Continue to Site

Welcome to EDAboard.com

Welcome to our site! EDAboard.com is an international Electronics Discussion Forum focused on EDA software, circuits, schematics, books, theory, papers, asic, pld, 8051, DSP, Network, RF, Analog Design, PCB, Service Manuals... and a whole lot more! To participate you need to register. Registration is free. Click here to register now.

Do you know roughly what is power factor of SMPS with this VAC and IAC input?

Status
Not open for further replies.
T

treez

Guest
Hi,
Its from LTspice, i know that its distortion factor * displacement factor but dont know how to extract the data from LTspice.
(this is mains input voltage and current to a flyback smps with only 1uF dc bus capacitor.)

I reckon its about 0.85...do you agree?
 

Attachments

  • Power factor of waveform.pdf
    1.1 MB · Views: 113

Power factor = P/S. Can you do that in LTSpice to your SMPS ?
Its from LTspice, i know that its distortion factor * displacement factor but dont know how to extract the data from LTspice.
Find out first harmonic of the current. FFT can help you out but I do not know if LTSpice can do it since I do not use LTSice.
 
  • Like
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
The strange thing is that in LTspice, the FFT of the input current makes the 50Hz fundamental come out as 82mA RMS. Now, the total RMS of this current is 165mA RMS. That means that the distortion factor is 0.5 .
Now its obvious that the fundamental of the current waveform is in phase with the mains voltage, therefore, the displacement factor is unity. That means that the power factor is just 0.5.
That doesn’t make sense, because the standard “Mains rectifier/big smoothing capacitor” power supply has a power factor of 0.6, and that has a mains input current waveform that is much more discontinuous than the shown current waveform.
So do you know why the power factor of the shown mains input is so low?
 

Use BV sources (arbitrary functions) to add in your missing pieces, instantaneous power in this case.


And/or you can add arbitrary expressions in the plot window as well.


The waveform has a large chunk of its current near the voltage zero crossing which is quite bad for power factor.
 
Last edited:

PF = real power/apparent power, really easy to measure in Ltspice.

Real power = power delivered by the sine source, apparent power = Irms*Vrms.
 

PF = real power/apparent power, really easy to measure in Ltspice
Thanks, though its easy to click and get the apparent power, LTspice certainly doesnt make it easy to get the real power.

- - - Updated - - -

The below are the schematic and the LTspice sim
 

Attachments

  • Flyback forum _fixed ipk.pdf
    39.9 KB · Views: 92
  • Flyback forum _fixed ipk.txt
    12.7 KB · Views: 60
  • Like
Reactions: asdf44

    asdf44

    Points: 2
    Helpful Answer Positive Rating
LTspice certainly doesnt make it easy to get the real power.
You certainly didn't think thoroughly.

Plot V(in)*I(in) in a second plane, display average.

I get real power of 45.38 W, apparent power of 77 VA, PF = 0,59.
 
  • Like
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
Thankyou, The waveforms of the power supply in the pdf described as "distortion factor 0.63" has a distortion factor of 0.63......that seems amazingly low given that it is an obvious improvement on a typical "Mains Rectifier/Big smoothing cap" type waveform. (as you know distortion factor = I1RMS/IRMS).
We are trying to get as near to 0.7 power factor as possible, but with as high smps bandwidth as possible.
 

Attachments

  • Distortion factor 0.63.pdf
    1.3 MB · Views: 43

Hello,
This LTspice simulation (attached) gives a power factor of 0.96 when done with the “Real Power/ Apparent power” method.
However, when you do the FFT of the mains input current in LTspice, the 50Hz component (fundamental) comes out as 99mA RMS. The overall RMS of the mains input current is 157mA. ..This means that the distortion factor is 0.63.
..And with a distortion factor of 0.63, the power factor couldn’t possibly be 0.96.
Do you know what’s gone wrong here? These are all measurements from LTspice.

Also attached is the mains I and V input waveforms. (its a offline flyback with little dc bus capacitance).
Also attached is the flyback schematic
 

Attachments

  • Flyback forum _SEMI PFC.TXT
    12.6 KB · Views: 128
  • Mains I and V waveforms.pdf
    733.8 KB · Views: 145
  • Schematic _Flyback.pdf
    39.5 KB · Views: 76
Last edited by a moderator:

Don't know how you performed the FFT, but you did it apparently wrong.
.four command reports power factor of 0.97.
 
  • Like
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
Don't know how you performed the FFT, but you did it apparently wrong.
To find the 50Hz component of I(V2), I clicked I(V2) in the waveform window, then clicked FFT, then the FFT dialog box came up, and I chose the number of points etc. Then it gives the dB value of the 50Hz component. (you find this by sliding the cursor over the FFT plot, then read it off). The dB value of the 50Hz component was -20.08dB.
This means that 20 * log(10) [ IRMS/1 Amp] = -20.08dB
From this, IRMS = 99mA.

.four command reports power factor of 0.97.
Surely the waveforms attached to post #9 couldn’t possibly be from a Power Factor of 0.97? The mains input current is nothing like sinusoidal.
The algorithm used to control the primary current was very very simple, and couldn’t surely of produced a power factor that high?
 
Last edited by a moderator:

To calculate components quantitatively, you can't use a windowed FFT as used by the waveform viewer.
.four command with 50 Hz fundamental is the correct method.

I agree that PF of 0.97 is surprising at first sight, but it's true. Consider that the error has to be squared to give the difference between apparent an real power. 17 percent harmonic current make only 3 % harmonic power.
 
  • Like
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
To calculate components quantitatively, you can't use a windowed FFT as used by the waveform viewer.
..Thanks but i tried it with simple 50hz current source and my method of post #11 works....it calculates the irms exactly...by conversion from dB as i described in post #11
 

It may work under circumstances, e.g. with a sufficient number of cycles. But you're surely aware of the fact that a correct FFT would show lines at mainly odd multiples of 50 Hz. That's not what the waveform viewer FFT looks like. You made it even worse by performing FFT not over an integer number of cycles.

But whatever the waveform viewer shows, you have two alternative methods that give both consistent measurements, average V(IN)*I(IN) and .four function. That should be pretty sufficient.
 

Thanks for your help on this..

Do you know how to interpret the results of the .four command in ltspice……
The attached LTspice offline flyback smps , when using the .four command for 50Hz , gives a spice error log which says harmonic number 1 is 50Hz and then says “Fourier component” is 0.2195.

What does the 0.2195 mean?

The RMS input current is 157mA
 

Attachments

  • Flyback SMPS.TXT
    12.6 KB · Views: 33

Do you know how to interpret the results of the .four command in ltspice……
The attached LTspice offline flyback smps , when using the .four command for 50Hz , gives a spice error log which says harmonic number 1 is 50Hz and then says “Fourier component” is 0.2195.

What does the 0.2195 mean?

The RMS input current is 157mA
I have no idea of the .four command and I do not use LTSpice. So the next is just a wild guess.

You gave me this hints:
  • .four command to 50 Hz
  • harmonic number 1 is 50 Hz
  • Fourier component is 0.2195

My guess is that it gives you the amplitude of that harmonic (as every FFT would do).

Verification: 0.2195/sqrt(2) = 155.2 mA (pretty close to your number).
 
  • Like
Reactions: treez

    T

    Points: 2
    Helpful Answer Positive Rating
Verification: 0.2195/sqrt(2) = 155.2 mA (pretty close to your number).

Thanks, i believe you have cracked it....the power factor is around 0.97 so the 50hz component would be expected to be just below the total irms input component
 

The below is related to this thread so i hope its OK to put it here....

Hello,
Is LTspice accurate in its Power Factor and FFT calculations as follows….?...

The attached shows mains input current and voltage waveforms for a PFC’d offline Buck converter.
LTspice simulation also attached.
From the simulator the Active input power is 56.6W. The Apparent power is 0.257A * 240V = 61.8W. Therefore, that would make the Power Factor equal to 0.92
Qu 1: Do you agree that this seems amazingly high for such a horrendously non-sinusoidal input current wave shape? Could there be some error in the LTspice calculation?
Using the LTspice FFT function on the current waveform, this gives -12.33dB for the magnitude of the 50Hz component. This FFT was taken using the Blackman-Harris function. The magnitude of the 50Hz component is therefore 10^(-12.33/20) = 242mA. The total RMS input current was 257mA, so from that the Power Factor = 0.242/0.257 = 0.94
…This agrees quite well with the value of 0.92 calculated further up the page..
For the FFT, the current waveform of the FFT calculation was between 10ms and 30ms (ie one mains cycle). However, the FFT, in order to be accurate, needs to be done over an infinite number of cycles, or at least, a very large number of cycles. If an FFT is done on a single mains cycle of current, then that is termed a “truncated” waveform, and its FFT cannot be representative of a continuous waveform of that period.
Qu 2: So how has the LTspice FFT function managed to be so accurate when it only considered a single cycle?
 

Attachments

  • Mains input current and voltage waveforms.pdf
    732.1 KB · Views: 105
  • Schematic Buck PFC LED driver.pdf
    32.5 KB · Views: 95

The Apparent power is 0.257A * 240V = 61.8W
It is VA by the way.
The magnitude of the 50Hz component is therefore 10^(-12.33/20) = 242mA. The total RMS input current was 257mA, so from that the Power Factor = 0.242/0.257 = 0.94
Where is the displacement factor?
 

Good point, i need to go back to LTspice and find out by what angle the 50Hz component is out of phase withthe actual 50hz voltage input.

It will take ages to run the sim again and do the FFT, but from memory i think it was 11 degrees out of phase with the 50hz voltage input...so the displacement factor is cos(11) = 0.98, and then the power factor comes out as 0.92

Once again, how has ltspice managed to do such an accurate fft with only one cycle?
 
Last edited by a moderator:

Status
Not open for further replies.

Similar threads

Part and Inventory Search

Welcome to EDABoard.com

Sponsor

Back
Top