BGA's are killing my project

It's a testing and QC/QA issue.

No. you have to help the board assembler to solve the problem.

Yes, it does. Lead-free requires higher temperature and more expensive solder (silver).

Yes, it should help, together with boundary scans. Are they Jtag scanable?

Zero, they should go back to be oven.

Possibly. It may be a board layout problem, as well. Assuming good layout then yes, the soldering process can be improved.

I'd make sure to get together with the chip vendor to make sure that you (or your layout people) understand the layout requirements and are adhering to them, then I'd start pounding on the board house.

No.

I don't know, but from what I understand about lead-free processes your biggest two hurdles will be getting it tuned right to begin with, and tin whiskers down the road. If your assembly house can't even do it with leaded solder that's not the problem.

No. X-ray inspection just looks down through the joint -- if there's solder there that's not sticking it can be very difficult to tell from a good joint.

It does make a difference, however, so it's not to be ignored.

I stand around with my hands in my pockets laughing at folks who actually have to worry about this stuff, so I don't know. But I _do_ know that we've used them in an environment where a 2% or 5% reject rate for the whole board would be considered "way bad", so you can bet we're seeing much less than that for BGA parts.

If I remember I'll check and let you know this evening.

I think you need to find an assembly house who has some mileage with BGA parts, or you need to see your current assembly house start some serious discussions with your chip vendor. BGA parts have been around for nearly 10 years now, and they're becoming ubiquitous. Any assembly house worth its salt really should know how to do it.

Well, that's for production, right?

Most of the assembly houses that do tiny runs for proto purposes request a 10% overage on special parts (including BGAs) and yield is often not guaranteed. Protos are often hand-assembled.

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.

Cheers

PeteS

Could you explain the difference?

Lead soldering of BGA's has been an almost zero defect process for our vendor. (< 0.1% error)

Switching to no-lead has caused some yield issues early on, but thay seem to have straightend them selves out.

It seems that the No-lead soldering has a lower margin for error. Board must be properly designed, properly plated, and clean.

Paul

The main problem we are having with BGAs are the houses that do not have the technique down yet to mount them correctly. It has been a hell of a problem.

Phil

PS.. The fab houses are having a hell of a problem with the lead free requirements and BGA problems for us have included that issue.

What about finish? I mean, HASL vs flash vs immersion vs whatever?

Also, what about adding solder paste to the pads, or flux?

Inquiring minds want to know...

Hello John,

I don't use BGA if at all possible so I can't recommend an assembler. As others have said the first thing is to look whether your board layout and fab instructions are top notch and ideal for each BGA location.

If they are then my suggestion would be to find an assembly house that has a good track record with BGA. Maybe post in sci.electronic.design, "Recommendations for BGA assemblers" or similar. There are a lot of folks who have to deal with BGA. You could also call the sales guys at the manufacturer of your BGA chip. They know good places and if not they can certainly find out via a few calls to their other clients. After all they have a vested interest in you sticking with their chip and not looking for alternatives.

IME when there is a reliability problem with an assembler and they can't immediately point to QC test results and say "aha!" then chances are it won't get better fast enough.

Oh, and make sure the engineers at the assembly house didn't take the liberty to "improve" your layout. I had that happen a month ago where all my prototypes failed. Every one of them. Turned out they had increased some clearances and inadvertantly split a power plane island into four floating chunks.

I meant at board fab. That's where it happened, not at the assemblers.

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

which shouldn't be a problem, IMO.

And I can hand solder TQFP even at 0,5mm pitch without any problem. And desolder it with little effort and without damaging the board.

Try this with BGAs.

Oliver

In an automated process, things are completely different

Have you ever been in those situations?

Cheers

PeteS

certainly I referred to automated placement when I wrote "which shouldn't be a problem, IMO" - we use an several years "old" Siemens so I can't imagine that "current" equipment is worse.

But I love the possibility to hand solder prototypes or to replace a microcontroller when I zapped it during ESD tests. All I need is a matching funnel (wording?) and hot air to remove the IC and a soldering iron with a hoof shaped tip and a magnifier to solder the new one. Well, some solder wick could be necessary.

Oliver

Hello Oliver,

It's usually called nozzle. As you said, you can buy square nozzles for stations such as Metcal that blow hot air only onto the pin rows. In our systems production it was never a problem to swap a flat pack, even large ones. The techs could do that in minutes. BGAs are a whole 'nother matter, a real pain to get off the board without damage.

thanks, nozzle is the word I didn't remember. We have one with a spring loaded vacuum cup, so the TQFP is lifted automatically as soon as the solder is molten. Really easy to use and not very expensive.

Oliver