PCB Design Perfection Starts in the CAD Library – Part 11
There is a reasonable solution for via fanout and a routing solution for the 0.5 mm pitch BGA but we need to think outside the box. The board thickness is an important factor because it affects the hole plating aspect ratio. If you use a 1 mm PCB thickness and want to achieve a 7:1 aspect ratio (this is common among all manufacturers) then the smallest hole size is 0.15 mm (6 mil). There are manufacturer’s that can hard drill a 0.15 mm (6 mil) hole through a 1 mm PCB. There are manufacturers that claim they can easily handle 10:1 aspect ratios. This means that they can drill 0.15 mm (6 mil) holes through 1.57 mm (0.062”) thick PCB material and plate the hole without problems. Drilling all the way through the PCB is important because sequential lamination is an expensive process.
For all via-in-land technology, a thermal relief on the voltage and ground plane connections must be used to prevent cold solder joints. A direct via-in-land connection to the plane will dissipate the heat required to melt the solder around the BGA ball and this will result in a cold or cracked solder joint. The exception to this rule is if the via only contacts a single plane with ½ OZ. copper or less.
If traces are routed between pins of the 0.5 pitch BGA land, the solder mask must be a 1:1 scale to create a “solder mask defined” BGA land. In this way, the traces between the lands will be protected from exposure and possible short circuiting.
The 0.5 mm pitch BGA via-in-land drill hole through the PCB is leading edge technology. When laser drills are capable of producing 0.125 hole sizes entirely through the board and PCB manufacturers can accurately fill the holes with conductive metal epoxy, this technology will become mainstream.
Micro-via technology is the mainstream solution for 0.5 pitch BGA components when a 0.1 – 0.15 laser hole is drilled one, two or three layers deep. This involves sequential lamination but before we get to that subject let’s discuss the via fanout process. Using via-in-land technology, we must offset the drill holes to create adequate routing channels. This is the only routing solution that I know of to maintain manufacturability. See Figure 1 for a via fanout solution for the outer layer. Notice that you will have to add additional copper land for via annular ring.
See Figure 2 for a via fanout solution for the inner layers. The most important feature here is the 0.1 mm (4 mil) trace width & 0.1 mm space between Trace to Via and Via to Via.
Depending on how many rows and columns in the BGA will determine the number of routing layers required.
Sequential lamination process requires the inner layers to be laminated, drilled and plated in Phase 1 and then add 2 additional outer layers and back through lamination, drill and plate in Phase 2. Then add 2 additional outer layers and back through lamination, drill and plate in Phase 3. See Figure 3 for the various phases of sequential lamination.
Let me try to explain why sequential lamination is so expensive and why most people avoid it unless they absolutely need it for high volume production. The PCB inner layer manufacturing goes through the entire fabrication process in Phase 1. Then the first HDI layers that are added to the PCB have to go through the entire fabrication process over again. This basically doubles the cost in Phase 2. Then the second HDI layers that are added to the PCB have to go through the entire fabrication process over again. This basically triples the cost in Phase 3 and the manufacturer’s say that they are basically building the same PC board 3 times.
There are 2 methods of via drilling for sequential lamination. Staggered vias and stacked vias. See Figure 4 for the staggered micro-via process.
Notice in the Staggered Micro-via picture that the via plugging color is green. This could be an epoxy fill because the vias are staggered and there is no manufacturing stress. Discuss staggered vs: stacked vias with your manufacturer to find out if one technique is less expensive than the other. See Figure 5 for the stacked micro-via process.
The Stacked Micro-vias must be filled with conductive metal to prevent the outer laser drill from damaging the inner layer hole. See Figure 6.
The latest generation technology developed by Dow Electronic Materials for advanced via fill plating, MICROFILL™ EVF Via Fill provides enhanced via filling, with simultaneous through-hole plating, at surface thicknesses unattainable. Formulated to operate in existing equipment over a broad range of operating conditions, MICROFILL™ EVF Copper Via Fill is suitable for HDI applications. It is proved by sufficient experience that MICROFILL™ EVF could help to reduce 20% plating thickness and helps to improve varied plating defects. See Figure 7 for stacked micro-via conductive fill techniques. To read more on this topic see: http://www.rohmhaas.com/wcm/information/em/interconnect/microfill/index.page
Notice the lower right image in Figure 7 that shows a 0.15 mm via hole going all the way through a 1 mm thick PCB with 20um (0.000787”) or ½ OZ. copper plating thickness. The normal hole plating thickness on an average PCB is 25um (0.001″) or 1 mil.
Posted January 21st, 2011, by
- PCB Design Perfection Starts in the CAD Library – Part 19
- PCB Design Perfection Starts in the CAD Library – Part 18
- PCB Design Perfection Starts in the CAD Library – Part 17
- PCB Design Perfection Starts in the CAD Library – Part 16
- PCB Design Perfection Starts in the CAD Library – Part 15 QFN
- Inch to Metric Conversion Tables for PCB design
- Do you use Imperial or Metric units for PCB design?
- PCB Design Perfection Starts in the CAD Library – Part 13
- PCB Design Perfection Starts in the CAD Library – Part 12
- PCB Design Perfection Starts in the CAD Library – Part 11