THD in LTspice?

[mading2018]

Do anyone know how to check the THD (fft) in a easy way in LTspice?
When I press the FFT-button, I got this window popping up. What should I select there?

Maybe an alternative is to do this instead:
I found somewhere that you need to write a SPICE directive like this:
".fourier {Freq} V(output)"
and then open and check "the spice error log."
according to this source: https://www.diyaudio.com/forums/solid-state/177820-thd-ltspice.html

 

[MikeMl]

Read the "Waveform Arithmetic" topic in the help file. Note the discussion about .OPTIONS plotwinsize=0 numdgt=15. Add that to the schematic. Plot about five cycles of the waveform.

In the upper plot window, VIEW/FFT generates the FFT plot, which shows that the third harmonic is down 20db from the fundamental, which is what the two sources add to...

How to convert that to THD.

 

[alec_t]

I found somewhere that you need to write a SPICE directive like this:
".fourier {Freq} V(output)"
and then open and check "the spice error log."

That works, and is easy to do.

 

[unclejed613]

the spice directive should be put on the schematic. if you are using a 1khz tone to test your device, and your output node is marked "out", the correct way to type the spice directive is:
.fourier 1000 V(out)

after running the sim, open the spice error log, and you will get the overall thd, plus a list of the magnitudes of the harmonics

 

[mading2018]

the spice directive should be put on the schematic. if you are using a 1khz tone to test your device, and your output node is marked "out", the correct way to type the spice directive is:
.fourier 1000 V(out)

after running the sim, open the spice error log, and you will get the overall thd, plus a list of the magnitudes of the harmonics

Hmm, I may do something wrong, I don't find that list. I found this instead.

First I run the simulation by plotted Vout, then I took FFT of Vout, then I open the spice error log.

 

[MikeMl]

Without the .options statement. The .fourier statement has to refer to a node that actually exists in your schematic.

click:

This is with the .options statement. Notice how much cleaner the FFT is, and that is reflected in the error Log.

click:

 

[unclejed613]

and your output node is marked "out"

you missed that part... put a flag on your output called "out"

 

[tomizett]

I've recently been using this, and can't recommend it highly enough:

https://www.audio-perfection.com/au...mplitude-and-frequency-sweeps-in-ltspice.html

I believe the author was on this forum a while ago... in any case, they deserve a lot of credit for this. It's far easier then thinking about the measurements yourself, and is very well documented.

 

[mading2018]

Without the .options statement. The .fourier statement has to refer to a node that actually exists in your schematic.

click:View attachment 112779

This is with the .options statement. Notice how much cleaner the FFT is, and that is reflected in the error Log.

click:View attachment 112780

I still don't get it. I have added all the SPICE directives, and I can not see the anything in the error log it is just empty.

you missed that part... put a flag on your output called "out"

It is already named 'OUT'.

Can you please show me how you obtain the list from my file?

 

[MikeMl]

THD is meaningless in the context of the circuit you posted. Doing an FFT on the output ripple shows that it has horrible ripple fed through from the full-wave rectified AC. You dont even need to do the FFT, you can see it...

 

[alec_t]

I can not see the anything in the error log it is just empty

Did you wait for the sim to finish running before looking in the log?

Edit: To speed up the sim, edit the simulation command by ticking the 'Skip initial operating point solution' box.

Edit 2: Ignore that, since for some reason the 1248 doesn't oscillate if Skip is enabled.

 

[mading2018]

THD is meaningless in the context of the circuit you posted. Doing an FFT on the output ripple shows that it has horrible ripple fed through from the full-wave rectified AC

Ah, I see. Yeah you right. So it would be more appropriate to do a THD on the current input instead, just to see how good quality the input current is? Like they did here in the document.

 

[mading2018]

Did you wait for the sim to finish running before looking in the log?

No I did not, I changed the running time to 5 ms, and after I waited for the simulation to finish, I can now see the error log window with results

 

[mading2018]

THD is meaningless in the context of the circuit you posted. Doing an FFT on the output ripple shows that it has horrible ripple fed through from the full-wave rectified AC. You dont even need to do the FFT, you can see it...

Is it common to do a THD on AC current input instead? At the output, I think THD was very high...

 

[MikeMl]

Is it common to do a THD on AC current input instead? At the output, I think THD was very high...

THD is something that is measured in a hifi audio amplifier. You put in a perfect sine wave, at say, 1000Hz. You analyze the output waveform to see if the non-linearity in the amplifier has contaminated the output signal with harmonics of 1000Hz. This has nothing to do with what you are doing; namely evaluating how well filtered (compared to DC) the output of a switching regulator is.

 

[unclejed613]

THD measurements are usually done on audio systems, not power supplies. what you want to look at on a power supply output is the percentage of ripple, and that's a different measurement. if you have a 5V supply, and the ripple is 100mV, that's 2% ripple, which for most purposes is fine.

 

[mading2018]

THD measurements are usually done on audio systems, not power supplies

But how about the document that I posted in #12? There they check the THD for a charger..

 

[alec_t]

In that's what you're after, you could plot the supply input current and check for harmonics of the input frequency. Ideally, the input current will be perfectly in phase with the input voltage so, if the output load is a constant resistance and the PFC is 100% efficient, there would be no harmonics. In the real world that wouldn't happen .

 

[mading2018]

In that's what you're after, you could plot the supply input current and check for harmonics of the input frequency. Ideally, the input current will be perfectly in phase with the input voltage so, if the output load is a constant resistance and the PFC is 100% efficient, there would be no harmonics. In the real world that wouldn't happen .

Yes I expect some THD cause the PF can't be perfect as you say in the real world. So my input frequency is 50 Hz from the grid, but how do I select the input current in the FFT window?

--edit--
Oh, wait, is that "I(V4)" at the voltage source that I should use to get the input current? And how long should the running time be?

 

[mading2018]

Now I tested for 100 ms, but is it strange that I only got 9 harmonic numbers, tough I have 15?

--edit2--
Is it possible to obtain see the image "graph.png"? Is that possible in Spice ? If not, do anyone how I create a graph like that?
Or could I used "freq4A.png" or "THD.png" like a clear result. What do you suggest? Sorry that I have so many questions