Internal corner radii for CNC pockets

End mills are round. Every inside corner of a milled pocket keeps at least the radius of the cutter, so the radius you draw decides which tool the shop must use and how fast it can cut.

The rule of thumb

Make vertical inside corner radii at least one third of the pocket depth. A 12 mm deep pocket gets R4 or larger, which lets the shop use an 8 mm or smaller cutter that is stiff enough to cut the full depth at normal speed.

Make the radius slightly larger than a standard cutter radius, for example R3.2 instead of R3. When the radius equals the cutter exactly, the tool wraps around the corner with full engagement, chatters and leaves marks. A slightly bigger radius lets it sweep the corner smoothly.

What small radii cost

A tool can reach about 3–4 times its diameter deep before it starts to bend and chatter. A R1 corner in a 20 mm deep pocket needs a 2 mm cutter reaching 10 diameters deep. That tool must run very slowly, takes many shallow passes and breaks easily. The corner alone can double the cycle time of a pocket.

When a square part must fit

If a square component must sit in the pocket, do not ask for sharp corners. Add a dog-bone or T-bone relief: a small round cut-out at each corner, extending past the corner, so the square edge clears the radius. It is quick to mill and costs almost nothing. Truly sharp corners need wire or sinker EDM, which adds a separate process and a lot of cost.

Floor radii

The radius between the pocket wall and the floor is a different matter. A flat end mill makes a sharp floor corner for free. A rounded floor needs a ball or bull-nose cutter and extra passes. Only specify floor radii where they are needed for strength or cleaning.