LM3886 based 8 Channel amps for linkwitz Orion

[paskal9]

if you could source for custom wound toroid then by all means proceed with your multiple voltage config. maybe afterwards after the amp is built you could try and run it with different voltage to hear if there's any audible difference between running the amp at different voltages.

[ST7677]

Originally Posted by pacificblue

I propose that you check the circuit in Spice to see the effect. C1 and Cf1 form a frequency-dependent voltage divider and changing either will affect the entire response. Their values need to fit to each other.

I made a model in LTspice and tried running it, however I am not able to run this. I am a complete newbie on this and need some help here.

I am attaching the schematics and model in ZIP file, if some one can run this model and check it will be of great help...
or guide me how to run this

Bridge Amplifier schematics.zip

The ZIP file includes
LM3886.sub - model
LM3886.sym - LTspice autogenerated symbol
LF411.mod - LF411 model
Bridge Amp schematic - circuit model in LTspice (Pic below)

Bridge amp schematics.GIF

[pacificblue]

Originally Posted by ST7677

if some one can run this model

LTSpice does not work with the .mod extension. Rename the LF411 file to .sub, then you should get results. I have the LF411.sub file in the corresponding LTSpice folder and after deleting the include command, your file worked.

The LM3886 model is not realistic. All transistors in it are ideal models, and the current source values are all guessed. Especially for the purpose of determining compensation this model is not useful, because it does not behave like the real LM at high frequencies.

[ST7677]

Thanks Pacificblue for trying this.
Did you notice any issue with the circuit in Spice, or it seems fine?

I could not find any LM3886 model on National Website. Is there any reliable LM3886 model available to simulate this?

I am still not able to run the model. I have changed the include file to (.include LF411.sub).
I see something happening in status bar below (image below), but do not get the black screen with charts.
Spice.GIF

What is the simulation command you are using? I used .ac dec 20 20 100

[pacificblue]

Yes, the file works fine.

No, there are no reliable spice models around.

I used the same simulation command.

In your file Spice looks for LF411/NS, which is not the same as LF411. The op amp value must be changed to LF411.

I already had the LF411 model renamed to LF411.sub in my *\LTC\LTspiceIV\lib\sub\ directory, so I could delete the include command. In theory your method should work the same, provided you have the file in the same directory as the sim file. Either that or you have to state the complete directory path in the include command as well.

[KSTR]

Hi,

Here is my try on making a proper AC model of the LM3886.



U2 is the standard single pole OpAmp (LT's opamp.sub) with parameters made visible and adjusted.

E1 introduces a set of higher poles. For convenience a squared 2nd order lowpass was choosen, with f0 and q selected to provide a close fit of the magnitude and especially the phase response compared to the published plot.

Zout -- required to see the effect of load capacitance -- is more or less guesswork based on the datasheet (R) and some minimum assumed open-loop output inductance. A zobel was simulated, too, because it tapers the open-loop transfer a bit as well, although usually higher up and not very significant for the phase margin at the intercept with the typical 26dB closed-loop gain.