How to Manage Burrs After Machining: 5 Proven Steps

• 1
  Key takeaways
• 2
  What creates the burr when you manage burrs after machining
• 3
  Cutting parameters that reduce burrs after machining
• 4
  Tool and edge geometry choices that help manage burrs after machining
• 5
  Removal methods and when each one fits
• 6
  How to manage burrs after machining in 6 steps
• 7
  Deburring methods compared

A burr is material that plastically deformed instead of shearing off. At the exit face of a cut, the remaining wall is thin, so the tool pushes it sideways rather than cutting it. The softer the material and the thinner the remaining section, the larger the burr. Aluminum 6061 and 5052 tear badly; 7075 and 17-4PH fracture more cleanly.

Four variables drive most of what you see. Tool edge radius, feed per tooth, depth of cut at the exit, and how much material is left beyond the cut. A sharp tool with a small edge radius shears; a worn tool with a 40 μm edge radius rubs and rolls material over the edge.

Coolant matters more than people expect. Without flood or high-pressure coolant, chips weld to the edge and drag material along the face. In steel and stainless, chip welding adds a secondary burr layer on top of the primary one.

Burr size is also a geometry problem. A cross-hole drilled into a curved surface exits at an angle, so the wall thickness varies around the circumference. The thin side produces a tall, thin burr; the thick side produces almost none.

• 1
  Ductile materials burr moreAluminum, copper and low-carbon steel deform before they break.
• 2
  Worn tool, bigger burrEdge radius above roughly 30 μm turns cutting into plowing.
• 3
  Thin exit wall, tall burrBelow about 0.5 mm remaining wall, expect heavy rollover.

Feed per tooth is the strongest lever you control at the machine. In aluminum 6061, dropping from 0.15 mm/tooth to 0.08 mm/tooth on the finishing pass typically cuts burr height by a third. Going too low backfires: below roughly 0.03 mm/tooth the edge rubs and the burr grows again.

Depth of cut at the exit changes the failure mode. Taking a heavy final pass leaves a thick, hard burr that is difficult to remove. A 0.2–0.3 mm finishing pass on the exit face produces a thin, brittle burr that breaks off during tumbling.

Cutting speed has a smaller effect, but it is not zero. In stainless 304, too low a surface speed builds a built-up edge that smears material across the exit. Keep the speed in the range recommended for the insert grade and the burr stays predictable.

On 5-axis work, the tool exit angle is a parameter too. Exiting at an angle rather than perpendicular spreads the deformation over more edge length and lowers peak burr height. The trade-off is a slightly longer cycle time.

• 1
  Finishing feed0.05–0.10 mm/tooth in aluminum; 0.03–0.06 mm/tooth in steel.
• 2
  Exit pass depth0.2–0.3 mm leaves a burr that breaks off cleanly.
• 3
  Avoid the rub zoneBelow about 0.03 mm/tooth, burr height rises again.

A positive rake angle cuts rather than pushes. In aluminum, a 12–15° positive rake with a polished flute reduces the exit burr noticeably compared with a neutral insert. In hardened steel above 45 HRC, a negative rake is stronger but produces a heavier burr, so plan for a deburring step instead.

Corner radius matters at internal edges. A tool with a 0.4 mm corner radius leaves a smaller fillet than one with a 1.2 mm radius, but the smaller radius concentrates stress and wears faster. Match the radius to the number of parts you intend to run.

Chamfering the exit edge on the drawing is the cheapest fix of all. A 0.3 mm × 45° chamfer on the far side of a cross-hole moves the burr off the functional surface. The chamfer can be added in the same setup with a chamfer mill.

For bores, a reamer with a slight back taper and a honed edge produces far less burr than a standard twist drill. If the bore is a seal surface, ream after drilling and skip the drill's exit burr entirely.

• 1
  Positive rake for aluminum12–15° with polished flutes reduces rollover.

Hand deburring with a scraper or a rotary file gives the most control and works on any geometry. It is also the most variable. Two operators produce two different edge conditions, so reserve hand work for prototypes and low volumes where the edge is critical.

Mechanical tumbling, including vibratory and barrel finishing, removes burrs from every edge at once. It cannot reach deep bores or blind cross-holes, and it rounds sharp corners in the process. If the drawing calls for a sharp edge, tumbling is the wrong choice.

Thermal energy method (TEM) burns the burr off in a gas mixture. It reaches internal passages that no tool can touch and leaves no mechanical marks. It only works on burrs thin enough to oxidize, typically under about 0.1 mm, and it slightly alters the surface chemistry.

Electrochemical deburring removes material at the burr because the burr's high current density concentrates the reaction there. It is precise, but the electrolyte must be compatible with the material and the setup cost is high. For a 10,000-piece run with tight edge specs, it pays back.

• 1
  Hand workBest for prototypes and awkward geometry; hardest to repeat.
• 2
  TumblingFast and cheap; rounds every corner it touches.
• 3
  TEMReaches internal passages; only for thin burrs under about 0.1 mm.