How to Remove Burrs From CNC Machined Metal Parts

• 1
  Key takeaways
• 2
  Why burrs form on CNC machined metal parts
• 3
  Which deburring method fits your part
• 4
  Reduce burrs at the cutting stage
• 5
  Edge and surface targets to put on the drawing
• 6
  How to check deburring results
• 7
  Step by step: how to remove burrs from CNC machined parts
• 8
  Deburring methods compared

A burr is metal that deformed instead of shearing. When a cutting edge meets ductile material, the tool tip pushes a small volume of metal ahead of it. That material plastically flows, then fractures or tears at the exit. The result is a raised lip, a rolled edge, or a fine feather along the cut. Softer and more ductile metals burr more. Aluminum 6061, 5052, copper C110, and austenitic stainless such as 304 and 316L are the usual offenders. Hardened steel and cast iron fracture more cleanly, so their burrs tend to be smaller and more brittle.

Burr size follows the cutting parameters. A large edge radius on a worn insert, a shallow depth of cut, and a low feed per tooth all increase the amount of plastic flow. High cutting speed with a sharp, positive-rake tool reduces it. In practice, the worst burrs on a milled part sit on the exit face of the cut, where the tool leaves the material. On a drilled hole, the entry is usually clean and the exit carries a crown of torn metal. Cross-drilled holes burr at both intersections.

Geometry makes it harder. A burr at the outside corner of a plate is easy to reach. A burr at the intersection of a 1 mm cross-hole and a 6 mm bore is not. That difference decides which deburring process you can use, and often whether the part can be deburred at all without a special tool or a process change. Read the drawing for edge callouts before you choose a method. A general note like 'deburr all edges' gives the shop no measurable target.

• 1
  Ductility drives burr size6061-T6, 316L, and C110 burr heavily. 4140 and hardened tool steel burr less.
• 2
  Exit side is worse than entryIn drilling and milling, the exit face carries the largest burr.
• 3
  Worn tools make more burrsReplace or index inserts before the edge radius grows past the feed per tooth.

Hand deburring with a file, scraper, or rotary burr is the default for low volume and for edges a machine cannot reach. It is slow and depends on operator skill. Use it when you have one or two parts, a single critical edge, or a feature that needs a controlled radius. Keep a 10× loupe at the bench and check every edge against the drawing callout. The common error is over-deburring: a few extra strokes take a 0.2 mm edge break down to 0.5 mm and change the fit of a mating part.

Mechanical methods scale better. Vibratory tumbling with ceramic or plastic media handles thousands of small parts per batch and produces a consistent edge break, typically 0.05–0.2 mm. It also deburrs internal passages if the media can reach them. Abrasive flow machining pushes a viscous, abrasive-laden medium through a passage to deburr and polish internal intersections, which is the usual answer for hydraulic and fuel-path parts with cross-drilled holes. Thermal deburring uses a brief, controlled gas explosion inside a chamber to burn off burrs on every exposed surface at once.

For edges that need a defined radius and a fine finish, brush deburring with an abrasive nylon brush on a CNC spindle gives repeatable results. Electrochemical deburring removes material at the edge by anodic dissolution and leaves no mechanical marks, but it needs a tool shaped to the edge and is best for high-volume runs. Pick by three questions: how many parts, how deep is the burr, and can the tool reach the edge without touching a functional surface.

• 1
  One-off or awkward edgeHand tools with a loupe and a defined callout.
• 2
  Thousands of small partsVibratory tumbling, 0.05–0.2 mm edge break, batch consistency.
• 3
  Internal cross-holesAbrasive flow machining or thermal deburring.
• 4
  Defined radius at volumeCNC brush deburring or electrochemical deburring.

The cheapest deburring is the burr you never make. Tool geometry is the first lever. A sharp, positive-rake carbide insert with a small edge hone shears material instead of pushing it. For aluminum, a polished, uncoated or DLC-coated tool with a high helix angle clears chips fast and limits built-up edge. For stainless and titanium, a sharp edge and a light hone matter more than coating. Replace or index the insert when the edge radius grows past roughly half the feed per tooth, or when you hear the cut change pitch.

Parameters matter too. Increase feed per tooth within the tool and finish limits. A deeper cut per tooth reduces the number of passes the edge takes through the same material and reduces rubbing. Climb milling on the finish pass moves the exit burr to the side that is easier to reach. For drilling, use a split-point or pilot hole to reduce the exit crown, and back the exit face with a sacrificial plate or a support bushing when the material is thin. On cross-holes, drill the smaller hole first, then the larger bore, so the intersection burr ends up on the surface the larger tool can clean.

Coolant and chip evacuation are not optional. Recut chips score the finished wall and roll a secondary burr along the edge. High-pressure through-tool coolant on deep holes and cross-holes keeps the intersection clear. On thin-wall parts, reduce the radial engagement on the last pass so the wall does not deflect and tear at the exit.

• 1
  Sharp positive-rake toolingShears instead of pushes. Change the insert before the edge radius grows.
• 2
  Higher feed per toothFewer passes through the same material means less rubbing and smaller burrs.
• 3
  Drill order on cross-holesSmall hole first, then the larger bore to clean the intersection.

'Deburr all edges' is not a measurable requirement. State an edge break or a radius. A 0.2 mm edge break is a common default for general machined parts and removes the sharp feel without changing function. A 0.05 mm radius is a controlled edge for parts that must not have a raised lip, such as a sealing face or a sliding contact. A 0.5 mm radius or larger is a structural feature and should be modeled in CAD, not left to deburring.

Surface finish and deburring interact. If the drawing calls for Ra 0.8–1.6 μm on a bore, the deburring method must not degrade that wall. Abrasive flow and tumbling both remove material from functional surfaces, so protect or mask them, or set the finish callout after deburring. For parts that go to anodizing, the deburr step comes first. Anodizing does not hide a burr, it locks the oxide around it and can make the edge feel sharper.

For threads, a rolled-over crest is the most common complaint. Chase the thread after deburring with a tap or a thread mill, and gauge it. A go/no-go gauge is the only reliable check. On sealing faces and O-ring grooves, a burr or a raised edge will leak. Inspect those edges at 10× and keep a reference part on the bench.

• 1
  0.2 mm edge breakGeneral default for machined edges that must not be sharp.
• 2
  0.05 mm radiusControlled edge for sealing faces and sliding contacts.
• 3
  Model radii above 0.5 mmThat is a design feature, not a deburring task.

Visual check at 10× is the baseline. Look at the exit side of every cross-hole and the intersection of every milled pocket. A clean edge shows a continuous, slightly broken line with no raised lip. A feather or a rolled edge shows as a bright line under the loupe. On anodized parts, inspect before anodizing, because the oxide layer hides small burrs and makes the edge feel sharper than it is.

Measure the edge break where the drawing calls for a radius. A radius gauge or an optical comparator works for external edges. For internal edges, a cast or a silicone replica of the edge lets you measure the profile without cutting the part. On threads, a go/no-go gauge is the only reliable check. On sealing faces, run a light dye-penetrant check if the part is safety-critical.

Keep a reference part. A known-good, deburred part on the bench settles arguments about whether an edge is inside or outside the callout. Update it when the drawing changes. For production runs, check the first part, then sample at a set interval. Document the interval and the method in the inspection plan so the result is repeatable.

• 1
  10× loupe on every exit edgeThe fastest check for feather and rolled-lip burrs.
• 2
  Radius gauge or comparatorFor external edges with a numeric radius callout.
• 3
  Reference part on the benchA known-good deburred sample settles edge disputes.