Maker Pro
Maker Pro

Half bridge DC-DC converter topology

P

P E Schoen

Jan 1, 1970
0
There is a thread in
http://www.diyelectriccar.com/forums/showthread.php/evnetics-developing-dc-dc-converter-72862p5.html
which suggests a half-bridge DC-DC converter with the following topology:
http://www.diodes.com/zetex/?ztx=3.0/application@app~49!top~5!curr~13

Originally I thought it was only useful for low power applications like
phone chargers, and I think the capacitor in series with the primary is
superfluous because of the two series capacitors across the DC bus. I found
a similar topology here:
http://www.st.com/internet/com/TECH...AL_LITERATURE/APPLICATION_NOTE/CD00003910.pdf

I modeled the converter using LTSpice and it seems to work quite well with
reasonable components, and it seems to have less problem with transients
than my direct drive push-pull topology. It also seems to be fairly tolerant
of imbalance and it does allow the use of PWM, although it works best at
50%.

http://www.enginuitysystems.com/pix/Half_Bridge_144V-12V.png

The simulation ASC file is there also:
http://www.enginuitysystems.com/pix/Half_Bridge_144V-12V.asc

In this case, it is a high power step-down DC-DC converter. Apparently many
EVs use a separate 12V battery for accessories so they can use the same
components as wiring as the original ICE donor (or transplant recipient)
car. The 144V is typical for a battery pack and the DC-DC converter uses
power from that to keep the battery charged and run the lights, fans,
wipers, and other usual accessories. But apparently some of the commercially
available converters are not very reliable or efficient, and just using an
ordinary switching supply and/or charger such as are available from
Mean-Well are prone to failure in an automotive environment.

I may try a similar design for my purposes, which is essentially the
reverse. I want to use 24-48 VDC from batteries and boost it to 320 VDC or
640 VDC for a VFD and three-phase motor. I have the previous push-pull
design modified with a capacitor precharge circuit and adjustable PWM but it
has become complicated, and this topology seems simpler and perhaps better.
There seem to be many more drive ICs and complete controllers for
half-bridge than for push-pull, so maybe it's the way to go.

Thanks,

Paul
 
T

Tim Williams

Jan 1, 1970
0
The reason it works better is because it has a choke input filter. Although
you still get nasty inrush current with a voltage-mode controller, at least
without a lot of precautions. Current mode control is best.

Tim

--
Deep Friar: a very philosophical monk.
Website: http://webpages.charter.net/dawill/tmoranwms

There is a thread in
http://www.diyelectriccar.com/forums/showthread.php/evnetics-developing-dc-dc-converter-72862p5.html
which suggests a half-bridge DC-DC converter with the following topology:
http://www.diodes.com/zetex/?ztx=3.0/application@app~49!top~5!curr~13

Originally I thought it was only useful for low power applications like
phone chargers, and I think the capacitor in series with the primary is
superfluous because of the two series capacitors across the DC bus. I found
a similar topology here:
http://www.st.com/internet/com/TECH...AL_LITERATURE/APPLICATION_NOTE/CD00003910.pdf

I modeled the converter using LTSpice and it seems to work quite well with
reasonable components, and it seems to have less problem with transients
than my direct drive push-pull topology. It also seems to be fairly tolerant
of imbalance and it does allow the use of PWM, although it works best at
50%.

http://www.enginuitysystems.com/pix/Half_Bridge_144V-12V.png

The simulation ASC file is there also:
http://www.enginuitysystems.com/pix/Half_Bridge_144V-12V.asc

In this case, it is a high power step-down DC-DC converter. Apparently many
EVs use a separate 12V battery for accessories so they can use the same
components as wiring as the original ICE donor (or transplant recipient)
car. The 144V is typical for a battery pack and the DC-DC converter uses
power from that to keep the battery charged and run the lights, fans,
wipers, and other usual accessories. But apparently some of the commercially
available converters are not very reliable or efficient, and just using an
ordinary switching supply and/or charger such as are available from
Mean-Well are prone to failure in an automotive environment.

I may try a similar design for my purposes, which is essentially the
reverse. I want to use 24-48 VDC from batteries and boost it to 320 VDC or
640 VDC for a VFD and three-phase motor. I have the previous push-pull
design modified with a capacitor precharge circuit and adjustable PWM but it
has become complicated, and this topology seems simpler and perhaps better.
There seem to be many more drive ICs and complete controllers for
half-bridge than for push-pull, so maybe it's the way to go.

Thanks,

Paul
 
L

legg

Jan 1, 1970
0
There is a thread in
http://www.diyelectriccar.com/forums/showthread.php/evnetics-developing-dc-dc-converter-72862p5.html
which suggests a half-bridge DC-DC converter with the following topology:
http://www.diodes.com/zetex/?ztx=3.0/application@app~49!top~5!curr~13

Originally I thought it was only useful for low power applications like
phone chargers, and I think the capacitor in series with the primary is
superfluous because of the two series capacitors across the DC bus. I found
a similar topology here:
http://www.st.com/internet/com/TECH...AL_LITERATURE/APPLICATION_NOTE/CD00003910.pdf

I modeled the converter using LTSpice and it seems to work quite well with
reasonable components, and it seems to have less problem with transients
than my direct drive push-pull topology. It also seems to be fairly tolerant
of imbalance and it does allow the use of PWM, although it works best at
50%.

http://www.enginuitysystems.com/pix/Half_Bridge_144V-12V.png

The simulation ASC file is there also:
http://www.enginuitysystems.com/pix/Half_Bridge_144V-12V.asc

In this case, it is a high power step-down DC-DC converter. Apparently many
EVs use a separate 12V battery for accessories so they can use the same
components as wiring as the original ICE donor (or transplant recipient)
car. The 144V is typical for a battery pack and the DC-DC converter uses
power from that to keep the battery charged and run the lights, fans,
wipers, and other usual accessories. But apparently some of the commercially
available converters are not very reliable or efficient, and just using an
ordinary switching supply and/or charger such as are available from
Mean-Well are prone to failure in an automotive environment.

I may try a similar design for my purposes, which is essentially the
reverse. I want to use 24-48 VDC from batteries and boost it to 320 VDC or
640 VDC for a VFD and three-phase motor. I have the previous push-pull
design modified with a capacitor precharge circuit and adjustable PWM but it
has become complicated, and this topology seems simpler and perhaps better.
There seem to be many more drive ICs and complete controllers for
half-bridge than for push-pull, so maybe it's the way to go.

Thanks,

Paul

The topology that you are admiring works well in the application
because the primary voltage is high. The half bridge lends an
automatic reduction in turns ratio. It will not work as well, if the
primary voltage is reduced by an order of magnitude, to produce a high
voltage output, because it pushes the turns ratio in the wrong
direction - away from the ideal unity.

If you examine the circuit and imagine active switches on the low
voltage side, you will see that the low voltage end of the admired
circuit becomes a current-fed push pull topology. If you wanted to
maintain the utility in reverse power transmission, you should try to
preserve this form, as it can function naturally as a boost converter
if low voltage switch conduction overlaps.

The issue of inrush is not avoided, however. If you expect it to
operate into low voltage loads it must be manipulated to run without
an overlap on the low voltage side, with some allowance for energy
transfer in the non-overlapping period. Some kinds of switched snubber
have been employed to do this successfully, although the added
switches do tend to increase component count and cost.

This is not an issue if you're charging batteries with terminal
voltages that don't reduce to abnormally low values - so you should
decide whether this thing is intended to operate without batteries
early on. In an automotive application, it would be highly abnormal to
expect anything to run without the fuel source.

RL
 
P

P E Schoen

Jan 1, 1970
0
"legg" wrote in message
The topology that you are admiring works well in the application
because the primary voltage is high. The half bridge lends an
automatic reduction in turns ratio. It will not work as well, if the
primary voltage is reduced by an order of magnitude, to produce a
high voltage output, because it pushes the turns ratio in the wrong
direction - away from the ideal unity.
If you examine the circuit and imagine active switches on the low
voltage side, you will see that the low voltage end of the admired
circuit becomes a current-fed push pull topology. If you wanted to
maintain the utility in reverse power transmission, you should try to
preserve this form, as it can function naturally as a boost converter
if low voltage switch conduction overlaps.
The issue of inrush is not avoided, however. If you expect it to
operate into low voltage loads it must be manipulated to run without
an overlap on the low voltage side, with some allowance for energy
transfer in the non-overlapping period. Some kinds of switched
snubber have been employed to do this successfully, although the
added switches do tend to increase component count and cost.
This is not an issue if you're charging batteries with terminal
voltages that don't reduce to abnormally low values - so you should
decide whether this thing is intended to operate without batteries
early on. In an automotive application, it would be highly abnormal to
expect anything to run without the fuel source.

I redesigned the circuit for 24V to 320V, and it is not a battery charger,
but a source of high voltage from a small battery pack.. I had some problems
with some extremely high short duration (40 nSec) power surges in the
MOSFETs at turn-off, and I found that most large capacitors for the center
tap had fairly high ESR so that they were eating up about 40 watts each. So
I found that I could use much smaller value capacitors which are actually
polypropylene film, with ESR of 2-4 mOhms, and things worked much better. I
had put some hefty snubbers in the circuit but they may not really be
needed. It seems like this should work OK for about 1 kW and hopefully up to
2 kW or so. Maybe 5 kW, although for that I might use 36 or 48 VDC input. I
want to keep the battery current under 100 amps.

So, here is the simulation:
http://www.enginuitysystems.com/pix/Half_Bridge_24V_320V.png

and the ASC file:
http://www.enginuitysystems.com/pix/Half_Bridge_24V-320V.asc

I might see if I can fix my existing push-pull DC-DC converter pretty much
as-is but adding the precharge and some series inductance to lower the
inrush. I'll see if I can get it to work at 16 kHz with the iron core
toroid. That should be interesting.

The new design uses 50 kHz and a ferrite transformer. I need to implement a
precharge and/or current limit as well. I'll package it in a smaller box and
add some hooks for measurement and datalogging. I may actually build it in a
couple of weeks.

Thanks,

paul
 
L

legg

Jan 1, 1970
0
"legg" wrote in message




I redesigned the circuit for 24V to 320V, and it is not a battery charger,
but a source of high voltage from a small battery pack.. I had some problems
with some extremely high short duration (40 nSec) power surges in the
MOSFETs at turn-off, and I found that most large capacitors for the center
tap had fairly high ESR so that they were eating up about 40 watts each. So
I found that I could use much smaller value capacitors which are actually
polypropylene film, with ESR of 2-4 mOhms, and things worked much better. I
had put some hefty snubbers in the circuit but they may not really be
needed. It seems like this should work OK for about 1 kW and hopefully up to
2 kW or so. Maybe 5 kW, although for that I might use 36 or 48 VDC input. I
want to keep the battery current under 100 amps.

So, here is the simulation:
http://www.enginuitysystems.com/pix/Half_Bridge_24V_320V.png

and the ASC file:
http://www.enginuitysystems.com/pix/Half_Bridge_24V-320V.asc

I might see if I can fix my existing push-pull DC-DC converter pretty much
as-is but adding the precharge and some series inductance to lower the
inrush. I'll see if I can get it to work at 16 kHz with the iron core
toroid. That should be interesting.

The new design uses 50 kHz and a ferrite transformer. I need to implement a
precharge and/or current limit as well. I'll package it in a smaller box and
add some hooks for measurement and datalogging. I may actually build it in a
couple of weeks.

Thanks,

paul

If you examine your simulation more closely, you'll find some
difficulties exist that are being glossed over.

The power train ripple current, determined by the output inductor,
could not be larger (producing AC losses in the internal source
impedance of over 400W). 20uH is a very small value for the forward
topology at 300V.

Source internal loss can be reduced by two orders of magnitude if the
output inductor value increases by one order. This is not normally the
major design criteria in choosing an output filter inductor, but it's
a good indication that you don't know enough about this design process
to proceed.

I suggest more reading and comprehension, with less bravado, in future
'work'. I doubt your simulations will ever accurately predict behavior
in any low voltage, high current, high frequency circuit, unless some
attempt is made to introduce the physical strays of wiring inductance
and leakage inductance accurately. This requires at least physical
model for first estimation. Admittedly, these precautions were more
commonly enforced in the past, when real hardware, real expense and
real safety were involved.

RL
 
P

P E Schoen

Jan 1, 1970
0
"legg" wrote in message
If you examine your simulation more closely, you'll find some
difficulties exist that are being glossed over.
The power train ripple current, determined by the output inductor,
could not be larger (producing AC losses in the internal source
impedance of over 400W). 20uH is a very small value for the forward
topology at 300V.
Source internal loss can be reduced by two orders of magnitude if the
output inductor value increases by one order. This is not normally the
major design criteria in choosing an output filter inductor, but it's
a good indication that you don't know enough about this design
process to proceed.

I don't really see how the source losses come into play. I was getting close
to 90% efficiency at about 1 kW power level so there can't be any more than
100W total losses. And I can see that most of that is in the MOSFETs and the
capacitors. Do you calculate the source losses by using I(in)^2 * R(in)?

I increased the value to 100 uH and then 50 uH, and both seemed to work
well, although output voltage and total power dropped. I will need to look
at practical inductors to see what would be a good fit. I also tried
increasing the resistance of snubber resistors R3 and R4, from 0.1 ohm to 1
ohm or 10 ohms, and the higher values produced short duration power surges
of 1 to 2 kW. A 0.2 ohm value brings it down to about 500W, which may be
safe, depending on the actual MOSFETs I use.
I suggest more reading and comprehension, with less bravado, in
future 'work'. I doubt your simulations will ever accurately predict
behavior in any low voltage, high current, high frequency circuit,
unless some attempt is made to introduce the physical strays of
wiring inductance and leakage inductance accurately. This
requires at least physical model for first estimation. Admittedly,
these precautions were more commonly enforced in the past,
when real hardware, real expense and real safety were involved.

I understand some of the basics but I don't have a strong background in
mathematics and magnetism, so my design process tends to be more
"instinctive" and determined largely by trial and error simulation. I also
don't have much experience in high frequency circuits, which is probably why
I have had problems with some designs when I have committed them to a PCB.
The information about skin effect and high frequency AC resistance was an
eye-opener. There is an incredible amount to learn in order to be truly
proficient, and there's a limit to how much I can learn by reading and
comprehension.

When the explanation becomes peppered with calculus my mind shuts down. I
seem to do better by running a simulation and trying to observe effects that
I did not expect, I look for probable causes and make changes to see if
there is an improvement. It may not be the best way to proceed, but I have a
feel for what will happen in real world circuits and usually they have
worked about as expected. My problems have usually been due to ignoring the
start-up transients, and when I deal with them, I think it will be reliable.

These circuits are more or less on a hobby level at this time. I'm using
them for my own electric tractor project and I'm trying to apply what I
learn to larger systems such as electric cars and trucks, in the DIY market.
There are some things that I am still learning from the experiences of
people on that forum, but I can also see that they often do not have a solid
understanding of some basic principles. It's quite a leap from my own
projects of 2 kW or so, to some of their projects which usually involve
20-50 kW and in some cases into the megaWatt range. I'm used to dealing with
such power at line voltage levels and 60 Hz, and AC currents in the 10k to
100k range, but their use of high capacity batteries and exotic motors and
controllers is something else. Mistakes at that level, especially in
automotive use, can be costly and dangerous, especially when so many DIYers
do not really understand what they are dealing with and what they are
measuring.

Thanks,

Paul
 
L

legg

Jan 1, 1970
0
I understand some of the basics but I don't have a strong background in
mathematics and magnetism, so my design process tends to be more
"instinctive" and determined largely by trial and error simulation. I also
don't have much experience in high frequency circuits, which is probably why
I have had problems with some designs when I have committed them to a PCB.
The information about skin effect and high frequency AC resistance was an
eye-opener. There is an incredible amount to learn in order to be truly
proficient, and there's a limit to how much I can learn by reading and
comprehension.

When the explanation becomes peppered with calculus my mind shuts down. I
seem to do better by running a simulation and trying to observe effects that
I did not expect, I look for probable causes and make changes to see if
there is an improvement. It may not be the best way to proceed, but I have a
feel for what will happen in real world circuits and usually they have
worked about as expected. My problems have usually been due to ignoring the
start-up transients, and when I deal with them, I think it will be reliable.

These circuits are more or less on a hobby level at this time. I'm using
them for my own electric tractor project and I'm trying to apply what I
learn to larger systems such as electric cars and trucks, in the DIY market.
There are some things that I am still learning from the experiences of
people on that forum, but I can also see that they often do not have a solid
understanding of some basic principles. It's quite a leap from my own
projects of 2 kW or so, to some of their projects which usually involve
20-50 kW and in some cases into the megaWatt range. I'm used to dealing with
such power at line voltage levels and 60 Hz, and AC currents in the 10k to
100k range, but their use of high capacity batteries and exotic motors and
controllers is something else. Mistakes at that level, especially in
automotive use, can be costly and dangerous, especially when so many DIYers
do not really understand what they are dealing with and what they are
measuring.

Thanks,

Paul

There is nothing shameful about working with circuits below 1KW. It's
the most practical method of developing preliminary physical models
and prototypes.

The principles involved apply at all power levels. What changes is the
physical limitations of materials and methods, when scaled. Your
circuit is a good example. Try running the simulation with reduced
transformer Lp, while maintaining turns ratio. Even with a coupling
coefficient of 0.99, your current values are dominating permissible
Di/Dt in the power transfer, due to leakage terms.

In real life, Lp will be selected only to be high enough so that
magnetizing energy doesn't dominate function unintentionally and
copper losses are minimized, so long as core losses remain manageable.

Another example - see what happens when 50nH is present in battery
lead wiring....

Neither of these factors would be so noticeable at 100w. One of the
major purposes of modeling in software is that these effects can be
predicted before hardware is constructed.

There's usually not much calculus required, it's usually just basic
algebra, with a little trig thrown in.

http://cp.literature.agilent.com/litweb/pdf/5952-4020.pdf
http://www.onsemi.com/pub_link/Collateral/SMPSRM-D.PDF

DIYers may try to use readily available subassemblies and materials
from similar, if not directly related applications. It's just as
important to understand the potential and limitations of these
materials as it is when developing from scratch.

RL
 
P

P E Schoen

Jan 1, 1970
0
"John Larkin" wrote in message
This IR driver chip is pretty nice:

at least for fixed duty cycle.

I have some similar products, IR2104, IR2136, IRS2001, IRS24531. The
IRS2153D http://www.irf.com/product-info/datasheets/data/irs2153d.pdf seems
similar to the IR21531 and in fact the added 1 on the part number signifies
a smaller deadband. I like the idea of the built-in timer for
self-oscillation although I also like to drive with a PIC for more accurate
frequency.

The topology of your application shows the transformer primary driven
through capacitors, and that might be even better than what I have with a
center tap between two capacitors. It seems to me that an output voltage
control of sorts could be done by adjusting the frequency of the square
wave. And the start-up surge would be easily controlled by starting with a
small duty cycle and ramping up to 50%. That would require a bridge driver
like the IRS2001 which has separate high and low drivers.

For my low voltage high power application the capacitors would need to be
able to handle high ripple current with low ESR. Those are somewhat rare and
expensive. Here is a 22,000 uF 63V cap with 20A ripple for $38.
http://www.digikey.com/product-detail/en/PEH200MJ5220MB2/399-5653-ND/2193731

For a 24V system with half-bridge I figure that's about 12V RMS so for 1000
watts I need about 80 amps. So four of those would be $150.

It seems better to use polypropylene film. Here is a 10uF 300V capacitor
with 2.9mOhms ESR and 15A ripple, for $3.51ea/10:
http://www.digikey.com/product-detail/en/B32674D3106K/495-2915-ND/1277679

The high voltage is "wasted" but the cost is much better. 6 in parallel is
still reasonable, $21. And I can easily go to a 48V system or even higher
with no worries. In the EV world it would be very useful to have a 144V-144V
booster to get 288V for a 240 VAC motor drive. Probably about 20 kW. And
probably best to build with multiple 2 kW units in parallel. $50/kW would be
an acceptable selling price.

Thanks!

Paul
 
P

P E Schoen

Jan 1, 1970
0
"John Larkin" wrote in message
If you need a lot of filter cap, center-tapping the filter caps
makes sense. My 24 volt input is already DC, so I didn't need
a lot of filtering.

My application will be powered by batteries, so very little filtering is
needed. Mostly for high frequency current surges to compensate for cable
inductance and battery ESR.
The center-tapped filter cap is interesting in that it reduces DC
inrush surge. The low side of the primary powers up at V+/2. Of
course, you still have to charge the caps on the load side.

They also draw a huge surge on the line side from the battery. The series
capacitor draws nothing until the output of the half-bridge starts
oscillating. I tried using a 5% duty cycle and I got 65 VDC output. Should
work to ramp up the duty cycle for a soft start, or for output regulation.
Full bridge operation mitigates some of those problems. I think.

Well, yes, I think so. Or I could go back to the direct drive push-pull CT
topology. So there are trade-offs, and direct coupling may be best. But it
seems that the series capacitance helps reduce the spikes. Maybe a full
bridge with a capacitor in series with the primary? Could there be a problem
with resonance?

Thanks,

Paul
 
P

P E Schoen

Jan 1, 1970
0
"legg" wrote in message
There is nothing shameful about working with circuits below 1KW.
It's the most practical method of developing preliminary physical
models and prototypes.
The principles involved apply at all power levels. What changes
is the physical limitations of materials and methods, when
scaled. Your circuit is a good example. Try running the simulation
with reduced transformer Lp, while maintaining turns ratio. Even
with a coupling coefficient of 0.99, your current values are
dominating permissible Di/Dt in the power transfer, due
to leakage terms.
In real life, Lp will be selected only to be high enough so that
magnetizing energy doesn't dominate function unintentionally and
copper losses are minimized, so long as core losses remain manageable.
Another example - see what happens when 50nH is present in battery
lead wiring....

There's an interesting thread in the DIYelectricCar forum that shows how
much battery lead and motor lead wiring inductance and resistance can affect
the waveforms and operation of a rather simple but high-power PWM DC
traction motor controller. I tried to give some advice, but I think much of
the difficulty is the OP's lack of understanding as well as poor wiring and
measurement techniques:
http://www.diyelectriccar.com/forums/showthread.php/open-revolt-igbt-driver-blew-igbts-74629p8.html
Neither of these factors would be so noticeable at 100w. One of
the major purposes of modeling in software is that these effects
can be predicted before hardware is constructed.

The transformer design seems to be the major problem, especially at higher
frequencies. I need to rethink my original method of using thicker wire, and
go to a bifilar winding with multiple smaller strands in parallel. But I
don't know just how to determine leakage inductance, and I'm not sure if my
LCR meters are good enough to measure it after building one. I just guessed
at the 0.99 for the coupling. I know everything works better if I set it to
1.00, but that's unrealistic. I have sometimes added external inductance to
the model, and that seems to work a little better. And I also guessed the
magnetizing inductances shown in this simulation, but I used measured values
for my previous simulations for the toroid transformer at 2 kHz.
There's usually not much calculus required, it's usually just basic
algebra, with a little trig thrown in.

Those are some excellent references. You're right, it's not that hard to
understand. But it will take some time to grasp all the pros and cons of
various topologies.
DIYers may try to use readily available subassemblies and materials
from similar, if not directly related applications. It's just as
important to understand the potential and limitations of these
materials as it is when developing from scratch.

Yes, but it's probably a good idea to see what is commonly available, such
as the cores and bobbins I have seen on eBay. I have some ferrite cores and
bobbins that I picked up from who knows where, and even where the parts that
have markings I've had a hard time finding data. For a much smaller (2W)
DC-DC transformer I was able to get samples from Lodestone Pacific and
Cosmo, but they have rather high minimum order levels.

I think there are two approaches to engineering and design, with one extreme
(perhaps the Tesla method) being a very careful and specific design process
which should produce a product that works pretty much as specified, to the
other extreme (perhaps the Edison method), where you might make 99 mistakes
running simulations and building actual units, and with good measurement
techniques and some experience and "instinct", coming up with a winner on
try #100. I admire Tesla, and others who can use a very solid theoretical
approach, but I find the Edison method more to my liking.

Thanks,

Paul
 
L

legg

Jan 1, 1970
0
"legg" wrote in message




There's an interesting thread in the DIYelectricCar forum that shows how
much battery lead and motor lead wiring inductance and resistance can affect
the waveforms and operation of a rather simple but high-power PWM DC
traction motor controller. I tried to give some advice, but I think much of
the difficulty is the OP's lack of understanding as well as poor wiring and
measurement techniques:
http://www.diyelectriccar.com/forums/showthread.php/open-revolt-igbt-driver-blew-igbts-74629p8.html

Did you actually try either of the suggestions in your model?
The transformer design seems to be the major problem, especially at higher
frequencies. I need to rethink my original method of using thicker wire, and
go to a bifilar winding with multiple smaller strands in parallel. But I
don't know just how to determine leakage inductance, and I'm not sure if my
LCR meters are good enough to measure it after building one. I just guessed
at the 0.99 for the coupling. I know everything works better if I set it to
1.00, but that's unrealistic. I have sometimes added external inductance to
the model, and that seems to work a little better. And I also guessed the
magnetizing inductances shown in this simulation, but I used measured values
for my previous simulations for the toroid transformer at 2 kHz.
Rest assured, both magnetizing and leakage inductance are directly
measurable, using basic inductance meters, or indirectly, using simple
calculations based on recorded transient current waveforms, at easily
developed power levels. Their ratio produces the coefficient of
coupling required for more accurate simulation at higher power levels.

An unaltered winding pair will have the same leakage inductance, with
respect to each other, regardless of the core material or other
external environmental factors.

The effects of leakage on power transfer and Di/Dt is most easily
demonstrated in low power flyback circuits.

http://www.ti.com/lit/ml/slup078/slup078.pdf

The same Di/Dt limitation occurs in power transfer where the winding
polarity and direction of current flow is expected to reverse.

The point is - if your leakage is mistakenly made artificially high or
low in the simulation, you'll get effects that aren't reproduceable in
real life. Choosing a high coupling coefficient should produce low
leakage in the simulation - but by picking an unrealistically high
magnetizing inductance, you also ballooned the associated leakage term
out of the ballpark for a low turns count, high frequency
construction.

Yes, but it's probably a good idea to see what is commonly available, such
as the cores and bobbins I have seen on eBay. I have some ferrite cores and
bobbins that I picked up from who knows where, and even where the parts that
have markings I've had a hard time finding data. For a much smaller (2W)
DC-DC transformer I was able to get samples from Lodestone Pacific and
Cosmo, but they have rather high minimum order levels.
Look for dead equipment that previously performed at roughly the same
high frequency power level. This stuff is marketed by weight as
non-ferrous scrap. You're looking for re-usable core assemblies.
Preformed bobbins aren't often used at this power level - ground
insulation and formers being constructed as required.
I think there are two approaches to engineering and design, with one extreme
(perhaps the Tesla method) being a very careful and specific design process
which should produce a product that works pretty much as specified, to the
other extreme (perhaps the Edison method), where you might make 99 mistakes
running simulations and building actual units, and with good measurement
techniques and some experience and "instinct", coming up with a winner on
try #100. I admire Tesla, and others who can use a very solid theoretical
approach, but I find the Edison method more to my liking.

Thanks,

Paul

The issue here is the
 
F

Fred Abse

Jan 1, 1970
0
The transformer design seems to be the major problem, especially at higher
frequencies. I need to rethink my original method of using thicker wire,
and go to a bifilar winding with multiple smaller strands in parallel.

AKA litz wire. Suggested by many already.
But
I don't know just how to determine leakage inductance,

I've told you once...
and I'm not sure if
my LCR meters are good enough to measure it after building one.

What are they? What specification? You might be pleasantly surprised. Most
commercial LCR meters should be up to the job.
I just
guessed at the 0.99 for the coupling. I know everything works better if I
set it to 1.00, but that's unrealistic. I have sometimes added external
inductance to the model, and that seems to work a little better. And I
also guessed the magnetizing inductances shown in this simulation, but I
used measured values for my previous simulations for the toroid
transformer at 2 kHz.

Don't guess - measure.

I think there are two approaches to engineering and design, with one
extreme (perhaps the Tesla method) being a very careful and specific
design process which should produce a product that works pretty much as
specified, to the other extreme (perhaps the Edison method), where you
might make 99 mistakes running simulations and building actual units,
and with good measurement techniques and some experience and "instinct",
coming up with a winner on try #100.

How do you know that try #100 is the optimal solution, without calculation?
I admire Tesla, and others who can
use a very solid theoretical approach, but I find the Edison method more
to my liking.

Whose electrical distribution system is almost universally used today?

Edison's, or Tesla/Westinghouse ?
 
P

P E Schoen

Jan 1, 1970
0
"legg" wrote in message
Did you actually try either of the suggestions in your model?

I tried the 50 nH in series with the battery with minimal observed change. I
also rewound the ferrite core transformer I plan to use as a first
approximation to see what to expect. The core is about 2" square and 1/2"
thick. I have two layers of 36 turns #16 AWG each followed by two bifilar
windings each consisting of 3 parallel windings of #16 AWG. So the total 72
turn winding is 19.95 mH and the six turns reads 0.10 mH. It should be a
12:1 ratio but the ratio of the square roots of the inductance comes to
14.14. Probably an error in the measurement.

But previously I read 8.38 mH for the 72 turns, so either there was more of
a gap previously or there had been some shorted turns. I had used 10 turns
of #12 AWG and I had to squash it to fit the core around it.

So I'm hoping to get 5 to 10 volts per turn at 50 kHz, and with 12 V P-P
square wave on the 3 turn primary I should get about 288 V P-P on the
secondary. I figure the transformer has 3.8 uH/sqrt(turns) so 3 turns should
be about 35 uH. That should be about 11 ohms at 50 kHz so I'll have about 1
amp magnetizing current. Since I expect up to 50 amps at 12V for 600 watts
that's only 2% so it seems OK. This is where I usually just put it on the
test bench and run the voltage up and see where the current starts rising
faster than voltage and shows saturation. And I can also look at the current
waveform. Otherwise I'd need to go through the calculations, and since I
don't really know what material this is I still have to wing it.
Rest assured, both magnetizing and leakage inductance are directly
measurable, using basic inductance meters, or indirectly, using simple
calculations based on recorded transient current waveforms, at easily
developed power levels. Their ratio produces the coefficient of
coupling required for more accurate simulation at higher power levels.

I do have a better LCR meter with a 10kHz signal, but I haven't used it for
awhile. I realize I can measure the magnetizing and leakage inductance but I
wasn't sure how to calculate it by the physical construction of the
transformer.

Does a coupling factor of 0.99 mean that the leakage inductance is 1% of the
magnetizing inductance? And is it analogous to the regulation of the
transformer? Our high current 60 Hz transformers typically have a regulation
of 5-10% which means that they will put out 20x to 10x of their normal
rating into a short, which is essentially how we use them. However, the open
circuit current draw is probably 1/10 that at the normal output current, so
that would indicate the leakage inductance would be about 1% of the
magnetizing inductance.

For instance, we may have a transformer rated at 480V input and 4.8 volts
output at 1000 amps. The open circuit current draw might be 1 amp, while it
would draw 10 amps at its rated 4.8 kVA output, and 100 amps into a short
circuit. Thus the magnetizing inductance would be 785 mH. The leakage
inductance would be 7.85 mH. Does this sound about right?
An unaltered winding pair will have the same leakage inductance, with
respect to each other, regardless of the core material or other
external environmental factors.
The effects of leakage on power transfer and Di/Dt is most easily
demonstrated in low power flyback circuits.

The same Di/Dt limitation occurs in power transfer where the winding
polarity and direction of current flow is expected to reverse.
The point is - if your leakage is mistakenly made artificially high
or low in the simulation, you'll get effects that aren't reproducible
in real life. Choosing a high coupling coefficient should produce low
leakage in the simulation - but by picking an unrealistically high
magnetizing inductance, you also ballooned the associated leakage
term out of the ballpark for a low turns count, high frequency
construction.
Look for dead equipment that previously performed at roughly
the same high frequency power level. This stuff is marketed by
weight as non-ferrous scrap. You're looking for re-usable core
assemblies. Preformed bobbins aren't often used at this power
level - ground insulation and formers being constructed as required.

For one-off designs that's a good idea, but I want to be able to order the
right materials so that once it works, it will be reproducible and
manufacturable. The cores don't seem to be terribly expensive. But maybe
it's useful to see how such transformers are made.

I wish I had the time and energy to devote to learning all the details of
such designs, but I have many more irons in the fire and I need to
concentrate on those, where I know a bit more what I'm doing and mostly I
just need to attend to some details.

Thanks for everyone's help.

Paul
 
L

legg

Jan 1, 1970
0
"legg" wrote in message

I tried the 50 nH in series with the battery with minimal observed change. I

You should se a 20Vppk waveform on 'in' and primary current exhibiting
a dual slope. V'in' will show up on the driven end of L1.
also rewound the ferrite core transformer I plan to use as a first
approximation to see what to expect. The core is about 2" square and 1/2"
thick. I have two layers of 36 turns #16 AWG each followed by two bifilar
windings each consisting of 3 parallel windings of #16 AWG. So the total 72
turn winding is 19.95 mH and the six turns reads 0.10 mH. It should be a
12:1 ratio but the ratio of the square roots of the inductance comes to
14.14. Probably an error in the measurement.

But previously I read 8.38 mH for the 72 turns, so either there was more of
a gap previously or there had been some shorted turns. I had used 10 turns
of #12 AWG and I had to squash it to fit the core around it.

With a magnetic Xsection of 144mm, estimated for a core of this size
(eg E40/16/12), your 50KHz drive waveform on a three turn winding
produces core flux excursions of +/-140mT, and typical total core
losses of 1.4W. This will vary with input voltage, as the circuit is
unregulated.

When fully wound, this core's surface temperature will rise 50degC
under a total loss burden of ~4.2W in free air.
So I'm hoping to get 5 to 10 volts per turn at 50 kHz, and with 12 V P-P
square wave on the 3 turn primary I should get about 288 V P-P on the
secondary.

With a 24V source, the drive voltage is approximately 24Vppk,
approximately 12Vpk. It's the peak voltage that is produced on the
full wave output rectifier, but only if the total input voltage is
reflected accurately.

Look at the output voltage of your simulation, before the choke.
You'll see that the voltage there only goes positive about a third of
the conversion period. The rest of the time, the voltage is dominated
by the leakage inductance of the simulated transformer during phase
reversal. This loss of conduction period shows up as reduced filtered
output voltage, in spite of expectations due to turns ratio.

This is mostly the effect of leakage inductance occuring in your
model.

While the effect is real, the scale of this effect in your simulation
is masking realistic performance.

RL
 
P

P E Schoen

Jan 1, 1970
0
"legg" wrote in message
You should se a 20Vppk waveform on 'in' and primary current
exhibiting a dual slope. V'in' will show up on the driven end of L1.

Well, V(in) is more like a distorted sine wave with peaks of 27V and valleys
of 20V. And it does form the upper waveshape of the driven end of L1, so I
can see where battery lead inductance is a major factor.

I was a bit surprised at how much inductance a length of wire can have. I
used an inductance calculator and found that a 36" length of battery cable
0.25" diameter has 1025 nH of inductance.
http://www.consultrsr.com/resources/eis/induct5.htm

But when I used that in the simulation it actually seemed to improve the
operation. V(in) varies from 25.5 to 20.5 volts (looks like a rectified sine
wave) and the DC output actually seems to increase. The peaks seem to be
shifted to the center of the conduction cycle and the current in the primary
L1 looks almost like a sine wave.
With a magnetic Xsection of 144mm, estimated for a core of this
size (eg E40/16/12), your 50KHz drive waveform on a three turn
winding produces core flux excursions of +/-140mT, and typical
total core losses of 1.4W. This will vary with input voltage, as
the circuit is unregulated.
When fully wound, this core's surface temperature will rise
50degC under a total loss burden of ~4.2W in free air.

Sounds reasonable. Do you know of a calculator that can obtain these
figures? The following seem to be pretty good:
http://www.bcae1.com/trnsfrmr.htm
http://www.smps.us/magnetics.html
http://www.epcos.com/web/generator/Web/Sections/DesignSupport/Tools/Ferrites/Page,locale=en.html
With a 24V source, the drive voltage is approximately 24Vppk,
approximately 12Vpk. It's the peak voltage that is produced
on the full wave output rectifier, but only if the total input
voltage is reflected accurately.
Look at the output voltage of your simulation, before the
choke. You'll see that the voltage there only goes positive
about a third of the conversion period. The rest of the time,
the voltage is dominated by the leakage inductance of the
simulated transformer during phase reversal. This loss of
conduction period shows up as reduced filtered output
voltage, in spite of expectations due to turns ratio.
This is mostly the effect of leakage inductance occuring
in your model.
While the effect is real, the scale of this effect in your
simulation is masking realistic performance.

With the higher battery lead inductance of 1025 nH, the voltage at the
output of the bridge only briefly drops to a minimum of 89V, has a peak of
413V, an average of 306V, and RMS of 315V. I get input power of 1.03 kW and
output of 939W for an efficiency of 91%.

With an (unrealistic) lead inductance of 1 nH, the input power is 963 W and
output is 872 W, for 90.5% efficiency. It is interesting and useful to know
that realistic battery lead inductance may actually help the operation. I'm
still using the 0.99 coupling factor.

Thanks for the tips. I can see that, at these power levels, everything needs
to be modeled as accurately as possible. But in the end I will still need to
build it and test it.

I still don't know what the problems are for the OP in the thread:
http://www.diyelectriccar.com/forums/showthread.php/open-revolt-igbt-driver-blew-igbts-74629p9.html

It may very well be battery and motor lead inductance, which should be
minimized by using twisted or bundled pairs. But I think the main problem is
measuring the waveforms using a cheap USB scope with long, unshielded leads
within a giant loop that may be seeing current surges of 100 amps or more at
8 KHz.

I'm trying to give advice on ways to check what's really happening and ways
to reduce the problem, but I think there is a lack of understanding and
experience. Maybe on my part as well, but I have encountered similar bogus
waveforms and I have been able to reduce the effects considerably by keeping
measurement leads tightly twisted and outside of the magnetic loop.

Paul
 
L

legg

Jan 1, 1970
0
"legg" wrote in message


Well, V(in) is more like a distorted sine wave with peaks of 27V and valleys
of 20V. And it does form the upper waveshape of the driven end of L1, so I
can see where battery lead inductance is a major factor.

I was a bit surprised at how much inductance a length of wire can have. I
used an inductance calculator and found that a 36" length of battery cable
0.25" diameter has 1025 nH of inductance.
http://www.consultrsr.com/resources/eis/induct5.htm

But when I used that in the simulation it actually seemed to improve the
operation. V(in) varies from 25.5 to 20.5 volts (looks like a rectified sine
wave) and the DC output actually seems to increase. The peaks seem to be
shifted to the center of the conduction cycle and the current in the primary
L1 looks almost like a sine wave.

It's possible that the disparity is due to viewing different time
frames. I was looking at around 1.5mS, where there are still surge
influences. Things settle down under static conditions if you wait for
15mS. If loads were only static....and the simulation was remotely
accurate.....
Sounds reasonable. Do you know of a calculator that can obtain these
figures? The following seem to be pretty good:
http://www.bcae1.com/trnsfrmr.htm
http://www.smps.us/magnetics.html
http://www.epcos.com/web/generator/Web/Sections/DesignSupport/Tools/Ferrites/Page,locale=en.html
A pencil and paper are quicker, and more portable. Was off topic here,
originally thrown off by a reference to measuring 6 turns on LV
primary - you meant 3 turns, which made more sense, but by the time I
figured that out....
With the higher battery lead inductance of 1025 nH, the voltage at the
output of the bridge only briefly drops to a minimum of 89V, has a peak of
413V, an average of 306V, and RMS of 315V. I get input power of 1.03 kW and
output of 939W for an efficiency of 91%.

With an (unrealistic) lead inductance of 1 nH, the input power is 963 W and
output is 872 W, for 90.5% efficiency. It is interesting and useful to know
that realistic battery lead inductance may actually help the operation. I'm
still using the 0.99 coupling factor.

Thanks for the tips. I can see that, at these power levels, everything needs
to be modeled as accurately as possible. But in the end I will still need to
build it and test it.

You know that Lp and Ls can swing simply due to micro-gap quality /
cleanliness of core butt joints etc... Leakage inductance doesn't.
If you use the coupling coefficient to set leakage inductance, as the
simulator does, it WILL swing just as wildly as the Lp being used in
the simulation.

The relationship used by the simulation is

Llk= (1-k)Lm , where

Llk is the leakage inductance seen in one winding when the other
winding is shorted.
Lm is the magnetizing inductance of same single winding.
k is the coupling coefficient.

Note that leakage inductance effects in the secondary use Lm and Lk
measured on the secondary winding, with the primary being opened or
shorted, as required. While the two leakage terms are normally related
by the usual N^2 factor, low voltage structures' lead-out effects can
be signifigant, as they form part of the turn structure and are often
missing from the measurement.

One last thing, in a full wave rectifier fed by near 100% duty, stress
on the filter inductor is usually pretty small. Even so, in this
simulation the current zeros during the phase change. This means you
should probably check for core loss in the filter choke, before sizing
it.

RL
 
Top