Milling: Operations and Tooling
Facing, pocketing, slotting, profiling and drilling, with end mill geometry, coatings, holders and chip load.
Milling operations
Milling removes material with a rotating multi-tooth cutter that moves across the work. Almost every milled part is built from a handful of operations.
| Operation | What it does | Typical tool | Notes |
|---|---|---|---|
| Face milling | Flattens the top of the stock to a known surface | Face mill (inserts) or a large end mill | First operation on rough stock; take 0.3–1 mm; the cutter should be 20–30 % wider than the cut |
| Pocketing | Clears material inside a closed outline | End mill | Rough with adaptive or offset paths, then finish; corners need a smaller tool or a radius |
| Slotting | Cuts a channel as wide as the tool | End mill | Full-width cut: highest load; shallower than other cuts, with chip clearance in mind |
| Profiling (contouring) | Cuts around the outside or inside of a shape | End mill | The path is offset by the tool radius; leave 0.1–0.5 mm for a finishing pass |
| Drilling | Makes round holes | Spot drill, twist drill, reamer, tap | Spot first, peck for depth; see below |
| Thread milling | Cuts a thread by moving a small threaded cutter in a helix | Thread mill | Works in blind holes, any material, no tap breakage |
| Chamfering and deburring | Breaks sharp edges | Chamfer mill or engraver | Always specify: sharp edges cut and chip |
| 3D contouring | Follows a sculpted surface | Ball nose or bull nose end mill | Step-over decides finish; see CAM and Toolpaths |
End mills: parts and types
| Type | Use | Notes |
|---|---|---|
| Flat (square) end mill | Pockets, slots, walls, floors | The general-purpose tool; a sharp corner wears fast |
| Bull-nose (corner radius) | Pockets and walls with a small corner radius | Much stronger corner; leaves a radius at the floor |
| Ball nose | 3D surfaces, fillets, scooped slots | Zero speed at the tip: poor cutting at the very center; tilt the tool or use a larger depth |
| Roughing (corn-cob) end mill | Fast bulk removal of steel and tough metals | Wavy flutes break the chip and cut forces; leaves a rough wall |
| Chamfer mill, engraver | Chamfers, text, V-grooves | Cutting speed depends on the contact diameter, not the nominal one |
| Slot drill / center-cutting mill | Plunging and slotting | Cuts on the end; can plunge straight down |
| Thread mill, dovetail, T-slot cutters | Specialized cuts | Light cuts; the tool is weak at the neck |
Tool materials and coatings
| Material | Strengths | Weaknesses | Use |
|---|---|---|---|
| HSS (high-speed steel) | Tough, cheap, forgiving; can be re-ground | Soft: low cutting speed (about 15–30 m/min in steel) | Hand-fed work, drills, rigid-poor machines, wood and plastic |
| HSS-Co (cobalt) | Holds its hardness hot; for tough metals | More brittle than HSS | Stainless, harder steels on older machines |
| Solid carbide | Hard, stiff, 3–5 × the cutting speed of HSS | Brittle: chips if it vibrates or is struck; costly | Most CNC milling; the default for production |
| Coated carbide | Higher speed and longer life | The wrong coating shortens life | See the coating table |
| PCD (diamond), CBN | Extreme hardness; very long life | Very expensive; PCD cannot cut ferrous metals | Aluminum, graphite, composites (PCD); hardened steel (CBN) |
| Coating | Color | Good for | Avoid |
|---|---|---|---|
| Uncoated, polished | bright | Aluminum, copper, plastics: sharp, smooth, chips do not stick | Steels at speed (wear) |
| TiN | gold | General steel, HSS tools | Hard or hot cutting |
| TiCN | blue-gray | Tough steels, cast iron; abrasion resistant | Dry high-speed cutting |
| TiAlN / AlTiN | violet-black | Steels, stainless, titanium, hardened steel: handles heat | Aluminum: it sticks |
| ZrN, TiB2, DLC | gold / silver / black | Aluminum and non-ferrous: slippery, resists the built-up edge | Steel at speed |
Flutes, helix and geometry
| Choice | Best for | Why |
|---|---|---|
| 1 flute | Plastic, acrylic, wood, foam, thin aluminum | Maximum chip space; the chip leaves in one piece, with less heat |
| 2 flutes | Aluminum, brass, slotting, general purpose | Large chip space; slightly weaker core than 3 or 4 |
| 3 flutes | Aluminum and general use | A good balance for aluminum on most machines |
| 4–6 flutes | Steel, stainless, finishing | Stronger core and smoother finish; chips pack in deep cuts |
| Variable pitch / helix | Any, especially long tools | Uneven tooth spacing breaks up chatter |
| High helix (45°) | Aluminum | Pulls chips out smoothly; thinner cutting edge |
| Standard helix (30°) | General purpose | Strong and versatile |
| Low helix (≤ 20°) or straight | Plastics, brass, thin sheet | Does not pull a thin or soft workpiece upward |
A tool with more flutes can feed faster (the feed rate is n × z × fz), but each flute has less room for chips. In aluminum, where chips are bulky, two or three flutes are usually best.
Tool holders and run-out
- ER collets (ER11, ER16, ER20, ER32, ER40) are the standard for small machines. Each collet grips a range of about 1 mm, so a 6 mm tool belongs in a 6 mm collet, not a 6.5 mm collet squeezed down. Clean the collet and nut, tighten to the specified torque, and never grip a tool by its flutes.
- Solid holders (side-lock, shrink-fit, hydraulic) give the lowest run-out and the stiffest hold for production or fine finishing.
- Run-out is how far the tool tip wobbles as it turns. 0.01 mm of run-out means one flute does more work than the others, which shortens life and leaves a poor finish. Keep it below 0.01–0.02 mm for finishing and for small cutters.
- Tool length offset. The controller must know every tool’s length (see G-code and Programming). Measure it with a probe or a setter for repeatable results.
- Torque the nut, do not hammer it. An under-tightened tool pulls out; an over-tightened nut distorts the collet.
Stick-out and deflection
The part of the tool that sticks out of the holder acts like a cantilever beam. Under a side force F, the tip deflects by δ = F × L3 ÷ (3 × E × I), where L is the stick-out, E the stiffness of the tool material (about 600 GPa for carbide, 210 GPa for steel) and I = π D4 ÷ 64 the second moment of area of the shank.
Worked example: a 6 mm carbide end mill, 50 N side force
- I = π × 64 ÷ 64 = 63.6 mm4; E × I = 600 000 × 63.6 = 38.2 × 106 N·mm².
- With 18 mm stick-out (3 × D): δ = 50 × 18³ ÷ (3 × E × I) = 2.5 µm.
- With 30 mm (5 × D): δ = 11.8 µm, 4.6 times as much.
- The flutes make the cutting part thinner than the shank, so real tools deflect more than this solid-shank figure; the cubic trend is the point. A deflection of 10 µm leaves a tapered wall: the tool is pushed away most at the bottom of a deep wall.
- The rule: hold the tool as short as the job allows, use the largest diameter that fits, and take a finishing pass with light engagement to remove the error.
Chip load, engagement and climb milling
- Climb milling (the cutter rotates with the feed at the cut) starts the chip thick and finishes thin: a better finish and cooler cut. It is the default in CAM for a rigid machine. Conventional milling starts thin, rubs, and ends thick; it can be safer on a machine with backlash or on a hard skin such as scale or casting.
- Axial depth ap is limited by tool length, flute length and rigidity. Typical: up to 1–1.5 × D in aluminum, 0.5–1 × D in steel, less in stainless and titanium; slotting is shallower.
- Radial depth ae (width of cut) of 5–50 % of D for roughing, a few percent for finishing. At low ae the chip becomes thin, so the feed must rise (chip thinning).
chip-thinning factor = D ÷ (2 × √(D × ae − ae2)) (applies when ae is less than D ÷ 2)
Worked example: a 10 mm, 3-flute carbide mill in mild steel
- Cutting speed 100 m/min: n = 1 000 × 100 ÷ (π × 10) = 3 183 rpm. Feed per tooth 0.04 mm gives Vf = 3 183 × 3 × 0.04 = 382 mm/min at half-diameter engagement.
- At a radial depth of only 2 mm (20 % of D) the chip is thinner. The factor is 10 ÷ (2 × √(10 × 2 − 4)) = 1.25, so the feed becomes 382 × 1.25 = 477 mm/min to keep the same chip thickness.
- Deeper axial cuts at the same low width (for example 15 mm deep and 2 mm wide) use the whole flute length, spread the wear and cut faster than a shallow, wide cut. This is the idea behind adaptive toolpaths; see CAM and Toolpaths.
For starting feeds and speeds for your material, see Speeds & Feeds, Machining Metals and Machining Plastics, Wood and Composites.
Drilling, reaming and tapping
- Spot drill first with a short, stiff center or spot drill so that the drill starts in the right place and does not walk. Then drill.
- Twist drills have a point angle of 118° (general) or 135° (self-centering, for steel and stainless). Feed per revolution is about 0.02 × the drill diameter as a start, less for small drills and hard materials.
- Pecking. For holes deeper than about 3–4 × the diameter, drill in steps (pecks) and retract to clear chips and let coolant in. Deep holes (over 5 × D) need peck drilling or a through-coolant drill.
- Reaming finishes a hole to size and roundness: leave 0.1–0.3 mm for the reamer in small holes (up to 10 mm), run at about half the drill’s speed and twice its feed. A reamed hole is typically H7.
- Boring with a boring head or a single-point bar gives precise diameters and position, and corrects the hole’s position, which a drill follows from its start.
- Tapping. Drill the tap-drill size, then tap with a rigid-tapping cycle (the spindle and Z feed are synchronized) or a tension-compression holder. For the drill size see the Tap Drill Size & Thread Pitch Lookup.
- Thread milling avoids a snapped tap in an expensive part, makes several sizes with one cutter, and works in any material.
Worked example: an 8 mm hole in aluminum
- Cutting speed for HSS or coated carbide drill in aluminum: about 60 m/min, so n = 1 000 × 60 ÷ (π × 8) = 2 387 rpm.
- Feed per revolution ≈ 0.02 × 8 = 0.16 mm, so the drill feeds at 2 387 × 0.16 = 382 mm/min.
- A 24 mm deep hole is 3 × D: peck in 8 mm steps, or use a through-coolant drill.
Face mills and special tools
- Face mills carry replaceable carbide inserts on a large body. They remove a large area of material per pass with a low cost per edge, and leave a flat, finished surface. Choose a diameter 20–30 % larger than the width of the cut and keep the cutter’s center off the edge of the work.
- Shell mills, fly cutters do the same job for small machines; a single-point fly cutter gives an excellent finish at a low speed.
- Indexable end mills (round or square inserts) take deep roughing cuts in steel cheaply; each insert has several edges.
- Slitting saws cut narrow slots; dovetail and T-slot cutters cut undercuts after a slot is made.
Tool wear and tool life
| Sign | Cause | Try |
|---|---|---|
| Rising noise or squeal | Dull edge, too little feed, rubbing | Raise the feed per tooth; replace the tool |
| Flank wear (wear land behind the edge) | Normal abrasion; excess speed | A land of about 0.3 mm on carbide is the usual limit; lower the speed |
| Built-up edge | Soft metal welded onto the tool | Higher speed, sharper polished tool, lubricant |
| Chipped edge | Vibration, interrupted cut, run-out, hard spots | Shorten the tool, reduce the load, check run-out |
| Burnt or blue chips | Too much speed or rubbing | Reduce speed, increase feed, add coolant or air |
| Broken tool | Chip jam, excess depth, high feed, collision | Clear chips, reduce depth, check zero and program |
Keep a tool log: tool, material, cutting data and how many minutes it lasted. A tool that fails earlier than usual is a sign that something has changed.
Related
- CNC Machining: the overview of this guide.
- CAM and Toolpaths: strategies, entry moves and step-over.
- Workholding and Fixturing: holding the work against the cutting force.
- Machining Metals and Machining Plastics, Wood and Composites: tools and settings by material.
- Speeds & Feeds.
FAQ
How many flutes should an end mill have?
Two or three for aluminum, plastics and wood (more chip space); four or more for steel and stainless (stronger core, better finish). One flute is best for plastics and thin sheet.
Why is my end mill wearing so quickly?
Common causes are too little feed (rubbing), too high speed, run-out, a long stick-out that makes it vibrate, or the wrong coating for the material. Check the feed per tooth first.
Can I use a carbide end mill on a hobby router?
Yes, and it is usually the best choice, but carbide chips if it vibrates or is plunged. Use small depths, ramp or helix in, and a short stick-out.
What is the difference between an end mill and a drill?
A drill cuts with its tip and is made to cut a hole axially. An end mill has teeth on the side and the end and is made to cut sideways, although some can plunge. Do not use a standard end mill like a drill in steel.
What is “chip thinning”?
When the radial depth of cut is less than half the tool diameter, each tooth removes a thinner chip than the feed per tooth suggests. To keep a proper chip thickness, increase the feed rate by the chip-thinning factor.
References
- Oberg, E. et al., Machinery’s Handbook, 31st ed., Industrial Press: milling cutters, cutting speeds, drilling and reaming.
- Sandvik Coromant, Milling Handbook and Formulas and Definitions.
- Harvey Tool, Technical Guides and Helical Solutions, End Mill Basics (flutes, helix, coatings).
- ISO 3685, Tool-life testing with single-point turning tools (wear criteria, also used for milling).
- Kalpakjian, S. and Schmid, S., Manufacturing Engineering and Technology, Pearson.
Last reviewed: October 2026. Cutting data are starting points: machines, tools and materials differ, so test on scrap and follow the tool maker’s data.