How Does a CNC Machine Cut?

• 1
  What actually removes the metal
• 2
  How does a CNC machine cut metal, step by step
• 3
  Tool geometry, coating, and what it does to the cut
• 4
  Speeds, feeds, and depth of cut in practice
• 5
  Workholding and setup decisions that change the result
• 6
  How to set up and run a first CNC cut
• 7
  Which machine and setup fits the part

A CNC machine does not cut with a blade in the way a saw does. It spins a multi-flute cutter at 3,000 to 15,000 rpm and pushes it sideways through the stock. Each flute bites a small slice of material and shears it off as a chip. The control reads G-code, drives the ball screws, and keeps the tool on a programmed path. That is the whole idea: a rigid frame, a sharp edge, and a motion system that does not wander.

The cut starts as elastic deformation. The tool edge presses into the workpiece until the stress passes the material's shear strength, and a chip separates. For aluminum 6061, that happens at a modest force. For 17-4PH stainless or Ti-6Al-4V, the force climbs fast and the heat does not leave with the chip as easily. That difference drives almost every parameter choice later on.

Heat splits three ways: into the chip, into the tool, and into the workpiece. In aluminum, 70 to 80 percent leaves with the chip, so the part stays cool. In titanium the split is worse, so we flood coolant and keep surface speed low. If the heat goes into the part, thin walls move after the cut and the dimension you measured at the machine is gone by the time the part cools.

The chip itself tells you whether the cut is healthy. Aluminum should throw short, bright, curled chips. Steel should give grey-blue chips that break at 6 to 12 mm. Long stringy chips mean the feed is too low or the chipbreaker is wrong. Fine dust means the tool is rubbing, not cutting. Read the chips at the machine before you trust the numbers on the screen.

An end mill is a compromise. A higher helix angle, 40 to 45 degrees, lifts chips out of a deep pocket but weakens the edge. A 30-degree helix is stronger for steel. The number of flutes matters too: 2 or 3 flutes leave room for chips in aluminum, while 4 to 6 flutes give a better finish on steel and stainless at lower feed per tooth.

Corner radius is the spec engineers miss most often. A sharp 0.5 mm corner on a deep pocket will chip the first time it hits a hard spot. A 0.4 mm corner radius spreads the load and lasts far longer. Draw the internal corner radius into the model, not into the CAM setup. If the print says R0.2, the tool must be smaller than that, and the cutter gets fragile.

Coating is not decoration. TiAlN handles steel and stainless at high temperature. AlTiN is harder and runs hotter, which suits dry or minimal-lubrication cuts in hardened steel. Uncoated carbide is still the right answer for aluminum, because AlTiN tends to weld to aluminum and tear the edge off. Diamond-like coatings help on abrasive plastics and carbon fiber.

Tool overhang is the quiet killer. A 12 mm cutter held 40 mm out of the holder deflects roughly eight times more than the same cutter held 20 mm out. Every extra millimeter of stick-out costs you depth of cut. When a job chatters, we shorten the holder before we touch the feed rate. Nine times out of ten the noise drops and the finish cleans up.

Surface speed is the starting point. For aluminum 6061 we run 300 to 500 m/min with uncoated carbide. For 304 stainless, 80 to 150 m/min. For Ti-6Al-4V, 40 to 60 m/min. Take the surface speed, divide by the cutter diameter, and you get the rpm. Then feed per tooth times number of teeth times rpm gives the feed rate in mm/min.

Depth of cut should load the tool, not the spindle. A common shop rule is 5 to 10 percent of the cutter diameter for radial engagement in steel, and up to 30 percent in aluminum with a strong setup. Axial depth can go much deeper, often 1 to 2 times the diameter, as long as the tool has the flute length and the holder is short. This is the high-efficiency approach: lighter radial cuts, deeper axial cuts, longer tool life.

Coolant is a choice, not a default. Aluminum likes flood coolant or a mist. Stainless needs flood to carry heat away and break chips. Cast iron is usually cut dry because the graphite dust turns coolant into a sludge. Titanium needs high-pressure through-tool coolant, or the heat stays in the cut and the edge fails in minutes.

Watch the spindle load meter on the first pass. If it sits below 40 percent, you are leaving money on the table. If it spikes past 85 percent on entry, back off the feed before the tool breaks. The load meter is the fastest feedback you have, faster than any calculator.

Every cut pushes back on the part. A vise with 2 mm of grip on a 50 mm block will lift the part on a heavy face mill pass. We aim for at least 4 to 6 mm of jaw engagement on steel, more on aluminum. Parallels should be tapped down so the part sits flat, and the vise should be dialed in to within 0.01 mm before the first tool touches metal.

Thin walls are the classic failure. A 1.5 mm wall in aluminum will bow under clamping pressure and spring back after unclamping. The fix is to leave a roughing allowance of 0.3 to 0.5 mm, release the clamps, let the part rest, then take a light finishing pass at 0.1 to 0.2 mm radial engagement. Skip the rest step and the wall measures differently in the vise than on the granite plate.

For 5-axis work, the rotary table adds a second setup axis. We indicate the table center and set the work offset once, then let the CAM post handle the rotations. A Ø400 mm rotary table covers a lot of parts, but the part still has to clear the table and the spindle nose at every angle. Check the collision model before you run the program, not after.

First-article inspection is not optional on tight work. We cut one part, measure the critical features, and adjust the wear offset before running the rest. On a ±0.005 mm job, a 0.008 mm drift on the first part means the whole batch is at risk. Ten minutes of measuring saves a scrapped run.