You are here:

Minimum Internal Corner Radius in CNC Machining

Views: 1013 Publish Time:
Renjie Precision
Precision CNC Machining, Sheet Metal & Injection Moulding
specializes in precision CNC machining, rapid prototyping, sheet metal fabrication, laser cutting, plastic injection molding, and surface finishing
follow me on:


Minimum Internal Corner Radius in CNC Machining

Ask a designer to draw a pocket and they will draw four sharp 90-degree corners. Ask a machinist to cut it and the first question is which end mill you are willing to pay for. An internal corner cannot be sharp with a rotating cutter: the tool has a radius, and that radius becomes the corner. Every internal corner on a CNC milled part is, by definition, a fillet.

That single geometric fact drives tool selection, cycle time, surface finish and cost more than most people expect. This guide gives the practical radius ranges, explains the depth-to-diameter relationship that quietly sets the real minimum, and shows what to put on the drawing so the shop does not have to guess.

The Short Answer

For a standard pocket in aluminum or steel, specify an internal corner radius of at least 3 mm (0.125 in) if you want a normal quote. Smaller is possible, but it is never free.

Specified internal radiusTool it impliesPractical consequence
R6 mm or larger12 mm end mill or biggerFast, rigid, one roughing pass
R3 mm6 mm end millComfortable default for most pockets
R1.5 mm3 mm end millSlower feeds, limited depth, higher tool cost
R0.5 mm1 mm end millVery slow, shallow passes, frequent breakage
R0 (sharp)Not millableRequires EDM, broaching, or a dogbone relief

The rule of thumb: the corner radius should be at least one sixth of the pocket depth, and ideally larger. A 30 mm deep pocket with R1 mm corners is a part that will be quoted slowly, or declined.

Why a Sharp Internal Corner Is Physically Impossible

An end mill is a cylinder. Sweep it around a 90-degree internal corner and the cutter centre follows an arc whose radius equals the tool radius. The material left in the corner is a quarter-circle of exactly that radius. There is no feed rate, no toolpath strategy and no controller setting that changes this; it is geometry.

External corners are different. A sharp outside edge is easy because the tool approaches from free space. This asymmetry explains why drawings that mix sharp external edges with sharp internal corners look perfectly reasonable in CAD but cannot be made as drawn.

The confusion usually comes from other processes. A laser-cut blank, a waterjet part, an injection moulded part or a wire EDM part can have near-sharp internal corners, because those processes do not use a rotating cylindrical tool. If a designer has spent more time on sheet metal or moulded parts than on milled parts, sharp internal corners feel normal. Our guide to the differences between moulding and machining covers where that assumption breaks down.

The radius is set by the tool, not by the drawing

If the drawing says R2 and the shop uses a 6 mm end mill, the corner comes out R3. The part is out of spec even though every other dimension is correct. Conversely, if the drawing says R6 and the shop uses a 6 mm mill, the corner is R3 and it is still out of spec — too small a radius leaves a step where the mating part expects clearance.

This is why a corner radius callout is really a tool diameter callout. Writing "R3" tells the machinist "use a 6 mm cutter here", and that in turn constrains how deep they can cut.

Depth-to-Diameter: The Limit That Actually Bites

Tool deflection scales with the cube of the overhang and inversely with the fourth power of the diameter. In plain terms, a long thin cutter is dramatically less stiff than a short thick one. A 6 mm end mill cutting at 3x diameter (18 mm) of flute length is routine; the same tool at 6x diameter (36 mm) needs reduced radial engagement, lighter passes and often a completely different strategy.

Tool diameterComfortable max depthAbsolute max with careTypical corner radius
12 mm24–36 mm48 mmR6
8 mm16–24 mm32 mmR4
6 mm12–18 mm24 mmR3
3 mm6–9 mm12 mmR1.5
1 mm1.5–2 mm3 mmR0.5

So a 25 mm deep pocket with R1 mm corners is contradictory: the radius demands a 2 mm cutter, but that cutter cannot reach 25 mm. The shop must either use a tapered or necked tool, switch to a different process, or ask you to change the design. Most of the "unexpected" cost on small-radius deep pockets comes from exactly this conflict.

For a deeper treatment of the related depth problem, see our article on minimum wall thickness, where the same stiffness limit shows up as wall deflection rather than corner radius.

What a Small Radius Actually Costs

Three costs compound:

  • Cycle time. A 3 mm cutter removes material at roughly a quarter the rate of a 12 mm cutter. Even if the small tool only runs the corner-cleanup pass, that pass still has to happen on every pocket, on every part.
  • Tool consumption. Small end mills break. A 1 mm cutter in a slotting pass has a short and unpredictable life, and a broken tool in a deep pocket can scrap the part.
  • Extra setups. If the corner radius is smaller than the floor radius the main tool can leave, the job needs a second tool, a tool change, and a separate finishing toolpath. On a 20-part run that is a noticeable share of the quote.

A useful mental model: specifying R1 instead of R3 on a mid-size aluminum housing typically adds 15–40% to the milling time, and on hardened steel it can double it. Enlarging the radius is one of the highest-leverage DFM changes available — see our cost-reduction checklist for the other levers.

When You Genuinely Need a Sharp Corner

Sometimes a mating part has a square shoulder and the assembly really does need the pocket to seat fully. There are four standard solutions:

1. Dogbone (undercut) corners

The shop extends the cutter slightly past the corner in each direction, leaving a small circular relief. The mating square corner now fits, and the pocket walls remain straight where they matter. Dogbones are cheap and are the default answer for a square insert in a milled pocket. They do require the designer to accept a visible relief, and they need to be called out explicitly — a shop will not add them unasked.

2. T-bone corners

A single relief on one side of the corner, rather than both. Easier to program, slightly weaker in the corner region, and common on larger enclosures where one wall is non-critical.

3. Wire EDM or broaching

Wire EDM produces a genuinely sharp internal corner with a small wire radius, but only on through-features in conductive material, and at a much higher cost per part. Broaching works for specific profiles. Both are viable for low volumes of hardened tooling components.

4. Radius the mating part instead

Usually the best answer. If the insert can carry an R3 chamfer or radius, the pocket can be cut with a 6 mm tool in one pass and the whole problem disappears. This is a conversation worth having before the drawing is released.

What to Put on the Drawing

Four things remove ambiguity:

  • State the radius explicitly on every internal corner, or use a general note such as "all internal corners R3 unless noted". Do not leave the corner undefined and hope the shop picks something sensible.
  • Make the radius larger than the tool radius you expect, not exactly equal. R3.2 with a 6 mm cutter gives the tool a little room and produces a better finish than a dead-on R3.0.
  • Call out floor radius separately if the pocket has a filleted bottom-to-wall transition. A ball-end mill leaves a floor radius equal to half its diameter; this is a different feature from the vertical corner radius and is easy to omit.
  • Mark dogbones where required, with a detail view. A note like "dogbone relief at four corners to accept square insert" is enough.

Tolerance on a corner radius deserves the same restraint as any other non-functional feature. Holding R3 ±0.05 requires inspecting a radius, which is slower and less repeatable than measuring a linear dimension. R3 ±0.2, or simply "R3 max / R2.5 min", is usually enough. Our tolerances guide explains which callouts actually drive inspection cost.

Material-Specific Notes

MaterialEffect on small internal radii
6061 / 6082 aluminumForgiving; small cutters work well with good chip evacuation
7075 aluminumSimilar, but thin corner sections can distort after roughing
Mild and alloy steelHigher cutting force; deflection increases with smaller tools
304 / 316 stainlessWork hardening; avoid rubbing in corners with light radial engagement
Titanium Grade 5Heat concentration in corners; small tools have very short life
POM, PEEK, G10Deflection and melting rather than tool wear set the limit

In stainless and titanium, corner cleanup passes are where tools fail most often, because the cutter engagement angle spikes as it enters a corner. A constant-engagement toolpath (trochoidal or adaptive) keeps the load steady and is worth specifying for deep pockets in these materials.

How the Radius Is Inspected

Radius gauges, a CMM with a small probe, or an optical comparator all work, but a radius is inherently harder to verify than a diameter. On a production run, shops often verify the pocket width and the corner clearance with a gauge pin or a mating part instead of measuring the radius directly.

If the corner radius is functional — for instance it controls stress concentration at a loaded fillet — say so on the drawing. A functional radius gets measured; a cosmetic one gets a visual check, and treating them identically adds cost without adding confidence.

Frequently Asked Questions

What is the minimum internal corner radius for CNC machining?

There is no hard minimum, but R0.5 mm is about the practical floor for milled metal parts, and it requires a 1 mm cutter, shallow depths and slow feeds. For a normal production quote, R3 mm is the sensible default. Anything below R1 should be treated as a deliberate cost decision.

Why can a milled pocket not have sharp inside corners?

Because the cutting tool is a rotating cylinder. The tool centre traces an arc, leaving a quarter-circle of material at every internal corner. Only non-rotating processes — wire EDM, broaching, laser or waterjet cutting, and moulding — can produce a near-sharp internal corner.

Does a larger corner radius make the part weaker?

Usually the opposite. A larger radius reduces stress concentration at the corner. The concern is assembly clearance: a mating part with a square shoulder may no longer seat. That is solved with a dogbone relief or by radiusing the mating part, not by shrinking the pocket radius.

How does corner radius relate to pocket depth?

The radius determines the maximum tool diameter, and tool diameter determines how deep the cutter can reach before deflection becomes unacceptable. As a working rule, keep pocket depth below 3x the tool diameter for comfort, which means the corner radius should be at least one sixth of the depth.

Should I call out a tolerance on an internal corner radius?

Only if the radius is functional. A loose callout such as R3 ±0.2 or "R3 max" is enough for clearance features. Tight radius tolerances slow inspection and rarely improve fit, since the mating part is what actually determines whether assembly works.

If you are unsure whether a corner radius on your drawing will survive contact with a real end mill, send the model before releasing it. A five-minute DFM review at the design stage is considerably cheaper than a re-quote after the first article. For more on that process, see our DFM rules for machined parts.