6
\$\begingroup\$

I have a 10 seconds of sampled data. Sampling rate is 1kHz. I uploaded the text file which is a two column time vs voltage data; it can be downloaded here.

I performed FFT in MATLAB, Python and LTspice. MATLAB and Python agrees when I plot but I get different result in LTspice.

Here below is the code I use and the plot with MATLAB:

ts = 0.001; %sampling interval (sec) Fs = 1./ts; %sampling frequency (Hz) L = length(y); %number of samples complex = fft(y)/L; % complex signals f = 0 : Fs/L : Fs/2; % frequency bins amplitude = 2*abs(complex(1:L/2+1)); % amplitudes pow = (amplitude).^2/2*(L/Fs); % power semilogx(f,20*log10(amplitude),'-b'); grid on; xlabel('Frequency [Hz]') ylabel('dB')

enter image description here

Below is the code I use and the plot with Python:

plt.figure() y = v_in T = 1/sampling_rate N = len(y) yf = scipy.fftpack.fft(y) xf = np.linspace(0.0, 1.0/(2.0*T), N/2) amplitude = 2.0/N * np.abs(yf[:N//2]) pow = (N/sampling_rate)*amplitude*amplitude/2 plt.semilogx(xf, 20*np.log10(amplitude),'b') plt.grid() plt.xlabel('Frequency [Hz]') plt.ylabel('dB')

enter image description here

And finally I fed the signal from the text file to the signal generator in LTspice(by using PWL file option) and performed FFT and I get the following plot:

enter image description here

MATLAB and Python both show the max db point as -46.2dB but Ltspice shows this point as -49.3dB. This is not a very small difference.

What could be the reason for this difference? Am I doing something wrong in MATLAB and Python when evaluating FFT or LTspice is wrong?

\$\endgroup\$
5
  • 1
    \$\begingroup\$ The difference is suspiciously close to 3dB. Is there some different assumption about whether the power is single or two-sided? I always mistrust the scaling on any FFT I do, and run a calibration with synthetic data just to check what assumptions the FFT is making. \$\endgroup\$ Commented Apr 16, 2018 at 16:58
  • \$\begingroup\$ @Neil_UK I added a comment below that addresses this issue. \$\endgroup\$ Commented Apr 16, 2018 at 16:59
  • \$\begingroup\$ What window function did you use when doing the LTSpice FFT? \$\endgroup\$ Commented Apr 16, 2018 at 17:18
  • \$\begingroup\$ Window function set to "none" \$\endgroup\$ Commented Apr 16, 2018 at 17:19
  • \$\begingroup\$ Since I am after dB(power ratio) should I convert amplitude to rms always in a 20*log10(amplitude) formula? If you couple 1V amplitude sine wave to a scope, would the max FFT point of the scope show 1V or Vrms=0.7V? \$\endgroup\$ Commented Apr 16, 2018 at 17:41

2 Answers 2

Reset to default
7
\$\begingroup\$

Despite the fixed timings provided by the PWL file, LTspice is a SPICE engine, analog simulator, which means the simulation will not have even steps. In Matlab and Python, you can correctly account for the exact samples that are described in the definition. LTspice needs to simulate it, so, like all analog SPICE engines, it has an uneven time.

You could increase the timestep and/or add .opt plotwinsize=0, numdgt=15, which will improve the result. See if that helps.

[edit] However, no matter what you do, LTspice will show RMS values in the FFT window (unlike with the .four command).[/edit]

Here's my attempt by using the above (timestep 25u):

fft

Seems quite close to the Python version. In LTspice FFT I used 24000 points and set "Number of points" to 1 (polynomial smoothing).

\$\endgroup\$
7
  • \$\begingroup\$ These didn't make any change on mine. I added .opt plotwinsize=0, numdgt=15 and set "Number of points" to 1 at binomial smoothing. \$\endgroup\$ Commented Apr 16, 2018 at 17:07
  • \$\begingroup\$ If all you need to account for is the 3dB difference, then my first comment should do the trick: just multiply with sqrt(2). The rest are for a better resolution, that's all. \$\endgroup\$ Commented Apr 16, 2018 at 17:24
  • \$\begingroup\$ Yes when I do amplitude=amplitude/sqrt(2) in MATLAB and Python it matches to LTspice. But I dont get why. Something related to RMS. But where is the mistake I could not figure out. \$\endgroup\$ Commented Apr 16, 2018 at 17:26
  • \$\begingroup\$ @cm64 Well, now you know why. I don't know why Mike decided to make it like this, but that's how it is. It doesn't seem to be a big deal. After all, the .four command calculates the peak amplitudes. Go figure... \$\endgroup\$ Commented Apr 16, 2018 at 17:54
  • \$\begingroup\$ Please write these to your answer so I can select. Pls if you know also add what would a real scope show Vrms or Vamp. Thanks \$\endgroup\$ Commented Apr 16, 2018 at 18:00
0
\$\begingroup\$

In my view, LTSpice's FFT takes RMS value to calculate the spectrum of a signal. This is the reason why you have a 3dB discrepancy

\$\endgroup\$
1
  • \$\begingroup\$ If you'll read the answer and the comments, this has been addressed. Therefore what you wrote would be more appropriate as a comment, rather than an answer. \$\endgroup\$ Commented Feb 17, 2022 at 16:29

Start asking to get answers

Find the answer to your question by asking.

Ask question

Explore related questions

See similar questions with these tags.