SPICE distortion analysis - diyAudio
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 7th February 2008, 02:17 AM   #1
jgedde is offline jgedde  United States
diyAudio Member
 
jgedde's Avatar
 
Join Date: Dec 2006
Default SPICE distortion analysis

I have a stupid question... I realize that the SPICE distortion analysis is fanciful at best, but if I see an improvement in SPICE's distortion report when I change something, does that generally mean I would see an improvement in real life?

Thanks,
John
  Reply With Quote
Old 7th February 2008, 03:57 AM   #2
diyAudio Member
 
Join Date: Sep 2007
Send a message via Yahoo to linuxguru
Small changes (0.5-2 dB) in magnitudes of harmonics can be artefacts of rounding, precision, etc.; larger changes are usually real. The way I differentiate between the two is to continue varying the control input (resistor/capacitor value, etc.) in the same direction and see if the harmonic magnitude continues to follow in the same direction (usually a real effect), stays put or reverses (requires further investigation to determine if a local minimum/maximum has been encountered).
  Reply With Quote
Old 7th February 2008, 04:03 AM   #3
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
I would guess so. But a lot might depend on how good your modeling is.

Also, with good modeling, including parasitics and thermal effects, the calculated THD should be closer to reality.

I am only familiar with LTspice. And with that, you do have to make sure that the maximum timestep is set small-enough. You can simultaneously calculate the THD of your input, and make sure that the max timestep is small-enough that the input's THD is extremely small; almost zero for an ideal voltage source; maybe .000003% max.

With LTspice, it's also very important to turn off the data-compression features, in order to get reasonable THD calculations.
__________________
The electrolytic capacitors ARE the signal path: http://www.fullnet.com/~tomg/zoom3a_33kuF.jpg
  Reply With Quote
Old 7th February 2008, 05:40 AM   #4
diyAudio Member
 
Join Date: May 2007
Quote:
Originally posted by gootee
With LTspice, it's also very important to turn off the data-compression features, in order to get reasonable THD calculations.
That is: .options plotwinsize=0
  Reply With Quote
Old 7th February 2008, 08:26 AM   #5
diyAudio Member
 
jan.didden's Avatar
 
Join Date: May 2002
Location: Great City of Turnhout, Belgium
Blog Entries: 7
Quote:
Originally posted by revintage


That is: .options plotwinsize=0

I also understand that it is important to relate the frequency of the test signal, the simulation time and the FFT number of points to each other for max resolution. Do that wrong, and the results are meaningless, but if you do it right, the results are pretty reliable.

In the LTspice yahoo group files section there are several examples for this.

Jan Didden
__________________
If you don't change your beliefs, your life will be like this forever. Is that good news? - W. S. Maugham
Check out Linear Audio!
  Reply With Quote
Old 7th February 2008, 08:30 AM   #6
diyAudio Member
 
PigletsDad's Avatar
 
Join Date: Jul 2007
Location: South Worcestershire
Depending on your circuit and simulation setup, you may need to put a long settling period into the simulation, so that any startup transients can stabilise.

If you are using a small time step for good simulation accuracy, this can get very tedious.
  Reply With Quote
Old 8th February 2008, 04:57 PM   #7
diyAudio Member
 
unclejed613's Avatar
 
Join Date: Dec 2006
ive found that LTSice generally gets pretty close to reality. one thing you might do however is to introduce intentional mismatches in your resistor values, especially in diff amps, current mirrors and any symmetrical VAS or output stages. most resistor tolerances ar either 5% or 10%, so you'll never get a perfect match in real life. same goes for transistor betas, they vary quite a bit. electrolytic caps are usually rated at +20%/-10% tolerance. if you know how to edit the model files, you might want to create mismatched versions of the transistors, by copying the model and slightly changin the beta between models. you would have, for instance, an MJ15024 model with a beta of 75, an MJ15024LO model with a beta of 50, and MJ15024HI model with a beta of 100. for best results, you would choose your models at random, just as you would be picking them at random out of a parts bin.
__________________
Vintage Audio and Pro-Audio repair ampz(removethis)@sohonet.net
spammer trap: spammers must die
  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
DIY Distortion Analyzer/Analysis? mlloyd1 Solid State 139 18th November 2013 07:12 PM
Scaling voltage waveforms for distortion analysis okapi Everything Else 1 10th September 2008 01:58 AM
How to use OrCAD P-Spice to simulate TIM and Distortion correctly??? mclarenpingu Solid State 1 28th January 2008 10:03 PM
Distortion Analysis using an Oscilloscope gingertube Tubes / Valves 5 14th November 2007 04:14 PM
Distortion analysis mu follower docali Tubes / Valves 12 7th April 2005 06:54 AM


New To Site? Need Help?

All times are GMT. The time now is 10:44 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