Not every design is practical for every volume.
Not long ago, a customer sent us an 8-layer rigid PCB design for quotation. On the surface, nothing unusual – until we noticed the minimum finished hole size (FHS) was 4 mils. That number might not sound alarming, but in PCB manufacturing, 4 mils is a red flag. Here’s why.
The issue arises when fabricators drill a plated through-hole (PTH) and deposit copper during plating. The remaining diameter after this process becomes the finished hole size. A 4-mil FHS with a tolerance of ±4 mils technically ranges from 0 to 8 mils. That kind of spread becomes nearly impossible to maintain in volume production.
To make a PTH, fabricators start with a larger drill size and plate copper along the walls. The smaller the drill, the shorter its flute length – and the fewer panels manufacturers can drill in a stack. Large-scale factories typically drill 10–20 panels at a time for efficiency, but a tiny drill bit can’t survive that workload, which drives up cost and limits throughput. In practice, the smallest common drill diameters used in offshore volume production sit around 8 mils (0.2 mm). After plating (about 1 mil per side for IPC Class 3), that leaves a finished hole closer to 6 mils.
Designing for 4 mils simply doesn’t align with what’s achievable at scale. Could we force it? Yes, by over-plating, doubling the copper thickness and dramatically slowing the line. But that’s a recipe for higher costs, longer lead times and questionable yield.
Bottom line: A 4-mil finished hole is feasible only in small prototype runs, not in cost-sensitive, high-volume production.
Why do designers specify 4 mils? There are two common reasons:
- A designer arbitrarily picks a small drill size without realizing the manufacturability implications.
- A tight-pitch BGA (0.5mm or below) forces via and pad sizes smaller to make room for routing traces between pads.
It’s the second case we see most often. Picture a dense BGA footprint: solder pads closely packed, leaving almost no real estate for escape routing. Shrinking the via seems like the only option, but mechanically drilling a 4-mil FHS is not manufacturable.
The HDI solution. Instead of forcing smaller through-holes, the solution is high-density interconnect (HDI) design using laser-drilled microvias. Unlike mechanical vias, which extend top to bottom, microvias consist of shallow, conical holes that connect only one or two layers.
By stacking or staggering microvias, designers can “step down” through layers and create routing channels on innerlayers where no pads exist. For example:
- 5mm pitch BGAs often require a 1-step HDI build.
- 4mm pitch BGAs typically need 2–3 HDI steps.
This approach keeps hole sizes within manufacturable limits while still meeting dense routing demands.
Part of the confusion stems from chip vendors. Semiconductor companies may publish evaluation boards showing 4-mil FHS designs. Those demos were manufacturable because only a handful of boards were built, often domestically, without cost constraints.
What’s feasible for five prototypes in a lab doesn’t translate to thousands of boards in offshore, high-volume production. The design rules need to reflect that reality.
Key takeaway. When considering 4-mil finished holes in a PCB design, pause. Building prototypes in a specialized facility is possible, but impractical for volume production. Instead, explore HDI strategies with laser-drilled microvias to achieve density without sacrificing manufacturability or cost.
In PCB design, manufacturability is just as important as functionality. A 4-mil FHS may work on paper, but in the real world, it spells trouble.
Jeffrey Beauchamp is director of technology & engineering at NCAB Group USA (ncabgroup.com); This email address is being protected from spambots. You need JavaScript enabled to view it.. He started his career in the PCB industry in 2003 at PD Circuit, now part of NCAB Group, and works with PCB customers to provide optimal solutions.
