Blind Vias

DFM  - BLIND AND BURIED VIAS

During a recent discussion with some PCB designer colleagues, the subject of blind and buried vias came up, and before the discussion progressed very far, it became obvious that even experienced designers have conflicting information on the subject, even though the technology of blind and buried vias is more than ten years old.  Many designers who are relatively new in the industry are confused as to what a blind or buried via is.  So, to start at the beginning, a blind via is a copper plated hole, just like a regular via, except that it interconnects only one external layer of the PCB with one or more internal layers, but does not go all the way through the board.  A buried via is a copper plated hole that interconnects one or more internal layers, but does not connect to an external layer, hence the hole is completely internal or buried within the board.

Using blind and buried vias in a PCB design has its advantages and disadvantages.  The advantage, of course is that this technology offers a viable design technique to help meet the density constraints of lines and pads on a typical design without increasing the layer count or board size.  The disadvantage of the technology is that due to the additional operations in manufacturing the board, the cost of a board using blind and/or buried vias is significantly higher than a typical multilayer board with the same number of layers.

Designing a PCB with blind and buried vias is not that much different from using standard vias that go all the way through a board, and most designers with even moderate levels of layout experience will soon get a feel for it.  The designer must be vigilant when it comes to the placement of the vias, perhaps more so than with conventional vias.  Buried vias are easy, because they do not impact any trace or surface mount component on the top or bottom layers of the board.  Remember that they are completely  buried  within the board.  As long as the designer maintains the typical clearances from other pads or traces within the inner layers, they are really no different than conventional vias.  Since they are completely buried, the designer can now place a trace or an SMD pad on the outer layers directly over the buried via, thereby gaining some added space on the outside layers.  The placement of blind vias is not much different.  Again, standard clearance rules apply. It is often tempting to place blind vias under SMD  components to save just that extra bit of space, but this practice is not recommended.  Solder flux has a nasty tendency to become trapped in the blind via hole, and although the flux is not highly corrosive, it can cause corrosion problems with time.  This can cause hard to find and often mysterious failures of electronic equipment long after the assembled board passed all tests, even if the board has never been installed.

As in any other design where design for manufacture ( DFM ) is part of the overall strategy, due consideration must be given to the pad and hole sizes for all vias.  The most common design problem, from a manufacturing standpoint, is insufficient hole to pad ratio, resulting in breakout.  Designers can avoid such problems by using vias with reasonable hole to pad ratios.  For internal layers, a via pad that is 0.016" over the drill size is a good choice, as it provides a good yield in manufacturing.  For external layers, a via pad 0.012" over the drill size is acceptable, although the same via size for both internal and external layers is preferred.
 

Peck Drilling Blind Vias

When using blind vias, one aspect of the design that must be carefully monitored is drill depth.  In other words, from the outside layer of the board, the blind via hole can go only so deep.  In a typical 8 layer board, 62 mil thick, using 35 mil vias with 18 mil hole, the maximum depth of the via hole must no exceed 18 mils.  If the top layer of the board is designated as layer 1, and the bottom is layer 8, then the maximum depth of the blind via from the top is to layer 3, or to layer 6 from the bottom side of the board (assuming that all layers are evenly spaced). In effect what this means is that if layers 4 and 5 are the ground and power planes, you can not use blind vias to access these planes from either top or bottom.  You can change the stack-up or use conventional vias for power and ground.  In either case, it would be prudent to talk to your board vendor and get their advice and avoid a very costly if not an impossible to manufacture board.  Since your board vendor has a good understanding of the true process capabilities, they can and will advise you on the best approach to your design.

Peck drilling, however is a very iffy although cheap way to build a blind via board. The problem is in plating the blind hole barrel. If air is trapped in the hole during the plating process there will be no plating and no connection to the inner layers. Peck drilling obviously will not work with buried vias.
 

Sequential Layer Build

Blind and buried vias are more successfully plated if the connections are built and plated according to the manufacturing specifications and the layer build up. With sequential layering the via hole size is not an issue, or at least no greater an issue than the regular thru hole vias. With this method , layers are drilled, imaged, plated , etched, and laminated several times (depending on the connections to be made) This will add considerable cost to the manufacture of the multi-layer board, and your board vendor should be contacted regarding the layer sequence and spacing. Early consultation with your board vendor could mean the difference between a merely expensive board and a very expensive board.

This article was contributed by Nandor Kerek of Systems 80 Tel: (604)596-2655