The yet tiniest single-sided LM3886?

Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.
Jump to Latest
infinia

infinia

Member
Joined 2005
Consider swapping places with the 0.1uF decoupling caps and small electros to bring the critical parts closer to chip amp power pins.
The 0.1 uF parts look big. Shop for smaller pin spacing (5mm) narrow leads means better HF performance.
Consider wiring the amp output speaker return going off PCB to the stiffer PS PCB instead. This is key to keeping a quiet gnd on the amp board esp since you choose very small value electos.

look at other chip amp power PCB layouts for ideas on central grounding. Think about all yer in /out connectors, their location, connection numbers, and chassis wire dressing with either a mono block, stereo, or even a HT amp for a future growth configuration. IMO Bunching all the ins and outs together in the middle with a circular ground is kinda like painting yerself into a corner.
 
A

AndrewT

R.I.P.
Joined 2004
discrete said:
In the simulation below, do you want to feed your amplifier with V1, V2 or V3?

Using V1 is a good way to have mains hum on your speakers.
Click to expand...
Yes, take account of the wiring/trace resistance.

An ordinary Capacitor Input Filter is actually an rC filter. Don't throw away that useful small r by connecting to the wrong terminal.
Similarly the bank of caps have connections all with a small r. Power comes out cleaner at the opposite end from the rectifiers. Looks like a 15dB reduction in hum/buzz. Note also the frequencies in the hum of V1 ref V3. V3 is substantially 100Hz and a few odd harmonics.
V1 is very spiky and consists of substantial HF harmonics.
 
Last edited:
H

hurtz

Member
Joined 2010
discrete said:
In the simulation below, do you want to feed your amplifier with V1, V2 or V3?
Click to expand...

Wow a huge thankyou to you :) Finally I can visualize what is going on!
PSU design has been altered accordingly (I hear 4 caps are the new wave ;))

Amp design was also changed quite a bit. 0.1uF caps were moved closer to the power pins, also were exchanged for 2.54mm spacing instead of 5mm.
Also Cin was moved closer to the chip, reduing the path from input to chip significantly. The AMP PCB is at the moment just below 10mm^2.

infinia said:
Consider wiring the amp output speaker return going off PCB to the stiffer PS PCB instead.
Click to expand...
I'll keep that in mind and will try it if I have problems with noise on the speakers, but for now I keep the return on the AMP PCB itself (one less connector ;)).

Hopefully the nearly last revision:

AMP v3.0:
An externally hosted image should be here but it was not working when we last tested it.


PSU v3.0:
An externally hosted image should be here but it was not working when we last tested it.
 
H

hurtz

Member
Joined 2010
The Parts list:

Code: 
-LM3886TF   x1

-Cin: Wima MKS-2   4.7uF   50V=   5%   5mm   *1
-Cz,Cs2,Cs4: Wima MKS-02   0.1uF   63V=   20%   2.5mm   *3
-Cs1,Cs3: Panasonic   68uF   35V   20%   2.5mm   Inpedance:0.35Ohm   Ripple:290mA *2

-Rm: 10k  1W     *1
-Rf: 22k  0.25W  *1
-Ri: 680R 0.25W  *1
-Rg: 22k  1W     *1
-Rz: 2R7  2W     *1

Some changes were made to the layout, the size of some of the components were updated. The speaker out was moved out of the 2.54mm grid, to allow for bigger drill-holes/connectors. For Cs1/Cs3 caps with either 5mm or 2.5mm grid can be used with a diameter up to 8mm. The input was moved into a 3.5mm grid that allows for PCB-connecters with screws (or whatever they are called) The purple box outlines the plastic casing.
also I've decided to call it the "mü-amp" :). Size of the board is 40mm * 24mm = 9.6cm².

After printing it today for the first time, I have some doubts whether it is possibly to toner-transfer the PCB... but well, we'll see.

AMP: v3.1
An externally hosted image should be here but it was not working when we last tested it.


PSU: unchanged
Parts List:

Code: 
-Cn: Jamicon   4700uF   35V   20%   7.5mm   *8
-Dn: MUR820   *4


As always, further suggestions/critics welcome, around next week I think I will order the parts and build it, when everything fits, I will publish the layout of the mü-amp.

thank you everyone again, I really appreciate the effort you take helping some "random stranger" ;)

Cheers!
 
P

Piggy

Member
Joined 2009
Nice work. How about not to connect the zobel and the speaker return on the signal ground bus?
An-1849, fig 11 may be useful for your design.
You may also consider fit the Rm under the Lm3886 and move the Rf closer to the chip.
Leave some space for the feedback cap and RF filter as well.
 
A

AndrewT

R.I.P.
Joined 2004
3.5mm pin/pad pitch does not sound right.
Almost all connectors use increments of 0.1inch (2.54mm) for pitch, The screw down terminals are usually 0.2inch (5.08mm) pitch. The single in-line pin and socket are usually in 0.1inch (2,54mm).
Mica (silvered mica caps) are usually not available in 0.1inch pitch increments.
 
H

hurtz

Member
Joined 2010
Nice work. How about not to connect the zobel and the speaker return on the signal ground bus?
Click to expand...
What do you mean? Technically there is a connector on the AMP for the speaker return, but should anyone want to build this, he/she can still return the speaker directly to the PSU.

3.5mm pin/pad pitch does not sound right.
Click to expand...
They are from: RIA CONNECT Article: 31059102

Mica (silvered mica caps) are usually not available in 0.1inch pitch increments.
Click to expand...
I'm not using any ;)

cheers!
 
infinia

infinia

Member
Joined 2005
The output zobel actually belongs on the amp board or the signal ground. Contrary to some folks belief this RC network is NOT for the speaker. It is used for feedback stability ie phase margin around the unity gain frequency > 2MHz. Due to high frequencies, when wired remotely, it's almost useless. It's very important not to mix power and signal grounds, so it's good to wire the speaker return to the PS common (power ground).

Also since this a gain clone copy, ie minimal design
A) there is NO DC block on the inverting network. so it's possible to have significant DC offsets at the speaker.
B) there is NO RF filtering either on the input or output. The user can and should provide some provision for this in the final design. Same is true on the PS PCB.
 
Last edited:
H

hurtz

Member
Joined 2010
Juergen Knoop said:
there is a short between pin 10&11 and pin 7 doesn't need to connected to ground via such a large track width, 0,5-1mm would be enough
Click to expand...

Yep, but since pin 11 is not connected, it doesn't matter and I wanted to give the input line more room.
Wait isn't pin 7 the ground pin on the board? where at least the dissipated power flows through?

infinia said:
Also since this a gain clone copy, ie minimal design
A) there is NO DC block on the inverting network. so it's possible to have significant DC offsets at the speaker.
B) there is NO RF filtering either on the input or output. The user can and should provide some provision for this in the final design. Same is true on the PS PCB.
Click to expand...

And again I have no idea what this is about :eek: could you explain this a little bit further/point me in the direction where I can read about this?
Since I plan to use single sided PCBs with a dimension of 120x80 it would still be convenient to have a 40x30 board rather than 40x24 now.

mü-amp v3.1
An externally hosted image should be here but it was not working when we last tested it.


Some minor changes, I moved some parts around to use caps with 8mm diameter, and nearly four times the capacity, 2.54mm pads are still present, so updated:
Code: 
-Cs1,Cs3: Panasonic   220uF   35V   20%   5mm   Impedance:0.09Ohm   Ripple:730mA *2

cheers!
 
Last edited:
infinia

infinia

Member
Joined 2005
The NS schematic with some parts marked "optional" are not really, except for advanced users or risk takers. The major item that impacts your amp PCB is the DC blocking cap in series with Rg. almost everything you need is in the NS data sheet.
RF filtering on all inputs / outputs including AC entry, is generally good design practice and depends on the PCB final application circuit/s or parts, layout wiring, and chassis design.
 
Last edited:
A

AndrewT

R.I.P.
Joined 2004
I cannot agree with your layout philosophy of mixing the Signal Ground with the everything else Ground.
I recommend that Signal Ground and what needs to be connected to it, be kept completely separate from the Power Ground and Zobel Ground and PIN7 Ground and Speaker Ground.
 
wintermute

wintermute

Just another Moderator
Joined 2003
Paid Member
Agree 100% with Andrew on this point :) The data sheet is your friend.

LAYOUT, GROUND LOOPS AND STABILITY
The LM3886 is designed to be stable when operated at a
closed-loop gain of 10 or greater, but as with any other
high-current amplifier, the LM3886 can be made to oscillate
under certain conditions. These usually involve printed circuit
board layout or output/input coupling.
When designing a layout, it is important to return the load
ground, the output compensation ground, and the low level
(feedback and input) grounds to the circuit board common
ground point through separate paths. Otherwise, large currents
flowing along a ground conductor will generate voltages
on the conductor which can effectively act as signals at
the input, resulting in high frequency oscillation or excessive
distortion. It is advisable to keep the output compensation
components and the 0.1 μF supply decoupling capacitors as
close as possible to the LM3886 to reduce the effects of PCB
trace resistance and inductance. For the same reason, the
ground return paths should be as short as possible.
In general, with fast, high-current circuitry, all sorts of problems
can arise from improper grounding which again can be
avoided by returning all grounds separately to a common
point. Without isolating the ground signals and returning the
grounds to a common point, ground loops may occur.
Click to expand...

You might note that this is a larger excerpt to what I posted before ;)

Tony.
 
H

hurtz

Member
Joined 2010
Just to make sure we're on the same page here, the marked grounds are those that the datasheet speaks of right? the common ground point can now be either on the AMP itself or on the PSU as I understand it. (I assume with the cGND on the AMP it is better to have seperate grounds on the PSU)
And interpreting the datasheet, Those GNDs should be returned individually, except for (low-level) feedback and input?


An externally hosted image should be here but it was not working when we last tested it.


Note to self: Get better in english >.<
 
Last edited:
Status
This old topic is closed. If you want to reopen this topic, contact a moderator using the "Report Post" button.
Top Bottom