LM386 Schematic

[Bullet]

Hi, first post, be gentle

I am trying to model the LM386 here:
http://lushprojects.com/circuitjs/circuitjs.html

I am using the schematic from the datasheet here:
http://www.ti.com/lit/ds/symlink/lm386.pdf

I can't figure out what the symbol near the top right of the schematic is. It looks like a circle with a black triangle in it. Tried Googling - nothin. Anyone got a clue? If I can figure it out I'd be happy to post the finished txt file so others can use it.

[PRR]

Welcome.

That is a current source. (Read-up on basic power amplifier design.)

For initial modeling, try 2mA.

Why 2mA?

1) The specified 4mA idle current must cover this, the several 15K resistors, and the output stage idle current. At 6V spec-test, the 15Ks are drawing 0.17mA twice. The power device idle is "usually" greater than the bias-diode current. So maybe 1mA?

2) The upper power device must pass the maximum output current with that current-source as Base drive. Top-right page 5 shows max 3.8V p-p in 4 Ohms which is 475mA. Taking hFE as 200 gives current source as 2.3mA. In fact the output devices are deliberately tiny and their hFE is falling bad, so I would guess 4mA.

Split-difference of conflicting 1mA and 4mA guesses gives 2mA.

You will not be able to *exactly* model the LM386 unless you have chip-level transistor models. Integrated circuit process limits give parts much different than discrete parts. The designer can tailor the device to crap-out at a fairly predictable limit, which is why the LM386 survives without any proper over-current protection.

Designing Analog Chips by Hans Camenzind is a good reference for integrated circuit design and simulation. Free book.

[PRR]

ALSO note that a SPICE "current source" is NOT what we call "current source" in general design. The SPICE part can deliver infinite power. What we use is really more of a current-limiter. I guess the cheapest fake is two PNP transistors (in SPICE the Vbe will match exactly), both Emitters to V+, one diode-connected with a resistor to V- passing 1mA, the other current-mirroring that to the output stage.

Also the LM386's PNP devices will be "lateral". Hans says "It is the world's worst transistor, you couldn't sell it as a discrete component: low cutoff frequency, very limited current range and an inferior noise figure." Your discrete-based PNPs will work far better. (Perhaps so good as to invite MHz instability.)

[tubegeek]

Hans says "It is the world's worst transistor, you couldn't sell it as a discrete component: low cutoff frequency, very limited current range and an inferior noise figure." Your discrete-based PNPs will work far better. (Perhaps so good as to invite MHz instability.)

Here's a page where a guy proves this, with testing and everything:

Homo Ludens: Small Audio Amplifiers

[PRR]

> I can't figure out what

The '386 is a cheapo '380. Read AN-69 LM380 Power Audio Amplifier.

The '380 "simplified schematic" shows a different implementation of the part you asked about. Q10 catches the current from the left side 15K+15K (25K here) string and current-mirrors it through Q11 as the load for Q12 and pull-up for Q7.

That does not add-up right as-is. I suspect Q11 is a much larger device than Q10, and the mirror has current gain. While there are several ways to hack this, for simplicity add say 5K from Q10 Q11 Bases to V-, to force Q11 to a decent current.

[mac]

To avoid "perfect" Spice devices as Paul said above, you can copy a transistor model, say 2n3906, and paste it N times in your design to be used as .model xxx1, ..., .model xxxN. You can change gain, cutoff freq, Vbe, etc, to have N similar but different transistors.

Also the LM386's PNP devices will be "lateral". Hans says "It is the world's worst transistor, you couldn't sell it as a discrete component: low cutoff frequency, very limited current range and an inferior noise figure."

I could use one of those low cutoff freq in a FF

mac

[signality]

Sorry for joining this thread so late but I've just joined this forum.

If you are interested in simulating the LM386 then you may be interested in these simulations and the associated spice model that was developed for the LM386 power amplifier stage:

https://easyeda.com/example/Tesseract_Guitar_Practice_Amp_simulation_files-H0ca8IFDB

You have to join EasyEDA to run the simulations but it's free to use.

You can open the page with the model in it here:

https://easyeda.com/editor#id=z93lDxP6o

then just double-click on it to copy the model text.

The model runs in ngspice (which is what EasyEDA uses anyway) and LTspice. It'll run in SIMetrix and probably run in PSpice.

BTW, for comparison, this:

https://easyeda.com/example/Demonstrating_the_EasyEDA_LM386_spice_subckt_model-pgoiAgM4m

compares the "No Frills" LM386 model with the improved EasyEDA model.

There's a bit more about the LM386 simulation models here:

https://en.wikipedia.org/wiki/LM386