|
On Fri, May 9, 2025 at 05:18 PM, <arhamishtiaq42@...> wrote:
Also i want to make the PCB of this circuit in KICAD software if you have any idea how can i design this transformer do i have to place the ADuM3190-chip in my pcb??
Note that LTspice can export (convert) the schematic into netlist files for a variety of CAD programs.? In the schematic viewer, go to Tools > Export Netlist, and read the Help page for Schematic Capture > PCB Netlist Extraction.? KiCad is not one of the listed file formats, but I am assuming it can open at least one of the listed file types.
Accel, Algorex, Allegro, Applicon Bravo, Applicon Leap, Cadnetix, Calay, Calay90, CBDS, Computervision, EE Designer, ExpressPCB, Intergraph, Mentor, Multiwire, PADS, Scicards, Tango, Telesis, Vectron, and Wire List
?
About the transformer and ADuM3190, if you plan to use them in your design, then I think it only makes sense to put them on your PCB.? Otherwise, they would need to float in space with wires going to the PCB.? If you don't plan to use the ADuM3190 then it does not need to be there, of course.? It was there for a reason, but you might not need that reason.? It's up to you.? If I remember correctly, Udo's schematic had two transformers, one purchased and the other hand-made (or maybe manufactured according to your specifications).
?
Andy
?
|
Thank you so much for taking the time to help me. I truly appreciate it.?
Can you please tell the purpose of ADuM3190-chip . this circuit is quite complex for me to understand as I am undergraduate student . how did you give pulse to mosfet surely from UC3875 gate driver but how you put PULSE command i can't understand how did you manage the switching frequency? at 30kHZ? can transformer work without this ADuM3190-chip?. .
Also i want to make the PCB of this circuit in KICAD software if you have any idea how can i design this transformer do i have to place the ADuM3190-chip in my pcb??
Thanks in Advance?
-------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------------
1. The ADuM3190-chip was used to regulate the DAB-Converter. Open the datasheet to see what is inside the chip. This chip is operating much more linear, compared to other regulator configurations, such as
the combination of "voltage reference, together with an OP-Amp + Optocoupler". The optocoupler is known for it's nonlinearities and therefore more complicated to stabilize the converter.
?
?? ?I just used the ADuM3190-chip to show an alternative solution. Its use is not mandatory, you don't need it.
????????
It is assumed you want to use the Transformer for isolation purposes, right?
In that case the regulation feedback loop needs to have an isolation as well.
Another alternative, for which an isolated regulation loop can be omitted, is the use of an isolated transformer-coupled Driver. In that case you will have the freedom to put the regulation circuitry to any ground point
- output Ground for instance - without the need for an isolated feedback loop. The isolated Driver provides a floating Ground. So, the regulator inside the UC3875 could be directly used for regulation.?
?
2. The UC3875 gate driver outputs A,B and C,D can drive a transformer coupled driver or a Low side/-High side driver instead. For simplicity, I used voltage-dependent-voltage sources, which LTspice offers in its library as "e-sources". The switching frequency is accomplished by the R12,C8, connected to the FREQSET-Pin of the UC3875. For more information, pls refer to the datasheet, in which you find a curve for Rt=f(CT, frequency).
?
3. The transformer(s) have nothing to do with the ADuM3190-chip at all.
?
4. I can't assist you regarding KICAD. As mentioned above, ADuM3190-chip is not mandatory.
?
5. For transformer design, pls refer to the following articles
? ? ? ?
and
?
best regards
Udo
?
|
Thank you so much for taking the time to help me. I truly appreciate it.?
Can you please tell the purpose of ADuM3190-chip . this circuit is quite complex for me to understand as I am undergraduate student . how did you give pulse to mosfet surely from UC3875 gate driver but how you put PULSE command i can't understand how did you manage the switching frequency? at 30kHZ? can transformer work without this ADuM3190-chip?. .
Also i want to make the PCB of this circuit in KICAD software if you have any idea how can i design this transformer do i have to place the ADuM3190-chip in my pcb??
Thanks in Advance?
|
Hi John,
pls refer to my "Add-on"-file ----- Udo
Thank you, but we really want .ZIP archives,
not 7z or any other sort.
On 2025-05-09 12:40, Udo
Huhn-Rohrbacher via wrote:
Hi All,
i have uploaded a zip-file named DAB500_zip.7z, placed in the
temp.-folder.
?
You will find the following files:
- Simulation file for the 500W DAB-Converter with same
specifications as previously discussed.
- one for static Load operation, to mdeasure the Efficiency,
which reached realistic 93% to 95%
- one for pulsed Load operation from 0,83A to 3,33A with
di/dt of 2,5Amps/usec.
- Also attached are lib-files, such as for the
UC3875-controller, the current transformer and a Compensator?
with isolated feedback loop. (Replacement for optocoupler).
?
Of course, the UC3875 phase shift controller is
old-fashioned, but enough to demonstrate the functionality of
the DAB-converter.
If anyone has a modern, up-to-date controller for LTspice,
kindly give me an input.?
?
With some minor modifications, the circuit may be used for
bidirectional power flow.
------
Udo
?
?
--
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
-- Dipl.Ing.Udo Huhn-Rohrbacher Albert-Kratz-Str.1 D-75180 Pforzheim phone: +497231-352339 fax: +497231-140338 mobile: +491523-3612096 E-mail: u.huhn.rohrbacher@...
|
Thank you, but we really want .ZIP archives,
not 7z or any other sort.
On 2025-05-09 12:40, Udo
Huhn-Rohrbacher via groups.io wrote:
Hi All,
i have uploaded a zip-file named DAB500_zip.7z, placed in the
temp.-folder.
?
You will find the following files:
- Simulation file for the 500W DAB-Converter with same
specifications as previously discussed.
- one for static Load operation, to mdeasure the Efficiency,
which reached realistic 93% to 95%
- one for pulsed Load operation from 0,83A to 3,33A with
di/dt of 2,5Amps/usec.
- Also attached are lib-files, such as for the
UC3875-controller, the current transformer and a Compensator?
with isolated feedback loop. (Replacement for optocoupler).
?
Of course, the UC3875 phase shift controller is
old-fashioned, but enough to demonstrate the functionality of
the DAB-converter.
If anyone has a modern, up-to-date controller for LTspice,
kindly give me an input.?
?
With some minor modifications, the circuit may be used for
bidirectional power flow.
------
Udo
?
?
--
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
|
Hi All,
i have uploaded a zip-file named DAB500_zip.7z, placed in the temp.-folder.
?
You will find the following files:
- Simulation file for the 500W DAB-Converter with same specifications as previously discussed.
- one for static Load operation, to mdeasure the Efficiency, which reached realistic 93% to 95%
- one for pulsed Load operation from 0,83A to 3,33A with di/dt of 2,5Amps/usec.
- Also attached are lib-files, such as for the UC3875-controller, the current transformer and a Compensator?
with isolated feedback loop. (Replacement for optocoupler).
?
Of course, the UC3875 phase shift controller is old-fashioned, but enough to demonstrate the functionality of the DAB-converter.
If anyone has a modern, up-to-date controller for LTspice, kindly give me an input.?
?
With some minor modifications, the circuit may be used for bidirectional power flow.
------
Udo
?
?
|
On Wed, May 7, 2025 at 10:50 AM, John Woodgate wrote:
... Using CTRL-left click, I see 5.9124 A, but that includes the inrush current at t=0+. Is there any way to change the 'Interval start', other than changing the sim time to omit the inrush current? ...
Yes.? LTspice calculates the Average and RMS values over the displayed plot only.? Right-click on the X-axis and change the Left: value to something after the waveforms have stabilized.? Then use Ctrl-Left-Click on the name at the top of the plot.? As long as the displayed interval contains many many cycles, it should be a "good enough" average even if it is not an exact integral number of cycles.
?
Andy
?
?
|
On Wed, May 7, 2025 at 07:32 AM, Andy I wrote:
It would be interesting to see why LTspice 24 simulates badly whereas LTspice XVII does not.
Switching to the Alternate solver in LTspice 24.1.8 allows the simulation to run successfully without stalls.
?
I also changed the simulation command to ".tran 0 5m 2m" eliminate the uic and skip past the initial transient. I also commented out the erroneous measure statements.
?
Alternatively, I also noticed that some of the transient currents can be limited substantially by adding a 10m series resistance to the input source, the inductors, and the input and output capacitors. I also added a 1 ohm series resistance to the gate drive sources. With these changes the circuit simulates in 24.1.8 using the Normal solver.?
?
|
On Wed, May 7, 2025 at 10:36 AM, John Woodgate wrote:
...? 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. ...
No.? But I get hundreds of "Heightened Def Com" warnings, without the 1 ohm series resistor.? With it, those warnings disappear.
?
Andy
?
|
Yes, my 8A/16A figures were what I saw without
expanding the waveform. Using CTRL-left click, I see 5.9124 A,
but that includes the inrush current at t=0+. Is there any way
to change the 'Interval start', other than changing the sim time
to omit the inrush current? Doing that, I get 5.8583 A, so we
are in violent agreement on that point.
On 2025-05-07 15:10, Andy I via
groups.io wrote:
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
?
--
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
|
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
|
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
?
|
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
?
?
|
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
|
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
|
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
?
|
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 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.
?
?
|
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 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
?
|
John Woodgate