Milling Foundation 101: How a Rotating Tool Cuts Metal

• 1
  Key takeaways
• 2
  What actually happens at the cutting edge
• 3
  How the axes change what a part can look like
• 4
  Tool choice sets radii, finish and cycle time
• 5
  Material behavior on the mill
• 6
  Workholding and the real tolerance floor
• 7
  Which milling setup fits the part

Milling is a chip-formation process. A cutter with multiple teeth spins at a set surface speed, and each tooth shears off a chip as it enters the material. The workpiece is clamped to a table or a fixture and stays still while the tool moves along programmed paths. Nothing is melted, stamped or built up. Material is removed, and the final shape is whatever the tool left behind.

Three numbers govern every cut: cutting speed, feed per tooth and axial depth. Cutting speed is the surface speed at the tool edge, usually 100–400 m/min in aluminium and 20–60 m/min in stainless. Feed per tooth is how far the tool advances per edge, commonly 0.02–0.15 mm. Depth is how much the tool bites in one pass.

Those three values trade against each other. Push the speed and the tool wears. Push the feed and the surface finish roughs up. Push the depth and the spindle loads up, which shows on thin walls as chatter marks. The operator's job is to find a combination that keeps the tool alive, holds size, and finishes the part in a reasonable cycle time.

Heat is the other half of the story. Most of the heat leaves with the chip, but some goes into the tool and some into the part. On a long finishing pass in titanium, the part can grow enough to move a tight dimension. That is why roughing and finishing are kept separate, and why a spring pass often follows a heavy cut.

• 1
  Climb millingTool tooth enters at maximum chip thickness; standard on modern CNC mills.
• 2
  Conventional millingUsed mainly for rough castings or when backlash cannot be controlled.
• 3
  Chip evacuationAir blast or flood coolant keeps recut chips from dulling the edge.

A 3-axis mill moves X, Y and Z. The tool always comes down from one direction. To machine a second face, someone must unclamp the part, turn it, and re-zero it against a datum. Each of those setups adds time, and each adds a small positional error that stacks into the finished part.

A 4-axis mill adds a rotary table, usually around X. This lets a shaft-like part be indexed to several faces without a human touching it. A Ø400 mm rotary table is enough for most pump housings, manifolds and drive shafts. The limitation is that the rotary axis indexes rather than follows a contour.

A 5-axis mill moves the tool or the table on two rotary axes at the same time. That lets the cutter stay normal to a curved surface, which keeps the effective tool radius constant and the finish even. It also reaches undercuts, angled holes and deep pockets that a 3-axis machine cannot touch without a special fixture.

The trade is not free. Simultaneous 5-axis paths need more programming, more simulation, and a machine that can hold position while two axes move at once. On a simple plate with holes, 3-axis is faster and cheaper. On an impeller or a bone plate with compound angles, 5-axis is often the only way to hold the drawing.

• 1
  3-axisFlat plates, pockets, drilled holes, one or two faces.
• 2
  4-axisCylindrical parts, slots around a bore, indexed faces.
• 3
  5-axisContoured surfaces, undercuts, angled ports, single-setup complex parts.

The single most common design mistake is asking for an internal corner sharper than the cutter can leave. A pocket cut with a Ø6 mm end mill carries a 3 mm corner radius. If the drawing calls for a 0.5 mm corner, the shop must switch to a small tool, run it slowly, and often break one or two in the process. Cost climbs fast.

Flat end mills leave a stepped floor if the tool has a corner radius. A bull-nose cutter with a small corner radius blends the floor and the wall, which reduces hand work on moulds and housings. Ball nose cutters are for contoured surfaces; they leave a scallop pattern whose height depends on stepover, and that pattern must be polished out if the surface needs to be smooth.

On aluminium, two- and three-flute cutters clear chips well and run at high speed. On stainless and titanium, more flutes and slower surface speed keep the heat down and the edge alive. On plastics, a single-flute cutter with a polished flute reduces melting and stringy chips. The right tool for the material is not optional.

Reach matters as much as diameter. A long, thin cutter deflects under load. If a pocket is 60 mm deep and the cutter is Ø6 mm, the tool sticks out at least 70 mm and will bend. The fix is either a wider pocket floor, a shorter depth, or a design change that lets the shop use a stiffer tool from both sides.

• 1
  Minimum internal radiusMatch it to the largest cutter that can still reach the feature.
• 2
  Floor-to-wall blendA 0.5–2 mm corner radius on the cutter saves hand finishing.
• 3
  Aspect ratioKeep tool length under 5× diameter where the drawing allows.

Aluminium 6061 and 7075 cut freely and hold tight tolerances. They are the default for prototypes and for housings that need anodizing. 7075 is stronger but less weldable and slightly more prone to stress movement, so a heavy roughing cut on a thin wall can warp the part before finishing starts.

Stainless 303 machines well and is common for shafts and fittings. 304 and 316 work-harden, so a cutter that rubs instead of cutting will glaze the surface and dull quickly. 17-4PH holds strength after heat treatment and is used for medical and aerospace parts where corrosion resistance and hardness both matter.

Titanium Ti-6Al-4V and Inconel cut slowly and generate heat at the edge. Tool life is measured in minutes, not hours, and the shop plans extra passes to protect the cutter. These materials are chosen for the service environment, not because they are easy to machine, and the cost of the part reflects that.

Plastics behave differently again. POM and PEEK machine cleanly but expand with heat, so a dimension measured right after the cut can read small. ABS and PC are softer and prone to burrs. Carbon fibre wears tools fast and needs dust extraction. Each family has its own feeds, and a general-purpose program will not work across all of them.

• 1
  Free-cutting6061, 7075, 303, brass C36000, POM.
• 2
  Work-hardening304, 316, 17-4PH; keep the cutter moving, never rub.
• 3
  Heat-sensitiveTi-6Al-4V, Inconel, PEEK; low speed, high coolant, sharp edge.

A part is only as accurate as the way it is held. Vises are fine for blocky parts, but a thin plate will bow when the vise closes and spring back when it opens. Vacuum chucks and dedicated soft jaws spread the clamping load. For a part with a 2 mm wall, the fixture design is often more work than the toolpath.

Tolerance is a budget, not a wish. A general milled feature can hold ±0.05 mm without much fuss. Tightening to ±0.005 mm is possible, but it needs a stable setup, a warm machine, a sharp tool and an operator who checks the feature while it is still in the fixture. Spending a tight tolerance on a cosmetic face wastes money.

Surface finish follows the same logic. As-machined faces land at Ra 1.6–3.2 μm. A careful finishing pass reaches Ra 0.8–1.6 μm. Below Ra 0.8 μm, the shop usually adds a secondary operation such as lapping or polishing, because a milling cutter leaves a periodic pattern that no feed rate can fully remove.

Inspection closes the loop. A 100% check before shipment catches a drifted dimension before it leaves the building, but it cannot fix a drawing that asks for two tolerances the process cannot hold at the same time. When a print has conflicting callouts, the fastest route is a short call between the designer and the shop before the first cut.

• 1
  Thin wallsBelow 1 mm, expect multiple light passes and a custom fixture.
• 2
  Deep pocketsAdd corner radii and draft where the function allows.
• 3
  DatumsPick datums the shop can reach in the first setup.