How to eliminate burrs in CNC milling

• 1
  How burrs form, and why the exiting edge matters
• 2
  Toolpath choices that eliminate burrs in CNC milling at the source
• 3
  Cutting parameters that shrink burr height
• 4
  When to remove burrs instead of preventing them
• 5
  Deburring method vs. part type and edge tolerance

A burr is material that deforms instead of shearing off. During milling, the cutting edge pushes the workpiece ahead of it. Most of that material becomes a chip. A thin layer near the tool nose bends plastically instead, and it stays attached to the part edge. The result is a raised lip along the exit side of the cut.

Burr size depends on ductility, edge sharpness, and how thin the uncut chip gets at the end of the pass. Soft aluminium such as 6061 or 5052 tears rather than breaks cleanly, so it produces a taller, more ragged burr than 4140 steel at the same feed. Work-hardened 304 stainless sits in between. It shears cleanly at first, then rolls a hard lip that is difficult to file off.

The exit geometry decides where the burr lands. When the cutter leaves the part on a free face, the chip thins to zero and a burr is almost guaranteed. When the cutter exits into a chamfer, a pre-cut groove, or another solid face, the chip keeps a finite thickness and breaks off. That single difference explains why the same tool makes a clean edge on one feature and a burr on the next.

Burrs also form on the entry side, though usually smaller. The tool rubs before it bites, especially at low feed per tooth. Rubbing heats the edge, work-hardens it, and leaves a lip that grows with each additional pass. Entry burrs matter on sealing faces and on any hole that will take a dowel pin.

• 1
  Ductile materials burr moreAluminium and soft copper roll a taller lip than hardened steel.
• 2
  Thin chips at exit burrBurr size peaks when the uncut thickness approaches zero.
• 3
  Rubbing creates entry burrsToo low a feed per tooth lets the edge slide instead of cut.

The cheapest burr is the one you never create. Before touching speed and feed, look at how the cutter leaves the material. A climb-cut exit on a 0.5 mm chamfer, a corner radius of at least 0.5 mm, and a lead-out arc that carries the tool away from the wall all reduce burr height. On aluminium, switching from a sharp exit to an arc lead-out can cut burr height by half.

Adding a chamfer or a 0.2 mm × 45° edge break to the drawing is the most reliable fix. The burr still forms, but it forms on the chamfer instead of the functional edge. A follow-up pass with the same tool removes it in the same setup. This works on housings, brackets, and any part where the edge is not a sealing or mating surface.

Order of operations matters too. If you drill or tap after the final profiling pass, the drill exit burr lands on a finished edge. Rough first, then semi-finish, then drill, then finish. The finishing pass cleans up the drilling burr. On parts with many cross-holes, this sequencing saves an entire deburring operation.

For thin walls under 1 mm, the wall itself deflects and the burr grows. Support the wall with a sacrificial rib, or leave 0.3 mm of stock and take it off in a light finishing pass at 0.05 mm depth of cut. The low radial engagement keeps the wall stiff enough that the chip shears instead of bending.

• 1
  Arc lead-out on exitsKeeps chip thickness finite so it breaks instead of rolling.
• 2
  Add a 0.2 mm × 45° edge breakMoves the burr onto a face you can machine away.
• 3
  Rough before drillingFinish cuts then clean up the drill exit burr in the same setup.

Feed per tooth is the strongest lever. Below roughly 0.03 mm per tooth on aluminium, the edge rubs, heat builds, and the burr grows. Pushing to 0.08–0.15 mm per tooth lets the edge bite and shear. The chip thickens at the exit and breaks off with a smaller attached lip. On a 10 mm carbide end mill in 6061, 0.10 mm per tooth at 8,000 rpm is a reasonable starting point.

Spindle speed has a smaller effect than feed, but it changes how much heat reaches the edge. Very high speed on a light feed softens the material at the tool tip and produces a stringy burr. Very low speed with a heavy feed can chip the edge instead, which is worse. Keep surface speed inside the tool maker's range for the material and let feed do the work.

Tool geometry is often overlooked. A sharp edge with a small hone radius, around 5–10 μm, shears cleanly. A worn tool with a 40 μm hone rubs and pushes material sideways. One dull end mill can double burr height across an entire batch. Track tool life by cutting distance, not by the clock, and change before the edge rounds over.

Coolant helps on gummy materials. Flood coolant on 5052 or pure copper keeps the edge cool and flushes chips that would otherwise be re-cut. On cast iron and most steels, dry or minimum-quantity lubrication is fine. Re-cutting an already-cut chip is one of the fastest ways to raise burr height, so chip evacuation matters as much as the numbers.

• 1
  Feed per tooth 0.08–0.15 mmA working range on aluminium with a 10 mm carbide end mill.
• 2
  Keep the hone under 10 μmSharp edges shear; rounded edges push metal sideways.
• 3
  Flush chips on gummy alloysRe-cut chips drive burr height up fast.

Some burrs cannot be designed away. Cross-drilled holes that intersect a bore, slots narrower than 1 mm, and internal edges inside a deep pocket all leave a burr that no toolpath removes. Here the plan shifts from prevention to controlled removal. Decide the removal method before the part is quoted, because it changes the process and the price.

Hand deburring with a file, scraper, or abrasive cord suits one-off parts and prototypes. It is flexible and needs no fixture, but the result depends on the operator. On a 50-piece run, edge radius can vary from 0.05 mm to 0.3 mm between parts. That variation is acceptable on a bracket and not acceptable on a valve seat.

Mechanical deburring scales better. Vibratory tumbling with ceramic media rounds edges evenly and reaches into pockets. Thermal deburring uses a brief, controlled gas ignition to burn away thin burrs in places no tool can reach, which suits hydraulic manifolds and fuel rails. Brush deburring with an abrasive nylon wheel handles edges on a defined path and is easy to automate.

Electrochemical deburring is the precise option. It removes material from the burr because the burr has a higher current density than the bulk surface. Tolerances of ±0.02 mm on edge radius are realistic. It fits medical and aerospace parts where a burr inside a cross-hole would otherwise need manual work. The trade-off is fixturing and cycle time.

• 1
  Hand work: one-offs onlyFlexible but edge radius varies part to part.
• 2
  Thermal deburring: hidden edgesReaches internal intersections no brush can touch.
• 3
  Electrochemical: tightest controlEdge radius held near ±0.02 mm, higher tooling cost.