BGA land pattern and assembly issues: while saving plenty in board real estate, BGAs and chip-scale packages carry host of other considerations, from coplanarity to rework reliability.

Designers face a number of issues when working with BGAs: pad layout, cost, manufacturability and reliability of the final product. Assemblers may encounter a number of issues too. In addition, even though fine-pitch BGAs are not standard, they have become popular. Herein are the main issues that designers must be aware of when using BGAs, in particular the effect as pitch decreases from 1.27 mm to 0.4 mm.

BGAs were introduced as a packaging technology counter to peripheral-leaded surface mount components, in order to address space and functionality demands. Peripheral-leaded components such as quad flatpacks (QFPs) are characterized by leads that extended from the perimeter of the component body. These leads provide the electrical requirements and mechanical joints to the PCB. In BGAs, the interconnect location is below (at the base of) the package, in the form of balls (FIGURE 1). These balls are either eutectic tin-lead solder or high-melt solder consisting of 90% lead.

[FIGURE 1 OMITTED]

BGAs typically have ball pitches of 1.27 mm (0.050") and 1.0 mm (0.040"). Development work has resulted in components with ball pitches of less than 1.0 mm (0.040") and as tight as 0.4 mm (0.016"). To achieve this, the size of the packaging body has been reduced nearly to the size of the silicon die it houses. For components with a body-to-die area of 1.2:1, this technology is known as the chipscale packaging or fine-pitch BGA (FBGA). The latest development is the wafer-scale pack age (WS-CSP), a CSP with dies the same size as the package.

Drawbacks to BGA package technology include the inability to inspect all solder joints after assembly and the inability to rework the individual solder joints. Other issues become apparent from the design stage. As components decrease in size, so too does the operating process window. Whereas peripheral-leaded components have been characterized, specifications for BGAs are limited and not entirely standardized as pitches decrease. And for even finer pitches, more limitations become apparent, especially during PCB layout. Above all, designers must ensure that the components will fit and be readily assembled.

Typically, components that provide a specific function are available only in a BGA footprint, leading the designer to employ technologies that are not fully mature. As the size and pitch of BGA components decrease, the cost of the product trends higher, a result of the higher cost of fabrication and assembly technology required to manufacture it. The designer must juggle cost, manufacturability and reliability.

Advanced PCB technology is necessary in order to support the infrastructure for BGAs. Signal traces that were once routed from the perimeter of the component are now routed from below the component to the rest of the PCB. This is not an issue with large bump-to-bump pitches, as there is sufficient space between the rows of balls to route signals. But at smaller pitches, narrower traces are required to route the inner signals between the balls (FIGURE 2).

[FIGURE 2 OMITTED]

The space between the balls of the outermost array quickly becomes crowded. There is a limit to how many traces can be routed in this fashion, because of the minimum line width and spacing determined by electrical requirements and the fabricator's capabilities. Tu address the line and space issue, other designs may be incorporated, including dog-bone vias and via-in-pad design (FIGURE 3 and FIGURE 4). In dog-bone vias, the trace is routed to an interstitial via or hole drilled through the board. The hole is plated and provides access to innerlayers with the trace routed internally, not on the surface. A variation of the dog-bone design is the via-in-pad design. In this technique, a via is drilled from the top layer to the second or, possibly, the third layer and then plated. This method permits routing of the signal directly to innerlayers from the pad. Although this method may seem straightforward, limitations are dictated by fabrication capability, cost and assembly-related issues.

[FIGURES 3&4 OMITTED]

The line and space issues discussed above are problematic because not all fabricators have the capability to build these designs. Positional registration of electrical and non-electrical features becomes critical, including the reliability of the fabrication process. For instance, registration of the soldermask is vital; the soldermask must not encroach the pad. Soldermask registration becomes increasingly difficult to achieve on large PCBs. These requirements ha turn drive up the cost of fabricating the PCB. TABLE 1 outlines issues to consider for these layout options.

Assembly Process

The assembly process may be directly or indirectly impacted by the use of BGAs and the PCB designs required to implement BGAs. Use of advanced PCB technology requires more sophisticated assembly techniques. These may entail process optimization such as designing the solder paste stencil to accommodate solder volume requirements, or upgrading equipment such as placement machines whose vision systems are unable to process BGA balls. Comments on specific aspects of assembly follow; the extent to which a designer can affect these issues are summarized in TABLE 2.

Solder paste printing. The pad on the PCB surface that connects the BGA (or BGA solder pad) decreases in size as finer pitches are used. A typical stencil design for BGAs is approximately a 1:1 ratio of stencil aperture to BGA pad. The stencil apertures decrease as smaller pitches and pads are used. The aspect ratio (width to thickness) or area aspect ratio (area opening to wall area) is an indicator of the ability of the aperture to release the solder paste. For a given stencil thickness there will be a minimum aperture opening (or aspect ratio) below which paste will not be deposited consistently or at all. Hence, stencil design becomes more crucial as BGA pad sizes decrease. Designers should communicate with fabricators and assemblers when designing BGA pads to determine an adequate solution and head off potential pitfalls.

Process yield. At finer BGA pitches optimization of the assembly process becomes critical. Developing a robust assembly process is a greater challenge due to the smaller process window. Yield expectations for BGAs have not been fully characterized due to the limited number of fine-pitch parts in high-volume production. There are more data available for larger BGAs with pitches of 1.0 mm and higher. Data analysis of these components show that optimized assembly processes can yield results as good as, or better than, other leaded SMT parts. It is important to be aware that some placement machines are not capable of placing fine-pitch BGAs consistently, due to the inability of their vision software/equipment to properly recognize the balls, and this would have a direct impact on assembly yield. Within the allowable space, the largest BGA package possible should be chosen to increase the probability of obtaining higher process yields. In addition, bigger solder joints in large packages would have higher solder joint reliability and be easier to inspect.

Coplanarity. Variation in BGA bumps can be large, due to "offspec" packages. This may cause coplanarity issues during assembly: A bump that is considerably smaller than the other balls in the array may not form a proper solder joint, resulting in an open after reflow. This type of defect may be detectable through x-ray but repair requires reworking the whole component. However, there is little a designer can do to mitigate this issue.

Inspection. It is difficult to optimize BGAs for inspection, particularly with the lack of visibility to the inner rows of the BGA array. Available tools permit inspection under the soldered BGA, but the field of view tends to be limited. Transmissive x-ray and x-ray laminography techniques are employed to inspect joints, hut the information gathered from these methods is difficult to interpret and analyze compared to direct inspection. As the size of the component decreases, the difficulty of inspection increases.

Rework. Rework of small BGAs requires machines equipped to remove and replace the defective component consistently. Most rework applications employ hot air methods in which the defective component is heated locally to the melting temperature of the solder, with small BGAs this becomes a challenge due to the shorter distances between components and the small size of the components themselves. Care must be taken to ensure that the affected site is heated evenly while adjacent and mirror-imaged components are not inadvertently compromised. Subsequently, when a new BGA is replaced, care should be taken not to blow it off the PCB during reflow. Designers can support rework by maximizing the space around each component.

Testing. The lack of access to the inner balls of a BGA can prevent full coverage testing of the component. In-circuit-test fixtures used to test the whole assembly can also stress BGA joints, which can lead to early failure.

Handling and Care. The small size of BGAs makes them more vulnerable to damage caused by improper handling prior to and following assembly. Although the joints are robust, they are susceptible to damage. PCB flexing of the assembly during transfer from one operation to another can stress the solder joints. Designers should try to place components away from the edge of the PCB and areas of high strain.

Reliability. BGAs have tended to exhibit lower thermomechanical and mechanical reliability than peripheral-leaded components. Thermomechanical failure is caused mainly by the thermal expansion mismatch between the component and PCB when an assembly temperature increases due to power cycles. Leaded components relieve the thermal mismatch through compliant leads. In a BGA, stresses are absorbed by the bulk solder joints themselves. Bulk solder is comparatively smaller in size than a lead. Therefore, BGA solder joints are not as compliant as joints formed with leads and have lower solder joint reliability. Component

designers add features to the package structure to address the mismatch and increase the reliability of the component. These features have not been standardized within the industry; reliability can vary even for packages of the same size. Before specifying a new package, designers should obtain reliability data from package suppliers.

Also, the mechanical strength of the BGA solder joints is not as robust as their leaded counterparts. BGA joints tend to be susceptible to high strain rates. This issue can be addressed to some extent by choosing a large PCB pad to increase the surface area of the joint. Other methods employ the use of an underfill material to reduce the stress on solder joints. While this can be a successful method the added complexity and cost to the assembly process and inability to rework may not justify usage.

There is no single package available that will be cost-effective and reliable for all applications. Products for consumer, industrial and telecommunications have different requirements. Different working conditions will cause different failure modes. Understanding the inherent failure modes would help the designer make an informed decision.

Other issues to consider include lead-free solders, which have higher melting points.

TABLE 1. Via Design Differences

DESIGN                        DOG-BONE VIA

Typical use                   Components with 0.75
                              mm pitch and above.

Advantage                     Technology already
                              developed for large
                              BGAs of coarse pitch.
                              Mechanical drilling
                              compliant.

Disadvantage                  Via formation dependent
                              on aspect ratio and
                              thickness of the PCB.

Cost                          Moderate. Increases
                              as component size
                              decreases and PCB
                              thickness increases.

Limitations                   Limited by board
                              thickness and
                              interstitial space
                              available between pads.

PCB fabrication yield         Good. Features are robust.

Assembly issues               Rework--solder web between
                              via and pad must be robust.

Solder joint reliability      Good. Technique is mature
                              with known key controls.

DESIGN                        VIA-IN-PAD

Typical use                   Component pitch less
                              than 0.75 mm pitch.
                              HDI applications.

Advantage                     Reduces the number of
                              layers required for
                              interconnect.

Disadvantage                  Laser drilling required.
                              Reliability varies
                              among fabricators.

Cost                          High. Few board
                              fabricators have required
                              technology and capability.

Limitations                   Limited to 1 or 2 layers.

PCB fabrication yield         Fair. Dependent on the
                              accuracy of the laser
                              drilling and plating process.

Assembly issues               Typically increases voiding
                              if profile of the via is
                              too circular.

Solder joint reliability      Fair. Some unknown factors.

TABLE 2. Impact of Design on Assembly

ASSEMBLY ISSUE          DESIGNER'S IMPACT   DESIGNER MITIGATION

Solder paste printing   Direct              Communicate with
                                            fabricators and assemblers
                                            to design appropriate BGA
                                            pad layout.

Process yield           Direct              Select a package with as
                                            large a ball pitch as
                                            possible.

Coplanarity             Limited             Select a package with
                                            largest balls possible.

Inspection              Limited             Select a package with as
                                            high a standoff as
                                            possible.

Rework                  Direct              Communicate with
                                            fabricators specifications.

Test                    Limited             None.

Handling and care       Direct              Move BGAs away from PCB
                                            edge and areas of high
                                            strain.

CHRIS ACHONG is in advanced process development at Celestica (celestica.com). He can be reached at 416-443-7223; [e-mail]. Alex Chen is a development engineer at Celestica. He can be reached at [e-mail].