What’s the Smallest Via Size Most PCB Fabricators Can Handle?

Are you pushing the density limits on your PCB design? Choosing a via size that's too small can lead to costly manufacturing failures. Let's look at what fabricators can actually deliver reliably.

Most PCB fabricators can reliably produce vias with a mechanical drill size of 0.2 \(\text{mm}\) (about 8 \(\text{mils}\)). Advanced fabricators can push this to 0.15 \(\text{mm}\) (6 \(\text{mils}\)). Anything smaller typically requires more expensive laser-drilled microvias, which are in a different class of manufacturing.

Choosing the right via size isn't just about what's physically possible. It's a critical engineering trade-off between board density, signal integrity, power delivery, and, most importantly, manufacturing cost and reliability. In my nearly 20 years as a hardware engineer, I've seen countless projects get delayed or go over budget because of aggressive via choices that weren't truly necessary. The key is to understand the different thresholds where cost and risk start to climb. We will explore not only the standard choices but also the advanced techniques and trade-offs that separate a good design from a great one.

---

What is a standard, cost-effective via size for a typical PCB?

Struggling to keep your prototype costs down? 😟 Your choice of via size could be the culprit, adding hidden expenses without you realizing it. Let's define the sweet spot for cost and manufacturability.

For maximum cost-effectiveness, the industry standard via uses a 0.3 \(\text{mm}\) (\(\approx\)12 \(\text{mil}\)) drill with a 0.6 \(\text{mm}\) (\(\approx\)24 \(\text{mil}\)) pad. This combination is robust, supported by virtually all manufacturers at their lowest price tier, and offers excellent production yield.

Understanding Cost Tiers for PCB Vias

The 0.3 \(\text{mm}\) drill / 0.6 \(\text{mm}\) pad via is the industry workhorse for a reason. A key factor behind this dimension is the drill-to-copper clearance rule. Most fabricators require a minimum clearance of 0.2 \(\text{mm}\) (8 \(\text{mils}\)) from the edge of a drilled hole to any adjacent copper feature. This clearance rule, more than any other, often dictates your maximum routing density.

Here is a breakdown of how via sizes typically map to cost.

Cost Tier	Drill Size	Pad Size	Relative Cost Index 💰	Use Case
Standard	\(\geq\) 0.3 \(\text{mm}\) (12 \(\text{mil}\))	\(\geq\) 0.6 \(\text{mm}\) (24 \(\text{mil}\))	1x	General purpose, non-dense areas
Advanced	0.2 \(\text{mm}\) (8 \(\text{mil}\))	0.45 \(\text{mm}\) (18 \(\text{mil}\))	1.5x - 2x	Denser routing, some BGA breakouts
Leading-Edge	0.15 \(\text{mm}\) (6 \(\text{mil}\))	0.40 \(\text{mm}\) (16 \(\text{mil}\))	>3x	High-density, fine-pitch components

---

What is the difference between the drill size and the finished hole size for a via?

Have you ever specified a via hole size in your design, only to find the physical hole on the finished board is smaller? This common confusion can cause problems. It’s crucial to understand the manufacturing step that causes this difference.

The drill size is the diameter of the physical bit that creates the hole in the laminate. The finished hole size is the diameter that remains after the hole is plated with copper. The finished hole is always smaller than the initial drill size.

The Role of Copper Plating in Determining Finished Via Size

The reduction in hole size is directly related to the plating thickness, which is influenced by your specified copper weight. For a high-power board with 2\(\text{oz}\) (70\(\mu\text{m}\)) finished copper, the plating in the barrel will be significantly thicker than on a standard 1\(\text{oz}\) (35\(\mu\text{m}\)) board. This means the fabricator needs a larger drill bit to achieve the same finished hole size.

The table below illustrates this critical relationship.

Target Finished Hole	Plating Thickness (1\(\text{oz}\) Cu)	Required Drill (1\(\text{oz}\) Cu)	Plating Thickness (2\(\text{oz}\) Cu)	Required Drill (2\(\text{oz}\) Cu)
0.20 \(\text{mm}\) (8 \(\text{mil}\))	\(\approx\)25 \(\mu\text{m}\)	0.25 \(\text{mm}\)	\(\approx\)50 \(\mu\text{m}\)	0.30 \(\text{mm}\)
0.30 \(\text{mm}\) (12 \(\text{mil}\))	\(\approx\)25 \(\mu\text{m}\)	0.35 \(\text{mm}\)	\(\approx\)50 \(\mu\text{m}\)	0.40 \(\text{mm}\)
0.40 \(\text{mm}\) (16 \(\text{mil}\))	\(\approx\)25 \(\mu\text{m}\)	0.45 \(\text{mm}\)	\(\approx\)50 \(\mu\text{m}\)	0.50 \(\text{mm}\)

---

What is the minimum required annular ring size for a via?

Ever get back a batch of prototype boards where some vias are breaking out of their copper pads? 😱 This is called a "tangency" or "breakout" and it can create an open circuit. It’s caused by an insufficient annular ring.

The absolute minimum annular ring for a standard commercial product (IPC-A-600 Class 2) is 0.05 \(\text{mm}\) (\(\approx\)2 \(\text{mils}\)). However, to ensure good yield and reliability, I strongly recommend designing with a minimum annular ring of 0.127 \(\text{mm}\) (5 \(\text{mils}\)) whenever possible.

Why the Annular Ring is Your Manufacturing Safety Margin

The annular ring is your guard band against misregistration during PCB fabrication. Its size is calculated as:
\(\text{Annular Ring} = \frac{(\text{Pad Diameter} - \text{Finished Hole Diameter})}{2}\)
The IPC defines specific requirements based on the product's intended reliability, which are crucial to understand.

IPC Class	Description	Annular Ring Requirement	Allowed Breakout Condition
Class 1	General Electronic Products	Not explicitly defined; relies on minimum land.	90\(^\circ\) breakout is permitted.
Class 2	Dedicated Service Electronics	0.05 \(\text{mm}\) (2 \(\text{mil}\)) minimum (internal & external).	90\(^\circ\) breakout is permitted, but undesirable.
Class 3	High Reliability / Aerospace	0.05 \(\text{mm}\) (2 \(\text{mil}\)) minimum, with no breakout allowed on internal layers.	Not permitted.

For any design pushing the limits, I enable teardrops¹ in my EDA tool. This adds a copper fillet where a trace joins a pad, reinforcing the connection and providing cheap insurance against breakout.

---

What is the aspect ratio of a PCB via and why does it matter?

Have you ever designed a thick board with very small vias, only to be told by the fabricator that it's not manufacturable? The problem is likely the via's aspect ratio. This is a critical constraint that limits how small your vias can be.

The aspect ratio is the ratio of the PCB's total thickness to the via's drill diameter. Most fabricators can reliably achieve an 8:1 aspect ratio using standard processes. Advanced fabricators might offer 10:1 or 12:1, but at a significantly higher cost and risk.

Via Aspect Ratio: A Critical Manufacturing Limit

Achieving uniform plating in a deep, narrow hole is a major chemical challenge. To overcome this, fabs use advanced plating technologies.

PCB Thickness	Smallest Drill Size	Resulting Aspect Ratio	Risk Level	Plating Technology Recommendation
1.6 \(\text{mm}\)	0.20 \(\text{mm}\)	8:1	Standard ✅	Standard DC Plating
1.6 \(\text{mm}\)	0.16 \(\text{mm}\)	10:1	Advanced ⚠️	Pulse Plating2
2.4 \(\text{mm}\)	0.30 \(\text{mm}\)	8:1	Standard ✅	Standard DC Plating
2.4 \(\text{mm}\)	0.24 \(\text{mm}\)	10:1	Advanced ⚠️	Pulse Plating
2.4 \(\text{mm}\)	0.20 \(\text{mm}\)	12:1	Leading-Edge 🚨	Advanced Pulse / Via-Fill Required

Pulse plating uses a complex electrical waveform to deposit copper more evenly in deep holes, enabling reliable manufacturing at higher aspect ratios.

---

How does via size affect PCB manufacturing cost?

You've finished a dense layout using tiny 0.15 \(\text{mm}\) vias, and the prototype quote comes back 3x higher than expected. What happened? 💸 The via size itself is a primary driver of PCB fabrication cost.

Cost rises sharply when you use a drill size smaller than 0.2 \(\text{mm}\) (8 \(\text{mils}\)). Smaller vias require more expensive, fragile drill bits, slower machine speeds, and more complex plating processes. These factors combine to increase both the time and risk of manufacturing.

Key Cost Drivers for Manufacturing PCB Vias

The total cost impact is a combination of several factors, some of which are not obvious.

Cost Driver	Why it Increases Cost with Smaller Vias	Impact
Tooling (Drill Bits)3	Smaller bits are more expensive and have a shorter lifespan.	Moderate
Machine Time	Slower 'peck drilling' is required to prevent breakage.	High
Plating Process	Higher aspect ratios require advanced, slower plating chemistry.	High
Panel Yield	Higher probability of defects (breakout, bad plating) per panel.	High
Multiple Drill Cycles	Designs with many unique hole sizes require more machine setups.	Moderate

A classic DFM strategy is to minimize the number of unique drill sizes used in your design to reduce the number of machine setups.

---

What is a microvia and when should it be used instead of a standard via?

You're trying to route a 0.5 \(\text{mm}\) pitch BGA, but there's no way to get a trace out from the inner balls. Standard vias are simply too large. This is the exact problem that microvias were invented to solve. 💡

A microvia is a laser-drilled via, typically 0.1 \(\text{mm}\) (4 \(\text{mils}\)) or smaller, that connects only adjacent layers (blind via) or an outer layer to the one just below it. You must use microvias for High-Density Interconnect (HDI) designs, especially for breaking out of fine-pitch BGAs (0.5 \(\text{mm}\) pitch or less).

Microvias: The Solution for High-Density Interconnect (HDI) PCBs

HDI technology is formally classified by the IPC-2226⁴ standard based on the complexity of the board's layer build-up. Understanding this helps you communicate your needs clearly to a fabricator.

IPC-2226 Type	Structure Description	Complexity / Cost 💰
Type I	1 layer of microvias on a simple laminate core.	Low
Type II	1 layer of microvias on a core that also contains buried mechanical vias.	Medium
Type III	2+ layers of microvias on a core (enables stacked vias).	High
Any Layer HDI	A core-less build-up made entirely of HDI layers.	Very High

For most BGA breakouts, a Type I or Type II structure is sufficient.

---

What are the limitations of mechanical drilling versus laser drilling for vias?

You know you need to create holes in your board, but should they be drilled with a bit or a laser? Choosing the wrong method can either limit your design's density or massively inflate its cost. Understanding their core differences is key.

Mechanical drilling is the workhorse for cost-effective through-holes, with a practical lower limit of \(\approx\)0.15 \(\text{mm}\) (6 \(\text{mils}\)). Laser drilling is a premium process for creating much smaller vias (\(<\)0.15 \(\text{mm}\)) for HDI boards, but it's more expensive.

Mechanical vs. Laser Drilling⁵: Choosing the Right Tool for Vias

The two technologies are optimized for completely different tasks.

Feature	Mechanical Drilling ⚙️	Laser Drilling ⚡
Smallest Hole Size	\(\approx\)0.15 \(\text{mm}\) (6 \(\text{mils}\))	\(\approx\)0.025 \(\text{mm}\) (1 \(\text{mil}\)), typically 0.1 \(\text{mm}\)
Via Type	Primarily Through-Holes	Primarily Blind Vias (one layer deep)
Aspect Ratio Limit	Plating-limited (\(<\)12:1)	Focus-limited (\(\approx\)1:1)
Special Process	Enables Back-drilling to remove stubs	Enables Via-in-Pad6 Plated Over (VIPPO)
Cost	Low	High
Primary Application	Standard PCBs, Power Boards	HDI, BGA Breakout, Miniaturization

Often, a dual-laser process (CO₂ for bulk removal, UV for cleaning) is used to create the highest quality microvias.

---

How should the appropriate via size be selected for a PCB design?

You're starting a new layout and it's time to set up your design rules. Picking a via size can feel arbitrary, but making a thoughtful choice now will save you countless headaches during routing and manufacturing.

Always start with a standard, cost-effective via like a 0.3 \(\text{mm}\) drill / 0.6 \(\text{mm}\) pad as your default. Only deviate from this standard when a specific design constraint—such as BGA breakout, high-current needs, or routing density—absolutely forces you to use a smaller or larger size.

A Practical 5-Step Process for Selecting Via Sizes

This "Via Selection Cheat Sheet" summarizes the process I follow for every design.

Design Consideration	Recommended Via Type	Key Parameter to Define	Rule of Thumb / Best Practice
General Routing	Standard Through-Hole	Drill/Pad Size	Start with 0.3\(\text{mm}\) / 0.6\(\text{mm}\). It's cheap and reliable.
Fine-Pitch SMT/BGA	Smaller Through-Hole	Drill/Pad Size	Use 0.2\(\text{mm}\) / 0.45\(\text{mm}\) only where routing space is tight.
High Current (\(>\)1\(\text{A}\))	Power Via(s)	Finished Hole Diameter	Use IPC-21527 calculator. Use multiple vias for \(>\)2\(\text{A}\).
Thermal Dissipation	Thermal Via Array	Via Quantity & Placement	Place an array of 0.3\(\text{mm}\) vias directly under the thermal pad.
High-Speed Signals	Impedance-Controlled Via	Antipod Diameter	Model with a field solver. Add ground return vias nearby.

Following a structured approach like this ensures that every via on your board is fit for its specific purpose, balancing performance, density, and cost.

---

Conclusion

Choosing the right via is a core engineering decision. Always start with a robust, low-cost standard via and only shrink it when density forces your hand, always staying aware of your fabricator's capabilities.

---