Forums

diode recovered charge

Started by John Larkin September 6, 2014
On 09/12/2014 02:31 PM, Jim Thompson wrote:
> 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.)
I mean SPICE, not semiconductors. "Modeling real-world phenomena" works better if you understand what's going on under the hood, IME.
> > Good behavioral models create the waveform responses is ways much > simpler than trying to compose the device physics into the model. >
Sure, just like other sorts of curve fitting. The problem is when you reach the limits of the data set used to make the fit. A physics-based model can avoid that limitation, provided of course that the physics is well-enough understood.
>>> >>>> >>>> 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 >
You're in for a treat. Grekhov & Co. figured out how to make certain types of power rectifiers into SRDs--picture a 3 kV, subnanosecond pulse into 50 ohms from the equivalent of a 1N4007. John L described one that he made earlier in the thread. Cheers Phil -- 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. ;)
Since Spice doesn't do diffusion, maybe one could model a diode as several different diodes strung out on a lumped transmission line, namely coupled with inductors. Sort of like a shock line but accesses at just one end. Longer forward-bias times would pump charge into diodes farther along the line, recovery ditto. -- John Larkin Highland Technology, Inc jlarkin att highlandtechnology dott com http://www.highlandtechnology.com
On 09/12/2014 02:54 PM, John Larkin wrote:
> 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. ;) > > > Since Spice doesn't do diffusion, maybe one could model a diode as > several different diodes strung out on a lumped transmission line, > namely coupled with inductors. Sort of like a shock line but accesses > at just one end. Longer forward-bias times would pump charge into > diodes farther along the line, recovery ditto. > >
Some sort of nonlinear RL transmission line might work too, but that's an awful lot of cobbling. 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
"Jim Thompson"  wrote in message 
news:bc361a52up1qnosrpblnoaod24gpiskk5t@4ax.com...

On Thu, 11 Sep 2014 21:48:16 -0700, Robert Baer
<robertbaer@localnet.com> wrote:

>* 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.)
I was going say something about this in my last post...because it s one of those spicy exception exceptions. Actually, continuous DC hysteresis is not something Spice3 can really handle. If a value that changes dependant on time is involved, L and C might be an approach, but for DC an additional ingredient is needed as spice doesn't know how to deal with multivalued functions. DC hysteresis doesn't care when the last value occurred in order to determine the next value, only what the last value was. Essentially, a mem-resistor function in needed. However... 10 or so years ago I implemented the hysteresis function that Mike put into LTSpice, into SuperSpice. This works by way of a "core" component that is a DC component, but forms the actual hysteresis bit. For example, if you voltage drive the core with a DC sine wave (say by driving a dc sweep into a sine function), the output current will not be the same on same periodic points of the input sine. So, in principle, one could wrap other non-linear functions around the "core" to produce a variety of different DC hysteresis characteristics. Kevin Aylward www.kevinaylward.co.uk www.anasoft.co.uk - SuperSpice
"Phil Hobbs"  wrote in message 
news:F_qdnZfVAvejiY7JnZ2dnUU7-IudnZ2d@supernews.com...

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 agreed with that point. I don't agree that it really mattes in spice . A set of graphs of i against time and volts simply does not care what the underlying physics is.
> 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 disagree with the implied meaning of "cobbled together". Behaverial black box, modelling is a well tried and trusted method of getting results when the detail are intractable.
>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.
I disagree, as I noted, the final result of a model is simple an i=f(v,t) function. Kevin Aylward www.kevinaylward.co.uk www.anasoft.co.uk - SuperSpice
"Jim Thompson"  wrote in message 
news:70361alm3d6euf88it447qe0ffk7v72e39@4ax.com...

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.
>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 >:-}
30 years ago I went through the sums of the diffusion equation to show that there was a small signal capacitance proportional to dc current, but that was 30 years ago... The overall concept of C=k.I is actually important in understanding why Cbe= gm/2.pi.ft allows for an approximate contestant Ft parameter in the bipolar model for a wide range of currents
>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.
The basic diode tt isn't that far off in many cases. Just needs some extra tweaking around it. Kevin Aylward www.kevinaylward.co.uk www.anasoft.co.uk - SuperSpice
On 09/12/2014 03:59 PM, Kevin Aylward wrote:
> "Phil Hobbs" wrote in message > news:F_qdnZfVAvejiY7JnZ2dnUU7-IudnZ2d@supernews.com... > > 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 agreed with that point. I don't agree that it really mattes in spice . > A set of graphs of i against time and volts simply does not care what > the underlying physics is. > >> 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 disagree with the implied meaning of "cobbled together". Behaverial > black box, modelling is a well tried and trusted method of getting > results when the detail are intractable. > >> 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. > > I disagree, as I noted, the final result of a model is simple an > i=f(v,t) function. > > Kevin Aylward > www.kevinaylward.co.uk > www.anasoft.co.uk - SuperSpice
If you can get the full range of behaviour of a Grekhov diode using that approach, you have my admiration. My hunch is that the smart money would bet the other way. 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 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] None of the ordinary Spice variants seem to model forward and reverse recovery time. Can you provide some scope photos of forward and reverse recovery at different current levels? Several papers I've run across suggest that a fairly simple subcircuit may be possible... but, being IEEE crap, their data is naive and vague
>:-}
...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 Sun, 14 Sep 2014 12:44:19 -0700, Jim Thompson
<To-Email-Use-The-Envelope-Icon@On-My-Web-Site.com> wrote:

>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] > >None of the ordinary Spice variants seem to model forward and reverse >recovery time. > >Can you provide some scope photos of forward and reverse recovery at >different current levels? > >Several papers I've run across suggest that a fairly simple subcircuit >may be possible... but, being IEEE crap, their data is naive and vague >>:-} > > ...Jim Thompson
I posted some 1N914 pics, taken at four different current step levels. Looks sorta like constant-area overshoot. Forward recovery doesn't matter in my current application, since I'll have plenty of time to pump current into my diodes. Controlling the amount of reverse charge matters, and I need to simulate reverse recovery accurately in the higher-level simulation. -- John Larkin Highland Technology, Inc jlarkin att highlandtechnology dott com http://www.highlandtechnology.com
On Sun, 14 Sep 2014 12:53:09 -0700, John Larkin
<jlarkin@highlandtechnology.com> wrote:

>On Sun, 14 Sep 2014 12:44:19 -0700, Jim Thompson ><To-Email-Use-The-Envelope-Icon@On-My-Web-Site.com> wrote: > >>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] >> >>None of the ordinary Spice variants seem to model forward and reverse >>recovery time. >> >>Can you provide some scope photos of forward and reverse recovery at >>different current levels? >> >>Several papers I've run across suggest that a fairly simple subcircuit >>may be possible... but, being IEEE crap, their data is naive and vague >>>:-} >> >> ...Jim Thompson > >I posted some 1N914 pics, taken at four different current step levels.
I saw those but couldn't determine the current levels... that green drives my eyes nuts.
> >Looks sorta like constant-area overshoot. > >Forward recovery doesn't matter in my current application, since I'll >have plenty of time to pump current into my diodes. Controlling the >amount of reverse charge matters, and I need to simulate reverse >recovery accurately in the higher-level simulation.
...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.