Every machined pocket carries an inside corner radius, and that radius comes straight from the cutting tool. An end mill is a cylinder, so it can only trace a matching arc where two walls meet. If your drawing shows a sharp 90-degree internal corner, the machine physically cannot produce it. This guide explains the geometry, the cost consequences, and the design strategies that keep parts affordable.
Inside corner radius decisions ripple through tool selection, cycle time, and price. Get them wrong and the cost shows up on every single piece. As a result, they belong among the most consequential DFM conversations you can have before machining starts.
Why Every Inside Corner Radius Comes From the Tool
First, picture an end mill cutting a rectangular pocket. The centerline of the tool stays one tool-radius away from each wall. Where two walls meet, the round cross-section leaves a quarter-circle arc in the material. That arc is the inside corner radius, and it equals the tool radius exactly.
Consequently, a 6 mm end mill leaves a 3 mm radius. Getting a 1 mm radius requires switching to a 2 mm tool. The geometry is fixed, and no amount of skill changes it. Only wire EDM or broaching cuts truly sharp internal corners, and both cost far more than milling.
This constraint also explains why drawings and models sometimes disagree at the corners. The drawing states design intent, while the tool decides physical reality. Bull-nose end mills complicate the picture slightly, because their corner edge carries a smaller radius than the tool body. For most pocket work, though, the flat end mill case tells the whole story.
Deep Pockets Demand Small Tools, and Small Tools Cost Money
Unfortunately, the problem compounds with depth. End mills deflect and snap when unsupported length grows too large. A common rule keeps stick-out under four or five tool diameters. Therefore, a 20 mm deep pocket with a 1 mm corner radius needs a 2 mm end mill reaching 20 mm or more. That tool runs slowly, flexes under load, and breaks easily. Long-reach tools exist, but they cost more and still demand gentle parameters.
In practice, small tools force conservative parameters. Spindle speed tops out, feeds drop, and each pass removes little material. Cycle times climb, and broken-tool risk adds scrap risk. Chip evacuation suffers too, because chips pack against the tool in deep, narrow corners. Coolant pressure helps, yet it cannot fully rescue an aggressive depth-to-radius combination.
For these reasons, a tiny inside corner radius in a deep pocket ranks among the most expensive features in CNC milling. That single feature can dictate the entire setup.
The One-Third Rule and Standard Radii
A simple rule prevents most of this trouble. Make the inside corner radius at least one-third of the cavity depth. A 12 mm pocket then accepts a 4 mm radius and a comfortable 8 mm tool. The tool stays stiff, cuts fast, and survives the job.
Of course, depth is not the only variable. A wide, shallow pocket can afford a smaller radius than a deep one. Still, the one-third rule is a safe default when you first sketch the part. When depth and radius conflict, reduce the depth, change the assembly, or accept a slower process. Apply the rule early and the design stays friendly to standard tooling.
Standard sizes matter as well. Shops stock end mills in common diameters, and using one off the shelf avoids delays. Radii like 1, 1.5, 2, 3, 4, 5, 6, and 8 mm map directly to stock tools. Odd values such as 2.7 mm force a special purchase or an extra setup. When you design to standards, the inside corner radius works for you instead of against you.
Dogbone and T-Bone Relief for Press-Fit Corners
Admittedly, some assemblies need a genuinely square corner. Imagine a rectangular plate pressing into a machined pocket. The plate has square corners, but the pocket has round ones, so nothing seats flush. Two classic reliefs solve this.
- Dogbone relief: a small circular pocket extends past the corner, giving the square part somewhere to go. The cutout resembles a dog bone in plan view.
- T-bone relief: the extension runs along one wall only, which saves space and suits thin slots.
Both strategies let the shop keep a large, cheap tool for the main cavity. They also cut machining time versus chasing a tiny radius. Just keep the relief slightly deeper than the mating feature, so debris has room.
Press-fit details like these appear everywhere: fixture plates, electronics enclosures, motor mounts, and frame joints. Deciding on a relief style early keeps drawings clean and avoids surprises at first article. Note the appearance trade-off too, since reliefs leave visible cutouts. For cosmetic faces, weigh whether a rounded mating part preserves the look you want.
Alternatively, round the corners of the mating part so both pieces share the same inside corner radius. That is usually the cheapest option of all.
What a Tiny Inside Corner Radius Costs
For example, consider the same pocket quoted two ways. With a 3 mm radius, the shop roughs with a 10 mm end mill and finishes quickly. At 0.8 mm, though, it must semi-finish and finish with a 1.6 mm tool at a fraction of the feed rate. Machine time can triple, and the thin tool may snap mid-job. Quotes track that risk, so prices rise accordingly. Lead time feels the effect as well, since small tools often must be ordered.
Crucially, the lesson scales across the whole part. Each feature that forces a smaller tool multiplies cost. A part with five deep, tight corners can double the cycle of an otherwise identical part with sensible radii.
Our guide to DFM for outsourced CNC projects covers radius selection alongside other cost drivers. If you are unsure how small to go, send XAP Precision your model for free DFM feedback on your inside corner radius before you release the drawing.
Frequently Asked Questions About Inside Corner Radius
Can CNC milling produce a sharp inside corner?
Not with standard milling. A rotating end mill always leaves an arc equal to its own radius. Truly sharp internal corners require wire EDM or broaching, which add cost. For most designs, accepting the natural inside corner radius or adding a dogbone relief is the smarter path.
How small is too small for an inside corner radius?
As a working rule, keep the radius at least one-third of the cavity depth. Below that, tools get slender, cycle times grow, and breakage risk rises. Radii under 0.5 mm should always trigger a design review with your machine shop before quoting.
Does the inside corner radius affect surface finish or coatings?
Slightly. Sharp internal corners concentrate stress and can show finish variation, while generous radii coat more evenly. More importantly, a radius that allows stable machining produces a better base surface for any finish. Mention critical cosmetic faces during DFM review.
Design Corners That Machine Fast and Stay Cheap
Ultimately, corner decisions made in CAD echo through every quote you receive. Generous, standard radii keep tools stiff, cycles short, and prices low. Well-designed corners are free engineering. XAP Precision reviews inside corner radius, tooling strategy, and tolerances on every drawing we receive, under our ISO 9001 quality system. Send your files through our contact page for a free quote and free DFM feedback.
