BeagleBone PCB stackup

[manatarms]

Dear All

Does someone have the stackup of the BeagleBone PCB? I couldn't find
it on the hardware design page and it would help many people who want
to do their own design.

[Gerald Coley]

I will post it for you in the next day or so.

 

Gerald

 

--
To join: http://beagleboard.org/discuss
To unsubscribe from this group, send email to:
beagleboard...@googlegroups.com
Frequently asked questions: http://beagleboard.org/faq

[Gerald Coley]

The layer stackup is already posted. It is included in PCB Files ZIP file. It is in the form of a PDF file, beaglebone_revC1_PDF.zip.

 

http://circuitco.com/support/index.php?title=BeagleBone#Hardware_Files

 

Gerald

[Gerald Coley]

I get a kick out of those "Guidelines". They are just that, guidelines. One of the key functions of a PCB is to control the impedance of a signal, something that is done by a combination of the trace width, length, and the distance to ground, the "air gap". That is the key aspect of the stack-up and it varies from PCB shop to PCB shop depending on their processes and the equipment they use.

These models they mention again, make for a nice document. Yes the BeagleBone layout has good EMC, it did pass FCC part 15 and CE. There was no model used in the design of the BeagleBone. In fact, I have never heard of any PCB guy relying on models to lay out a board. Models do not comprehend things like power planes, cross talk, signal integrity, trace length, impedance, and length matching that are dictated by things like, schematic and mechanical restrictions.

The six layer design was dictated by needing enough layers to make all the connections. Needing the DDR signals to run over  a ground plane and all signals to me matched lengths. USB impedance to meet the USB specification and making sure the signals did not cross over breaks in the power planes so as to pick up noise. LCD signal to be matched lengths so as not to create any skewing of the data. Having enough ground planes to pull the heat off the various devices. Ensuring that the power connections were large enough to connect to all pints and provide proper isolation between the various rails as needed. And making sure it all fit in the constraints of the board size.

I hope I was able to answer your question. One other side note. The board was not autorouted and it was done out by a guy with over 30 years of experience.

Gerald

On Mon, Feb 18, 2013 at 5:38 PM, <alexandr...@i9lab.com> wrote:

Hello,

I need to design a PCB like a Beaglebone, i.e., with sitara soc, including the WL1270 wifi module. The PCB files are a good start point. But, would you have any additional references beyond PCB files?

I am studying the "High-Speed Layout Guidelines" from Texas Instruments. In section "Board Stackup" of this document there are a table with 6 suggestions (models) of possible board stackup on a six-layer PCB comparing each of them in terms of decoupling, EMC and signal integrity. Unfortunately, the stackup solution employed for Beaglebone (signal-gnd-signal-signal-vcc-signal) doesn't use any of those 6 models. This model has a good EMC?

Would anybody know what this model (used in the Beaglebone) was employed? Is it have a good EMC?

My regards,

Alexandre

--
For more options, visit http://beagleboard.org/discuss
---
You received this message because you are subscribed to the Google Groups "BeagleBoard" group.
To unsubscribe from this group and stop receiving emails from it, send an email to beagleboard...@googlegroups.com.
For more options, visit https://groups.google.com/groups/opt_out.
 
 

--

Gerald

 

ger...@beagleboard.org

g-co...@ti.com

http://beagleboard.org/

http://circuitco.com/support/

[AnBer]

Hi Gerald,

Regarding PCB stackup, I loooked at the layer stackup defined in the BBB Altium PCB file.
I can see that:
  - Top and bottom signal layers are 2.4 mil copper
  - Inner layers (signal and power planes) are 1.2 mil copper

How much plating is there on top and bottom layer?
Is 2.4 mils just copper or copper + plating?

I am trying to do some pre-layout sim for a BBB and a cape and I need to model the PCB.

Thanks in advance
Antbert

[Graham]

AnBer:

Normal PCB manufacturing process is to to use 1.2 mil copper
(also known as 1/2 ounce copper) on the inner layers
and a subtractive process (etching) to remove unwanted copper.

Outer layers are originally (the same) 1.2 mil copper then etched to provide the
desired features, then all the through holes for vias
are drilled through the stack, and an additional 1.2 mils of copper plated
on top of the original copper. This as well provides the copper plating inside
the drilled holes to form the via connections between layers.

So, the outer layers are 1.2 mils of rolled, dead soft copper plus another
1.2 mils of hard plated copper for a total of 2.4 mils (also known as 1 Ounce copper.)

--- Graham

==

[John Syn]

From: AnBer <ant.b...@gmail.com>
Reply-To: "beagl...@googlegroups.com" <beagl...@googlegroups.com>
Date: Thursday, November 20, 2014 at 5:56 AM
To: "beagl...@googlegroups.com" <beagl...@googlegroups.com>
Cc: <siebel....@googlemail.com>
Subject: [beagleboard] Re: BeagleBone PCB stackup

Hi Gerald,

Regarding PCB stackup, I loooked at the layer stackup defined in the BBB Altium PCB file.
I can see that:
  - Top and bottom signal layers are 2.4 mil copper
  - Inner layers (signal and power planes) are 1.2 mil copper

How much plating is there on top and bottom layer?
Is 2.4 mils just copper or copper + plating?

I am trying to do some pre-layout sim for a BBB and a cape and I need to model the PCB.

Numbers in Altium refer to the final thickness which is used for impedance calculations. 

Regards,

John

Thanks in advance
Antbert


On Wednesday, February 8, 2012 9:00:30 AM UTC+1, manatarms wrote:

Dear All

Does someone have the stackup of the BeagleBone PCB? I couldn't find
it on the hardware design page and it would help many people who want
to do their own design.

--

For more options, visit http://beagleboard.org/discuss
---
You received this message because you are subscribed to the Google Groups "BeagleBoard" group.
To unsubscribe from this group and stop receiving emails from it, send an email to beagleboard...@googlegroups.com.

For more options, visit https://groups.google.com/d/optout.

[AnBer]

Graham, John,

Thanks for the comments.

I finally found the layer stackup document for the BBB (revB4).
Strangely enough I could not find it in a readable format from:
http://elinux.org/Beagleboard:BeagleBoneBlack#Hardware_Files
I found it at the below page for an older BBB version:
https://github.com/SweedJesus/Beaglebone-Black-Stuff/tree/master/Docs/Beaglebone%20Black/BBB_PCB/BeagleBone_Black_RevB4_MFG

From the beaglebone_black_RevB4_NOLOGO_FAB.pdf enclosed file looking at the different info I can see:
   - TOP and BOTTOM layers are:    1/2 oz + 150 microinches of plating (ie 0.150 mils)
   - INNER layers are:                      1 oz
which seems different from what is defined from the BBB Altium PCB stackup (beaglebone_black_RevB4.pcbDoc):
   - TOP and BOTTOM layers are:     2.4 mils
   - Inner layers are:                         1.2 mils
Using the below convert 1/2 oz should be 0.88 mils and 1 oz 1.37 mils:
http://www.referencedesigner.com/cal/cal_02.php

Am I missing something in the oz to mils conversion?
Even if the Layer stack-up table from the .pdf file says that all dimension are in INCHES it looks like that the that it is oz and mils instead.

In both document the total board height is 62 mils.

AnBer

On Wednesday, February 8, 2012 9:00:30 AM UTC+1, manatarms wrote:

[Graham Haddock]

AnBer:

I realize that it is in writing on the Internet, therefore it must be true.

But, the board as documented by "SweedJesus" is a non-standard

and unusual construction for PC boards, therefore there is a slight
chance that the information is wrong.

I would suggest that you use the dimensions suggested by myself
and John.

Please also realize that the dimensions and parameters in building

PC boards that affect your E&M modeling are typically +/- 10 percent,

sometimes +/- 20 percent, so do not spend a lot of time chasing

decimal places for the input to your modeling program.

--- Graham

==

--

For more options, visit http://beagleboard.org/discuss
---

You received this message because you are subscribed to a topic in the Google Groups "BeagleBoard" group.
To unsubscribe from this topic, visit https://groups.google.com/d/topic/beagleboard/OUpHBFIA1uc/unsubscribe.
To unsubscribe from this group and all its topics, send an email to beagleboard...@googlegroups.com.

[Nick]

Hello gerald/forum

I had a look at BeagleBone_Black_RevB4_FAB.pdf

in there i can see for the 50 ohm impedance signal with a track width of 4.75 on external layers and 5.25 on internal layers

so does that mean power supply lines are also 4.75 track width on external layer and 5.25 on internal layer

Regards

Nick

[Gerald Coley]

Power supply lines? Power supplies are power planes with a connection from the pad to the plane using a via. 

Gerald

--
For more options, visit http://beagleboard.org/discuss
---

You received this message because you are subscribed to the Google Groups "BeagleBoard" group.

To unsubscribe from this group and stop receiving emails from it, send an email to beagleboard...@googlegroups.com.

For more options, visit https://groups.google.com/d/optout.

--

Gerald

 

ger...@beagleboard.org

http://beagleboard.org/

gco...@emprodesign.com

[John Syne]

Power is supplied via power planes which are on layers 2 and 5.

Regards,

John

[John Syne]

I guess I should have scrolled up before answering this post.

Regards,

John