Internal CNC Machining Services: 7 Checks Before You Choose a Shop

• 1
  Key takeaways
• 2
  Internal feature, process and what to check
• 3
  What internal CNC machining actually covers
• 4
  Depth-to-diameter ratio and the tooling behind it
• 5
  How to read a tolerance and finish callout on an internal feature
• 6
  Inspection: the step most quotes skip
• 7
  Materials, finishes and internal features that fight back
• 8
  Machine choice: when 3-axis is enough and when it is not
• 9
  Seven steps to qualify a shop for internal CNC machining

Internal CNC machining is every operation that cuts the inside of a part. Deep hole drilling, boring, reaming, internal threading, pocketing, internal grooving, splines and cavities. External profiles are usually a single pass with a large cutter. Internal work uses small tools on long holders, so rigidity drops and deflection climbs.

The reason this matters commercially is simple. A shop can turn an external profile on almost any 3-axis mill. Internal features are where capability separates. A Ø6 mm bore, 60 mm deep, at Ra 0.8 μm needs through-tool coolant, a rigid holder and an operator who checks the taper before the part leaves the machine.

Internal features also drive function. Hydraulic manifolds seal on bore roundness. Fuel injector bodies meter flow through hole diameter. Medical instruments pass through internal lumens that must be burr-free. Robotics actuators rely on internal splines to transmit torque without backlash. Get the inside wrong and the part fails in service, not on the bench.

We cut internal features on 16 simultaneous 5-axis centers, 16 mill-turn centers and 27 three-axis machines. For parts up to 4,000 mm we use the large gantry travel. For small, deep work the compact platforms hold tighter geometry because the spindle is closer to the cut.

• 1
  Internal, not externalBores, threads, cavities, grooves and splines are the internal set.
• 2
  Rigidity is the limitLong, thin tools deflect. Depth-to-diameter ratio predicts the risk.
• 3
  Function follows geometrySealing, flow and torque all depend on internal dimensions.

Take the hole depth and divide by the diameter. Under 4× is routine on a milling machine. Between 4× and 8× you need through-tool coolant above 40 bar, a peck cycle and a boring head that reaches full depth without chatter. Past 8× the process changes: gun drilling, or milling from both ends with a reamed pilot.

The practical failure mode is drift. A long drill wanders, and the exit position moves. If the hole is a dowel pin bore, that error kills assembly. Shops that run deep work quote a straightness value, not just a diameter tolerance. Ask for it.

Threads have their own ratio. A form tap needs a hole diameter matched to the material. In 304 stainless a form tap that works in 6061 aluminium will seize. Thread milling is slower but gives a cleaner flank and works when the thread sits near a shoulder or a cavity floor.

Internal grooving bars are the tool most often missing from a small shop's cabinet. A groove 2 mm wide at the bottom of a Ø20 mm bore needs a bar with a head small enough to enter and stiff enough not to chatter. If the shop has to order the bar, your lead time is the tool delivery, not the cut.

• 1
  Under 4×Standard milling with a boring head and a finish pass.
• 2
  4× to 8×Through-tool coolant, peck cycle, taper check.
• 3
  Over 8×Gun drilling or two-sided milling with a pilot.
• 4
  Threads near shouldersThread mill, not a tap, to avoid collision.

A drawing that says Ø12 H7 tells the shop the bore must land between 12.000 mm and 12.018 mm. That is achievable on a boring head with a finish pass. A drawing that says Ø12 ±0.005 mm across a 90 mm deep bore is a different job. It needs a rigid bar, a temperature-stable shop and an in-process probe.

Surface finish matters more inside than outside. A bore at Ra 3.2 μm may seal, but a dynamic bore running against an O-ring or a piston usually wants Ra 0.8–1.6 μm. For hydraulic and pneumatic sealing surfaces we work down to Ra 0.2–0.8 μm where the drawing calls for it. Below that, honing or internal grinding is the right process, not milling.

Position tolerance is the callout buyers forget. A pattern of internal holes referenced to a datum face needs a true position value, often Ø0.05 mm or tighter. Without it, the shop has no way to fixture the part for the second operation. Send the GD&T frame, even on a prototype.

Our standard machining tolerance is ±0.005 mm (±0.0002 in) on features we can reach with rigid tooling. We say 'we can reach' because depth, tool reach and material all shift the number. A shop that quotes one tolerance for every internal feature is quoting a wish.

• 1
  Bore toleranceH7 fits are routine; ±0.005 mm needs rigid tooling and probing.
• 2
  Sealing surfacesRa 0.8–1.6 μm typical; Ra 0.2–0.8 μm for critical seals.
• 3
  Position mattersTrue position to a datum controls the second operation.

You cannot measure a Ø4 mm bore, 40 mm deep, with calipers. The jaws do not reach and the reading is meaningless. Internal features need bore gauges, plug gauges, air gauges, or a CMM with a custom stylus and fixture. Each of those is a cost line in the quote, and a shop that leaves it out is either absorbing it or skipping it.

Thread quality is verified with go/no-go gauges at the pitch diameter, plus a visual check on the flank. For medical and aerospace work, thread inspection records travel with the part. For general industrial work, a gauge pass is usually enough. Decide which one your drawing requires before you ask for price.

Burrs are the silent defect. A cross hole intersecting a main bore leaves an internal burr that a deburring tool must reach. If the intersection is 80 mm inside the part, the shop needs a long-reach deburring tool or an abrasive flow process. Ask how they plan to remove it.

GreatLight inspects 100% of parts before shipment. That covers raw material check, in-process monitoring and final inspection, with reports on request. Our historical qualification rate is 99.99%. For internal features we treat the first article as the gate: if the bore tapers or the thread gauge drags, the process changes before the run continues.

• 1
  Right gauge, right featureBore gauges and air gauges for small deep bores; go/no-go for threads.
• 2
  Burr plan upfrontAsk how internal intersections will be deburred at depth.
• 3
  First article gates the runTaper or gauge drag stops the batch before it scales.

Aluminium 6061 and 7075 cut clean internal threads and hold good finish. 7075 is stronger but more prone to chip welding on deep bores, so coolant pressure and peck depth matter. We keep 6061-T6, 2024, 5052, 5083, 6063, 6082 and ADC12 in the aluminium set.

Stainless 304 and 316L work-harden. A form tap that runs fine in aluminium will bind and snap in 304 unless the hole diameter and speed are right. 17-4PH in the H900 condition machines well but needs sharp tooling to avoid a smeared bore. Titanium TC4 (Ti-6Al-4V) and Inconel are a different class again: low speeds, high coolant volume and generous tool changes.

Plastics have their own rules. PEEK and POM move with temperature, so a bore measured hot will not match the cold drawing. ABS, PC, PMMA, PA, PP and HDPE need sharp tools and air blast rather than flood coolant to avoid swelling. Carbon fibre needs diamond tooling to stop delamination at the bore edge.

Finishes change internal dimensions. Anodizing adds a few micrometres; hardcoat adds more. Electroless nickel and plating build up on the bore wall. If the bore is a press fit, tell the shop the final dimension after finishing, not the machined dimension. For laser marking inside a cavity, the minimum character height is 1.5 mm.

• 1
  AluminiumClean threads and finish; watch chip welding on deep 7075 bores.
• 2
  Stainless and titaniumWork hardening and heat drive tool changes and speed down.
• 3
  PlasticsThermal growth means measure cold, cut with air blast.
• 4
  Finish build-upQuote the bore to its post-finish dimension, not the machined one.

A single-axis bore on a flat face is 3-axis work. A bore on an angled face, or a cross hole that must intersect a main bore at a compound angle, is 4-axis or 5-axis work. The difference in price is real, but so is the difference in setup count and position error.

With 5-axis control the tool or the part tilts to the ideal angle. That lets us cut a continuous internal contour in one pass instead of blending three setups. Fewer setups means fewer datum shifts and less stack-up on true position. On a manifold with six angled ports, that is often the difference between passing and reworking.

Mill-turn centers help when a part needs both turning and internal milling. A hydraulic spool with a turned OD and cross-drilled internal ports can come off one machine instead of two. One chucking means one datum. For parts with tight concentricity between OD and bore, that matters.

Do not buy 5-axis when 3-axis will do. If your internal feature is a straight bore with a generous tolerance, a 3-axis machine with a good boring head is faster and cheaper. We quote the simplest process that holds the drawing, and we say so when the cheaper route is the correct one.

• 1
  3-axisStraight bores and pockets on accessible faces.
• 2
  4-axisCross holes and radial ports at indexed positions.
• 3
  5-axisCompound angles, blended internal contours, fewer setups.
• 4
  Mill-turnConcentric OD and internal features in one chucking.