How to do IMD simulation in LTspice!!!

[nicholas1113]

Hi Everyone,

Can anyone tell me how to simulate IMD in LT spice ?
For example THD need to put the command of .four 10K V(out) and how about IMD ? how should it be ?
Thank you for your advises..

[djoffe]

Put two input sources in series, say 19 kHz and 20 kHz, at the input to your device. Run a transient sim. Look at the output with the waveform viewer. Make sure that the waveform viewer is highlighted. Then click view...FFT. The not displayed in the oscilloscope will be highlited...pick a window...I like Hann...
say OK...you'll see the intermod of 19 and 20 kHz at 1 kHz (of course, there are other sum and difference frequencies, but this might be the most interesting one for audio work...)

Hope this helps...

Dan

[nicholas1113]

Hey Dan,
Thank you for giving me advice on it .. I have tried the way you u advised me and following is the diagram tat the Blameless circuit diagram, output waveform and FFT with IMD.
Is this correct?
Another question is the command written in this form ?
.fourier 1K 2K V(OUTPUT)
.options plotwinsize=0

12.JPG

14.JPG

13.JPG

[Terry Demol]

Originally Posted by nicholas1113

Hi Everyone,

Can anyone tell me how to simulate IMD in LT spice ?
For example THD need to put the command of .four 10K V(out) and how about IMD ? how should it be ?
Thank you for your advises..

Originally Posted by nicholas1113

Hey Dan,
Thank you for giving me advice on it .. I have tried the way you u advised me and following is the diagram tat the Blameless circuit diagram, output waveform and FFT with IMD.
Is this correct?
Another question is the command written in this form ?
.fourier 1K 2K V(OUTPUT)
.options plotwinsize=0

Attachment 150235

Attachment 150236

Attachment 150237

WRT Intermod simulations remember that to get an accurate result from the
simulator, each of the two sine waves must have completed full cycles and
not be truncated mid cycle. Ltspice will see the truncated cycle as
distortion and generate additional sidebands.

So for an IM sim on 19kHz and 20kHz the sim time will have to be
1/(20-19)kHz=1mS minimum. Depending on your PC and the accuracy
required this may take some time.

T

[jcx]

another useful point is to use relatively prime frequency ratios so IMD and Harmonic distortions don't all fall on top of each other

I usually use integer KHz values so that the waveforms will repeat every 1 mS, and usually run the sim for 5 mS so that Blackman windowing fully resolves the frequencies

I also never look at .four output - given modeling inadequacies I only belive sim is useful for some tests of relative distortion changes - to me numerical output like .four is harder to compare than .step or duplicated circuit fft plots

[djoffe]

JCX's advice is on the money...with the 1kHz and 2kHz you chose, you really can't tell the difference between harmonic and intermod distortion.

I also agree with JXC...waveform viewer based FFT is much more informative.

[nicholas1113]

I tried to simulate it in 19KHz and 20KHz. and the result it based on below.
But I still wondering the .fourier 19K 20K V(OUTPUT) is it the correct way to command it ?
15.jpg

[Rafael L]

See this post:
Spice simulation

[Terry Demol]

Originally Posted by nicholas1113

I tried to simulate it in 19KHz and 20KHz. and the result it based on below.
But I still wondering the .fourier 19K 20K V(OUTPUT) is it the correct way to command it ?
Attachment 150320

Can you post the .asc file

[nicholas1113]

Hey Terry Demol:
Sorry that i dun know how to post the .asc file ... i cannot add it into the attachment there .. invalid file .

My command for the IMD　.fouriｅｒ　１９Ｋ＋２０K, 50BW, V(output)
and it show below FFT diagram.

fft.JPG