Corner Radius Guidelines for CNC Machining: Internal and External Corner Design

How tool geometry sets the minimum corner radius on a CNC machined part, why sharp internal corners drive up cost, and how to call out radii so your supplier doesn’t have to guess.
Sharp 90° corners look clean in CAD. On a CNC machined part, they rarely exist. Every internal corner cut with a rotating tool carries the imprint of that tool’s radius, and ignoring this on a drawing is one of the most common reasons parts come back for rework. This guide explains how corner radius works in CNC machining, how to size it against tool diameter, and when a sharp corner is worth the added cost.

What Is a Corner Radius in CNC Machining?

A corner radius is the curved transition machined where two walls of a feature meet, instead of a sharp right angle. In CNC milling, corner radius is not just a style choice — it is a direct result of using a cylindrical cutting tool to remove material from a pocket, slot, or step.

Internal Corner Radius vs External Corner Radius

An external corner radius sits on the outside edge of a part and is easy to produce, since the tool simply profiles around the outer boundary. An internal corner radius sits inside a pocket or cavity, where the cutter’s own diameter physically limits how tight that corner can be. This distinction drives most of the cost and lead-time questions buyers ask about corner geometry.

Why Corner Radius Design Matters for Cost and Tolerance

Specifying the wrong internal corner radius forces a shop to either swap to a smaller, more fragile tool, slow the feed rate near every corner, or use a secondary process. Any of those options adds cycle time and cost, and a corner radius left undefined on a drawing means the machinist has to guess and the buyer risks a first-article rejection.

Tool Radius and the Minimum Achievable Corner Radius

The rule that governs internal corner radius is straightforward: the minimum radius equals half the tool’s diameter. A 6 mm end mill cannot cut an internal corner tighter than a 3 mm radius, because the rotating cutter sweeps an arc as it changes direction. Most shops recommend designing to roughly 1.3 to 1.5 times the tool radius, not the bare minimum, to reduce tool engagement stress at the corner and protect surface finish.

Radius-to-Depth Ratio in Pockets and Cavities

Deeper pockets need proportionally larger corner radii. A tool that holds a tight radius at 5 mm depth can chatter and deflect at 25 mm depth using the same diameter, because tool rigidity drops as length-to-diameter ratio increases. Checking corner radius against pocket depth belongs in the same review as your part’s overall wall thickness and tolerance checks.

Minimum Corner Radius by Tool Diameter

Approximate minimum and recommended internal corner radius by end mill diameter
Tool DiameterAbsolute Min. Radius (D/2)Recommended Design Radius
3 mm1.5 mm~2.0 mm
6 mm3.0 mm~4.0 mm
10 mm5.0 mm~6.5 mm
12 mm6.0 mm~8.0 mm
20 mm10.0 mm~13.0 mm

Internal Corner Radius vs External Corner Radius: Side-by-Side

Internal corner radius vs external corner radius in CNC machined parts
FactorInternal CornerExternal Corner
Radius constraintSet by tool diameter (D/2 minimum)No practical minimum — can be sharp
ToolingLimited to end mill or specialty tool radiusAny profile tool can trace it
Cost driverSmaller radius = smaller, slower toolMinimal cost impact
Common fix for sharp requirementDog-bone/T-bone relief, EDM, wire cuttingNot usually needed

When Sharp Corners Are Unavoidable

Some assemblies genuinely need a square internal corner — a mating part with its own sharp edge, for example. When that is unavoidable, there are two practical paths.

Dog-Bone and T-Bone Fillets

A dog-bone or T-bone fillet adds a small extra relief cut at the corner so a round tool can complete its arc without leaving material behind, letting the mating part’s sharp edge seat fully while the machined corner itself stays radiused just outside the visible mating line.

EDM for Sharp Internal Corners

Wire or sinker EDM can produce genuinely sharp internal corners because it erodes material with an electrode rather than a rotating cutter. It is slower and more expensive than milling, so it is usually reserved for features where a radius truly cannot be tolerated. For general background on fillet geometry, see this reference on fillets in mechanical design.

Practical Manufacturing Examples

Aluminum mounting plate

A 6 mm end mill pocket specified with a 4 mm internal corner radius machined cleanly in one pass, avoiding the tool slowdown a 3 mm minimum radius would have required.

Steel die component

A mating punch needed a sharp internal corner. The shop added a dog-bone relief at the corner and held the visible mating edges sharp, avoiding a costly EDM operation.

Deep pocket in a stainless housing

A 30 mm deep pocket originally called out a 3 mm radius. Because depth exceeded the safe length-to-diameter ratio for that tool, the radius was increased to 5 mm, allowing a shorter, stiffer tool and cutting cycle time significantly.

Common Corner Radius Design Mistakes

  • Leaving internal corners marked “sharp” with no radius value, forcing the shop to assume a tolerance
  • Specifying a radius exactly equal to the tool’s minimum, with no clearance margin
  • Using the same radius on both the floor and wall of a deep pocket, which complicates tool selection
  • Ignoring radius-to-depth ratio on deep cavities, leading to chatter and tool deflection
  • Requesting sharp internal corners across an entire part instead of only where function requires it

Running these checks during a DFM review before quoting catches most corner radius issues before they affect lead time.

Table of Contents

Frequently Asked Questions About Corner Radius in CNC Machining

The minimum internal corner radius equals half the diameter of the tool used — a 6 mm end mill produces a 3 mm minimum radius. Designing slightly larger than this minimum is recommended.
No. External corners can be machined sharp without added cost, since the tool profiles around the outside edge rather than cutting into an enclosed pocket.
Use a dog-bone or T-bone relief cut to let a round tool clear the corner, or specify EDM for a genuinely sharp internal edge where a relief feature isn’t acceptable.
A smaller radius requires a smaller, more fragile tool and slower feed rates at the corner, which increases cycle time and tool wear — both of which raise the machining cost.

Get Your Corner Radii Reviewed Before You Quote

Upload your CAD file and our team will check every internal and external corner radius against tool access and cost as part of a free DFM review.

Get it free