CNC Machining

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.

The short answer

The default is a standard, not a number

When a drawing does not put a tolerance on a dimension, the shop still has to make a decision, and ISO 2768 is the decision. Part one of the standard covers linear and angular dimensions in four classes, fine, medium, coarse and very coarse, and part two covers straightness, flatness, perpendicularity and symmetry in classes H, K and L. The block that appears on most CNC drawings is ISO 2768-mK, medium linear tolerance with K geometric tolerance, and it represents the natural economic capability of a modern machining centre rather than a compromise.

The size dependence is the point that surprises many buyers. A medium-class tolerance is 0.1 mm on a 10 mm feature and 0.5 mm on a 300 mm feature, because the same absolute error on a long dimension is a much smaller fraction of it. That is also why demanding a blanket plus or minus 0.05 mm across a 250 mm part is expensive: it forces multiple finish passes, thermal stabilisation and full CMM verification on dimensions that may not matter at all.

Three tolerance tiers and what each costs

Above the standard classes sits a set of named machining tiers, and it is worth separating them from the ISO block because they describe what a machine and a process can hold rather than what a drawing inherits. Standard machining holds roughly 0.1 to 0.2 mm on a general feature. Precision machining, on a calibrated machine with a dedicated finishing pass, holds 0.025 to 0.05 mm and is what a bearing bore or a sealing face usually needs. Tight tolerance machining reaches 0.005 to 0.01 mm and needs thermal stabilisation, in-process touch probing and full CMM verification. Ultra precision below that is a different industry, served by diamond turning or jig grinding in a climate-controlled room.

Cost does not rise linearly across those tiers. As a rule of thumb, specifying one class tighter than the part needs adds 30 to 50 percent to the unit price, because the shop has to slow the cut, add passes and add inspection. The same logic explains the title-block contradiction that costs buyers money: a drawing that states ISO 2768-mK but also carries a note demanding plus or minus 0.05 mm on every dimension forces the tighter reading, and estimators commonly add a 30 to 45 percent buffer to the price to protect against incoming inspection. One clear general-tolerance rule and specific callouts on the features that matter is cheaper and clearer than a blanket tight number.

Geometric tolerances are a separate standard

Dimensional tolerance says how big a feature may be; geometric tolerance says how straight, flat or square it must be. ISO 2768-2 covers this with classes H, K and L, and the numbers are small: flatness for a feature under 10 mm is 0.02, 0.05 and 0.10 mm across the three classes, rising to 0.10, 0.20 and 0.40 mm for a feature from 30 to 100 mm, and perpendicularity is 0.2, 0.4 and 0.6 mm up to 100 mm of the shorter side. On a machined part the geometric callout is often the one that decides whether the part assembles, because two faces can both be within their size tolerance and still not meet.

One geometric convention is worth a note because it changes what a shop can hold without changing the function. A hole position written as plus or minus coordinates creates a square tolerance zone, while the same requirement written as a true position with a diameter creates a round one. Because the diagonal of the square is longer than its side, converting to a cylindrical zone increases the allowable area by about 57 percent, giving the machinist real margin without loosening the fit. That is a design edit that costs nothing and buys process capability.

Surface finish is quoted in Ra, and it multiplies cost

Finish and tolerance are separate requirements that are frequently confused. Surface finish is given as Ra, an average roughness in micrometres, and it is set by feed rate, tool condition and the number of passes rather than by the machine's positioning accuracy. Standard milling leaves Ra 3.2 micrometres, which suits most non-functional faces. A dedicated finishing pass reaches Ra 1.6; reaching Ra 0.8 usually needs grinding or high-speed milling with a specific tool; and Ra 0.4 needs a secondary grinding or lapping operation.

The cost lesson here is about scope. A part might need Ra 0.8 on a sealing surface and nothing better than Ra 3.2 anywhere else, and the economical route is general machining for the bulk of the part with a local finishing pass confined to the sealing area. Specifying the finer finish across every face is one of the more avoidable cost mistakes in this category, because each step down the Ra ladder requires slower cutting, more passes or a different process entirely.

What drives a shop above or below its brochure figure

• Machine positioning is the ceiling. A well-maintained three-axis vertical machining centre holds roughly 0.0127 to 0.0254 mm across its travel with repeatability near 0.005 mm; five-axis and high-speed machines do better on the same part, but only if the fixture is equally good.
• Aluminium moves three times as much as steel. Under the same cutting force an aluminium feature deflects about three times as far, and its thermal expansion coefficient, 23.1 parts per million per kelvin, is more than double that of carbon steel, so thin walls and long parts need control that a brochure figure ignores.
• Every re-clamp adds error. A part machined in three setups carries the tolerance of three fixtures, which is why five-axis work often holds a tighter feature-to-feature tolerance than the individual machine accuracy suggests.
• Inspection decides the honest number. A tolerance is only real if it is measured; ask for a first-article CMM report and confirm which features were checked, not just that the report exists.
• General tolerances do not cover fits or threads. ISO 2768 does not set a shaft fit, a thread class or a feature-specific control, so those still need an explicit callout.
• A blanket tight note is a cost, not a benefit. Tightening a non-functional dimension buys nothing and slows the cut.

How to write a drawing that gets the tolerance you need

Put one general-tolerance block in the title area, normally ISO 2768-mK, add explicit callouts only on the features whose function depends on them, mark which dimensions are functional and which are reference, and state the finish per surface rather than per part. Then send the STEP model, the drawing, the material and the annual quantity. That set lets an engineer tell you which features can be milled in one setup and which will need a controlled process. See CNC machining for the capability, surface finishing for the finishes below Ra 0.8 and aluminium die casting where a cast body plus a light machining pass is the cheaper route at volume.