100W Ultimate Fidelity Amplifier

Here is a simulation done with ltspice for the AX20. As I'm trying to learn more on ltspice, I was curious about the AX20 and wanted to simulate it.

I embedded the models not in the ltspice default database so anyone using it should be able to run that sim with the same models.

I encountered a few discrepancies about part numbering around the output stages, so although most of the parts have the same number as on the schematic (attaching the one I used), some resistors have different numbers.

Once the simulation is able to run, I can immediately see that something can't work as it is on that schematic, as there is nothing to fix the potential on Q1's base, so I see a huge offset there at nearly 20V, so the output signal is totally offset as well and with a signal not pushing it to clipping, it does clip on the top side.

This thing is missing something to bring Q1's base to ground level...
SGND and PGND is both conneect to PSU GND only with separate wires.
 
SGND is floating - it's not connected to GND anywhere. I think that's your problem.

Right, so there are connections external to this schematics. On the psu.

Try again.

Ok, that was the connection missing on the schematic. But there is an offset anyway, although not huge on the output. Who knows what you get when not matching transistors...

SGND and PGND is both conneect to PSU GND only with separate wires.

Yes, this might be a nice thing to mention on the schematic, in case one only looks at it without looking at the other related ones.

The simulation now runs, with a bit of an offset on the output. But to make it run with a bias at about 50mA for each power output, the bias spreader's resistors don't work with the values on the schematic.

I raised the value of R16 from 1k to 2k7 and the trimmer P1 doesn't need to be 1k, it could be 100 or 220ohms.

The signal looks nice at 1khz, but not so good at 20khz though.

Something is wrong there, but that could be related to screwy models...
 

Attachments

  • Screen Shot 2014-02-06 at 6.27.00 PM.png
    Screen Shot 2014-02-06 at 6.27.00 PM.png
    299.2 KB · Views: 1,535
  • AX20_.asc
    15 KB · Views: 106
N-Period=4
Fourier components of V(out)
DC component:-0.00437193

Harmonic Frequency Fourier Normalized Phase Normalized
Number [Hz] Component Component [degree] Phase [deg]
1 2.000e+04 3.176e+01 1.000e+00 -8.72° 0.00°
2 4.000e+04 8.707e-04 2.742e-05 -73.60° -64.88°
3 6.000e+04 1.620e-03 5.101e-05 115.03° 123.75°
4 8.000e+04 1.301e-04 4.096e-06 -128.28° -119.56°
5 1.000e+05 3.664e-04 1.154e-05 -60.05° -51.33°
6 1.200e+05 1.589e-04 5.005e-06 -146.69° -137.96°
7 1.400e+05 3.076e-04 9.687e-06 14.95° 23.68°
8 1.600e+05 1.414e-04 4.451e-06 -167.68° -158.95°
9 1.800e+05 4.448e-04 1.401e-05 1.82° 10.54°
10 2.000e+05 1.144e-04 3.604e-06 164.80° 173.53°
Total Harmonic Distortion: 0.006206%

1K THD is 0.001%

Disconnected the diode, add a 100K ohm from Q1-B to sgnd
Added a 8 ohm load from out to gnd
300/3K ohm bias R's to get a idle I of 83mA.
800mV input sig, 1V seems to be putting it into a bit of clipping action

DC Offset is 625uV
Run the .op and then go to the schematic, click on the nets to display a few more important nets to place static DCV markers so that you can investigate bias settings.

Thx for drawing it up for us to play with.
 
Last edited:
D1 is to improve clipping and recovery behavior. Apex apparently decided that not having that diode was worse than having higher THD. So would removing it be an improvement of the overall quality of the circuit or would it be a deal with the devil?

Also: With the diode in this position Q4 needs to have 0V Vce so that both it and the diode are furthest away from turning on. This will increase the linear bandwidth, because at 20KHz D1 is turning on, causing distortion.

Looking at your schematic, all of those models may be flawed and hardly represent the originals. This could be affecting the simulation results. I recommend you take the time to include my library that I shared in the SPICE thread. To get excellent FFTs with a low noise floor, along with square, triangle, and saw signal generators (these are hard to get right in SPICE!), and an OLG probe, use the attached amplifier simulation rig I made.
 

Attachments

  • ampsim5.asc
    6.5 KB · Views: 118
Total Harmonic Distortion: 0.006206%

That's not at 20khz!

And definitely not with the diode in there on the diff amp.

1K THD is 0.001%

Maybe, with the following mods...

Disconnected the diode, add a 100K ohm from Q1-B to sgnd
Added a 8 ohm load from out to gnd
300/3K ohm bias R's to get a idle I of 83mA.
800mV input sig, 1V seems to be putting it into a bit of clipping action

I ran it with about 50mA of bias. Maybe the higher bias reduces thd a bit.

I used 2k7 and left 220 at the spreader, so a trimmer of 100 or 220ohms works fine.

You must be referring to rms voltage on the input. I put 1.32V and it doesn't clip, but that's peak, not rms.

DC Offset is 625uV

I assume on the output. It was a bit over 12mV without mods. Perhaps your mods get that offset better under control.

Run the .op and then go to the schematic, click on the nets to display a few more important nets to place static DCV markers so that you can investigate bias settings.

Thx for drawing it up for us to play with.

Sure. You should post back if you made changes and ran other sims. Leaving the spice commands used to run those sims in there.

I noticed it tends to clip unevenly too, starting to clip at the bottom first.

But in any case, that diode can't stay on that diff amp, unless someone wants distorted sound...
 
D1 is to improve clipping and recovery behavior. Apex apparently decided that not having that diode was worse than having higher THD. So would removing it be an improvement of the overall quality of the circuit or would it be a deal with the devil?

The distortion with it is huge. Although hardly noticeable at 1khz. I wouldn't want it in there.

Also: With the diode in this position Q4 needs to have 0V Vce so that both it and the diode are furthest away from turning on. This will increase the linear bandwidth, because at 20KHz D1 is turning on, causing distortion.

I don't see a way that it can work and not cause distortion.

Looking at your schematic, all of those models may be flawed and hardly represent the originals. This could be affecting the simulation results. I

Quite possible. (oh boy! don't we need that model sharing platform? ;-)

Some are from bob cordell, some from phillips, maybe one or 2 from yours.

recommend you take the time to include my library that I shared in the SPICE thread. To get excellent FFTs with a low noise floor, along with square,

I'll switch and check again.

triangle, and saw signal generators (these are hard to get right in SPICE!), and an OLG probe, use the attached amplifier simulation rig I made.

Ok, I'll take a peek and try this. Thanks for posting this stuff. I want to understand spice better.
 
That's not at 20khz!
1 2.000e+04 3.176e+01 1.000e+00 -8.72° 0.00°
All I did was change ".param freq=20K".
Measure after a few cycles have started, just like Bob C. explains in his book.
Looking at your schematic, all of those models may be flawed and hardly represent the originals.
My numbers are based on the supplied models and schematic with changes as noted

Thx for the spice stuff!! More to learn what else is new :)
 
Here it is again.

I changed the models, but couldn't do it for the bc547s because I didn't have any on hand. The original schematic calls for bc547 but I used the bc547b that comes with ltspice. We can change that later when we get "better" models.

The outputs were the same, so nothing changed from that. Same thing for the mje340/50. The bd139 was mostly the same but not quite. The previous bd139 model was from philips and it had several more parameters in there.

The drivers were exactly the same. However the few changes did make a difference in the biasing, so I had to up the trimmer's value to get the roughly 50mA in each output. To do this in a real amp if the transistors matched those models, the bias trimmer would need to be 470ohms probably. Perhaps changing the bc547s as well would change this again.

Without any other mods beside disabling the diode on the diff amp, I get 0.003828% thd at 1khz/8ohms, with the signal right at the limit before it starts clipping at the bottom. thd goes up a lot once it starts clipping, of course, but with an input signal at 1.33V (peak) as on the current sim attached, we get nearly 38V rms on the load, so that's not far from 180W.

The thd goes up to 0.039923% at 20khz, with everything the same. So that's one order of magnitude higher. But still not so bad.

Things might actually worsen if bc547 are used instead of bc547b, especially on the diff amp. And in reality, the plain bc547 could be anything from a to c, so without prior matching, the result could be very unpredictable. Matching and selecting parts is a must!

Now I'll have to figure out how we clean up that grass on the fft plot.
 

Attachments

  • AX20.asc
    15 KB · Views: 110
  • Screen Shot 2014-02-06 at 10.14.47 PM.png
    Screen Shot 2014-02-06 at 10.14.47 PM.png
    204.1 KB · Views: 1,689
I think you attached the wrong file. I don't see any changes.

BTW, leaving the end of D1 floating like that is bad practice and will cause the simulator to give convergence errors. It's inconvenient but I always delete the diode instead. Otherwise I end up with a simulation that won't converge and keeps throwing errors without giving any hints that it's a floating diode causing the problem.
 
I think you attached the wrong file. I don't see any changes.

The schematic hasn't changed, but the models have. I put all the models from your file, except for the ones that aren't in there.

You can see the order of the models isn't the same as the previous one.

Actually one small change on the schematic is there, P1 to adjust the bias, since changing the models has also changed the operating point.

BTW, leaving the end of D1 floating like that is bad practice and will cause the simulator to give convergence errors. It's inconvenient but I always delete the diode instead. Otherwise I end up with a simulation that won't converge and keeps throwing errors without giving any hints that it's a floating diode causing the problem.

Ah! That's good to know, thanks. I have been doing this sometimes when I only wanted to try something temporarily and put it back later. Maybe disconnect each end and grounding them would avoid removing the part and wouldn't disturb the sims.

I tried adding that 100k resistor on Q1's base to sgnd, and that does bring the output offset down a whole lot, and even reduces very slightly thd.

I would change the models from the library as well, but then I'd have to open it up to comment them out afterwards. I have found ltspice extremely crash prone when there are duplicate parts models. And once we have it in that state, it crashes as soon as we reload the sim file and the only way to make it work again and load without crashing, is to manually edit the source to remove the models in question. I just had to go through that now.
 
reviving my Sony sa-rv990 100w sub woofer by replacing stk404-130s with apex ax14 and really like the bass of this amp but the sound is low compare to stk404-130s maybe i need to add preamp so i can drive it into full.
apex what is you suggestion?
 

Attachments

  • IMG00148-20140207-1403.jpg
    IMG00148-20140207-1403.jpg
    279.1 KB · Views: 1,555
  • IMG00152-20140208-1833.jpg
    IMG00152-20140208-1833.jpg
    270.6 KB · Views: 1,453
  • IMG00157-20140208-1906.jpg
    IMG00157-20140208-1906.jpg
    273.5 KB · Views: 1,347