Every inside corner on a milled part starts with the same question the drawing never asks: what radius is the tool leaving in there? A rotating cutter is a circle, and a circle cannot fill the last fraction of a square corner — the inside corner of any milled pocket or shoulder will always carry the radius of the tool that cut it. The drawing says "sharp corner," the CAM says "the smallest cutter is 3 mm," and somewhere in between a decision gets made that decides whether the part is cheap or expensive, whether it fits a mating part or does not. This is what actually happens at the corner, how the tool radius becomes your minimum feature size, and how to design and machine parts so the corners are not where the project stalls.
The tool is a circle, and the corner is the radius that circle leaves
The physical limit at work here is simple and absolute. An end mill is a rotating cylinder, so in plan view it is a circle. When that circle sweeps into an inside corner of a pocket or a step, the material it cannot reach is exactly the shape of the corner minus the shape of the circle. The leftover is not a sharp corner; it is a fillet whose radius equals the radius of the cutter. A 6 mm end mill leaves a 3 mm inside corner radius. A 12 mm end mill leaves a 6 mm corner radius. No amount of programming, no clever toolpath, and no post-processor setting will make that corner sharper — the geometry of the rotating tool sets a hard floor on the smallest inside radius a given cutter can produce.
That floor is the single most useful number to know about a milled part, because it connects the drawing directly to the cost. Every reduction in the required inside corner radius forces the use of a smaller tool. A smaller tool is weaker, spins faster, feeds slower, and — critically — reaches less deep before it starts to flex and chatter. A corner radius of 3 mm can be cut with a stout 6 mm tool that feeds hard and clears chips fast. A corner radius of 1.5 mm needs a 3 mm tool that has to be babied. A corner radius of 0.5 mm needs a 1 mm tool that is slow, fragile, and limited to shallow depths. The tighter the corner, the more the whole pocket slows down to accommodate it, and that slowdown is where the money goes.
It is worth stating the one asymmetry most designers miss: the limit applies to inside corners, not outside corners. An outside corner — the corner on the edge of a boss or a tab — can be left genuinely sharp, because the tool passes around the outside of the material and nothing stops it from turning the corner. The inside corner is the only place the tool's own diameter fights you. When a drawing calls out a radius, knowing whether that radius sits on the inside of a pocket or the outside of a feature tells you immediately whether it is a cost driver or a free detail.
Inside corner radius is your minimum feature size
Once you see the corner radius as a hard limit, it becomes the ruler for the rest of the part. Any pocket, slot, or internal step has a smallest inside corner, and that corner dictates the largest tool that can rough the entire cavity, which dictates the cycle time, which dictates the price. This is why a smart designer sets the corner radius to the largest value the function will tolerate, rather than the smallest, and why a machinist reading a drawing goes straight to the smallest inside radius first — it is the number that tells them how hard the whole job will be.
The practical rule is to match the corner radius to a standard tool diameter wherever possible. A radius of 3.175 mm, for example, matches a 1/4-inch tool exactly; a 3 mm radius matches a 6 mm tool; a 1.5 mm radius matches a 3 mm tool. When the corner radius is a little bigger than half a standard tool diameter, the tool can cut the corner in a single clean pass instead of having to slow down and nibble at it, and the pocket stays fast. When the radius is an odd, arbitrary value, the shop either uses the next smaller standard tool and eats the slowdown, or grinds a custom tool, which adds cost and lead time for no functional reason.
There is also a structural reason to open the radius up. Sharp inside corners concentrate stress — the tighter the fillet, the higher the stress concentration at the root, and the more likely a crack starts there under load. A generous corner radius is not just easier to machine; it makes the part stronger. When a part cracks, the crack almost always starts at a sharp inside corner, so a designer who rounds the corners to a machinable value is usually improving fatigue life and manufacturability in the same stroke.
| Corner radius | Tool diameter | Typical use | Cost effect |
|---|---|---|---|
| 6 mm or larger | 12 mm+ | Large pockets, housings | Fast, rigid, cheap |
| 3 mm | 6 mm | Standard pockets, brackets | Normal speed and cost |
| 1.5 mm | 3 mm | Compact parts, fine detail | Slower, lighter cuts |
| 0.5 mm | 1 mm | Micro features, shallow only | Slow, fragile, shallow |
What a sharp corner actually costs, in time and in risk
When a part genuinely needs a sharp inside corner — a mating face that must sit flush against another part, a seal that cannot tolerate a gap — the cost shows up in two places: cycle time and failure risk. The cycle-time cost is straightforward. To cut a sharp corner, the tool has to be small enough to get into the point, and a small tool feeds slowly. Worse, the corner is exactly where a tool loads up — as the cutter rounds the corner, its engagement with the material spikes, because the same tool suddenly has material on two sides of it instead of one. That engagement spike is where tools snap, where the finish tears, and where chatter starts.
The standard fixes for a true sharp corner each carry their own trade-off. The first is to drill the corner out with a small drill before milling, which leaves a round relief hole at the corner — but that only works if the design can tolerate a drilled relief. The second is to cut the corner with a smaller tool, accepting the slowdown. The third, and the one that usually wins for a mating part, is to change the design so the corner does not have to be sharp at all — add a clearance radius on the mating part, or put the sharp corner on the outside feature instead of the inside pocket. The right answer depends on which face actually matters, and it is almost always cheaper to move the sharp corner than to machine it.
The failure risk is the part most people forget. A sharp inside corner is a stress riser, and a machined sharp corner is also a weak, thin sliver of material that burrs easily and chips under anodizing or handling. The corner that looks clean on a CAD screen can come off the machine with a ragged burr, and the deburring pass that fixes the burr can round the corner you were trying to keep sharp. Holding a true, clean sharp corner is a finishing problem as much as a machining problem, which is why it should be designed out wherever the function allows.
The dog-bone corner and other ways to keep the corner sharp on paper
When two machined parts have to mate in a pocket, the classic trick is the dog-bone, or corner relief, and it is worth understanding because it lets you have a sharp-looking corner without paying for a sharp-machined corner. The idea is that the pocket is drawn with a round cutout punched into each inside corner — the cutout is wider than the tool, so the tool can sweep through the corner and clear it completely, while the flat walls around the cutout still locate the mating part. The mating part's sharp corner then sits inside the round relief and touches the flat walls, not the radius, so the fit is just as tight as if the corner were truly sharp.
The dog-bone costs almost nothing — it is cut with the same tool that clears the pocket, so it adds no tool change and no slowdown — and it eliminates both the engagement spike and the stress riser at the corner. The only requirement is that the relief must not interfere with whatever seals, sits, or fastens in the pocket. When it does not, the dog-bone is the single cheapest way to turn a "sharp corner" drawing into a part that mills clean, and it is the first thing to reach for on any pocket that mates with another part.
A related option is the standard corner radius on the pocket with a matching radius or chamfer on the mating part, so the two radii nest instead of fighting. This is the same principle — let the corner be round, and make the mating feature round too — and it has the added benefit that a chamfered or radiused corner on a mating part is also easier to deburr and less likely to catch or chip. The through-line of all these tricks is the same: do not fight the tool's circle, design around it.
Machining a corner cleanly, once the design is settled
Even with a sensible corner radius, the corner is still where the tool is most likely to misbehave, and there are a handful of things the machinist does to keep it clean. The first is to clear the corner with a smaller finishing tool after the big rougher has removed the bulk, so the finishing pass sees a light, even load instead of a sudden engagement spike. The second is to slow the feed as the tool enters and leaves the corner — many controls do this automatically — because the corner is where the engagement jumps, and a lighter feed through the corner keeps the tool from loading up and snapping.
The third is to watch the finish, because the corner is where the surface first shows tear-out, chatter marks, or a burr. A corner that chatters is usually a rigidity problem — the tool is hanging too far out for the radius it is cutting — and the fix is a shorter tool, a bigger corner radius, or a slower pass, not a faster one. The fourth is to plan the deburring, because the inside corner burr is the hardest to reach, and a part that specifies a sharp corner needs a deburring method that will not round it. A quick pass with a hand tool can do more damage to the corner than the machining did.
The last thing is to check the actual radius, not assume it. The corner radius a tool leaves is not always exactly half the nominal tool diameter — the tool wears, the corner rounds slightly, and the machine's path in and out of the corner can blend it. On a part with a critical mating corner, the radius gets inspected with a pin gage or a radius gage, because the difference between a clean 3 mm radius and a worn, blended 3.3 mm radius is the difference between a part that nests and one that does not. The corner is small, but it is where a lot of parts earn their tolerance.
- Know the floor — the smallest inside radius equals the cutter radius; a 6 mm tool leaves a 3 mm corner.
- Design to a standard tool — pick corner radii that match standard diameters so the pocket stays fast.
- Bigger radius, stronger part — sharp inside corners concentrate stress and start cracks.
- Inside corners cost, outside corners don't — only the inside corner fights the tool's circle.
- Use a dog-bone relief — a corner cutout lets a mating part sit sharp without sharp machining.
- Move the sharp corner — put it on the outside feature or the mating part when the design allows.
- Finish the corner light — clear it with a smaller finishing tool after the roughing pass.
- Ease the feed through the corner — engagement spikes at the corner; slow down to avoid loading up.
- Plan the deburr — inside corner burrs are the hardest to reach and the easiest to round over.
- Inspect the radius — a worn or blended corner is a fit problem, so gage the critical ones.
"A machined corner is never truly square, and the sooner the drawing accepts that, the cheaper the part gets. The tool is a circle, so the inside corner will always carry the radius of that circle — the only real question is whether you set that radius deliberately to match a standard tool, or let it be whatever the shop's smallest cutter happens to be. Every sharp corner on a drawing is a silent instruction to use a smaller, slower, weaker tool, and most of the time it is an instruction nobody meant to give. Round the corner to a machinable value, add a dog-bone where two parts mate, and the corner stops being the most expensive line on the print and becomes the part that mills clean the first time."
The corner is where the part's geometry meets the tool's, and the meeting is not negotiable — a rotating cutter leaves its radius behind. Design the radius to match a standard tool, use a dog-bone where parts mate, and machine the corner light, and what looked like a hard limit turns into a routine detail. What looked like a free "sharp corner" on the print was actually the most expensive feature on the part, and the fix costs nothing but a line on the drawing.
If your drawing is full of sharp corners that are fighting the tools, send it over and we will flag the radii that drive your cost and show you the dog-bone or radius changes that get the same fit for less. See how we handle corner radii and pocket geometry in multi-axis milling and tight internal geometry in a single setup, or get a quote on your machined parts.