How to Measure the Hollow of CNC Equipment With High-Precision Instruments

• 1
  Key takeaways
• 2
  What the hollow of CNC equipment means in this guide
• 3
  Thermal soak and machine check before any hollow measurement
• 4
  Clamping and datum choices that keep the hollow round
• 5
  Probe setup and measurement strategy inside a hollow
• 6
  Reading the numbers: what each deviation tells you
• 7
  Step by step: measure the hollow of CNC equipment
• 8
  Which hollow measurement method to use

In this guide, the hollow of CNC equipment means any internal feature a CNC machine produces or controls: a bored hole, a deep pocket, an internal cavity, a turned bore in a mill-turn part, or the hollow space inside a die-cast or billet housing after machining. The measurement problem is the same in all cases. The feature is inside the material, the probe or gauge has to reach it, and every thermal and mechanical error along the way shows up in the number you write on the inspection report.

The hollow of CNC equipment is harder to measure than an outside surface for three reasons. Access is limited, so you often use extension bars that add their own deflection and cosine error. Chip evacuation is poor, so a chip sitting in a blind bore reads as a size error. And the wall around the hollow is usually thinner than the rest of the part, so clamping and cutting forces deflect it more than the drawing model predicts.

We machine hollow features on 5-axis centers, mill-turn centers and 4-axis mills, with a maximum processing size of 4,000 mm and a Ø400 mm rotary table for parts that need to be indexed around a bore. The tolerance we hold in production is ±0.005 mm, with surface finish down to Ra 0.2–0.8 μm on bores that see a seal or a bearing. Those numbers only hold when the measurement process is as controlled as the cutting process.

Heat is the largest single error source in deep hollow measurement. Aluminum expands about 23 μm per meter per °C, steel about 11 μm, and cast iron about 10 μm. A 200 mm aluminum bore measured at 24 °C against a 20 °C drawing condition is roughly 0.018 mm larger than nominal. That is more than three times our production tolerance, so the number is meaningless until the part is at reference temperature.

The floor rule here is simple. Small parts under 100 mm soak for 30 minutes on a granite plate. Medium parts up to 500 mm soak for 1 hour. Parts near the 4,000 mm machine limit soak for 4 hours or overnight. Measure the part skin with a contact thermometer, not the air. A cold air stream from a door or a fan across one side of a hollow wall will bend the bore oval in the reading even after the bulk of the part has stabilized.

Before you blame the part, prove the machine. Run a 30-minute spindle warm-up program, then a ballbar circle test at the radius closest to your bore depth. A circularity deviation above 8 μm at that radius means the machine is contributing to the hollow error. Check the spindle growth curve too: a spindle that grows 15 μm over the first hour of running will taper a deep bore even when the toolpath is perfect.

• 1
  Thermal mappingLog room temperature and part temperature every 15 minutes during soak. Two readings within 0.5 °C is the release condition.
• 2
  Warm-up programRun the spindle at the finishing speed for 30 minutes before the first measurement pass.
• 3
  Ballbar radiusTest at the radius that matches your deepest hollow, not at a convenient short radius.

Most out-of-round hollows we investigate are not cutting problems. They are clamping problems. A three-jaw chuck closed on a thin-wall cylinder will push the bore into a triangle, and the part springs back after unclamping. The measured size on the machine looks fine; the measured size on the CMM after release is 0.02 mm out. The fix is to clamp on a thick boss or on an internal mandrel, and to keep clamping pressure low enough that you cannot see the wall move on a 0.001 mm indicator.

Datum strategy matters just as much. Pick the datum that the hollow actually locates against in the assembly, and machine it in the same setup as the hollow where possible. If the hollow is a bearing bore, the mounting face and the bore should come off one setup on a mill-turn center or a 5-axis machine. Re-datuming between operations adds the fixture repeatability error, typically 0.005–0.015 mm, on top of the machining error.

For deep pockets, support the floor of the cavity from below. An unsupported pocket floor deflects under tool pressure and springs back after the cutter leaves, which produces a floor that is flat on the machine and dished after release. Use adjustable supports or a low-melt fixturing compound, and verify the floor flatness with a dial indicator before cutting the side walls.

• 1
  Thin wallsBelow 3 mm wall thickness, use internal support or a filled cavity rather than chuck jaws.
• 2
  One-setup ruleLocating face and hollow in the same setup removes one stack-up term.
• 3
  Release checkMeasure the bore clamped and unclamped. Any shift above 0.005 mm means the fixture is the problem.

A spindle probe is fast but it is not a CMM. Stylus length, ball diameter and approach direction all add error. For a bore deeper than 3× diameter, use a stylus that is as short and as stiff as the geometry allows, and calibrate the stylus in the same orientation you will measure. A stylus calibrated vertically and then used horizontally on a deep bore can read 0.01 mm off before the part is even considered.

Take at least three points per circle and two circles per bore: one at 20% depth and one at 80% depth. The difference between the two circle centers is your taper. The difference between the largest and smallest radius on one circle is your roundness. That is enough data to separate a tool deflection problem, which shows up as taper, from a clamping problem, which shows up as roundness.

For bores below Ø20 mm or deeper than 150 mm, move to a bore gauge or an air gauge. Set the gauge against a ring gauge at the same temperature as the part, and take readings at the same two depths. Record the gauge temperature on the inspection sheet. A bore gauge used straight out of a cold toolbox will read 0.004–0.008 mm small until it equalizes.

• 1
  Two-depth ruleAlways measure near the top and near the bottom of the hollow to capture taper.
• 2
  Stylus orientationCalibrate the stylus in the same direction you will probe the bore.
• 3
  Ring gaugeSet bore gauges on a certified ring at part temperature, not room temperature.

A bore that is consistently small at both depths is a tool or offset problem. Check the tool wear offset and the cutter diameter compensation. On a mill-turn center, check that the tool is on center; a boring bar 0.02 mm off center cuts an oversize bore and a poor finish on one side. Adjust the offset and re-cut a test feature before touching the program geometry.

A bore that is on size at the top and small at the bottom is taper, and taper in a deep hollow usually comes from tool deflection or spindle growth. Shorten the boring bar overhang, reduce the depth of cut, or add a second finishing pass at low radial engagement. On a machine that has been running for two hours, spindle growth alone can add 0.01–0.015 mm of taper over a 200 mm depth.

A bore that measures round on the machine and out of round after unclamping is a fixture or residual stress problem. Thin-wall aluminum and stainless parts often need a stress-relief step between roughing and finishing. A bore that changes size overnight in the inspection room is thermal or, in some castings, moisture-related. Both cases call for re-measurement at controlled temperature before any scrap decision.

• 1
  Small at both depthsTool wear or offset. Check cutter compensation and tool on-center position.
• 2
  Taper top to bottomDeflection or spindle growth. Shorten overhang and let the machine stabilize.
• 3
  Round clamped, oval freeFixture or residual stress. Add support or a stress-relief step.