How Internal Corner Radius Affects CNC Cost

A Sharp Internal Corner Is Not Possible
CNC milling cuts with a rotating cylindrical tool. With the path of a cylindrical tool, a radius equal to the tool radius always remains in an internal corner.
Even if the drawing shows a right angle, the result has a radius. If you do not specify the radius, the shop decides it arbitrarily. If assembly interference is expected, always state it.
By contrast, external corners can be made sharp. The tool cuts while moving off the outside. The constraint exists only on the inside.
How Reducing the Radius Affects Cost
A small radius requires a small-diameter tool. A small-diameter tool brings the following constraints.
- Reduced cutting conditions: depth of cut and feed must be lowered to prevent breakage. Removing the same volume takes longer
- Tool breakage: it incurs changeover time and tool cost. If a broken carbide fragment remains in the part, even the stock is scrapped
- Added operations: rest machining is needed, where a large tool removes most of the material and a small tool machines only the corners separately. Setups increase
In other words, a single radius governs the entire machining time. Tool diameter, not shape complexity, determines cost.
Engagement Angle Spikes at Corners
On straight sections, only part of the tool's side contacts the material. The moment it enters a corner, the engagement angle (the radial contact angle) spikes.
As the engagement angle grows, chip thickness and cutting force rise together and the tool deflects. As a result, chatter, sidewall taper, abnormal noise, and tool breakage can occur. For this reason, feed must be reduced at corners.
Conditions are worst when the radius equals the tool radius. The tool effectively stops at the corner, changes direction by 90°, and re-accelerates, and the engagement angle is at its maximum in that section.
Make the Radius Larger Than the Tool Radius
If there is room for the tool to sweep around the corner, it can pass without slowing down. The recommended multiple is given as 1.1 to 1.3 times the tool radius depending on the vendor, with no single standard value. The point is not to set it equal to the tool radius.
Rule of Thumb Based on Depth
The commonly used industry rules of thumb are as follows.
- Specify the corner radius at 1/3 of the cavity depth or more
- Keep the cavity depth within 2 to 3 times the tool diameter
For example, for a cavity 12mm deep, set the corner radius to 5mm or more so that high-speed machining with a φ8 tool is possible.
However, this is a recommended rule of thumb, not an engineering derivation. It varies with material and tool rigidity.
Depth and Radius Are Linked
A deep pocket requires a long tool, and for a long tool to be rigid, its diameter must be large. A large-diameter tool can produce only a large radius.
As a result, a shape that is "deep with a small corner radius" is the most unfavorable.
| Shape condition | Difficulty | Reason |
|---|---|---|
| Shallow, large radius | Low | Large-diameter, short tool |
| Shallow, small radius | Moderate | Small diameter but short, so rigidity is secured |
| Deep, large radius | Moderate | Large diameter, so rigidity is secured |
| Deep, small radius | High | Small-diameter, long tool. Deflection and breakage |
Drawing Guidelines
- Apply the largest acceptable radius. Not the minimum. If R 3 is acceptable functionally, write R 3
- Increase the radius for deeper pockets. The key is to avoid the bottom condition in the table above
- Unify the radius. If radii differ within a part, tool changes repeat. With a uniform radius, a single tool handles it
- Consider the bottom radius too. A radius may also be needed where the pocket floor meets the sidewall (ball end mill or corner radius end mill)
- If a sharp corner is functionally essential: milling cannot produce it. Consider wire EDM or a corner relief
Corner Relief
In most cases where the internal radius is a problem, the cause is interference from the mating part's sharp edge.
In that case, instead of reducing the radius, machine a relief groove into the corner.
- Dog-bone: adds circular reliefs at the corner in two directions (offset 45° and 135° by the tool radius)
- T-bone: adds a relief in one direction only
With the inside of the corner locally cut away, the mating part's edge enters that space. It looks out of place, but it is advantageous in both cost and certainty. It is an alternative worth considering actively if the surface is not exposed.
Frequently Asked Questions
What happens if I don't specify the radius?
It is decided based on the shop's standard tools. It is usually not a problem, but if there is assembly interference it is discovered then. Specify it if it is a functional surface.
Is R 0.5 possible?
It requires a φ1 end mill. It is possible for shallow shapes, but for deep ones the cost spikes or it cannot be made. Depth must be given together to judge.
How much does cost drop if I increase the radius?
It depends on the shape. The reduction is large when the entire small-diameter tool operation is eliminated.
Summary
- An internal sharp corner is impossible given the tool geometry
- A small radius leads to small-diameter tool → reduced cutting conditions → higher cost
- Make the radius larger than the tool radius (1.1 to 1.3 times recommended by vendors). If equal, the engagement angle is at its maximum
- Rule of thumb: corner radius ≥ 1/3 of cavity depth, cavity depth ≤ 2 to 3 times tool diameter
- If assembly interference is the reason, a dog-bone or T-bone relief is the alternative
Corner radius is not a shape feature but a cost variable. Upload your drawing and you can see which corners determine cost.
Have a part to machine?
Upload a drawing to see your quote.



