Chamfer vs fillet in CNC machining: when each one actually matters

Chamfers and fillets show up on every CNC drawing. Most articles treat the choice as cosmetic. It isn’t — the wrong edge feature in the wrong spot either wastes machining time or plants a fatigue crack. This guide covers the engineering tradeoff with real Kt data, verified costs, and DFM rules from our shop floor.

Geometry: what’s actually different

A chamfer removes a sharp edge with a flat, angled cut — usually 45°, though 30° and 60° exist for weld prep and specific assembly needs. It’s defined by two numbers: leg length and angle (e.g., 1 × 45°), or two leg lengths for asymmetric cuts (e.g., 0.5 × 1.0 mm). The ASME Y14.5-2018 standard allows a simplified note for 45° chamfers and requires explicit distance + angle callouts for all other angles.

Source: ASME Y14.5-2018, Section 7.3 — Chamfer Dimensioning

A fillet replaces the corner with a circular arc defined by a single radius R. The critical difference isn’t shape — it’s tangency. A fillet surface stays tangent to both adjacent faces, so loads transition smoothly through the curve. A chamfer surface meets the original faces at two distinct edges, creating two abrupt direction changes instead of one.

That tangency distinction drives everything downstream: stress behavior, tooling selection, and cost.

Stress concentration — the Kt numbers that matter

When a load passes through a geometric transition, stress doesn’t spread evenly. It piles up at the sharpest point. The stress concentration factor Kt tells you how much peak stress exceeds the nominal — and it’s the reason fillet-vs-chamfer is an engineering decision, not a cosmetic one.

The real numbers from Peterson’s

The table below draws from Peterson’s Stress Concentration Factors (Pilkey & Pilkey, 4th Edition, Wiley, 2020), the standard reference for Kt values in mechanical design. Note: many competing articles online claim a sharp 90° corner has Kt ≈ 3.0. That’s misleading. ❌ Error

Source: Pilkey, W.D. & Pilkey, D.F. (2020). Peterson’s Stress Concentration Factors, 4th Ed., Wiley. Charts 3.1–3.4 (stepped shafts under bending/torsion).

Why this matters for fatigue life

Fatigue life in metals scales roughly with stress raised to the power of 3–5 (Basquin’s law). So reducing Kt from 2.7 to 1.4 by adding a proper fillet doesn’t just cut peak stress in half — it can extend part life by 10× or more under the same cyclic load.

Here’s a nuance that no competitor article mentions: Kt is the theoretical elastic stress concentration factor. What actually governs fatigue is Kf — the fatigue notch factor — which accounts for the material’s notch sensitivity. Kf is always ≤ Kt, and the gap widens for ductile materials and large radii. For aluminum alloys, notch sensitivity q is roughly 0.8–0.95; for quenched and tempered steels, it’s 0.95–0.99.

Source: Shigley’s Mechanical Engineering Design, 11th Ed., Budynas & Nisbett, Ch. 6.

Source: Yahr, G.T. (1993). “Fatigue Design Curves for 6061-T6 Aluminum,” ORNL/TM-12011, Oak Ridge National Laboratory. See also: Engineers Edge summary.

Machining cost: where the budget goes

The engineering preference for fillets collides with a machining reality: chamfers are faster to cut. But the cost gap is widely misquoted online. Some articles cite “$0.25–$0.50 per chamfer edge” — that figure assumes a specific US shop rate, specific material, and specific batch size. It’s not a universal constant. ⚠️ Caution

What we can say from our production floor (200+ CNC machines, running 6000+ unique part numbers per year):

The real cost driver isn’t the feature itself — it’s the tool change. Each unique radius that doesn’t match the existing tool lineup adds 30–90 seconds of tool change time. On a 50-part run, three unnecessary tool changes compound into 75–225 minutes of lost spindle time. Standardize your fillet radii and most of this evaporates.

The “free fillet” that everyone overlooks

Internal pocket corners on milled parts already have a fillet. The end mill is round — a ∅6 mm end mill leaves a 3 mm radius in every internal corner whether you want it or not. If your design calls for R3 internal fillets and your shop runs ∅6 end mills for roughing, those fillets cost exactly zero. But specify R2.7 and the shop either accepts the R3 it gets naturally, or switches to a smaller tool to chase a non-standard dimension.

Tooling and material-specific notes

Chamfer tooling

A standard 90° included-angle chamfer mill handles most 45° chamfers on external edges. The same tool handles countersinks on fastener holes. Programming is one toolpath line — coordinates plus depth. Feed rates are aggressive: 0.05–0.1 mm/tooth for aluminum, 0.03–0.06 mm/tooth for stainless.

Fillet tooling by material

Aluminum 6061-T6: Ball end mills at 10,000–18,000 RPM. Surface finish Ra 1.6 µm achievable in a single contour pass with 0.3–0.5 mm stepover. Low hardness means long tool life — we typically see 400–600 parts per ball end mill before replacement.

316L stainless steel: Work hardening is the primary risk. Maintain feed above 0.03 mm/tooth — dwell or interrupted cuts cause the material to harden under the tool and accelerate wear. TiAlN-coated carbide ball end mills at 2,800–3,500 RPM with flood coolant. Nose wear is the failure mode; apply a 0.1 mm flank wear limit.

4140 Q&T steel (HRC 28–34): Effective cutting speed at the ball nose center approaches zero because the tool rotates around its own tip. Actual chip formation happens on the flank. Keep radial engagement ≤ 30% of ball diameter. AlTiN-coated carbide, Ra 0.8–1.6 µm finish achievable.

Standard ball end mill radii — design to these

Most CNC shops stock ball end mills in these diameters: 2, 3, 4, 5, 6, 8, 10, 12 mm — producing fillet radii of R1, R1.5, R2, R2.5, R3, R4, R5, R6 mm. Specifying R2.7 forces a non-standard tool or multiple passes with a smaller cutter. Specifying R3 uses a stock ∅6 ball end mill. Faster, cheaper, more repeatable.

When to use which — decision framework

The choice isn’t always either/or. Most well-designed CNC parts use both — fillets at structural transitions, chamfers everywhere else. The question is placement, not preference.

Use a fillet when:

The corner carries load. Shaft shoulders that seat bearings, bracket base transitions, gearbox housing internal corners, gear root geometry (per ISO 6336). Anywhere subject to bending, torsion, or cyclic loading. For shaft shoulders, the r/d ≥ 0.1 rule from standard fatigue design practice is a reliable starting point: on a 40 mm shaft stepping to 30 mm, specify R4 mm minimum at the transition.

Also use fillets where fluid flow matters — sharp internal corners cause turbulence and dead zones in manifold passages and flow channels. And on consumer product edges where tactile quality drives perceived value.

Use a chamfer when:

Assembly insertion (shaft-to-bearing, pin-to-hole, thread lead-in). Deburring external edges for handling safety. Countersinks for flush fastener seating. Weld prep per AWS D1.1 / D1.2 (V-groove, J-groove — these require specific chamfer angles, not 45°). Anywhere machining cost matters more than stress performance.

The alternative nobody mentions: dog-bone relief cuts

When a mating part requires a sharp internal corner (e.g., a square tenon fitting into a square mortise), neither a fillet nor a chamfer solves the interference. A dog-bone relief — a small circular cut at each internal corner, extending beyond the 90° intersection — clears the mating geometry while keeping the cutter large enough to be practical. It’s not pretty, but it’s a standard CNC technique for parts that must assemble with tight-fitting square features.

DFM rules from the shop floor

These aren’t textbook guidelines — they come from reviewing 800+ DFM reports per month in our factory.

Rule 1: Standardize to 3–5 fillet radii per part family. R1.5, R2, R3, R4, R5 mm cover nearly every structural application. Standardizing reduces tool inventory, setup time, and programming complexity. In our experience, this single change reduces per-part programming time by 20–30%.

Rule 2: Apply fillets only at genuine stress points. Not every internal corner needs a structural fillet. Non-loaded pocket corners can take whatever radius the roughing end mill leaves naturally. Reserve deliberate fillets — with specific radii called out on the drawing — for shaft shoulders, bracket transitions, housing load-transfer corners, and gear roots.

Rule 3: Avoid sub-R1 mm fillets in hard materials. Fillets below R0.5 in 316L or hardened steel require ≤ 1 mm diameter ball end mills — fragile, slow, $15–40 per tool, and they break without warning. If the design forces a tight corner, consider wire EDM for that feature instead of trying to push a tiny ball end mill through hardened steel.

Rule 4: Match fillet R to your mating part’s corner condition. If your fillet on Part A interferes with a sharp corner on Part B, the assembly won’t close. Either add a matching fillet on Part B or add a relief groove. This is the #1 assembly interference we catch in DFM review — and it’s preventable in CAD.

Rule 5: Chamfer tolerances — stop overspecifying. A deburring chamfer at ±0.5 mm is fine. Calling out ±0.05 mm on a 0.5 × 45° edge break adds inspection cost with zero functional benefit. Reserve tight chamfer tolerances for functional features like countersinks for flush fasteners or weld prep geometry.

Common drawing mistakes we see

These show up repeatedly in the 2D drawings our engineering team reviews:

Zero-radius internal corners on milled parts. Physically impossible. The shop will call you and the project stalls while you revise. Always specify a minimum internal radius in your CAD model — R1.5 mm or larger unless the geometry demands tighter. Some CAD software defaults to sharp corners; override this before exporting your STEP file.

Mixing five or more fillet radii on a single part. Each unique radius may require a different ball end mill. More tools = more tool changes = more cycle time = higher cost. Two or three standardized radii cover most parts. If you find yourself specifying R1.7, R2.1, R2.4, and R3.2 on the same bracket, something went wrong in design intent.

Filleting every external edge. External fillets on non-loaded edges add cost without adding structural value. A 0.3 × 45° chamfer removes the burr, protects the handler, and adds 5 seconds of machine time. An external R2 fillet on the same edge adds 30–60 seconds and a tool change. Unless you’re making a consumer device where radius edges define the product feel, chamfer external edges.

Ignoring the injection molding crossover. If this CNC prototype will eventually transition to injection molded production, internal fillets are mandatory for moldflow anyway. Design them in during prototyping, not after. The prototype fillet radii become your mold cavity radii — one less variable to change during the production transition.

FAQ