PCBs please comment - 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 13th July 2004, 04:37 AM   #1
diyAudio Member
 
Join Date: Jun 2004
Location: HKSAR
Default PCBs please comment

Hi guys,

I am working on a MOSFET amplifier but over the weekend, I would like to do something different (just paper work) and I found this :

http://users.otenet.gr/~athsam/power_amp_300w.htm also at:
http://www.alphalink.com.au/~cambie/ETI466Web.htm

The first one had a double side PCB while the second one had the power part on it. I decide to try laying out the PCB myself. I put the 'big guys' in position first and then interconnecting them as the schematic along with the rest on the components list. I then try to straight-out the traces and move the 'small guys' around (moving and rotating) and come up with the following (as in attachment) :

If you gurus are generous enough, please give me some advice and comments in general. It's my first PCB that I did it all on my own and I am worried about interference, crosstalk and all that stuff. In particular I am concerned about the lengthy traces under R39,40 reaching for Q7-11. Could there be potential problems with these?

Any material I can read to get a better grip of PCB laying technique (or at least the do's and dont's) ?

PS. Anybody interest in having the layouts for the seperate layers? I can post them if you guys want it.
Attached Files
File Type: pdf pcb-layout.pdf (79.2 KB, 202 views)
  Reply With Quote
Old 13th July 2004, 11:44 AM   #2
diyAudio Member
 
Join Date: Dec 2003
Location: Mumbai
hi

there are lots to learn in an audio ampifier pcb layout drawing - speacially high power amps where the high current flow has to be thought about

this is how i went about it

take a sample pcb drawing - which you know is allright with no problem (construct it)

re lay out the stuff you want , add the power supply on the bord , add protections of all types , add output capacitors , ets

then build this new designed amp - connect a scope and see how this amp performs in all applications - square , triange , sine , entire freq range against the amp constructed inthe original design

then go about checking other amplifier design layouts a trip to a library - lots of ref books find out your mistakes and correct your own design

when you have comleted - u wil know quite a few things like where to place the input differential and how - upto the output

like this over the net i will give you a change to your drwaing - then some one else will , I would have my own theories about the change to your design - unless it is one to one it will be a mess - with others approving or disapproving and the fact is if i offer a change you will never know if it is for the better or ofr worse

suranjan

transducer design engineer
  Reply With Quote
Old 15th July 2004, 10:26 AM   #3
diyAudio Member
 
Join Date: Jun 2004
Location: HKSAR
Hey guys,

Don't tell me it is so nice that there is nothing to critisize and I hope that it is not that bad that it doesn't worth commenting on.
  Reply With Quote
Old 15th July 2004, 02:00 PM   #4
jcx is offline jcx  United States
diyAudio Member
 
Join Date: Feb 2003
Location: ..
Default well you did ask what we really think...

Power entry/distribution sucks; in class B the current in the output devices and power supply lines is highly nonlinear so that the inductive coupling from the ps current magnetic field can become a significant distortion source

By sending +/- rail current around the left/right edges of the board with the gnd/in/out in the middle you have nearly the worst possible power distribution scheme

Itís usually best to begin a layout with power/ouput/gnd, visualizing current flow and minimizing loop areas by putting high current source/return lines on top of each other with magnetic coupling cancellation from symmetry a second choice
  Reply With Quote
Old 17th July 2004, 04:54 AM   #5
diyAudio Member
 
Join Date: Dec 2003
Location: Mumbai
hi

what i tried telling in a sweet fashion above - u got it in verbatim now

take care

suranjan
  Reply With Quote
Old 17th July 2004, 10:44 AM   #6
diyAudio Member
 
traderbam's Avatar
 
Join Date: Jan 2002
Location: Earth
Quote:
please give me some advice and comments in general
Good start. It's very tidy and neat and not too densly laid out.

The typical things that need to be considered:
1) Are the electrical connections correct (does the layout match the schematic)?
2) Are the tracks big enough for the current they must conduct?
3) Are the track to track and track to pad spacings sufficient for the voltages between them and to reduce the chance of accidental shorting?
4) Copper does not have ZERO resistance (accidental signal mixing on shared conductors).
5) Unwanted magnetic pollution due to long tracks and current loops forming inductors
6) Unwanted electostatic pollution due to capacitance between tracks and pads
7) Radio frequency interference, both susceptance and pollution (usually only ciritcal for very high frequency circuits)
8) Reliability - pcb strength and mechanical resonances

In my experience both in audio and in commericial servo designs for computer drives, item 4 causes the most hair to be torn out. I cannot say this strongly enough to people: copper has resistance! Not all points on a ground plane will have the same voltage if there is any current flowing in it. I can't tell you how many problems this causes and how hard they are to find if you don't know what to look for. This is the main reason that people advocate star grounds - it is a way to avoid two current loops sharing the same resistive copper track and accidentally causing a mixing of the signals. Look at all your current loops, particularly those around your ground (0V) areas and make sure they don't share track where an interaction could cause a problem. Think of tracks as being small resistors - even draw them on your schematic and cosider what effects they will have.

Items 5 and 6 are often missed and have adverse affects on audio power amps. It is necessary to identify the high current paths and trace them across the pcb and through the psu cables back to the psu. All wires generate magnetic fields around them when current flows - this filed can induce currents in nearby conductors. Find the LOOPS (current flows in loops). Avoid having small signal circuits enclosed within a high current loop - a loop is an inductor even if it has just one turn and isn't a perfect circle. Capacitance exists between any adjacent tracks and pads - normally, at audio frequencies, this is a minor consideration and not as important as magnetic considerations. However, keep some distance between tracks and components that have large voltage changes and tracks and components that are voltage sensitive. For example, in a high feedback design the LTP inputs are very voltage sensitive and should be kept away from, say, the speaker output pad. At high frequencies, large pads and long tracks act like antennas and can pick up, or emit, RF noise. This is not normally important in an auio amp provided the amp circuit is adequately damped and stable at RF frequencies.

Quote:
I am concerned about the lengthy traces under R39,40 reaching for Q7-11.
See above, you can decide for yourself.
  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
FS: Aleph-X PCBs , NIGC PCBs , OPA541AM OpAmps e.lectronick Swap Meet 25 6th March 2013 07:40 PM
Please comment my pcb P3a roly3055 Solid State 53 8th June 2012 08:36 PM
please comment my pcb east electronics Solid State 75 10th November 2008 02:32 PM
Trade Aleph X PCBs for Aleph P 1.7 PCBs highbias Pass Labs 0 27th September 2004 05:59 PM


New To Site? Need Help?

All times are GMT. The time now is 02:51 PM.


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