Go Back   Home > Forums > Amplifiers > Solid State

Solid State Talk all about solid state amplification.

Please consider donating to help us continue to serve you.

Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving
Reply
 
Thread Tools Search this Thread
Old 5th December 2009, 07:55 PM   #1
diyAudio Member
 
Join Date: Nov 2009
Default How to do IMD simulation in LTspice!!!

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..
  Reply With Quote
Old 12th December 2009, 02:19 AM   #2
djoffe is offline djoffe  United States
diyAudio Member
 
Join Date: Oct 2008
Default IMD in LTSpice

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
  Reply With Quote
Old 14th December 2009, 09:33 PM   #3
diyAudio Member
 
Join Date: Nov 2009
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
  Reply With Quote
Old 14th December 2009, 10:46 PM   #4
diyAudio Member
 
Terry Demol's Avatar
 
Join Date: Apr 2002
Location: *
Quote:
Originally Posted by nicholas1113 View Post
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..
Quote:
Originally Posted by nicholas1113 View Post
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
  Reply With Quote
Old 15th December 2009, 03:01 AM   #5
jcx is offline jcx  United States
diyAudio Member
 
Join Date: Feb 2003
Location: ..
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

Last edited by jcx; 15th December 2009 at 03:03 AM.
  Reply With Quote
Old 15th December 2009, 03:52 AM   #6
djoffe is offline djoffe  United States
diyAudio Member
 
Join Date: Oct 2008
Default On the money...

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.
  Reply With Quote
Old 15th December 2009, 07:46 AM   #7
diyAudio Member
 
Join Date: Nov 2009
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
  Reply With Quote
Old 15th December 2009, 09:40 AM   #8
diyAudio Member
 
Join Date: Nov 2008
Location: Brazil
See this post:
Spice simulation
  Reply With Quote
Old 15th December 2009, 10:14 PM   #9
diyAudio Member
 
Terry Demol's Avatar
 
Join Date: Apr 2002
Location: *
Quote:
Originally Posted by nicholas1113 View Post
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
  Reply With Quote
Old 17th December 2009, 06:31 AM   #10
diyAudio Member
 
Join Date: Nov 2009
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
  Reply With Quote

Reply


Hide this!Advertise here!
Thread Tools Search this Thread
Search this Thread:

Advanced Search

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are Off
Refbacks are Off


Similar Threads
Thread Thread Starter Forum Replies Last Post
Distortion simulation with LTspice tiagor Solid State 32 22nd December 2012 09:33 PM
About LTSpice Simulation. nicholas1113 Solid State 2 15th November 2009 07:52 AM
LTSpice Simulation template?! ipop07 Tubes / Valves 5 13th May 2009 06:17 PM
LTSpice PSU simulation help - SoftStart modeling ninjanki Power Supplies 10 21st March 2005 04:04 PM
Ltspice.... mikeks Solid State 10 13th June 2004 08:10 PM


New To Site? Need Help?

All times are GMT. The time now is 02:59 AM.


vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2014 DragonByte Technologies Ltd.
Copyright 1999-2014 diyAudio

Content Relevant URLs by vBSEO 3.3.2