LM4780 stereo Power-amp PCB design - diyAudio
Go Back   Home > Forums > Amplifiers > Solid State

Solid State Talk all about solid state amplification.

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 27th August 2010, 10:57 AM   #1
diyAudio Member
 
Join Date: Aug 2010
Default LM4780 stereo Power-amp PCB design

Hi

I have started an amplifier design and have found that LM4780 is a good choice. I examined datasheet and thought that reference PCB design is complex and big.

I have designed a smaller PCB, wherein i used LM4780 in inverting configuration. But i have doubts on grounding. Datasheet says that a star ground is good but instead i have placed a large ground plane and placed as much possible as ground connections on the plate.

Any opinions?

BTW, later on i may post .dsn .lyt (proteus) files.
Attached Images
File Type: png lm4780pcb.PNG (118.9 KB, 412 views)
  Reply With Quote
Old 27th August 2010, 11:48 AM   #2
diyAudio Member
 
donpetru's Avatar
 
Join Date: Jun 2007
Location: Romania
The ground plane is not well draw. The assembly will work like this, but not very well. I recommend to place electrolytic capacitors on the right or left LM, and their common terminals leading to ground, represent a point common to the entire PCB assembly.

Nice day.
__________________
AV400v2 and GX400 audio amplifier projects
PCB Design Services - for prototypes OR serial products, Today Tehnium and Forums
  Reply With Quote
Old 27th August 2010, 11:50 AM   #3
AndrewT is offline AndrewT  Scotland
diyAudio Member
 
Join Date: Jul 2004
Location: Scottish Borders
get rid of the ground plane.

Save it for when you understand why a ground plane works, at what frequencies it works, and how to design your ground plane to achieve the performance you desire. That might be never if you stay with analogue audio.
__________________
regards Andrew T.
  Reply With Quote
Old 27th August 2010, 11:52 AM   #4
diyAudio Member
 
Join Date: Aug 2010
@donpetru, where should i connect the other ends of the cap? what do you mean by left and right of LM?

@AndrewT, i thought it provides a low resistance path to all ground connections, which would probably reduce effect of high currents.

Furthermore, it's still a star topology, u c?

Last edited by thepcman; 27th August 2010 at 12:03 PM.
  Reply With Quote
Old 27th August 2010, 12:07 PM   #5
diyAudio Member
 
donpetru's Avatar
 
Join Date: Jun 2007
Location: Romania
I mean right or left side LM4780 in the your PCB. More specifically, the power connector should be one (not two as you) and electrolytic capacitors to be close to the connector.

Secondly, it is important to respect the distance between the PCB traces according to the latest normative (see here last attachment - you need to log in if you wish view):
Standarde si notiuni teoretice utile in proiectare PCB - Comunitatea Tehnium Azi
__________________
AV400v2 and GX400 audio amplifier projects
PCB Design Services - for prototypes OR serial products, Today Tehnium and Forums
  Reply With Quote
Old 27th August 2010, 12:14 PM   #6
diyAudio Member
 
Join Date: Jun 2004
Location: the Netherlands
Quote:
Originally Posted by thepcman View Post
Hi

I have started an amplifier design and have found that LM4780 is a good choice. I examined datasheet and thought that reference PCB design is complex and big.

I have designed a smaller PCB, wherein i used LM4780 in inverting configuration. But i have doubts on grounding. Datasheet says that a star ground is good but instead i have placed a large ground plane and placed as much possible as ground connections on the plate.

Any opinions?

BTW, later on i may post .dsn .lyt (proteus) files.
Dear,

I am sorry but I don't really like your PCB layout.

I am sure others have other opinions but for me a good PCB layout follows the rules below:

1: Differential signals and power supply lines are always routed in close pairs.
2: Input and output are separated
3: High current signals (PSU and OUTPUT) close together, staged with multilayers
4: PSU capacitors close together, and PSU routing on the left side, line input routing on the right side (keep them separate)

5: Grounding, In case of star-ground, route each ground-trace separate back to the common ground point (avoid serial grounding). In case of a ground-plane, They can work really well, but only if you do it right, and in most cases to do it right you need a 4 layer board. A ground-plane should be unbroken (no traces or lines) and on a layer of it's own all reserved to function as ground-plane. Then you must place components very careful and study the current return loop of each part, and keep those currents in mind when you place components.

In your particularity case, Your low level line input signals are all buried in a loop of high current signals. A better choice would be to route the PSU all on the right side, and feed the chip from the right side. The audio line signal on the right side. The outputs in the middle in front of the chip. Please take a look here for an example: sjostromaudio.com - QRP02 The SMD Gainclone - high performance mono power amplifier

Get rid of the serial ground polygon. This doesn't work as real ground-plane. Make a common ground point, and route each ground trace separate to here. PSU capacitors should be close together, and not with a long ground joint between them.

Good luck!

With kind regards,
Bas
  Reply With Quote
Old 27th August 2010, 12:37 PM   #7
diyAudio Member
 
Join Date: Aug 2010
Yeah Sebastian, i got your points

In fact i do not want to use a double layer PCB cos my man cannot put through a good pcb with two sides, i generally construct my designs on a single layer and if necessary i use jumpers (which are seen as top layer of pcb in the pic)

Then i will give it another try and post it.

Meanwhile, i will of course accept any other comments
  Reply With Quote
Old 27th August 2010, 12:44 PM   #8
diyAudio Member
 
Join Date: Jun 2004
Location: the Netherlands
Quote:
Originally Posted by thepcman View Post
Yeah Sebastian, i got your points

In fact i do not want to use a double layer PCB cos my man cannot put through a good pcb with two sides, i generally construct my designs on a single layer and if necessary i use jumpers (which are seen as top layer of pcb in the pic)

Then i will give it another try and post it.

Meanwhile, i will of course accept any other comments
Okay,

In that case you just need clever routing. Take your time to consider all points. For sure in your case use a star ground then. Even though you are using a single layer PCB with jumpers, you can still keep the PSU lines together and feed it from the left side, and feed the line level from the right side.

Good luck!

With kind regards,
Bas
  Reply With Quote
Old 27th August 2010, 12:59 PM   #9
diyAudio Member
 
Join Date: Aug 2010
Yeah, i will consider those
  Reply With Quote
Old 27th August 2010, 01:17 PM   #10
AndrewT is offline AndrewT  Scotland
diyAudio Member
 
Join Date: Jul 2004
Location: Scottish Borders
Quote:
Originally Posted by Sebastiaan View Post
1: Differential signals and power supply lines are always routed in close pairs.
Hi,
this is important.
Both in the flow and return wires to the PCB and in the flow and return traces carrying currents across the PCB.
__________________
regards Andrew T.
  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
Power Amp PCB design, grounding prairiemystic Solid State 77 6th July 2010 01:48 PM
LM3886 stereo - PCB design Razor_x Chip Amps 2 3rd July 2009 01:18 PM
LM4780 Bridged PCB Design Gcollier Chip Amps 3 14th February 2005 02:50 AM
LM4780 PCB power transformer Jim Karr Chip Amps 1 6th January 2005 07:29 PM
LM4780 PCB Design Thoughts Gcollier Chip Amps 0 4th March 2004 06:51 PM


New To Site? Need Help?

All times are GMT. The time now is 05:57 AM.


vBulletin Optimisation provided by vB Optimise (Pro) - vBulletin Mods & Addons Copyright © 2014 DragonByte Technologies Ltd.
Copyright 1999-2014 diyAudio

Content Relevant URLs by vBSEO 3.3.2