Drilling & Hole Making
Holes are the most common machining feature — and the most trouble-prone. A hole drilled in open air is easy; a deep, cross-hole, threaded, or precision hole requires the right sequence of tools and operations. This page walks through the full hole-making process from start to finish.
Why Holes Are Hard
A drill works in a confined space: chips must exit through flutes that are only slightly larger than the chip itself. Coolant can't reach the cutting tip easily. The drill has two cutting edges that may not be perfectly symmetric. All of this means drilling has more failure modes than milling or turning.
The Precision Hole-Making Sequence
A hole that needs ±0.02 mm tolerance or a good surface finish is never drilled in one step. The standard sequence:
1. Spot Drilling (Center Drill)
A spot drill has a short, stiff geometry and a 90° or 142° included angle. Its job is not to drill deep — it creates a conical starting dimple that centers the twist drill that follows. Without it, the drill point can "walk" sideways on a flat surface, especially on angled or curved faces.
Drill wander is the #1 cause of hole position errors. A standard twist drill has a chisel edge that is essentially negative rake — it doesn't cut, it pushes. On a smooth surface, that chisel edge can skate sideways 0.1–0.3 mm before it bites. A spot drill eliminates this completely. Always spot-drill first, especially on angled or curved surfaces.
2. Twist Drilling
The twist drill does the bulk of the work. It has two flutes, two cutting edges, and a chisel edge at the point. Standard drill point angle is 118° for general-purpose drilling; 135° for harder materials and thinner sheets.
Drilling parameters
| Parameter | Typical range (carbide drill) | Notes |
|---|---|---|
| Cutting speed (Vc) | 60–100 m/min steel, 100–200 aluminum | Lower than milling — poor chip evacuation |
| Feed per rev (f) | 0.1–0.25 mm/rev (Ø5–10 mm drill) | Too low = rubbing and work hardening; too high = drill breakage |
| Point angle | 118° general, 135° hard/thin | Softer materials = sharper point |
Worked example — drilling Ø8.5 mm hole in steel: Carbide drill, Vc = 80 m/min, f = 0.15 mm/rev.
RPM = (80 × 1000) / (π × 8.5) = 2,990 RPM.
Feed rate = 0.15 × 2,990 = 449 mm/min.
Calculate: Drilling Parameter Assistant
Deep hole drilling (L/D > 3)
When hole depth exceeds 3× diameter, chips can't escape and the drill burns. Solutions:
- Peck drilling (G83): retract fully every 1–2× diameter to clear chips. Standard peck depth: 1–1.5× D.
- High-pressure coolant (HPC): 70–120 bar coolant through the drill flushes chips out. Essential for deep holes.
- Internal coolant drills: drills with holes through the flutes (often called "gun drills" for very deep holes).
3. Reaming
A reamer finishes the drilled hole to close tolerance and good surface finish. It has many flutes (6–10) and cuts very lightly — only 0.1–0.3 mm stock on diameter. Reaming does not correct hole position or straightness — it only follows the existing hole. If the drilled hole is misaligned, the reamer will follow that misalignment.
| Operation | Tolerance achievable | Surface finish |
|---|---|---|
| Twist drill only | ±0.05–0.10 mm | Ra 3.2–6.3 µm |
| Ream (after drilling) | ±0.01–0.02 mm | Ra 0.8–1.6 µm |
| Bore (after drilling) | ±0.005 mm | Ra 0.4–0.8 µm |
Reaming speed is slow: run at 25–33% of drilling speed. Too fast and the reamer wears quickly; too slow and it rubs, causing work hardening and poor finish. Always use flood coolant when reaming.
4. Boring
Boring uses a single-point boring bar to machine the hole to final size, roundness, and straightness. Unlike reaming (which is a fixed-size tool), boring is done by infeeding the boring bar — you can adjust the diameter by 0.001 mm increments. Boring is used when hole position, straightness, or roundness matters more than just diameter.
Read more: Turning Operations — Boring · Boring-Bar Deflection Check
5. Tapping and Threading
Tapping cuts internal threads. The tap is a threaded tool with flutes that cuts the thread as it feeds in at the exact pitch. Rigid tapping (G84) is standard on modern CNC machines — the spindle synchronizes Z feed with rotation.
| Thread size | Tap drill size | Example |
|---|---|---|
| M3 × 0.5 | 2.5 mm | Small electronics |
| M6 × 1.0 | 5.0 mm | General M6 bolt |
| M8 × 1.25 | 6.8 mm | Common 8 mm bolt |
| M10 × 1.5 | 8.5 mm | Common 10 mm bolt |
Calculate: Tapping Parameter Assistant · Threading Calculator
Counterboring, Countersinking, Spot Facing
| Operation | What it does | Why |
|---|---|---|
| Counterbore | Square, flat-bottomed recess for bolt head | Socket head cap screw seats flush |
| Countersink | Conical recess (usually 90°) | Flat-head screw seats flush |
| Spot face | Shallow flat spot on a rough/cast surface | Give a washer a flat seat |
Bolt circle and hole patterns: when you need to drill multiple holes on a bolt circle or rectangular pattern, use: Bolt Circle Calculator · Hole Pattern Generator