IGBT Failure in BOOST Converter what may be the reasons?

i think your statement above is a bit implausible & sweeping.

Click to expand...

I'm aware of the possibility that you didn't fully understand it.

i tried to outline my calculations & the resulting inconsistency in #16

Click to expand...

I know, I appreciate the calculation. But what are you particularly asking?

If you are asking where the simulation error is, I suggested a solution. If we presume the simulator is calculating correct, the energy is lost in the transistor.

imo simulations help tremendously in understanding & experimenting.

Click to expand...

Basically yes. The shown simulation results are simply too vague for clear conclusions. The said diode current contradiction is the most obvious example for this problem, I think.

P.S.: To add a quantiative consideration, current fall time is about 3 us. Thus a few us transistor switching time are sufficient to get the observed 30 % efficiency. But without transistor and diode specifications and control waveforms, the assumption can't be further founded.

BradtheRad said:

Glad we've reached some kind of understanding.

Click to expand...

It's because the simulator sometimes displays oscillations during dead time. I believe it is tiny coil energy 'kicking' the diode open repeatedly each time the diode is full off.

By putting a resistor across the diode (or switching device), I find it eliminates the oscillations.

Click to expand...

I don't think thats it. This circuit has some steady state/ slow phenomena, but also some very sharp/ high-speed transients at work.

What you need to do is set the "Time Step Size" under Options--Other Options to a smaller value. Like 100nS or so, maybe less, and not the default 5uS. This will better capture & model the parameters during the firing of the diode.

You will find that your inductor current undershoot (ringing) disappears - you won't need the 20K anymore, and ALSO the diode peak current is the same as the inductor peak current, which it obviously HAS to be. Your earlier screenshot showed the diode peak as ~200mA, but this was clearly a time-averaged value of the pulse across the 5uS time step. Both these are artifacts of the larger time-step.

The simulation works perfectly once this is done.

And now - for my better understanding of this simulator - a couple of questions, if you still have your original setup:
1) what were the settings of the CLK you used ? Freq/Duty Cycle/ voltages/ offset ?
2) what was the BJT beta you used ? Was it the default 100?

What you need to do is set the "Time Step Size" under Options--Other Options to a smaller value. Like 100nS or so, maybe less, and not the default 5uS. This will better capture & model the parameters during the firing of the diode.

You will find that your inductor current undershoot (ringing) disappears - you won't need the 20K anymore, and ALSO the diode peak current is the same as the inductor peak current, which it obviously HAS to be. Your earlier screenshot showed the diode peak as ~200mA, but this was clearly a time-averaged value of the pulse across the 5uS time step. Both these are artifacts of the larger time-step.

The simulation works perfectly once this is done.

Click to expand...

Sounds plausible. Working with SPICE since V2.x, this behaviour of the Falstad simulator sounds pretty weird. Although tuning of the simulation time step in transient analysis can be necessary to improve accuracy, you won't see a completely wrong result like the present one with default settings. This supports my previous impression, that Falstad is probably good to visualize principle behaviour, e.g. how a boost converter works, but you shouldn't expect quantitative results. It's most likely able to get better results, but apparently it's not designed for quantitative simulations.

rohitkhanna said:

What you need to do is set the "Time Step Size" under Options--Other Options to a smaller value. Like 100nS or so, maybe less, and not the default 5uS. This will better capture & model the parameters during the firing of the diode.

Click to expand...

Yes, it is as you state. I didn't realize what that option does.

I should have experimented with it, because I have been baffled that a simulator as well put together as this one, doesn't seem to handle frequencies above 20 or 25 kHz. Now I find it can when I set a narrower time-step.

(Yet I notice it has transmission line simulations at frequencies in the GHz. The time-step is the key to making this possible. I see it says '1p' in the option field. 1 pico-second.)

This is progress. Thank you. I know I can use Falstad's simulator to greater effect now that I know about this.

You will find that your inductor current undershoot (ringing) disappears - you won't need the 20K anymore, and ALSO the diode peak current is the same as the inductor peak current, which it obviously HAS to be. Your earlier screenshot showed the diode peak as ~200mA, but this was clearly a time-averaged value of the pulse across the 5uS time step. Both these are artifacts of the larger time-step.

The simulation works perfectly once this is done.

Click to expand...

I was planning to go back to your post #16, and see if I could track down the root of the discrepancies you found.
Instead I believe you have taken care of it by setting a narrower time-step.

The diode now carries approximately the same current as the coil is discharging.

I should have caught the glaring discrepancy previously. I chalked it up to the 'wild card' nature of a coil as it discharges in these situations. It's a behavior that is difficult to model. So it seemed plausible that 1.7 A would have to be converted to 200mA in order to produce the high V needed to overcome the capacitor charge.

Also solved is the reverse flow back up through the coil, shown happening after the coil discharges (negative spike on the coil, post #9). There should be no way this would happen either in real life or the simulation. This has stopped once I set the time-step narrower.

I would have thought the simulator would flag such inconsistencies.

And now - for my better understanding of this simulator - a couple of questions, if you still have your original setup:
1) what were the settings of the CLK you used ? Freq/Duty Cycle/ voltages/ offset ?
2) what was the BJT beta you used ? Was it the default 100?

Click to expand...

Transistor beta 100 (default).

Clock 5 kHz, 73 % duty cycle.

At first I alternated the clock between 12 and 0V. (The setting is for 6V Max Voltage, and 6V DC Offset.)
In my unsuccessful attempts to reduce above-mentioned anomalies, I changed it to 9V and 1V. (4V Max V, and 1V Offset.)

BradtheRad said:

...Transistor beta 100 (default).

Clock 5 kHz, 73 % duty cycle.

At first I alternated the clock between 12 and 0V. (The setting is for 6V Max Voltage, and 6V DC Offset.)
In my unsuccessful attempts to reduce above-mentioned anomalies, I changed it to 9V and 1V. (4V Max V, and 1V Offset.)

Click to expand...

this is exactly as i thought... and hence my successful emulation of your pioneering simulation.

It turns out you need a beta > 1.77/ Ib, otherwise the bjt goes into a Reverse-active mode ( mode #4 for bjt's that few folks talk about, but Falsted does model), which limits the Ic. Alternately you can increase the Ib (by increasing Vb as in your case) if you want to stay below the Ic max allowed by the Beta.

In my final simulation I increased the CLK voltage to 8V, no offset. This is just enough to achieve > 1.77A Ic with the 390 ohm resistor.

Also with a freq of 5Khz, and duty =75% i was at 1.79A. ... close enough to your 1.77A. The 1.79A gave a Vcap of ~630v, while yours gave a Vcap ~605. It all makes sense !!!

All in all, falsted seems a sweet little simulator for quick analysis & insights. A little care in using it/ knowing its limitations & capabilities goes a long way.
Thanks brad...

- - - Updated - - -

Thanks FvM.... i usually use the freebie LTspice, but Falsted free's you from LTspice limitations of always having to deal with REAL components which already have proper models.

Now THAT is very useful if you want to push the boundaries of whats possible. And of course to visualise behaviour... like you said.

Thats what simulation is about after all.... right ?
:grin:

cheers1

Thats what simulation is about after all.... right ?

Click to expand...

Without a full transistor specification, or a high resolution Vce and Ic plot, I can't say if it's right.

But what I can say, it's a poor boost converter with less than 50% efficiency. With an ideal switch, the same inductor current waveform gives about 935 V output voltage.

....But what I can say, it's a poor boost converter with less than 50% efficiency. With an ideal switch, the same inductor current waveform gives about 935 V output voltage.

Click to expand...

i sense a repeat of my post #16