CNC Edge Cutting Technology: How an Edge Gets Its Final Geometry

• 1
  Key takeaways
• 2
  What actually happens at the cutting zone
• 3
  Tool geometry sets the smallest edge you can hold
• 4
  Why 5-axis changes what an edge can be
• 5
  How the alloy decides the method
• 6
  Deburring, polishing, and what they change
• 7
  Edge cutting method by feature and volume

Every edge starts as a stress concentration. The sharper the corner, the higher the local stress when the part is loaded. Cutting technology exists to replace that sharp corner with a defined geometry: a chamfer, a radius, a relief, or a controlled burr-free break. The tool does not simply remove metal at the edge. It reshapes the load path through the part.

Material removal at an edge differs from bulk milling. The tool is often cutting with only part of its diameter engaged, which changes chip thickness along the contact arc. On a chamfer pass, the effective engagement width shrinks to a fraction of the axial depth. Feed rates that work in the middle of a pocket will chatter at the rim. We usually drop feed by 20–30% on the final profile pass and keep the stepover under 0.5 mm for a clean break.

Heat is the second variable. At a thin edge, there is less material to conduct heat away, so the local temperature climbs faster than in the body of the part. Titanium and 17-4PH stainless show this clearly: the edge can discolor or work-harden while the rest of the part stays cool. Air blast or through-spindle coolant matters more here than on a flat face. The edge is where the process is least forgiving.

• 1
  Engagement drops at the rimLess radial contact means a different chip load than the pocket floor.
• 2
  Thin sections heat fasterCoolant strategy matters more at an edge than in the body.
• 3
  Work hardening is localTi-6Al-4V and 17-4PH harden at the cut, not across the part.

The corner radius on the drawing must exist on the tool first. A 0.4 mm edge break needs a tool that can reach into that corner without rubbing. For internal profiles, the tool shank diameter has to clear the wall, and the flute length has to reach the depth without deflection. Deflection of 0.01 mm at the tool tip becomes a visible taper on a 40 mm deep edge.

Coating selection follows the material. AlTiN holds up in dry cutting of steels and stainless. DLC reduces built-up edge on aluminium and copper alloys. For aluminium 6061 and 7075, a polished uncoated carbide with high helix works better than a coated tool because the coating itself can drag on the soft material. We keep separate tool sets for aluminium and steel to avoid cross-contamination of chips.

Runout is the quiet killer. A tool with 0.02 mm runout will cut one flute harder than the others, and the edge finish will show it as a repeating pattern. Checking runout with an indicator before the finishing pass takes 30 seconds and prevents a scrapped part. On a 4,000 mm gantry part, that check is worth far more than the time it costs.

• 1
  Draw the corner, then pick the toolThe drawing radius must be reachable by the cutter.
• 2
  Match the coating to the materialAlTiN for steel, DLC for aluminium and copper.
• 3
  Check runout before finishing0.02 mm runout leaves a visible pattern on the edge.

A 3-axis machine can cut a chamfer if the edge faces the spindle. Turn the part so the edge is on the side wall, and the same feature needs a second setup. Each setup adds a datum shift. Two setups mean two chances for the edge to land 0.05 mm off where the drawing says it should be. That is often the real cost, not the cutting time.

Simultaneous 5-axis moves the tool, not the part. The rotary table tilts the workpiece while the spindle follows, so a continuous edge profile can be cut in one pass without repositioning. On a Ø400 mm rotary table, a wheel rim or a turbine housing keeps its datum from the first face to the last chamfer. The edge stays continuous because nothing was unclamped.

This does not mean every edge needs 5-axis. A simple plate with four chamfers is faster on a 3-axis machine with a good fixture. The judgment call is about edge continuity and datum count. When the profile wraps around more than two faces, or when the edge must blend into a curved surface, the multi-axis approach wins on both accuracy and setup time. For flat parts with straight edges, it does not.

• 1
  Count the setups firstEach re-clamp adds a datum shift and a chance for error.
• 2
  Continuous profiles favor 5-axisEdges that wrap around faces stay continuous in one setup.
• 3
  Simple flat edges do notA 3-axis machine with a solid fixture is faster and cheaper.

Aluminium 6061 and 7075 cut cleanly at high spindle speed. Edges can be taken to Ra 0.8–1.6 μm with a sharp tool and a light finish pass. The risk is built-up edge, which shows as a smeared layer on the chamfer. A generous coolant flow and a positive rake angle keep the chip moving away from the edge.

Stainless 304 and 316L work-harden at the cut. If the tool rubs instead of cutting, the surface gets harder and the next pass gets worse. The fix is to keep the chip load up and never dwell. A 0.05 mm radial engagement with a slow feed will harden the edge and dull the tool. We run stainless edges with a minimum chip load per tooth and accept a slightly rougher finish that polishing will remove later.

Titanium Ti-6Al-4V and Inconel are the hard cases. Both hold heat at the cut and both work-harden. Edge cutting on these alloys usually runs at 30–50 m/min surface speed with high-pressure coolant. The tool path must be smooth, because any reversal at the edge creates a dwell mark that is nearly impossible to polish out. For these materials, the edge is often finished by EDM or by hand rather than by a final milling pass.

• 1
  Aluminium: watch built-up edgePositive rake and strong coolant keep the chamfer clean.
• 2
  Stainless: never let the tool rubMinimum chip load prevents work hardening at the edge.
• 3
  Titanium and Inconel: smooth paths onlyTool reversal at the edge leaves a dwell mark.

A machined edge carries a burr. The burr size depends on the material, the tool wear, and the exit angle of the cutter. Soft aluminium leaves a larger burr than hardened steel, but it is easier to remove. Stainless can leave a work-hardened burr that resists a hand file. The deburring method has to match the burr, not the material alone.

Hand deburring with a file or a scraper is still the most flexible method for one-off parts. It is also the least repeatable. For runs of 10,000 pieces, a vibratory tumbling process with the right media gives a consistent 0.1–0.2 mm edge break across the batch. The trade-off is that tumbling also rounds every other edge on the part, which may not be acceptable if some edges must stay sharp.

Polishing takes the edge from functional to cosmetic. Bead blasting gives a uniform matte finish and hides tool marks. Brushing leaves a directional grain. Buffing brings aluminium or stainless to a mirror look, but it also rounds the edge slightly, so a 0.2 mm chamfer can become a 0.4 mm radius after buffing. If the drawing calls for a sharp cosmetic edge, the polishing step has to be specified tightly or the geometry will drift.

• 1
  Match deburring to the burrA work-hardened stainless burr resists a hand file.
• 2
  Tumbling is repeatable, not selectiveIt rounds all edges, including the ones you want sharp.
• 3
  Polishing moves the geometryBuffing can turn a 0.2 mm chamfer into a 0.4 mm radius.