FOM Systems Inc.

Embedded Systems Hardware & Software

Skip
to content

Home

About

Contact

Blog

« Welcome to FOM Systems

RoHS Manual Soldering Hints »

BGA Solder Joint Failure (pad cratering) on RoHS PC

I’ve been working on a new project using the Intel Atom processor and 945GSE
chipset.  In the platform design guide that Intel published they have
various recommendations for routing traces to the corners of BGA PCB footprints
for the parts and I was curious as to why these were being recommended.
It turns out I’ve been fortunate in my past experience with RoHS-based designs
since most of the boards I work on are small, fairly rigid (most are 1.6mm
thick) and the BGA components were few and of fine pitch. However, there is an
ugly failure mode with RoHS process boards and BGA’s which has come to be known
as “pad cratering”. This is a bit of a misnomer, since the “crater” is the
space left vacant when a BGA ball pad lifts off the board.

Causes of pad cratering

Simply put, pad cratering is merely the failure of the resin bond between
the board and the surface ball pads of a BGA footprint.  This has been
exacerbated by RoHS because of the higher reflow temperatures needed
(embrittles the resin) and the greater hardness of RoHS compliant
solders.  There are at least two main causes: mechanical stress due to
thermal cycling of the board during reflow, and stress on the joints caused by
board flexing during handling and other mechanical shocks.  The failures
normally begin at the outside corners of the BGA package and may not be
apparent at first if the connecting traces to the pads don’t immediately
fracture.  The most common electrical failure point is at the perimeter of
the ball pad where a routing trace connects to the pad.

Dealing with pad cratering

Note that this heading does not say “preventing pad cratering” as it appears
that simply attempting to prevent pad cratering will not yield significant
increases in board reliability. The most extreme example I’ve seen in the
attempt to prevent pad cratering  is to apply epoxy to the 4 corners of
each BGA package to provide mechanical stress relief for the corner pads.
For most of us however that’s simply not practical.  What has apparently
been working for me is to break out the corner BGA pads and those of the next
row back on the diagonal with trace widths equal to the diameter of the ball
pads.

PXA270 Corner Ball Pads

In this view the yellow shapes represent pads with a 4mil via-in-pad blind
via connecting to the second layer, purple pads do not have vias. Via-in-pad
was mentioned in one study I read as another possible way to mitigate pad
cratering but that not enough research had been done to determine its
effectiveness. The idea behind the wide traces at the pad is to eliminate
copper trace fracturing at the pad perimeter.  Evidently the dual approach
of using fat traces plus via-in-pad has worked for me as none of the boards on
which I’ve used this approach have yet to experience a failure due to pad
cratering. These boards are only 0.8mm thick and are used in a hand-held
product, unfortunately a prime candidate for pad cratering failure. But so far
so good…

It’s been suggested that for attaching traces to the corner ball pads one
should route away from the pad at a 45 degree angle relative to the pad with a
wide trace for about 1.2mm, then neck down to normal routing width and go off in
the direction of the route. The image below illustrates this:

Using short fat trace stub to mitigate pad
cratering

Another approach to reducing the stress at the pad to trace boundary is to
use solder mask defined pads rather than metal defined pads for the entire
array. Jon Manning (you can find him on Linkedin) suggested using solder mask
defined pads for the first 3 rows in on the diagonal, using the same solder mask
size as pad metal size for the balance of the array, and increasing the pad
metal size in the corners appropriately. Depending on the ball pitch of your
parts and your board layer structure it seems that some combination of these
approaches should work for you to sufficiently mitigate the effects of pad
cratering. Since shock and flexing are a significant contributor to pad
cratering that’s one place the mechanical design group can make
contributions.  We don’t use solder mask defined pads on all ball pads as a
rule since metal defined pads appear to have somewhat highter soldering
reliability and less problems with joint cracking.

Nicholas Vickers, Kyle Rauen, Andrew Ferris and Jianbiao Pan of Cal Poly
State University published a study of BGA soldering reliability. Their research
conclusions can be found here.  Also, thanks to Jon Manning for sharing his
considerable pcb design experience.

-Jeff

This entry was written by admin,
posted on February 11,
2010 at 9:51 AM, filed under PCB Design and tagged avoiding pad cratering, BGA pad cracking, BGA pad cratering, cratering, metal defined, RoHS,
solder
mask defined. Bookmark the permalink. Follow any comments here with the RSS feed for this post. Both
comments and trackbacks are currently closed.

« Welcome to FOM Systems

RoHS Manual Soldering Hints »

comment_form

Search

Pages

Home

About

Contact

Blog

Categories

Case Studies

PCB Design

Uncategorized

Archives

April 2012

November 2011

February
2010

External Links

The Value Engineering Foundation

Value
Engineering Reference Center

RSS Feeds

All posts

All comments

Meta

Log
in

© Copyright 2010 FOM
Systems, Inc.   |   Powered by Wordpress   |   Designed with The Sandbox