CNC machining TX: how the process actually works

• 1
  What CNC machining TX actually does to metal
• 2
  3-axis, 4-axis, 5-axis: which geometry fits the part
• 3
  Tolerance and surface finish: where the real limits sit
• 4
  Material behavior that changes the cut
• 5
  When CNC machining is the wrong process
• 6
  Machine and process selection by part type

CNC machining TX is subtractive: a rotating cutter removes material in controlled passes until the remaining geometry matches the CAD model. The machine does not shape metal by force or heat. It shears it. Each tooth of the cutter takes a chip of a defined thickness, and the feed rate, spindle speed and depth of cut decide whether that chip forms cleanly or rubs.

That single fact drives most machining decisions. A clean chip carries heat away with it. A rubbing edge leaves heat in the part, and the part moves. On a 300 mm aluminum plate, a few degrees of local heating is enough to shift a bore by more than the tolerance you are trying to hold. So coolant, toolpath order and fixture rigidity are not extras. They are the process.

The control system reads G-code and interpolates motion across several axes at once. Three linear axes handle the simple cases. Add one or two rotary axes and the cutter can reach five faces of a part in a single setup, which removes the repositioning error that stacks up when you flip a part between operations.

That is the whole mechanism in plain terms: controlled chip formation, rigid clamping, and axis motion that keeps the tool normal to the surface. Everything else in this article is a boundary condition on those three.

A 3-axis machine moves the tool in X, Y and Z only. It is the right choice for prismatic parts with features reachable from one direction: plates, brackets, housings with open pockets. Setup is fast and programming is predictable. The limit appears when a part has features on five sides or a contoured surface that needs the tool tilted to reach it.

A 4-axis machine adds a rotary table, usually around the X axis. Now you can index the part to a new face without unclamping it. Shafts with cross-drilled holes, parts with features at 90° intervals, and cylindrical forms all get simpler. The rotary table here is Ø400 mm, which sets the practical size envelope for indexed work.

A 5-axis machine adds a second rotary axis, and the two can move at the same time. That simultaneous motion is what lets the tool stay normal to a sculpted surface, or reach under a flange without a long, flexible tool. Impellers, turbine blades, and deep cavities with undercuts are the classic cases. The trade is programming time and a tighter setup budget.

Pick the lowest axis count that reaches every feature. Extra axes cost cycle time, and they only pay back when the geometry genuinely needs them.

Tolerance is not a single number you apply to a whole drawing. Feature by feature, the achievable value depends on the feature type, the material, and the number of setups. A bored hole in aluminum can hold ±0.005 mm when the machine, tool and thermal conditions are stable. The same hole across a 400 mm steel part, machined from two sides, is a different problem.

Surface finish follows a similar logic. Ra 1.6–3.2 μm is a normal as-machined result. Ra 0.8–1.6 μm is achievable with a finishing pass and a sharp tool. Ra 0.2–0.8 μm usually means a dedicated finishing operation, sometimes with a small stepover, and it takes longer. Specifying a fine finish on every face is one of the most common ways to add cost without adding function.

Thermal drift matters more than most drawings admit. A machine warming up over a shift can move the tool by more than the tolerance band on a tight feature. Shops that hold tight tolerances control this with warm-up cycles, stable coolant temperature, and finishing cuts scheduled after roughing has stopped moving the part.

The practical rule: put tight tolerances only on the features that mate with something. Everything else can be general tolerance, and the part gets cheaper without losing function.

Aluminum 6061 and 7075 cut fast and hold good finish. 7075 is stronger and machines cleanly, but it moves more after roughing because of residual stress in the plate. Rough it, let it rest, then finish. That rest step is not optional on thin 7075 parts.

Stainless 304 and 316 work-harden. If the tool rubs instead of cutting, the surface gets harder and the next pass is worse. The fix is a positive feed that keeps the edge biting, not a slower feed. 17-4PH behaves differently again and is usually machined in the solution-treated state, then aged.

Titanium Ti-6Al-4V conducts heat poorly, so the heat stays in the cutting edge. Tool life drops fast if speeds are pushed. Inconel is worse. Both need lower surface speeds, generous coolant, and a rigid setup. These are jobs where the machine and the tooling matter more than the CAM strategy.

Plastics like POM and PEEK cut easily but hold heat and expand. Sharp tools, air blast and modest depth of cut keep dimensions stable. PEEK is often machined slightly oversize and finished after it cools.

Machining removes material, so it wastes stock and time on parts that are mostly empty space. A thin-walled enclosure with complex internal ribs is often cheaper as a die casting or an injection-molded part. The tooling cost is real, but it spreads across volume. Below a few hundred units, machining usually wins anyway.

Very thin features are also a bad fit. Walls under about 0.5 mm in aluminum deflect under cutting force. You can machine them, but the process becomes slow and the yield drops. If the design allows a thicker wall, take it.

Hardened materials above roughly 45 HRC are difficult to cut with standard tooling. EDM or grinding handles those features better. A common path is to machine soft, then harden, then finish the critical features with EDM.

Parts with no flat surface to clamp are another boundary case. A custom fixture can solve it, and that fixture is a real cost. It still beats a casting if the quantity is low.

Finally, surface texture is a design choice, not a default. If the drawing calls for a mirror finish on a non-functional face, that is money spent on nothing.