Metal CNC Machining Guide: How Cutting, Heat Treatment and Finishing Interact

• 1
  What Cutting Actually Does to Metal
• 2
  Axis Count and Part Geometry: When 3 Axis Is Not Enough
• 3
  Heat Treatment Before and After Machining
• 4
  Surface Finish: Numbers and What They Hide
• 5
  Where Tolerance Limits Come From
• 6
  Step by Step: From Model to Inspected Part
• 7
  Machining Route by Part Type

Every CNC cut is a controlled fracture. The tool edge pushes into the workpiece until the metal shears along a plane ahead of the edge. That shear plane is where the part is made, and it is also where damage starts. Heat, strain and residual stress all enter the material at the same moment.

Three variables decide whether the cut stays clean: cutting speed, feed per tooth and radial depth of cut. On 6061 aluminium, a 12 mm carbide end mill typically runs at 300–500 m/min surface speed with 0.05–0.15 mm feed per tooth. Drop to 304 stainless and the same tool wants 80–120 m/min. Push stainless at aluminium speeds and the edge breaks down in minutes.

Chip shape tells you if the parameters are right. Aluminium should throw short, bright, curled chips. Stainless should produce a straw or blue chip that breaks cleanly. A fine powder means the tool is rubbing instead of cutting, and the surface will work-harden under the next pass.

Coolant is not optional on stainless, titanium and Inconel. Through-spindle high-pressure coolant clears chips from deep pockets and keeps the cutting zone below the temperature where the material hardens. On aluminium, air blast plus a light mist often beats flood coolant because it avoids thermal shock on thin walls.

A 3-axis machine moves the tool in X, Y and Z while the part stays fixed. That is enough for plates, brackets, housings with open faces and any feature you can reach from one direction. Setup count is the hidden cost. A part with features on four faces needs four setups on a 3-axis mill, and each setup adds alignment error.

A 4-axis mill adds a rotary table, usually Ø400 mm, that indexes the part between cuts. This removes most re-fixturing on cylindrical or square parts with features around a single axis. Indexing accuracy is high because the part never leaves the table.

A 5-axis machine moves the tool and the part at the same time. Simultaneous 5-axis lets a short, stiff tool reach into deep pockets and cut undercuts, blended fillets and impeller vanes in one setup. It also holds true position better across faces because there is no re-clamping. GreatLight runs 16 simultaneous 5-axis centers alongside 27 three-axis machines, so the axis count is chosen from geometry rather than habit.

The trade-off is programming time and machine rate. A simple bracket on a 5-axis center costs more per hour than the same part on a 3-axis machine. Use 5-axis when the geometry demands it, or when setup error on a multi-face part would eat the tolerance budget.

Heat treatment changes grain structure, hardness and internal stress. It also changes how the part machines. The four foundational processes are annealing, normalizing, quenching and tempering, and the order in which they run against machining matters as much as the process itself.

Annealing softens metal and relieves stress. It is usually done before machining on 4140 or 4340 so the cutter is not fighting hard stock. Normalizing refines grain after forging or casting and gives a more uniform structure to cut. If a part arrives normalized, expect consistent hardness across the section instead of soft and hard bands.

Quenching and tempering raise strength and toughness, and they are normally done after rough machining. Quench a finished thin-wall part and it will move. The standard sequence is rough machine, stress relieve, semi-finish, harden, then finish grind or finish mill to size. That leaves the final tolerance cut for after the distortion has already happened.

Some materials skip heat treatment entirely. Most 6061 aluminium is used as supplied or in the T6 condition. Titanium Ti-6Al-4V is usually machined in the annealed state. For hardened tool steel above 45 HRC, plan on carbide or ceramic tooling, lighter radial engagement and a finishing allowance of 0.3–0.5 mm per side.

Ra is the arithmetic average of surface deviations from the mean line. It describes roughness, not waviness, not porosity and not subsurface damage. A part can measure Ra 0.8 μm and still fail if the surface has torn metal or a folded chip.

As-machined finish on aluminium and steel normally lands at Ra 1.6–3.2 μm. Careful finishing passes with a sharp tool, higher speed and a small feed get to Ra 0.8–1.6 μm. Below that, you are usually polishing, lapping or bead blasting, and the geometry of sharp internal corners changes.

Finishing passes are cheap compared to grinding. A spring pass with 0.1–0.2 mm radial engagement and 0.05 mm/rev feed removes the witness marks from the roughing pass without loading the tool. On deep pockets, use a tool with the shortest possible overhang; chatter shows up as waviness that no Ra number will explain.

Anodizing, plating and powder coating add or remove material. Hardcoat anodizing builds 25–50 μm per surface and moves a Ø20 mm bore toward Ø19.95 mm. Mask critical fits or specify the pre-plate dimension. Laser marking needs a minimum character height of 1.5 mm to stay legible after coating.

±0.005 mm is a process capability, not a wish. It holds on a rigid setup with a sharp tool, stable temperature and short tool overhang. It gets harder as the part grows, as walls thin, and as the number of setups rises.

Thermal expansion is the quiet killer. Aluminium grows about 23 μm per metre per °C. A 500 mm aluminium part measured at 25 °C and machined at 30 °C is 57 μm off before any tool deflection. Shops that hold tight tolerance control temperature and let parts stabilize before the final measurement.

Tool deflection scales with the cube of overhang length. Doubling overhang makes the tool eight times softer in bending. That is why deep cavities need a smaller tool, a longer reach and a lighter cut, and why the tolerance on a 4:1 depth-to-diameter pocket is looser than on a shallow face.

Inspection closes the loop. A tolerance that cannot be measured is a tolerance that will be argued about at receiving. Tell us the measuring method and the report you need, and the machining plan will be built around it.