CNC Machining Cavity Parts: How Pockets, Cores and Deep Cavities Are Actually Cut

• 1
  What makes a cavity part different from a surface part
• 2
  The four numbers that decide whether a cavity is machinable
• 3
  When 3-axis is enough and when 5-axis cavity machining pays off
• 4
  How we sequence a cavity so the walls stay straight
• 5
  Material choice changes cavity rules more than most engineers expect
• 6
  How cavity accuracy is verified before the part ships
• 7
  Cavity feature versus machining approach

A surface part is cut from the outside in. The tool approaches the stock from open space and every point on the finished face is reachable by a straight line. A cavity part is the opposite. The finished geometry encloses volume, so the tool must enter through a restricted opening and cut material it cannot see. That single fact drives almost every design rule that follows.

The cutting tool is a cylinder with a flute length. It has a diameter, a corner radius and a maximum depth it can reach without chattering. When we machine a pocket or an internal core, the tool body has to fit through the opening, reach the floor, and still have enough stiffness to hold tolerance. If any of those three conditions fails, the feature is not machinable as drawn, no matter how good the CAM software is.

This is why cavity parts are quoted differently from open parts. We look at the deepest cavity, the smallest internal radius and the number of faces that need a second setup. Those three numbers usually decide whether the part runs on a 3-axis machine, a 4-axis mill-turn, or a simultaneous 5-axis center.

• 1
  Enclosed volumeThe tool enters through an opening, so reach and clearance matter more than raw spindle power.
• 2
  Tool stiffnessA long, thin tool deflects. Deflection shows up as taper on the wall and a floor that is not flat.
• 3
  Setup countEvery side of a cavity part that cannot be reached in one orientation adds a setup and a re-datum.

Depth-to-diameter ratio is the first gate. A carbide end mill cutting aluminium or stainless is stable up to roughly 4:1 in a rigid holder. Beyond that, we step down to a smaller radial engagement, reduce feed per tooth, and often accept a rougher wall that needs a finishing pass with a longer reach tool. At 8:1 you are in specialty-territory: reduced neck tools, high-pressure coolant through the spindle, and slower cycle time.

Internal corner radius is the second gate. A pocket cut with an Ø10 mm end mill always leaves an Ø10 mm corner before finishing, unless you use a smaller tool or a corner-radius cutter. If your drawing calls for a sharp internal corner in a pocket deeper than 20 mm, the answer is usually a wire EDM insert or a broached corner, not a milled one. Designers who specify R0.5 in a 40 mm deep pocket should expect either a very slow smaller tool or a design change.

Wall thickness is the third gate. Thin walls deflect under cutting force. In aluminium, a 1.0 mm wall at 30 mm tall is workable with light finishing passes. In 304 stainless or Ti-6Al-4V, the same wall needs support material, a fixture that backs the wall, or a different process. We have run walls down to 0.5 mm in aluminium on parts that were later anodized, but that requires a conversation before the drawing is frozen.

Floor radius is the fourth gate. A flat-bottom pocket with a sharp internal floor corner is only possible if the tool can plunge. Ball-nose tools leave a scalloped floor. If the floor has to be flat and the corner sharp, you need a fillet radius at the floor equal to at least the corner radius of the cutter, typically R0.5 to R2.0 mm.

• 1
  Depth to diameterKeep under 4:1 for standard tooling. 4:1 to 8:1 needs reduced-neck tools and slower feeds.
• 2
  Internal radiusMatch the corner radius to the largest tool that fits the pocket, not the smallest you can find.
• 3
  Wall thicknessAluminium: 1.0 mm workable. Stainless and titanium: 2.0 mm and up unless supported.
• 4
  Floor cornerAdd R0.5–R2.0 mm at internal floor corners so a radiused cutter can reach the floor.

A 3-axis vertical mill can cut any cavity that opens upward. If the pocket floor is perpendicular to the Z axis and the walls are vertical or drafted, a 3-axis machine with a good fixture handles it. The limitation is orientation. Every face that is not normal to Z needs either a re-setup or an angle fixture.

A 4-axis mill with a rotary table adds rotation about one axis. For cavity parts with features on four sides of a prismatic block, this removes two or three setups. The rotary table on our 4-axis mills is Ø400 mm, which suits cavity housings up to roughly 300 mm across without a tailstock.

Simultaneous 5-axis is where curved cavity geometry becomes practical. A 5-axis center tilts the tool so a short, stiff cutter can reach a deep wall at the correct contact angle. The tool stays short, the wall finish improves, and the number of setups drops to one or two for the whole part. Our 16 simultaneous 5-axis machining centers run cavities with compound angles, blended internal radii and non-planar floors without special fixturing.

The trade-off is programming time and machine rate. A cavity that can be cut in two 3-axis setups should stay on a 3-axis machine. Simpler setup, easier inspection, lower cost. Move to 5-axis when the geometry forces it: intersecting pockets at compound angles, deep cavities with undercut walls, or a tolerance that depends on a single datum that cannot be re-established between setups.

• 1
  3-axisBest for open pockets, vertical walls, floors normal to Z. Lowest cost per part.
• 2
  4-axisAdds a single rotary axis. Good for prismatic housings with features on four sides.
• 3
  5-axisNeeded for compound angles, undercut walls, non-planar floors, single-datum tolerance.

Roughing removes most of the volume with a large tool. We use adaptive or trochoidal paths to keep radial engagement constant and reduce heat. On aluminium 6061 and 7075, a Ø16 mm carbide end mill at 12,000 rpm and 3,000 mm/min feed removes material quickly without loading the flutes. On 17-4PH stainless, the same cutter runs much slower and we accept a longer roughing cycle to protect the tool.

Semi-finishing brings the walls within 0.3 to 0.5 mm of final size. This pass is where we correct any deflection from roughing. If the cavity is deep, we check the wall with an on-machine probe before finishing. That step catches a bent tool before it becomes scrap.

Finishing uses the shortest possible tool. In a deep cavity we often switch to a reduced-neck end mill or a high-feed cutter with a small corner radius. Cutting forces drop, wall straightness improves, and surface finish lands in the Ra 0.8–1.6 μm range without a separate polish. Where the drawing calls for Ra 0.2–0.8 μm, we add a finishing pass at lower feed per tooth and higher spindle speed, sometimes followed by bead blasting.

Inspection happens in two stages. In-process probing checks critical wall positions and floor depths while the part is still in the fixture. Final inspection on a CMM confirms the cavity dimensions against the model. Every part is inspected before shipment, and dimensional reports are available on request.

• 1
  RoughLarge tool, adaptive paths, constant radial engagement, controlled heat.
• 2
  Semi-finishLeave 0.3–0.5 mm. Probe deep walls before committing to finish.
• 3
  FinishShortest reach tool available. Lower feed per tooth for Ra 0.2–0.8 μm.

Aluminium is the easiest cavity material. 6061-T6 and 7075 cut fast, hold a 1.0 mm wall at moderate depth, and finish well with standard carbide. 2024 is stronger but gummier and tends to build up on the cutting edge, so we slow the spindle and increase coolant pressure. ADC12 die-cast aluminium behaves differently again because porosity in the casting can open up when a thin wall is machined.

Stainless is where cavity design gets strict. 303 and 304 work-harden if the tool rubs instead of cuts, so we keep a minimum chip load and never dwell. 17-4PH (SUS630) in the H900 condition machines cleanly but requires more tool changes. 316L for medical and food-contact parts is machinable, but deep cavities should be designed with a minimum 2.0 mm wall unless the part is backed by a fixture.

Titanium and Inconel are the hardest cavity materials we run. Ti-6Al-4V conducts heat poorly, so the cutting edge stays hot and the tool wears quickly. Deep cavities in titanium usually mean reduced depth of cut, slower speeds, and a design review before the part is quoted. Inconel is worse; we often recommend a cast or additively manufactured near-net shape with only the critical faces machined.

Surface finish options interact with cavity geometry. Anodizing adds a few micrometres and can round a sharp internal edge. Electroless nickel builds uniformly, which helps a worn cavity but changes the dimension. Bead blasting inside a deep pocket is difficult to do evenly, so we usually restrict blasting to reachable faces and specify a machined finish for the cavity floor.

• 1
  Aluminium 6061 / 7075Fast, stable, 1.0 mm walls workable. Best cavity material.
• 2
  Stainless 304 / 17-4PHWatch work hardening and tool wear. Keep minimum chip load.
• 3
  Titanium and InconelSlow, hot, expensive. Review the design before quoting.

A cavity part cannot be checked with calipers on the bench. The walls are inside, the floor is often not flat, and the datum is frequently a face that is no longer accessible. We plan inspection at the same time we plan the machining sequence, so the datum used for the CMM matches the datum used in the fixture.

In-process probing is the first line. After semi-finishing, we probe the wall positions and floor depths on the machine. If a wall has drifted more than 0.05 mm from nominal, we adjust the finishing pass rather than scrap the part. This is especially useful on deep cavities where a long tool has deflected.

Final inspection runs on a CMM with a scanning head for curved cavity surfaces. We verify critical dimensions, wall thicknesses and floor flatness against the model. Tolerances down to ±0.005 mm (±0.0002 in) are achievable on cavity features when the design allows a rigid setup and a short finishing tool.

Reports are available on request. Raw material certificates, in-process records and final dimensional reports can be packaged with the shipment. For medical and automotive cavity parts, the inspection plan is written before production starts so the records match the qualification requirements.

• 1
  Datum planningCMM datum matches the machining datum to avoid stacked error.
• 2
  In-process probingCatches drift before finishing, when the part can still be corrected.
• 3
  CMM finalScanning head for curved cavity surfaces, reports on request.