Uniform Hole Offset and MMC Bonus on a CNC-Bored Plate
A 6061-T6 fixture plate has four Ø10.00-10.10 mm holes on a 100 × 80 mm rectangular pattern. The drawing calls out position Ø0.25 Ⓜ to datum A (bottom face), B and C (two perpendicular edges). The holes are drilled and bored on a vertical CNC mill; the program uses a probe to set X and Y from the B and C edges. The CMM report at 20 °C shows all four holes at X +0.12 mm and Y +0.02 mm from nominal, with diameters of 10.06, 10.07, 10.06 and 10.12 mm. The inspector rejects the entire lot because the position is 0.24, which is too close to 0.25, and one hole is oversize. The operator wants to rerun the finish boring with the same work offset and a tool radius compensation of -0.01 mm.
1. Compute the true position for the holes and the allowed tolerance including bonus. Determine which holes conform.
Read the worked answer
Radial deviation = √(0.12² + 0.02²) = 0.1217 mm. True position is diametral: 2 × 0.1217 = 0.243 mm.
At MMC 10.00 mm, the stated position tolerance is 0.25 mm. Bonus tolerance equals the actual size minus MMC. For the 10.06 holes, bonus = 0.06, so allowed position = 0.31 mm. For 10.07, bonus = 0.07, allowed = 0.32 mm. For 10.12, bonus would be 0.12, allowed = 0.37 mm, but 10.12 mm is outside the 10.00-10.10 mm size limit.
Therefore the three holes at 10.06, 10.07 and 10.06 conform on both size and position. The 10.12 mm hole fails size independently of position. The inspector is wrong to reject on position: 0.243 mm is less than 0.25 mm even before bonus, and bonus makes it more favorable. The lot should be sorted, not rejected on position.
2. Explain the uniform X shift. Should the operator apply tool radius compensation of -0.01 mm? Propose the corrective action.
Read the worked answer
A uniform +0.12 mm X shift on all four holes points to a datum or work-offset error, not random tool deflection. Likely causes are chips or burrs on the B datum edge during probing, probe stylus calibration drift, or a fixture stop that moved. Check the probe with a ring gauge, clean the B and C edges, and re-probe. Then shift the work offset X by -0.12 mm and cut a test part.
Tool radius compensation changes hole size, not location. A -0.01 mm compensation would make the holes smaller and would not correct the X shift. It could also make the 10.06 mm holes approach the low size limit. Correct the offset and probe condition first, then adjust size if needed.
3. What is the virtual condition for these holes, and what functional gauge would verify it? How should the oversize hole be handled?
Read the worked answer
For an internal feature at MMC, virtual condition = MMC size - geometric tolerance = 10.00 - 0.25 = 9.75 mm. A functional gauge pin of 9.75 mm must enter each hole; this verifies the worst-case boundary that protects assembly. The CMM should report size and position separately with bonus clearly shown.
The 10.12 mm hole is oversize and must be confirmed with a plug gauge or bore gauge. If it is truly 10.12 mm, the part is nonconforming. Rework is possible only if the drawing allows an insert or a larger approved hole; otherwise scrap or sort the part.