Turning, milling and drilling: the three core machining processes

Machining removes metal as chips until the part has the right shape, size and finish. Almost every precise mechanical part, whether a shaft, a bracket or a gearbox housing, passes through at least one of three processes: turning, milling or drilling. They all use a hard, sharp tool, but they differ in what rotates and what moves.

Turning

In turning, the workpiece rotates in a lathe chuck and a single-point tool moves along it. Because the part spins about one axis, turning makes round shapes: shafts, pins, bushes, pulleys and threaded parts.

Lathe operations

• Facing: the tool moves across the end of the bar to make a flat face.
• Straight and taper turning: the tool moves along the bar to reduce its diameter, or at an angle to make a cone.
• Grooving and parting off: a narrow tool plunges in to cut a groove or to cut the finished part off the bar.
• Threading: the tool moves along by exactly one thread pitch per revolution.
• Boring: a tool on a bar enlarges a hole along the axis.
• Knurling: hardened wheels press a diamond or straight pattern into the surface for grip.

The process, step by step

1. Hold the bar in the chuck (or between centres for long shafts) with as little overhang as possible.
2. Face the end and centre-drill it if the part needs support from the tailstock.
3. Rough-turn with a deep cut and a heavy feed to remove most of the material.
4. Finish-turn with a light cut and a fine feed for size and surface finish.
5. Cut grooves, chamfers and threads, then part off.

Advantages and limitations

Turning is fast and accurate for round parts. A CNC lathe holds diameters to about IT7 (around ±0.01 mm on a 25 mm diameter) with a surface finish of Ra 0.8–3.2 µm. It is limited to shapes that are round about one axis. Flats, cross-holes and keyways need milling, although CNC turning centres with driven tools can do both in one setup.

Milling

In milling, the cutter rotates and the workpiece moves under it on the machine table. A milling cutter has several teeth, each taking a small chip as it passes. Milling makes flat faces, steps, slots, pockets and 3D surfaces, so it shapes most prismatic (box-like) parts: brackets, plates, housings and moulds.

Milling operations

• Face milling: a large cutter flattens the top of a part.
• Side (peripheral) milling: the side of the cutter machines a vertical wall.
• Slotting and keyway cutting: the cutter makes a slot its own width.
• Pocketing: an end mill clears an enclosed area to a set depth.
• Contouring and 3D milling: on CNC machines, the cutter follows the CAD surface with a ball-nose end mill.

The process, step by step

1. Clamp the part in a vice or fixture, square to the machine axes.
2. Set the zero point (datum) on the part, usually with an edge finder or probe.
3. Face the top, then rough out the profile and pockets, leaving a small allowance.
4. Finish the walls and floors with a light cut.
5. Turn the part over or reclamp it to reach the other faces, then deburr.

Climb and conventional milling

In climb milling the cutter’s teeth move in the same direction as the feed, so each chip starts thick and ends thin. It gives a better finish and longer tool life, and it is the default on rigid CNC machines. Conventional milling (teeth against the feed) is safer on older manual machines with backlash in the table screws.

Advantages and limitations

Milling is very flexible. With 3-, 4- and 5-axis CNC it can produce almost any shape a CAD model contains, to IT7–IT8 and Ra 0.8–3.2 µm. It is slower than turning for round parts, internal corners always have the radius of the cutter, and deep, narrow pockets are hard to reach.

Drilling

In drilling, the drill rotates and feeds into the work. A twist drill has two cutting edges at its point (usually at 118° for general work) and two helical flutes that carry chips out of the hole. Drilling is the quickest way to make round holes, and most parts have several.

Hole-making operations

• Centre drilling (spotting) gives the drill an accurate start.
• Drilling makes the hole, typically to IT10–IT12 with Ra 3.2–6.3 µm.
• Reaming takes a small cut to bring the hole to an accurate size (around IT7) and a smooth finish, for dowels and bearings.
• Tapping cuts an internal thread. The tap drill size for a coarse metric thread is the nominal diameter minus the pitch, so M10 × 1.5 needs an 8.5 mm drill.
• Counterboring and countersinking recess the hole for socket head and countersunk screws.

The process, step by step

1. Mark or program the hole position and spot it with a centre drill.
2. Drill a pilot hole first for large diameters.
3. Drill to size, pecking (backing out regularly) on deep holes to clear chips.
4. Ream, tap, counterbore or chamfer as the drawing requires.

Advantages and limitations

Drilling is fast and cheap, but the hole is not very accurate in size or position, the drill can wander on curved or angled surfaces, and the bottom of a blind hole has a cone from the drill point. Accurate holes are drilled undersize and then reamed or bored.

Comparison table

Designing parts that are easy to machine

• Use standard sizes: hole diameters that match standard drills and reamers, and threads from the standard series.
• Give internal corners a radius slightly larger than a standard cutter radius, so the cutter doesn’t have to stop and turn in the corner.
• Limit pocket depth to about four times the cutter diameter.
• Add undercuts at shoulders on shafts that need threading or grinding up to the shoulder.
• Keep features on as few faces as possible, so the part needs fewer setups.
• Tolerance only what matters. A fit for a bearing needs a tight tolerance; the outside of a cover usually doesn’t.

Our design for manufacturability guide covers these rules in more detail, and the formulas for speeds, feeds and cycle time are in manufacturing calculations.