Ground pplane - Page 2 - diyAudio
Go Back   Home > Forums > Amplifiers > Power Supplies

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 24th November 2011, 12:35 AM   #11
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
Quote:
Originally Posted by epilot View Post
Hi, and thanks.

What do you really mean by "conductor pairs"? I though that the enclosed loop problem is just for ground or each trace itself, now you seem to say that it happens between pairs too (for instance between VCC trace and ground)!
Furthermore plz how it acts as an antenna!?

It would be ok if you could plz show me what you are meaning by a pic...

Thanks again
Google Faraday's Law.

In practical terms, for the layout you gave, just make the distance between the power rails and the large copper ground area as small as possible, everywhere. And twist tightly together any wire pairs that go from or to the board, and everywhere else in your power supply and other circuits.

It will also be very important for things like input signal and signal ground pairs. Either twist tightly together, all the way from input jack to input resistor, or, even better, use shielded twisted pair with shield connected to chassis (NOT signal ground to chassis!) at input end and not connected to anything at other end. Signal ground conductor connects ONLY at the input and at the ground end of the input resistor of the first amplification device (which then has a conductor of its own that goes to the main star ground point. i.e. the input jack (both signal and signal ground portions), must be completely isolated (electrically insulated) from the chassis.

Last edited by gootee; 24th November 2011 at 12:57 AM.
  Reply With Quote
Old 24th November 2011, 12:54 AM   #12
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
Quote:
Originally Posted by epilot View Post
But plz google the schematics for the 78/79xx regulators. MOST of them have big caps at their outputs....
And you would believe "most schematics" instead of believing the manufacturer's datasheet?!

You should probably read several different linear regulator datasheets from each of several different manufacturers. ALSO, search their websites for Application Notes about linear regulators. Sometimes, they might say that you could use a somewhat-larger capacitor at the regulator's output, but they almost always mention, in some way, that it shouldn't be "too large".

Unless you have a proper mathematical justification, just follow the recommendation on the manufacturer's datasheet for the exact device that you are using.

If you are going to use a capacitor on the load side of a regulator, then you would want to place it as close as possible to the point of LOAD, where it can do the most good. And often or usually you would want to have both large and small capacitors at the point of load, e.g. some electrolytic and some small ceramic such as 0.1 uF. ("What C values?", you ask. Ideally, the capacitors' self-resonant frequencies will cover the frequencies of the currents demanded by the load. Caps' self-resonant freqs depend on C values and caps' parasitic inductances and the trace's parasitic inductance. If in doubt, first try 10 uF electrolytic in parallel with 0.1 uF X7R ceramic, at each chip power pin, to ground. Larger current demands would need larger than 10 uF. Higher frequencies would need lower than 0.1 uF.)

But still you have to be careful that none of those capacitances will form an unwanted high-frequency resonance with either the trace inductance or the inductance of any of the capacitors. Lossy capacitors are sometimes best.
  Reply With Quote
Old 24th November 2011, 11:47 AM   #13
marce is online now marce  United Kingdom
diyAudio Member
 
Join Date: Jun 2007
Location: Blackburn, Lancs
http://www.x2y.com/filters/TechDay09...%20_JohnWu.pdf

http://www.elmac.co.uk/pdfs/Lord_of_the_board.pdf

Last edited by marce; 24th November 2011 at 11:53 AM.
  Reply With Quote
Old 24th November 2011, 05:47 PM   #14
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
Perfect! Thanks for these, marce!
  Reply With Quote
Old 24th November 2011, 05:52 PM   #15
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
Quote:
Originally Posted by epilot View Post
Hi, and thanks.

What do you really mean by "conductor pairs"? I though that the enclosed loop problem is just for ground or each trace itself, now you seem to say that it happens between pairs too (for instance between VCC trace and ground)!
Furthermore plz how it acts as an antenna!?

It would be ok if you could plz show me what you are meaning by a pic...

Thanks again
You PCB would be much better if you would use a two-sided board and use the entire bottom side as a ground plane. You would only need to etch small areas on the bottom ground-plane side that were below a through-hole pad that would be soldered on the top side. (OK, you might need a couple of very short traces on the bottom side, for the large capacitors, unless you can angle them enough, or lay them on their sides or something, to enable soldering two of their leads on the top side of the board. And the jacks might need some short bottom-side traces to get to vias next to them, unless you used right-angle jacks.)

Last edited by gootee; 24th November 2011 at 06:04 PM.
  Reply With Quote
Old 24th November 2011, 08:03 PM   #16
diyAudio Member
 
Join Date: Nov 2010
Location: The City, SanFrancisco
marce

Thanks for the links.
Briefly went through the first, one area where I dont typically comform is the placing bypass caps on the same layer as the active parts and avoiding via's.
For me the added via inductance is still near the capacitors ideal self inductance and being able to place them elsewhere clears up the critical io routing. This can be done with ground and power planes, then I am able to place the connecting via's right at the active components power leads. Even without power planes I still find that I am able to better able to keep the supply impedance lower out to higher frequencies with large traces on the bottom side (especially since the by-pass capacitors spacing can then more easily straddle power leads, in the absence of planes).
This is just a practical situation that I seem to run into all the time.
Hope this helps
-Antonio
  Reply With Quote
Old 25th November 2011, 11:34 AM   #17
AndrewT is offline AndrewT  Scotland
diyAudio Member
 
Join Date: Jul 2004
Location: Scottish Borders
Good links.
Thanks.
__________________
regards Andrew T.
  Reply With Quote
Old 25th November 2011, 11:43 AM   #18
marce is online now marce  United Kingdom
diyAudio Member
 
Join Date: Jun 2007
Location: Blackburn, Lancs
Henry Ott, page 458
Most of my data is in PDF form with my CAD libaries so I can access the info readily,
at the moment I have to use a DVD to back this lot up! So I am trying to do some housekeeping and checking documents for updates etc, as I have been collecting this stuff for years (including magazines such as Printed Circuit Design and Fabrication and SMT) and as I am rather disorganised its a bit of a long term project... But here is a zip of a collection of PCB related links including soem good Signal Integrity sites that you may find useful.
One day I will get organised...
Attached Files
File Type: zip MARCs-PCB-stuff.zip (8.0 KB, 20 views)
  Reply With Quote
Old 3rd December 2011, 06:34 PM   #19
gootee is offline gootee  United States
diyAudio Member
 
Join Date: Nov 2006
Location: Indiana
Blog Entries: 1
I ordered the latest version of Henry Ott's book.
  Reply With Quote
Old 5th December 2011, 09:13 PM   #20
tvrgeek is offline tvrgeek  United States
diyAudio Member
 
Join Date: Dec 2009
Location: Md
78/79 regulators are not the best by today's standards, but that was not your question.
Let me be very contrary: There is no such thing as ground, just a place arbitrarily designated as a circuit reference point. There is no magic in shape. You should treat the source and sink with the same diligence. My habit is to use double side board and make the top all ground. This gives me more space to deal with V+ and V- on the bottom side and a cleaner, more straight, and more compact layout. ref: comment by gootee.
  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
Should I directly connect my signal ground to chassis ground? Bricolo Solid State 4 18th March 2014 09:42 PM
Parallel LM3886, input ground, power ground, safety resistor and oscillations. markiemrboo Chip Amps 5 9th August 2007 03:50 PM
DC filament ground and high voltage ground mikeyho Tubes / Valves 0 15th September 2005 05:52 PM
Chassis Ground = Circuit Ground --> Problems? rhildenbrand Pass Labs 5 23rd April 2004 01:08 AM
does connecting mains ground with circuit ground create a ground loop? jarthel Everything Else 0 25th June 2003 12:55 PM


New To Site? Need Help?

All times are GMT. The time now is 03:21 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