Chamfer vs Fillet: Which Edge Treatment Belongs on the Drawing

Every machined part has edges, and every edge is a decision. A chamfer removes material at an angle, a fillet adds it in a curve, and a raw edge is a burr waiting to cut somebody. The choice changes fatigue life, assembly behavior, coating adhesion and cycle time — and drawings usually settle it with a note reading "break all sharp edges".

What each treatment actually does

A chamfer is a straight cut across an edge: fast, because a 45° chamfer mill runs the profile in one pass, and predictable, because the geometry is a line. It removes a burr, guides a mating part, protects a coating at a thin edge and starts a thread.

A fillet blends two surfaces with a radius. On an external edge it softens the corner; on an internal corner it removes the sharp notch that concentrates stress. It is slower, needing a ball-nose or corner-radius tool, a separate pass and often a very small cutter.

The split is simple: chamfers handle handling, assembly and coating. Fillets handle structure.

Stress concentration in numbers

On a 40 mm shaft stepping down to 30 mm under bending, the fillet radius as a fraction of step height sets Kt. At r/t = 0.05 — a 0.5 mm radius on a 10 mm step — Kt is about 2.2. At r/t = 0.2, a 2 mm radius, it falls to 1.6; at 0.4 it is near 1.35 and more radius buys little.

So going from 0.5 mm to 2 mm raises the alternating stress the part survives by roughly 35 percent, with no change to the section. Going from 2 mm to 5 mm buys another 10 percent and starts to crowd the bearing seat.

A 45° chamfer at the same shoulder is better than a sharp corner and much worse than a fillet. It removes the notch but creates a new one at each end of the chamfer, and Kt typically lands around 1.8 to 2.0 — worse than a 1.5 mm fillet and better than nothing.

For a rotating part, that difference is the difference between infinite life and a crack that starts at the shoulder after a few million cycles.

See also: Surface Finish Callout: Ra, Rz and How to Specify per Surface and Wafer Handling End Effector Machining: Flatness, Edge Radius and Mass.

When 0.5 mm is enough

Most edges carry no structural load, and 0.5 mm is enough for nearly all of them, provided it is actually made. The useful sizes:

• 0.2 to 0.3 mm edge break on internal edges, small parts, and anywhere a 0.5 mm chamfer would eat a thin wall.
• 0.5 × 45° on external edges that get handled, on bores that receive a shaft or a pin, and on the ends of threads.
• 1 × 45° on a threaded hole or a shaft end that must self-guide during assembly, and on the entry of a bore with an O-ring.
• 0.2 × 45° on a dowel hole or a precision bore where a larger chamfer would reduce the bearing length.

Below 0.2 mm a chamfer stops being producible at a stated size and becomes a deburr: the edge is broken but the dimension is not controlled. A "0.1 mm chamfer" on a drawing is a deburr with a tolerance nobody can hold.

What a fillet costs

An external chamfer is one pass with a chamfer mill, roughly 5 to 10 seconds per edge. A 0.5 mm fillet in an internal corner needs a tool no larger than Ø1 mm: slow feeds, short tool life, a separate pass, 20 to 40 seconds per corner.

"All internal corners R1" can double the cycle time of a pocketed aluminum part. "Break all sharp edges 0.3 to 0.5 mm" adds almost nothing, because the deburr was going to happen anyway.

The expensive case is a small fillet deep in a pocket. A 0.5 mm radius at the bottom of a 30 mm pocket needs a Ø1 tool with 30 mm of reach, a 30:1 ratio no cutter survives. If the fillet is structural, widen the pocket or add a relief; if it is cosmetic, delete it.

Drawing callouts that get made

Vague notes produce variable parts. These forms are unambiguous:

• "Break all sharp edges 0.3 mm max." The word max avoids a 0.3 mm minimum that would remove too much on a thin feature.
• "0.5 × 45°" rather than "0.5 chamfer". A chamfer specified only by leg length is ambiguous between the axial leg and the face width; 45° makes them equal, and any other angle needs both numbers.
• "R0.5 ±0.2" on an internal corner, with the radius referenced to the corner it blends.
• "Undercut 0.3 × 0.3 at shoulder" where a fillet would interfere with a bearing or a seal. A relief undercut removes the grinding notch and is often better than a small fillet in the same place.
• "No chamfer on the sealing face" — a chamfer across an O-ring land is a leak path, and a well-meant edge break note can destroy a seal.

The treatments we see most often, with cost relative to a plain machined edge:

A sequence note that saves rework

Cut chamfers after the functional surfaces are finished. A 0.5 mm chamfer on a bore edge cut before the bore is finished gets recut by the boring bar and ends up 0.8 mm wide, which matters on a 6 mm bearing seat. On turned parts, keep the chamfer tool in the same turret as the finishing tool; on milled parts, run one chamfer toolpath at the end of the cycle over every external edge.

Edges also matter after machining. Anodize chips at a sharp corner because the coating is brittle and thin there, so a 0.5 mm chamfer gives it something to build on — which is why we check edge callouts against the surface finishing spec before quoting.

If the drawing has a structural fillet, tell us the load direction: a fillet sized for bending is not necessarily right for torsion. Send the file and we will flag the edges that cost money and the ones that are free.

Frequently asked questions

Is a chamfer or a fillet stronger?

A fillet, in almost every load case. It spreads stress over a radius instead of ending at two new corners, so Kt is lower for the same removed material. A chamfer beats a sharp edge and loses to a well-sized fillet.

What does "break all sharp edges" mean in practice?

A deburr of roughly 0.2 to 0.5 mm with no controlled dimension. Right for non-functional edges, wrong for a sealing face or bearing seat, where it can remove material you needed.

How small a chamfer can be machined reliably?

About 0.2 mm. Below that the edge is deburred rather than chamfered, and the size is not inspectable with normal shop equipment. If you need a 0.1 mm edge break, specify a deburr and a visual standard instead of a dimension.

Does a fillet always cost more than a chamfer?

On an external edge, yes: a separate tool and pass. In an internal corner it costs much more, because the tool must be small enough to enter and long enough to reach. A structural fillet at a shoulder is usually worth the cost; a cosmetic one in a deep pocket usually is not.

Related reading

• Thin Wall Machining: Deflection, Support Methods and Realistic Tolerances2026-09-29
• O-Ring Groove Machining: Tolerances That Decide Whether the Joint Seals2026-10-01
• Dowel Pin Hole Tolerance: Reamed, Bored or Interpolated Holes2026-10-03