ENGINEERING REFERENCE CHART

End Mill Size Chart

This end mill size chart is a single-page reference covering standard end mill dimensions in both imperial (1/32 inch to 1 inch) and metric (0.5 mm to 20 mm), plus all 11 end mill types, 8 coating options, flute count selection, and a material compatibility matrix that tells you which coating works with which workpiece.

View Size Chart Get Instant Quote

✓

Imperial & Metric Sizes

✓

11 Types & 8 Coatings

✓

Material Compatibility Matrix

Imperial 1/32″ – 1″

Metric 0.5 – 20 mm

Types Square, ball, radius

Coatings AlTiN, TiN, DLC & more

Material compatibility & selection

AlTiN · TiCN · DLC · ZrN

TOOLING REFERENCE

What Is an End Mill Size Chart?

An end mill size chart is an engineering reference table that lists the standard dimensions of end mills: cutting diameter, shank diameter, flute length, and overall length. Every CNC machinist, CAM programmer, and manufacturing engineer uses one — whether it is a laminated card next to the tool crib, a table in Machinery’s Handbook, or a browser tab open to a reference like this one.

End mill dimensions follow two standards: imperial sizes defined by inch fractions per ANSI B94.19, and metric sizes defined by millimeter diameters per ISO 1641. Most CNC machines can run either, but the drawing determines the tooling standard, and mixing them produces dimensionally wrong parts.

Imperial Sizes

Standard end mill diameters range from 1/32 inch to 1 inch, defined by inch fractions per ANSI B94.19. Common sizes include 1/8″, 1/4″, 3/8″, 1/2″, and 3/4″ — the standard tooling for most North American machine shops.

Metric Sizes

Metric end mills range from 0.5 mm to 20 mm in diameter per ISO 1641. Standard increments include 1 mm, 2 mm, 3 mm, 4 mm, 6 mm, 8 mm, 10 mm, 12 mm, 16 mm, and 20 mm — the global standard for tooling in Europe and Asia.

Key Dimensions

Every end mill size chart lists four dimensions: cutting diameter (the working size), shank diameter (tool holder fit), flute length (depth of cut capacity), and overall length (tool stickout). Matching all four is critical for proper tool setup.

TOOLING REFERENCE DATA

End Mill Types Chart — All 11 Types Compared

An end mill types chart helps you match the tool geometry to the operation. No single end mill does everything well. The end mill selection guide below explains when to use each type.

The corner radius end mill is the single most underrated tool in CNC machining. Adding a 0.5 mm or 0.020 inch radius to an otherwise square end mill increases corner strength 3 to 5 times with no penalty other than the need to specify that radius in your CAM toolpath. For any production job in steel, stainless, or titanium, the default should be a corner radius tool — reserve square end mills for features that genuinely require a sharp 90-degree corner.

Type	Geometry	Best Applications	Typical Flutes	Surface Finish	Edge Strength
Square (Flat)	Flat bottom, sharp 90° corners	Slotting, pocketing, profiling, shoulders	2–6	Good	Baseline
Ball Nose	Hemispherical full-radius tip	3D contouring, mold & die, sculpting	2–4	Smooth on contours	Good
Corner Radius (Bull Nose)	Flat bottom, rounded corners (0.2–3 mm)	General CNC pocketing, semi-finishing	3–5	Better than square	3–5× longer than square
Roughing (Corncob)	Serrated / wavy cutting edges	Heavy stock removal, high MRR	4–6	Rough (needs finishing pass)	Excellent under heavy load
Chamfer	Flat bottom + 45° angled edge	Edge chamfering, deburring, countersinking	2–4	Good	Good
Tapered	Conical body, narrows toward tip	Mold/die draft angles, tapered slots	2–4	Good on sloped walls	Moderate
T-Slot Cutter	Wide flat cutter on narrow neck	T-slots, undercuts, fixture work	2–4	Good	Fragile neck — light cuts only
Dovetail	Angled edges (45° / 60°)	Dovetail slots in fixtures, slides	2–4	Good	Moderate
Drill Mill	Square end + 60°/90° drill point	Spotting, drilling, milling, countersinking	2	Good	Good
Thread Mill	Thread-form cutting edges	Internal/external threads, large diameters	Single-point or multi-form	Excellent thread finish	Good
Engraving / V-Bit	Conical V-shape, sharp tip	Engraving, fine text, detailed marking	1–2	Excellent detail	Fragile tip

ANSI B94.19 & ISO 1641

Imperial end mill dimensions follow ANSI B94.19 with inch-fraction sizes. Metric end mills follow ISO 1641 with millimeter diameters. Both standards define cutting diameter, shank diameter, flute length, and overall length for every tool size.

Flute Count & Material Match

Flute count affects chip evacuation and surface finish. 2-flute tools excel in aluminum, 3–4 flutes are general-purpose for steel, and 5–6+ flutes are for finishing and hard materials. Match flutes to material and operation for best results.

SELECTION GUIDE

How to Choose the Right End Mill

Follow these five steps in order of priority, using the charts on this page, and you will arrive at the correct tool for your material and operation every time.

Match Material to Coating

Find your material in the compatibility matrix. Note the coating, flute count, and helix angle. This eliminates tool-wrecking mistakes before you consider size.

Choose Largest Diameter

For a slot, diameter equals slot width. For a pocket, check the minimum corner radius — your tool radius cannot exceed it. Pick the largest diameter that clears all features.

Select Shortest Flute Length

Deflection scales with the cube of stick-out. If feature depth is 12 mm, do not use a 25 mm flute. Use the shortest one that reaches.

Choose Type by Geometry

Flat bottom features need square or corner radius. 3D surfaces need ball nose. T-slots need T-slot cutters. See the types chart above.

Verify Chip Thinning

Below 25% radial engagement, actual chip thickness is less than programmed. Multiply by the chip thinning factor — rubbing wears tools rapidly.

Example: Selecting a Tool for 6061 Aluminum

A pocket in 6061 aluminum is 12 mm deep with a 1.5 mm minimum corner radius. Aluminum calls for uncoated or ZrN, 2–3 flutes, 40° helix. The largest diameter that fits the 3 mm corner radius is 6 mm. A 6 mm tool with 12 mm flute length reaches exactly. Choose corner radius for edge strength. At 10% radial engagement, chip thinning factor is 1.2 — adjust feed accordingly.

Tool 6 mm Corner Radius

Coating ZrN / Uncoated

Result Optimal Selection ✓

COATING REFERENCE

End Mill Coatings by Material

Recommended coating, flute count, and helix angle for common machined alloys. Verify with your tooling supplier for specific grades.

Material	Grade	Coating	Flutes	Helix
Aluminum	6061, 7075	Uncoated, ZrN, DLC	2–3	40°–45°
Carbon Steel	1018, A36	TiN, TiCN	3–4	30°–35°
Alloy Steel	4140, 4340	AlTiN, TiCN	4–5	35°–40°
Stainless	304, 316	AlTiN, TiAlN	4–5	35°–40°
Tool Steel	A2, D2, H13	AlTiN, TiAlN	4–6	30°–35°
Titanium	Ti-6Al-4V	AlTiN, TiAlN	4–5	35°–40°
Nickel Alloy	Inconel 718	AlTiN, TiAlN	5–6	30°–35°
Copper / Brass	C360, C110	Uncoated, TiN	2–3	40°–45°

Flute Count Selection Guide

Flute count determines chip clearance, feed rate, and surface finish. Fewer flutes mean larger chip valleys — essential for soft, gummy materials that produce long chips. More flutes mean more cutting edges engaging the workpiece per revolution — faster feed rates but less room for chips. This end mill flute chart summarizes the trade-off.

Flutes	Best Materials	Feed Rate Multiplier*	Chip Clearance	Surface Finish	Key Rule
1	Plastics, soft aluminum, composites	1×	Maximum	Adequate	Only for hobby/DIY where chip evacuation is everything
2	Aluminum, brass, copper, acetal, slotting	1× (baseline)	Excellent	Good	Center-cutting capable; default for non-ferrous
3	Aluminum (modern preferred), general non-ferrous	1.5× vs 2-flute	Good	Good	Best balance for aluminum; ~50% faster than 2-flute
4	Steel, stainless, cast iron, tool steel	2× vs 2-flute	Moderate	Excellent	Workshop default for ferrous metals
5–6	Stainless, titanium, Inconel, hard milling	2.5–3× vs 2-flute	Limited	Excellent	Requires <20% radial engagement or chip packing results
7–8+	Specialist finishing, hard die/mold steels	3.5–4× vs 2-flute	Very limited	Ultra-fine	Niche; only at very light radial engagement

*Feed rate multiplier is relative to a 2-flute tool at the same spindle speed and chip load per tooth. Actual productivity gain depends on radial engagement, material, and machine rigidity.

CNC TOOLING GUIDE

Beginner CNC Starter Toolset Recommendations

If you just acquired a CNC mill and need a first set of tools, start here. These recommendations cover 90% of learning and light-production work without requiring a large inventory.

Steel & Stainless Set — 4-flute, TiAlN or AlTiN, solid carbide. Aluminum Set — 3-flute, uncoated or ZrN, high helix, solid carbide. Plus specials worth adding to any material set.

Steel & Stainless

4-Flute Carbide Set

1/4″ (6.35 mm) — small slots, detail work
3/8″ (9.53 mm) — general purpose
1/2″ (12.70 mm) — heavier roughing
+ 1/4″ ball nose for 3D contouring

Aluminum

3-Flute High Helix Set

1/4″ (6.35 mm) — general purpose
3/8″ (9.53 mm) — bulk removal
1/2″ (12.70 mm) — large pockets, facing

Specials

Worth Adding to Any Set

Corner radius — 3/8″ with 0.020–0.030″ radius extends tool life 3–5× for steel
45° chamfer mill — breaks edges and deburrs in seconds
1/8″ end mill — fine details and small pockets

Why These Tools?

This starter set gives you the ability to slot, contour, face, chamfer, and finish in both ferrous and non-ferrous materials. The 1/4″, 3/8″, and 1/2″ sizes cover the most common feature widths, and the corner radius tool dramatically extends tool life without sacrificing capability. Add the ball nose and chamfer mill as you move into 3D work and edge finishing.

3/8″ Most versatile starter size

3-Flute Best for aluminum chip evacuation

4-Flute Standard for steel & stainless

Standard imperial sizes: 1/32, 1/16, 3/32, 1/8, 5/32, 3/16, 1/4, 5/16, 3/8, 7/16, 1/2, 5/8, 3/4, 7/8, and 1 inch. Standard metric sizes: 0.5, 1, 1.5, 2, 2.5, 3, 4, 5, 6, 8, 10, 12, 14, 16, 18, and 20 mm. Full dimensions are listed in the chart above.

Choose the largest diameter that fits your tightest internal feature. Use the shortest flute length that reaches — deflection increases with the cube of stick-out. Select coating and flute count based on material: 2–3 flutes for aluminum, 4 for steel.

2-flute tools have larger chip valleys for aluminum, copper, and plastics. 4-flute tools have more cutting edges for higher feed rates and better finish in steel, stainless, and cast iron. Using 4-flute on aluminum causes chip packing and tool failure.

Uncoated polished carbide is the baseline. ZrN (zirconium nitride) is the preferred coated option — it reduces friction and improves tool life without chip-welding. DLC (diamond-like carbon) is the premium option with near-zero friction. Never use TiAlN, AlTiN, or AlCrN on aluminum.

No. Never. AlTiN contains aluminum and chemically bonds with aluminum workpiece material. Chips friction-weld to the edge within seconds, destroying the tool. Use uncoated polished carbide, ZrN, or DLC for aluminum instead.

For steel: 1/4″, 3/8″, and 1/2″ square (4-flute, TiAlN), plus one 1/4″ ball nose and one 3/8″ corner radius. For aluminum: 1/4″, 3/8″, and 1/2″ (3-flute, uncoated or ZrN). Add more as specific jobs require. See the starter toolset recommendations above for complete lists.

ER16 handles shanks up to 3/8″ (10 mm) — covers most general- purpose end mills. ER20 handles up to 1/2″ (13 mm). ER32 handles up to 3/4″ (20 mm). Match the collet series to your shank diameter for proper clamping.

Parts Machined with the Right Tooling, Every Time

This end mill size chart exists because tool selection is the difference between a good part, a scrapped part, and a broken tool. The right coating on the right material with the right flute count and the right diameter — that is what Baetro’s CNC programmers apply to every job that comes through our facility.

Upload Your CAD File Get Instant Quote