How do you layout a printed circuit board like this - 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 27th August 2014, 11:40 PM   #1
diyAudio Member
 
Join Date: Aug 2010
Default How do you layout a printed circuit board like this

This is a top layer of an audio amp by IR in their AP note "iraudps1.pdf".

The layout looks like it was carved out of a solid copper layer, almost as if there was an anti trace command that lays down voids in the copper instead of traces.

I never heard of an anti trace command so it was probably copper fills. But even so it really looks like it was carved out, not poured.

Does anyone know what the procedure is for laying out a board like this.
Attached Images
File Type: jpg top layer audio amp.JPG (150.9 KB, 148 views)
Attached Files
File Type: pdf 12v car audio power supply IR design details 500W iraudps1.pdf (738.3 KB, 12 views)
  Reply With Quote
Old Yesterday, 12:55 AM   #2
rayma is offline rayma  United States
diyAudio Member
 
Join Date: Apr 2011
Location: Upper midwest
Quote:
Originally Posted by powerbob View Post
The layout looks like it was carved out of a solid copper layer, almost as if there was an anti trace command that lays down voids in the copper instead of traces.I never heard of an anti trace command so it was probably copper fills. But even so it really looks like it was carved out, not poured.
Does anyone know what the procedure is for laying out a board like this.
This particular pcb was made in the usual way, with a layout program that can "copper pour" in the blank areas,
with a small space left between the pour areas, and the traces and pads. Many recent programs can do this.

There are also pcb engraving machines that can make a single pcb that looks similar, but these pcbs lack plated through holes,
solder mask, and silk screen.

Last edited by rayma; Yesterday at 12:57 AM.
  Reply With Quote
Old Yesterday, 01:25 AM   #3
diyAudio Member
 
Join Date: Aug 2010
Quote:
Originally Posted by rayma View Post
This particular pcb was made in the usual way, with a layout program that can "copper pour" in the blank areas,
with a small space left between the pour areas, and the traces and pads. Many recent programs can do this.

There are also pcb engraving machines that can make a single pcb that looks similar, but these pcbs lack plated through holes,
solder mask, and silk screen.
So did they first draw out all of the shapes of the pours and then use a fill command?

And how are the traces handled. If you have a large copper pour area and it has traces in it, does the defined area just fill up with copper and flow around pre-existing traces with a specified clearance?
  Reply With Quote
Old Yesterday, 01:28 AM   #4
rayma is offline rayma  United States
diyAudio Member
 
Join Date: Apr 2011
Location: Upper midwest
Quote:
Originally Posted by powerbob View Post
So did they first draw out all of the shapes of the pours and then use a fill command?

And how are the traces handled. If you have a large copper pour area and it has traces in it, does the defined area just fill up with copper and flow around pre-existing traces with a specified clearance?
Normally the blank areas are automatically filled with the command, using a specified clearance from the pre-existing traces, pads, etc.
You don't have to draw the shapes, the pour is just set back from the existing copper areas.

Eagle does this, and there's a free version. http://www.cadsoftusa.com/download-e...e/?language=en

Last edited by rayma; Yesterday at 01:32 AM.
  Reply With Quote
Old Yesterday, 03:21 AM   #5
diyAudio Member
 
Join Date: Aug 2010
Quote:
Originally Posted by rayma View Post
Normally the blank areas are automatically filled with the command, using a specified clearance from the pre-existing traces, pads, etc.
You don't have to draw the shapes, the pour is just set back from the existing copper areas.

Eagle does this, and there's a free version. Free EAGLE PCB Design Software, Layout Software - CadSoft Freeware
I can understand a basic copper fill were it flows around all other copper and the fill is just a poor mans ground plane. But in this case the copper fill is actually the routing of the circuit. That is what i am impressed with. Very high current low impedance traces.
  Reply With Quote
Old Yesterday, 09:07 PM   #6
rayma is offline rayma  United States
diyAudio Member
 
Join Date: Apr 2011
Location: Upper midwest
Quote:
Originally Posted by powerbob View Post
I can understand a basic copper fill were it flows around all other copper and the fill is just a poor mans ground plane. But in this case the copper fill is actually the routing of the circuit. That is what i am impressed with. Very high current low impedance traces.
Looks like some of this is used as the ground plane. The larger signal areas can be placed manually by a polygon command, for example.
  Reply With Quote
Old Yesterday, 09:27 PM   #7
JMFahey is offline JMFahey  Argentina
diyAudio Member
 
JMFahey's Avatar
 
Join Date: Mar 2009
Location: Buenos Aires - Argentina
Quote:
Originally Posted by powerbob View Post
I can understand a basic copper fill were it flows around all other copper and the fill is just a poor mans ground plane. But in this case the copper fill is actually the routing of the circuit. That is what i am impressed with. Very high current low impedance traces.
Theres 2 ways to do this.

1) the bad/poor one, and which I see a lot in home designed magazine projects, is to design the PCB the conventional way, almost any software is enough, often with thin/inadequate tracks, and afterwards copper pour is invoked.

On first sight the PCB looks very solid, copper everywhere ... until you realize tracks are very thin, copper just fills empty space, does not "help" any track, it actually serves no useful purpose.

Ok, it might be used as a ground plane .

2) the good one.
The PCB is probably laid out first just with relatively thin tracks, but afterwards its filled up with useful copper, meaning its contiguous and attached to important tracks, mainly ground, power rails, speaker connections, etc.

Im an oldtimer and can only do that with fills, polygons, and playing with track thickness, but Im certain modern software can be programmed to do that automatically.

Even more, I guess software linked to simulators already "knows" which tracks carry most current and prioritize them.
  Reply With Quote
Old Yesterday, 10:27 PM   #8
dmills is offline dmills  United Kingdom
diyAudio Member
 
Join Date: Aug 2008
Location: High Wycombe
The usual way to skin this sort of thing is to use a combination of polygon pours and the ability to set the pour order.

So you might for example set the ground pour on the top side to happen last and define that polygon to occupy most of the board area then define polygons for your heavy current stuff to be poured before the ground polygon.
Nets that do not match the polygons net will cause the polygon to releave around them to meet the appropriate design rule, and where the polygon has the same net as a track you can often configure the behaviour to either flood over or keep clear (useful for things like analogue grounds heading to specific reference points).

Well, that is how Altium does it, most other tools have equivalent functionality.

Regards, Dan.
  Reply With Quote
Old Yesterday, 10:33 PM   #9
diyAudio Member
 
nigelwright7557's Avatar
 
Join Date: Apr 2008
Location: Carlisle, England
PCBCAD53 does it by filling in copper with a gap around anything not connected to the copper pour netname. This allows ground planes or in fact any plane connected to a set netname.

Sometimes a copper pour can cause problems by connecting two grounds that need star grounding.

I tend to just use grounded selective copper pours to protect sensitive audio signals.
__________________
PCBCAD50 software. http://www.murtonpikesystems.co.uk
  Reply With Quote
Old Today, 04:32 AM   #10
diyAudio Member
 
dchisholm's Avatar
 
Join Date: Mar 2011
Location: St Louis, Mo
Quote:
Originally Posted by dmills View Post
. . . use a combination of polygon pours and the ability to set the pour order . . . .
. . . . define polygons for your heavy current stuff . . .
Nets that do not match the polygons net will cause the polygon to releave around them to meet the appropriate design rule . . .
. . . where the polygon has the same net as a track you can often configure the behaviour to either flood over or keep clear . . .
I'm a bit rusty regarding my own PWB software, but I think that's how mine works.

Although a ground plane is typically created with a copper pour, don't think that "copper pour" is synonymous with "ground plane".

As I recall, my PWB software lets you define fixed-geometry copper polygons and specify them as electrically connected to ANY net on the board. And, you must provide a trace which makes that connection.

In fact, my software throws a design rule squawk for any "floating" copper. Every copper polygon, or copper pour, must be associated with a circuit net - but the pour or polygon can be defined as connected to ANY of the circuit nets on the board (not just ground).

You govern the behavior of traces, polygons, and pours by specifying design rules - the required clearance from a trace to a pour, how a trace connects to its associated net, the minimum area for a pour, etc.

You then pour all of the specified areas to create a PWB similar to what's shown in your photo.

Dale
  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
Make your Printed Circuit Board (PCB): mistygirl01 Power Supplies 3 19th March 2014 08:27 PM
Prototype Printed Circuit Board vendors RussT Solid State 0 13th March 2014 02:40 PM
Printed Circuit Board Manufacturer david1115 Vendor's Bazaar 1 16th December 2009 06:25 AM
Printed circuit board designing? Psychobiker Tubes / Valves 11 23rd March 2008 12:41 AM
Printed circuit board options? DanK Solid State 49 20th February 2003 11:35 AM


New To Site? Need Help?

All times are GMT. The time now is 04:20 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