CNC Basics Getting Started

• 1
  What Actually Happens Inside the Machine
• 2
  Tolerance, Finish and Datum Are Three Separate Conversations
• 3
  Why 3-Axis and 5-Axis Give Different Quotes
• 4
  Material Chooses the Cut, Not the Other Way Around
• 5
  Setup, Fixturing and Where the Cost Sits
• 6
  Which Process Fits the Part

CNC stands for computer numerical control. A program tells a spindle where to move, how fast to spin, and how fast to feed through the workpiece. The tool is harder than the workpiece, so it shears material off in chips. Nothing is molded or bent. You start with a solid block and end with less of it.

Milling uses a rotating multi-flute cutter that moves in X, Y and Z. Turning uses a single-point tool against a rotating cylindrical blank, which is why turned parts are round. A mill-turn center does both in one setup, and that matters when a part has a turned diameter and milled flats that must stay concentric.

Every cut is defined by four numbers: spindle speed (rpm), feed rate (mm/min), depth of cut (mm), and cutter engagement. Change one and the other three usually need to change too. Push feed too high and the tool chips. Push speed too high and the edge burns. Too slow and the tool rubs instead of cutting, which wears it faster than cutting hard does.

Toolpath strategy is where cost is decided. A part can be programmed to cut air for 40 minutes or to remove the same material in 12. That difference shows up in your quote, not on your drawing.

• 1
  MillingRotating cutter, workpiece mostly stationary. Best for pockets, slots, faces and profiles.
• 2
  TurningRotating workpiece, single-point tool. Best for shafts, bushings and threaded diameters.
• 3
  Mill-turnBoth motions in one setup. Best for parts that need concentricity between features.

Tolerance is how much a dimension may drift. General tolerance on a machined part might sit around ±0.1 mm. Tighten a single bore to ±0.005 mm and the shop has to slow down, take lighter passes, and often measure on a CMM before the part leaves the machine. That one callout can change the price of the whole part.

Surface finish is separate. As-machined surfaces land around Ra 1.6–3.2 μm. A good fine finish sits around Ra 0.8–1.6 μm. Below that you are usually talking about a secondary operation, not a different cutter. Polishing, lapping or bead blasting all cost time, and none of them fix a dimension that is already out.

Datums are the third conversation. A tolerance only means something relative to the feature it is measured from. If your drawing calls out a true position without a clear datum, the shop will pick one, and it may not be the one you had in mind. Engineers who specify datums up front get fewer first-article surprises.

A practical rule: keep tight tolerances on the features that mate with something else. Let the rest run loose. On a typical bracket, two bores and one face matter. The rest of the profile can sit at ±0.15 mm and nobody will notice.

A 3-axis machine moves the tool in three linear directions. Simple pockets, plates, and parts that can be reached from one direction are cheapest here because setup is quick and the program is short. Most flat brackets never need anything more.

A 4-axis machine adds rotation about one axis, usually the X. That lets the tool reach four sides of a part without re-clamping it. The win is not speed, it is positional accuracy. Every re-clamp introduces a small error, and stacked errors are what kill a tight true-position callout.

A 5-axis machine adds a second rotary axis, so the tool can approach from nearly any angle. This is how you cut an impeller, a turbine blade, or a housing with undercut features. It also lets the tool tilt so a shorter, stiffer cutter can reach deep pockets, which improves finish and extends tool life.

The trade is programming time. A 5-axis toolpath takes longer to prove out and often needs simulation before it runs. For a one-off flat plate, that overhead buys you nothing. For a part with compound angles that would otherwise need four setups, it usually wins on total cost.

Aluminum 6061 machines fast and holds tolerance well. It is the default for prototypes and most enclosures. 7075 is stronger but gummier and more prone to distorting after heavy material removal, so a shop may leave stock and take a finishing pass later.

Stainless 303 is free-machining and behaves. 304 and 316 work-harden if the tool rubs, so the feed has to stay aggressive enough to cut under the hardened layer. Slow down on stainless and you make the problem worse, not better.

Titanium and Inconel sit at the other end. Heat stays in the cutting zone instead of leaving with the chip, so tool life drops sharply and coolant strategy matters as much as the program. These parts take longer, and the quote should reflect that.

Plastics are their own problem. POM and ABS cut cleanly. PEEK is abrasive and expensive, so scrap hurts. Carbon fibre eats tool edges and needs dust control. A program written for aluminum will not transfer to carbon fibre without changes.

Every job carries a fixed setup cost: programming, workholding, first-article inspection. On one part, that fixed cost dominates. On 500 parts, it spreads out and the per-part price drops toward the cost of run time and material.

Fixturing is the quiet cost driver. A part with a flat bottom and two parallel sides clamps in a vise in minutes. A thin-walled part or an odd shape may need a custom soft jaw or a support fixture, and that tooling has to be made before the first good part exists.

This is why a simple part can be cheaper on a manual mill at quantity one. There is no program to write and no simulation to run. As volume or geometric complexity rises, CNC takes over, and the crossover often happens sooner than people expect.

Thin walls are the classic failure mode. A 0.8 mm aluminum wall will deflect under cutting force and may spring back after the clamp comes off. If the design allows 1.5 mm, take it. The part will be straighter and cheaper.