Oct 20, 2026CNC Machining Guides
CNC Machining Precision Holes: Drilling, Reaming, Boring and Inspection Guide
A buyer-focused guide to precision CNC holes covering drilling, reaming, boring, H7 fits, true position, surface finish, inspection, cost and RFQ requirements.
Precision holes often determine whether a machined part assembles, seals, locates, or rotates correctly. A hole may carry a bearing, locate a dowel, guide a shaft, seal around a valve, or align two components. Yet a drawing that states only “Ø20 H7” does not fully define how the feature should be produced or verified.
This guide helps buyers and design engineers choose realistic hole requirements, compare quotations, and prevent disputes about size, position, form, finish, and inspection.
1. Start with function, not the process
Hole function | Usually critical | RFQ question |
|---|---|---|
Clearance hole | Diameter and location | Is assembly clearance more important than exact size? |
Dowel hole | Size, position, perpendicularity | Is the dowel fixed in one part and sliding in the other? |
Bearing seat | Size, roundness, finish, coaxiality | What bearing fit and operating temperature apply? |
Valve or spool bore | Diameter, cylindricity, finish | Is leakage, friction, or straightness the limiting function? |
Thread preparation | Minor diameter and depth | Is full thread depth required in a blind hole? |
Sealing bore | Size, finish, edge condition | What seal type, pressure, and leakage limit apply? |
A supplier can often reduce cost when the function is clear. A bolt-clearance hole rarely needs H7, while a bearing seat may need more than size alone.
2. Drilling, reaming, boring and finishing options
Process | Typical role | Advantage | Limitation |
|---|---|---|---|
Drilling | Create the initial hole | Fast and economical | Size, straightness, and finish depend on depth and material |
Reaming | Finish a pre-machined hole | Efficient repeatable sizing | Follows the existing hole; limited location correction |
Boring | Correct size and centerline | Good control of size, position, and geometry | Slower; tool reach and access matter |
Circular interpolation | Mill a hole with an end mill | Flexible diameters and position control | Finish and roundness depend on machine dynamics |
Honing | Improve bore geometry and finish | Excellent finish and form | Specialized secondary operation |
Internal grinding | Finish hardened precision bores | Strong control after heat treatment | Higher cost and setup burden |
EDM | Hard material or difficult geometry | Low cutting force | Slower and may leave a recast layer |
A common sequence is drill undersize, semi-finish, then ream or bore. Stock allowance matters: too little may not clean up the previous operation; too much can overload the finishing tool.
3. How to interpret an H7 hole
Under ISO 286, the capital letter identifies the hole tolerance position and the number identifies the tolerance grade. For an H hole, the lower deviation is zero and the allowed size extends above nominal. The tolerance changes with nominal diameter.
Nominal diameter range | Planning value for H7 | Example permitted size |
|---|---|---|
Over 6 to 10 mm | 0 / +0.015 mm | Ø10: 10.000–10.015 mm* |
Over 10 to 18 mm | 0 / +0.018 mm | Ø12: 12.000–12.018 mm |
Over 18 to 30 mm | 0 / +0.021 mm | Ø20: 20.000–20.021 mm |
Over 30 to 50 mm | 0 / +0.025 mm | Ø40: 40.000–40.025 mm |
Over 50 to 80 mm | 0 / +0.030 mm | Ø60: 60.000–60.030 mm |
*Boundary diameters must follow the standard’s size-step rules. Verify the controlled drawing and current ISO 286 data.
Example: Ø20 H7/h6 clearance fit
A representative H7 hole is 20.000–20.021 mm. A representative h6 shaft is 19.987–20.000 mm.
- Minimum clearance = 20.000 − 20.000 = 0.000 mm
- Maximum clearance = 20.021 − 19.987 = 0.034 mm
This is size clearance only. Surface finish, roundness, alignment, coating, lubrication, temperature, and assembly force still affect function.
4. Size tolerance does not control hole location
A hole can be within diameter tolerance and still be misplaced. Control location separately with coordinate tolerances or a position tolerance relative to defined datums.
For measured center offsets ΔX and ΔY, diametrical true position is:
Position = 2 × √(ΔX² + ΔY²)
If the center is +0.030 mm in X and −0.040 mm in Y:
Position = 2 × √(0.030² + 0.040²) = 0.100 mm
A Ø0.12 mm positional tolerance at RFS would accept this result. If MMC is specified, bonus tolerance may apply, but the drawing and report must show how it was calculated.5. Form and orientation controls
Diameter alone does not control a long bore. Add only the controls the function needs:
- Roundness for rotating, sealing, or bearing surfaces.
- Cylindricity when the complete bore form matters.
- Straightness for long guide bores or spool motion.
- Perpendicularity when the axis must be square to a mounting face.
- Position or runout for related bores and rotating features.
Avoid stacking several controls that regulate the same function without a clear measurement plan. Over-specification increases programming, process control, inspection time, and dispute risk.
6. Depth changes manufacturability
Use depth-to-diameter ratio as an early planning indicator.
Depth-to-diameter ratio | Planning view | Buyer implication |
|---|---|---|
Up to about 3:1 | Usually straightforward | Standard tooling may be practical |
About 3:1 to 5:1 | Moderate depth | Chip evacuation and straightness need attention |
About 5:1 to 10:1 | Deep-hole region | Dedicated drills, coolant, or intermediate inspection may be needed |
Above about 10:1 | Special review | Consider gun drilling, alternative access, or a design change |
A Ø6 mm hole that is 48 mm deep has an 8:1 ratio. If only the final 20 mm needs close control, show that instead of applying the tight tolerance through all 48 mm.
For blind holes, distinguish drill-point depth from full-diameter depth. A standard drill leaves a conical bottom, so “20 mm deep” is ambiguous unless the drawing identifies the required cylindrical depth.
7. Surface finish must match function
A hole may pass size inspection but fail because it is tapered, lobed, scratched, burred, or too rough. State whether the bore carries a static seal, dynamic seal, bearing, or sliding element; whether finish applies before or after coating; and whether the entrance edge can be broken without damaging a sealing land.
A low Ra value does not automatically guarantee roundness, straightness, or leak tightness. These are different characteristics.
8. Heat treatment and coating affect final size
If the part is heat treated, anodized, plated, nitrided, or coated, state whether dimensions apply before or after finishing. A uniform coating reduces bore diameter by approximately twice the coating thickness.
Example: a 12.000 mm bore receives 0.010 mm coating per side. Its diameter may reduce by about 0.020 mm. Masking, post-finish honing, or a pre-coating allowance may be needed.
9. Agree the inspection method before production
Method | Best for | Limitation |
|---|---|---|
Pin or plug gauge | Fast pass/fail checks | Does not report actual diameter or full form |
Bore gauge | Diameter and taper comparison | Requires calibration and correct technique |
Internal micrometer | Larger accessible bores | Access and alignment matter |
CMM | Position, orientation, diameter, patterns | Probe reach and point strategy affect results |
Air gauge | High-volume bore comparison | Requires masters and controlled conditions |
Roundness machine | Detailed form analysis | Specialized equipment and added cost |
For a CMM report, define datum alignment, measurement depths, number of circles or points, filtering, and evaluation method. One circle near the opening does not prove a 60 mm-deep bore.
10. Temperature and uncertainty matter
Dimensional standards normally reference 20 °C. A simple thermal-expansion estimate is:
ΔL = α × L × ΔT
For a 100 mm aluminum feature, α ≈ 23 × 10⁻⁶ /°C and ΔT = 5 °C:
ΔL = 23 × 10⁻⁶ × 100 × 5 = 0.0115 mm
That shift is meaningful against a 0.020 mm tolerance. Precision inspection should consider stabilization time, part temperature, calibration, instrument capability, and measurement uncertainty.11. Common drawing problems that increase cost
- Applying H7 to every hole, including ordinary clearance holes.
- Specifying diameter without position or datum requirements.
- Requiring a tight tolerance through unnecessary depth.
- Omitting whether dimensions apply before or after surface treatment.
- Calling for a square bottom in a drilled blind hole without functional need.
- Using a plug-gauge requirement when actual diameter and taper data are expected.
- Omitting burr, cleanliness, and intersecting-hole requirements.
12. Buyer example: two locating holes
A plate uses two Ø8 H7 holes to locate a fixture. The original RFQ controls size but gives only ±0.10 mm coordinate dimensions. Assembly variation remains high because the datum scheme and relationship between holes are unclear.
A stronger approach is to define the mounting face as primary datum A, choose functional secondary and tertiary datums, use basic dimensions for the pattern, apply a position tolerance based on assembly clearance, and state the inspection depth. If two dowels could over-constrain assembly, consider one fixed pin and one relieved or diamond pin.
13. RFQ checklist for precision holes
- Native 3D CAD and controlled 2D drawing revision.
- Nominal diameter, tolerance or fit, and functional depth.
- Datum system, basic location, position, orientation, and form controls.
- Material grade, heat treatment, coating, and final-size condition.
- Surface roughness and critical sealing or bearing zones.
- Quantity, repeat demand, capability, and sampling expectations.
- Approved inspection methods and required report format.
- Edge break, burr, cleanliness, and intersecting-passage requirements.
- Mating component or functional-gauge information when available.
- Permission for the supplier to propose a lower-cost process or tolerance strategy.
Frequently asked questions
Is reaming always more accurate than drilling?
Reaming usually improves size and finish, but it follows the existing hole. Boring may be better when location, straightness, or correction is critical.
Does H7 define the manufacturing process?
No. H7 defines a tolerance zone. A capable supplier may use reaming, boring, interpolation, honing, grinding, or another suitable process.
Can a plug gauge prove roundness and taper?
No. A functional gauge is valuable for pass/fail acceptance but does not fully quantify diameter distribution, taper, roundness, or cylindricity.
Should every bearing bore use the same tolerance?
No. Select the fit from load, rotation, housing material, temperature, assembly method, service conditions, and the bearing manufacturer’s recommendations.
Request a precision-hole DFM review
Send Zync Precision your CAD model, drawing, material, quantity, mating-part information, hole depth, fit requirements, surface treatment, and inspection expectations. We can review the process route, tolerance stack, datum strategy, measurement plan, and cost-reduction options before quotation.