CNC Machining

The short answer

Three jobs, three tools

The three operations are separated by what each one is allowed to change. A twist drill creates a hole in solid stock and removes the bulk of the material quickly, but it follows its own deflection: the hole it leaves is usually slightly oversize, slightly tapered and not perfectly round, and its position depends on the entry. A boring bar is a single-point tool mounted on a rigid bar, so its diameter can be adjusted on the machine and it is aligned to the intended centreline; that means boring can correct the position and straightness of a hole that drilling has already produced. A reamer is a multi-flute finishing tool of fixed diameter that removes a small, even allowance and produces a very consistent round hole; what it cannot do is change where the hole is. Understanding that one distinction, boring changes geometry and reaming only changes size, prevents most of the arguments between a designer and a machine shop.

Tolerances and surface finish side by side

Drilling alone is a clearance-grade process. It lands somewhere in the IT12 to IT14 range with surface finish around Ra 3.2 to 12.5 micrometres depending on the feed, the drill quality and whether the chips cleared; that is perfectly adequate for a fastener hole, a cable route or a drain. Boring takes the same hole to IT7 to IT9 and Ra 0.8 to 3.2 micrometres, and because the size is set by the operator rather than by the tool it also handles diameters for which no standard reamer exists. Reaming holds IT6 to IT7 with Ra 0.4 to 1.6 micrometres and is the standard answer for a dowel hole, a bearing seat or an H7 press fit. The weakest common specification is an H7 callout on a hole that only ever sees a bolt pass through it: forcing a reaming operation onto every hole on a bracket adds roughly 1.5 to 2 times the machining cost for no functional benefit at all.

Why boring can fix a hole and reaming cannot

A reamer has no independent way to find the centre of the hole it is entering: it follows the path the drill left behind, so if the hole is off position or tapered, the finished hole is off position and round but off position. A boring bar is set on the machine's own axis, so the first pass removes the high side of an eccentric hole and the hole moves towards the true centreline. That is why the practical sequence for a tight bore is drill, then bore to correct and roughly size, then ream or fine-bore to the final figure. It is also why reamers are a poor choice for interrupted cuts such as a cross-drilled hole, and why they must not be asked to remove a heavy allowance: reaming more than about 0.3 mm on diameter overloads the flutes and produces the bell-mouthed hole that everyone then blames on the operator.

Stock allowance, entry and blind holes

Leave the sizing tool a predictable amount of material rather than a generous one. For reaming, 0.10 to 0.30 mm on diameter is the normal allowance, and the pre-drill should be about 0.2 to 0.3 mm under the reamer size; for boring, aim to come within 0.05 to 0.10 mm of the final diameter. A reamer needs a chamfered lead-in at the entry and either a through exit or an undercut at the bottom, so a genuinely blind precision hole is usually bored rather than reamed. Where a blind hole must be reamed, the drill depth has to be set deeper than the reamed depth to leave room for the chips and the tool nose. Standardising on the sizes your shop already stocks for drills and reamers avoids the lead time and cost of special tooling, and if a non-standard diameter has to hold a tight tolerance, boring is the cheaper route.

Deep holes change the rules

Up to about five times the diameter, a standard drill behaves acceptably. Beyond that, drill deflection grows, chips have a long way to travel and heat builds up, so the hole drifts, tapers and comes out rough; peck drilling cycles and high-pressure through-coolant flushing are the minimum counter-measures above a depth-to-diameter ratio of about four to one. Where both depth and accuracy are needed, gun drilling with a single-flute tool and internal coolant delivery holds roughly twenty times diameter or more and reaches tolerance bands well under what standard drilling can manage. Deep-hole work is also where the sequence matters most, because a defect created at the entry is amplified all the way to the bottom and no later operation can bring a curved hole back to a straight line.

What to put on the drawing

Specify the tolerance and the finish you actually need, and specify them on the hole diameter only where it matters. Give the depth with a clear reference face, because hole depth measured from a rough casting face is a different hole from one measured from a machined datum. State whether the hole must be round, straight or concentric, since reaming will satisfy the first and boring is required for the others, and name the inspection method: a plug gauge, a bore gauge and a CMM can differ by more than a fine tolerance, and the difference is discovered at goods-in rather than in the drawing office. Wall thickness and hole-to-edge distance matter too, because a hole placed within about two material thicknesses of an edge will bulge or tear the edge during machining. Finally, say how many holes are involved, because the cost of a finer process is multiplied by every hole on the part.

See CNC machining services for drilled, bored and reamed holes quoted from your drawing, metal stamping for punched holes at production volume, and die casting for holes that are cast in and then finished by machining.

The short answer

Why copper hardens under the tool

Work hardening, also called strain hardening, happens when the cutting edge deforms the metal instead of shearing it. Copper has a face-centred cubic lattice with many slip systems, so dislocations move easily and pile up against each other quickly; the result is a thin layer at the surface that is harder, stronger and far less ductile than the metal underneath it in a single pass. Once that layer exists, the next pass finds a harder material, and a tool that is slightly dull simply polishes it and hardens it further. This is why copper rewards a decisive cut and punishes a timid one: the classic mistake is to slow the feed and take a light pass, which converts a cutting operation into a rubbing operation and makes the problem worse on every subsequent pass.

Alloys that machine cleanly and alloys that fight back

Pure copper C11000 is the worst offender and it is also the grade most often specified, because it has the highest electrical and thermal conductivity. Alloying is the easiest fix. Free-cutting brass C36000 contains zinc and lead that break up the lattice and stop the chips from welding, which is why it is the benchmark material for machinability. Tellurium copper C14500 keeps conductivity close to C11000 but machines far more easily because the tellurium inclusions break the chip. Beryllium copper C17200 is a different problem: it is strong and abrasive, so it needs slower speeds and a very rigid setup rather than clever chip control. If a drawing says pure copper and the part is a prototype, it is worth asking whether a free-machining grade would do the same job.

Cutting parameters that avoid the hardened skin

The single most important number is not speed but depth of cut. To cut below any layer that has already been hardened, the tool needs a minimum depth of about 0.13 mm per pass, and 0.2 to 0.4 mm is a comfortable working range for copper in a rigid setup. Feed should also be generous for the material, in the region of 0.03 to 0.05 mm per tooth on a cutter, or roughly 0.1 to 0.3 mm per revolution when turning, because thin chips bend the edge and rub instead of shearing. Cutting speed is then set to control heat rather than to control the cut: as a first cut, around 150 to 200 m/min works for C11000, 200 to 350 m/min for the tellurium grades and C10300, and 250 to 300 m/min for free-cutting brass on uncoated carbide. Tool life improves markedly if the speed is pulled back rather than pushed up when the edge starts to wear.

Tool geometry, coating and coolant

Use a tool with a sharp, high positive rake and a polished flute surface so the chip slides away rather than welding to the edge. Uncoated carbide and PVD-coated carbide both work; on copper, thick coatings are counter-productive because the soft workpiece pulls coating particles off the edge, and polycrystalline diamond is reserved for high-volume work where its hardness justifies the price. A fine edge hone of about 0.005 to 0.01 mm keeps the edge sharp without leaving it fragile. Coolant is not optional: flood the cutting zone generously, and for copper a chilled water-based fluid delivered through the spindle at around 16 to 18 degrees Celsius keeps the edge temperature stable and stops heat-driven hardening. Oil-based fluids can stain copper and encourage chip adhesion, so a water-soluble or a minimum-quantity vegetable-based lubricant is the safer choice.

1. Take a decisive depth of cut so the edge bites below the surface layer instead of riding on it.
2. Feed generously enough for a chip that curls and breaks rather than one that smears.
3. Keep the tool sharp; a dull edge is the fastest way to raise the local hardness.
4. Flood the cut, and keep the fluid cold on the grade that hardens fastest.
5. Use climb milling on profiles so the cutter shears from the thick part of the chip, and keep overhang short.
6. Grip with soft jaws; copper marks and deforms easily and a crushed surface is a hardened surface.

Deburring, and when copper needs a stress relief

Copper produces tough, tenacious burrs that survive a light brush and smear if you attack them mechanically. Thermal energy deburring or cryogenic tumbling handles complex parts without smearing the edges, and on simple parts a controlled handheld or abrasive-flow operation is enough; the point is to finish the edge without cold-working the faces around it. Dimensional stability is the other end of the same problem: heavy material removal leaves residual stress in the part, and a thin-walled copper busbar can creep out of flatness weeks after delivery. Where stability matters more than cycle time, a low-temperature stress relief at roughly 205 degrees Celsius before final finishing puts the part back into a predictable state.

See CNC machining services for the turning and milling work we quote on copper grades, surface finishing for the plating, tinning and passivation routes that follow machining, and metal stamping for copper busbars and contacts that are formed rather than cut.