Drilling is a machining process used to produce round holes by rotating a cutting tool and feeding it axially into a workpiece. It is one of the most widely used machining operations and can be carried out on drilling machines, lathes, milling machines and CNC machining centres.
Related hole-making operations include reaming, boring, counterboring, countersinking, spot facing and tapping. The appropriate process depends on the required hole diameter, depth, dimensional accuracy, surface finish and function.
A drilling machine provides rotation and axial feed of the cutting tool while supporting the workpiece. Machine selection depends on the component, hole size, required spindle-speed range, available feed, workpiece size and the required accuracy.
Important considerations when selecting a drilling machine or planning a drilling operation include:
Traditional drilling machines remain widely used for workshop and production operations. Modern CNC machining centres can perform drilling together with milling, boring, reaming, tapping and other operations, allowing several features to be produced in a single workpiece setup.
The fundamental drilling principles remain the same: the drill must be guided accurately, the workpiece must be restrained securely, and the selected cutting conditions must be suitable for the tool, material and hole geometry.
A bench drill is a compact drilling machine normally mounted on a bench. The workpiece is supported on an adjustable table or machine base and should be held securely using an appropriate vice, clamp or fixture.
The spindle provides drill rotation and axial movement. On conventional bench drills, axial feed is commonly controlled manually using a lever, while spindle speed may be changed using belts, gears or variable-speed drive systems depending on the machine.
A pillar or floor-standing drill uses the same basic principles as a bench drill but generally provides a larger and more rigid structure, greater workpiece capacity and increased machine capability.
Depending on the machine and tool size, drills and other tooling may be held using a drill chuck or directly through a standard machine taper. Morse tapers have traditionally been widely used for this purpose.
A radial arm drilling machine allows the drilling head to be positioned relative to a stationary workpiece. This arrangement is particularly useful where a component is too large or inconvenient to move repeatedly beneath a fixed spindle.
The radial arm and drilling head provide adjustment of the spindle position, allowing holes at different positions on a large workpiece to be produced without continually relocating the component.
The twist drill is the most familiar drilling tool. It normally consists of a cylindrical body containing helical flutes, cutting edges at the point and a shank for holding and driving the tool.
Drills are available in many materials and constructions, including high-speed steel, coated high-speed steel, solid carbide and indexable or replaceable-tip designs. Tool selection depends on the workpiece material, hole diameter and depth, machine capability, production requirements and required hole quality.
Straight and taper shanks are both widely used. The appropriate shank and toolholding system depend on drill size, machine spindle and the torque, accuracy and rigidity required.
| Operation | Purpose |
|---|---|
| Drilling | Produces a new hole using a rotating drill. |
| Reaming | Sizes and finishes an existing hole using a multi-edge reamer. |
| Boring | Enlarges or corrects an existing hole using a cutting tool whose path defines the finished diameter. |
| Counterboring | Produces a cylindrical recess, commonly to accommodate a bolt or screw head. |
| Countersinking | Produces a conical recess, commonly for a countersunk fastener or for edge preparation. |
| Spot facing | Machines a local flat seating surface around a hole. |
| Tapping | Produces an internal screw thread in a previously formed hole. |
Cutting speed is the peripheral speed of the drill at its effective cutting diameter and is normally expressed in metres per minute.
For a drill diameter D in millimetres rotating at N revolutions per minute:
Vc = πDN / 1000
where:
The spindle speed required for a selected cutting speed is therefore:
N = 1000Vc / (πD)
Drilling feed is commonly specified as the axial distance advanced by the drill for each spindle revolution, normally in millimetres per revolution (mm/rev).
If the feed per revolution is fn and the spindle speed is N, the axial feed rate is:
Vf = fnN
where:
The appropriate feed per revolution depends on drill diameter and design, workpiece material, hole depth, required hole quality and the rigidity and power of the machining system.
As hole depth increases, chip evacuation and coolant access become more important. Chips which are not removed effectively can be recut or packed into the drill flutes, increasing torque, temperature and the risk of tool damage.
The appropriate strategy depends on the drill design and application. Modern drills may incorporate internal coolant passages and geometries designed specifically for deeper holes. Other drilling operations may require controlled withdrawal or other methods of assisting chip evacuation.
The accuracy of a drilled hole depends on the complete tool and workpiece setup. Excessive spindle, chuck or tool runout can cause uneven loading of the cutting edges and affect hole size, position and tool life.
Long drills are less rigid than short drills of the same diameter and are more susceptible to deflection. The shortest practical tool should therefore normally be used while maintaining the access and hole depth required.
The workpiece should be positively restrained against the forces and torque generated during drilling. The required method depends on the component and operation and may include a machine vice, clamps, fixture or dedicated workholding system.
Before an internal thread is produced with a cutting tap, a suitable tapping hole must first be drilled. The required tapping-drill diameter depends on the thread diameter, pitch, thread form and the required thread engagement.
For ISO metric threads, the familiar engineering approximation:
Tapping drill diameter ≈ nominal thread diameter − pitch
provides a useful first estimate for many standard coarse metric threads. It should not be treated as a substitute for the appropriate specified tapping size where thread engagement, material, tap type or production requirements are important.
The table below retains RoyMech's metric tapping-drill data and provides general-purpose clearance-hole sizes. The clearance-hole series correspond to close, medium and free clearance applications.
| Metric Thread Diameter × Pitch |
Tapping Drill mm |
Clearance Hole Diameter (mm) | ||
|---|---|---|---|---|
| Close | Medium | Free | ||
| M1.6 × 0.35 | 1.2 | 1.7 | 1.8 | 2.0 |
| M2 × 0.4 | 1.6 | 2.2 | 2.4 | 2.6 |
| M2.5 × 0.45 | 2.05 | 2.7 | 2.9 | 3.1 |
| M3 × 0.5 | 2.5 | 3.2 | 3.4 | 3.6 |
| M3.5 × 0.6 | 2.9 | 3.7 | 3.9 | 4.2 |
| M4 × 0.7 | 3.3 | 4.3 | 4.5 | 4.8 |
| M5 × 0.8 | 4.2 | 5.3 | 5.5 | 5.8 |
| M6 × 1.0 | 5.0 | 6.4 | 6.6 | 7.0 |
| M8 × 1.25 | 6.8 | 8.4 | 9.0 | 10.0 |
| M10 × 1.5 | 8.5 | 10.5 | 11.0 | 12.0 |
| M12 × 1.75 | 10.2 | 13.0 | 14.0 | 15.0 |
| M14 × 2.0 | 12.0 | 15.0 | 16.0 | 17.0 |
| M16 × 2.0 | 14.0 | 17.0 | 18.0 | 19.0 |
| M20 × 2.5 | 17.5 | 21.0 | 22.0 | 24.0 |
| M24 × 3.0 | 21.0 | 25.0 | 26.0 | 28.0 |
| M30 × 3.5 | 26.5 | 31.0 | 33.0 | 35.0 |
| M36 × 4.0 | 32.0 | 37.0 | 39.0 | 42.0 |
| M42 × 4.5 | 37.5 | 43.0 | 45.0 | 48.0 |
| M48 × 5.0 | 43.0 | 50.0 | 52.0 | 56.0 |
| M56 × 5.5 | 50.5 | 58.0 | 62.0 | 66.0 |
| M64 × 6.0 | 58.0 | 66.0 | 70.0 | 74.0 |
| M72 × 6.0 | 66.0 | 74.0 | 78.0 | 82.0 |
Clearance-hole reference: ISO 273:1979, Fasteners — Clearance holes for bolts and screws, specifies general-purpose fine, medium and coarse clearance hole series. In the UK this is adopted as BS EN 20273:1992.
Drill performance depends strongly on the cutting-tool material and geometry. High-speed steel remains useful for many applications, while carbide and coated tools can provide substantially different machining capabilities when used under appropriate conditions.
For further information see:
The drilling method should be selected from the requirements of the finished hole rather than simply from its nominal diameter. Important considerations include:
The following external resources were included on the original RoyMech page and provide additional information relating to drilling and cutting tools.