Continue to Site

# How to improve the efficiency of the Class-E DC-DC converter circuit

Status
Not open for further replies.

##### Member level 3
Hello,

I am working on the Class-E DC-DC converter circuit. The efficiency of the circuit is 91% when the circuit simulates with ideal transformer and the 40% efficiency yielding when the circuit simulates with the practical transformer.

As per my knowledge, here the Zero Voltage Switching (ZVS) plays a crucial role in order to get the high efficiency in the Class-E converters.

When comparing the Vds and Vgs waveforms of the ideal and practical transformers are different. The peak of the Vds is high in the practical one when comparing with the ideal. In the Ideal waveforms, the Vds waveform is start to rise after immediate the Vgs (MOSFET) to zero voltage and end the Vds waveform almost Vgs (MOSFET) is ON. In the practical waveforms, the Vds waveform is start to rise after immediate the Vgs (MOSFET) to zero voltage and end the Vds waveform in the middle of Vgs zero voltage then after some time the Vgs (MOSFET) is ON.
So, because of this ZVS the efficiency of the converter is low? If it is the major problem, how to over come this problem?
(or)
Is there any parameters affecting on the circuit?
How to reduce the peak of Vds voltage?
How to improve the efficiency of the circuit with practical transformer?

Here, I have attaching the circuit simulation schematic and waveforms.

try lower Rds on mosfets with lower gate charge, try a 45% duty cycle, try increasing the resonant freq of the ckt so the mosfet turns off as the current rings down to 20% of peak...

If I understand correctly, the only change you made is due to the transformer model? What is the magnetizing inductance of P1?

Neither of those waveforms look like a well tuned class E. The first image (the practical one?) has the FET conducting in its third quadrant for a long time, probably because the circuit is underdamped. eGaN FETs have high losses in that quadrant so it should be avoided, either by changing the tuning or the duty cycle of the drive waveforms. Much of the losses are also going to occur in that magnetizing shunt resistor R8.

The second set of waveforms (the "ideal" one?) is overdamped, and has switching with Vds much larger than zero. It should be retuned a bit.

Also the EPC2012 is only rated to 200V, but you're pushing up against that limit already and breaking it completely with the "practical" circuit. Might want to try the EPC2025. Are you using the device models provided by EPC?

- - - Updated - - -

try lower Rds on mosfets with lower gate charge, try a 45% duty cycle, try increasing the resonant freq of the ckt so the mosfet turns off as the current rings down to 20% of peak...
Unllikely, the EPC2012 has possibly the best figures of merit for this type of application for 200V devices. I use it at frequencies over 100MHz. If you find another one available to purchase, I'd love to hear about it.

Hello mtwieg,

Magnetizing inductance means primary inductance of the transformer. If I understand correctly, the value of magnetizing inductance is 6.2uH.

If I use the EPC2025 also the pack of Vds value is 400V with out placing the shunt capacitor parallel to the MOSFET. If I placed the shunt capacitor (110pF) parallel to the MOSFET then the Vds value comes to the 300V around. But, the circuit is running with Zero Voltage Switching (ZVS) and the efficiency is too low (40%).

In this case, Is it the right one to choose the EPC2025 MOSFET because the Vds is touches to 300V. Otherwise, Is there other MOSFET which is with stand at the voltage of 300V?

How to improve the efficiency of the circuit? Please, can you tell me what is the problem with my circuit and how to solve that problem.

The peak Vds should be roughly Vin*pi, if the drain waveform is approximately a half sinewave. This is because the average voltage across the input choke inductor must be zero, and therefore the average Vds must be equal to Vin.

The reason you are seeing higher voltages is because of the poor tuning. The drain waveform is resonating with a frequency much higher than the drive frequency, so you're getting a narrower pulse which must be much higher in amplitude in order to have its average value be the same.

I roughly recreated your practical circuit and am getting around 90% efficiency. I used a 0.1ohm ideal switch with Coss=100pF for the FET, and ideal diodes, and assumed Lsec was 500nH, and adjusted the frequency to around 5MHz. As expected, most of the losses are in R8.

The frequency has to adjusted to within 10% to get decent efficiency, I suggest you start by varying that.

Hello mtwieg,

Magnetizing inductance means primary inductance of the transformer. If I understand correctly, the value of magnetizing inductance is 6.2uH.

.

You mean magnetizing current.

The magnetizing current's imaginary term is indeed inductance. But the real term, that which causes power losses, are the core and wire losses.

Most likely you are operating the transformer above its saturation flux density.

The frequency has to adjusted to within 10% to get decent efficiency, I suggest you start by varying that.

Hello mtwieg,

I have changed the frequency within 10%, but there is no that much changes in the efficiency. Just the efficiency is increased from 41% to 47% at the 5.1Mhz.

So, now I am planning to concentrate on core and copper looses at the transformer. Do you think is it make sense?

According to my circuit, How to know the primary and secondary resistances of the transformer in the copper losses?

Hello mtwieg,

I have changed the frequency within 10%, but there is no that much changes in the efficiency. Just the efficiency is increased from 41% to 47% at the 5.1Mhz.

So, now I am planning to concentrate on core and copper looses at the transformer. Do you think is it make sense?

According to my circuit, How to know the primary and secondary resistances of the transformer in the copper losses?
I used the same resistances and parasitics as those you showed, and got ~90% efficiency. I don't use multisim, so I can't check your simulation directly. But I'm sure the transformer isn't preventing you from getting good efficiency. Your problem is still probably just bad tuning. You should aim to have waveforms looking more like your ideal circuit simulations, with Vds touching 0V right at turn on, and the slope of Vds being near zero as well.

5.1 Mhz, this is critical information

What core material are you using?
Are you using Litz wire?

From what I understand he doesn't have any physical system, just simulations. At some point transformer design will be an issue, but for now he/she is just trying to get the simulation working.

Anyways Litz wire won't be useful at 5MHz.

So what sort of wire would you use then?

Solid magnet wire, or maybe coaxial cable.

You mean multiple strands of solid magnet wire?

One per winding, so three in total for a primary and split secondary. For very high frequency resonant converters, many rules of thumb from hard switched converters don't apply. You don't care much about leakage, proximity losses are much more important.

I have played some with those EPC FETs (designing a
very high frequency capable driver, at my last straight
job). I found that their switching behavior on the high
side depends greatly on the source impedance (kind
of a "Duh!", but still). The gate-source charge
displacement current needs somewhere to go, and
quick. Point being that you may need to lead the
desired turnoff and switch the gate before Vds=0 to
get clean minimally-dissipative switching and no
"braking".

I once worked on some derivatives of Vicor proprietary
parts which used a -Near- Zero Current switching scheme
by creating a leading drive waveform, by feedback. It's
hard to servo a one sided loop against zero, better to
have a small but tolerable pedestal to make things two
sided.

Now I will observe that while the 50% duty cycle case
is a good enough place to start, and is where RF guys
always want to sit, this has little to do with a wide
range (Vin, Iout) DC-DC converter. Try working at
minimum pulse width and maximum pulse width that
are appropriate to your range of operation, and you
will find additional challenges relating to narrow pulse
operation. So much so, that I'd recommend spending
functions at all.

My other bit of advice is, to decompose the efficiency
to its component -inefficiency- terms. You can't get
useful pespective from the rollup, but looking to the
various inefficiencies will immediately tell you where
your efforts are best spent. Presuming that you have
a good analytical grip on these things and the numbers
are worth believing.

I used the same resistances and parasitics as those you showed, and got ~90% efficiency. I don't use multisim, so I can't check your simulation directly. But I'm sure the transformer isn't preventing you from getting good efficiency. Your problem is still probably just bad tuning. You should aim to have waveforms looking more like your ideal circuit simulations, with Vds touching 0V right at turn on, and the slope of Vds being near zero as well.

Have you used Ideal or practical transformer in order to simulate the circuit?
If you used Practical one which core you selected ?
Which simulation tool have been used ?

In my case, I have used the 4F1 ferrite core material of the transformer. Below I have attached the core details...**broken link removed**

If not using those parameters, now add them into the circuit and simulate then see how much the efficiency is it...

- - - Updated - - -

What core material are you using?

I have used the 4F1 ferrite core material of the transformer.

I get an invalid link when I try to look at that 4F1 core
info.

I used the same resistances and parasitics as those you showed, and got ~90% efficiency. I don't use multisim, so I can't check your simulation directly. But I'm sure the transformer isn't preventing you from getting good efficiency. Your problem is still probably just bad tuning. You should aim to have waveforms looking more like your ideal circuit simulations, with Vds touching 0V right at turn on, and the slope of Vds being near zero as well.

As far now, The results of the circuit is Vout = 16.225, Iout = 1.154 and Vin = 60, Iin = 0.441. So, the efficiency is 70%
If I decrease the input current to 0.350m with out changes in the output voltage and current, then the efficiency is more high.
So, how you can do this in the circuit ? If I want to tune which one have to tune?

Have you used Ideal or practical transformer in order to simulate the circuit?
If you used Practical one which core you selected ?
I'm using the circuit you show in your attachments. I don't see any core model in there, I assume you are using simple resistors to approximate core and copper losses (R8 and R6).
Which simulation tool have been used ? [/quote]LTspice.

- - - Updated - - -

As far now, The results of the circuit is Vout = 16.225, Iout = 1.154 and Vin = 60, Iin = 0.441. So, the efficiency is 70%
If I decrease the input current to 0.350m with out changes in the output voltage and current, then the efficiency is more high.
So, how you can do this in the circuit ? If I want to tune which one have to tune?

What do your drain waveforms look like now? dick_freebird suggested that you search for the power losses in the circuit, I suggest you do that to determine whether it's the transformer or the FET.

Take a look at the figures at the end of this document. They show some simple guidelines for tuning class E amplifiers. Since your load is a rectifier instead of a simple resistance, the tuning method isn't identical but should still be close.

Last edited:

V
Points: 2
Hello mtwieg,

I have used the 4F1 core of the transformer. Now, I have changed to 3Mhz switching frequency of my circuit. I have tuned the components in the circuit in order to get the soft switching (ZVS). But, still the efficiency is 76% only. Here, I have used the two different types of the MOSFET's (i.e: EPC2025 and IPZ65R019C7) are used and see the results how it be. Please, can you tell me that how to improve the efficiency of the circuit.

When the circuit running with the EPC2025 MOSFET, Even the circuit satisfying the ZVS (zero-voltage switching) condition, the circuit efficiency is 76%.

When the circuit running with the IPZ65R019C7 MOSFET, the circuit not satisfying the ZVS (zero-voltage switching) condition (see in the waveforms), I have tune the component values as following the above mentioned document. So, how to satisfy this ZVS condition and how to improve the efficiency.

Here, I have attached the Circuit's and its wave forms.

Status
Not open for further replies.