Amplifier can't drive 5,7 and 13 ohm loads

Hi everyone,

I'm simulating an amplifier based on one of Bob Cordell's designs, but in the simulation, when I use 5, 7 and 13 ohm loads the output stays at 40V, I don't know what is causing this, for 4,6,8 and 16 ohm the output graph is ok, what's happening?
I'm using LTSpice.

Attached examples of the outputs, simulation file and Bob Cordell's models.

Best regards,
Daniel Almeida
 

Attachments

  • MOSFET2_test.asc
    8.7 KB · Views: 14
  • Cordell Models.txt
    11.8 KB · Views: 5
  • 4ohm_load_drive.png
    4ohm_load_drive.png
    24.8 KB · Views: 167
  • 5ohm_load_drive.png
    5ohm_load_drive.png
    12.8 KB · Views: 160
Well I never used Spice for simulation. I hash it out with pencil, paper, and calculator just like I was trained to do decades ago.

These results don't make sense to me. If an amplifier can drive 4, 8, and 16 ohm loads, but not 5, 7, and 13 ohm loads, then it will never be able to drive a real world speaker. There must be some kind of glitch.

Hopefully someone with Spice simulation experience can clear it up. My opinion is that Spice is wrong in this application.
 

Rundmaus

Member
2005-08-21 10:46 pm
Spice does funny things if inadequate accuracy settings are chosen. If you simulate for extended times, the automatically chosen timestep might be too large, causing the simulation output to be garbage.

Rundmaus

EDIT: Looked into your file. I wouldn't trust a simulation starting at time zero. Let it 'run' for 10-20s and start taking data then.
 
Last edited:
Here's the helpscreen (F1) on UIC;

UIC
Use Initial Conditions. Normally, a DC operating point analysis is performed before starting the transient analysis. This directive suppresses this initialization. The initial conditions of some circuit elements can be can be specified on an instance-per-instance basis. Uic is not a particularly recommended feature of SPICE. Skipping the DC operating point analysis leads to a nonphysical initial condition. For example, consider a voltage source connected in parallel to a capacitance. The node voltage is taken as zero if not specified. Then, in the first time step, an infinite current is required to charge the capacitor. The simulator cannot find a short enough time step to make the current nonsingular, and a "time step too small convergence fail" message is issued.
 
OK...I have duplicated the problem.

It's a latchup issue in the simulator, that might actually happen in the real world.
The simulator starts at a bad output voltage, that puts a bad voltage on C3, and pretty well ruins the operation of the input stage, and then everything stays bad. Place back-to-back 1N4148 across C3, which is probably a good idea anyway, and the problem is solved.

Update My Dynaco
Akitika GT-101 Audio Power Amplifier Kit
 
That's the interesting question.

The diodes are a good idea, as it prevents too much voltage across the cap under fault conditions. Still, the funny thing is that C3 starts out with about -37 volts across it...that just wouldn't happen in real life unless the positive rail was missing.

Interestingly, if you let it sim for 800 ms, it comes out of the funny state around 700 ms.

More interestingly, I changed Q2's model from the 2N5401C model to a different 2N5401 model on my machine, and the problem went away.

Hmmm...I'll report more if I see something definite.

Dan
 
I can cut the positive rail with a switch transistor to make a shutdown network?
This seems to work fine in simulation, STK series from Sanyo uses a similar network.
Or this is dangerous?
I can also make a mute network at the input with an analog mux with one or more bits for control, with ground, and the audio signal(s).

Best regards,
Daniel Almeida
 

Attachments

  • MOSFET2.asc
    10.1 KB · Views: 3
  • Cordell Models.txt
    11.8 KB · Views: 0