What types of holes and threaded features can be created with CNC drilling services?

The short answer

Every hole starts as one of seven feature types

Holes are the most common machined feature and the easiest to over-specify. Each type below exists for a reason, and each one adds a tool and an operation to the price. A through hole drilled in a single pass is the cheapest hole you can buy; a reamed fit is roughly one and a half to two times the cost of the same hole drilled, because it needs a second tool and a second pass.

Two of these are worth a second look. A spotface exists only because a cast or forged surface around a hole is not flat enough to seat a fastener reliably, so leaving it out is a real risk on a rough surface and a waste of money on a machined one. A blind hole is more than a shallow through hole: the twist drill leaves a conical bottom, so the drawing has to allow for the drill point as well as the depth, and the chips have to evacuate upward through the flutes.

Counterbores, countersinks and spotfaces: the three fastener seats

These three features are the most confused in incoming drawings, and they are not interchangeable. A counterbore is a flat-bottomed cylindrical recess that hides a socket head cap screw so the head sits below the surface; its diameter has to clear the head and its depth has to be at least the head height. A countersink is a conical recess matched to the angle of a flat head screw, usually 82 or 90 degrees, and an angle that is one degree out will show as a screw head that sits proud on one side. A spotface is a shallow flat cut, not a recess, used where a washer or a nut has to seat on a surface that is otherwise rough or out of flat.

All three need a second tool after the drilling pass, and the cost shows up as cycle time rather than as tooling. Where several of them appear on one part, the machining centre makes repeated tool changes, so consolidating a drawing to one screw type across a face is often the cheapest single edit a designer can make.

Threaded features: standards, classes and depth rules

Threads are cut either by tapping, which cuts a thread into a pre-drilled hole with a tap, or by thread milling, which cuts the thread with a rotating mill on a machining centre. Tapping is faster and cheaper for standard sizes; thread milling produces a better thread and can reach closer to the bottom of a blind hole, which is why it has grown in use on deep and precision threads. The standards that appear most often are UNC and UNF from the unified series, metric coarse and fine, NPT for pipe threads and BSPT for the equivalent British standard.

Three rules cover almost every threaded callout. First, specify diameter, pitch, class of fit, thread depth and total hole depth separately, because a note that says only "M6 threaded hole, 12 deep" leaves both the pitch and the thread-versus-hole distinction undefined. Second, allow at least one and a half times the nominal diameter of extra hole depth beyond the last full thread, so the tap can bottom out without damaging the thread it has just cut. Third, use the standard classes: a 2B or 6H fit is the normal choice for a fastener, and a tighter 3B class is reserved for applications that actually need it.

Precision bores: reaming, boring and gun drilling

When a hole has to hold a shaft, a bearing or a dowel pin, drilling alone will not do it. A drill produces slight ovality and size variation that a fit class will not tolerate, so the bore is drilled undersize and finished with a reamer, which brings the diameter to 0.005 to 0.02 mm and the finish to around Ra 0.4 to 1.6 micrometres. Larger bores are finished with a single-point boring bar instead, which can correct position and straightness as well as size and reaches much deeper. Genuinely deep, straight holes are made on a gun drilling machine, which produces the oil galleries and cooling channels that a twist drill cannot follow over that length.

The smallest hole each process can make is a practical limit rather than a theoretical one. A standard twist drill works down to roughly 0.5 mm, a reamer down to about 1 mm, a gun drill to about 2 mm, and small-hole EDM to about 0.1 mm. Below 2 mm in stainless steel or titanium, drills become fragile and break more often, so peck cycles and carbide micro-drills are the normal answer and wire EDM is sometimes the cheaper route once breakage is counted.

Depth-to-diameter ratios decide the process

The single number that decides whether a hole is routine, awkward or specialist is its depth divided by its diameter. A standard twist drill is comfortable to 5 to 8 times diameter; past that, chip evacuation rather than the spindle becomes the limit, and peck drilling with reduced speed is the usual answer. Reaming works from 10 to 15 times diameter, boring from 20 up to 50, and gun drilling from 100 to 150 times diameter on a dedicated machine. Deep holes on a machining centre without through-tool coolant are the routine way to break a drill.

Where the feature list runs out

• True position drives cost more than diameter. A pattern with a tight positional callout needs precision fixturing and CMM verification, and that cost is set by the tolerance, not by the number of holes.
• Thread depth beyond about three diameters is a risk. Tap breakage rises with depth, small threads carry more risk than large ones, and a broken tap in a finished part is often a scrap decision.
• Very small holes in hard material are fragile. Below 2 mm in stainless or titanium, expect higher tool breakage and slower feeds than the diameter suggests.
• Sharp-bottomed blind holes are not a drill feature. The 118 degree point leaves a cone, so a flat-bottomed blind hole needs a second operation or a specific callout for the flat depth.
• Gun drilling is not universal equipment. Where a hole needs a 100 to 1 ratio, confirm that the shop owns the machine rather than subcontracting it, because the subcontract adds days and splits accountability.
• Cross-drilled intersections change the pressure story. Where two holes meet inside a part, the intersection is where a leak or a burr hides, and it needs an explicit inspection step rather than a general note.

How to specify holes and threads on a drawing

Send the STEP model and a drawing with every hole called out by diameter, depth, feature type, thread class and positional tolerance; list the material; mark the two or three holes whose position is functional; and state the annual quantity. That is enough for an engineer to choose between drilling and reaming, to size the peck cycles and to tell you which features should be milled and which cast or left as-drilled. See CNC machining for the process, surface finishing for what happens after the hole is cut and metal stamping where a pierced hole is the cheaper route at volume.