LM 3886 PCB Based On Carlos Fm Schemetic

[neeraj]

Hi

This is my try to make a P2P PCB for CFM NI LM3886 V4.
Its single sided PCB. Need Expert suggestion for improvements if required.

Thanks

[tangmonster]

I am no expert.

But there aren't any differences between that circuit diagram and any other basic lm3886 i have built so far.

except i didn't bother with R4 , R5, C7, C8

MY personal minimum suggestion for c2 and c4 for 8 ohm load is 4700uF but 2200 will probably also do. Depending what size you have on the powersupply. side.

One person says the feedback resistor should be big 200k and higher and next person say feedback resistor should be small, you will have to experiment.

one person says use carbon film resistors , the next person say metal film has better properties and the 3rd guy will say anything less than dale or military spec gives crap sound and you are wasting your money if you don't use them.

my 2 cents

[neeraj]

Hi Tangmonster,
Thanks for reply.

Yes the load is 8Ohms & the cap on PS Side is 24700mfd/rail (10000X2, 4700X1)
that too is based on Carlos schematic.

2nd Option PCB is attached

[AndrewT]

that Carlos schematic includes all the options, except the DC blocking cap in the NFB loop.
That means that any output offset generated inside the chipamp will be multiplied by the gain of the amp, i.e. about 21times.
In addition the resistance seen by the -IN input is 2k//100r ~95r.
The +IN input sees 15k+330r ~15330r.
This difference in input source resistances will give a higher output offset and the resulting offset will vary more with chip temperature than if the resistances matched.

If you are using Carlos amp with Carlos PSU, then stick with his capacitor values, except if your experimentation proves that improved performance is obtained by doing otherwise.

Next, do not read all the Ground symbols as being the same. They are not the same.
The ground at the bottom of the 15k (R1) is the Signal Return. Connect this with it's Signal Hot as a twisted pair to the RCA input socket.
The ground at the end of 100r (R2) is also signal referenced. Connect it to the bottom of R1. these are the Signal Ground. Never mix Signal Ground with Power Ground through a common trace/wire.

Connect top of C3 to bottom of C5 directly by the shortest possible route, even soldering the two pins together.
Connect top of C2 to bottom of C4, using a short trace.
Connect C3/5 to C2/4. This is Power Ground.
Connect C7 to Power Ground.
Connect C8 to Power Ground.
Connect Cz to Power Ground.
Connect Power Ground to your Main Star Audio Ground.
Connect Signal Ground to Main Star Audio Ground.
Connect Speaker Return to Main Star Audio Ground.
Connect Chassis to Main Audio Star Ground.
Connect Protective Earth (the third wire in the mains cable) to the Chassis.

[neeraj]

Hi AndrewT,

You are talking about attachment 1 or 2.

[AndrewT]

I am using Attachment1 for reference.

Att2 is just PCB layouts.

[neeraj]

Hi AndrewT,
Thanks for reply.I am bit confused with
1. Connect top of C3 to bottom of C5 directly by the shortest possible route, even soldering the two pins together.
2. Connect top of C2 to bottom of C4, using a short trace.
Please Explain.


Do you mean 2000+.1uf or 0.1+0.1uf Please go through PCB lauouy & guide.

[AndrewT]

Hi,
the decoupling capacitors meet the very short term current demand of the amplifier.
They can only do this if the total route length from +ve power pin to -ve power pin through the decoupling capacitors is VERY SHORT.
Any wasted length adds to trace/route inductance and reduces the ability of the decoupling to meet instant current demand.
The slower transients that are fed from the electrolytic can tolerate some trace/route inductance and so the electrolytic route can be longer. The long term current demand is met by the PSU capacitors and since they are at the far end of the PSU connecting cables the inductance in this long routes does little harm. That is, provided you have made allowance for the decoupling to properly meet the short term demands of the amplifier.

Back to

Connect top of C3 to bottom of C5 directly by the shortest possible route, even soldering the two pins together

The route from the +ve pin to C3 must be VERY SHORT. Some builders solder the cap pin directly to the +ve pin.
The next part is the length of the route through the cap, i.e. pin to pin. Keep the cap pins VERY SHORT. Use a small capacitor with close pitch pins (2.5mm is better than 5mm, is far better than 10mm).
Then the route from +ve cap to -ve cap, soldering the pins together is the shortest possible route. Then through the -ve cap and finally to the -ve pin.
This total route from +v to -ve power pins must be VERY SHORT for the ceramic or MKT capacitor. MKP and FKP are physically too big.

[neeraj]

Hi AndrewT,
Thanks for your guidance.Will implement the same on PCB Layout.
What is the suggested value of DC blocking cap in the NFB loop.

Originally Posted by AndrewT

Back to The route from the +ve pin to C3 must be VERY SHORT. Some builders solder the cap pin directly to the +ve pin.

I have mounted the 0.1MKT directly on 2200 uf ( solderside of PCB).
please suggest the best suited PCB Layout.

[AndrewT]

I calculate the NFB cap as follows.

NFBcap >= 1.4 * Cin * Rin / Rfb

where:
Cin is the DC blocking cap at the input.
Rin is the resistance to ground following Cin that sets the high input filter
Rfb is the lower leg NFB going to ground.

For Carlos schematic

1.4 * 2u2 * 15k / 100 = 467uF.

Cnfb >=467uF so that the input filter sets the LF bandwidth of the amplifier and reduces distortion brought about by having an AC voltage across the NFB cap.