Help on LM3886 PCB Routing

[yatgai]

Hi

I am trying to make chipamp with LM3886 output 30W RMS per channel, my config as under

Transfo 200VA , 20-0-20 secondaries unregulated power supply with Capacitor 10,000uF/63V on each power rail
Speaker 8 Ohms
Gain 20X

Attached picture of single sided PCB layout with component placement. Are there any deficiencies ? any improvements needed ?

Thanks for your time

Yatin

[jcx]

for some reason nearly all chip amp pcb layouts I've seen mistakenly go for "symmetry" in the pwr routing with +.- on opposite edges of the board, as far apart as possible - can't get more wrong from a circuit operation point of view

I'd put pwr traces, PS caps on the same (left) edge of the board, move the gnd trace from the left inwards

look at current paths, minimize loop areas - this means pwr wires, traces need to be as close together as possible, as well as close to gnd

the "star gnd" is poorly conceived - you should really want input signal ref, feedback network gnd and load gnd to be the "star" point - the jumpers to the gnd "racetrack" give many loops, paths for "gnd contamination" from the Class B currents that look half-rectified in the separate +,- ps wires and ps cap gnd return paths



for just a single stereo build I'd just do point-to-point "air wire" or with at most a perf board - can be done really well and give better performance than many PCB layouts I see

the only reason I can see for a PCB is if you want multichannel or active XO - then I'd think about system level power, gnd routing - probably add a op amp differential receiver for signal input

and with the extra parts 2-layer becomes more attractive, gives better routing - I really don't care to work with home etched boards, of course a small batch from a PCB manufacturer that has prototyping deals only costs about what I now consider a "nice" restaurant dinner

[jcx]

Mick Feuerbacher Audio Projects

[GloBug]

Originally Posted by jcx

Mick Feuerbacher Audio Projects

Too cool! That's more like the real gaincard.

[pinkmouse]

Originally Posted by GloBug

Too cool! That's more like the real gaincard.

But nowhere near good enough heatsinking to run at full rail voltage.

[yatgai]

Thanks for detailed reply JCX, I wanted it to be on PCB because threre are other PCBs like Speaker Protection and Bass & Treble control

Would this be a better layout sonically ?

Power ground and signal grounds are in separate traces tied via 10R/2W resistor

Thanks
Yatin

[madtecchy]

Hi
Is there supposed to be a 10R 2W resistor in series with the output.

[AndrewT]

Hi Yat.
the Power traces are far better located now.
Try to thicken up the thin parts of those traces. They do have to pass high transient currents, or at least as large as the 3886 will allow. Look at PIN2. It is not connected. You can use this spare PCB area to thicken traces.
Remove the 90degree internal corners from your traces. Imagine your electrons as yourself driving around a race track (Indianapolis). Round the corners.

Re-trace the inputs to PINs 9 & 10.
They are too far apart. Keep them as a close coupled pair from the two input terminals all the way to the two input PINs.

Keep the Signal Return separate from the Power Ground.
This is very important if you adopt the same PCB for a multi-channel amplifier. In monoblock you can get away with Main Audio Ground on the PCB, but not in multi-channel.

Finally,
you may find that very small ceramic caps make for excellent power pin decoupling. These can be fitted much closer to the Power PINs than those big 0.2" pin pitch film caps shown.

[madtecchy]

Hi andrew.
Them traces will be fine with that 10R resistor in series with the output

[GloBug]

Originally Posted by pinkmouse

But nowhere near good enough heatsinking to run at full rail voltage.

Duly noted.