PCB Design Perfection Starts in the CAD Library – Part 11

0.5 mm Pitch BGA Routing Solution

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.

Figure 1 – 0.5 mm Pitch BGA Via-in-Land

Figure 1 – 0.5 mm Pitch BGA Offset Via-in-Land

The vias are 0.05 mm offset from the land center and grouped together.

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.

Figure 2 – 0.5 mm Pitch BGA fanout Inner Layers

Figure 2 – 0.5 mm Pitch BGA fanout Inner Layers




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.

Figure 3 - Sequential Lamination

Figure 3 - 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.

Figure 4 – Staggered Micro-vias

Figure 4 – Staggered Micro-vias

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.

Figure 5 – Stacked Micro-vias

Figure 5 – Stacked Micro-vias

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.

Figure 6 – Stacked Micro-via Conductive Fill

Figure 6 – Stacked Micro-via Conductive Fill

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

Figure 7 – Stacked Micro-via Conductive Fill

Figure 7 – Stacked Micro-via Conductive Fill

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.

Post Author

Posted January 21st, 2011, by

Post Tags

, ,

Post Comments


About Tom Hausherr's Blog

New component package technology and CAD library standards. Tom Hausherr's Blog

@MentorPCB tweets

  • HyperLynx can tackle challenges for any type of high-speed digital #PCB, all in a single, unified environment. https://t.co/oERzYVGCmP
  • Ensure the performance of your AMS circuits by exploring and simulating mixed-signal circuitry… https://t.co/0SvDgpjrDH
  • In this first of two blogs on component libraries, we examine tools and techniques to address two common challenges… https://t.co/8WkmFdPKHd

Follow MentorPCB


2 comments on this post | ↓ Add Your Own

Commented on August 18, 2011 at 8:27 pm
By Imam Kasim

i am working in now high end microvia designing using mentor pads 2000. i require latest updation on pcb designing.

Commented on February 24, 2012 at 10:21 pm
By Albin

Sketch-up is very easy to use but it lacks the tools for a pdoruction CAD. I’ve tried it about a year ago but I cannot use it for mold design it lacks 2D drawing capability. It’s very good for presentation though.

Add Your Comment