CNC Hole Quality: Tolerance, Geometry, Surface Finish and Inspection
A hole that is on size can still fail inspection. This guide separates the five things a drawing can control — size, location, form, surface and burr — and shows which process and which gauge actually delivers each one.
Quick answer
Hole quality is five independent characteristics, not one number: diameter, location, form (roundness, cylindricity, straightness), surface finish and burr condition. A drilled hole can pass a plug gauge and still be out of true position, lobed, tapered or burred. Each characteristic is delivered by a different part of the process chain and verified by a different instrument — so a hole tolerance is only meaningful when the measurement method is agreed with it.
01What actually defines hole quality
This is the single most useful idea on this page, and it is where most hole disputes between buyer and supplier begin. A machinist checks a hole with a plug gauge, it passes, the part ships. The customer puts it on a CMM, and the true position is out. Both measurements were correct — they were measuring different characteristics.
02Diameter and size tolerance
Size is the characteristic engineers are most comfortable with, and still the one most often mis-specified — usually by applying a fit class to a hole that does not need one.
How holes are dimensioned
- Nominal plus limits — for example Ø12 +0.05 / −0.00. Unambiguous, and the easiest for a supplier to quote against.
- ISO fit class — for example Ø12 H7. Compact and standard, but it implies a finishing operation and a matching gauge. Use it when a mating part depends on it.
- Drill size callout — for example "Ø10.2 drill". Signals clearly that a drilled hole is acceptable, which is helpful and cheap.
- Tapping callout — for example M12×1.75. The tap drill is determined by the required thread engagement; state the engagement if it is critical.
03Position and true position
Position tolerance answers a different question from size: not "how big is the hole" but "where is its axis, measured from the features the drawing says to measure from".
What actually controls position on the shop floor
- Fixture and clamping repeatabilityIf the part does not sit in the same place every time, nothing downstream can recover it. This is the first thing to verify when position scatters.
- Datum scheme and work offsetsThe datums on the drawing must be the features the part is actually located from, and the work offset must be set from those. A mismatch here produces parts that are internally consistent and still wrong.
- Number of setupsEvery re-fixturing adds positional uncertainty between the features machined before and after. Holes that must be tightly related should be produced in one setup — a strong argument for 4- and 5-axis machining.
- Entry conditionA drill entering an angled, curved or uneven surface deflects before it is fully engaged. Spotting, piloting or a rigid short drill controls this.
- DepthPosition at the entrance and position at the bottom of a deep hole are different measurements. If a deep hole has a position callout, agree where it is measured.
- Finishing operationBoring and helical interpolation cut to the spindle axis, so they can correct position. Reaming cannot — it follows the drilled axis.
04Form: roundness, cylindricity and straightness
Form errors are the ones that pass a gauge and fail a function. A hole can measure Ø12.01 at the entrance, Ø11.98 at the bottom, and be visibly three-lobed — and a go/no-go plug gauge will happily call it good.
Roundness (circularity)
How circular a single cross-section is. Drilled holes are commonly slightly lobed because of the two-lip cutting action.
Improved by: boring, honing, better runout control.
Cylindricity
Roundness and straightness and constant diameter over the full depth. The strictest of the three, and the one deep holes struggle with.
Improved by: boring, honing, rigid short tooling, good coolant reach.
Straightness of the axis
Whether the hole runs straight or curves away with depth. It matters for long holes, fluid passages and anything a shaft passes through.
Improved by: piloting, self-guiding tools, gun drilling on deep features.
| Shape error | What it looks like | Typical cause | How it is detected |
|---|---|---|---|
| Bell mouth | Flared at the entrance, correct deeper in | Tool wander before full engagement; runout; unsquare entry face | Bore gauge near the entrance vs mid-depth |
| Taper | Steadily narrows or widens with depth | Tool deflection; progressive wear during the cut; poor coolant at depth | Bore gauge at three or more depths |
| Barrel | Wider in the middle than at either end | Tool deflection under load in a long unsupported bore | Bore gauge profile along the depth |
| Lobing | Three- or five-sided rather than circular | Multi-lip cutting action; chatter; insufficient rigidity | CMM or roundness instrument — a plug gauge will not see it |
| Axis curvature | Hole drifts off line with depth | Unequal lip lengths; long unsupported drill; material inclusions | CMM at multiple depths, or sectioning |
Table 1. Form errors and their signatures. Each is diagnosed by where in the hole you measure — which is why a single entrance reading is not evidence of a cylindrical hole.
05Surface finish inside the bore
Bore surface finish matters when the hole seals, slides, presses or carries fluid. It is controlled by the finishing operation, the tool condition and — more than most people expect — by chip evacuation.
| Process | Relative finish | Where it is used |
|---|---|---|
| As-drilled | Roughest — tool marks, possible scoring from recut chips | Clearance holes, tap drills, roughing before a finish pass |
| Reamed | Considerably finer and more consistent | Standard-size fit holes; the usual answer to a moderate finish callout |
| Bored | Fine and controllable by adjusting parameters | Non-standard sizes, larger bores, where form also matters |
| Honed | Finest and most uniform; produces a cross-hatch pattern | Hydraulic and pneumatic bores, sealing and sliding surfaces |
Table 2. Relative finish by process. We confirm achievable Ra per feature against material, diameter, depth and tooling rather than quoting a universal value.
06Entrance, exit and cross-hole burrs
Burrs are the quality characteristic most often left off the drawing and most often argued about afterwards. "Break all sharp edges" and "no burr permitted in the intersecting bore" are separated by an entire operation and a significant cost.
Entrance burr
Raised material around the top of the hole. Usually the easiest to remove — a chamfer tool or countersink handles it in the same setup.
Exit burr
Forms when the last layer of material is too thin to shear and bends away instead. Controlled by reducing feed at breakthrough, backing the exit face, keeping the drill sharp, and adding a deburr pass.
Cross-hole burr
Forms inside the intersecting bore, where no standard tool can reach afterwards. This is a sequencing problem before it is a tooling problem.
07Process capability by characteristic
Rather than one tolerance table, here is how each process performs against each of the five characteristics. Read it as relative capability under a rigid setup in common materials.
| Process | Size | Position | Form | Finish | Relative cost |
|---|---|---|---|---|---|
| Drilling | Moderate — typically oversize | Inherits the setup; no correction | Modest — lobing, drift | Rough | Lowest |
| Reaming | Good at standard sizes | No correction — follows the drilled axis | Improves roundness; inherits axis errors | Good | Low |
| Boring | Very good, any size | Corrects — cuts to the spindle axis | Very good | Very good | High (slow) |
| Helical interpolation | Good on shallow bores | Corrects — toolpath defines the axis | Degrades with reach and deflection | Good | Moderate |
| Honing | Very fine control | No correction | Best cylindricity | Finest | Highest |
Table 3. Capability by characteristic. Note that only boring and interpolation can correct position — the single most important column on this table.
08Requirement → process → inspection matrix
This is the working matrix we apply to incoming drawings. Find the row that matches the controlling requirement, and read across for the process chain and the measurement that goes with it.
| What the drawing controls | Recommended chain | Inspection | Note |
|---|---|---|---|
| Diameter only, loose | Drill | Pin gauge or calliper | Cheapest possible hole — specify this whenever function allows |
| Thread | Spot → drill → chamfer → tap or thread mill | Go/no-go thread gauge | State engagement depth if it is critical |
| Fit class at a standard size | Spot → drill undersize → ream | Plug gauge; bore gauge for an actual value | Reaming cannot fix position — check the position callout too |
| Fit class + true position | Spot → drill → bore (or interpolate) | Bore gauge + CMM | The finishing pass is what delivers position |
| Non-standard diameter | Drill → rough bore → finish bore | Bore gauge + CMM | No stock reamer exists — boring is the practical route |
| Cylindricity over depth | Drill → bore → hone if required | Bore gauge at multiple depths; CMM | Measure the profile, not one point |
| Fine bore finish | Bore → hone | Profilometer + bore gauge | Verify probe access into the bore before specifying |
| No internal burr | Sequence cross holes before the sizing pass; dedicated deburr if unavoidable | Borescope; sectioned first article | A real operation — must be on the RFQ |
| Large diameter | Pilot → insert drill or interpolate → bore | Bore gauge / CMM | Solid drilling large holes wastes spindle power and tool cost |
Table 4. The requirement-to-process-to-inspection matrix. If a hole appears in more than one row, the strictest row governs the chain.
09GD&T and datum strategy for holes
Geometric dimensioning and tolerancing exists to state function rather than just dimensions. For holes it also determines how the part must be fixtured and how it will be measured — which is why the datum scheme belongs in the manufacturing conversation.
| Callout | What it controls | Manufacturing implication |
|---|---|---|
| Position ⊕ | Location of the hole axis within a cylindrical zone, relative to datums | Drives fixture design, setup count and usually a CMM check |
| Circularity ◯ | Roundness of individual cross-sections | Points towards boring or honing rather than drilling |
| Cylindricity | Roundness, straightness and constant size over the full length | The most demanding form control — verify depth is achievable first |
| Perpendicularity | Squareness of the axis to a datum face | Depends on setup and entry condition more than on the tool |
| MMC modifier △ | Bonus tolerance as the hole departs from maximum material condition | Genuinely useful on clearance holes — can turn a marginal feature into a comfortable one |
Table 5. Common hole callouts and what each one implies for how the part must be made and measured.
Three datum habits that save money
- Choose datums that are real, accessible locating features. If the drawing datums are not surfaces the part can actually be clamped and probed from, the shop invents its own and the correlation between our measurement and yours breaks down.
- Use maximum material condition on clearance holes. The bonus tolerance is free capability — it costs nothing functionally and widens the process window considerably.
- Group functionally related holes to one datum scheme. Holes that mate with the same component should be controlled together, ideally machined in a single setup.
10Inspection methods, ranges and limits
Every gauge is right somewhere and misleading somewhere else. This is the honest version of the inspection table — including what each method cannot tell you.
| Method | Gives you | Best for | Limits you must respect |
|---|---|---|---|
| Pin / plug gauge | Pass or fail against a limit | Fast go/no-go on standard fits in production | No numeric value, no trend; can pass a bell-mouthed or tapered hole; wears over time |
| Bore gauge | Actual diameter at a chosen depth | Detecting taper, barrel and bell mouth by profiling depth | Must be set against a master; reading depends on operator technique and seating |
| Air gauge | High-resolution diameter, very fast | Repetitive precision bores in volume | A master is needed per size; geometry and cleanliness affect the reading |
| CMM | Size, position, form, orientation, all referenced to datums | The only practical verification of geometric callouts | Slower and costlier; probe access, point density and probing force all affect the result |
| Profilometer | Surface roughness parameters | Verifying an Ra or Rz callout on the bore wall | Physical access into small or deep bores is often impossible |
| Borescope | Visual condition inside the bore | Cross-hole intersections, internal burrs, scoring | Qualitative — it shows a problem but does not measure it |
| Sectioning | Full ground truth on the internal condition | First-article validation of difficult internal features | Destroys the part; a sample method only |
Table 6. Inspection methods with their real limits. The right question at RFQ is not only "what is the tolerance" but "how will it be measured, and by whom".
11Defect diagnosis: symptom to cause to action
When a hole fails inspection, work in this order. Changing cutting parameters first is the most common and least productive response.
- Check first
- Runout at the tool tip; holder and collet condition; drill point symmetry
- Then
- Entry condition — is the face square, is there a spot, is the tool longer than it needs to be
- Action
- Correct runout and grind before parameters. If the drawing needs the size, add a reaming or boring pass rather than chasing it with a drill
- Check first
- Tool wear across the batch — measure the first, middle and last parts
- Then
- Coolant concentration and delivery consistency; material batch variation; thermal growth over a long run
- Action
- Set a tool-life limit instead of running to failure; add in-process checks at an interval matched to the tolerance
- Check first
- Fixture repeatability; whether the part is located from the drawing datums; work offsets
- Then
- Number of setups involved; entry condition; whether position was measured at entry or at depth
- Action
- Fix the setup. Parameters cannot recover position — only a boring or interpolation pass can, and only within the stock available
- Check first
- Bore gauge readings at three or more depths to confirm the shape
- Then
- Tool deflection and overhang; coolant reach at depth; wear developing during the cut
- Action
- Shorten the tool, pilot the hole, improve coolant delivery; add a finishing pass sized to the full depth
- Check first
- Chip shape and evacuation; coolant concentration and flow at the tool
- Then
- Tool margins and edge condition under magnification; built-up edge
- Action
- Restore evacuation before changing speeds. If the drawing calls a finish, plan reaming, boring or honing rather than optimising the drill
- Check first
- Operation sequence — are cross holes drilled before or after the sizing pass
- Then
- Feed at breakthrough; tool sharpness; whether the exit face is supported
- Action
- Re-sequence first, then reduce breakthrough feed, then add a dedicated deburring operation and quote it
12What actually drives the cost of a hole
Hole cost does not rise smoothly with tolerance. It steps up each time the requirement forces an additional operation, a slower operation, or a more demanding inspection.
| Requirement step | What is added | Cost effect |
|---|---|---|
| Clearance hole | One drill, one pass | Baseline |
| + fit class at a standard size | Spot, undersize drill, reamer; plug gauge check | Step up — extra tools and cycle time |
| + true position callout | Boring or interpolation; more careful fixturing; CMM time | Larger step — slower operation plus inspection |
| + cylindricity or fine finish | Possibly a honing operation and profilometry | Large step — often a separate process |
| + depth beyond 10×D | Specialist drilling, dedicated tooling and setup | Large step, plus schedule risk |
| + no internal burr | Re-sequencing or dedicated deburring; borescope or sectioning | Step up, and the inspection is slow |
| + full documentation | FAI, CMM reports, certificates | Fixed addition per batch, not per part |
Table 7. Cost steps at process boundaries. The useful design question is always: does the function actually need the next step up?
13DFM checklist for hole features
Before you release the drawing
- Apply a fit class only to the holes that genuinely mate with something
- Use standard drill and reamer sizes where the function allows
- State true position with datums that are real locating features
- Consider maximum material condition on clearance holes
- Keep depth under 5×D wherever the design permits
- Give a realistic surface finish for the function
- Say explicitly what burr condition is acceptable, and where
- State the inspection or documentation you require
- Group functionally related holes so they can be machined in one setup
- Tell the supplier what each critical hole does
Flags that will come back at RFQ
- A fit class on every hole on the part
- Tolerances tighter than the nominated gauge can resolve
- Position callouts referencing datums the part cannot be located from
- Deep holes with a straightness or cylindricity requirement
- Non-standard diameters with a tight band
- Fine finish specified in a bore no probe can enter
- "No burrs anywhere" with no verification method
- Holes breaking into angled, curved or already-finished surfaces
- Holes very close to a wall, an edge or each other
14The Goldcattle hole inspection workflow
Xiamen Goldcattle has run in-house precision manufacturing for 26 years under an ISO 9001 quality system, as a Chinese National High-Tech Enterprise. Hole characteristics are planned and verified as their own feature class rather than being absorbed into a general dimensional check.
- Feature classification at quotationEvery hole is tagged by its controlling characteristic — size, position, form, finish or burr. Anything with a geometric callout gets a process chain and a measurement plan before the price goes out.
- Measurement plan agreed with youWhich characteristics are measured, with which instrument, at what sample rate, and in what report format. Agreed before machining, not negotiated after a rejection.
- Fixture and datum verificationWe confirm the part can be located from the drawing datums and that the fixture repeats. If the datum scheme is not practical, we raise it with you rather than quietly substituting our own.
- First article inspectionMeasured against the full requirement — size, position, form, finish and burr condition — not just diameter. Bore gauge profiling at multiple depths on anything deep or form-controlled.
- In-process controlCheck interval set from the tolerance band and the observed tool wear rate. Tool life is treated as a limit, not something to discover by failure.
- Final inspection and documentationPin gauge, bore gauge, CMM and surface roughness inspection as agreed. FAI, CMM reports and material certificates supplied to the level the project requires.
Case: dowel-located bracket, 7075-T6
What the drawing implied. The H7 alone would have suggested reaming. But the ∅0.05 position callout ruled reaming out as the sole finishing operation, because a reamer follows the drilled axis and cannot correct location. The dowel holes and the mating datums also had to be produced without an intervening re-fixture.
What we changed. The dowel holes were drilled undersize and finished by boring in the same setup as the datum faces, so position came from the machine axes rather than from a second fixture. The fourteen clearance holes stayed as plain drilled holes — there was no functional reason to finish them, and treating them the same as the dowels would have added cost for nothing.
Verification. Bore gauge on every part for the H7 size, CMM on the first article and at an agreed sample rate for position to A B C. The clearance holes were checked with a pin gauge.
Result. Separating the two hole classes — and recognising that the position callout, not the fit class, dictated the process — kept the part in two setups and the inspection focused where it mattered. These values describe this part, this material and this setup; they are not a general capability claim.
FAQFrequently asked questions
What tolerance can a drilled hole hold?
As a planning figure, a drilled hole in a rigid setup lands somewhere around IT10–IT12, and it is usually slightly oversize. That is a starting point for discussion, not a promise: the achievable band depends on diameter, depth-to-diameter ratio, material, drill type and condition, holder runout, fixture rigidity and how the hole is measured. We assess every hole against those factors rather than publishing a single tolerance for all drilling.
What is the difference between hole tolerance and true position?
Diameter tolerance controls how big the hole is. True position controls where its axis sits relative to the datums on the drawing. They are completely independent — a hole can be perfectly on size and 0.3 mm out of position, or dead on position and 0.05 mm oversize. Size comes largely from the tool and the finishing operation; position comes from the fixture, the datum scheme and the work offsets.
Does a hole that passes a go/no-go plug gauge meet the drawing?
Only for size, and only at the point the gauge reaches. A plug gauge cannot detect true position, cylindricity, taper along the depth, or surface roughness. A bell-mouthed hole may accept the go gauge at the entrance while being undersize deeper in. If the drawing carries geometric or finish callouts, the plug gauge is not sufficient evidence of conformance.
When should I specify reaming instead of drilling?
When the drawing calls a fit class such as H7, a diameter band tighter than roughly ±0.05 mm, or a bore finish that drilling will not produce — and the required size is a standard reamer size. Reaming is a light, fast second pass that improves size and finish. It will not correct a hole that is in the wrong place, because the reamer follows the existing axis.
Why is my hole tapered?
Taper usually comes from tool deflection, an asymmetric point grind, progressive tool wear through the cut, or poor coolant reach at depth. It is invisible to a single entrance measurement — you find it by taking bore gauge readings at several depths. If a drawing needs a cylindrical hole over its full length, that requirement should be stated with a cylindricity callout so the right process and inspection are quoted.
What surface finish can I expect inside a hole?
Broadly: as-drilled surfaces are relatively rough, reaming improves finish considerably, boring can be controlled finer still, and honing produces the finest, most consistent bore surface. Actual values depend on material, tooling, parameters and coolant, so we confirm finish capability per feature rather than quoting a universal figure. Specifying a finer finish than the function needs is one of the most common avoidable cost drivers on a machined part.
How do you control burrs inside cross holes?
Sequence usually matters more than tooling. Where possible we drill the intersecting holes before the final sizing pass on the main bore, so the reaming or boring operation removes the intersection burr as it sizes the hole. Where that is not possible we use dedicated internal deburring tools or abrasive processes. A "no burr permitted" callout inside a bore is a real operation with a real cost and needs to be stated at RFQ.
Do you provide CMM reports and first article inspection?
Yes. We can supply first article inspection, CMM reports, material certificates and dimensional reports. The scope is agreed per project — which characteristics are measured, at what sample rate, and in what format — because 100% CMM inspection of every hole on every part is rarely the most sensible use of your budget.
How much does a tighter hole tolerance cost?
There is no fixed multiplier, but the steps are predictable. Moving from a clearance hole to a reamed fit adds a tool and a pass. Moving to a bored, position-controlled feature adds a slower operation, often a more careful fixture, and CMM inspection time. Adding a cylindricity or fine finish requirement can add a honing step. The jump in cost happens at those process boundaries, which is why it is worth checking whether the function truly needs the next step up.
What should I include on an RFQ for precision holes?
Diameter and tolerance, true position with the datum references, depth, any form callouts, surface finish, burr requirement, material and condition, quantity, and the inspection or documentation you need. If a hole is functionally critical, tell us what it does — a dowel location, a bearing seat, a sealing face or a fluid passage each imply a different process chain even at the same nominal size.
●The CNC drilling & parameters library
This page defines what a hole must achieve. The pages below cover how to achieve it — parameters, cycles, tooling and coolant.
The complete hole-making framework: operations, drill types, accuracy, cycles and process selection.
How cutting speed, RPM, feed per revolution and chip load fit together, with starting points by material.
Built-up edge, long chips, burrs, deep holes and hole accuracy in 6061, 7075, 2024 and 5052.
Feed per tooth vs feed per revolution, chip thinning, and what chip shape tells you about your parameters.
What SFM and m/min measure, why diameter changes RPM, and how to convert between them correctly.
Convert surface speed and tool diameter into spindle RPM, in both imperial and metric units.
Feed rate from RPM and chip load (milling) or feed per revolution (drilling), plus reverse calculation.
Canned cycle selection, Q/R/P/K parameters, G98/G99 returns, commented examples and alarms.
A decision framework from operation and material to geometry, coating, holder, reach and volume.
Flood, through-tool, MQL, air blast and dry machining, plus concentration, filtration and troubleshooting.
Identify flank wear, cratering, BUE, chipping and thermal cracking, then correct them in the right order.
Upload your drawing for hole tolerance, process and inspection review
Send the print and we will go through every hole feature: which ones a drill can hold directly, which need reaming, boring or interpolation, what the realistic capability is for your material and depth, and how each characteristic will be measured. You get the process chain and the inspection plan with the price — not a surprise at first article.
- Feature-by-feature tolerance and capability review
- Pin gauge, bore gauge, CMM and surface roughness inspection
- FAI, CMM reports and material certificates on request
- ISO 9001 quality system, 26 years, in-house machining
- 3-, 4- and 5-axis CNC to minimise setups and position error
- Honest answers — we flag holes we cannot hold as drawn
