10 Common CNC Machining Defects and How to Fix Them

Dimensional drift shows up as a feature that measures right on the first part and out of tolerance by part twenty. The usual causes are thermal growth in the spindle and ballscrew, chips packed under a locating face, or a fixture that lets the part creep. Check the machine's warm-up cycle first. A spindle that runs thirty minutes before the first cut holds a different geometry than one that starts cold. Then look at chip evacuation around locating pads. A 0.05 mm chip under a pad becomes a 0.05 mm error in the part.

Angular error on a milled face often traces back to a spindle that is not square to the table, or to a vise that lifts the part when it is clamped. Indicate the vise jaw and the part face, not just the vise body. On a five-axis machine, a rotary table that is out of center will make every hole pattern shift as the table indexes. Probe the table center and the tool length before the run, and re-check after a long cut.

Cutter marks that look like a washboard come from runout, an unbalanced holder, or a feed rate that is too high for the tool's flute count. Measure runout at the tool tip, not at the holder. If runout is under 0.01 mm and the marks remain, reduce feed per tooth and check the tool's helix angle against the material. A three-flute cutter in aluminium behaves differently from a four-flute cutter in the same cut.

Chatter is a self-excited vibration. It starts when the tool, holder, and workpiece form a system with too little stiffness for the cutting force. The fix is rarely one setting. Shorten the tool overhang first, because stiffness drops with the cube of length. A tool hanging 60 mm out of the holder can be four times less stiff than the same tool at 30 mm. Then check the holder for wear and the collet for chips.

Vibration also comes from the part itself. Thin walls and long, unsupported sections ring when the cutter passes. Add support, reduce radial engagement, or climb mill with a smaller stepover. On aluminium, a high helix cutter and a light radial cut often beat a heavy cut with a low helix tool. On stainless, the same approach can work-harden the surface, so keep the cutter moving and never let it rub.

Poor surface finish is a symptom, not a single defect. Ra 1.6–3.2 μm is normal as-machined. Getting to Ra 0.8–1.6 μm needs a sharper tool, a smaller feed per tooth, and stable coolant. Getting below Ra 0.8 μm usually means a finishing pass with a dedicated tool, not a slower version of the roughing pass. If the finish looks smeared rather than torn, the tool is rubbing. Increase feed and check the edge radius.

Burning and discoloration mean heat is going into the part instead of the chip. The cutting speed is too high, the feed is too low, or the coolant is not reaching the edge. In titanium and stainless, heat stays in the cut longer, so the window is narrower. Check that the coolant stream hits the cutting zone, not the top of the tool. Through-spindle coolant helps on deep pockets where a flood nozzle cannot reach.

Built-up edge is material welding to the cutting edge and then breaking off, taking part of the edge with it. It shows as a rough, gummy surface and a tool that wears fast. The cause is usually a speed and feed combination that lets the material pressure-weld to the tool. Increase surface speed and feed per tooth, use a coating matched to the material, and keep the coolant consistent. Interrupted cuts make built-up edge worse because the edge cools and heats on every pass.

Chip congestion is common in deep slots, small holes, and pockets with tight corners. Chips pack into the flutes, the tool rubs instead of cuts, and heat climbs. Peck drilling with a full retract clears the hole. In milling, use a cutter with a chip-breaker geometry and adjust the coolant to flush the pocket, not just cool the tool. A recut chip is harder than the parent material, so it dulls the edge faster than a clean cut.

Warping on thin parts comes from residual stress in the material and from heat added during cutting. A plate that is machined on one side only will bow as the stressed layer is removed. Rough both sides, stress-relieve if the material allows it, and take light finishing passes on both faces. For long parts, support the underside and avoid clamping that bends the part into place before the cut.

Burrs form where the tool exits the material. The size depends on edge sharpness, feed, and material ductility. Aluminium and copper burr more than cast iron. A sharp tool with a positive rake and a small exit feed reduces the burr. Deburring by hand is fine for one part, but a tumbler or a brush deburring step holds consistency across a run. On medical and sealing surfaces, specify the deburring method on the drawing so the edge is not left to chance.

Hole defects include oversize, taper, bellmouth, and poor position. Oversize and taper usually come from a drill that is not sharp, a speed that is too high, or a machine with backlash in the axis. Bellmouth at the entry comes from the drill wandering on a curved or angled surface. Spot the hole first, or use a flat-bottom spot drill. Position errors often trace to a fixture that does not locate the same way on every part, so check the locating scheme before blaming the machine.