LM3886 PCB layout questions - diyAudio
Go Back   Home > Forums > Amplifiers > Chip Amps

Chip Amps Amplifiers based on integrated circuits

Please consider donating to help us continue to serve you.

Ads on/off / Custom Title / More PMs / More album space / Advanced printing & mass image saving
Reply
 
Thread Tools Search this Thread
Old 19th April 2015, 01:31 PM   #1
zAAm is offline zAAm  South Africa
diyAudio Member
 
zAAm's Avatar
 
Join Date: Mar 2014
Location: Potchefstroom
Default LM3886 PCB layout questions

Hi guys,

First post, but I have read a lot of comments here on the LM3886, and I've come up with a PCB that I'd like some feedback on.

Some points I'm not clear on (I've seen/read some conflicting comments on these):

1) Should PIN7 (GND) be connected to the PS ground or to the star signal ground?
2) Should the output ground return (at the terminal) be connected to the PS ground or to the star signal ground?
3) I've read somewhere that it may be better to connect the Zobel network (RSN+CSN) directly to the ground at the output terminal? Feels like this would only increase the length of the loop?

Any comments would be greatly appreciated!
Attached Images
File Type: png board.png (30.0 KB, 218 views)
File Type: png schem.png (13.9 KB, 209 views)
  Reply With Quote
Old 19th April 2015, 04:33 PM   #2
diyAudio Member
 
palstanturhin's Avatar
 
Join Date: Jun 2011
You have two layers. Use that advantage to create a audio ground plane. To this you connect everything that has to do with AUDIO. Connect the audio ground to the power ground at the C2+/C2- ground point. Connect the zobel to the C2+/C2- ground point.
  Reply With Quote
Old 20th April 2015, 01:05 PM   #3
zAAm is offline zAAm  South Africa
diyAudio Member
 
zAAm's Avatar
 
Join Date: Mar 2014
Location: Potchefstroom
Would a low impedance path (i.e. signal ground plane) be better than a star ground? I know the National datasheet recommends a star ground...
  Reply With Quote
Old 20th April 2015, 01:34 PM   #4
AndrewT is online now AndrewT  Scotland
diyAudio Member
 
Join Date: Jul 2004
Location: Scottish Borders
With the thick PCBs that we use for 2 layer boards, I don't think there can be any advantage in adopting one plane for one of:- Power +, or Power-, or Power Zero, or Signal Return.

Component layout rules.

That is more important than just about anything else.
They control where your traces must run. The trace/component loops control the tolerance to interference effects.
__________________
regards Andrew T.
  Reply With Quote
Old 20th April 2015, 05:07 PM   #5
zAAm is offline zAAm  South Africa
diyAudio Member
 
zAAm's Avatar
 
Join Date: Mar 2014
Location: Potchefstroom
Thanks for the input.

Would you care to give some pointers on component layout rules for the LM3886 Andrew?

I tried to keep loops as short as possible, but it seems that this is mostly dictated by the size and number of components... Inevitably it also leads to prioritizing small loops for some components over others (i.e. Rf gets priority over Rsn etc.)

Also, I'm thinking of mounting the Cc compensation capacitor on the bottom of the board since I guess the extra lead inductance would counteract the working of it. How critical is this extra inductance to avoid high frequency oscillations?

palstanturhin, I gather from your post that you recommend connecting the Zobel network to the power ground as well as the output ground. Granted the noise level is much larger at the output, but wouldn't it potentially pick up noise from the power ground?
  Reply With Quote
Old 20th April 2015, 05:18 PM   #6
tomchr is offline tomchr  United States
diyAudio Member
 
tomchr's Avatar
 
Join Date: Feb 2009
Location: Greater Seattle Area
My advice to you would be exactly the same as the advice I gave in this thread: My take on a LM3886 layout

If you're interested in the background, I suggest reading through my Taming the LM3886 Chip Amplifier pages. The only edit I need to make to those pages is that the "optional stability components" (Rf2, Cf, Cc in the data sheet schematics for the LM3886) actually do improve stability and should be included.

Tom
__________________
Modulus-86: Composite amp achieving 0.00014 % THD. Damn Good 300B, Novar Spud, 21st Century Maida Reg., Filament Reg., etc.
Neurochrome : : Audio - http://www.neurochrome.com - Engineering : : Done : : Right
  Reply With Quote
Old 20th April 2015, 08:44 PM   #7
zAAm is offline zAAm  South Africa
diyAudio Member
 
zAAm's Avatar
 
Join Date: Mar 2014
Location: Potchefstroom
Sorry, I actually read that thread a while ago, somehow it didn't stick apparently.

I added a signal ground plane on the top (red) and bottom (blue) layers as well as fills for all the power traces.

Cc will be soldered on the bottom of the PCB so I removed it from the board.

How does this look?
Attached Images
File Type: png board2.png (26.7 KB, 143 views)
File Type: png board2t.png (20.6 KB, 141 views)
File Type: png board2b.png (22.7 KB, 139 views)
  Reply With Quote
Old 20th April 2015, 09:47 PM   #8
diyAudio Member
 
Join Date: Jul 2014
.
Every TI data sheet I've seen lately makes the following recommendation, slightly edited by me.

===

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 which can act as signals at the input, resulting in high frequency oscillation or excessive distortion.

===

The below illustration calls out the various grounds referenced by the data sheets.

It might be worth noting that ground planes can create more problems than they solve. The reason is that the ground plane, like all conductors, has resistance, and this resistance varies throughout the layer of copper.

This means that currents do not flow through the ground plane in an idealized smooth sheet, but take the path of least resistance from any point to any other point. The result can be unexpected inductance and/or capacitance where they will do the most harm.

The bottom line is that the factory works out its ground plane recommendations--if any--with considerable engineering expertise. Lacking such expertise using a ground plane might be something of a crap shoot, and discrete conductors to the single circuit ground point might give a better result.

On the other hand, that's a seriously good looking board you posted.
.
Attached Images
File Type: jpg audio-amp-grounding-points-042015.jpg (48.4 KB, 71 views)
  Reply With Quote
Old 20th April 2015, 09:48 PM   #9
tomchr is offline tomchr  United States
diyAudio Member
 
tomchr's Avatar
 
Join Date: Feb 2009
Location: Greater Seattle Area
For best performance, you want a low-impedance connection between the input/feedback ground and the speaker ground terminal. I pointed that out in Post #10 of the thread linked to above. You can see the difference such a low-impedance ground makes in the LM3886 P2P vs PCB (with data) thread. It's Post #30 of that thread.

Low impedance --> short, wide trace. The shortest and widest trace you can get is a plane.

Tom
__________________
Modulus-86: Composite amp achieving 0.00014 % THD. Damn Good 300B, Novar Spud, 21st Century Maida Reg., Filament Reg., etc.
Neurochrome : : Audio - http://www.neurochrome.com - Engineering : : Done : : Right

Last edited by tomchr; 20th April 2015 at 09:50 PM.
  Reply With Quote
Old 20th April 2015, 09:53 PM   #10
tomchr is offline tomchr  United States
diyAudio Member
 
tomchr's Avatar
 
Join Date: Feb 2009
Location: Greater Seattle Area
Quote:
Originally Posted by bentsnake View Post
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.
Which is why my recommendation is to set up a quiet section of ground plane for the signal ground (= feedback and input) and connect it to the power ground plane at the speaker connector ground connection.

Tom
__________________
Modulus-86: Composite amp achieving 0.00014 % THD. Damn Good 300B, Novar Spud, 21st Century Maida Reg., Filament Reg., etc.
Neurochrome : : Audio - http://www.neurochrome.com - Engineering : : Done : : Right
  Reply With Quote

Reply


Hide this!Advertise here!
Thread Tools Search this Thread
Search this Thread:

Advanced Search

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are Off
Refbacks are Off


Similar Threads
Thread Thread Starter Forum Replies Last Post
LM3886 PCB Layout undefinedza Chip Amps 9 5th July 2012 07:52 AM
My tiny single sided LM3886 PCB layout. :) Russ White Chip Amps 74 14th September 2008 06:53 PM
pa100 pcb single sided layout lm3886 dgaxeman Chip Amps 6 24th May 2006 01:45 AM
pcb layout for lm3886 squadra Chip Amps 27 18th July 2004 07:57 PM


New To Site? Need Help?

All times are GMT. The time now is 06:57 PM.


vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2015 DragonByte Technologies Ltd.
Copyright 1999-2015 diyAudio

Content Relevant URLs by vBSEO 3.3.2