Re: BGA's are killing my project

PeteS wrote:
Jim Stewart wrote:

PeteS wrote:

Arlet wrote:

johnspeth@xxxxxxxxx wrote:


My project uses several BGA parts. We're in the second board rev stage
(rev 2). Our board manufacturer doesn't seem to be able to 100%
reliably solder those parts down. It makes SW debugging troublesome
because one never knows if the SW or the part is misbehaving. We've
had 15 boards built and I estimate 20% have BGA problems.





BGA solder problems can also be related to the PCB design. Make sure
your pads have the recommended size and shape. Vias in the pad, or very
near the pad can also cause problems by wicking the solder away from
the pad and into the hole.

A specific piece of board design that will _kill_ you in BGAs is the pad. You really _must_ use non Solder Mask Defined pads if you want high yield (and I define that as 100% - I don't accept failures due to failed soldering).

I once worked at a company that had soldermask defined pads under a pretty large (768 balls) BGA, and the yield was horrendous. Went to non-SMD and the yields went way up.

I would be very surprised, assuming the layout is properly done and the CM has edxperience with BGAs, to _ever_ see a BGA failure rate higher than that for TQFP for soldering issues. BGAs are _easier_ on the process.



Could you explain the difference?


Not sure which difference, so I'll do both :)

A solder mask defined pad is simply that; the pad opening is defined by solder mask, which covers some part of the pad. A non-SMD pad is defined by the pad itself, and no solder mask is in contact with it.

On a solder mask defined pad, there is, by definition, a raised 'lip' through which the solder ball has to flow for soldering, and this can cause no connection at all to high impedance connections (which are really frustrating - the JTAG tests will all pass, but nothing works at speed).

There are some really good app notes on this; I'll see if I have any. I seem to remember app notes from Xilinx, Altera, TI, Intel and Micron at the least.

As to BGAs being easier on the process - on SnPb the solder ball wicking effect actually 'pulls' the BGA onto the pads. The placement accuracy for a BGA is 0.5 pad spacing because of this, which is less accurate than final soldered placement accuracy and very easy to achieve with automated pick'n'place.
Whether this holds true in a non SnPb world has yet to be seen.

For a TQFP, because there are pads on each side, the wicking effect doesn't work this way (the forces apparently cancel) so the placement accuracy has to be the same as the final soldered placement accuracy. For a highspeed part (to minimise impedance offsets) this may be as low as 0.1 pad spacing, which may itself be 0.5mm. That's a very tight tolerance, and very difficult to achieve.

Empirically, I have also had many more problems with cold joints, soldersplash and solder shorts with TQFPs than with BGAs. I've personally designed many dozens of boards with both and I have had very few problems (except the non-SMD issue) with BGAs. Most of my solder problems are with TQFP and QFN (and that's a process issue although the process is harder to get right the first time for those).

Cheers

PeteS

FWIW, the board finish makes a lot of difference. My preferred finish for BGA boards is gold over nickel, and since RoHS that's the finish I use for all boards.

HASL is _not_ suitable for large BGAs (or any BGAs, imo), especially full grid types. Many BGAs have outer rows, and a central area where power and ground connect, and a nice clear zone between them. Full grid devices have no such clear zone (See the FT256 package from Xilinx for an example).

As an interesting note on solder mask defined pads, I worked with one device from IR (IPwr200x, ISTR) where a _solder mask defined pad_ was specified as a requirement. Although that was unusual, I did it that way and never had a failure. The ball spacing on that part was quite wide, however.

Cheers

PeteS
.

Relevant Pages

  • Re: What exactly does this mean? (pcb fab)
    ... If those are just vias, ... A Soldermask pad is a "pad" that is meant to mask out the solder mask(so it ... Is it od why I am puting a solder mask over them them? ...
    (sci.electronics.design)
  • Re: PCB track fault - infuriating one
    ... Number of control inputs (o/p DC fault sense etc) that takes ... :solder pad came away with the molten solder. ... The copper pad had a greyish oxide film over it thus ...
    (sci.electronics.repair)
  • Re: plastic flat-packages with 0.5mm pin spacing (was Cantaloupes)
    ... Put a little dab of paste on the center pad (not too much or you will have ... that happens), place the part, reflow it using hot air, and make sure it's ... solder the pins by hand. ...
    (sci.electronics.design)
  • Re: Choosing Solder Mask Expansion Value
    ... the material of the gap is bare fiberglass. ... prevents solder bridges. ... You don't want soldermask on a pad. ... tolerance has gotten quite good and you can certainly use 1 or 2 mils. ...
    (sci.electronics.design)
  • Re: PCB track fault - infuriating one
    ... :Next time coming across similar fault I will change the 100uF,3 second ... showing under the solder blob, with the cap wire still in place ... :around the pad. ... I will explore the bare copper rail sections a bit more and the saved ...
    (sci.electronics.repair)