PoP-based PCBs move to center stage
Package-on-package (PoP) technology is coming on strong and continues to overshadow the ever popular system-on-chip (SoC) and other similar packaging types. The rationale behind PoP is simple. More OEMs are miniaturizing their products, but are intent on adding more functionality. Hence, the only way to go to meet these challenges is to make the printed circuit board (PCB) smaller and stack packages on top of each other.
PoP-populated PCBs are expected to continue gaining popularity in three stages over time as shown in the chart. Today, most designs are at the first stage with two-level ball grid array (BGA) PoThe logic or microprocessor (µP) chip is the bottom BGA packaged chip while the BGA packaged memory chip is on top.
Designing PoP-populated boards is certainly challenging. But when BGA packaging moves from 0.5-mm pitch to ultra-fine 0.4-mm and 0.3-mm pitch, you’re adding in a major dimension to the design. That means major design flaws can be introduced when 0.5-mm pitch design guidelines are inadvertently used for 0.4/0.3-mm pitch BGA/PoP-based PCB designs.
When designing with BGAs and pitch sizes of 0.5 mm and earlier ones, there are certain rules of thumb associated with pad sizes and the solder mask opening. One is to keep pad size to about 85 percent of a BGA’s ball size. Another is to use a non-solder mask defined (NSMD) pad. In this case, the solder mask is larger than the BGA pad. Typically, the solder mask is opened to a diameter of about the ball size of the BGA. The recessed solder mask provides stress relief to the NSMD pad during reflow. In short, it creates a protective barrier and lets solder go around it.
It’s also important to note that published design guidelines for 0.4-mm pitch PoP-based PCBs do not exist as of this writing. Instead, you come across conflicting reports relating mostly to PCB pad sizes and solder mask openings. One classic example is the use of NSMD pad sizes for a 0.4-mm pitch BGA PCB design. At times it may be seen that the results at low volume are highly favorable.
But when it comes to high-volume production runs, there is a high probability of low yields. Instead, for 0.4-mm and below pitch BGA PCB designs, the savvy designer opts for solder mask defined (SMD) pads. In this case, the solder mask opening is smaller than the pad size, thus better yields and results are achieved.
There are three major considerations the designer needs to take into account when dealing with 0.4-mm pitch and below. One is the fact ball sizes of 0.4-mm pitch BGAs are smaller than those of 0.5-mm and earlier pitch BGAs. Reducing the pad size even further by 15 percent may cause an insufficient solderable area on the BGA pads. This will cause the boards to be rejected at assembly inspection, or worse, may cause intermittent failures in the field. Second, it is highly probable that bridging can be created between pads when using NSMD pads for 0.4-mm and 0.3-mm pitch BGA/PoPs Bridging results because there isn’t enough solder mask webbing between pads. Third, since pad sizes are so small, and there is no solder mask webbing to provide adhesive strength, the pad may peel off, during reflow, or in the field. Figure 1 shows the differences between SMD and NSMD pads.
SMD is therefore the choice for 0.4-mm pitch BGA/PoP. The SMD pad is created the same size as the BGA ball. The solder mask opening is around 15 percent less than the ball diameter. In this instance, the solder mask laps over the edge of the copper pad to strengthen the connection in two ways. One, it strengthens the bonding between the copper and the PCB’s laminate; two, with the copper pad going further into the solder mask, copper area is larger. That larger copper area provides a greater surface for the PCB laminate to adhere, making the connection twice as strong.
Other design considerations
Aside from BGA/PoP pitch issues, the designer must also keep high reliability and signal integrity at the top of his or her consideration list. High reliability starts at the trace level for BGA-based PoP board design. Ideally it is best to have no trace between two BGA pads and because having them introduces shorts at pitches of 0.4 and smaller on external layers. On internal layers, there should be just one trace between the pads. Also, PCB fabrication problems surface when running multiple and thin 2- to 3-mil traces between two BGA pads. Other issues come about if the length of those thin traces is exceedingly long, and those types of traces are spread throughout the board. There is a greater chance of over etch, thereby eliminating these traces.
Ideal traces are about 5 mils and highly acceptable as good manufacturing practice. But the reality is 5-mil traces may not be practical or possible. In the small PCB world requiring PoP, high reliability and excellent signal integrity demand that a single trace be no more than 2.5 to 3 mils between BGA pads.
Blind vias, solid ground planes, and decoupling capacitors are three other design factors to consider. Compared to buried vias, blind vias are more acceptable because they are easier to work with at manufacturing. However, they pose difficulties since they require one further lamination cycle at the PCB fabrication stage. As far as solid ground planes, it’s important to use them as much as possible. Doing so, ultra-clean noise suppression is maintained and signal-to-noise ratio (SNR) is kept under control.
Regarding decoupling capacitors, the basic principle of locating them as close as possible to BGA balls is as critical as ever. It is even more important for PoP for high signal integrity and particularly so if high-speed switching is involved. Assurances must be made to have the decoupling capacitor distance between the capacitor and the BGA ball as short as possible in order to reduce parasitic inductances.
Depending upon the switching frequencies along with a number of other factors, typically one decoupling capacitor can support up to three BGA pins. It’s important to ensure there are sufficient decoupling capacitors so all BGA pins are properly decoupled. If enough decoupling capacitors aren’t available, the probability increases of getting a signal considerably noisier and more out of control than expected.
In summary, 0.4 mm pitch BGA PoP-based PCB design is in its infancy. Therefore, it is a good idea for the seasoned PCB designer to perform preliminary experimental layouts and prototype rounds to get the lay of the design before launching into a full-fledged layout. This means the PCB designer must be on top of his/her game, and certainly not be complacent after successfully completing many 0.5mm pitch and above BGA/PoP-based designs.