Double-sided PCBs with SMD components are not new, and placement of these components follows some simple design rules to ensure reliable PCBAs are produced during manufacturing. In very dense boards, you should not be surprised if a board contains multiple BGA package in the same PCBs. In some cases, where many components are placed into a tight area, you might find an advantage in placing overlapping BGAs on both sides of the PCB.
Is there any kind of problem with this, and should overlapping BGAs be used in double sided PCBs? It all depends on the type of component and what supporting passives or peripherals are needed. But most importantly, you can’t overlap any high-density BGAs without first designing an appropriate layer stack.
Double Sided BGAs Require the Right PCB Layer Stack
Placement of BGAs on two sides of a PCB is possible in three possible configurations. Not all BGAs can be placed and assembled in this way due to differences in pad pitch, pin count, and via types required for routing. The three main configurations are:
- Non-overlapping - Can be used with conventional through-hole
- Partially overlapping - Requires blind/buried vias in overlap region, but through-holes allowed elsewhere
- Fully overlapping - Through-holes not allowed in overlap region
Depending on the placement of BGAs on each side of the board, specific via transitions may be required in the stackup so that connections can be routed across the PCB. In the case of fully overlapping BGAs, the presence of through-hole vias would create overlapping via transitions, which would create shorts and would not be allowed. In this case, you would need at least a Type II HDI stackup that uses blind-buried via transitions.
Full overlap involves placement of two BGA packages on opposite sides of the PCB, where the two regions fully overlap in the same region. The BGAs could be of different sizes and pin pitches. In general, the pin region of one package is fully overlapping the pin region of the other package as shown below.
With full overlap, there will almost always need to be blind and buried via stacks, although there could be a conventional buried via (Type II or III). When the pin count on one BGA is high and the pitch is very dense, every layer interconnect (ELIC) will most likely be needed. This is because dense BGA fanout routing for both components will need to terminate on the internal layers.
However, if one of the BGAs is a large digital processor, you may have trouble mounting the bypass capacitors needed to support low PDN impedance. These capacitors are normally mounted on the back side from a BGA package, and if there is another BGA on the back side then there will not be room for the capacitors. Therefore, we need another strategy in the case of large digital components.
Offset or No Overlap
In both of these cases, through-holes may be allowed in the stackup beneath the BGA components. The two BGAs could use through-holes to route in/out of pins as long as the packages are offset far enough from each other. Here the goal is to place the BGAs such that any through-hole connections do not bridge across the BGAs.
In the overlap region, blind/buried vias are needed to prevent collisions between the two components. When there is no overlap, through-holes can be used for fanout as long as the pin pitch is large enough to accommodate the drill diameter and hole-to-hole distance. This means that the no-overlap case could still be done with a traditional stackup (no HDI layers).
Based on the above factors relating to required via types and layer counts, fully overlapping BGAs are possible on double-sided boards, but only certain components are practically useful in these cases. The use of double-sided BGAs is practical when we don’t require direct mounting of passive components (like capacitors) on the back side of the BGA, and therefore it is possible to place another BGA on the back side instead. For larger processors, like high pin count FPGAs, this is not practical and these should not be overlapped with other BGA components.
The other point not mentioned above is related to rework. If two BGAs are overlapping in the same board region, attempting to rework one of the BGAs will likely desolder the other BGA. Therefore, if rework will be needed, you will probably need to totally desolder both BGAs and re-solder both sides with a fixture in reflow or in a rework station. Quality procedures need to be in place to ensure rework will be minimized in higher volume production.
Wherever you plan to place and route BGA components in your PCB, you can easily define the layer stack you need for double sided assembly with the industry-standard PCB design features in OrCAD from Cadence. Only Cadence offers a comprehensive set of circuit, IC, and PCB design tools for any application and any level of complexity.