Complete Guide to CNC Drilling and Precision Hole Making
Drilling is only one way to make a hole. This guide maps the whole hole-making system — operations, drills, depth limits, cycles, accuracy, defects and inspection — so you can pick the right process before you cut metal.
Quick answer
CNC drilling is the machine-controlled production of round holes with a rotating drill fed along its axis. It is fast and cheap, but on its own it is a roughing operation: expect roughly IT10–IT12 diameter capability, some positional drift and an as-drilled finish. Precision holes are produced by a chain — spot, drill, then ream, bore or helically interpolate — selected from the tolerance, depth-to-diameter ratio, material and inspection called out on the drawing.
01CNC drilling is a subset of hole making
The single most expensive mistake in hole machining is quoting or programming a hole as "just a drilled hole" when the drawing actually demands a finishing operation. A Ø12 H7 hole and a Ø12 clearance hole look almost identical on a 2D print. One is a drill. The other is a spot, an undersize drill, a ream and a gauge check — three extra tools and roughly three times the cycle time.
So before any parameter discussion, answer one question: what does the print actually require, and can a drill deliver it directly? That is the job of this page. Everything downstream — cutting data, canned cycles, coolant, tooling, wear — lives on the dedicated pages linked throughout.
02The operations that make up hole making
These are the operations you will actually specify on a CNC machining centre. Each one has a job it does well and a job it should not be asked to do.
| Operation | What it does | Typical use | Do not use it for |
|---|---|---|---|
| Spot drilling | Creates a short conical start that locates the drill point | Angled, curved or rough surfaces; long drills; tight position | Flat faces with a rigid carbide drill — it can chip the corner |
| Centre drilling | Combined pilot and 60° centre for lathe work | Supporting a shaft on a live centre | General spotting on a machining centre |
| Drilling | Produces the hole from solid | Clearance holes, tap drills, roughing before a finish pass | Anything with a fit tolerance or a tight position callout |
| Peck drilling | Drilling interrupted by retracts to clear chips | Deep holes, gummy material, no through-tool coolant | Shallow holes — it only adds cycle time |
| Counterboring | Flat-bottomed enlargement for a socket head | Recessing fasteners | Producing a bearing fit |
| Countersinking | Conical enlargement | Flat-head screws, deburring the entry | Deep chamfers in one pass on hard material |
| Reaming | Removes a small, even stock allowance at a fixed size | H7-class holes at standard sizes, good finish | Correcting a badly positioned or bell-mouthed hole |
| Boring | Single-point enlargement, adjustable diameter | Non-standard sizes, roundness, correcting position | High-volume small holes — it is slow |
| Helical interpolation | An end mill spirals down and around the bore | One tool, many sizes; thin walls; large holes; prototype work | Deep small-diameter holes |
| Tapping / thread milling | Produces the thread in a prepared hole | Threaded features | Fixing an undersized or oversized tap drill |
| Honing | Abrasive finishing of a bore | Very fine finish, cylindricity, hydraulic bores | Changing hole position |
Table 1. Hole-making operations and their honest limits. Reaming follows the existing hole — it improves size and finish but will not move a hole that was drilled off position.
03Drill types and tool materials
Drill choice is a rigidity-and-evacuation problem long before it is a cutting-speed problem. The two variables that matter most are how stiff the drill is for the depth you need, and how well the flutes can clear chips out of that depth.
By construction
Solid carbide drill
Stiff, holds size well, runs at high cutting speed. The default for production work in aluminium, steel and stainless when the machine has the rigidity and coolant to support it.
Watch: brittle. Punishes runout, interrupted cuts and unstable setups.
HSS and cobalt HSS
Tougher and far cheaper. Tolerates less rigid machines, hand-fed work and interrupted entry. Cobalt grades handle stainless and higher temperature better than plain HSS.
Watch: much lower cutting speed, so cycle time suffers in volume.
Indexable insert drill
Replaceable inserts, very productive above roughly Ø16–20 mm and in the 2–4×D range. Low cost per hole on larger diameters.
Watch: asymmetric cutting forces; not for a fit hole without a finishing pass.
Parabolic-flute drill
Wide, open flute form built for chip evacuation. The usual answer between about 5×D and 15×D where a standard drill would pack up.
Watch: less core strength — feed discipline matters.
Gun drill
Single-flute, self-guiding, high-pressure internal coolant. The real tool for deep holes beyond roughly 10–15×D with straightness and finish requirements.
Watch: needs suitable coolant pressure, a bushing or pilot, and setup time.
Step drill
Drills and chamfers, or drills two diameters, in one plunge. Saves a tool change on high-volume work.
Watch: a special — regrinding and lead time are real costs.
Geometry features worth specifying
- Point angle. Roughly 118° is the general-purpose grind; around 135° self-centres better and suits harder materials and stainless; sharper points near 90–118° suit soft materials and plastics. A split point reduces the thrust needed to start and helps the drill locate without a spot.
- Helix angle. High helix lifts chips faster — good for aluminium and other gummy materials. Low helix gives edge strength for hard or abrasive materials and for cross-hole and interrupted entries.
- Flute length vs reach. Use the shortest drill that reaches the depth. Stub drills are dramatically stiffer than jobber drills; the stiffness of a cantilevered tool falls off very quickly as it gets longer.
- Coolant through the tool. The single biggest enabler for deep and gummy-material holes. It changes both the achievable depth and whether pecking is needed.
- Coating. Coating choice follows the workpiece: uncoated or polished flutes resist aluminium sticking, while AlTiN/TiAlN families are common for steels and higher-temperature cutting. Confirm the exact grade against the tool maker's data.
04How to select a hole-making process
This is the decision most drilling articles skip. Work from the hole requirement to the process chain, not from the tool you happen to have in the carousel.
| Hole requirement | What actually drives it | Recommended chain | Inspection |
|---|---|---|---|
| General clearance hole | Diameter only, loose tolerance, position from the fixture | Drill | Pin gauge or calliper |
| Tapped hole (tap drill) | Thread engagement depends on tap-drill size and hole straightness | Spot → drill → chamfer → tap or thread mill | Go/no-go thread gauge |
| Precision fit hole (H7-class) | Diameter, roundness and finish at a standard size | Spot → drill undersize → ream | Plug gauge, or bore gauge for an actual value |
| Bearing / non-standard bore | Diameter, cylindricity, position; size is not a stock reamer | Spot → drill → rough bore → finish bore | Bore gauge plus CMM for position and form |
| Deep hole (>5×D) | Chip evacuation, coolant reach, straightness drift | Spot or pilot → through-coolant or parabolic drill with peck → ream or bore only if the depth allows | Bore gauge at several depths to reveal taper |
| Cross hole / intersecting bore | Interrupted entry and exit, internal burrs | Drill the main bore first → reduce feed at breakthrough → dedicated internal deburr | Borescope or sectioned first article |
| Thin wall or sheet | Deflection, exit burr, hole distortion after clamping release | Support the exit → helical interpolation or a sharp low-thrust drill → light finishing pass | CMM with light probing force; check free-state |
| Large diameter (>25 mm) | Spindle power and thrust; solid drilling gets expensive | Pilot → insert drill or helical interpolation → bore to size | Bore gauge / CMM |
| Very fine finish bore | Surface texture and cylindricity beyond boring capability | Bore → hone | Profilometer plus air or bore gauge |
Table 2. Requirement-driven process selection. Chains are starting points for a rigid setup on a machining centre — diameter, depth, material and fixture all shift them.
The four-question engineering check
Before committing a hole to "drill only", we run this check on every drawing. It takes a minute and it prevents most first-article surprises.
- Is there a fit, a limit or a class on the diameter? An H7, a G6, a ±0.02 mm or a stated fit means a finishing operation. A ±0.2 mm or a drill-size callout does not.
- Is there a geometric callout — true position, cylindricity, perpendicularity? Geometry is controlled by the setup and the finishing pass, not by the drill. A tight true position also implies a datum strategy and probably a CMM report.
- What is the depth-to-diameter ratio? Above roughly 3×D the conversation becomes chip evacuation and coolant. Above roughly 10×D it becomes a specialist operation with its own tooling.
- Is a burr acceptable, and where? "Break all sharp edges" is cheap. "No burr permitted in the intersecting bore" is a separate operation and must be quoted as one.
05Hole depth and the depth-to-diameter ratio
Depth-to-diameter ratio (L:D, sometimes written ×D) is the most useful single number in drilling. It predicts whether chips will clear, whether you need pecking, whether coolant can reach the cutting edge, and how much the hole will drift off straight.
What gets worse with depth
- Chip packing. Chips have further to travel up the flute and more chance to weld or wedge. A packed flute spikes torque and snaps drills without warning.
- Coolant reach. External flood coolant struggles to get past the chips coming the other way. Through-tool coolant reverses the problem — it pushes chips out.
- Straightness. Small asymmetries in the point grind steer the drill. Over a long hole those tiny errors integrate into measurable positional drift at the bottom, which is why deep-hole position is checked at depth, not just at entry.
- Heat. The tool spends longer in the cut per hole and has less opportunity to shed heat, accelerating wear.
- Taper and bell mouth. Entry conditions and tool deflection produce a hole that is not the same diameter at the top and the bottom. A single gauge check at the entrance will not detect it.
06Feeds, speeds and chip formation — the overview
Four variables control every drilling operation, and they are linked: change one and at least one other moves with it.
Spindle speed from cutting speed
- Vc
- cutting speed, m/min
- D
- drill diameter, mm
- RPM
- spindle speed, rev/min
Imperial: RPM = (3.82 × SFM) / Dinch
Feed rate from feed per revolution
- Vf
- feed rate, mm/min (or IPM)
- fn
- feed per revolution, mm/rev (or IPR)
Drilling is programmed per revolution, not per tooth — a two-flute drill removes fn/2 per lip.
Because these four variables are the shared language of the whole cluster, we keep the full treatment on dedicated pages rather than duplicating it here:
Reading chips: the fastest diagnostic in the shop
| Chip appearance | What it usually means | First thing to check |
|---|---|---|
| Short, tight curls or figure-6 sections, silver to light straw | Parameters are in a healthy window | Nothing — record the settings |
| Fine powder or dust | Feed too low; the edge is rubbing instead of cutting | Raise feed per revolution before touching speed |
| Long stringy chips wrapping the drill | Feed too low for the material, or wrong helix/point for a gummy alloy | Raise feed, consider a peck cycle to break chips |
| Dark blue or purple chips | Excessive heat — speed too high or coolant not reaching the cut | Verify coolant delivery first, then reduce cutting speed |
| Thick, deformed, welded chunks | Feed too high, built-up edge, or a worn drill | Inspect the drill point; check runout and holder |
Table 3. Chip appearance is direct feedback from the cutting zone. Diagnose from the chips before you change numbers in the program.
07Coolant and chip evacuation
In drilling, coolant does three separate jobs and they are not equally important at every depth: it cools the cutting zone, it lubricates to reduce friction and built-up edge, and it flushes chips out of a confined hole. Past roughly 3×D, flushing quietly becomes the dominant one.
| Delivery method | Where it works | Limits |
|---|---|---|
| Flood coolant | General drilling to roughly 3–4×D; the shop default | Cannot reach the tip of a deep hole against escaping chips |
| Through-tool coolant | Deep holes, gummy materials, high-productivity drilling; often removes the need to peck | Requires a through-coolant drill, holder and machine capability |
| MQL (minimum quantity lubrication) | Aluminium and other materials where lubrication matters more than cooling; cleaner parts | Very limited chip flushing — not a deep-hole solution on its own |
| Air blast | Clearing chips in shallow holes, plastics and some cast irons | No cooling or lubrication; dust and chip control needed |
| Dry | Some cast irons and specific tooling systems designed for it | Heat and chip packing rise quickly; a deliberate choice, not a default |
Table 4. Coolant delivery by application. Concentration, pressure and fluid selection must follow your coolant supplier's data sheet.
08G81, G73 and G83 canned cycles — overview
A canned cycle compresses the whole rapid-feed-retract sequence of a hole into one program line, so a pattern of fifty holes becomes fifty coordinate pairs rather than two hundred motion blocks. Three cycles cover most machining-centre drilling.
G81 — standard drilling
Rapid to R, feed to Z, retract. One continuous cut with no interruption.
Use for: shallow holes, roughly up to 3×D, where chips clear on their own.
G73 — high-speed peck
Feeds down in increments of Q with a small retract between pecks — enough to break the chip, not to clear the hole.
Use for: moderate depth where the chip needs breaking but full evacuation is not necessary. Faster than G83.
G83 — deep-hole peck
Feeds down in increments of Q but typically retracts fully to the R plane each peck, clearing chips and letting coolant back in.
Use for: deep holes and materials that pack. Slower, but far safer.
Cycle choice is not only about depth. Chip character, coolant delivery, material and drill construction all feed into it: a through-coolant drill in free-machining steel may run G81 to 5×D happily, while a solid drill in stainless may need G83 at 3×D.
09Hole accuracy: drilling vs reaming vs boring vs interpolation
"Accuracy" is four separate things, and a process can be excellent at one and poor at another. Confusing them is why holes pass a diameter check and still fail inspection.
Size
Is the diameter within the limits? Checked with a plug gauge, pin gauge or bore gauge.
Location
Is the hole axis where the drawing says, relative to the datums? This is true position, and it is a CMM characteristic.
Form
Roundness, cylindricity, straightness. A hole can be exactly on size at one depth and lobed or tapered along its length.
Surface
Roughness of the bore wall, plus burr condition at entry, exit and cross-hole intersections. Measured with a profilometer, not a gauge.
| Process | Size capability | Can it correct position? | Form | Relative cycle time |
|---|---|---|---|---|
| Drilling | Roughly IT10–IT12; commonly oversize | No | Modest — lobing and drift are normal | Fastest |
| Reaming | Roughly IT7–IT8 at standard sizes | No — it follows the existing hole | Good on size and finish; inherits the drilled axis | Fast (a light second pass) |
| Boring | IT7 or better, any size, adjustable | Yes — single point cuts to the spindle axis | Very good roundness and cylindricity | Slow, especially in volume |
| Helical interpolation | Depends heavily on machine and tool deflection | Yes — the toolpath defines the axis | Good on shallow bores; degrades with reach | Moderate; one tool covers many sizes |
| Honing | Very fine size control | No | Best-in-class cylindricity and surface | Slowest; a specialist step |
Table 5. Capability bands are broad indications for a rigid setup in common materials. Real capability must be assessed per feature against diameter, depth, material, fixture and the measuring method — we do not quote a single tolerance for all holes. Hole tolerance and quality in depth →
10Common drilling defects and what causes them
Most drilling problems present as one of six visible symptoms. The value of an atlas like this is that it separates the symptom from the cause — and most symptoms have several plausible causes that must be checked in order.
- Likely cause
- Tool runout; unequal lip length from a poor point grind; drill flex on entry; built-up edge on the margins
- Check first
- Runout at the drill tip with an indicator, then the point grind under magnification, then the holder and collet condition
- Then adjust
- Change holder or regrind; add a spot or pilot; if the drawing needs the size held, add a ream or bore — do not chase it with parameters
- Likely cause
- Drill wandering before it is fully engaged; excessive runout; entering on an angled or uneven surface
- Check first
- Whether the entry face is square to the drill; spot condition and included angle; drill length relative to diameter
- Then adjust
- Spot with a larger included angle than the drill point; reduce feed for the first 0.5×D; use a shorter, stiffer drill
- Likely cause
- Remaining material too thin to shear so it bends; worn drill; unsupported exit face
- Check first
- Drill sharpness; whether the exit face is backed; the breakthrough feed
- Then adjust
- Reduce feed at breakthrough; back the exit with a support plate or stacked parts; add a chamfer or a dedicated deburr operation and price it in
- Likely cause
- Chip packing in the flutes; coolant not reaching the tip; no peck cycle where one is needed; a worn drill pushed past its life
- Check first
- Coolant delivery at the tool, not at the nozzle; chip appearance from the last good hole; L:D against the drill type
- Then adjust
- Introduce or shorten the peck increment; move to through-tool coolant or a parabolic drill; set a tool-life limit instead of running to failure
- Likely cause
- Recut chips dragging along the wall; built-up edge breaking away; worn margins
- Check first
- Chip shape and evacuation; coolant concentration and flow; the drill margins under magnification
- Then adjust
- Improve evacuation before touching speeds; raise feed slightly to break chips; if the drawing calls a finish, plan a reaming or boring pass rather than optimising the drill
- Likely cause
- Part not located or clamped repeatably; work offset or datum error; no spot on a long drill; drift in a deep hole
- Check first
- Fixture repeatability and clamping; work offsets and the datum scheme; whether position is measured at entry or at depth
- Then adjust
- Fix the setup first — parameters cannot recover position. Then spot, pilot, or finish with a bore/interpolation pass. How to set CNC work offsets →
11Inspection methods for precision holes
The inspection method should be agreed at quotation, because it changes both what the hole costs and what "in tolerance" means. Every method has a range where it is the right tool and a range where it will mislead you.
| Method | What it tells you | Where it is the right choice | Where it misleads |
|---|---|---|---|
| Plug / pin gauge | Pass or fail against a limit — no numeric value | High-volume go/no-go checking of standard fits | Gives no trend data; a go gauge entering the bell mouth can pass a tapered hole |
| Bore gauge | An actual diameter at a chosen depth | Finding taper and drift by measuring at several depths | Needs setting against a ring or micrometer; operator technique affects the reading |
| Air gauge | Very high-resolution diameter, fast | Repetitive precision bores in production | Requires a master for each size; limited to suitable geometry |
| CMM | True position, cylindricity, perpendicularity, size, all referenced to datums | The only practical way to verify geometric callouts | Slower and costlier; probing force and point density affect the result on thin walls |
| Surface profilometer | Bore-wall roughness parameters | Verifying an Ra or Rz callout | Access into small or deep bores can be impossible |
| Borescope / sectioning | Visual condition, internal burrs, cross-hole intersections | Cross-drilled and internal features nothing else can see | Qualitative; sectioning destroys the part |
Table 6. Match the method to the characteristic. A hole that passes a plug gauge can still be out of position, out of round or too rough — those are different measurements.
12Material-specific drilling considerations
Material changes the failure mode, not just the numbers. Here is what actually goes wrong in each common family, and what the accepted counter-measure is.
| Material family | Dominant problem | Usual counter-measure |
|---|---|---|
| Aluminium alloys (6061, 7075, 2024, 5052) | Built-up edge, long stringy chips, oversize holes, exit burrs | Polished or uncoated flutes, high helix, generous feed, strong evacuation; deburr planned as an operation. Aluminium drilling guide → |
| Low-carbon and free-machining steel | Generally forgiving; chip control on deeper holes | Standard carbide drills, flood or through-coolant, peck beyond 3–4×D |
| Alloy and tool steel (hardened) | Tool wear, heat, edge chipping | Rigid setup, appropriate grade and coating, reduced cutting speed, no interrupted entry |
| Stainless steel (304, 316) | Work hardening, heat, gummy chips welding to the edge | Never dwell or rub — maintain feed; sharp edges, cobalt or coated carbide, strong coolant delivery |
| Titanium alloys | Low thermal conductivity concentrates heat in the tool; galling | Low cutting speed, firm feed, high-pressure through-coolant, short tools, no rubbing |
| Cast iron | Abrasive; dust rather than chips | Wear-resistant grades; often run dry with air or vacuum extraction |
| Copper and brass | Brass can grab and self-feed; copper is gummy | Zero or negative rake geometry for brass; sharp, high-helix tools for copper |
| Plastics and composites | Melting, delamination, fibre pull-out at exit | Very sharp tools, low heat, support the exit face; specific geometries for composites |
Table 7. Failure modes by material family. Specific cutting data should come from the tool manufacturer for the exact grade and geometry you are running.
13DFM checklist for drilled features
Design decisions made in ten seconds in CAD can double the cost of a hole. Run this checklist over any drawing before it goes out for quotation — it is the same list our engineers work through on incoming RFQs.
Cost-reducing choices
- Use standard drill and reamer sizes wherever the function allows
- Keep depth under 3×D if you can; under 5×D if you must go deeper
- Apply a fit tolerance only to the holes that genuinely need one
- Group holes so they can be machined in one setup and one orientation
- Allow a chamfer or radius at entry and exit — it doubles as deburring
- Enter and exit on flat, square faces
- Give a realistic surface finish; Ra 3.2 µm is far cheaper than Ra 0.8 µm
Cost-driving choices
- Non-standard diameters that force a boring operation
- Depth beyond 10×D, especially with a straightness requirement
- Flat-bottomed deep holes
- Tight true position across multiple setups or faces
- "No burr permitted" inside a cross-hole intersection
- Holes breaking into an angled, curved or already-machined surface
- Holes very close to a wall, edge or another hole
- Tolerance bands tighter than the specified gauge can resolve
14The Goldcattle precision hole-making workflow
Xiamen Goldcattle has run in-house precision manufacturing for 26 years as a Chinese National High-Tech Enterprise. Holes are not a side-effect of our process — they are reviewed, planned and verified as their own feature class on every job.
- Drawing and feature reviewEvery hole is classified: clearance, fit, threaded, deep, cross, thin-wall. Anything with a geometric callout is flagged for a finishing operation and a measurement plan at this stage, before the quotation goes out.
- Process chain decisionWe select the chain per hole using the matrix in section 04 — not one blanket process for the part. If a hole cannot be held as drawn, we raise it with you during quotation.
- Fixture and datum strategyPosition capability comes from the setup. We agree the datum scheme, minimise setups, and design clamping that will not distort thin sections.
- CAM programming and simulationCycles, peck increments, retract planes and coolant commands are programmed and simulated before the machine runs. Deep-hole and cross-hole programs get particular attention on breakthrough feed.
- Proving outSingle block and dry run on the first part, then a first article measured against the drawing — not just the diameter, but position, form and finish as specified.
- Locked parameters and monitoringOnce the first article passes, the parameter set is locked to the job. Tool life is set as a limit rather than run to failure, and in-process checks are scheduled at an interval that suits the tolerance.
- Final inspection and documentationPin gauge, bore gauge, CMM and surface roughness inspection as agreed. Reports supplied to the level the project requires.
Worked case: hydraulic manifold, 6061-T6
- Part
- Hydraulic manifold6061-T6, 120 × 80 × 45 mm
- Critical hole
- Ø12 H762 mm deep — about 5×D
- Cross holes
- 4 × Ø6intersecting the main bore
- Requirement
- No internal burrplus true position on the H7 bore
- Volume
- 250 pcsrepeat order
What the drawing implied. The H7 callout ruled out drilling alone. At roughly 5×D, chip evacuation was the governing constraint, and the cross holes meant burrs would form inside the main bore where no standard deburring tool could reach after the fact.
The chain we ran. Spot, then a through-coolant carbide drill at Ø11.7 with a G83 peck cycle, then ream to Ø12 H7. Critically, the cross holes were drilled before the main bore was reamed, so the reaming pass removed the intersection burrs from the main bore wall as it sized the hole. Breakthrough feed on the cross holes was reduced to control the outer burr, and a chamfer tool cleaned the external edges.
Verification. Bore gauge readings at three depths on every part to catch any taper, CMM on the first article and on an agreed sample rate for true position, and a sectioned part from the first batch to confirm the intersections were clean.
Result. The sequence change — cross holes before reaming, not after — removed a manual internal deburring step that would have been slow, inconsistent and difficult to inspect. Values above are specific to this part, this material and this setup; they are not a general capability claim.
FAQFrequently asked questions
Is CNC drilling accurate enough for a press-fit hole?
Usually not on its own. A twist drill is a self-guided tool with two cutting lips, so it tends to produce a hole slightly larger than nominal, with some lobing and positional wander. For a press fit or bearing fit you normally spot, drill 0.2–0.5 mm undersize, then ream or bore to size. The exact allowance depends on diameter, depth, material and the tooling used — treat any published figure as a starting point and confirm on a first article. See our hole quality guide.
What depth-to-diameter ratio can be drilled without pecking?
As a general shop rule, holes up to about 3×D are drilled straight through with a standard jobber or stub drill and flood coolant. From roughly 3×D to 5×D many shops switch to a peck cycle or a through-coolant drill; beyond 5×D, chip evacuation and coolant delivery, not cutting force, become the limiting factor. Deep-hole work above 10×D generally needs a dedicated gun drill or parabolic-flute drill. Actual limits depend on material, drill geometry, coolant pressure and machine rigidity.
Should I always spot drill first?
No. Spotting helps when the surface is uneven, angled or curved, when the drill is long relative to its diameter, or when true position is tight. With a modern rigid carbide drill on a flat, square face, spotting can actually hurt — a spot with the wrong included angle can chip the drill corner. Many shops use a stub pilot or a centring drill with a larger included angle than the drill point instead.
Drilling, reaming, boring or interpolation — how do I choose?
Work backwards from the drawing. If only diameter matters and the tolerance is loose, drill. If diameter and finish matter at a fixed size, ream. If diameter, roundness and position all matter, or the size is non-standard, bore. If you need one tool to cover many sizes, or the part is thin and fragile, helically interpolate with an end mill. The trade is cycle time and tooling cost against capability — see the selection matrix above.
Why is my hole bigger than the drill?
Almost every drilled hole is oversize. The usual contributors are tool runout in the holder or spindle, an asymmetric point grind that makes one lip cut more than the other, drill flex on entry, and built-up edge welding onto the margins. Check runout at the drill tip first, then the point grind, then the entry condition (spot, surface angle, rigidity), before you change cutting parameters.
What causes a burr on the exit side of a hole?
Exit burrs form when the remaining material under the drill point is too thin to shear and instead bends away. Reducing the feed for the last portion of the hole, backing the exit face with a support plate or stacked part, using a sharper point angle, or adding a deliberate deburr step all help. On cross holes the burr forms inside the intersecting bore and usually needs a dedicated deburring tool or abrasive process.
Can CNC drilling hold true position?
Position capability comes from the machine, the fixture and the entry condition more than from the drill. On a rigid vertical machining centre with the part properly located and a spot or pilot, positional scatter of a few hundredths of a millimetre is realistic for short holes. Tight true position on deep or angled holes normally needs a bored or reamed finishing pass and a datum strategy agreed before machining.
Do I need through-tool coolant?
Not for shallow holes. Through-tool coolant becomes valuable once the hole is deep enough that chips cannot clear the flutes on their own — roughly from 4–5×D upward — and in gummy materials such as aluminium and stainless where chips weld and pack. It also lets you drop or shorten peck cycles, which recovers cycle time. See the coolant guide.
What inspection does a precision hole need?
Match the method to the characteristic. Diameter on a production hole is commonly checked with plug or pin gauges; a bore gauge gives an actual reading and shows taper if you measure at several depths; a CMM is used for true position, cylindricity and relationships to datums; a profilometer is used for surface finish. Each has a usable range and an uncertainty, which is why the inspection method belongs on the drawing, not only the tolerance.
Can Goldcattle drill and finish holes to drawing?
Yes — hole making is part of nearly every job we run. We machine in-house on more than 100 machines, with 3-, 4- and 5-axis capability, and we quote the full chain (spot, drill, ream or bore, deburr, inspect) rather than assuming a drill alone will meet print. Upload your drawing and we will tell you which holes are straightforward, which need a finishing operation, and what inspection we would supply.
●The CNC drilling & parameters library
Every page below owns one job. This hub decides which process to use; the linked pages go deep on parameters, code, tooling, coolant, wear and inspection.
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.
Diameter, true position, cylindricity, finish, burrs, process capability and how each one is inspected.
Need precision drilling or complete hole-making support?
Send us the drawing. We will review every hole feature — diameter, tolerance, true position, depth-to-diameter ratio, finish and burr requirements — and come back with the process chain, the inspection method and a price. If a hole cannot be held as drawn, we say so before you place the order, not after the first article.
- 26 years, ISO 9001, National High-Tech Enterprise
- In-house machining — no outsourcing of your holes
- 3-, 4- and 5-axis CNC, 100+ machines
- Pin gauge, bore gauge, CMM and surface roughness inspection
- Samples in 7–15 days, production in 15–25 days
- 24-hour response, 99.8% on-time delivery
