Ball-grid array (BGA) packages come in a variety of pitches and sizes. As device complexity increases and OEMs continue their drive toward smaller components, ball pitches of 0.5 mm and lower are becoming more popular.
Pitch is defined as the space between the center of one BGA ball to the center of the next one. Today, you find 0.4 mm pitch BGAs in virtually every smartphone, and 0.3 mm ultra-fine pitch BGAs are the next generation. Currently, the major transition taking place with a move from 0.5mm to 0.4m, initially in ASICs (application specific integrated circuits) and WLCSPs (wafer level chip scale packages).
The next step is to increase functionality within the same real estate. This is the next generation where 0.3mm pitch has been selected. Early OEM adopters are venturing into this unfamiliar and uncharted territory. Most are unknowingly relying on previous 0.5 mm pitch design guidelines since the IPC(Association of Connecting Electronics Industries ) has not as of this writing set forth design standards for 0.3mm pitch. Unfortunately, these OEMs will soon confront certain particular issues by placing their faith on 0.5mm pitch guidelines.
The most important and difficult aspect of printed circuit board (PCB) designs using fine pitch BGAs is the layout of their “lands” and fan outs. PCB lands are where device balls sit and get soldered to. Fan outs are traces from the device lands to adjacent via. A via is required to distribute the I/Os, powers and grounds from the device to the peripherals and typically there is one via per land, as shown in Figure 1 below.
Design missteps incurred at PCB layout when the designer innocently takes the 0.5mm pitch design route can have adverse effects on board fabrication and assembly. A wide range of issues arises in those areas to include problems associated with stencils, solder paste, and pick and place, among others. In particular, the designer must be aware of the current manufacturing capabilities in addition to the PCB’s electrical requirements.
As the industry makes greater inroads into 0.3mm ultra-fine pitch BGAs, the industry is already pushing current manufacturing capabilities to the limits. In other words, there’s concern focused specifically on fabrication registration tolerances, as well as on the device mounting tolerances of pick and place machines on the assembly floor.
Typical tolerances for both have been +/- 3mils. But recent advances in manufacturing technology and equipment have reduced them to +/-1 mils. Additional equipment is also required for such fine pitches for manufacturing validation and rework. This means 3D X-ray may be necessary for validation, and advanced BGA placement/rework stations are required for rework.
Hence, the layout must not in any way add to the problems to the already difficult tasks of board fabrication and assembly. If land size and solder mask openings are not discussed and finalized with the manufacturing group in the initial stages of the layout, it may be the difference between a working product and one that fails during testing or inhibits intermittent failures in the field.
Consequently, it behooves the PCB designer to show diligence while laying out with fine pitch BGAs and things like type of solder paste used, equipment tolerances, stencil thicknesses and type of under-fill used, should be taken into account.
No Industry Specifications/Design Guidelines
As indicated earlier, the electronics industry hasn’t yet developed the specifications nor the expertise to effectively perform 0.3mm ultra-fine pitch design and layout. This leaves many PCB layout engineers with few options other than to base their 0.3mm ultra-fine pitch on conventional 0.5mm pitch IPC design guidelines and layout rules.
For 0.5mm pitches or greater, using non-solder-mask-defined (NSMD) pads for devices was generally preferred. This allowed for better solder-mask registration and stress relief for the BGA solder joints. Boards that followed these guidelines performed better during stress testing.
In the case of 0.3mm pitch devices, if the same guidelines are used, it can lead to potential failures during manufacturing or in the field.
Use of NSMD requires the pad size to be reduced by as much as 20% of the ball size. The solder-mask is then opened with about the same aperture as the BGA ball, size. Now consider this, ball dimensions of a typical 0.3mm package are around 8 mils.
When we talk about soldering, this is already very small. After a further reduction of the pad size, one ends up with an area that may be too small for a reliable solder joint. Also pads of such a small size don’t have sufficient adhesion to the board and may even peel off. Secondly, since the solder mask is recessed, in this case, it opens the door to the possibility of solder shorts.
A better approach is using a solder-masked-defined (SMD) pad in this case. Not only does this allow a slightly more solder area on the BGA pad, solder shorts are less likely. Moreover, since the mask now encroaches on part of the pad, it allows for better registration as well as providing adhesive protection to the pad from getting peeled. More details on NSMD and SMD are given below.
Routing guidelines for PCBs populated with fine pitch BGAs represent another key area that demands special consideration at layout. The main concerns are BGA land size, solder mask definition, BGA fan-out, and fan-out via features.
There are two main categories of BGAs based on the pitch and solder mask definition. The first one is non-solder masked defined (NSMD) pads, discussed briefly above. This is also known as the “collapsing” category.
As shown in Figure 2 below , NSMD pads have the solder mask opening that is larger than the copper pads. Most chip manufacturers have historically insisted on implementing NSMD since it provides tighter control of copper artwork registration compared to the positional tolerance of the solder masking process.
Moreover, NSMD pad definition may introduce stress concentration points that may result in solder joint cracking under extreme fatigue conditions.
Clickon image to enlarge.
However, using this method of solder mask definition is being debated in the industry for being of any benefit for BGA pitches of less than 0.5mm. In fact, many assembly manufacturers stress that NSMD causes more problems than it solves for finer pitches.
Rules followed for 0.5mm pitches may not work for 0.3mm cases, especially when working at high volumes. Typically, ball sizes of 0.4mm pitches are smaller. Reducing it even further by 15% may cause insufficient solder able area. Secondly, using NSMD in cases of 0.4mm may cause bridging between adjacent pads. Thirdly, since the pad sizes are so small, and there is no solder mask webbing to provide adhesive strength, it may peel off, during reflow, or in the field.
BGA land size is created based on the ball size. Table 1 below shows an extract from IP-7351B “Generic Requirements for Surface Mount Design and Land Pattern Standard” when using NSMD. For NMSD, the pad size is typically reduced by 15% over the BGA diameter.
The other category focuses on SMD pads, also known as the “non-collapsing” category. SMD is used for devices that have 0.5mm or finer pitches. In this case, the land is created larger than the ball size. But the solder mask slightly encroaches over the land and the “exposed” or solder-able pad is slightly reduced, as shown in Figure 3 below.
Clickon image to enlarge.
The benefits of using SMD pads include solder mask protection on any traces routed between the lands (which by the way should never be done with pitches of 0.4mm or less.) Secondly, they help to secure the lands to the pre-impregnated composite (pre-preg) and prevent the joint from getting ripped away during mechanical stresses to the assembly. Table 2 below shows an extract from IP-7351B “Generic Requirements for Surface Mount Design and Land Pattern Standard” when using SMD.
Once the proper type of solder mask definition based on the pitch of the BGA is determined, the next aspect is deciding on the fan out and the via structure. For 0.3mm ultra fine pitch, it is strongly advised to use via-in-pad technology, since there is no room to do a dog-bone type fan out.
Via in pad may still be relatively new to many board designers since a good number of OEMs have yet to venture into ultra fine pitch BGAs and CSPs. In those cases, those designers are still using conventional dog-bone fanouts.
However, once system designers move into ultra fine pitch devices and deploy via in pad, they’ll realize the technology helps reduce parasitic inductance, as well as increase density.
Density increases because the via is directly placed under the device’s contact pads, and at the same time, routing is improved. When the via is placed on the pad, it is filled with an epoxy and plated to give a flat finish. Via hole size should be 3 mils or even less if possible. Laser drills are typically used for these types of vias.
As the industry marches on towards more miniaturization, it is safe to predict a need for more processing power in gadgets like hearing aids and embedded medical devices. Even though phones and tablets may have stabilized in size and the trend is more toward system in chip than it is toward more shrinking, we definitely will be seeing more chips with pitches of 0.3mm and less.
Syed Wasif Ali is an advanced certified designer (CID+) and a layout engineer at NexLogic Technologies, Inc. , San Jose, CA. He received his BSEE from N.E.D. University of Engineering and Technology in Karachi Pakistan.