PCB Layout Process and Guidelines? - Page 6 - 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 October 2012, 09:52 AM   #51
AndrewT is offline AndrewT  Scotland
diyAudio Member
 
Join Date: Jul 2004
Location: Scottish Borders
look at the length of the route from V+ through C7 to Power Ground and then back to V- thro' C8. That route has to pass transients approaching and maybe even exceeding tens of MHz.

The total route length should be <20mm and preferably <10mm.

To achieve this the Power Ground must be located between the V+ & V-

Speaker Ground/Return does not need to be on the PCB.
The output R//L of the Thiele Network does not need to be on the PCB.
I believe they are both better located off PCB.

Add multiple Pin Pitch options to as many caps as you can manage in the layout as is.
__________________
regards Andrew T.

Last edited by AndrewT; 13th October 2012 at 09:57 AM.
  Reply With Quote
Old 13th October 2012, 04:20 PM   #52
diyAudio Member
 
jkuetemann's Avatar
 
Join Date: Dec 2010
Location: Paris, Ontario
Quote:
Originally Posted by AndrewT View Post
look at the length of the route from V+ through C7 to Power Ground and then back to V- thro' C8. That route has to pass transients approaching and maybe even exceeding tens of MHz.

The total route length should be <20mm and preferably <10mm.

To achieve this the Power Ground must be located between the V+ & V-

Speaker Ground/Return does not need to be on the PCB.
The output R//L of the Thiele Network does not need to be on the PCB.
I believe they are both better located off PCB.

Add multiple Pin Pitch options to as many caps as you can manage in the layout as is.
OK, I was concerned about the bypass returns being so long. Could a separate ground be provided solely for the bypass return or is it best fed to the board's main star? Relocating the main star will require a complete redo. Are you referring to the total path from +V through C7 and C8 to -V being under 20mm or each rail through its respective bypass capacitor to ground being less than 20mm?

I understand the output inductor and speaker return can be located off board but aside from lost real estate is there any real disadvantage? That said the RC Zobel (C6 and R20) should remain local, correct?

Additional pin pitch options do make sense for a public consumption project. In this case, for this little project, I already have what I will be using, so the pitch is fixed at the moment.

All this said I'm seriously looking at scrapping the chosen board size and going with a larger PCB, but not just yet. This is to retrofit into a project I did over 10 years ago and would like to reuse the heatsink and not disturb the existing layout if possible.

Thanks for you input thus far. I'm slow with the artwork, I find I spend much time just looking and mentally routing and repositioning. I'll post some different options as they present themselves.
__________________
---Jason Kuetemann---
When the student is ready, the master appears.
  Reply With Quote
Old 13th October 2012, 04:37 PM   #53
AndrewT is offline AndrewT  Scotland
diyAudio Member
 
Join Date: Jul 2004
Location: Scottish Borders
Quote:
Originally Posted by jkuetemann View Post
OK, I was concerned about the bypass returns being so long. Could a separate ground be provided solely for the bypass return or is it best fed to the board's main star? Relocating the main star will require a complete redo. Are you referring to the total path from +V through C7 and C8 to -V being under 20mm or each rail through its respective bypass capacitor to ground being less than 20mm?.............................That said the RC Zobel (C6 and R20) should remain local, correct?
total length from V+ to V- via the HF decoupling <10mm. The MF decoupling route can be much longer maybe 50mm for total route. And yes, the decoupling Ground is actually the Power Ground. The HF decoupling Ground should be connected to the MF decoupling Ground and the ground from the PSU connects here. The speaker does not need to connect here. The Zobel does need to connect here. It too passes HF and it too needs a very short route.
Quote:

...........is there any real disadvantage?
the air cored coil should not be near iron components, maybe just as important, other sensitive audio components should not be near the field of the air core. If that is the case, then the coil and it's damping resistor need to be off PCB.

Once you have the HF & MF decoupling grounds connected and you bring power into this same Ground and also bring the Zobel capacitor to here as well there are only two other connections on the PCB that need referencing to the Power Ground. The Signal Ground isolating resistor comes here and other small current grounds come here.

In summary:
Locate the Power Ground right in the middle of the output stage and bring all the other connections to this location.

Don't spread the Ground around the PCB. I don't think that achieves any benefits. Guess what? That's the opposite to a ground plane. I have regularly argued against that unless you know how and why that plane is needed/works.
__________________
regards Andrew T.

Last edited by AndrewT; 13th October 2012 at 04:45 PM.
  Reply With Quote
Old 13th October 2012, 05:27 PM   #54
diyAudio Member
 
jkuetemann's Avatar
 
Join Date: Dec 2010
Location: Paris, Ontario
So I will move the output inductor and damping resistor to a separate board at the speaker terminals as shown. I then elected to make the output network a Pi network by following up the inductor with another Zobel, R22 and C9 on the revised schematic.
Attached Images
File Type: jpg Output Board.JPG (138.4 KB, 262 views)
File Type: jpg Generic Amp Schematic.jpg (389.2 KB, 263 views)
__________________
---Jason Kuetemann---
When the student is ready, the master appears.
  Reply With Quote
Old 13th October 2012, 05:36 PM   #55
diyAudio Member
 
Join Date: Oct 2011
Quote:
Originally Posted by jkuetemann View Post
So here's a version that has no large high current traces on opposing edges of the PCB, fusing will be off board on the PSU instead. Some components are a little better spaced and more distance between many of the traces. Any comments? Better or worse than the one on post #40 and why?
The bias is tracking the output transistors rather than the drivers. This is very strong tracking indeed. How would mounting everything on main heat sink work out ? So that all dies are almost at the same temperature together with the added benefit of higher hfe, although would this cause instability ?

The layout looks interesting and you have covered most issues although a few may need addressing
__________________
www.harrisonaudiolabs.com
  Reply With Quote
Old 13th October 2012, 05:41 PM   #56
diyAudio Member
 
Join Date: Oct 2011
Quote:
Originally Posted by jkuetemann View Post
So I will move the output inductor and damping resistor to a separate board at the speaker terminals as shown. I then elected to make the output network a Pi network by following up the inductor with another Zobel, R22 and C9 on the revised schematic.
Mouting them off-board may be ok, however where is that gnd connection to speaker coming from

Assume you have large decoupling caps on board which you dont, assume that this is a multi channel system which you will tell us Assume that due to the large onboard decoupling caps, there is a sizeable current running on the gnd about 4 A, assume that there is resistance between the star ground and onboard ground of about 0.15 ohms. What would be the voltage difference between the two grounds ?
__________________
www.harrisonaudiolabs.com

Last edited by OnAudio; 13th October 2012 at 05:49 PM.
  Reply With Quote
Old 13th October 2012, 06:21 PM   #57
AndrewT is offline AndrewT  Scotland
diyAudio Member
 
Join Date: Jul 2004
Location: Scottish Borders
The Speaker Return connects to the Main Audio Ground (MAG).

That MAG has connections running to>
1.) Signal Ground @ either the PCB, or at the RCA input.
2.) Speaker Return.
3.) Power Ground on the PCB.
4.) PSU Zero Volts.
5.) Chassis, either direct, or via a Disconnecting Network.
6.) optional auxiliary grounds/references.
__________________
regards Andrew T.
  Reply With Quote
Old 13th October 2012, 06:31 PM   #58
diyAudio Member
 
5th element's Avatar
 
Join Date: Oct 2002
Location: England
I find it amusing and frustrating at the same time, that almost everything regarding high performance in PCB design comes from optimising the return paths.
__________________
What the hell are you screamin' for? Every five minutes there's a bomb or somethin'! I'm leavin! bzzzz!
  Reply With Quote
Old 14th October 2012, 01:59 AM   #59
diyAudio Member
 
jkuetemann's Avatar
 
Join Date: Dec 2010
Location: Paris, Ontario
The design of a PCB I'm relatively new at. In the past I just connected everything that needed connected in what seemed to be the most logical fashion and it seemed to work. At this point I'm looking to learn a few tricks and up my skills in the PCB department. That is really to point of the thread, so I am going based on a relatively simple conventional design as the basis of my learning curve.

Thanks for the input so far and I'll continue to rework the design an post my progress. I'm not fast with the artwork, but I'm working on it.
__________________
---Jason Kuetemann---
When the student is ready, the master appears.
  Reply With Quote
Old 14th October 2012, 02:08 AM   #60
diyAudio Member
 
nigelwright7557's Avatar
 
Join Date: Apr 2008
Location: Carlisle, England
Ground loops can be a big problem in pcb design.
I laid out an audio mixer just as it came and when I got the pcb back there was loads of hum.

I relaid it out seperating the power supply ground from the rest of the circuit and there was almost zero hum. So using star grounds is a good tip. I have notcied a lot of amps have seperate power supply pcb's so perhaps they have coem across the same problem that I did.
__________________
PCBCAD50 software. http://www.murtonpikesystems.co.uk
  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
Eagle vs. Sprint-Layout for PCB design/layout hollowman Parts 11 12th January 2014 10:01 PM
About PCB layout gaetan8888 Solid State 14 11th January 2008 05:11 AM
PCB Manufacturing Process with Eagle PCB Algar_emi Parts 0 21st September 2007 02:07 AM
Amplifier PCB Layout Guidelines? ron.eddy Parts 19 18th December 2005 06:17 PM
PCB design guidelines mangrovejack Parts 3 10th July 2005 12:10 PM


New To Site? Need Help?

All times are GMT. The time now is 03:27 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