Time to read: 7 min
High-quality hole machining is critical for manufacturing parts with tight tolerances. Holes need to align with precision and accuracy, especially for functional assemblies and engineering fits.
Drilling, boring, and reaming are distinct machining processes used to create or refine holes, each offering different levels of precision and surface finish. However, these terms are often mistakenly used interchangeably, despite their unique functions. This misuse can lead to confusion, poor design choices, and costly manufacturing errors
This article will define each process, compare their unique roles, explain tolerances and tooling requirements, and help engineers determine which is best suited to their application.
What Is Drilling?
Most people have operated a drill for simple tasks around their homes or for repairs, but may not know how drilling works in CNC machining. Drilling is the most basic internal machining operation, used to create an initial cylindrical hole in a solid workpiece. Typically, such a hole is made with a twist drill bit, where the cutting action occurs primarily at the tip. Helical grooves, called “flutes,” form a spiral channel that facilitates the movement of metal or plastic chips up and out of the hole. The figure below shows the main components of a typical twist drill bit.
Drilling utilizes a combination of rotational force and axial feed to drive the drill bit into the material, both of which need to be tailored to the material’s conductivity and hardness. The process begins by aligning the drill at the desired angle to the surface, typically perpendicular for straight holes, although angled drilling is possible depending on the design needs.
Once the bit has penetrated the surface of the workpiece, the bit cuts into the material, forming a cylindrical path as chips are cleared through the flutes. For deeper holes, peck drilling cycles (intermittent withdrawals to clear chips and reduce heat) or through-spindle coolant can help prevent overheating.
Drilling creates the initial hole that can then be refined with boring and/or reaming. It can also be used to make the pilot hole for other operations, such as tapping.
Pro-Tip: The maximum depth of drilling should be 12 times the nearest bit diameter. Check out more tips and tricks for hole depth to diameter ratio in our CNC Machining Design Guide or our CNC Design Ebooks.
What Is Boring?
Boring is a precision machining process used to enlarge an existing hole, improving its alignment and surface finish. This operation is often performed with a single-point cutting tool held in a boring bar, and it offers some pretty exciting benefits (pun intended).
Boring can be performed on both CNC lathes and mills. When using a CNC lathe, the workpiece rotates while the boring bar remains stationary. On a milling machine, the boring head rotates while the workpiece remains fixed.
While drilling initiates a hole, boring improves upon it. Boring allows for better control over hole concentricity, roundness, and location, especially when a CNC boring head or boring bar is used.
What Is Reaming?
Reaming is a hole-finishing operation used to bring a pre-drilled or pre-bored hole to an exact diameter, resulting in an improved surface finish compared to drilling or boring alone. Reaming is performed after drilling or boring, not as a standalone process. Reamers are multi-edged tools that remove minimal material in a single pass.
Unlike boring or drilling, reaming doesn’t correct alignment or location. Instead, it fine-tunes the hole’s diameter and finish. A reamer is rotated and fed into the hole at a slower rate, trimming just 0.1 to 0.3 mm of material per pass.
Drilling vs. Boring vs. Reaming: Comparison Table
To better understand hole machining, it can be helpful to compare drilling, boring, and reaming side by side. Each technique serves a specific role in precision hole-making, and understanding their distinctions in terms of tolerances, surface finish, and use case can streamline decision-making.
| Drilling | Boring | Reaming | |
| Purpose | Removes bulk material quickly. Creates an initial hole. | Enlarges/refines hole. Corrects hole geometry and misalignment while allowing precise control of final diameter. | Ensures precise final size and smooth finish. Does not alter the hole path. |
| Typical Tolerance (diameter) | ±0.1–0.3 mm | ±0.05–0.1 mm | ±0.005–0.02 mm |
| Surface Finish | Fair (~125–250 µin Ra) | Good (~63–125 µin Ra) | Excellent (~16–32 µin Ra) |
| Tooling | Twist drill | Boring bar | Reamer |
Drilling vs. Boring vs. Reaming
In most precision manufacturing processes, drilling is followed by boring to correct alignment or enlarge the hole, and reaming is used last to fine-tune the diameter and finish to exact specs.
An example of a typical high-precision hole workflow might be:
- Drill a pilot hole
- Bore for alignment
- Ream for exact diameter and finish
Engineers must evaluate both functional and economic factors when selecting operations.
Design for Manufacturability (DFM) Considerations for Hole Machining
Some DFM best practices for these machining methods are:
- Tolerance Selection: Overly tight tolerances can drive up costs. Engineers should only specify reaming when the part’s function demands it.
- Stock Allowance: Leave sufficient material during drilling or boring to allow for reaming (~0.1 mm, typically).
- Documentation: Identify reaming operations in engineering drawings to avoid misinterpretation by machine shops.
- Cost Optimization: Minimize the use of reaming where a bored hole would suffice. In low-volume production, consider whether CNC boring can meet tolerance requirements before adding a reaming step.
Tolerances and Surface Finish Considerations
Hole tolerances directly affect functionality and interchangeability in machined parts. While drilling and boring offer acceptable fits for general assemblies, reaming is preferred for high-precision components.
Surface finish also affects friction, wear, and sealing. Reamed holes often meet ISO H7 fits, commonly required for bearings or dowel pins.
Engineers should also consider the impact of burr formation, tool deflection, and material hardness when setting expectations for each process.
Tooling and Setup Requirements
Choosing the right tools and setting them up properly is essential to achieving the required tolerances and surface finishes in hole machining.
Tool Overview
Common twist drills come in a variety of diameters and materials (high-speed steel, cobalt-containing tool steel, carbide-tipped, and solid tungsten carbide). These bits are commonly used in handheld drills, CNC machines, and drill presses.
Boring bars, typically used on mills and lathes, have adjustable cutting heads to refine and enlarge pre-drilled holes. Reamers, by contrast, have straight or helical flutes and fixed diameters, providing the final sizing and smooth finish.
Setup Considerations
Listed below are some critical setup considerations to follow when preparing your CNC machine for drilling, boring, and reaming operations:
- Use a rigid machine setup. Secure the workpiece firmly in a stable fixture and use rigid tooling holders to minimize vibration or deflection during machining. Even small movements can lead to dimensional inaccuracies.
- Match spindle speed and feed rate to the specific material being cut and the operation being performed. For example, aluminum may require higher speeds, while stainless steel demands slower feeds to prevent tool wear.
- Apply coolant or lubrication to reduce heat buildup, improve chip evacuation, and extend tool life, especially during deep-hole drilling and reaming.
- Minimize runout, which refers to the deviation of the tool’s rotation from its ideal axis. Excessive runout causes uneven cutting and poor hole quality. Use precision collets and regularly inspect tool holders to control them.
- Preserve hole tolerance and surface finish by avoiding vibration, deflection, and thermal expansion. All of which can compromise dimensional accuracy and finish quality.
- Use boring bars with vibration-dampening features for deep holes to maintain concentricity and prevent chatter marks.
- Choose reamer geometry based on material: spiral-fluted reamers are better for ductile or soft metals (like aluminum or brass), while straight-fluted reamers are more suitable for harder metals and alloys such as stainless steel and titanium.
- Use pilot holes before boring or reaming to improve tool guidance. Deburr edges to avoid tool snags and ensure smooth entry. Verify tool length offsets and tool wear compensation settings in the CNC program to maintain machining accuracy over long runs.
Common Applications by Industry
Many industries rely on different hole-finishing operations based on functional and tolerance needs. Drilling is used in creating pilot holes for further machining, producing clearance holes, and roughing operations in soft or non-critical materials. It is the starting point for internal machining operations that require additional refinement.
Boring’s typical applications include machining bearing seats or press-fit holes. It ensures tight alignment in assemblies (e.g., for shafts or dowels), large-diameter hole machining, and modifying cast or drilled holes in CNC parts.
Reaming is typically used in producing press-fit holes for pins or shafts and finishing high-precision assemblies. It is also used in producing parts requiring smooth internal surfaces, and for critical assemblies in aerospace, medical, and tooling industries.
The examples below illustrate typical hole-finishing applications by industry:
- Aerospace: Hydraulic system ports, deep-groove ball bearing housings, actuator mounts
- Automotive: Piston bores in engine blocks, valve guides in cylinder heads, differential gear housings
- Industrial Equipment: Mounting holes for precision alignment, bushing seats, fluid coupling ports
- Medical Devices: Surgical jig bores, orthopedic implant cavities, catheter alignment channels
What’s the Best Hole-Making Method for Tight Tolerances?
Understanding the differences between drilling, boring, and reaming is crucial when designing or manufacturing components with tight-tolerance holes. Drilling provides speed and ease; boring adds accuracy; and reaming delivers final precision. Choosing the right process ensures that your part can meet both functional and dimensional requirements.
Engineers, sourcing professionals, and machinists should evaluate material properties, tolerance needs, and budget constraints to determine whether drilling, boring, or reaming, or a combination of those three processes offers the optimal path forward. When in doubt, consult with a trusted manufacturing partner.
Need tight-tolerance holes machined to spec? Fictiv’s CNC machining services offer precision drilling, boring, and reaming, supported by expert guidance and lead times as fast as one day.
Get started today with an instant quote.
