How Do You Use a CNC Machine?

• 1
  Key takeaways
• 2
  What Happens Before You Use a CNC Machine
• 3
  Choosing the Machine and Workholding
• 4
  Setting the Work Zero and Tool Offsets
• 5
  Feeds, Speeds and the First Cut
• 6
  Errors That Scrap the First Part
• 7
  How to Use a CNC Machine: Step by Step
• 8
  Which Machine Setup Fits Which Part

A CNC machine does not decide anything. It repeats a path that someone already proved. So the real work starts at the drawing: you need the material, the blank size, the datums, the tightest tolerance and the surface finish on each face. A part with ±0.005 mm on one bore and ±0.1 mm everywhere else is a different job from a part that is tight all over.

Next comes the setup plan. Ask how many orientations the part needs. A plate with holes on one face is a single 3-axis setup. A part with features on four sides plus a compound angle usually needs a 4-axis or 5-axis machine, or two or three refixtures on a 3-axis. Every extra refixture adds stack-up error, so the axis count follows the setup count, not the other way around.

Then the CAM programmer builds the toolpath from the CAD model and posts G-code. Tool choice drives the rest: a Ø10 mm carbide end mill can rough aggressively but cannot enter a 6 mm corner. A Ø3 mm tool reaches the corner but must run slower and deflects more. If a corner radius is smaller than the smallest tool you are willing to run, the design should change before the machine runs.

Finally, the machine itself. A vertical mill handles prismatic parts. A lathe or mill-turn center handles round parts with turned diameters and milled flats. Wire EDM handles sharp internal corners and hardened steel. Knowing which process owns the feature saves a quote cycle.

• 1
  Drawing firstMaterial, datums, tightest tolerance and finish on each face.
• 2
  Setup countEach additional orientation adds stack-up error.
• 3
  Tool reachSmallest internal radius sets the smallest cutter.

For prismatic parts, a 3-axis vertical mill covers most work. Typical travels are 500 × 500 × 450 mm or 750 × 1,150 × 550 mm, which suits brackets, housings and plates. A 4-axis mill adds a rotary table, usually Ø400 mm, so you can index the part to a second or third face without touching the vise. That single addition often removes two refixtures.

Simultaneous 5-axis centers cut compound angles and contoured surfaces in one pass. They also let a short, stiff tool reach deep pockets by tilting the part instead of hanging the tool out. The trade-off is programming time and a smaller work envelope, so reserve them for parts that genuinely need the motion. Turning work goes to a lathe or mill-turn center, where a single setup can turn an OD and mill a flat.

Workholding decides whether the part moves. A vise is fast but leaves two faces open and can distort thin walls. Soft jaws machined to the part profile grip round or irregular shapes without crushing them. For thin plates, vacuum chucks or a fixture plate with toe clamps spread the load. For a second operation on a finished face, use a fixture that locates on a machined datum, never on the raw stock.

One rule: never clamp on a surface that has a tolerance callout unless that surface is supported underneath. Clamping pressure of a few hundred newtons is enough to spring a 2 mm wall, and the part will spring back after unclamping, out of tolerance.

• 1
  ViseFast, but leaves two faces open and can distort thin walls.
• 2
  Soft jawsMachined to the part profile; grips without crushing.
• 3
  Fixture plateLocates on a machined datum for the second operation.

The work zero is the point the program calls X0 Y0 Z0. Pick it from the drawing datums so the machine coordinates match the inspection coordinates. If the drawing dimensions a bore from a machined face, that face is your Z0, not the top of the raw stock. Getting this wrong shifts every dimension by the same amount, and the part will look correct but measure wrong.

Touch off each tool to a known surface and store the length in the offset table. A probe makes this repeatable to a few microns; a dial indicator and a gauge block still work but take longer. After touching off, verify by commanding the tool to a safe height above the stock and comparing the readout with a gauge block or a height setter.

Record the work offset and tool numbers on the setup sheet. The next operator should be able to reload the vise and the offsets without re-measuring from scratch. This is also what makes a repeat order fast: the fixture, the program and the offsets already exist.

If the machine has no probe, note the spindle warm-up. A cold spindle grows as it heats, and a Z offset set on a cold machine can drift 0.02 mm or more over the first hour. Warm up the spindle for 10 to 15 minutes before touching off on work that holds a tight tolerance.

Start from surface speed, not spindle RPM. Aluminium 6061 runs well at 300 to 500 m/min with carbide, which on a Ø10 mm tool gives roughly 10,000 to 16,000 rpm. Steel 1045 runs at 100 to 150 m/min, so the same tool turns at about 3,000 to 4,800 rpm. Titanium TC4 sits lower still, around 40 to 60 m/min, because the heat stays in the cutting edge.

Feed per tooth sets the chip load. For a Ø10 mm carbide end mill in aluminium, 0.05 to 0.10 mm per tooth is a normal range; in steel, 0.03 to 0.06 mm per tooth. Multiply feed per tooth by the tooth count and the rpm to get the feed rate, and check that the chip is a proper chip, not dust. Dust means the tool is rubbing and will wear fast.

For roughing, take depth of cut up to the tool diameter when the setup is rigid, and leave 0.3 to 0.5 mm on walls and floors for the finishing pass. Finishing with a small radial stepover, around 5 to 10% of the tool diameter, gives Ra 0.8–1.6 μm on most aluminium. A Ra 0.2–0.8 μm mirror finish needs a dedicated finishing tool and a rigid setup.

Coolant choice matters. Flood coolant controls heat in steel and stainless. Aluminium often cuts better with a mist or high-pressure air because it clears chips and avoids thermal shock on the edge. Titanium and Inconel need high-pressure coolant aimed at the cutting zone to break chips and protect the insert.

• 1
  Aluminium 6061300–500 m/min with carbide; 0.05–0.10 mm per tooth.
• 2
  Steel 1045100–150 m/min; 0.03–0.06 mm per tooth.
• 3
  Titanium TC440–60 m/min; high-pressure coolant at the edge.

The most common failure is the wrong Z zero. An operator touches off on the top of the raw stock when the drawing dimensions from a machined step. Every depth is then short or long by the stock allowance. The fix is written on the setup sheet: state the datum face in words, not just a coordinate.

Second is tool deflection on deep pockets. A Ø6 mm end mill hanging 40 mm out of the holder will bend under load, and the wall will taper. Listen for chatter and reduce the axial depth or use a shorter tool. If neither works, the pocket needs a different process, such as EDM or a relieved tool holder.

Third is clamping distortion. A thin wall clamped at 300 N will move by tens of microns, and the part springs back after unclamping. Support the wall from behind, reduce clamp pressure, or machine the wall in a finishing pass after the clamps are relaxed. Measure a suspect wall while it is still clamped and again after, and compare.

Fourth is chip recutting. If chips stay in the pocket, the tool cuts them instead of the workpiece and the finish turns ragged. Use through-spindle coolant, air blast or a peck cycle that lifts the tool clear. On aluminium, a strong air blast often works better than flood coolant because it clears chips faster.