How to improve efficiency of Full-Bridge SMPS?

Thread Starter

boruwkarz

Joined Nov 19, 2019
9
Hello, I am designing full-bridge SMPS with a linear voltage stabilizer in LTspice. When I was making measurements I discovered that the maximum efficiency of my power supply is around 30% at full load.

Project assumptions:
Input voltage: 230 AC
Output voltage: 0 - 25 V DC
Output current: 5 A (maximum)
Output power: 125 W (maximum) (I know Full-Bridge topology isn't the best fit for this power level)

I think the main problem with the low efficiency is that I have implemented an RC snubber circuit on the primary side of the transformer to prevent the voltage oscillations when turning transistors OFF.

Transformer inductance values:
L1 (primary) = 15 mH
L2 (secondary) = 0.15 mH

Switching frequency: f = 100 kHz

RC snubber values:
R_pararell = 100 Ohms
C_pararell = 10 pF

And I know why there is a lot of power dissipation, so I changed the values by increasing resistance up to 9k Ohms and capacitance to 100 pF. And then the maximum efficiency was around 75% at full load. This is much better.

However, with the RC snubber (9k, 100p) I cannot recieve good voltage regulation on the LC filter (on the secondary side of the transformer) because the turn off time is very long (I think due to lower current value) and that affects the duration of dead time (it is very well seen at low duty cycles ~ 10%). And that affects efficiency for lower output voltage values.

I am stuck with this problem and cannot think of any other solution how to:
1. Achieve better efficiency (I was hoping to get more than 85% or 88% at full load).
2. Achieve good voltage regulation by changing the duty cycle.
3. Prevent the voltage oscilations on the transformer (especially at low duty cycles).

Please find attached .asc file and the schematic of my power supply.

Feel free to ask any question you want,
Thank you for your help in advance.
 

Attachments

ArakelTheDragon

Joined Nov 18, 2016
1,350
1. Loose this "linear voltage stabilizer".
2. Reduce the frequency.
3. You can use the "LM2596" instead of an SMPS. It works on 150KHz built-in frequency. Of cource a transformer and bridge rectifier are mandatory before it. Check the datasheet of how they do it with "93%" efficiency.
 
Last edited:

Thread Starter

boruwkarz

Joined Nov 19, 2019
9
@ArakelTheDragon
The linear voltage stabilizer is mandatory is in the assumptions of my project.
Reducing the frequency means I would have to increase inductances of the transformer (It is okay to do it in the simulation but in the future I am planning to build the power supply, so the inductances should be quite low values in order to keep small transformer dimensions).
Also I have to measure the efficiency of this exact power supply, so measuring TI's step-down regulator doesn't solve my problem.

@ronsimpson
Oh, yeah. I'm sorry, should've put that information in the first post.
You can see the values of RC snubber by right clicking on the primary side inductance (L1) and there you can see the R and C values under "Pararell resistance" and "Pararell capacitance".

I was using the K = 1 value all the time, I didnt make any changes to that value.
I've attached .png with oscillations for 10% duty cycle and without RC snubber. However when I first occured the oscillations it looked much worse and I could count up to 20 overvoltages/oscillations (but back then I had lower transformer inductance values 500 uH and 5 uH).

On the plot you can see primary side voltage course (green one) and transistor driving signals (blue and red)

Thank you for your replies.oscillations.PNG
 

Thread Starter

boruwkarz

Joined Nov 19, 2019
9
----edited----
Is this what you are fighting? t=1mS??
No, by the oscillations I mean the course of the primary side voltage. They occour every time transistors are switched OFF (either High side or low side transistors). If you lower the output power and duty cycle you cou;d notice it much better.

Here is what I mean (the plot was made for very low inductances 100 uH and 1 uH) - blue primary side voltage
red/green - transistor driver signals.

oscillations100u.PNG

When I change the inductances to 15 mH and 0.15 mH, the oscillations are gone. But there appears one overvoltage every time the transistors are turned off, that causes problems with regulating voltage on the LC filter (the voltage keeps rising untill it reaches secondary side peak value) - that is the 1st factor of low efficiency and misses the whole point of applying LC filter since the voltage cannot be regulated.


osc15m.PNG
After applying RC snubber (here plot for the 100 ohms, 10p) the voltage on LC filter can be regulated almost "linearly" by changing the duty cycle, but the efficiency if VERY low (30% at full load). Notice the apperance of dead-time.

snubber.PNG

And I'm trying to acheive both: good efficiency (> 85% at full load) and linear or almost linear voltage regulation on LC filter by changing the duty cycle.

Thanks for help!
 

ArakelTheDragon

Joined Nov 18, 2016
1,350
Linear regulation is based on very low efficiency. The voltage over the transistors is because there is no freewheeling diode.

EDIT:
You can remove the regulation completely and use a transformer with a "bridge rectifier", then filter the voltage and add it to the transistors. It will increase your efficiency. Also SMPS use impulse transformers(hard to calculate). You are in need of creating an impulse transformer. If you need an SMPS with transistors, you can use the transistors to control the current and voltage based on the load. The "load" is very important. Its the first problem.


1. Impulse transformers.
 
Last edited:

ArakelTheDragon

Joined Nov 18, 2016
1,350
Here you can see a block diagram with explanations for an AC transformer power supply. The regulation is not done linearly, but the current is directly fed to the transistors.
 

ronsimpson

Joined Oct 7, 2019
807
I removed your RC.
The problem is at very low duty cycle you have moved to Discontinuous Mode. You need to have a duty cycle large enough to shift to Continuous Mode. In DM the transformer & filter inductor run out of power and ring. See how clean it is when the current in the filter inductor never drops to zero.
1577042159719.png
Also: D=4.2u gets to the right output voltage.
tr & ft are 20nS just because you can not have 0 in real life. (not important now)
1577042372455.png
 

ronsimpson

Joined Oct 7, 2019
807
I have used Switch Mode followed by linear. In your case 2V across the linear and 25 on the output. That is about 8% loss.

From my experience I would not go lower than 50khz. I like 100k to 250k. With a 300V supply it might be hard to run as fast as 250khz. At high frequency you need to watch your ac losses in the MOSFETs. I chose smaller parts to get the speed up and not fight internal capacitors. There is a trade off. DC losses and AC losses.
 

Thread Starter

boruwkarz

Joined Nov 19, 2019
9
@ronsimpson I was aware that I should always work in CCM, thats why at first I designed the converter so that the current in the LC filter inductor was constant for duty cycle equal to 10%.

Then I applied the Linear Regulator. It works okay, when the load current is high. But when the load current is low, then automatically inductance (L3) current went to DCM.

Can you post me your .asc file with the changes you applied?
What was the lowest duty cycle that you got CCM?

The LT1083 has a dropout voltage range from 1V to 1.3V at output currents so thats closer to 5%.

Thank you for your help :)

@ArakelTheDragon thank you for the links. I was aware of that but the link regarding impulse transformers had some new informations for me.
I'm not sure if I understood you correctly, but the IRF740 model has already built in reserve polarized diodes. Nevertheless I applied the "freewheeling diode" but It didn't change much, not for the low duty cycles nor for higher duty cycles.

Thank you guys,
Best regards.
 

MrAl

Joined Jun 17, 2014
7,748
Hello, I am designing full-bridge SMPS with a linear voltage stabilizer in LTspice. When I was making measurements I discovered that the maximum efficiency of my power supply is around 30% at full load.

Project assumptions:
Input voltage: 230 AC
Output voltage: 0 - 25 V DC
Output current: 5 A (maximum)
Output power: 125 W (maximum) (I know Full-Bridge topology isn't the best fit for this power level)

I think the main problem with the low efficiency is that I have implemented an RC snubber circuit on the primary side of the transformer to prevent the voltage oscillations when turning transistors OFF.

Transformer inductance values:
L1 (primary) = 15 mH
L2 (secondary) = 0.15 mH

Switching frequency: f = 100 kHz

RC snubber values:
R_pararell = 100 Ohms
C_pararell = 10 pF

And I know why there is a lot of power dissipation, so I changed the values by increasing resistance up to 9k Ohms and capacitance to 100 pF. And then the maximum efficiency was around 75% at full load. This is much better.

However, with the RC snubber (9k, 100p) I cannot recieve good voltage regulation on the LC filter (on the secondary side of the transformer) because the turn off time is very long (I think due to lower current value) and that affects the duration of dead time (it is very well seen at low duty cycles ~ 10%). And that affects efficiency for lower output voltage values.

I am stuck with this problem and cannot think of any other solution how to:
1. Achieve better efficiency (I was hoping to get more than 85% or 88% at full load).
2. Achieve good voltage regulation by changing the duty cycle.
3. Prevent the voltage oscilations on the transformer (especially at low duty cycles).

Please find attached .asc file and the schematic of my power supply.

Feel free to ask any question you want,
Thank you for your help in advance.

Hello,

I dont see any feedback in your circuit at all. Is it just that you dont want to simulate that yet?

When you use a linear with a switcher front end to get decent efficiency you have to regulate the output of the switcher section to always be equal to the output voltage plus the linear regulator overhead voltage. So say you want 24.00v output, and the linear regulator has 2v overhead, then you have to regulate the output voltage of the switcher to be 24+2=26 volts with a little extra like maybe 26.5 volts. This is necessary because the switcher has a variable output voltage with load and line with no feedback, and so you would have to set the output very high to make sure the linear always had enough voltage to provide the correct output voltage all the time. Having the output very high all the time results in very poor efficiency. Having it at just the right value (like 26.5v) means you get optimum efficiency at least due to that part of the design.

At 100kHz you have to pay close attention to the way the MOSFETs are driven. You might want to read up on that.
In close knit designs even the gate power is sometimes taken into consideration.

A note about simulators...
When you set the tr and tf to 0 (zero) the simulator may change that to some default value. Either check that to make sure it is really so, or set it to some value like 1ns. Actually you should set it to whatever the values are for whatever kind of driver you are going to use.
 
Last edited:

Thread Starter

boruwkarz

Joined Nov 19, 2019
9
Hello, I was about to make an update that I've dealt with the problem.
I assumed that the minimum output current will be 0.5 A, that solved the problems with the oscillations/overvoltages of the transformer voltage course and with the not-so linear voltage regulation.

The efficiency of the power supply (with the linear regulator) goes up to 90.5% at full load.
The efficiency of the converter (w/o the linear regulator) is in the range of 90% to 95% at every voltage/output power level.

I dont see any feedback in your circuit at all. Is it just that you dont want to simulate that yet?
I had in mind that the feedback will regulate the duty cycle regarding the output voltage (with added linear regulators' dropout voltage). I just didn't simulate it, made all measurements manually.

At 100kHz you have to pay close attention to the way the MOSFETs are driven. You might want to read up on that.
In close knit designs even the gate power is sometimes taken into consideration.
Yes, I know that. According to what you said and to what ronsimpson said the duty cycle that I could work with was in the range of 10% to 85% (0.5us to 4.25us per transistor). The lower limit was determined by the CCM mode of L3 inductor and the upper limit was determined by the dead-time appearance on the primary side voltage course.

A note about simulators...
When you set the tr and tf to 0 (zero) the simulator may change that to some default value. Either check that to make sure it is really so, or set it to some value like 1ns. Actually you should set it to whatever the values are for whatever kind of driver you are going to use.
Yes, when rise and fall time in pulse generator are set to 0 LTspice automatically sets default rise/fall time. In my case it is 55 ns.

Thank you all for the help and the time you spend to help me.
 

ronsimpson

Joined Oct 7, 2019
807
The LT1083 has a dropout voltage range from 1V to 1.3V at output currents so thats closer to 5%.
Worse case dropout is 1.5V at full current. But at the dropout voltage it will not regulate.
Most people will set the SMPS to 27V and the linear to 25V but I set the SMPS to regulate 2V across U1. When there is 2V across U1 FB=5V and that is what controls the SMPS.
1577137382754.png
 

Attachments

Top