principle. > > Spice and reality only care about an I = f(V,t) at the device terminals, > as a black box. It doesn't care how that relation was generated, be it > solving a partial differential diffusion equation, or some 3D integral > transport equation. The device physics don't even need to be solved at > all. I=f(V,t) can be determined from running lots of measurements. > Indeed, that's how individuals like Jim T,and I, that lack extensive > semiconductor physics and the time, actually get somewhat reasonable > models. We piss about with simulation graphs until we get a match.
You can't reduce a transport problem to a set of ODEs. I'm sure you can cobble something together that will agree to any accuracy you care to stop at, but it's just that, cobbled together. I'm not proposing using a Boltzmann equation solver to model circuits, just observing that carrier-diffusion dynamics aren't very well suited to the tool, so you'll probably have to cobble quite a bit harder than for, say, a varactor. 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, 12 Sep 2014 11:41:50 -0400, Phil Hobbs
<pcdhSpamMeSenseless@electrooptical.net> wrote:

>On 09/12/2014 09:24 AM, Kevin Aylward wrote: >> "Phil Hobbs" wrote in message news:5411BB67.4040201@electrooptical.net... >> >> >>> >>> The overshoot areas are sorta similar. >>> >>>> Even more fun is the DSRD (Grekhov drift step-recovery diode) power >>>> diode effect, where the time of forward bias affects the amount and >>>> especially the distribution of charge. We biased one diode to +48 >>>> volts for a couple of hundred ns, then reverse biased it at about 100 >>>> amps, and then it snapped, giving us a 2KV, 3 ns pulse. It wouldn't >>>> snap off fast if the forward bias had been DC. >>> >>> HP discovered, in the 1960's, that an SRD snaps off faster if the >>>> forward bias is only applied for a few ns. >>> >>> >> >>> ISTM that it's intrinsically hard to model carrier diffusion problems >>> in SPICE, because SPICE is an ODE solver, and diffusion is a transport >>> problem. >>> Transport problems require integral equations, which in general aren't >>> reducible to systems of ODEs. >> >> Sure, many integral equations cannot be solved as a differential >> equation, but I don't see that as being relevant to a Spice simulation >> being restricted to solving nonlinear ODEs. >> >> In principal, Spice does not solve the internal device equations that >> might be produced by an integral equation, it just takes the already >> solved internal device equations and solves an external set of >> equations. Ok, in practice, the internal equations may be >> transcendental, and these get solved in the wash of the external >> solution so that the internal equations sort of get solved by Spice, but >> it doesn't change the principle. >> >> Spice and reality only care about an I = f(V,t) at the device terminals, >> as a black box. It doesn't care how that relation was generated, be it >> solving a partial differential diffusion equation, or some 3D integral >> transport equation. The device physics don't even need to be solved at >> all. I=f(V,t) can be determined from running lots of measurements. >> Indeed, that's how individuals like Jim T,and I, that lack extensive >> semiconductor physics and the time, actually get somewhat reasonable >> models. We piss about with simulation graphs until we get a match. > >You can't reduce a transport problem to a set of ODEs. I'm sure you can >cobble something together that will agree to any accuracy you care to >stop at, but it's just that, cobbled together.
Spice is about modeling real-world phenomena... not writing a paper for some highfalutin physics society, all wrapped-up in narcissism
>:-}
> >I'm not proposing using a Boltzmann equation solver to model circuits, >just observing that carrier-diffusion dynamics aren't very well suited >to the tool, so you'll probably have to cobble quite a bit harder than >for, say, a varactor. > >Cheers > >Phil Hobbs
Naaaah! Watch me! ...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 09/12/2014 11:54 AM, Jim Thompson wrote:
> On Fri, 12 Sep 2014 11:41:50 -0400, Phil Hobbs > <pcdhSpamMeSenseless@electrooptical.net> wrote: > >> On 09/12/2014 09:24 AM, Kevin Aylward wrote: >>> "Phil Hobbs" wrote in message news:5411BB67.4040201@electrooptical.net... >>> >>> >>>> >>>> The overshoot areas are sorta similar. >>>> >>>>> Even more fun is the DSRD (Grekhov drift step-recovery diode) power >>>>> diode effect, where the time of forward bias affects the amount and >>>>> especially the distribution of charge. We biased one diode to +48 >>>>> volts for a couple of hundred ns, then reverse biased it at about 100 >>>>> amps, and then it snapped, giving us a 2KV, 3 ns pulse. It wouldn't >>>>> snap off fast if the forward bias had been DC. >>>> >>>> HP discovered, in the 1960's, that an SRD snaps off faster if the >>>>> forward bias is only applied for a few ns. >>>> >>>> >>> >>>> ISTM that it's intrinsically hard to model carrier diffusion problems >>>> in SPICE, because SPICE is an ODE solver, and diffusion is a transport >>>> problem. >>>> Transport problems require integral equations, which in general aren't >>>> reducible to systems of ODEs. >>> >>> Sure, many integral equations cannot be solved as a differential >>> equation, but I don't see that as being relevant to a Spice simulation >>> being restricted to solving nonlinear ODEs. >>> >>> In principal, Spice does not solve the internal device equations that >>> might be produced by an integral equation, it just takes the already >>> solved internal device equations and solves an external set of >>> equations. Ok, in practice, the internal equations may be >>> transcendental, and these get solved in the wash of the external >>> solution so that the internal equations sort of get solved by Spice, but >>> it doesn't change the principle. >>> >>> Spice and reality only care about an I = f(V,t) at the device terminals, >>> as a black box. It doesn't care how that relation was generated, be it >>> solving a partial differential diffusion equation, or some 3D integral >>> transport equation. The device physics don't even need to be solved at >>> all. I=f(V,t) can be determined from running lots of measurements. >>> Indeed, that's how individuals like Jim T,and I, that lack extensive >>> semiconductor physics and the time, actually get somewhat reasonable >>> models. We piss about with simulation graphs until we get a match. >> >> You can't reduce a transport problem to a set of ODEs. I'm sure you can >> cobble something together that will agree to any accuracy you care to >> stop at, but it's just that, cobbled together. > > Spice is about modeling real-world phenomena... not writing a paper > for some highfalutin physics society, all wrapped-up in narcissism >> :-}
In other words you don't actually know how it works. ;)
> >> >> I'm not proposing using a Boltzmann equation solver to model circuits, >> just observing that carrier-diffusion dynamics aren't very well suited >> to the tool, so you'll probably have to cobble quite a bit harder than >> for, say, a varactor. >> >> Cheers >> >> Phil Hobbs > > Naaaah! Watch me! > > ...Jim Thompson >
If you can model a Grekhov diode successfully in SPICE, my hat will be off to you, sir. 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, 12 Sep 2014 14:03:02 -0400, Phil Hobbs
<pcdhSpamMeSenseless@electrooptical.net> wrote:

>On 09/12/2014 11:54 AM, Jim Thompson wrote: >> On Fri, 12 Sep 2014 11:41:50 -0400, Phil Hobbs >> <pcdhSpamMeSenseless@electrooptical.net> wrote: >> >>> On 09/12/2014 09:24 AM, Kevin Aylward wrote: >>>> "Phil Hobbs" wrote in message news:5411BB67.4040201@electrooptical.net... >>>> >>>> >>>>> >>>>> The overshoot areas are sorta similar. >>>>> >>>>>> Even more fun is the DSRD (Grekhov drift step-recovery diode) power >>>>>> diode effect, where the time of forward bias affects the amount and >>>>>> especially the distribution of charge. We biased one diode to +48 >>>>>> volts for a couple of hundred ns, then reverse biased it at about 100 >>>>>> amps, and then it snapped, giving us a 2KV, 3 ns pulse. It wouldn't >>>>>> snap off fast if the forward bias had been DC. >>>>> >>>>> HP discovered, in the 1960's, that an SRD snaps off faster if the >>>>>> forward bias is only applied for a few ns. >>>>> >>>>> >>>> >>>>> ISTM that it's intrinsically hard to model carrier diffusion problems >>>>> in SPICE, because SPICE is an ODE solver, and diffusion is a transport >>>>> problem. >>>>> Transport problems require integral equations, which in general aren't >>>>> reducible to systems of ODEs. >>>> >>>> Sure, many integral equations cannot be solved as a differential >>>> equation, but I don't see that as being relevant to a Spice simulation >>>> being restricted to solving nonlinear ODEs. >>>> >>>> In principal, Spice does not solve the internal device equations that >>>> might be produced by an integral equation, it just takes the already >>>> solved internal device equations and solves an external set of >>>> equations. Ok, in practice, the internal equations may be >>>> transcendental, and these get solved in the wash of the external >>>> solution so that the internal equations sort of get solved by Spice, but >>>> it doesn't change the principle. >>>> >>>> Spice and reality only care about an I = f(V,t) at the device terminals, >>>> as a black box. It doesn't care how that relation was generated, be it >>>> solving a partial differential diffusion equation, or some 3D integral >>>> transport equation. The device physics don't even need to be solved at >>>> all. I=f(V,t) can be determined from running lots of measurements. >>>> Indeed, that's how individuals like Jim T,and I, that lack extensive >>>> semiconductor physics and the time, actually get somewhat reasonable >>>> models. We piss about with simulation graphs until we get a match. >>> >>> You can't reduce a transport problem to a set of ODEs. I'm sure you can >>> cobble something together that will agree to any accuracy you care to >>> stop at, but it's just that, cobbled together. >> >> Spice is about modeling real-world phenomena... not writing a paper >> for some highfalutin physics society, all wrapped-up in narcissism >>> :-} > >In other words you don't actually know how it works. ;)
Actually, as I pointed out earlier, I was schooled in semiconductor physics via Al Phillips... <http://www.semiconductormuseum.com/Transistors/Motorola/Haenichen/Haenichen_Page3.htm> and Warner et al texts, so I know how it works. (I joined that group in June 1962.) Good behavioral models create the waveform responses is ways much simpler than trying to compose the device physics into the model.
>> >>> >>> I'm not proposing using a Boltzmann equation solver to model circuits, >>> just observing that carrier-diffusion dynamics aren't very well suited >>> to the tool, so you'll probably have to cobble quite a bit harder than >>> for, say, a varactor. >>> >>> Cheers >>> >>> Phil Hobbs >> >> Naaaah! Watch me! >> >> ...Jim Thompson >> > >If you can model a Grekhov diode successfully in SPICE, my hat will be >off to you, sir. > >Cheers > >Phil Hobbs
I don't even know what a Grekhov diode is :-[ But I'll look it up. ...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.