Four layer board design using eagle

Am 21.12.2010 06:57, schrieb Sandeep:

Hello everybody,

I have to design a four layer pcb using eagle. It should have two outer

signal layers and inner ground and vcc layer. Can anybody provide me a link

which would give me all the stepwise details to four layer PCB design? Even

if you have some suggestion for a four layer design, please post here. Any

help would be highly appreciated! Thank you.

1. DRC - Layer - Setup  (12*1516)

2. define inner layer as power plane

    LAYER 2 $GND;

3. define inner layer as power plane

    LAYER 15 $VCC;

Please read

HELP LAYER (enter)

..\doc\manual_en.pdf

6.2 Considerations Prior to Creating a Board  (page 131)

6.5 Multilayer Boards  (Inner Layer  page 160)

<http://www.cadsoft.de/cgi-bin/download.pl?page=/home/cadsoft/html_public/download.htm.de&dir=eagle/userfiles/doc&sort=name>

layer-setup_designrules.pdf

Mit freundlichen Grüßen / Best regards

Alfred Zaffran

--

_____________________________________________________________

Alfred Zaffran              Support

CadSoft Computer GmbH       Hotline:   08635-698930

Pleidolfweg 15              FAX:       08635-698940

84568 Pleiskirchen          eMail: <alf@cadsoft.de>

                             Web:   <www.cadsoft.de>

Registergericht: Amtsgericht Traunstein HRB 5573

Geschäftsführer: Dipl.-Ing. Klaus Schmidinger, Bodo Badnowitz

_____________________________________________________________

sandeep4386 wrote on Tue, 21 December 2010 00:57

I have to design a four layer pcb using eagle. It should have two outer

signal layers and inner ground and vcc layer.

Are you sure you really need to dedicate a whole plane to power?  Usually

this is unnecessary and the extra plane is better used for more routing

flexibility.  Daisy chained power is OK as long as it's bypassed to the

ground plane at each point of use and of course the traces are big enough

to not cause excessive voltage drop.  This is where a net class is useful.

Quote:

Can anybody provide me a link which would give me all the stepwise

details to four layer PCB design? Even if you have some suggestion for a

four layer design, please post here. Any help would be highly

appreciated!

There is nothing magic about 4 layers.  The schematic is the same.  When

you first create the board, make sure to set up the DRC for four layers,

and of course your other constraints like minimum width/space.

Right from the start, create a polygon in layer 2 named "GND" (or whatever

the name of your ground net is).  After that, placement and routing is

really no different from a 2 layer board.  You manually route the critical

sections, then let the autorouter figure out the rest.

The autorouter needs to be set up for 4 layers, with a very high cost to

running traces in polygons.  This prevents it from breaking up your ground

plane unless it sees no other alternative.  Generally that won't happen

unless you seriously painted yourself into a corner with the layout.

--

Web access to CadSoft support forums at www.eaglecentral.ca.  Where the CadSoft EAGLE community meets.

On 12/21/2010 4:31 AM, Olin Lathrop wrote:

sandeep4386 wrote on Tue, 21 December 2010 00:57

>> I have to design a four layer pcb using eagle. It should have two outer

>> signal layers and inner ground and vcc layer.

 

Are you sure you really need to dedicate a whole plane to power? Usually

this is unnecessary and the extra plane is better used for more routing

flexibility. Daisy chained power is OK as long as it's bypassed to the

ground plane at each point of use and of course the traces are big enough

to not cause excessive voltage drop. This is where a net class is useful.

 

Quote:

>> Can anybody provide me a link which would give me all the stepwise

>> details to four layer PCB design? Even if you have some suggestion for a

>> four layer design, please post here. Any help would be highly

>> appreciated!

 

There is nothing magic about 4 layers. The schematic is the same. When

you first create the board, make sure to set up the DRC for four layers,

and of course your other constraints like minimum width/space.

 

Right from the start, create a polygon in layer 2 named "GND" (or whatever

the name of your ground net is). After that, placement and routing is

really no different from a 2 layer board. You manually route the critical

sections, then let the autorouter figure out the rest.

 

The autorouter needs to be set up for 4 layers, with a very high cost to

running traces in polygons. This prevents it from breaking up your ground

plane unless it sees no other alternative. Generally that won't happen

unless you seriously painted yourself into a corner with the layout.

 

I would go with Olin's excellent advice on this. I would not use power

planes, but rather polygons. If you have a lot high speed or impedance

controlled traces, you have to be very careful how you break up the

supply copper as it will be a current return, usually it's not an issue.