Bob,
Please see http://www.alchemyresearch.com/bga.jpg http://www.alchemyresearch.com/bga-soldermask.jpg
The via is in the pad as the pictures will show. Make a pad drill a via right through its center. The board layers are glued, then on the bottom side the via holes were coated in soldermask. My understanding is that the holes themselves were filled with some sort of epoxy ressin (after metalization). This hole filling prevents heat from rushing up the via and sucking the solder ball down the via during assembly.
Pad Details,
size 17.72 mils (.45mm) Clearance around pad is 15 mils solder mask 22 mils
vias in pads:
Copper Width 18 mils Drill Diameter 10 mils Clearance width 4.5 mils solder mask 0 mils
Trace Details:
width 4 mils clearance is 5 mils
Between two pads (metal portion) with or without the vias there is 21.4 mils of space
so
edge of pad 4.5 mils empty 4 mil trace 4 mils empty 4 mil trace 4.5 mils empty edge of pad
So far our assembly success (after the board manufacturor made a flat board ;) has been 6 for 6
Steve Meier
Bob Paddock wrote:
On Friday 07 January 2005 01:57 am, Stephen Meier wrote:
I feal like I have to step in here. With a 900 pin BGA (30 rows by 30
columns) at a 1mm (39 mil) pitch. Four signal layers are just bearly
able to route all the signals out from under the bga. That was using via
in pad and squeezing two 4 mil traces between pads/layer.
I know you can not post the design, but could you post the section relevant to the BGA? I'd like to know how to do these large BGA's myself.
Via "via in pad" does that mean each ball falls into a via, or are the balls on non-hole pads?
