Process and Precautions for CNC Machining

• 1
  Key takeaways
• 2
  What the CNC machining process actually involves
• 3
  Precautions for CNC machining that start at the CAD model
• 4
  Cutting parameters, tooling, and where the setup fails
• 5
  Inspection, finishing, and the moves that follow machining
• 6
  Where the process goes wrong and how to catch it early
• 7
  Step by step: from model to inspected part
• 8
  Which machine and finish fit the part

CNC machining turns a 3D model into a metal or plastic part by removing material with rotating cutters and turning tools. A CAM programmer converts the model into toolpaths, the machine follows that code, and a set of fixtures holds the workpiece at a known position for every cut. That is the whole idea. Everything else in the process is about controlling where the material goes and where the part sits.

The process runs in five stages: DFM review, material and stock preparation, fixturing and setup, roughing and finishing, then inspection and finishing. Each stage feeds the next. A DFM note that changes a corner radius can remove an entire second setup. A fixture that is not rigid will show up as chatter 40 minutes into roughing.

Precautions for CNC machining are mostly about the gaps between those stages. Most scrapped parts are not scrapped by a bad toolpath. They are scrapped by a stock allowance that was too small, a datum that changed between operations, or a finishing pass that ran on a part which had already moved from residual stress.

The good news is that these failure modes are predictable. If you know the tolerance, the material, and the geometry, you can decide in advance whether a part belongs on a 3-axis mill, a 5-axis center, or a mill-turn machine.

• 1
  Model in, part outCAM, toolpath, fixture, machine. Four inputs, one output.
• 2
  Tolerance sets the machine±0.005 mm usually means grinding or a finish pass on a rigid setup.
• 3
  Material sets the strategyAluminium runs fast and cool; titanium needs lower surface speed and more coolant.

Start with wall thickness. On aluminium, 0.8 mm is roughly the floor before chatter becomes hard to control; on stainless and titanium, stay above 1.5 mm where the part allows it. Thin floors behave the same way. If a pocket floor is 0.5 mm thick over a large area, expect it to deflect under clamping pressure before the cutter ever touches it.

Then check internal corners. A cutter has a radius, so an inside corner can never be sharper than the tool. If the drawing calls for a sharp internal corner, the shop either leaves a radius you did not want or adds a sinker EDM operation you did not budget. Add a corner radius at least equal to the largest reasonable cutter radius for that pocket depth.

Threads and holes need depth rules too. A blind tapped hole should be at least 1.5× the nominal diameter deep for the thread to be usable, and the drill point adds roughly 0.3× diameter beyond that. Deep holes, past 5× diameter, need peck drilling and often a gun drill, which changes both cost and lead time.

Finally, look at datum features. Pick faces that will still exist after every operation and that a fixture can actually reach. If your only datum is on a face that gets machined away in operation two, the shop has to invent a new one, and position tolerance will drift.

• 1
  Minimum wall0.8 mm aluminium, 1.5 mm stainless and titanium as a working rule.
• 2
  Internal corner radiusAt least the cutter radius. Sharp corners mean EDM.
• 3
  Blind thread depth1.5× nominal diameter of usable thread, plus drill point.
• 4
  Keep a stable datumDo not machine away the face you measure from.

On aluminium, a 3-flute carbide end mill runs at 300–500 m/min surface speed with a 0.05–0.15 mm feed per tooth. That is fast, and it works because aluminium carries heat away with the chip. On 304 stainless, drop to 60–100 m/min and expect work hardening if the cutter rubs instead of cuts. Titanium sits lower still, around 30–60 m/min, with high-pressure coolant aimed at the cutting edge.

Roughing should leave 0.3–0.5 mm of stock on finishing surfaces. Less than that and the finish pass cuts into the work-hardened skin left by roughing, which shortens tool life and roughens the surface. More than that and the finish pass becomes a second roughing operation with its own deflection.

Fixturing decides whether any of that matters. A vise on a 300 mm part with a 200 mm overhang will deflect, period. Support long parts with adjustable jacks or a tailstock, and keep the cutting force directed into the fixture rather than pulling the part out of it. For a part with a thin floor, back it with a soft jaw or a sacrificial plate.

Keeping the same zero across operations saves more accuracy than any other single decision. On a 5-axis center, one setup reaches five faces, so position error between faces stays inside the machine's own repeatability instead of accumulating through three separate fixtures.

• 1
  Surface speedAluminium 300–500 m/min, 304 stainless 60–100 m/min, Ti-6Al-4V 30–60 m/min.
• 2
  Finish allowanceLeave 0.3–0.5 mm so the finish pass cuts clean metal.
• 3
  Support the overhangRigid support matters more than a higher feed rate.

Inspection should happen before finishing, not after. Once a part is anodized or plated, a dimension that is 0.01 mm over is still over, but you can no longer touch it up. Check critical dimensions on the machine where possible, then run a first-article inspection before the run continues. Reports are available on request; the default is a dimensional check of the drawing's critical features.

Finishing changes dimensions slightly. Anodizing adds a few micrometres per surface, hardcoat more. Electroless nickel adds roughly 0.01–0.025 mm per side depending on the build. If a bore has a press fit, mask it or allow for the coating thickness in the pre-plate dimension. This is one of the most common precautions for CNC machining that gets missed on the drawing.

Deburring is not cosmetic. A sharp edge on a mating face will not seat, and a burr in a fluid passage can break loose later. Specify edge breaks explicitly. Laser marking needs a minimum character height of 1.5 mm to stay legible after coating.

For prototypes and small runs, plan the finishing step into the schedule. Anodizing and plating are outside processes, so they add calendar time even when the machining itself ships in 3–5 days.

• 1
  Inspect before coatingYou cannot re-cut a plated part.
• 2
  Allow for plating buildElectroless nickel adds 0.01–0.025 mm per side.
• 3
  Specify edge breaksA burr on a mating face is a fit problem, not a finish problem.

Chatter shows up as a rippled surface and a tone change from the cut. It comes from too much tool overhang, a weak fixture, or a feed and speed pair that lets the cutter rub. Fix the rigidity first. Raising the feed sometimes helps, but only if the setup is already stiff enough to take it.

Dimensional drift across a batch usually traces back to heat or tool wear. Let the part cool before the final measurement; a warm aluminium part can read 0.02 mm larger than it will be at 20 °C. Track tool wear on long runs and change inserts on a count rather than on a hunch.

Bowing after unclamping is residual stress releasing. It is common in 7075 and in cold-rolled steel. Rough, stress-relieve if the geometry allows, then finish. For thin plates, remove equal material from both faces where the design permits.

Scrap on the first article is the cheapest scrap you will get. That is why the DFM review and the first-article check exist. Catching a datum problem at part one costs one part. Catching it at part 500 costs the run.

• 1
  ChatterReduce overhang and stiffen the fixture before changing speeds.
• 2
  DriftMeasure cold. Warm parts read oversize.
• 3
  BowingRough, relieve stress, then finish.