Quick Answer
Internal corner radius in CNC machining is the radius at the inside corner of a pocket, slot, or feature. For milling operations, the radius should be as large as function allows, because the cutting tool must fit into that radius. A smaller radius forces the use of a smaller diameter end mill, which is less rigid, more prone to deflection, and increases machining time. A general rule is to design internal corner radii at least 30% to 50% of the pocket depth, and preferably larger than 0.5 mm for standard tools. Large radii also allow the use of standard tool sizes and reduce the number of finishing passes.
Key Takeaways
- Small internal corner radii (<3 mm) often require ball end mills or small diameter flat end mills, increasing tool wear and cycle time.
- A radius smaller than 0.5 mm is difficult to mill with standard cutters; consider EDM or wire EDM for sharp inside corners.
- Larger radii (R2, R3, R5) enable the use of larger, more rigid end mills that remove material faster and with better surface finish.
- For deep pockets, the radius should be at least 30% of the pocket depth to avoid excessive tool stick-out and deflection.
- Designing identical radii in multiple corners reduces tool changes and simplifies programming.
- When specifying a radius, always indicate it on the 2D drawing with a callout like R2 or R3, and ensure the 3D model matches exactly to avoid confusion.
Why Internal Radius Matters
Internal corner radius is one of the most influential design features affecting CNC machining cost and quality. It directly determines which cutting tools can be used, how many passes are needed, and whether additional operations like EDM are required. Engineers often specify sharp inside corners (R0) without understanding the machining consequences, leading to higher cost, longer lead times, or inspection failures.
In milling, the cutting tool is round, so the smallest theoretical radius that can be machined in a corner is limited by the tool's diameter. To create a truly sharp internal corner (zero radius), a flat end mill would need to have infinitesimally small diameter, which is impractical. Instead, the corner is finished with a radius equal to the tool's radius. Therefore, the designed radius must match (or exceed) the available tool radius. If a smaller radius is required, operators often use a smaller end mill for the corners, which increases machining time and tooling cost.
How Radius Affects Tool Selection
The relationship between corner radius and tool diameter is straightforward: an internal corner of radius R requires a cutter with diameter ≤ 2R to fit into the corner without leaving excess material. For example, an R1 corner requires an end mill of ≤ 2 mm diameter. However, a 2 mm end mill is much less rigid than a 10 mm end mill. It can only take shallow passes, deflects easily, and wears quickly. This directly impacts machining time and part accuracy.
| Required Internal Radius (mm) | Max Tool Diameter (mm) | Typical Tool Rigidity | Relative Machining Cost |
|---|---|---|---|
| 0.5 | 1.0 | Very Low | High (often uses EDM) |
| 1.0 | 2.0 | Low | High |
| 2.0 | 4.0 | Moderate | Medium |
| 3.0 | 6.0 | Good | Low |
| 5.0 | 10.0 | High | Low |
| 10.0 | 20.0 | Very High | Lowest |
As a rule of thumb, for general precision machining, internal corner radii should be at least 1.5 mm to allow use of 3 mm end mills (common in CNC shops). For prototypes or one-off parts, smaller radii can be tolerated but at additional cost. For production runs, radii of R3 or larger are strongly recommended to keep cycle times low.
Impact on Surface Finish and Tolerance
When a small end mill is forced to cut a deep corner, tool deflection increases. The actual cut may leave excess material near the bottom of the corner, and the surface finish in that region often deteriorates. If a tight tolerance (e.g., ±0.05 mm) is required on the corner profile, additional semi-finish and finish passes are necessary, which multiply cycle time. Larger radii allow the use of a single larger end mill that can rough and finish in fewer passes, achieving better surface roughness (Ra 0.8 μm or lower) without extra operations.
Design Guidelines for Corners in Pockets and Slots
Uniform Radius Across Features
Avoid mixing different radii in the same pocket if possible. All internal corners should ideally have the same radius, because each different radius requires a different tool diameter or a separate corner milling operation. Standardizing on R2, R3, or R5 (depending on shop capabilities) simplifies setup and reduces tool changes.
Corner Radius vs. Pocket Depth
For pockets deeper than 20 mm, the required internal radius increases to allow adequate tool reach. A rule of thumb: corner radius ≥ 0.3 × pocket depth. For example, a 30 mm deep pocket should have internal radii no smaller than R9 (or ideally R12). This avoids excessive stick-out and keeps the tool rigid.
Bottom Radius vs. Wall Radius
If the pocket has a floor, the transition between wall and floor also requires a radius if it is to be machined with a ball end mill or a bullnose cutter. If a sharp bottom corner is needed, it may require EDM or a flat end mill with sharp corners, which is extremely difficult. Designers should specify a fillet at the bottom whenever possible (e.g., R1 or R2).
When to Use EDM for Sharp Internal Corners
Some parts absolutely require sharp internal corners (R0.1 or less), such as for sealing surfaces, die cavities, or sharp-edge applications. In these cases, conventional milling cannot achieve the required sharpness. Wire EDM or sinker EDM can produce nearly perfect 90° inside corners, but they add significant cost and lead time. Engineers should only specify sharp corners when functionally necessary, and clearly indicate on the drawing that EDM is required.
How to Communicate Radius Requirements on Drawings
On a 2D drawing, every internal radius should be dimensioned with its value (e.g., R3). If all radii are identical, a single note
