1. Home
  2. Electronics Design
  3. diode recovered charge

diode recovered charge

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.

Version 4 SHEET 1 1104 680 WIRE 128 80 16 80 WIRE 336 80 208 80 WIRE 336 112 336 80 WIRE 16 128 16 80 WIRE 336 224 336 176 WIRE 416 224 336 224 WIRE 640 224 496 224 WIRE 784 224 640 224 WIRE 944 224 784 224 WIRE 1008 224 944 224 WIRE 1056 224 1008 224 WIRE 16 256 16 208 WIRE 336 256 336 224 WIRE 496 256 496 224 WIRE 416 272 416 224 WIRE 448 272 416 272 WIRE 640 272 640 224 WIRE 784 272 784 224 WIRE 944 288 944 224 WIRE 448 320 416 320 WIRE 336 368 336 336 WIRE 416 368 416 320 WIRE 416 368 336 368 WIRE 336 400 336 368 WIRE 496 400 496 336 WIRE 640 400 640 336 WIRE 784 400 784 352 WIRE 944 400 944 352 FLAG 16 256 0 FLAG 336 400 0 FLAG 496 400 0 FLAG 640 400 0 FLAG 784 400 0 FLAG 944 400 0 FLAG 1008 224 Qd_nC SYMBOL diode 352 176 R180 WINDOW 0 -69 44 Left 2 WINDOW 3 -84 14 Left 2 SYMATTR InstName D1 SYMATTR Value ES1D SYMBOL voltage 16 112 R0 WINDOW 0 51 57 Left 2 WINDOW 3 -16 -79 Left 2 WINDOW 123 0 0 Left 2 WINDOW 39 0 0 Left 2 SYMATTR InstName V1 SYMATTR Value PULSE(-10 100 10u 5n 5n 20u) SYMBOL res 112 96 R270 WINDOW 0 -45 58 VTop 2 WINDOW 3 -53 57 VBottom 2 SYMATTR InstName R1 SYMATTR Value 1 SYMBOL res 320 240 R0 WINDOW 0 -76 43 Left 2 WINDOW 3 -79 78 Left 2 SYMATTR InstName R2 SYMATTR Value 1m SYMBOL g 496 240 R0 WINDOW 0 46 61 Left 2 WINDOW 3 23 107 Left 2 SYMATTR InstName G1 SYMATTR Value 1000 SYMBOL cap 624 272 R0 WINDOW 0 57 22 Left 2 WINDOW 3 62 54 Left 2 SYMATTR InstName C1 SYMATTR Value 1n SYMBOL res 768 256 R0 WINDOW 0 56 40 Left 2 WINDOW 3 60 70 Left 2 SYMATTR InstName R3 SYMATTR Value 1g SYMBOL diode 960 352 R180 WINDOW 0 -53 48 Left 2 WINDOW 3 -55 17 Left 2 SYMATTR InstName D2 SYMATTR Value Dx TEXT 664 112 Left 2 !.tran 25u TEXT 600 64 Left 2 !.model DX D(Vfwd=0) TEXT 552 -32 Left 2 ;Diode Reverse Charge Tester TEXT 592 16 Left 2 ;J Larkin Sep 6, 2014 TEXT 936 176 Left 2 ;1 volt per nC

--

John Larkin         Highland Technology, Inc 

jlarkin att highlandtechnology dott com 
http://www.highlandtechnology.com
Reply to
John Larkin
Loading thread data ...

Adding UIC to the transient analysis does make Qrr depend on Ton, but not much.

--

John Larkin         Highland Technology, Inc 

jlarkin att highlandtechnology dott com 
http://www.highlandtechnology.com
Reply to
John Larkin

SPICE is notoriously bad at reverse recovery. I've heard of some models which claim to produce realistic results, but not seen.

Probably would help with transistors too. I typically see circuits going about 1/2 to 1/3 as fast as SPICE would claim.

Tim

-- Seven Transistor Labs Electrical Engineering Consultation Website:

formatting link

Reply to
Tim Williams

which claim to produce realistic results, but not seen.

about 1/2 to 1/3 as fast as SPICE would claim.

The transistor models that you get with LTSpice and from manufacturers are Gummel-Poon models.

What the manufacturers use in-house, are VBIC models, which LTSpice can run if you can find the parameters. The manufacturers won't give them to you - they are commercial-in-confidence. You could - in theory - work them out f or yourself, but I've never seen any actual VBIC model parameters for a rea l transistor.

formatting link

I raised this point here, a few years ago, when I was trying to get an LTSp ice model of a Baxandall class-D oscillator built with bipolar transistors to "squeg" with a relatively high feed inductance.

The simulations I ran made it fairly clear that it was something about the operation of a bipolar transistor in inverted mode (using the emitter as if it were a collector and the collector as if it were an emitter) that produ ced "squegging" but equally that the Gummell-Poon model didn't capture that particular behavior, because my LTSpice circuits always settled down to un iform oscillation where the real circuits had never settled down to a const ant amplitude oscillation.

--
Bill Sloman, Sydney
Reply to
Bill Sloman

Looks that way. I may have an application where an accurate power diode reverse recovery model really matters. We may wind up characterizing candidate diodes and then making some weird nonlinear capacitor behavioral model, nothing like a normal diode model.

--

John Larkin         Highland Technology, Inc 

jlarkin att highlandtechnology dott com 
http://www.highlandtechnology.com
Reply to
John Larkin

PIN diode Attenuator?

Cheers

Reply to
Martin Riddle

Come on, you heard it from Thompson. Spice has no charge issues. ;-)

Reply to
miso

I wish the Trr simulation were a bit better (I use LTspice) but I just exagerate the TT parameter and it seems to work "OK". I just thought I wasn't doing things right, but maybe it just doesn't work as good as it should ?

This is a very imporant issue for correct simulation IMO.

Seems most of my design problems are designing around all these defective parts ! :)

boB

Reply to
boB

No, a sort of nonlinear transmission line terminator, low impedance for smallish signals and high impedance for big ones. Kilovolts. We could do this with a series string of PN rectifier diodes, high-voltage PIN diodes, or maybe even Z5U nonlinear capacitors. But we'd need accurate models of whatever we use, to let us simulate the whole complex mess.

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:

formatting link

formatting link

Spice has no turn-on delay and gets the reverse charge wrong by maybe

3:1 or so. Could be worse, I guess.

That particular 1N914 makes a decent SRD, not as fast as the Spice model but still interesting.

Enough fun for now. Gotta go to Safeway.

--

John Larkin         Highland Technology, Inc 

jlarkin att highlandtechnology dott com 
http://www.highlandtechnology.com
Reply to
John Larkin

You might like to look at how Simetrix deal with this (they offer a node limited free version of their simulator).

Reply to
JM

oscillation.

Ltspice supports VBIC style. If you really tried to use your tools instead of blowing smoke, you'd know that.

Level 9 maybe a hint.

But you may need to supply a model card and that is more than likely is out side your scope.

Even if you did figure out how, it still would not make any improvements to that failed oscillator.

Jamie

Reply to
Maynard A. Philbrook Jr.

On Monday, 8 September 2014 11:33:26 UTC+10, Maynard A. Philbrook Jr. wrot e:

real transistor.

LTSpice model of a Baxandall class-D oscillator built with bipolar transist ors to "squeg" with a relatively high feed inductance.

the operation of a bipolar transistor in inverted mode (using the emitter a s if it were a collector and the collector as if it were an emitter) that p roduced "squegging" but equally that the Gummell-Poon model didn't capture that particular behavior, because my LTSpice circuits always settled down t o uniform oscillation where the real circuits had never settled down to a c onstant amplitude oscillation.

If your read all of what I posted, you'd be aware that I know that.

"What the manufacturers use in-house, are VBIC models, which LTSpice can ru n if you can find the parameters."

Snipping that bit of my post doesn't make it go away.

I did mention that I'd tried to get hold of a set of VBIC transistor parame ters, and I even spent some time seeing if I could fill in the numbers to get something that might be vaguely realistic, but it was indeed more than I could manage.

True. I'm not quite sure which oscillator you imagine has failed, but the q uestion I was addressing was why the bipolar version of the Baxandall Class

-D oscillator can squeg. Working out why this happens probably wouldn't imp rove the oscillator one iota - it works fine in areas where it's appropriat e (and has done since Baxandall first publicised it in 1959). The "squeggin g" is a trifle mysterious, but if you want to use a high value feed inducto r, you can avoid the "squegging" by using MOSFET switches (which weren't ar ound when Baxandall invented the circuit).

Congratulations on making a bigger prat of yourself than I'd have imagined possible, even for you.

--
Bill Sloman, Sydney
Reply to
Bill Sloman

For the analysis,dig out your Linvill (Transistors and active circuits).

Reply to
Robert Baer

Here is where Transistors and Active Circuits by Linvill will give the edge you are looking for..

Reply to
Robert Baer

.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.

Kevin Aylward

formatting link
formatting link
- SuperSpice

Reply to
Kevin Aylward

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)))

Kevin Aylward

formatting link
formatting link
- SuperSpice

Reply to
Kevin Aylward

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.

--

John Larkin         Highland Technology, Inc 

jlarkin att highlandtechnology dott com 
http://www.highlandtechnology.com
Reply to
John Larkin

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

formatting link
formatting link
- SuperSpice

Reply to
Kevin Aylward

Here are four cases:

formatting link

formatting link

formatting link

formatting link

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.

--

John Larkin         Highland Technology, Inc 

jlarkin att highlandtechnology dott com 
http://www.highlandtechnology.com
Reply to
John Larkin

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

--
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 to
Phil Hobbs

ElectronDepot website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.