Common Problems of CNC Treatment and How to Fix Them

• 1
  Symptom, cause, and fix at a glance
• 2
  Common problems of CNC treatment: where they start
• 3
  Why the bore drifts out of tolerance
• 4
  Chatter and poor Ra: reading the marks
• 5
  Holes that walk, and threads that drift
• 6
  Material-specific problems worth knowing
• 7
  Step by step: a repeatable way to fix a drifting process

Most problems do not appear at the machine. They start earlier, in the setup sheet, the stock condition, or the way the part is held. A boring bar that runs 0.01 mm out of round on the first article usually points to a holder that is too long for the depth, not to a bad spindle.

We see the same set of failures across aluminium, stainless and titanium jobs. The material changes the numbers, not the logic. A 6061 bracket and a 17-4PH valve body fail for the same three reasons: weak support, wrong cutting data, and heat that nobody measured.

This section covers the four groups we fix most often: dimensional drift, surface finish, hole location, and material-specific trouble. Each group has a symptom you can see on the part and a place in the process where it begins.

• 1
  Measure firstRecord the deviation in mm, not in 'looks off'.
• 2
  Change one thingOne variable per trial, or you learn nothing.
• 3
  Check the stockHardness and residual stress move the first cut.

A bore that grows 0.02 mm between the first and twentieth part is almost always a heat problem. The spindle, the coolant and the part all warm up over the first 20 minutes. If you inspect the first article cold and the tenth article hot, you are measuring two different machines.

The second cause is deflection. A boring bar at 6 × Ø overhang will push away from the cut and leave a taper. You can see it by measuring the bore at the top and the bottom. If the difference is 0.01 mm or more, shorten the overhang or take a spring pass at the same depth.

The third cause is workholding. Thin walls and unsupported floors move under clamping pressure. A 3 mm wall on a 100 mm pocket can flex 0.05 mm when the vise closes. Support the wall with a soft jaw or a plug, then measure again.

We hold ±0.005 mm on production parts, but only when the setup is stable. Tolerance is a result of the process, not a promise you can add later.

Chatter leaves a regular pattern. The spacing tells you the frequency: wide marks point to the workholding, tight marks point to the tool. Count the marks around the bore or along the wall before you change the speed.

Spindle speed is the fastest lever, but it is not always the right one. On a long tool, raising rpm makes chatter worse. Drop the speed by 20% and raise the feed per tooth instead. On a short tool in aluminium, raising rpm usually clears it.

Poor Ra on stainless and titanium often comes from a worn insert, not from the machine. A 17-4PH part at Ra 1.6–3.2 μm can drop to Ra 0.8–1.6 μm with a fresh edge and a 0.1 mm depth of cut. Check the insert corner under magnification before you touch the program.

Coolant matters more than people expect. High-pressure coolant through the tool breaks the chip and keeps the edge cool. Flood coolant on a deep pocket often leaves a built-up edge on the tool and a torn finish on the wall.

A drill walks when the entry surface is not flat or the point is not centered. On a cast or rough surface, spot drill 90° to a diameter of 0.5 × the drill Ø. On a curved surface, use a flat-bottom spot or mill a small pad first.

Position error also comes from the machine, not the tool. Check the backlash on the axis before you blame the drill. A 0.03 mm backlash shows up as a location error that changes direction with the approach.

Thread drift on aluminium is usually a speed problem. A form tap at 1,200 rpm in 6061 will stretch the pitch over a long thread. Drop to 300–600 rpm, or use a cut tap with the correct pitch diameter, and measure with a thread gauge, not a bolt.

Deep holes add a fourth cause: chip packing. Peck deeper than 3 × Ø and clear the flutes, or the drill will push the chips back into the hole and break at the flute.

Aluminium 6061 and 7075 cut fast but move after machining. A thin 7075 plate can bow 0.1 mm after the vise is released. Rough, stress-relieve, then finish in a second setup.

Stainless 304 and 316 work-harden. A light pass with a dull tool hardens the surface and makes the next pass worse. Keep the feed per tooth above 0.05 mm and never let the tool rub.

Titanium TC4 (Ti-6Al-4V) and Inconel hold heat at the edge. Use high-pressure coolant, keep the radial engagement low, and replace the insert before the corner wears. Inconel often needs a slower speed and a rigid setup more than a different tool.

Magnesium AZ31B and AZ91D cut easily but need chip control. Fine chips catch fire. Use sharp tools, high feed, and never let the fines pile up dry under the machine.