Land patterns for BGA packages: routing, spacing and soldermask requirements for coarse- and fine-pitch ball grid arrays.

Ball grid array packages are divided into two distinct groups based on contact pitch: coarse-pitch and fine-pitch. The coarse-pitch BGA group includes plastic and ceramic package outlines permitting 1.50, 1.27 and 1.0 mm contact pitch variations. The fine-pitch BGA (FBGA) package category includes the die size (DSBGA) package variation (a package that closely follows the actual die outline). Both FBGA and DSBGA standards permit ball contact pitch variations of 0.80, 0.65, 0.50 and 0.40 mm. The FBGA and DSBGA package evolved to maximize functionality in space-limited applications typical of that needed for handheld electronics. Many of the ICs packaged in the smaller format originally designed for miniature products are being selected for general use due to area-utilization efficiency and electrical performance characteristics. In order to minimize package size and maximize contact density, very few component manufacturers continue to provide BGA packaging with 1.50 mm contact pitch. And, although ball pitches of 0.40 mm and less are permitted in standards, their application may not be practical for conventional surface mount assembly due to difficulty in board level assembly processing.

Land pattern development for BGA packaging must consider a number of physical variables including the nominal diameter of the individual ball contact, ball pitch and the positional accuracy of the ball in relationship to a true position within the component outline. Ball contact pitch plays a large role in determining what ball diameters are selected for specific applications. The ball diameter, on the other hand, will determine the actual land pattern size criteria. The component manufacturers seldom furnish the PCB designer with a specific land pattern for attaching their products but in general recommend that the land pattern of component substrate (where the ball is attached) and the land pattern of the mounting structure (printed board) be as similar in diameter as possible. Component manufacturers have also deter mined that the land pattern or pad on the component should be slightly less than the ball contact diameter to maintain a somewhat spherical shape.

The attachment site or land pattern geometry recommended for BGA devices is typically round with the diameter adjusted to nicer contact pitch and ball size variation. The diameter of the land should be no larger than the diameter of the contact or ball on the package and is 10 to 20% smaller than the nominal diameter specified for the ball contact. The information furnished in TABLE 1 provides data on land patterns and their variation to accommodate six common ball diameters used for BGA packaging. The land pattern spacing (or pitch) on BGA packaged devices are "basic" and therefore, positional tolerances are non-accumulative; however, PCB fabrication tolerances must be considered. Routing channels between ball contact land patterns is progressively restricted as the contact pitch is reduced. Manufacturers of the 0.80 mm contact pitch devices, for example, may adopt any of the three optional ball contact diameter variations. Some suppliers of FBGAs and DSBGAs understand the challenges facing the designer in circuit routing and have maintained a constant 0.30 mm contact diameter to maximize conductor routing channels on the outer surface of the circuit board. However, manufacturers of coarse-pitch BGAs and wider pitch FBGAs may choose one of the larger-diameter ball variations. Because of these optional ball size variations, the designer should always refer to the specific supplier specifications for each package before establishing land pattern diameter.

Implementing the higher I/O BGA packaged ICs will require significant planning for both component placement and conductor routing. Routing channels on outer surface layers of the multilayer PCB will, after all, be restricted by the space reserved between land pattern sites (FIGURE 1). The designer may maximize conductor width and spacing by adding more circuit layers, but when the design demands higher component density the board may be more difficult to manufacture, thereby increasing overall product cost. In order to accommodate higher component density, subsurface layer circuit routing should be considered.

[FIGURE 1 OMITTED]

Soldermask Requirements

Surface mount PCBs, and especially those using fine-pitch BGA devices, require a low profile photoimageable soldermask. Although dry-film soldermask material is available, low profile liquid photoimageable (LPI) soldermask is more economical and commonly specified for surface mount applications. The soldermask's role in controlling solder process defects during assembly is of primary concern and designers should attempt to minimize clearance or air gap around land pattern features. In regard to soldermask for BGAs, most companies are specifying a mask that is clear of the land pattern, but the mask must also cover circuit features between lands to help prevent solder bridging between one land and another. Two methods used for defining the attachment site are:

* Coppe-defined land pattern Land patterns defined by the etched copper. Soldermask clearance should be a minimum of 0.05 to 0.07 nun from the etched copper land (depending on the land pattern size and contact pitch).

* Soldermask defined land pattern. If soldermask-defined patterns are used, adjust land pattern diameter accordingly to ensure mask coverage (a minimum of 0.1 mm diameter greater than the mask opening).

In general, soldermask openings for the FBGA package with a contact pitch between 0.65 and 0.8 mm should be 0.15 mm greater in size than the land pattern feature. This clearance permits a nominal 0.07 mm clearance on all sides of the land as illustrated in FIGURE 2. For FBGA devices furnished with 0.50 mm contact pitch, the land diameter is typically between 0.25 and 0.35 mm. The recommended soldermask clearance specified for this application may be narrowed to 0.05 mm as recommended in TABLE 2.

[FIGURE 2 OMITTED]

The finished ball diameter for the 0.50 mm contact pitch FBGA, for example, typically collapses to 0.35 mm. The land pattern recommended for this application is 0.25 to 0.28 mm, slightly smaller than the ball contact diameter. The smaller diameter land will restrict the degree of further collapsing during assembly. FIGURE 3 compares the recommended soldermask clearance for the 0.65 and 0.80 mm pitch device to the clearance recommended for the 0.50 mm pitch device.

[FIGURE 3 OMITTED]

For additional information refer to IPC-7095, Design and Assembly Process Implementation for BGAs, which describes design and assembly criteria for implementing BGA and FBGA technology.

TABLE 1. Land Size Approximation

NOMINAL BALL            RECOMMENDED LAND      LAND PATTERN
DIAMETER                PATTERN DIAMETER     SIZE VARIATION

0.75 mm                      0.55 mm          0.60-0.50 mm
0.60 mm                      0.45 mm          0.50-0.40 mm
0.50 mm                      0.40 mm          0.45-0.40 mm
0.45 mm                      0.35 mm          0.40-0.35 mm
0.40 mm                      0.30 mm          0.35-0.25 mm
0.30 mm                      0.25 mm          0.30-0.20 mm

TABLE 2. Recommended BGA Land Pattern and
Soldermask Clearance

NOMINAL BALL             LAND PATTERN         SOLDERMASK
DIAMETER                   DIAMETER            DIAMETER

0.70 mm (0.027")         0.65-0.70 mm        0-80-0.85 mm
0.60 mm (0.023")         0.55-0.60 mm        0.70-0.75 mm
0.50 mm (0.019")         0.45-0.50 mm        0.60-0.65inm
0.45 mm (0.018")         0.40-0.45 mm        0.55-0.60 mm
0.40 mm (0.016")         0.35-0.40 mm        0.45-0.50 mm
0.30 mm (0.012")         0.25-0.28 mm        0.35-0.40 mm

Source: IPC-7095

VERN SOLBERG is a senior applications engineer with Tessera Technologies Inc. (tessera.com). He is giving a series of workshops on BGA design and implementation this year. He can be reached at 408-383-3614; [e-mail].