Guide
Fillet vs chamfer on machined parts: which edge should you specify?
Fillet vs chamfer is the choice a designer makes at every edge that is not left sharp: a fillet is a rounded edge of a stated radius, concave in an inside corner and convex on an outside one (where drafters often call it a round), while a chamfer is a flat bevel cut across the corner at an angle, most often 45°. In CAD the two cost the same click, but on the machine, on the inspection bench and under load they behave differently.
By Saola Manufacturing engineering team · Published · Updated
The right answer depends on three things: whether the edge is an inside or an outside corner, whether the part is milled or turned, and whether it will be coated. This guide walks through stress, machining cost and tooling, deburring and coating, and how to dimension each edge so the shop and the inspector read it the same way. The drawing rules come from ASME Y14.5, ISO 13715 and ISO 2768-1; the coating rule comes from MIL-A-8625F.
On this page
Fillet vs chamfer: which is better for stress and fatigue?
In an inside corner a fillet is clearly better, because a smooth radius spreads the stress that a sharp or chamfered corner concentrates. On an outside edge the difference in strength is small, and the choice is usually made on cost, assembly and coating instead.
Stress concentration lives in inside corners: the shoulder of a stepped shaft, the root of a boss or rib, the junction of a flange and a hub, the floor of a pocket. Under load the lines of force have to turn the corner, and the tighter the turn, the higher the local peak. The ratio of that peak to the nominal stress is the theoretical stress concentration factor, Kt, and it falls as the radius grows relative to the size of the section. Fatigue design data are reported against Kt for exactly this reason: the notched-specimen fatigue curves in MIL-HDBK-5J show, alloy by alloy, how much life a notch costs compared with an unnotched bar.
An inside chamfer is a poor substitute for an inside fillet. A bevel in an inside corner removes one sharp corner but creates two new ones where the bevel meets each wall, so the peak stress moves rather than disappears. Where a radius cannot be used because a mating part with a square or small-cornered edge must seat against the shoulder, the usual fixes are a relief groove (an undercut) under the shoulder, or a larger chamfer on the mating part that clears the fillet. Rolling-bearing seats are the classic case: the shaft fillet must be smaller than the minimum chamfer dimension of the bearing ring, whose limits are set per ISO 582, so the ring sits on the shoulder face instead of riding up the radius.
Threads show the same principle. The external UNR thread form in ASME B1.1 requires a rounded root, because a thread root is an inside corner repeated along the whole length of a bolt and a rounded root resists fatigue better than a flat or sharp one.
Outside edges carry little stress in most parts, so a chamfer and a round of similar size behave about the same under static load. The exceptions are fatigue-critical edges, such as the edge of a hole in a part loaded in tension, where a burr or tool mark at a sharp edge can start a crack and a smooth blend is safer; and any chamfer that runs into a fillet, a thread or a thin wall, where the intersection can create a new notch.
Which costs more to machine, a fillet or a chamfer?
On a milled part an outside chamfer is usually the cheaper edge, because one chamfer tool cuts any size simply by how deep it runs. Inside corners are the reverse: the cutter leaves a fillet for free, and it is a sharp or chamfered inside corner that costs extra.
Outside edges on a mill. A chamfer mill or a 90° spot drill makes a 45° chamfer of whatever leg length the program asks for, so a drawing with several chamfer sizes can still be one tool and one short pass. A convex outside round needs a corner-rounding end mill ground to that exact radius, one tool per radius, and the tool has to be set so its arc blends tangent into both faces. Set slightly off, it leaves a visible step or lip along one tangent line. Rounds on curved, three-dimensional edges with no matching cutter fall back to ball-end surfacing, which is many small passes and much slower.
Inside corners on a mill. Every vertical inside corner of a pocket gets a radius at least equal to the radius of the cutter, whether the drawing asks for it or not. The corner between floor and wall takes the shape of the end mill's tip: a bull-nose cutter leaves a fillet, a square end mill leaves a nearly sharp corner. A truly sharp vertical inside corner needs a process other than milling, such as EDM or broaching, and an inside chamfer at a pocket floor usually means a second tool and a second pass. Industry guidance is to draw vertical pocket corners a little larger than the cutter radius you expect, so the tool sweeps around the corner instead of being wrapped by it, which reduces chatter and lets a shorter, stiffer cutter reach full depth.
On a lathe the gap mostly closes. The insert already has a nose radius, and the finishing toolpath can cut a chamfer or an outside radius as part of the same pass. The inside radius at a shoulder is simply the nose radius or a programmed arc. What costs money on a lathe is a shoulder fillet that does not match a standard insert nose, or a radius at the bottom of a groove narrower than standard grooving inserts, either of which can force a special tool.
| Consideration | Fillet (radius) | Chamfer (bevel) |
|---|---|---|
| Inside corner under load | Lowest stress concentration; preferred at shoulders and roots | Leaves two new corners; avoid where fatigue matters |
| Outside edge, strength | Similar to a chamfer statically; best on fatigue-critical edges | Adequate for most edges |
| Milling an outside edge | One corner-rounding cutter per radius; tangent blend must be set accurately | One chamfer tool covers many sizes |
| Milling an inside corner | Left by the cutter anyway | Extra tool and pass; a sharp inside corner needs EDM or broaching |
| Turning | Nose radius or programmed arc | Programmed in the finishing pass |
| Anodize, plating, powder coat | Even coverage; radiused edges recommended by MIL-A-8625F | Two new edges where coating can thin or void |
| Assembly | Can stop a square-edged mating part from seating | Natural lead-in for bores, shafts and threads |
| Inspection | Radius gauge or optical comparison; small radii are hard to measure | Width, or diameter at the surface, with simple gauges |
| Drawing callout | R, CR, R MAX, or the ISO 13715 edge symbol | Leg × angle, two legs, or diameter × included angle |
When should you choose a chamfer and when a fillet?
Choose a fillet for inside corners under load, for edges that will be anodized or coated, and for edges people handle or see; choose a chamfer for lead-ins on bores and shafts, for general edge breaks on milled parts, and wherever a mating part must seat square against a corner. When an edge has no job at all, a general edge note is cheaper than modeling it.
- Assembly lead-ins: chamfer. A chamfer on a bore entry or a shaft end guides the mating part, protects an O-ring during installation and starts a press fit straight. Follow the lead-in the seal maker or gland standard asks for rather than a generic size.
- Thread starts: chamfer. A chamfer or countersink at a tapped hole, and a chamfer on the end of an external thread, protect the first thread from damage and help the fastener start.
- Loaded shoulders and pocket roots: fillet. Use the largest radius the mating parts allow, and give it a minimum, not only a nominal.
- Mating corners: chamfer on one side, fillet on the other. The part with the inside corner gets the fillet for strength; the part that sits against it gets a chamfer large enough to clear that fillet.
- Coated parts: fillet. Coatings cover a radius more evenly than a sharp or chamfered corner, as the next section explains.
- Handled and visible edges: small, consistent round. A uniform light round looks deliberate and feels better than a narrow chamfer of varying width.
- Castings: fillets in the model, chamfers where machined. NADCA's design guidance is to fillet every sharp corner and edge of a die-cast part when it is modeled, except the parting line (NADCA, fillets). Faces and bores machined after casting then get chamfers or breaks like any machined edge.
How do fillets and chamfers affect deburring and coating?
A chamfer usually removes the machining burr in the same operation, while a fillet made by a corner-rounding tool can leave a small burr or lip at its tangent lines. For coated parts the order reverses, because coatings build evenly over a radius and thin out at the edges a chamfer leaves.
A burr forms where the cutter exits the material, and a chamfer pass run after the profile cut takes the exit burr off with it. That is a large part of why a chamfer is the default edge break on milled parts. Mass finishing, whether vibratory, barrel or magnetic, rounds every exposed edge to a small, uncontrolled radius. It is an efficient way to break edges, and magnetic finishing with fine pin media can also reach burrs inside small holes, but it cannot hold a dimensioned radius, and it will also round an edge that must stay sharp, such as a seal edge or a scraper edge. If an edge must stay sharp, say so on the drawing and list it as an exception to the general edge note. On the die-cast base program described on the factory page, casting flash and drill burrs are removed by hand at the bench and the whole part is then tumbled in a magnetic finisher, which reaches burrs inside small holes that a hand tool cannot.
Coatings change the answer. MIL-A-8625F, the US military specification for anodic coatings on aluminum, warns that anodic coatings develop voids at sharp corners and edges and that all edges and inside corners should be radiused before anodizing; it ties the recommended radius to coating thickness, so a thicker coat needs a larger round (MIL-A-8625F, section 6.10.3). The same section says chamfering should not be used unless the sharp edges it leaves are also radiused, because a 45° chamfer cut with a sharp tool leaves two new edges, each of which can still thin the coating. Electroplate goes the other way at outside edges: current concentrates there and builds extra thickness, while recesses and tight inside corners are starved (IZA, polishing and plating). Powder coating tends to pull back from sharp edges as it flows and cures, so industry guidance for powder is the same as for anodize: round the edges.
Anodizing on aluminum, zinc plating and powder coating are all on the surface finishing menu our partner plants apply, and the quote names where each step is done, so on a part that is both machined and finished, write the edge requirement and the finish on the same drawing and state whether edge dimensions apply before or after coating.
How do you dimension a fillet or a chamfer on the drawing?
Dimension a chamfer by its leg length and angle, by its two legs, or on a hole by the diameter at the surface and the included angle; dimension a fillet with R, CR or R MAX and a tolerance. Then cover every undimensioned edge with one general note so nobody has to guess.
- 45° chamfer: a leader note such as
0.5 X 45°, with the leg measured along the face, is the form shown in ASME Y14.5. TheC0.5shorthand common on drawings made to Japanese and Chinese drafting standards means the same 45° chamfer, but ASME Y14.5 does not define it, so spell it out on an ASME drawing. - Chamfer at another angle: give two linear dimensions, or one linear dimension and
the angle, and make clear which face the leg is measured on. A
1 X 30°note is ambiguous unless the angle is shown from a definite face. - Chamfer on a hole: give the diameter at the surface and the included angle, as in
Ø10.5 X 90°. A diameter can be checked with a countersink gauge; a leg length inside a hole cannot be measured easily. - Fillet:
R2with a tolerance, a limit such asR2 MAX, or a range. Per ASME Y14.5-2018, a plain R defines a tolerance zone that the surface may wander within, including flats and reversals, while CR (controlled radius) also requires a fair curve with no flats or reversals. Use CR where the shape of the curve matters, such as a fatigue shoulder. - Pocket corners: a general note such as
INSIDE CORNERS R3 MAX UNLESS NOTEDtells the shop how large a cutter it may use instead of leaving it to guess. - Everything else: an ISO 13715 edge symbol with a signed size near the title block, or a general note with a range, covers every undimensioned edge. ISO 13715:2017 sets the notation but no longer recommends sizes, per the BSI record for BS EN ISO 13715:2019.
A chamfer or radius with no tolerance of its own takes the general tolerance from the title block. ISO 2768-1 has a separate table for external radii and chamfer heights, so a drawing that cites it already has a default for every dimensioned edge; the ISO 2768 and NADCA tolerances guide explains how that note is read.
What are the most common fillet and chamfer mistakes on drawings?
The expensive mistakes are an edge with no size, a sharp inside corner the mill cannot make, and a fillet on one part that stops its mating part from seating. Each one either forces a clarification round before quoting or produces a part that matches the drawing and still does not work.
- CAD default fillets on every edge of a prismatic part. Each different outside radius is another corner-rounding tool or another surfacing pass. Standardize on one or two radii, or use chamfers where the edge has no function.
- Sharp inside corners left in a pocket model. The cutter will leave a radius anyway; if the mating part needs a square corner, add a relief instead of hoping.
- Small inside radius at the bottom of a deep pocket. A small corner radius demands a small cutter, and a small cutter at long reach is slow and prone to chatter.
- Shaft fillet larger than the mating chamfer. The bearing, gear or collar rides on the radius and never touches the shoulder face. Check the pair, not each part alone.
- General edge break swallowing a small feature. A thin wall, a narrow sealing land or the first thread can lose a real share of its size to a break that is trivial on a large face. List such edges as exceptions.
- No minimum on a stress-critical fillet. With only a nominal radius and a loose general tolerance, a much smaller radius can pass inspection. Give the fillet a minimum.
- Unstated coating condition. Say whether an edge dimension applies before or after anodizing, plating or powder coating, because the coating changes both its size and its shape.
What should the RFQ say about fillets and chamfers?
Send the 3D model and a drawing that gives every functional edge its own callout and covers the rest with one general edge note. Then flag which edges carry load, seal, guide assembly or will be coated, so the quote reflects the right tools and the first-article report measures what matters.
- Every dimensioned chamfer and fillet with a tolerance or a limit, and CR where curve shape matters.
- A general edge note with a size range or an ISO 13715 symbol, plus its exception list.
- Which edges must stay sharp, and whether mass finishing is allowed on the part.
- The finish, and whether edge dimensions apply before or after it.
- Mating parts, or at least the corner geometry they present, for any filleted shoulder.
Chamfers are among the features the CNC turning line cuts routinely, alongside knurls, NPT threads and grooves, and CNC milling here is mostly the second operation on aluminum and zinc die castings, where datum faces, bores, pockets and tapped holes are cut after casting. Every toleranced dimension on the drawing is measured on the first piece from new tooling and reported in the first-article inspection report described on the quality page, which is one more reason to give an important radius a tolerance: an untoleranced edge note gives the inspector nothing to measure. Send the model and drawing through the quote form.
Frequently asked
Is a chamfer cheaper than a fillet?
On the outside edges of a milled part, usually yes, because one chamfer tool covers many sizes and also removes the exit burr. On a lathe the two cost about the same. In an inside milled corner the fillet is the cheap option, because the cutter leaves it anyway.
Does adding a fillet always make a part stronger?
In an inside corner under load, a larger fillet lowers the stress concentration, but it can also stop a mating part from seating or reduce the bearing face of a shoulder, so it has to be sized with the mating part. On an outside edge a fillet adds little static strength; its benefit there is fatigue resistance at a highly loaded edge and better coating coverage.
What size should a general edge break be?
There is no standard size, because the 2017 edition of ISO 13715 dropped its recommended values. Typical light edge breaks on machined parts fall somewhere around 0.1 to 0.5 mm (0.004 to 0.020 in), but that is shop practice, not a standard value, so write the range you need. The break all sharp edges guide covers the options.
Can tumbling or vibratory finishing replace a specified radius?
No. Mass finishing breaks edges to a small, uneven radius that depends on the media, the time and where the edge sits on the part. It is a good way to satisfy a general edge-break note, but a radius with a tolerance or a CR callout has to be machined.
Why are the inside corners of a milled pocket always rounded?
Because an end mill is round, the smallest vertical inside corner it can cut equals its own radius. A sharp inside corner requires EDM or broaching; if a square part must fit into the pocket, add a relief cut into the corner instead.
Sources
- ASME Y14.5-2018, Dimensioning and Tolerancing, ASME, 2018
- BS EN ISO 13715:2019, Technical product documentation — Edges of undefined shape — Indication and dimensioning, BSI, 2019 (identical to ISO 13715:2017)
- ISO 2768-1:1989, General tolerances — Part 1: Tolerances for linear and angular dimensions, ISO, 1989
- MIL-A-8625F, Anodic Coatings for Aluminum and Aluminum Alloys, US Department of Defense, 1993 (section 6.10.3)
- MIL-HDBK-5J, Metallic Materials and Elements for Aerospace Vehicle Structures, US Department of Defense, 2003
- ASME B1.1-2024, Unified Inch Screw Threads (UN, UNR, and UNJ Thread Forms), ASME, 2024
- Fillets, NADCA Design, North American Die Casting Association, accessed October 2026
- Polishing and plating, International Zinc Association, accessed October 2026