i did use the models provided by steve in one of his posts..
of course, i was carefull to modify the bias slightly to not
miss the nulling point as i used increments of 2mV....
I misspoke yesterday. I tried 5.7 Ohms and .9mH for an 8 Ohm load at 45 degrees not 90 degrees. I also just played around with a simple CEF and got the same resut, you can tune the third harmonic down to <.002% but simply changing the phase it goes back to .02%. So I consider this matter moot unless you are driving purely resistive speakers.
Last edited:
Scott has brought up a valid point regarding speaker loads on distortion performance, so I looked into the performance, simulated only, of the output stage I posted in post 302, with a simulated loudspeaker load. The load I used can be found here:
Phase Angle Vs. Transistor Dissipation
This was run on Intusoft, my preferred program. Fourier analysis was run first with an 8 ohm resistive load. The frequencies were 20, 200, 2K and 20K. All runs were at rated output of 50W. Here are the results for the resistive load.
I was quite surprised at the results using the simulated speaker load. The total deviation from flat response from 1Hz to 100kHz was +/- 0.035 dB, but that was not the surprise. Here are the results at the same conditions as above. You will note that my program renumbered the output node when I added the simulated load.
As Scott pointed out, adding a reactive load does increase the distortion at some frequencies. I hope this gives some of you some insight into how my amp performs with a real world load.
Phase Angle Vs. Transistor Dissipation
This was run on Intusoft, my preferred program. Fourier analysis was run first with an 8 ohm resistive load. The frequencies were 20, 200, 2K and 20K. All runs were at rated output of 50W. Here are the results for the resistive load.
I was quite surprised at the results using the simulated speaker load. The total deviation from flat response from 1Hz to 100kHz was +/- 0.035 dB, but that was not the surprise. Here are the results at the same conditions as above. You will note that my program renumbered the output node when I added the simulated load.
As Scott pointed out, adding a reactive load does increase the distortion at some frequencies. I hope this gives some of you some insight into how my amp performs with a real world load.
The culprit is the Early voltage. Vbe modulation by the Early effect is actually quite substantial with these output devices (VA~40V). This is in phase with the input voltage. The Vbe modulation with current is in phase with the current. So changing the phase of the load will change the distortion cancelling effect. So there you go amplifier/cable/speaker interface effects without invoking quantum mechanics.
Thanks for the explanation Scott.
Just for fun, I ran the same circuit at an output of two watts (First Watt was taken) with the same load. I didn't bother with the 8 Ohm sims at this power as there really seems to be no point in it.
Just for fun, I ran the same circuit at an output of two watts (First Watt was taken) with the same load. I didn't bother with the 8 Ohm sims at this power as there really seems to be no point in it.
As something of a control, I ran the same sims on a conventional amp with feedback to see if it showed the same type of changes. The amp I used can be found here:
Distortion In Power Amplifiers
I ran the sims at the rated output of 50W into an 8 Ohm resistive load first. I set the bias for minimum distortion at the 2KHz frequency. The first thing I noticed was the rather high 20Hz distortion.
I thought I knew what was causing this, and made some changes to the amp to check. First I changed C2 from 220uF to 2200uF.
Next I changed it to 22000uF.
I still wasn't happy with the results, so I left C2 at 22000uF and changed C1 from 10uF to 100uF.
That was a big improvement, so I changed C1 to 1000uF.
This was looking much better. This had moved the -3dB point from 2.3Hz to 0.023Hz. This might well be worth considering when selecting the value of coupling and feedback caps.
Self address this in the link I gave earlier calling it "capacitor distortion".
Distortion In Power Amplifiers
I ran the sims at the rated output of 50W into an 8 Ohm resistive load first. I set the bias for minimum distortion at the 2KHz frequency. The first thing I noticed was the rather high 20Hz distortion.
I thought I knew what was causing this, and made some changes to the amp to check. First I changed C2 from 220uF to 2200uF.
Next I changed it to 22000uF.
I still wasn't happy with the results, so I left C2 at 22000uF and changed C1 from 10uF to 100uF.
That was a big improvement, so I changed C1 to 1000uF.
This was looking much better. This had moved the -3dB point from 2.3Hz to 0.023Hz. This might well be worth considering when selecting the value of coupling and feedback caps.
Self address this in the link I gave earlier calling it "capacitor distortion".
I reset the values of C1 and C2 back to the values given in the schematic I linked to in the previous post to run the sims. This is with an 8 Ohm restive load.
As you can see, the effects of C1 and C2 still show some influence at 200Hz. Next are the sims using the simulated speaker load.
The deviation from flat response from 20 Hz to 20Khz was only +/- 0.036dB. Most of this was the role off at 20Hz caused by C1 and C2. If the measurements are made from 50 Hz to 20KHz this deviation is reduced by half.
As you can see, the effects of C1 and C2 still show some influence at 200Hz. Next are the sims using the simulated speaker load.
The deviation from flat response from 20 Hz to 20Khz was only +/- 0.036dB. Most of this was the role off at 20Hz caused by C1 and C2. If the measurements are made from 50 Hz to 20KHz this deviation is reduced by half.
Hi Steve
There's something not right with your recent sim results - the high order distortion products aren't dropping off.
e.g. For your 2watts @ 2khz sim in post 426, all the harmonics are almost exactly 10ppm. That's totally unnatural - I'm sure it's sim artifacts and the real figures should be lower.
I think you need to improve the resolution somehow to get more meaningful results at very low distortion levels. Maybe reduce the time-step (or whatever it's called in your software) and/or let the sim run for a few cycles before starting the measurement.
If you're using LtSpice, there's tips on getting accurate results here: Common Issues Encountered By New Users - diyAudio
Regards - Godfrey
There's something not right with your recent sim results - the high order distortion products aren't dropping off.
e.g. For your 2watts @ 2khz sim in post 426, all the harmonics are almost exactly 10ppm. That's totally unnatural - I'm sure it's sim artifacts and the real figures should be lower.
I think you need to improve the resolution somehow to get more meaningful results at very low distortion levels. Maybe reduce the time-step (or whatever it's called in your software) and/or let the sim run for a few cycles before starting the measurement.
If you're using LtSpice, there's tips on getting accurate results here: Common Issues Encountered By New Users - diyAudio
Regards - Godfrey
Steve, the "capacitor distortion" is a problem with LTSpice's .four command here I think. Even the default capacitor models in LTSpice don't model capacitor distortion.
Also, square wave sources in the schematic not attached to the circuit can cause odd transients in other parts of the circuit, and on an FFT this can look like your amp's distorting especially if the square wave source is the at the test frequency. It helps if the risetime for the source is slower than the timestep.
- keantoken
Also, square wave sources in the schematic not attached to the circuit can cause odd transients in other parts of the circuit, and on an FFT this can look like your amp's distorting especially if the square wave source is the at the test frequency. It helps if the risetime for the source is slower than the timestep.
- keantoken
It has nothing to do with heat AFAIK there is no commercial SPICE that does a full thermal analysis at every time point.
Hi godfry,
I prefer Intusoft. To me, it is easier to use and much faster than LTspice. I will look into the time step (that is what it is called in Intusoft also), but I alredy let the sim run for a few cycles before starting the measurement.
I prefer Intusoft. To me, it is easier to use and much faster than LTspice. I will look into the time step (that is what it is called in Intusoft also), but I alredy let the sim run for a few cycles before starting the measurement.
As I pointed out, I am not using LTspice. Also, what my sims show is shown by D. Self in the link I gave. I will turn off the square wave and look again. I was not aware that could happen, thanks.
I reduced the time step and reran the 2W results with the simulated load. I like the results, but I'm not sure I believe they represent real world measurements.
The link "Phase Angle vs Transistor Dissipation" maybe useful but has nothing to do with this.
You are correct about that. If you scroll down a little, the simulated load I am using is shown. I gave the link instead of posting the schematic to avoid any issues concerning intellectual property or copyright.
Just adds to the confusion without some context. There must be some public domain phasor diagram somewhere.
I should have been more specific. The only thing I was trying to link to on that page was "Figure 1 - Loudspeaker Equivalent Circuit". That was so everyone could see what I was using as a simulated speaker load.
My sympathies.
Simming with LTspice is about as much fun as trimming the lawn with a nail scissors.
- Status
- Not open for further replies.