PCB drill size looks simple in CAD: choose a diameter, place a hole, and export the drill file. Manufacturing adds several layers of meaning. Is the number the finished diameter or the drill-tool diameter? Will the hole be plated? How much copper will reduce the opening? What tolerance applies? Does the annular ring remain after layer registration and drilling variation?
These questions affect vias, component leads, press-fit connectors, mounting hardware, tooling pins, slots, and depth-controlled features. This guide explains how a fabricator interprets PCB drill data and how to specify holes that assemble correctly without unnecessary cost.
PCB Hole Types and Their Size Meaning#
| Hole type | Plated? | Main purpose | Critical specification |
|---|---|---|---|
| Through via | Yes | Electrical connection between layers | Finished hole, annular ring, plating |
| Component PTH | Yes | Lead insertion and soldering | Finished hole and lead clearance |
| NPTH mounting hole | No | Mechanical fastener or alignment | Finished diameter and positional tolerance |
| Plated slot | Yes | Blade lead or mechanical/electrical feature | Finished width, length, radius, plating |
| Non-plated slot/cutout | No | Mechanical clearance | Finished geometry and routing tolerance |
| Blind or buried via | Yes | Connection between selected layers | Finished geometry, aspect ratio, stack-up |
Finished Hole Size vs. Drill Tool Size#
The finished hole is the opening the designer expects on the delivered PCB. The production tool size is the drill used before later processes. For a plated hole, the fabricator drills larger because desmear, electroless copper, electrolytic copper, and sometimes the final surface finish reduce the opening.
For a non-plated through hole, there is no copper barrel, so the tool and requested finished diameter are much closer. Mechanical drilling still has tool-size, wear, material, and routing tolerances. The finished hole should therefore be specified with a realistic tolerance rather than assumed to equal the nominal CAD value exactly.
Eurocircuits' published drilled-hole rules illustrate the distinction: its CAM system reads customer tool lists as finished sizes and applies its own production oversize for plated holes. That conversion is a supplier process rule, not a universal value. Do not manually add a generic plating allowance unless the fabricator specifically asks for production tool diameters.
Why Plated Holes Finish Smaller#
A multilayer panel is mechanically or laser drilled after lamination. The holes are cleaned and desmeared, a conductive seed layer is deposited, and copper is plated onto the barrel. Each deposition reduces the open diameter. Copper distribution across the panel can influence local plating thickness, so manufacturers use process controls and a tolerance band rather than promising one exact diameter.
Eurocircuits' current explanation of finished-hole tolerances identifies hole type, available drill increments, drill wear, desmear, plating, copper balance, and final finish as contributors. This is why the fabrication drawing should specify the required finished result and allow the manufacturer to select the production tool.
Common PCB Drill Size Ranges#
There is no single standard drill chart that fits every fabricator, laminate, thickness, and service level. Prototype suppliers may group sizes into preferred increments, while advanced processes support smaller mechanical drills and laser microvias. The following ranges are design-planning examples, not purchase-order tolerances:
| Application | Planning range | Design note |
|---|---|---|
| Mechanical through via | About 0.20–0.40 mm finished | Confirm minimum drill and aspect ratio |
| Small component lead | Lead size plus assembly clearance | Use the component drawing, not a generic value |
| Header pin | Often around 0.9–1.1 mm finished | Square pins need diagonal and tolerance review |
| M2 clearance | Application-dependent clearance above 2 mm | Check screw class, plating, and positional tolerance |
| M3 clearance | Application-dependent clearance above 3 mm | Coordinate with enclosure and washer geometry |
| Tooling/alignment hole | Set by the mating pin | Often needs tighter positional control |
Always use the connector, fastener, or component manufacturer's maximum-material dimensions. A nominal “1 mm pin” may have shape, coating, and tolerance that require more than a 1 mm hole. For wave-soldered through-hole parts, include insertion clearance and solder-fill considerations.
How to Size Component Holes#
Round leads
Start with the maximum lead diameter from the component drawing. Add clearance for component and PCB tolerances, insertion angle, board finish, and assembly method. Too little clearance causes difficult insertion or bent leads; too much can reduce solder fill and mechanical control.
Square and rectangular leads
A square lead's diagonal is larger than its side. Size the finished hole against the maximum diagonal, corner radius, and plating tolerance. Press-fit contacts are a special case: the connector supplier normally defines a narrow finished-hole range, plating system, and qualification process. Do not convert a standard header footprint into a press-fit footprint by tightening the hole alone.
Mounting hardware
Mechanical holes should come from the enclosure tolerance stack. Consider screw diameter, coating, washer, boss, standoff, board positional tolerance, and assembly access. If a metal fastener must be isolated from copper, add a copper keepout on every layer and confirm the required creepage or chassis relationship.
Annular Ring and Drill Size#
The annular ring is the copper remaining around a drilled hole. A pad diameter that looks generous in CAD can become marginal after drill position and layer registration vary. For a simple planning calculation:
Nominal radial annular ring = (pad diameter − finished hole diameter) ÷ 2
This is only the nominal geometric value. The fabricator's minimum finished annular ring or breakout allowance must include drill and registration tolerances. Smaller holes do not automatically solve the problem; they increase aspect ratio and may make plating or assembly more difficult.
Review internal and external lands separately when the stack-up or registration capability differs. For nonfunctional pads, discuss whether the manufacturer may remove them. For high-reliability designs, specify the applicable performance and acceptance requirements rather than relying only on the CAD rule.
Aspect Ratio: Hole Depth Divided by Diameter#
Mechanical via aspect ratio is commonly discussed as board thickness divided by drilled-hole diameter. A thicker board or smaller hole creates a higher aspect ratio and makes uniform plating more difficult. The exact limit depends on the supplier, hole type, material, plating process, and reliability class.
If a design pushes the manufacturer's standard limit, options include increasing the finished via, reducing board thickness, using sequential lamination, replacing a through via with a qualified blind structure, or moving to a more capable fabrication service. Each option affects cost and reliability. Confirm the proposed stack-up before routing is finalized.
Mechanical Drills, Laser Drills and Routing#
Mechanical drilling
Rotating carbide tools create most through holes and larger blind or buried holes. Very small tools wear faster and may require lower hit counts, increasing cost. Designers should reduce unnecessary drill-size variety and use preferred sizes where this does not compromise function.
Laser microvias
Laser drilling creates shallow microvias with geometry different from a conventional mechanically drilled barrel. Diameter, depth, capture pad, target pad, stacking, copper filling, and sequential lamination must be agreed as one HDI process. A laser microvia is not simply a smaller entry in the NC drill table.
Routed slots and cutouts
Slots may be produced by drilling, routing, punching, or another process. The available cutter diameter controls the internal corner radius. State whether the slot is plated, define the finished width and length, and include it in both drill/rout data and the mechanical drawing.
PTH vs. NPTH Data#
Plated and non-plated holes should be unambiguous. Many fabricators prefer separate drill files, while others accept attributes in an intelligent format such as ODB++. If Gerber and Excellon files are used, provide a drill map that labels every tool as PTH or NPTH and identifies slots.
A non-plated mounting hole with copper pads may be interpreted differently from an NPTH with a copper keepout. If chassis grounding, shielding, press-fit, or mechanical isolation matters, show the intended copper relationship on the drawing rather than expecting CAM software to infer it.
Drill File and Fabrication Drawing Checklist#
- Use one controlled unit system and zero-suppression format.
- Provide plated and non-plated identification.
- Specify finished hole sizes unless the manufacturer requests otherwise.
- Call out tolerances only where the function needs them.
- Identify plated and non-plated slots, countersinks, counterbores, and depth-controlled drilling.
- Include a drill table with tool count and finished dimensions.
- State board thickness, stack-up, via structures, copper, and plating requirements.
- Check the drill files against copper, solder mask, outline, and mechanical data in a CAM viewer.
Common PCB Drilling Mistakes#
Using lead nominal instead of maximum
The component may not fit once lead and finished-hole tolerances stack in the wrong direction.
Applying plating allowance twice
If the manufacturer expects finished diameters, manually oversizing the CAD hole can create an opening larger than intended.
Failing to distinguish NPTH
A mounting hole may receive copper plating or lose intended isolation when the data is ambiguous.
Specifying unnecessary tight tolerances
Tight limits increase inspection, tool selection, and process cost. Reserve them for press-fit, alignment, or other functions that truly need them.
Ignoring internal copper clearance
A mechanically safe hole can still violate copper clearance on hidden layers. Apply keepouts and anti-pads throughout the stack-up.
Preparing a Manufacturable Hole Strategy#
Group holes by function: electrical vias, component leads, mounting, tooling, slots, and special features. Set requirements from the mating part or electrical function, then compare them with the manufacturer's preferred sizes, minimum drill, tolerance, annular ring, and aspect-ratio capability. This prevents a global “smallest possible hole” rule from driving unnecessary cost.
Related PCBPit references include PCB via fundamentals, through-hole assembly, mounting-hole design, and counterbore and countersink features. To get a manufacturability review, send the drill files, fabrication drawing, stack-up, and quantity to PCBPit.
Frequently Asked Questions#
Should the drill file contain finished hole sizes?
Many fabricators expect finished dimensions and calculate their own production tool sizes. Confirm the supplier's rule and state the convention on the drawing to prevent double allowance.
Why is a plated hole drilled larger than its final size?
Copper and other process deposits build on the barrel wall and reduce the opening. The fabricator chooses an oversize tool so the finished hole remains within tolerance.
What is the smallest PCB drill size?
There is no universal minimum. It depends on mechanical versus laser drilling, board thickness, material, aspect ratio, plating process, and supplier capability. Use the current design rules for the selected service.
Are mounting holes plated?
They can be PTH or NPTH. Choose based on grounding, mechanical, and isolation requirements, then identify the choice clearly in the data and drawing.
How much larger should a component hole be than its lead?
Use the component's maximum lead envelope and an assembly tolerance analysis. The appropriate clearance depends on lead shape, plating, insertion method, soldering process, and product requirements.