RE: BGA Assembly

[Tom Stamp <toms@optiscan.com>]

Holes in BGA pads are ok IF they are small enough - we have three 256 ball
BGA packages mounted on one of our boards. Each BGA pad that requires a via
has a 10 thou (thousandth of an inch) via in the middle of the pad. There is
a very small degree of wicking that occurs, but the paste that is placed on
the pads more than compensates for this. So far we have a 100% hit rate with
this technique.

I am not sure how big the via hole has to be before the wicking away of
solder becomes significant.

Our  BGA's are just placed onto the paste which holds them in place before
they go to the reflow oven.

Hope this is useful.

regards,

Tom Stamp
Optiscan Imaging
Melbourne Australia

> -----Original Message-----
> From:	Rick Collins - Arius [SMTP:PCImail@arius.com]
> Sent:	Saturday, 25 November 2000 6:12
> To:	pci-sig@znyx.com
> Subject:	RE: BGA Assembly
> 
> I have been told that it is a very bad idea to put vias in the pads for
> BGAs. As discussed, the solder is drawn into the hole and there is not
> enough to provide a connection. 
> 
> I think the "limiting feet" are also a bad idea. I had several boards
> manufactured with BGAs and they use normal amounts of paste and flux and
> let the BGA "float" on the molten solder. The BGAs all came out perfectly
> (out of 28). 
> 
> We had another house attempt to assemble our prototypes by hand. They
> first tried using a *lot* of paste. This literally floated the chip off
> the pads. Then they tried using a small amount of glue. This had the same
> problem Dimiter found. The chip can't settle on the pads. 
> 
> So use normal amounts of paste and flux and let the chip float on the
> pads. These things are very easy to assemble in production. You just have
> to have faith that they will work and not try to force the issue. 
> 
> 
> At 01:27 PM 11/24/00, you wrote:
> 
> 
> 
> 	At one time Agilent (then HP) had a high density interconnect method
> for probing with their logic analyzers that required via-in-pad.
> 	
> 	As I recall, the relevant application note recommended applying
> solder paste and reflowing the board twice. 
> 	
> 	On the first pass one applied paste only to the pads that
> incorporated vias.  The amount of solder paste was sufficient to fill each
> via.  Then one reflowed the bare board, with no components.  After that,
> using a different stencil, one applied normal amounts of solder paste for
> the components, placed the components, and reflowed again.
> 	
> 	I never saw discussion of this by third parties, nor do I know what
> kind of yields one might experience using this approach.  Anyone?
> 	
> 	Philip Decker 
> 	
> 	-----Original Message----- 
> 	From: Dimiter Popoff [ <mailto:tgi_earth@yahoo.com>] 
> 	Sent: Friday, 24 November, 2000 9:25 AM 
> 	To: pci-sig@znyx.com 
> 	Subject: Re: BGA Assembly 
> 	
> 	Peter, 
> 	
> 	>I was specifically recommended not to put vias or holes under the
> ball, by 
> 	>someone with past experience of solder being drawn through the hole
> and away 
> 	>from the BGA. I guess this isn't what you wanted to hear - sorry. 
> 	
> 	I guess you just saved a board from an unsuccessful experiment :-). 
> 	
> 	Overall, though, this is no problem, because I don't expect the 
> 	device to go into automatic production quantities soon, and manually
> 
> 	I seem to manage it quite successfully. Moreover, from what I have 
> 	seen so far the solder drawn through the holes is not much (it 
> 	never makes a drop beneath the board, just fills the hole), unless 
> 	there is a big pad at the opposite side to be wetted; and even then 
> 	there is no problem, the connections are quite intact. Actually I 
> 	have hard times imagining what should happen to make the solder 
> 	be drawn away so there is no more a connection between the BGA 
> 	and the board (I guess we all know how do solder drops of this 
> 	size behave), but as I said earlier, I'll take easily avoidable 
> 	risks at a later stage :-) (trying if the BGA will float on 
> 	this without limiting feet, that is). 
> 	
> 	All this is valid for holes drilled with 0.3mm or less; this makes 
> 	about 0.2mm after plating. The holes had anyway to be that tiny 
> 	in order to allow 3 traces between each pair of BGA pads; which, in 
> 	turn, made routing possible on only two signal layers. 
> 	
> 	Thanks, 
> 	Dimiter 
> 
> 
> 
> 
> 
> 
> Arius - A Signal Processing Solutions Company
> Specializing in DSP and FPGA design
> 
> Arius
> 4 King Ave
> Frederick, MD 21701-3110
> 301-682-7772 Voice
> 301-682-7666 FAX
> 
> Internet URL <http://www.arius.com/>
>