CNC Machining Cavity Guide

• 1
  What a cavity is in CNC terms
• 2
  Why depth-to-diameter ratio decides the cut
• 3
  Corner radii, floor radii and draft
• 4
  Holding the part while the cavity is cut
• 5
  What 5-axis changes in cavity work
• 6
  How material changes the cavity cut
• 7
  Checking a cavity you cannot see
• 8
  Cavity features and how they machine

In CNC work, a cavity is any negative volume cut into a solid block: a pocket, a bore, a slot, a channel or an enclosed mould impression. The tool has to enter from outside the part, remove material it cannot see, and then leave. That single constraint explains almost every cavity problem we see on the shop floor.

A cavity is not defined by its shape but by its access. A 60 mm wide, 15 mm deep pocket is easy. The same width at 90 mm deep is a different job, because the tool that fits inside is long and narrow, and long narrow tools deflect.

The cavity also decides the machining sequence. Roughing clears volume, semi-finishing controls the remaining stock, and finishing follows the walls. Get the stock allowance wrong on the first pass and no finishing strategy will recover the tolerance.

• 1
  Open cavityTool reaches the floor from three or more sides
• 2
  Semi-enclosedOne wall limits entry; reachable with 4-axis indexing
• 3
  Closed cavityAccess from one direction only; defines tool length

The working limit of any cavity tool is its length-to-diameter ratio. A carbide end mill at 3×D is stiff. At 6×D it starts to sing. Beyond 10×D the tool bends under normal cutting force and the wall you cut is no longer where the program says it is.

Deflection scales with the cube of the overhang. Doubling tool length does not double the error; it multiplies it by roughly eight. That is why a cavity 80 mm deep is not simply "more passes" than one 40 mm deep. It is a different process with lower feed, lighter radial engagement and more passes.

Heat matters too. Inside a cavity the chips cannot leave, so they recut. Recutting raises edge temperature, dulls the coating and changes the effective tool diameter within a single operation. We plan air blast or through-spindle coolant before we plan the finishing pass.

• 1
  3×DFull-depth roughing is realistic
• 2
  6×DReduce radial engagement, keep axial depth moderate
• 3
  10×D+Step down, expect multiple passes, verify with a test cut

A cavity machined with a square internal corner is not machinable with a rotating tool. The cutter leaves its own radius. If the drawing calls for a 2 mm corner and the smallest tool that reaches the depth is 6 mm, the corner stays at 3 mm unless we add a separate operation.

Floor fillets help more than most designers expect. A fillet between wall and floor spreads stress and lets a larger, stiffer tool run the finishing pass. A sharp internal corner forces the smallest tool in the shop into the hardest place in the part.

Draft on vertical walls is usually unnecessary for machined cavities, unlike moulds. But a 0.5° to 1° wall taper does reduce rubbing on the flank, especially in stainless and titanium where the material springs back against the cutter.

• 1
  Corner radiusSet it at or above the largest tool that can reach the floor
• 2
  Floor filletR2–R5 spreads load and stiffens the cut
• 3
  Wall taper0.5°–1° reduces flank rub in gummy alloys

A cavity removes material from the middle of a part. That shifts the neutral axis and weakens the very section the vise is gripping. On thin-walled housings we often see the part move between roughing and finishing, not because the program changed but because the stiffness did.

The usual fix is to leave a sacrificial web or leave the part on a plate until the cavity is finished, then cut it free in a second setup. Vise jaws on the outside of a box section will not hold it flat once 60 percent of the internal material is gone.

For long cavities we sometimes use low-melt fixturing compound or a vacuum plate. Both add setup time. Both are cheaper than scrapping a part that has 20 hours of machining in it.

• 1
  Leave stock on the floor0.3–0.5 mm keeps the section stiff during roughing
• 2
  Machine in two setupsCavity first, then free the part and finish the outside
• 3
  Document the sequenceReordering setups is the most common cause of scrap

A 3-axis machine reaches a cavity from one direction. A 5-axis machine tilts the tool so the cutter engages the wall at its strongest point and the shank clears the pocket rim. The same cavity can be cut with a shorter tool, which is the same as saying it can be cut with a stiffer one.

Tilting also helps chip evacuation. When the tool axis is angled, gravity and coolant push chips out of the pocket instead of letting them pool around the cutter. In aluminium that difference shows up as better surface finish on the floor.

The trade-off is programming and setup time. Five-axis toolpaths need collision checking and a verified post-processor. For a shallow cavity with generous radii, 3-axis is faster and cheaper. We use 5-axis when reach, not complexity, is the limiting factor. Our shop runs 16 simultaneous 5-axis machining centers alongside 27 three-axis machines, and the choice is made per part, not per customer.

• 1
  ReachTilting shortens effective tool length
• 2
  Chip flowAngled axis drains pockets better
• 3
  CostUse 3-axis when the cavity is open and shallow

Aluminium 6061 and 7075 cut fast and clear chips easily, which makes them forgiving in deep pockets. Titanium TC4 (Ti-6Al-4V) is the opposite. It conducts heat poorly, so the edge stays hot, and it springs back against the tool. Cavity depth limits tighten considerably.

Stainless 316 and 17-4PH work-harden at the surface. A tool that rubs instead of cutting will make the next pass harder. We keep radial engagement high enough to stay in the cut instead of burnishing the wall.

Plastics behave differently again. POM and PEEK machine cleanly but expand with heat, so a deep cavity can close up on the tool. We take lighter passes and allow the part to cool between roughing and finishing.

• 1
  AluminiumFast, forgiving, good chip clearance
• 2
  TitaniumReduce depth, expect tool wear
• 3
  StainlessAvoid rubbing; keep the edge engaged
• 4
  PlasticsControl heat, allow cooling between passes

A cavity is the hardest feature on a part to measure. Calipers reach the rim, not the middle. The floor of a 70 mm deep pocket is checked with a probe, a deep bore gauge or a CMM with a long stylus that adds its own deflection.

We inspect cavities against the drawing at the section where they matter. Wall thickness is checked from the outside, floor thickness with an ultrasonic gauge on some parts, and the profile with a CMM or a shadowgraph for small features.

Any measurement inside a deep pocket carries more uncertainty than one on an open face. That uncertainty belongs in the tolerance discussion, not in a last-minute argument after the parts ship.

• 1
  CMM probingReliable but slow in deep pockets
• 2
  Ultrasonic gaugeFor floor and wall thickness
• 3
  Optical comparisonFor small profiles and radii