How to Do Hole Shaft Fit for CNC Machining

• 1
  Key takeaways
• 2
  Define the fit from the application, not the catalog
• 3
  Pick a tolerance standard and read the limits correctly
• 4
  Design the joint so the machine can hold it
• 5
  Match the process to the fit class
• 6
  Control the process and measure what matters
• 7
  Six steps from drawing to verified fit
• 8
  Common ISO 286 fits and where they belong
• 9
  Which fit class fits which situation

Before anyone opens a tolerance table, write down what the joint has to do. Does it rotate, slide, locate, or transmit torque? A shaft that spins at 3,000 rpm in a bearing housing needs running clearance. A dowel pin that positions a fixture plate needs a light press so the plate cannot creep. Same Ø20 mm, completely different limits.

Sort the joint into one of three families. Clearance fits always leave a gap: the shaft is smaller than the hole at every permitted size. Transition fits can end up with a small gap or a small interference depending on where the parts land inside their tolerance bands. Interference fits are always tight and are meant to hold without a key or a fastener.

The function also sets how much misalignment the assembly can absorb. Long shafts supported at both ends are sensitive to angular error, so the fit has to tolerate a little more play or the housing bores must be line-bored in one setup. Short, stiff joints can run tighter.

Write the intent in one sentence on the drawing: "locating pin, hand assembly, no relative motion under 200 N axial load." A machinist or inspector who reads that sentence will catch a wrong fit code faster than any tolerance table will.

• 1
  Rotating, lubricatedClearance fit with enough gap for an oil film.
• 2
  Locating, hand assemblyTransition fit, light tap with a soft mallet.
• 3
  Load-bearing, no fastenerInterference fit sized for the torque the joint must carry.
• 4
  Sliding under loadClearance fit with a wear-resistant finish on both surfaces.

ISO 286 is the default for most European and Asian drawings. A hole is written with a capital letter and a number, such as H7 or H8. A shaft uses a lowercase letter, such as h6, g6, or p6. The letter sets the position of the tolerance band; the number sets its width. H7 on a Ø20 mm hole means +0.021 / 0 mm. An h6 shaft at the same diameter means 0 / −0.013 mm.

The fit is the arithmetic between the two bands, and you have to check both the worst-case tight and worst-case loose conditions. For Ø20 H7/h6, the loosest assembly is a 20.000 mm hole with a 19.987 mm shaft, giving 0.013 mm clearance. The tightest is a 20.021 mm hole with a 20.000 mm shaft, giving 0.021 mm clearance. Both ends are clearance, so this is a clearance fit even though the numbers look tight.

ANSI B4.2 works the same way with different naming, and it is common on North American aerospace and defense drawings. If a customer sends a print with both, pick one and note the conversion on the drawing rather than leaving two systems side by side.

Watch the unit convention. Some prints give limits in inches with four decimal places, others in millimeters with three. A Ø0.7874 in callout and a Ø20.000 mm callout describe the same size, but 0.0002 in of tolerance is 0.005 mm, not 0.002 mm. Convert once, write the converted value on the drawing, and inspect to it.

A fit that is easy to specify can be hard to cut. Deep holes are the usual problem. A Ø10 mm bore that is 80 mm deep needs a boring bar with an 8:1 length-to-diameter ratio, and the bar will deflect. If the drawing allows, open the entry with a counterbore or shorten the precision length to 25 mm and leave the rest at a looser tolerance.

Interrupted bores, cross holes, and keyways break the cutting edge every revolution. They also make measurement harder because a two-point bore gauge cannot sit on a continuous surface. Where the design permits, move cross holes to a secondary operation after the main bore is finished, or specify the fit on the continuous section only.

Thin walls are the second trap. A 2 mm wall around a Ø40 mm bore will move when the part is unclamped, and a bore that measured 39.98 mm in the fixture can read 40.02 mm on the bench. For thin-wall parts, machine with light finishing passes and let the part relax before the final spring pass.

Finally, think about datums. If the bore and the mating shoulder are called out from different datums, the inspector has to stack two setups of error. Call both from the same datum and, where possible, machine them in one setup. A 5-axis machine with a Ø400 mm rotary table can often reach five faces of a housing without a re-clamp, which removes the biggest single source of fit error.

• 1
  Keep L/D under 5:1Beyond that, use a boring head with a larger bar or a line-boring setup.
• 2
  One datum for bore and faceStacking datums adds error the tolerance band cannot absorb.
• 3
  Finish after the part relaxesRough, unclamp, cool, then take the finishing cut.
• 4
  Avoid interrupted finish cutsCross holes and keyways belong in a later operation.

For a clearance fit in the H7 range, drilling plus reaming holds Ø tolerance well on holes up to about Ø20 mm and 5:1 depth ratio. Reamers cut to size, so the hole often lands near the low end of the band, around +0.005 to +0.010 mm on a +0.021 mm band. That is fine for clearance but wrong for a press fit where you need the hole near the high limit.

For transition and interference fits, boring is the better route because you can adjust the tool offset and hit a target within the band. A boring head with a 0.002 mm adjustment screw lets the operator dial in the size after a test cut. On a Ø20 mm H7 bore, aim for +0.012 mm to +0.016 mm, roughly the middle of the band, to leave room for the reamer or the final spring pass to drift either way.

Shafts follow the same logic from the other side. Turning with a carbide insert can hold ±0.005 mm on a rigid setup, but the insert wears and the last 50 parts of a run will trend larger or smaller depending on the wear mode. For diameters under Ø12 mm, use a collet instead of a three-jaw chuck and take a spring pass at 0.05 mm depth to remove deflection.

Grinding is the fallback when the tolerance goes below the turning range or the surface finish callout is tighter than Ra 0.8 μm. Cylindrical grinding can hold ±0.002 mm and Ra 0.2–0.4 μm, which is why bearing seats are often ground even when the rest of the shaft is turned. It adds a setup and a cost step, so reserve it for the surfaces that need it.

A single good part proves nothing about a run. The number that matters is whether the process stays inside the band across the whole order. Track the actual measured size on a simple chart and watch the trend. A boring tool that starts at +0.012 mm and drifts to +0.019 mm over 40 parts is still in tolerance on an H7 band, but the next 20 parts will not be. Adjust the offset at the midpoint of the drift, not at the limit.

Temperature is the quiet error. Steel expands about 11 μm per meter per degree Celsius. A Ø50 mm steel shaft measured at 30 °C reads roughly 0.006 mm larger than it would at 20 °C. On a tight transition fit with a 0.015 mm band, that is a third of the allowance gone to the thermometer. Let parts sit on a granite plate for 20–30 minutes before final measurement.

For holes, a two-point bore gauge reads diameter but not roundness or taper. Add an air gauge or a dial bore gauge with a three-point head for high-volume work, and check roundness at three depths. A bore that is Ø20.010 mm at the top and Ø20.002 mm at the bottom will pass a single-point check and still bind a shaft on assembly.

For shafts, measure with a micrometer at three positions along the length and two orientations 90° apart. A shaft that is round at the ends can be lobed in the middle after a centerless grind. If the fit is interference, also check the press force on the first assembly: a sudden force spike usually means the bore tapered or the shaft is out of round, not that the fit code was wrong.

• 1
  Chart the trend, not the pass/failOffset adjustments happen before the limit, not after.
• 2
  Settle at 20 °C20–30 minutes on a granite plate before final measurement.
• 3
  Check roundness and taperThree depths in the bore, two orientations on the shaft.
• 4
  Verify with one real assemblyFeel or press force is the final check the print cannot give.