[Date Prev][Date Next][Thread Prev][Thread Next][Date Index][Thread Index]
I have asked Axis this question before, so I hope I can save them the
trouble of having to answer again. we recently made two separate designs
with the following dimensions:
BGA Pad Diameter: 25mils
BGA Pad Soldermask Opening: 30 Mils
Vias Under BGA
Drill Diameter: 6mils
Pad Diameter: 20mils
I think this corresponds roughtly to the dimensions on the DevBoard. Our
vias may be a little smaller.
On the vias under the BGA, make sure you cover at least one side of the via
(either top or bottom) with soldermask, otherwise, there is the small chance
of shorts during the soldering process (if you use a wave solder).
Also, all of this depends on the capabilities of your board manufacturer. In
our case, we were using 6/6 trace and space, and our shop also required at
least +14mils annular ring over the finished drill size on the vias. I think
the DevBoard might be 7/7. As long as you can meet your board house's
manufacturing tolerance specs, then you may be able to use slightly
different numbers for the vias.
A few months ago there was an excellent article in Printed Circuit Design on
laying out BGA designs. Unfortunately, it is not online.
I hope this helps.
J. Patrick Frantz
Center for Multimedia Communication
Department of Elec & Comp Engineering
----- Original Message -----
From: "Simoncc" <firstname.lastname@example.org>
Sent: Tuesday, May 07, 2002 10:00 PM
> Dear all,
> Does anyone know the diameter of holes, including the via holes on the
> BGA pads, on devboard 100LX?