Burrs are the defect you will always get, so specify what you will accept
Deburring CNC parts is the removal of the raised ridge of material left at every edge where a tool cuts, shears or drills. It is not a finishing nicety. A burr is sharp, it is loose enough to break off inside an assembly, it stops parts from seating on a datum, it makes a plating bath deposit unevenly, and it is the single most common cause of "the parts are fine except" conversations between a buyer and a machine shop.
On medical parts the deburring method decides how much debris the cleaning line has to remove, which is why we sequence it as the first cleaning step: cleanliness and contamination control for machined medical parts.
The awkward truth is that burrs cannot be eliminated at source. Any cutting process produces some edge condition — the only question is how big it is, which way it points, and what you are going to do about it. This guide covers where burrs come from, the deburring methods in common use and what each one is good for, how to specify an edge on a drawing, and how deburring shows up in a quote.
Where burrs come from
Different processes leave different edges, and knowing which is which tells you which deburring method will work.
Kerf width, assist gas and the cut tolerances worth specifying are all covered in our sheet metal laser cutting guide.
| Process | Typical burr | Why |
|---|---|---|
| Milling, exit side | Roll-over burr along the edge of a milled slot or face | Material pushes ahead of the cutter instead of shearing |
| Milling, entry side | Small, usually negligible | Edge is supported as the cutter enters |
| Drilling, breakthrough | Crown burr around the exit of a hole | The drill pushes a cap of material out |
| Turning, parting off | Burr on the cut-off face | Supports the part at the moment of separation |
| Tapping | Feathered edge at the thread entry | Thread form is raised rather than sheared |
| Blanking and piercing | Shear burr on the die side, rollover on the punch side | Clearance between punch and die |
| Laser cutting | Hard re-solidified dross on the underside | Melt not fully ejected |
Two material properties dominate burr size. Ductile materials — soft aluminium, low-carbon steel, copper — tear rather than shear and produce large, stringy burrs. Brittle or hard materials — cast iron, hardened steel, some stainless grades — produce small, brittle burrs that break away but may leave a sharp edge behind.
The practical consequence: a deburring process tuned for 6061 aluminium will not necessarily work on 304 stainless, and a specification written for one will be wrong for the other.
How to specify an edge on a drawing
"Deburr and break all edges" is the most common note on engineering drawings and one of the least useful, because it is not measurable. Nobody can inspect against it.
Better options, in order of how precise they are:
- A maximum burr height in millimetres, with the permitted side stated. "Burr 0.05 max, on the non-mating face" is inspectable.
- An edge break dimension:
0.2 × 45°means remove material to produce a chamfer 0.2 mm across. This is measurable with a gauge or a microscope. - A maximum edge radius:
R0.1 maxfor a part where a rounded edge is acceptable and a chamfer is not. - A standard reference: ISO 13715 defines edge designation for workpiece edges — inside/outside edges, plus or minus material, and the edge size. It is the right vocabulary when the edge genuinely matters.
The most useful sentence a drawing can carry is the one that says which edges do *not* need work. A part with 200 edges and four that matter costs a fraction of the same part with "all edges" written on it — and the un-deburred 196 edges will never cause a problem. This is the same argument as tolerancing: name the characteristics that matter, and put the rest under a general note. Our tolerance guide covers the underlying principle.
Watch one trap: deburring changes dimensions. An edge break of 0.2 mm removes 0.2 mm of material from a feature. On a bore that is close to its lower limit, or a slot width that is already at minimum, deburring can push a part out of tolerance. Say where the edge break is not permitted.
The deburring methods, and what each is for
There is no universal method. Each one trades coverage, edge quality, cost and risk.
| Method | What it does | Best for | Watch out for |
|---|---|---|---|
| Hand deburring | File, abrasive pad, scraper, hand tool | Prototypes, one-offs, large parts, inaccessible edges | Inconsistent; operator-dependent; slow at volume |
| Vibratory tumbling | Parts tumble in media, abrasive action on all edges | Small parts, high volume, uniform radiused edge | Media lodging in holes and threads; rounded edges; surface dulling |
| Centrifugal / high-energy | Faster version of tumbling, higher force | Harder materials, shorter cycles | More aggressive; more dimensional change |
| Abrasive blasting | Media propelled at the surface | Large parts, uniform matte finish | Rounds edges unevenly; embeds media in soft alloys |
| Thermal deburring | Controlled combustion burns off the burr | Internal passages, cross-holes, hard-to-reach burrs | Leaves a thin oxide; not for tight-tolerance features |
| Electrochemical | Anodic dissolution removes burr metal | Precision parts, no mechanical contact, no stress | Conductive materials only; handling of electrolyte |
| Abrasive flow | Abrasive media extruded through passages | Internal edges, manifolds, medical components | Slow; fixture-dependent |
| Brushing, automated | Rotary brushes on a fixed head | Sheet and flat parts, consistent edge break | Directional finish; not for internal features |
| Machined chamfer | The CNC machine cuts the chamfer | Parts where the edge must be exact | Adds cycle time; needs a tool path |
Two rules of thumb cover most programmes. If the part is small, high volume and not cosmetically critical, tumbling is almost always the cheapest route to a consistent edge. If the part has threads, blind holes or a critical sealing face, tumbling is a risk and a machined chamfer or hand work is safer.
The machined chamfer is worth a special mention because it is the most under-used option. If a part is already on a CNC mill or a turning centre, adding a chamfer tool path costs seconds and produces an identical edge on every part. On five-axis parts with compound edges, it is often the only method that reaches every edge at all.
Deburring and surface finish: the interactions
Deburring is not the last word on surface condition; it changes what comes after.
Anodising and plating. A burr concentrates current in a plating bath and concentrates heat in an anodising bath, so burrs produce rough, burnt or uneven deposits on the edge. Deburr before coating, not after. See our anodising guide for how edge condition affects colour consistency.
Surface roughness. Tumbling and blasting change the roughness value of the faces they touch, not just the edges. If a drawing specifies Ra 1.6 on a face, confirm that the deburring method will not take it to Ra 3.2. Our surface roughness guide sets out how Ra, Rz and lay direction should be specified.
Cleanliness. Media, abrasive dust and blasting grit lodge in blind holes, threads and undercuts. A part that is deburred and then assembled without cleaning carries grit into the assembly. Medical and food-contact work usually requires a documented cleaning step after deburring — see medical device machining.
Marking. Sharp edges and laser-marked IDs interact: a burr across a laser-marked serial number reduces legibility, so deburr before marking.
What deburring costs and how to keep it down
Deburring is labour or machine time, and on complex parts it can be a larger line item than the machining. In our experience the cost splits roughly three ways: most of it is manual handling — loading, unloading, masking, inspection — and only a minority is the actual material removal.
Five things keep it down, and four of them are decided before the part is made:
- Specify only the edges that need it. The single largest saving available on almost every part.
- Let the machine do it. A chamfer in the tool path beats a second operation every time.
- Design out inaccessible edges. Cross-drilled holes and deep internal corners cannot be reached by tumbling or brushing and force hand work. A DFM review before the drawing freezes catches these.
- Choose a material that burrs less. Where the design allows, a free-machining grade or a harder temper produces a smaller burr than a soft, ductile one. Our materials guide notes which grades behave better.
- Batch it. Deburring setup is fixed cost. One batch of 200 costs far less per part than four batches of 50.
On stamped parts, burr control is a tooling maintenance problem rather than a finishing one: burr height grows with punch wear, so a progressive die programme should specify a burr limit and a regrind interval together. Our stamping overview covers where that line sits.
A short specification checklist
- Burr height limit in millimetres, and which side it is allowed on — or an edge break dimension.
- Which edges are excluded from deburring, especially sealing faces and close-tolerance features.
- Any prohibition on media contact: threads, bores, sealing faces, optical surfaces.
- Whether the deburring method may change the surface roughness of named faces.
- Cleaning and drying requirement after deburring, if the part is going into a clean assembly.
- Whether deburring happens before or after coating and marking.
Six lines on a drawing, and the whole subject stops being a dispute. If you are at the quotation stage and want a second opinion on which edges actually need work, send the drawing with the intended annual volume — a DFM review comes back with the quote, and we quote within 24 hours.
FAQ
What CNC machining services does Ruijin CNC offer?
Ruijin CNC provides CNC turning, CNC milling (3-axis and 4-axis), 5-axis CNC machining, sheet metal fabrication, metal stamping, and surface treatment including anodizing, plating and powder coating.
What tolerances and certifications does Ruijin CNC hold?
We hold tight tolerances down to ±0.01mm across all processes, and are certified to IATF 16949, ISO 9001 and ISO 13485.
What is the minimum order quantity and lead time?
We accept prototypes from 1 piece with no strict MOQ, provide free DFM review, and return a quote within 24 hours of receiving your CAD drawing and requirements.
How do I get a quote from Ruijin CNC?
Send your STEP file and drawing to gongtianbao@xhlmarketing.com or via WhatsApp +86 17620300785. We reply with a DFM review and a firm quote within 24 hours.
How do you deburr flame cut parts?
A flame cut edge (oxygen-fuel or plasma) carries a hard, rounded dross layer that behaves differently from a machining burr: it is thicker, the heat has changed its metallurgy, and it can be harder than the base metal. We remove it by grinding or abrasive belt work first, then finish the edge with fine abrasive or media tumbling depending on the cosmetic requirement, and we quote the edge break as a dimension rather than a note so the result is measurable. Tell us at quote stage if the part will be welded or powder coated, because those two processes need different edge conditions.