AMD provides the diameter of a land pad on the package side. This information is required prior to the start of the board layout so the board pads can be designed to match the component-side land geometry. The typical values of these land pads are shown in the following figure and summarized in the table. For AMD BGA packages, non-solder mask defined (NSMD) pads on the board are suggested to allow a clearance between the land metal (diameter L) and the solder mask opening (diameter M) as shown in the following figure.
|Flip-Chip BGA Packages||1.0 mm Pitch||0.92 mm Pitch||0.80 mm Pitch|
|Design Rule||BGA packages, non-solder mask defined dimensions in mm (mils)|
|Package land pad opening (SMD)||0.53 mm (20.9 mils)||0.53 mm (20.9 mils)||0.40 mm (15.7 mils)|
|Maximum PCB solder land (L) diameter||0.53 mm (20.9 mils)||0.51 mm (20.0 mils)||0.40 mm (15.7 mils)|
|Opening in PCB solder mask (M) diameter||0.63 mm (24.8 mils)||0.61 mm (24.0 mils)||0.50 mm (19.7 mils)|
|Solder ball land pitch (e)||1.00 mm (39.4 mils)||0.92 mm (36.2 mils)||0.80 mm (31.5 mils)|
An example of an NSMD PCB pad solder joint is shown in the following figure. The space between the NSMD pad and the solder mask, as well as the actual signal trace widths, depend on the capability of the PCB vendor. The cost of the PCB is higher when the line width and spaces are smaller.