Go Back   Home > Forums > >

Solid State Talk all about solid state amplification.

My attempts at a design of a 3 stage amplifier
My attempts at a design of a 3 stage amplifier
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 Yesterday, 06:40 AM   #51
edbarx is offline edbarx  Malta
幸运飞艇开奖直播 Member
 
Join Date: May 2018
Online, I read in this same forum, that LTSpice is unreliable for distortion analysis, especially, when it comes to calculating the distortion percentage. Yesterday, I did a distortion analysis for a perfectly looking sine wave and got 700%! This is worse than ridiculous. For anyone who took interest to study mathematics beyond secondary level, a distorted sinewave looks like a dented mud-guard and is horrible to look at. The Fourier Analysis results looked more realistic indicating distortion components starting from -20dB downwards. I estimate this as a figure of around 1% of distortion although this is plain guesswork.

I cannot imagine why the fundamental frequency is included in the Fourier distortion analysis. The fundamental is not a distortion but the signal component! A better way would be an analysis of the signal with a pure sinewave removed, so that, only distortion components are left. Plotting that difference would give a very clear idea of the actual distortion signal waveform. if LTSpice can give a list of (t, V), time, voltage, points for a waveform output, I should be able to process that information to get a clear visual idea of the distortion waveform. I assume LTSpice can be directed to draw custom graphs like that.
  Reply With Quote
Old Yesterday, 06:52 AM   #52
suzyj is offline suzyj  Australia
幸运飞艇开奖直播 Member
 
suzyj's Avatar
 
Join Date: Jan 2006
Location: Western Australia
There's a little bit you need to do with LTspice to do good distortion analysis. Straightforward things like ensuring you're simulating an integer number of cycles of your harmonic, turning off compression etc.

Lots of us make really extensive use of LTspice for distortion. It's a very accurate tool if driven intelligently.
__________________
http://www.animayayuda.com/611
  Reply With Quote
Old Yesterday, 07:19 AM   #53
edbarx is offline edbarx  Malta
幸运飞艇开奖直播 Member
 
Join Date: May 2018
Here are two attachments with one showing output voltage VS input voltage and the other is the edited circuit with more power transistors.

The output VS input chart shows some hysteresis, that is, distortion as this is a deptarture from the theoretical line form. As can be seen, the distortion figure should be very low.
Attached Images
File Type: png circuit-with-added-power-transistors.png (49.0 KB, 21 views)
File Type: png output-vs-input-voltage.png (32.6 KB, 21 views)
  Reply With Quote
Old Yesterday, 07:30 AM   #54
Mooly is offline Mooly  United Kingdom
幸运飞艇开奖直播 Moderator
 
Mooly's Avatar
 
Join Date: Sep 2007
My attempts at a design of a 3 stage amplifier
Have a look at this, a 20kHz voltage source and resistor (resistor isn't even needed actually).

We have added the commands to calculate distortion, and added the plotwinsize=0 to turn off compression.

Now I'll add a timestep. The simulation is set to run for 4ms and the FFT sample is at the default of 262144. Dividing 4ms by 262144 gives us 0.0000000152587890625 seconds. Now we'll paste that into the timestep window and run the simulation.

Finally another trick up our sleeve. We can add the command .options nundgt=7 which gives double precision to the calculation of variables. Again we run the sim. This is as good as it gets. The fundamental and nothing else. Distortion is 0.000000000000...?
Attached Images
File Type: jpg DS1.JPG (295.6 KB, 17 views)
File Type: jpg DS2.JPG (218.3 KB, 17 views)
File Type: jpg DS5.JPG (196.5 KB, 17 views)
  Reply With Quote
Old Today, 01:26 AM   #55
PRR is online now PRR  United States
幸运飞艇开奖直播 Member
 
PRR's Avatar
 
Join Date: Jun 2003
Location: Maine USA
Quote:
Originally Posted by edbarx View Post
I did a distortion analysis for a perfectly looking sine wave and got 700%! This is worse than ridiculous. ...
Then you did something wrong. (Good on you for "knowing the right answer", and not taking SPICE as "Truth".)

Quote:
Originally Posted by edbarx View Post
Online, I read in this same forum, that LTSpice is unreliable for distortion analysis,
Does LTspice still have the .DIST card? That was always under-developed and is why .FOUR (Fourier) was developed.

In .FOUR you may specify the Center Frequency. If this is not your source frequency (as when you plot THD vs Freq and get out of sync) then it will get the right answer for the wrong question.

Quote:
Originally Posted by edbarx View Post
I cannot imagine why the fundamental frequency is included in the Fourier distortion analysis. The fundamental is not a distortion but the signal component!
Because the % is the ratio of the garbage TO the desired signal. So the fundamental (or whatever reference) must be in the report. .FOUR often shows the actual value of Harmonic #1, then Normalizes it to 1.000. Normalizes the other harmonics by the same ratio. Then does the sum and division and %.

.FOUR does usually give the "right" results, if you ask the right question, if your models are complete (none are).

Mooly has given some Advanced Tips for SPICE distortion. I didn't have his notes when I blundered into Pspice and fooled-around. For "small simple" distortion it is not essential to run magic numbers and odd incantations (for extreme low numbers it is).

Here is a perhaps rude example. A vacuum bottle with a large drive and heavy load. Without SPICE I would expect 5%-15% THD (depending on drive level).
tubeout-circuit.gif

When I simulate over one cycle, I get a zig-zag plot and a plausible 8.1% THD.
tubeout-1cycle.gif
The 1KHz 2KHz 3KHz 4KHz 5KHz peaks look plausible; the troughs between look to be sketched-in with a matchbook.

I increase the run to 200 cycles. The in-between, which perhaps should be zero, are now way-low and in fact are numeric "noise". (You see the same coarse/fine curves with spectrum analysis on audio signals; same Fourier formulas.) The total still computes to 8.1%.
tubeout-200cycle.gif

As in analog THD measurement, we can't get cleaner than out sine source. What is SPICE giving me??
rawsource-200cycle.gif

Not 700% but zero point three-oh something.
Attached Images
File Type: gif tubeout-circuit.gif (6.8 KB, 0 views)
File Type: gif tubeout-1cycle.gif (25.8 KB, 0 views)
File Type: gif tubeout-200cycle.gif (24.4 KB, 0 views)
File Type: gif rawsource-200cycle.gif (27.5 KB, 0 views)
  Reply With Quote

Reply


My attempts at a design of a 3 stage amplifierHide this!Advertise here!

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

Forum Jump

Similar Threads
Thread Thread Starter Forum Replies Last Post
Phono stage design considerations part 1: choosing 1st stage tube Joshua_G Tubes / Valves 210 Yesterday 02:16 PM
Amplifier design: how to connect a stage with the next one? Bricolo Solid State 11 10th August 2018 07:34 AM
Pre-amplifier circuit not working despite attempts to fix it Rudi1441 Analog Line Level 5 18th July 2016 02:35 PM
LF Line Level Stage design to preceed class D amplifier undefinedza Analog Line Level 13 18th September 2014 08:26 AM
how to design mosfet amplifier stage? pzung Solid State 2 22nd January 2010 06:58 PM


New To Site? Need Help?

All times are GMT. The time now is 01:30 AM.


Search Engine Optimisation provided by DragonByte SEO (Pro) - vBulletin Mods & Addons Copyright © 2018 DragonByte Technologies Ltd.
Resources saved on this page: MySQL 15.00%
vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2018 DragonByte Technologies Ltd.
Copyright ©1999-2018 幸运飞艇开奖直播