# CNC Internal Corner Radius: Design Pockets for Real End Mills

Understand why CNC-milled internal corners need radii, how cutter diameter and tool access affect the result, and how to review pocket corners before sending a STEP file for quote.

This guide covers general CAD workflows. CADProps supports STEP, IGES, SolidWorks parts and ZIP assemblies, STL, OBJ, 3MF, static GLB/GLTF, and bounded 2D DWG/DXF preview and measurement. Validated conversions are downloadable. Partial assemblies carry warnings; properties cover loaded geometry only.

A CNC milling cutter is round, so it cannot create a perfectly sharp 90-degree internal corner by ordinary end milling. **Internal pocket corners inherit a radius from the cutter and the toolpath.** If a design requires a sharp internal corner, the manufacturing process has to change, or the part has to use a relief feature such as a dog-bone style clearance where appropriate.

Protolabs' CNC milling guidelines state the core rule plainly: sharp inside corners are radiused as a natural result of CNC machining, and the resulting radius is constrained by the cutting tool. See the [Protolabs CNC milling design guidelines](https://www.protolabs.com/services/cnc-machining/cnc-milling/design-guidelines/).

The useful design question is therefore not “what is the smallest possible radius?” It is **“what radius gives the shop enough tool diameter, reach and stiffness to machine this pocket reliably?”**

## Why a larger corner radius is usually easier to machine

A smaller internal radius generally demands a smaller cutter. A smaller cutter is less stiff, removes less material per pass and may require more toolpath time. If the pocket is deep, the same small tool may also need a long reach, increasing deflection and chatter risk.

That produces a three-way relationship:

- **corner radius** limits the cutter diameter that can enter the corner;
- **pocket depth** affects the tool length required;
- **tool slenderness** affects stiffness, vibration and achievable tolerance.

So a 1 mm corner radius in a shallow aluminum pocket is not the same manufacturing problem as a 1 mm radius at the bottom of a 40 mm-deep steel cavity.

## Do not design the radius exactly equal to the nominal cutter radius

Suppose a pocket corner is specified as R3.0 mm. A 6 mm end mill has a nominal 3 mm radius, but using the largest tool that geometrically just fits can force the tool into heavy engagement in the corner. Shops often prefer some clearance so the cutter is not suddenly buried at the corner transition.

The exact allowance depends on material, machine, toolpath, depth and tolerance. There is no universal percentage that every supplier follows.

A better drawing/RFQ conversation is:

> “R3 is functional only as a maximum? If not, what larger inside radius lets you use a stiffer cutter?”

That question gives the machinist room to optimize the operation instead of treating an arbitrary CAD fillet as sacred.

## Internal radius and external radius are different constraints

An external edge can often be profiled with many tool choices. An internal concave corner is constrained by the cutter's physical radius because the tool center cannot enter the corner beyond the cutter envelope.

This is why a CAD model full of visually sharp rectangular pockets can still be perfectly valid geometry while being inefficient—or impossible—to reproduce literally by 3-axis milling.

When the sharp corner is functionally required because a square mating part must seat inside the pocket, consider alternatives such as:

- adding corner reliefs;
- changing the mating part geometry;
- using EDM, broaching or another process for special cases;
- redesigning the pocket so the sharp corner is not a functional requirement.

The right answer depends on the production process and quantity.

## Review radius together with pocket depth

A useful pre-quote check is to make a small table for the deepest pockets:

| Pocket | Depth | Smallest internal radius | Critical tolerance? | Functional reason |
|---|---:|---:|---|---|
| A | 8 mm | R4 | No | Clearance only |
| B | 25 mm | R2 | Yes | Mating insert |
| C | 40 mm | R1.5 | No | Legacy geometry |

Pocket C should immediately trigger a discussion. The ratio of deep reach to small tool diameter may dominate cost more than the amount of material removed.

## What CADProps can and cannot tell you

CADProps does **not** currently certify pocket manufacturability or automatically recommend an end mill. It should not label a corner “machinable” merely because a radius can be measured.

You can use the [STEP viewer](https://www.cadprops.com/tools/step-viewer/index.md) and [dimensions tool](https://www.cadprops.com/tools/cad-dimensions/index.md) to inspect the geometry, verify units and check relevant dimensions. Treat that as evidence gathering for a DFM review, not as an automated process plan.

The same caution applies to the current feature-recognition workflow: simple cylindrical through holes and flat-bottom blind holes can be classified in bounded cases, but pocket recognition is not a general CADProps capability today.

## A practical design review before RFQ

For each machined pocket:

1. identify the smallest internal corner radius;
2. record the pocket depth;
3. ask whether that radius is functional or merely inherited from the CAD model;
4. check whether a mating square component actually requires relief;
5. identify any tight positional or profile tolerance near the corner;
6. let the supplier choose the cutter where the design allows it.

If the radius is not functional, increasing it can improve tool stiffness and reduce machining time. If it is functional, state why so the shop can evaluate the correct process rather than silently approximating the corner.

## Do not hide the requirement in the STEP model

A STEP file can communicate the nominal geometry, but it does not automatically tell the supplier which radius is negotiable. If an internal corner is functionally critical, put that intent in the drawing, PMI or RFQ notes.

The [CNC quote preparation guide](https://www.cadprops.com/guides/prepare-step-file-for-cnc-quote/index.md) covers the broader handoff: revision, material, quantity, tolerances, finish, threads and inspection requirements.

The engineering rule is simple: **model internal corners with the manufacturing process in mind, and give the cutter more room when the function allows it.** That is usually more valuable than chasing the smallest radius a catalog says might be possible.

## Related reading

- [Autodesk Fusion AutoTimeline: Why CAD Feature Recognition Matters Again](https://www.cadprops.com/guides/autodesk-fusion-autotimeline-feature-recognition/index.md)
- [Minimum Wall Thickness for CNC Machining: No Single Safe Number](https://www.cadprops.com/guides/cnc-minimum-wall-thickness/index.md)
- [Deep Hole Drilling: Use Depth-to-Diameter Ratio Before You Quote](https://www.cadprops.com/guides/deep-hole-drilling-depth-to-diameter-ratio/index.md)
- [Prepare a STEP File for a CNC Quote: A Shop-Ready RFQ Checklist](https://www.cadprops.com/guides/prepare-step-file-for-cnc-quote/index.md)
- [STEP Hole Recognition: Detect Through and Blind Holes](https://www.cadprops.com/guides/step-hole-recognition/index.md)

Original article: https://www.cadprops.com/guides/cnc-internal-corner-radius/

HTML page: https://www.cadprops.com/guides/cnc-internal-corner-radius/