Author Topic: Eagle PCB - Layer Stack Settings  (Read 15764 times)

0 Members and 1 Guest are viewing this topic.

Offline David

  • Frequent Contributor
  • **
  • Posts: 264
  • Country: gb
Eagle PCB - Layer Stack Settings
« on: January 19, 2010, 10:08:22 pm »
Hi all,
Just a quick question. I am trying to set-up a 4 layer board in eagle for production at PCB cart with the following layers:

1. Signal
2. GND
3. VCC
4. Signal

Does anyone know the correct settings? I think its something like (1*2+3*16)?

Dave
« Last Edit: January 19, 2010, 10:33:05 pm by David »
David
(United Kingdom)
Electronics Design Engineer
 

Offline Simon

  • Global Moderator
  • *****
  • Posts: 13920
  • Country: gb
  • Did that just blow up? No? might work after all !!
    • Simon's Electronics
Re: Eagle PCB - Layer Stack Settings
« Reply #1 on: January 19, 2010, 10:28:46 pm »
shouldn't GND and VCC be the outer layers ?
https://www.simonselectronics.co.uk/shop
Varied stock of test instruments and components including EEVblog gear and Wurth Elektronik Books.
Also, if you want to get ripped off: https://www.ebay.co.uk/usr/simons_electronics?_trksid=p2047675.l2559
 

Online EEVblog

  • Administrator
  • *****
  • Posts: 30082
  • Country: au
    • EEVblog
Re: Eagle PCB - Layer Stack Settings
« Reply #2 on: January 19, 2010, 11:53:03 pm »
shouldn't GND and VCC be the outer layers ?

Not usually, no.
GND and VCC on the inner layers is standard practice.
Advantages are you get physical access to the signal layers, far fewer vias (greater reliability, better controlled signal integrity), no crosstalk between signal layers, better power plane signal integrity (no cutouts for components), and greater bulk capacitive coupling between VCC and GND.
External EMC issues are usually moot. Only in special cases would you have no traces and all plane top and bottom.

Dave.
 

Offline David

  • Frequent Contributor
  • **
  • Posts: 264
  • Country: gb
Re: Eagle PCB - Layer Stack Settings
« Reply #3 on: January 20, 2010, 09:48:14 am »
I emailed PCB Cart asking for there default stack-up so thought I'd post it here if anyone else was wondering:

Normal layer stack up: 1.6mm thickness/ four layer?
 
----------------- copper weight
~~~~~~~~~~~ 7628/ prepreg
============= 1.2mm1/1
~~~~~~~~~~~ 7628/ prepreg
----------------- copper weight
 
If I am correct the layer settings should be: (1+2*3+16) where * represents a core layer and + prepreg.

Dave
David
(United Kingdom)
Electronics Design Engineer
 

Offline jahonen

  • Super Contributor
  • ***
  • Posts: 1046
  • Country: fi
Re: Eagle PCB - Layer Stack Settings
« Reply #4 on: January 20, 2010, 02:57:01 pm »
It does not matter for the PCB fabricators how the PCB software is configured (unless you want to send the work file to them), they need only four gerber files for the copper layers plus solder masks top/bottom and optional silkscreens. Rest is pretty irrelevant, although there might be some recommended practices with particular software where the PCB layers should be located internally. For example in PADS, copper layers are always 1 to n, where n is the number of PCB layers. 1 is the top layer and n is the bottom.

Regards,
Janne
 

Offline stewartallen

  • Contributor
  • Posts: 10
  • Country: 00
    • Stew's Spot
Re: Eagle PCB - Layer Stack Settings
« Reply #5 on: February 14, 2010, 09:28:38 am »
I use the following layer settings for 4 layer boards.  This specifies 4 layers with vias drilled though all the layers. ie no blind vias

(1*2+15*16)

If you have a look on the Eagle Help files, under Design Rules->Layers there is a explanation of the syntax with examples for more advanced uses.
« Last Edit: February 14, 2010, 09:37:44 am by stewartallen »
It might be popular but that doesn't mean it's RIGHT
 


Share me

Digg  Facebook  SlashDot  Delicious  Technorati  Twitter  Google  Yahoo
Smf