Author Topic: LT Spice THD + Noise ?  (Read 7171 times)

0 Members and 1 Guest are viewing this topic.

Offline WoodyBriggs

  • Newbie
  • Posts: 1
LT Spice THD + Noise ?
« on: January 21, 2015, 08:48:44 pm »
I have created a simple schematic for an amplifier in LT Spice, i was wondering if there is a way to compare the I/P Voltage vs O/P Voltage in terms of THD and Noise. I am very new to electronics and LT Spice so... I wont be expecting any answers more than "Google it."

Thanks
« Last Edit: January 22, 2015, 08:57:57 pm by WoodyBriggs »
 

Offline Jay_Diddy_B

  • Super Contributor
  • ***
  • Posts: 2160
  • Country: ca
Re: LT Spice THD + Noise ?
« Reply #1 on: January 21, 2015, 09:35:54 pm »
Hi,

Can you attach the LTspice model that you have to your post? The Forum does not allow you to attach .asc file. If you zip the file first you can attach the .zip file.

Regards,

Jay_Diddy_B
 

Offline Jay_Diddy_B

  • Super Contributor
  • ***
  • Posts: 2160
  • Country: ca
Re: LT Spice THD + Noise ?
« Reply #2 on: January 27, 2015, 11:19:05 pm »
Hi,

I didn't see that you added the model till today.

Here is the medication you need to do to the model and how to get the results:



Regards,

Jay_Diddy_B
 

Online Smokey

  • Super Contributor
  • ***
  • Posts: 1619
  • Country: us
Re: LT Spice THD + Noise ?
« Reply #3 on: January 28, 2015, 02:03:09 am »
You might want to pick up a copy of Bob Cordell's book.
http://www.amazon.com/Designing-Audio-Power-Amplifiers-Cordell/dp/007164024X

He goes through using LTspice for audio power amplifier design and analysis.  It's a really good book.
 

Offline krivx

  • Frequent Contributor
  • **
  • Posts: 763
  • Country: ie
Re: LT Spice THD + Noise ?
« Reply #4 on: January 28, 2015, 02:10:08 am »
Just something I've noticed - I think you need a longer transient simulation to get meaningful THD numbers. If you increase the time from 20ms to 200ms then THD increases to above 2%, which seems more realistic in this case. I'm not sure why LTSpice works this way but I suspect it's something to do with the DC voltage of the output settling to zero, the large 10u output cap might be making a slow time constant.

Harmonic   Frequency    Fourier    Normalized    Phase     Normalized
 Number      [Hz]      Component    Component   [degree]   Phase [deg]
    1      1.000e+03   8.557e-02   1.000e+00     179.42°       0.00°
    2      2.000e+03   6.684e-05   7.812e-04     120.80°     -58.62°
    3      3.000e+03   1.802e-03   2.105e-02      15.37°    -164.05°
    4      4.000e+03   5.373e-05   6.279e-04     155.64°     -23.78°
    5      5.000e+03   8.982e-05   1.050e-03      93.13°     -86.29°
    6      6.000e+03   4.121e-05   4.816e-04    -174.92°    -354.34°
    7      7.000e+03   3.739e-05   4.369e-04     129.73°     -49.69°
    8      8.000e+03   2.776e-05   3.244e-04    -150.11°    -329.53°
    9      9.000e+03   1.314e-04   1.536e-03     110.74°     -68.67°
Total Harmonic Distortion: 2.117315%(2.138807%)
« Last Edit: January 28, 2015, 02:12:52 am by krivx »
 

Offline Jay_Diddy_B

  • Super Contributor
  • ***
  • Posts: 2160
  • Country: ca
Re: LT Spice THD + Noise ?
« Reply #5 on: January 28, 2015, 03:16:18 am »
Krivx and the group,

The increase in distortion to around 2% by increasing the time 200ms can be explored in this experiment:



In this first test I have set the time to 200ms and the reported THD is 2.12%. The THD should be zero, since we are testing a pure sine wave source.


If I add a maximum time step limitation to the simulate command, to limit the maximum time to 0.1u, like this:



I get a more sensible result.

The increase in distortion comes from the limited number of points in the data collected during the simulation.

Regards,

Jay_Diddy_B
 

Offline krivx

  • Frequent Contributor
  • **
  • Posts: 763
  • Country: ie
Re: LT Spice THD + Noise ?
« Reply #6 on: January 28, 2015, 03:34:30 pm »
The difference seems to be mostly in the higher harmonics. Oddly enough, if you view the simulated time domain output in the original circuit it looks very similar in both cases, so a quick visual check is not good enough. It's a shame the .four command doesn't report the number of data points used and give warnings when higher harmonics can't be resolved accurately. Another simulation trap!
 

Offline f5r5e5d

  • Frequent Contributor
  • **
  • Posts: 349
Re: LT Spice THD + Noise ?
« Reply #7 on: January 28, 2015, 03:47:10 pm »
um guys - there is a fine graphical fft screen - you have to be something of a luddite to use .four today

with the graphical display you can see more evidence of settling, time step or windowing errors in the "noise" floor

THD as single lumped number is not too useful - looking at intermodulation from multi-tone stimulus in the graphical fft display can be more informative


I've never found the .noise analysis useful - the real issues are almost always noise sources not modeled in active devices


http://www.diyaudio.com/forums/software-tools/260627-installing-using-ltspice-beginner-advanced.html#post4031841 may be a useful intro ltspice for some
« Last Edit: January 28, 2015, 03:52:51 pm by f5r5e5d »
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf