Issue link: https://iconnect007.uberflip.com/i/431081
December 2014 • The PCB Design Magazine 13 • Long via stubs create impedance mismatches, reflections on single-ended nets. • Large via pads often force diff pairs to be split under BGAs. Recommendations There are a number of tipping points where standard lamination with through vias is not viable: • Once the board is over 28 layers, it becomes difficult to manufacture with acceptable yields and therefore can become cost-prohibitive. • If the board is over 28 layers, the dielectrics can be so thin that delamination can occur under the higher temperatures required for lead-free soldering. • Generally when using a few BGAs with less than 1500 pins and a 1mm pin-pitch, the breakout and routing of these devices is feasible using through vias. However, if you have a large number of these on a single design, then the route density may force the layer count up high enough to limit the effectiveness of this stackup. If you have multiple BGAs with over 1500 pins and 0.8mm pin-pitch (or less) it is likely that through vias will make it very difficult to route these devices. • When the thickness of the board, due to the number of layers, forces the via to be so large that it inhibits routability. Via length to hole diameter should be <10x, or reliability will decline significantly. Pad diameter should be hole size plus 0.01". If the via pad is so large that it prevents diff pairs or multiple single- ended traces from being routed between the BGA via arrays, then more layers will be required to complete the routing. Vias can be shifted off the standard matrix under BGAs; however, with through vias, not much is gained. 2. Sequential Lamination with Blind and Buried Vias Advantages • Potentially shorter via stubs. • Fairly simple via models. • Generally smaller vias than required for through hole vias. Minimum size for mechanically drilled vias are the same as for standard laminate; however, blind and buried vias will likely have a smaller aspect ratio, enabling more use of minimum via hole size, which is 8 th . • Simple dielectrics, primarily FR-4. • Effective use of blind & buried vias opens up routing channels, potential for fewer layers. Disadvantages • Not a widely adopted process; more and more fabricators do HDI instead. • Minimum size for drilled vias is 8 th . • Costs more than through hole laminated, yet minimum trace widths are still the same. • Practical reliability limits the number of sequential laminations to 2 or 3. Recommendations • Sequentially laminated boards have the same tipping points as standard laminates; however, since the via length to hole size aspect ratio will be less and pad sizes can be smaller, routability improves and it is less likely that the design would exceed 28 layers. • Since the feature sizes for traces can vias are still the same as with standard laminate, designing with multiple large BGAs of < 1 mm is very difficult. 3. Buildup with Microvias (HDI) Advantages • Smaller feature sizes for vias and traces en able higher route density and fewer layers. • Effective use of microvia patterns opens up routing channels, potential for fewer layers. • Only practical way to design with multiple large BGAs having <0.8 mm pitch. • Lowest cost for high density boards. • Improved signal and power integrity, with appropriate stackup definition. HDI LAYER STACkUPS FOR LARGE, DENSE PCBS continues feature