Blind, buried or smaller-sized holes can reduce plane voids and insertion loss.

High density interconnect technology can increase design density and reduce overall board size. It can also improve the signal and power integrity of a PCB. Here are two case studies that show how blind vias, buried vias and microvias can be used effectively.

Case 1: Improve power integrity by reducing voids in planes. High-power designs for high-speed digital signals require low impedance PCB power planes for proper operation. Therefore, solid planes for power and ground are always preferred. In many cases the power and ground planes under a BGA component have voids, as a result of through-hole vias. These voids have negative effects on power integrity, such as:

• Increased plane inductance.
• Increased plane resistance (as IR drop from power supplies to BGA pads).
• Decreased plane capacitance.

Figure 1 shows how 8mil through-hole vias under a 0.8mm-pitch BGA have created voids in the three split power planes. The copper webs between the voids are just 3.5 mils wide. By replacing the through-hole vias with blind or microvias, the plane voids can be reduced (Figure 2).

Figure 1. Voids and split power planes under BGA component.

Figure 2. Voids eliminated with HDI technology.

Case 2: Improve signal integrity by eliminating via stubs. At speeds of 5Gbps or 2.5GHz and faster, via stubs begin to have a noticeable impact on the insertion and return loss of a PCB. Through-hole via stubs can be removed mechanically in some applications, but in the case of PTH high-speed connectors, such as backplane connectors, pins cannot be back-drilled. One solution is to use surface-mount high-speed connectors and blind vias (Figure 3).

Figure 3. Through-hole via stub, before and after.

Figure 4 shows two via stubs in both ends of a through-hole via for layer exchange of striplines. Buried vias, then, can be employed to eliminate the stubs.

Figure 4. Through-hole via stub, before and after.

In these cases, the use of blind vias and buried vias completely eliminates the through-hole via stub, improving the signal integrity of the PCB.

These are just two situations where HDI technology enables a layout designer to produce better quality PCBs. With recent advancements in PCB manufacturing capabilities, look for many more case studies to come.

Pi Zhang is a senior design engineer at Nuvation Engineering (nuvation.com), a design firm specializing in electronic design services and product development; This email address is being protected from spambots. You need JavaScript enabled to view it..

With few exceptions, large vias are not ideal for ground pads.

I recently received a question on Twitter, asking: “What is your opinion on the ‘one big plated drill in QFN ground pad’ pattern?”

I answered back in 140 characters or less: “Bad for machine assembly, okay for hand assembly.” That’s definitely a true statement, but it’s worthy of a bit more explanation. Figure 1 shows the side opposite of where the QFNs are mounted. The two big openings in the square gold pads are the big vias (plated drill). This is often done when hand soldering QFNs. First, on the component side, solder the little pins on the outside edge of the QFN. Then turn the board over. Stick your soldering iron and solder into the big opening to solder the pad down.

Generally, there wouldn’t be any reason to do this with machine assembly, as we do here in our plant. The proper thermal approach is to put a number of small capped vias in the pad area. The solder paste layer (AKA stencil layer) in the CAD library needs to be segmented to allow for 50 – 75% paste coverage. Thus, we would never recommend using big vias, like those in Figure 1, for machine assembly.

However, I can envision some situations that might call for this. First, when hand soldering, as I mentioned above. Next, there may be some very specific need to expose a lot of the pad to open air for cooling. This is not the best way to get cooling, but it may work in some special instances. Third, perhaps access is needed to the pad as a test point and there’s not enough room to get access any other way.

None of those three steps would be taken in a production environment, but in a prototype world sometimes things happen differently.

SMT? Or not? Sometimes parts labeled as surface mount aren’t quite ready for prime time. In this case, I’m not referring to components that aren’t up to thermal par. Instead, I’m talking about components that can take the heat, but aren’t set up to be machine assembled.

Surface mount machines need a flat surface to pick on. The machines use small vacuum nozzles that need to seat on that flat spot. Chips, of course, are flat on top, as are most other components. Connectors, however, are often not flat on top. That doesn’t leave any place for the pick-and-place machine to pick.

Generally, manufacturers will place a small tab of Kapton tape or a small snap-in plastic pad on top of the connector, giving the machine a surface to work with (Figure 2). Once the board has been fully assembled, the tape or plastic pad is simply removed.

Every now and then, we’ll see connectors come in without that flat pick-and-place surface (Figure 3). That means the machine can’t place it, so it will have to be placed by hand. If there’s a choice between a part with the tape and one without, pick the one with the tape. No offense intended to all of you humans, but machine assembly is way better than human assembly.

Duane Benson is marketing manager at Screaming Circuits (screamingcircuits.com); This email address is being protected from spambots. You need JavaScript enabled to view it.. His Twitter handle is @pcbassembly.