Machining Tutorial for CNC Metal and Plastic Parts

• 1
  Key takeaways
• 2
  Read the drawing before you touch a machine
• 3
  Pick stock, setups, and tooling in that order
• 4
  Speeds, feeds, and the first cut
• 5
  How to hold ±0.005 mm without scrapping parts
• 6
  Finishing, deburring, and what changes the size
• 7
  Step by step: a repeatable machining workflow
• 8
  Machining parameters by material

A machining tutorial that starts at the spindle skips the part that costs the most money. Start with the drawing. Find the datum, the tightest tolerance, and the surface that must stay untouched. On a typical bracket, one bore at ±0.005 mm and every other feature at ±0.1 mm is common. That single tight bore decides the machine, the workholding, and how many setups the part needs.

Check the tolerance stack next. If two tight features sit on opposite faces and no datum links them, the machinist has to pick a setup that reaches both. Sometimes that means a 5-axis center with one rotation. Sometimes it means two operations on a 3-axis mill, and the second setup inherits the error of the first. Ask which features are functional and which are cosmetic before quoting.

Material matters at this stage too. Aluminum 6061 and 7075 cut fast and hold ±0.005 mm with a rigid setup. Stainless 316 and 17-4PH work-harden, so light passes and sharp tools matter more than speed. Titanium TC4 (Ti-6Al-4V) needs lower surface speed and plenty of coolant. Inconel is slower still. None of these are hard to machine, but the cycle time and tool wear change by a factor of three or more.

Send a STEP file, not just a PDF. A 3D model lets us check wall thickness, tool reach, and whether a 6 mm end mill can actually get into that pocket. Most revisions we flag come from tool access, not from tolerance. A drawing can look clean and still hide a corner no cutter can reach.

Choose stock size so the part sits inside it with 0.5–1.0 mm per side on milled faces. On turned parts, 0.3–0.5 mm on the diameter is enough. Extra stock is not free. It means more passes, more tool wear, and more chance the part moves as internal stress releases. On thin plates, take a roughing pass on both sides before finishing either one. That balances the stress.

Count setups before you program. One setup with a 5-axis center often beats three setups on a 3-axis machine, even at a higher hourly rate. The reason is simple. Every new setup adds a new source of position error. If your part has holes on four sides plus a contoured top, one 5-axis operation at ±0.005 mm is usually the safer plan.

Tooling follows geometry. A 6 mm carbide end mill is the workhorse for pockets. Corners smaller than 2 mm radius need a 3 mm or 2 mm cutter, and those deflect more, so reduce depth of cut. Deep pockets with a 4:1 depth-to-diameter ratio need a relieved neck or a smaller cutter with a step-down strategy. Thread milling beats tapping in hard stainless and titanium, because a broken tap in a nearly finished part is an expensive day.

Write down the critical dimension for each setup. The operator should not have to guess which feature matters. On our floor, the setup sheet lists the datum, the tight tolerance, and the inspection method for each operation. That sheet is what keeps a 10,000-part run consistent.

Start from surface speed, then work back to rpm. For aluminum 6061 with a carbide cutter, 300–500 m/min is a normal range. For 304 stainless, drop to 100–150 m/min. Titanium TC4 sits around 40–60 m/min. Inconel runs lower still. Convert with rpm = (surface speed × 1000) ÷ (π × cutter diameter). A 10 mm cutter in 6061 lands near 12,000 rpm, which most of our spindles reach.

Feed per tooth is the number that controls chip thickness, and chip thickness controls heat. Too thin a chip rubs and work-hardens stainless. A common starting point is 0.05–0.1 mm per tooth for aluminum and 0.03–0.06 mm per tooth for stainless and titanium. If the chips come off as dust, increase feed. If the cutter squeals, reduce radial engagement or check the setup.

Depth of cut depends on rigidity. A rigid setup in aluminum can take 1–2 × diameter in axial depth with 30–50% radial engagement. In titanium, keep axial depth low and radial engagement moderate, then use high-pressure coolant. On a long reach or a thin wall, take 0.1–0.2 mm passes and accept the longer cycle. Chatter marks are not a finish problem. They are a rigidity problem.

Roughing leaves 0.2–0.4 mm for the finishing pass. Then measure. If the feature is at +0.05 mm against a ±0.005 mm tolerance, adjust the tool offset and cut again. Cutting to the nominal number and hoping is how scrap gets made.

Tolerance is a system, not a single number. A ±0.005 mm bore needs a rigid setup, a temperature-stable shop, a sharp tool, and a measuring method that reads to 0.001 mm. If any one of those is missing, the tolerance will not hold across a run. Our shops work to ±0.005 mm (±0.0002 in) on features that need it, and we say so on the drawing review before cutting.

Heat moves metal. A 100 mm aluminum part grows about 0.0023 mm per °C. Rough it, let it cool, then finish it. On tight parts, we rough in the morning and finish after the part has returned to room temperature. That single pause removes more error than any tool change.

Measure with the right instrument. Calipers are fine for ±0.05 mm. Below that, use a micrometer, a bore gauge, or a CMM. Gauge the feature the same way the drawing defines it. A bore measured with a pin gauge and a bore measured with a CMM can differ by 0.003 mm, and both can be wrong if the datum is not the one on the drawing.

Inspection is where the numbers get proved. We check raw material on arrival, monitor in-process dimensions, and inspect 100% before shipment. Reports are available on request. If your program requires first article inspection with a ballooned drawing, say so at quote time. It changes the plan, not the price of the part.

Finishing is part of the machining plan, not an afterthought. Bead blasting hides tool marks and gives a matte surface. Tumbling rounds sharp edges on small parts. Brushing leaves visible direction lines. Polishing gets you toward a mirror finish but adds cost and hand work. Pick the finish from the function first: sliding surfaces, sealing faces, and appearance parts each need a different treatment.

Coating and plating add thickness. Anodizing typically adds 5–25 μm depending on the type, and hardcoat sits at the higher end. Electroless nickel adds a more even layer than zinc plating. If a bore must stay at Ø10.000 mm after anodizing, machine it undersize by the coating thickness. Tell the machinist the final requirement, not just the pre-plate number.

Laser marking needs at least 1.5 mm character height to stay readable. Small text on a curved or blasted surface loses contrast. If the mark is a serial number or a traceability code, place it on a flat face that stays visible after assembly.

Deburr every edge unless the drawing calls for a sharp corner. A 0.2–0.3 mm break is standard. On medical and food-contact parts, a larger radius or a full polish may be required. Those calls should come from the drawing, because the operator cannot guess the intent.