Milling and drilling are both cutting processes that use a rotating tool. They are not interchangeable operations. Drilling feeds a tool along its own axis to make a round hole. Milling moves a multi-edge cutter sideways as well as axially, so it can make flats, pockets, slots, contours, and—when programmed that way—holes.
On a CNC machining center the two operations often live in the same program. The useful distinction is the tool motion and the geometry each motion can produce, not the name of the machine.
What Each Process Does
Drilling uses a drill (twist drill, indexable drill, or similar) that cuts primarily at the point and along the margins. The tool rotates and feeds into the work along the tool axis, usually Z. The result is a cylindrical hole whose diameter is set by the tool. Depth is set by the feed distance. Chips leave up the flutes.
Milling uses an end mill, face mill, or similar cutter with cutting edges on the periphery and often on the end. The tool rotates while the machine interpolates X, Y, and Z. Side cutting makes walls and slots. End cutting makes floors. Combined motion makes pockets and 3D surfaces.
A drill is a hole-making tool. A mill is a shaping tool that can also make holes if the path is a plunge or a helix.
Tool Motion and Chip Formation
Drilling is an axial process. Almost all of the work happens at the point. The web of the drill is inefficient at the center, so thrust is high and heat concentrates in the hole. Peck cycles (commonly G83-type) break chips and clear the hole on deeper holes. The wall of a drilled hole is generated by the margins and lands, not by a programmed contour.
Milling is a peripheral and/or end-cutting process. Chip thickness depends on feed per tooth, radial engagement, and whether the path is climb or conventional. The machine can change hole size without changing tools by interpolating a larger path. That is why milling can make non-round openings and large bores that no standard drill covers.
This is also why a milling machine can drill, but a dedicated drill press or gang drill cannot mill a pocket. The mill has the extra axes. The drill does not.
Making Holes: Drill, Ream, Bore, or Mill
A round hole does not automatically mean “use a mill.”
- Drill when the hole is a standard diameter, depth is reasonable, and positional tolerance is within what a drill and a good location cycle can hold. It is usually the fastest way to remove the core of a hole.
- Peck drill when chips pack or the hole is deep relative to diameter.
- Ream after drilling when diameter and finish must be closer than a drill leaves.
- Bore when the hole must pick up a true position or a diameter that a reamer cannot correct well, or when the hole is large.
- Helical mill (circular interpolation with an end mill) when the hole is large or non-standard, when one tool must make several diameters, when a flat-bottom hole is required, or when a slot-mill or end mill is already in the spindle and a separate drill is not worth the tool change.
Helical milling a small, deep, standard hole is usually slower than drilling it. Drilling a shaped opening is impossible. Choose the motion that matches the feature, not the process that sounds more “CNC.”
What Each Process Cannot Do Well
Drilling does not create pockets, profiles, or flat floors except the conical or slightly concave bottom a drill point leaves. It does not correct a hole that is already off location except within the small amount a following bore or reamer can shift. Deep holes need chip-clearing strategy; a single plunge will pack flutes.
Milling is a poor first choice for a dense pattern of identical small holes. Each helical hole costs path time and tool wear that a drill cycle would not. Long, small-diameter holes favor a drill’s geometry and chip evacuation. Milling also does not automatically hold a tighter hole than drilling; an interpolated bore is only as good as the tool, the path, and the machine’s circular accuracy.
Typical Roles on One Part
Most prismatic parts use both. Faces, pockets, and profiles are milled. Fastener holes are drilled, then tapped or reamed if the fit requires it. Large bearing bores may be milled or bored. The program sequence is usually mill the datums and bulk features first, then drill, so hole location is taken from finished faces rather than from raw stock.
Treating milling and drilling as competing vendors is the wrong frame. On a machining center they are two tool groups in one setup. A dedicated CNC drill or multi-spindle drill earns its place when the part is mostly holes and volume is high enough that a mill’s extra axes add cost without adding features.
Selection Rules
- If the only features are round holes of catalog diameters, drill (and ream or tap as required).
- If the part needs pockets, slots, bosses, or profiles, mill those features; drill the holes in the same setup when that is faster.
- If the opening is not round, or the diameter is between standard drills, mill it.
- If hole location must match milled datums tightly, keep drilling on the same machining-center setup rather than moving to a separate drill press.
- If the hole is deep and small, prefer a drill and a peck cycle over a long helical path with a small end mill.
- Do not specify “mill all holes” or “drill all holes” on a drawing. Specify diameter, depth, tolerance, and bottom condition; let process planning pick the tool.
Milling vs drilling is a motion-and-geometry choice. Use drilling to make round holes efficiently. Use milling services to shape the part and to make holes that a drill cannot.
