|
Your inductor/transformer inductances are
probably too low. 11?H is only 2 ohms at 30 kHz. How did you
calculate them? Try 10 times higher values. You didn't mention
the error messages about the .MEAS statements. There are
probably other things wrong.
On 2025-05-06 17:52, arhamishtiaq42 via
groups.io wrote:
I am making Dual active bridge (DAB converter) for my
assignment . Power should be 500W , input is 100vdc and output
should be 150 my output goal is complete but my current from
primary side of transformer is very high it should be around 8A
and now be steady kindly help me to fix this problem . I've
attached my .asc file with the name of dabhw4_new.asc
--
Best wishes John Woodgate RAYLEIGH Essex OOO-Own Opinions Only
If something is true: * as far as we know - it's science *for
certain - it's mathematics *unquestionably - it's religion
|
On Tue, May 6, 2025 at 10:16 AM, John Woodgate wrote:
dabhw4_new
Thanks for replying. i put 11us so it made my output 150 if i increase 11us to above it changes the output I've uploaded my file in TEMP with the name of dabhw4_new can you tell what should i do should i change mosfet ?
?
|
You can't change L1 without also changing L2,
keeping their ratio constant. It would be OK to change L3 by the
same factor. So try L1=110? L2=250? and L3=1?.? It doesn't make
much sense to specify a very precise value for leakage
inductance unless you know exactly how the transformer will be
constructed.
On 2025-05-06 18:33, arhamishtiaq42 via
groups.io wrote:
On Tue, May 6, 2025 at 10:16 AM, John Woodgate wrote:
dabhw4_new
Thanks for replying. i put 11us so it made my output 150 if i
increase 11us to above it changes the output I've uploaded my
file in TEMP with the name of dabhw4_new can you tell what
should i do should i change mosfet ?
?
--
Best wishes John Woodgate RAYLEIGH Essex OOO-Own Opinions Only
If something is true: * as far as we know - it's science *for
certain - it's mathematics *unquestionably - it's religion
|
yes I've changed my inductance to 110us, 250us, 1us but current is still high around 40A. and it is steady
|
I've updated my file with the name Dabnew.asc in TEMP folder kindly someone fix the current issue of my primary side transformer of DAB
|
You have a huge inrush current due to the
capacitors being fed from a zero-impedance source V9. Put 1 ohm
in series with it. But the simulation still stalls without an
error message after less than 1 ms. As far as I can see, your
switching waveforms allow each pair of series FETs to be on
together, briefly, which is not good. But there is something
else that causes the simulation to stall, and I'm not an expert
on these circuits.
On 2025-05-06 18:51, arhamishtiaq42 via
groups.io wrote:
yes I've changed my inductance to 110us, 250us, 1us but
current is still high around 40A. and it is steady
--
Best wishes John Woodgate RAYLEIGH Essex OOO-Own Opinions Only
If something is true: * as far as we know - it's science *for
certain - it's mathematics *unquestionably - it's religion
|
Alright, Anyone else who can help?
|
On Tue, May 6, 2025 at 01:51 PM, <arhamishtiaq42@...> wrote:
yes I've changed my inductance to 110us, 250us, 1us but current is still high around 40A. and it is steady
Your messages are somewhat confusing.
?
Of course the inductances should be in uH (micro Henrys), not us (micro seconds), but we get the idea.? I may not understand what you meant by "steady".? I'm assuming you did not mean DC, but maybe you mean the steady state RMS current after transients die out.
?
Do we assume that we should start with the schematic named "Dabnew.asc" and change to these values:
- L1 = 110u
- L2 = 250u
- L3 = 1u
and that you see a primary (L1) current of 40 Amp, and you think that is too much?
?
I do not see a current near 40 Amps.? My simulation shows that the primary current is 12.9 Amps RMS.
?
Its waveform is rather peaky (distorted), and the peaks reach around +/- 28 Amps = 56 Amps peak-to-peak.
?
What do you expect the primary (L1) current to be?
?
The primary voltage is a +/-95 V square wave which comes out to 95.6 V RMS.? So the input VA product is 1233 Volt-Amps.? We know its volt-amps but not its power because the phase shift is not known.? If we look at the power source (V9), it supplies an average power of almost 600 watts to the circuit.? Therefore the power going into primary winding L1 must not be greater than 600 watts, even though its VA is 1233 Volt-Amps.
?
The load resistor, R1, dissipates about 460 Watts.? 600 watts in, 460 watts out, so 140 watts is lost somewhere.??You can check for places where energy is lost.? For example, each of the four MOSFETs on the secondary side (M4, M5, M6, and M7) dissipates 32.4 watts, so you lose almost 130 watts in those four transistors.? I'm guessing the losses are a lot smaller in the transistors driving the primary.? But I leave that to you.
?
In a real circuit, all inductors have resistance.? In LTspice, the default internal resistance of L1 and L2 is 0 ohms because they are coupled, and the internal resistance of L3 is 0.001 ohm.? It's unlikely that your transformer has that little DC resistance in it.
?
Where else do you need help?
?
Andy
?
|
On Tue, May 6, 2025 at 02:08 PM, John Woodgate wrote:
... But the simulation still stalls without an error message after less than 1 ms.
My simulation did not stall.? It is somewhat slow and I did not wait 100ms for it to finish, but it never stalled.? That might be because of different Control Panel settings, or it might be because of different LTspice versions.? My simulation had plenty of "Heightened Def Con" warnings, which are not a good sign.
?
As far as I can see, your switching waveforms allow each pair of series FETs to be on together, briefly, which is not good.
That is the short-circuit current (sometimes erroneously? called crowbar current) through the FETs, and can be the cause of much of their power loss which is where about 130 watts have gone.? Switching transistor circuits should be designed with non-overlapping drive signals so that it won't happen.
?
?
|
What version allowed the sim to run without
stalling? I am now using 24.1.8, and the sim stalls after a
different number of microseconds , depending on which tweak I
have made to the .ASC.? I don't tweak the Spice settings, like
Gmin and Abstol.? I let it run for minutes and the stall did not
resolve. The expanded netlist shows a huge number of reports of
'simulation tolerance relaxed' between time points that are
small to begin with and eventually appear identical at 17
significant figures. It looks to me that some sort of error
message should appear, rather than the stall just persisting.
On 2025-05-06 21:44, Andy I via
groups.io wrote:
On Tue, May 6, 2025 at 02:08 PM, John Woodgate wrote:
... But the simulation
still stalls without an error message after less than 1
ms.
My simulation did not stall.? It is somewhat slow and I did
not wait 100ms for it to finish, but it never stalled.? That
might be because of different Control Panel settings, or it
might be because of different LTspice versions.? My simulation
had plenty of "Heightened Def Con" warnings, which are not a
good sign.
?
As far as I can see, your
switching waveforms allow each pair of series FETs to be
on together, briefly, which is not good.
That is the short-circuit current (sometimes erroneously
called crowbar current) through the FETs, and can be the cause
of much of their power loss which is where about 130 watts were
lost.? Switching transistor circuits should be designed with
non-overlapping drive signals so that it won't happen.
?
?
--
Best wishes John Woodgate RAYLEIGH Essex OOO-Own Opinions Only
If something is true: * as far as we know - it's science *for
certain - it's mathematics *unquestionably - it's religion
|
On Tue, May 6, 2025 at 05:14 PM, <arhamishtiaq42@...> wrote:
Sorry, I uploaded the wrong file earlier
Good to know.
My desired output is 150?V, and I’ve noticed that changing the transformer inductances is affecting the output voltage.
As it must.
Currently, if I set the transformer values as L1 = 110??H, L2 = 250??H, and L3 = 1??H, the primary-side current becomes too high.
How much is "too much"?
Since I’m designing a 500?W Dual Active Bridge (DAB) converter, I expect the primary current to be around 8?A, because
I'm supplying 500?W at 100?V input:
So therefore it provides less than 500 W to the load, right?
Iavg=P/Vin=500/100=5 A
IRMS?≈1.3×Iavg?=6.5–8?A?but it’s exceeding that.
But some of that current into the primary represents reactive power, not real power.
Also, by “steady state,” I mean that the average current should not be zero
Um, we are not speaking the same thing.? The average current must be zero.? Transformers do not pass DC.
?
Andy
?
|
It should not be much larger than output
current x output voltage/input voltage. That is, power out/input
voltage. But I already told you that there is a very large
inrush current because of the large capacitor across the
zero-impedance source V9. The other capacitors also charge when
the associated FET switches off.
On 2025-05-06 22:33, arhamishtiaq42 via
groups.io wrote:
so do you think my primary side current is fine?
--
Best wishes John Woodgate RAYLEIGH Essex OOO-Own Opinions Only
If something is true: * as far as we know - it's science *for
certain - it's mathematics *unquestionably - it's religion
|
On Tue, May 6, 2025 at 06:35 PM, John Woodgate wrote:
.... But I already told you that there is a very large inrush current because of the large capacitor across the zero-impedance source V9. ...
I think that problem goes away if you get rid of the UIC.? There is no need for UIC here.? Don't use it unless it is needed.? Change:
? ? .tran 0 100m 0 uic
to:
? ? .tran 0 100m 0?
or:
? ? .tran 100m
or even this:
? ? .tran 10m
?
I do not think you can expect to see V*I at either primary or secondary to be only a little more than Vout*Iout.? Both waveforms very non-sinusoidal and in different ways from one another.? Thus, Average(V(time)*I(time)) does not come even close to Vrms*Irms.? I think you need to accept that the RMS current can not be calculated by dividing the power by the RMS current.? Math just doesn't work that way, so long as the waveforms are neither DC nor sinusoidal.
?
?
|
On Tue, May 6, 2025 at 05:33 PM, <arhamishtiaq42@...> wrote:
so do you think my primary side current is fine?
That is a somewhat difficult question for me to answer.? Maybe others can speak to this better than I can.
?
But I think the answer is "yes", I think it is normal.
?
Because the waveforms are not sinusoidal and the voltage and current waveforms are so very different from each other, you can not use Vrms*Irms to estimate power.? You must multiply V(time) by I(time) at every moment in time, then average the product over time.? And when you do that, you find that the power into the primary = 593 W, even though its Vrms * Irms = 95.6 * 12.9 = 1233 VA.
?
(I am still wondering where you got 40 A from.? My simulations did not come close.)
?
I think the only way for the primary current to be around 500 W / 100 V = 5 A, is if the transformer's primary current was also a square wave and in-phase with the voltage there.
?
The energy source (V9) provides 597 W, the transformer passes 593 W, and the load (R1) dissipates 458 W.? These are from simulating your third schematic, dd.asc, without UIC, and waiting until after the initial transients die out.
?
Andy
?
?
|
On Tue, May 6, 2025 at 05:12 PM, John Woodgate wrote:
What version allowed the sim to run without stalling?
Using computer #1 today, so it is lowly LTspice XVII.? Not LTspice 24.
?
You night have been hit by a yet-to-be-fixed bug - er, I mean side effect they added in version 24.1.x.
?
Andy
?
|
Without UIC, it runs under version 24.1.8. The
input voltage is 100 V, the input current is 8 A DC plus 8A peak
roughly sinusoidal (so the current goes from 0 to 16 A). The
output voltage is 132 V DC and the output current is 3 A. So I
think the input power is quite a lot bigger than the output
power, which is not what is wanted. But I have 1 ohm in series
with V9 to limit the inrush current. Without the 1 ohm, it still
stalls after a few hundred microseconds, with no error message.
On 2025-05-07 01:18, Andy I via
groups.io wrote:
so do you think my primary side current is fine?
That is a somewhat difficult question for me to answer.? Maybe
others can speak to this better than I can.
?
But I think the answer is "yes", I think it is normal.
?
Because the waveforms are not sinusoidal and the voltage and
current waveforms are so very different from each other, you can
not use Vrms*Irms to estimate power.? You must multiply V(time)
by I(time) at every moment in time, then average the product
over time.? And when you do that, you find that the power into
the primary = 593 W, even though its Vrms * Irms = 95.6 * 12.9 =
1233 VA.
?
(I am still wondering where you got 40 A from.? My
simulations did not come close.)
?
I think the only way for the primary current to be around 500
W / 100 V = 5 A, is if the transformer's primary current was
also a square wave and in-phase with the voltage there.
?
The energy source (V9) provides 597 W, the transformer passes
593 W, and the load (R1) dissipates 458 W.? These are from
simulating your third schematic, dd.asc, without UIC, and
waiting until after the initial transients die out.
?
Andy
?
?
--
Best wishes John Woodgate RAYLEIGH Essex OOO-Own Opinions Only
If something is true: * as far as we know - it's science *for
certain - it's mathematics *unquestionably - it's religion
|
Set Lp = 2,3mH Ls=5,1mH Llkg=76uH . Imagn=magnetizing current =8% of primary peak current, Llkg = 3% of Lp (values chosen for 30KHz).
Imagn/Ipeak may be a little bit higher, i.e. 15%
A small gap between the upper and lower Bridge MOS will prevent from cross-conducting current spikes. At present, currents are overlapping.?
Also check the phase angles between the primary and secondary side bridge drive pulses to achieve?output voltage, as desired.
-----
Udo
|
On Wed, May 7, 2025 at 05:04 AM, John Woodgate wrote:
Without UIC, it runs under version 24.1.8. The input voltage is 100 V, the input current is 8 A DC plus 8A peak roughly sinusoidal (so the current goes from 0 to 16 A). The output voltage is 132 V DC and the output current is 3 A.
Wow!? Which schematic was that?? What makes our simulations so utterly different?
?
I used dd.asc with UIC removed.? The input current from V9 is hardly sinusoidal.? If you had sinusoidal current, then something must be wrong.
?
My simulation's input voltage is 100 V (of course), but the average input current is 6.159 A, not 8 A DC.? Its waveform peaks at around +105 A (that's not a typo!) and at -23 A (yes, power going back into the voltage source).? Those peaks are quite narrow.? It is definitely not "roughly sinuoidal".
?
The RMS current from V9 is 12.6 A, which includes both the DC portion and the AC component which represents instantaneous power going both ways.
?
So I think the input power is quite a lot bigger than the output power, which is not what is wanted.
The important thing is, do the numbers make sense?? Do they add up?
?
In my simulation, they do.? Using Alt-Left-Click on V9, LTspice plots the instantaneous power (V*I) waveform of V9.? Then using Ctrl-Left-Click on the waveform label at the top of the plot, it says the Average Power is -597.32 W.? That is the power dissipated by V9, meaning that V9 sources +597.32 W to the circuit.
?
Doing the same thing with the load (R1), LTspice shows 458.39 W dissipated by the load.
?
The difference is 597-32 - 458.39 = 138.93 W that V9 sources but does not reach the load.? That is not so bad.? It's not ideal, of course, but nothing is perfect.? I think a lot of power is lost due to short-circuit current through the FETs.
?
Doing the same thing to each of the MOSFETs on the right side (M4, M5, M6, M7) shows that each of them dissipates (loses as heat) approx. 32.4 W, adding up to 129.6 W lost in those four FETs.? That compares favorably with the 138.93 W total power that did not make it from V9 into R1.? It shows that the four FETs on the right side caused most of the power loss.? You can improve that.
?
But I have 1 ohm in series with V9 to limit the inrush current.
Ah, of course!? That is what makes your simulation so much different than mine.
?
Without the 1 ohm, it still stalls after a few hundred microseconds, with no error message.
If it stalls, then it is still simulating, right?? If it is still simulating, then there won't be an error message (yet).? It would be great if LTspice always times out after a while, but when should it time out?? Apparently it thinks it is still making positive progress.??From what you wrote earlier, I think LTspice 24 was heading towards a "timestep too small" error, but not reaching it.? That rarely happens.? Usually when it is heading towards a "timestep too small" situation, it positively reaches it, and aborts.? Apparently it saves itself before that happens.? Hmm.
?
LTspice XVII does not stall at any point, with or without Rser-1 ohm.
?
It would be interesting to see why LTspice 24 simulates badly whereas LTspice XVII does not.
?
Andy
?
?
|
After adding Rser=1 ohm to V9:
?
The average current from V9 is 5.858 Amps, compared to the 8 Amps you said yours had.? Our simulations should not have differed by more than 2 Amps!? Something is wrong.? (Unless you eyeballed your "8 Amps" without measuring it.)? The current waveform there does look kind of sinusoidal with about 8 Amps peak amplitude, varying from -1 A to about +16.5 A.? But it is a highly distorted sinewave and that makes a big difference; the average is not in the middle.? LTspice says the average is 5.858 A DC, in my simulation.
?
The average power from V9 simulates as 507 W, which is nowhere near the roughly 800 W that you estimated.? Again, was that by ayeballing, or measuring it?
?
At the load, I measure 132 V DC as you did, plus some ripple.? Average power there is 385 W, so the converter loses 122 W to heat (76% efficiency).? That is not so bad, but again most of it is in M4, M5, M6, and M7, which can be reduced by building some dead-band into their gate waveforms.
?
Simulating with a discrete 1 ohm resistor instead of Rser=1, I have 640 W sourced by V9 and 108 W dissipated by the 1 ohm resistor.? Between the two, that is 532 W supplied by V9+1ohm to the rest of the circuit.? It is not quite the same as the 507 W when Rser was internal, but I don't know why (it should not have differed, right?).? Will check into that later.
?
In any event, with LTspice XVII, the power losses of the circuit are reasonable, and can be reduced further.? If LTspice 24 tells you a different story, that needs to be understood.? If LTspiceXVII says 122 W is lost and LTspice24 says 400 W is lost, that is a big problem.
?
Andy
?
|
I entirely agree. I may be doing something
wrong, but I can't see what. Do you get a very long series of
entries in the expanded netlist about relaxing tolerances to
seek convergence?? That occurs even with the 1 ohm in series
with V9, in the sim which runs OK to 100 ms. V9 current near
100ms is an 8 A peak sine wave with the positive peak clipped,
sitting on 8A DC.
On 2025-05-07 14:32, Andy I via
groups.io wrote:
?
It would be interesting to see why LTspice 24 simulates
badly whereas LTspice XVII does not.
?
--
Best wishes John Woodgate RAYLEIGH Essex OOO-Own Opinions Only
If something is true: * as far as we know - it's science *for
certain - it's mathematics *unquestionably - it's religion
|
John Woodgate