CNC hole depth to diameter ratio (L/D) is the hole’s depth divided by its diameter, and it decides whether a standard twist drill, a peck cycle, a mill, or a deep-hole process can hold size. For ordinary through-holes in 6061-T6 or 304, stay near 4-6xD with a twist drill unless you name a deeper method. Blind holes are stricter because chips pack at the bottom. Dimension full-diameter depth and overall depth separately: a 118° or 135° drill point does not give a flat Ø6 mm to the full tip depth. Put L/D on the PDF with the STEP so a Dongguan quote is not guessing gun drill versus a broken 2 mm drill.
US and EU drawings often show a long thin hole as if it were a short one. The CAM department then pecks forever, walks the drill, or asks for a process you never priced.
This page is the ratio to put on the print, plus how to call depth so inspection matches the tool. It is not a catalog of every drill.
Key takeaways
- Call both full-diameter depth and overall (tip) depth. They are not the same number.
- Treat about 4-6xD as the default twist-drill band. Deeper is a named process.
- Blind holes, small diameters, and gummy stainless all shrink the comfortable L/D.
- Thread depth is a second ratio: tap drill depth must exceed usable thread.
What CNC hole depth to diameter ratio limits
CNC hole depth to diameter ratio limits chip evacuation, drill stiffness, and how much the hole can wander off the axis. A long, skinny drill is a spring. It follows the point, not your CAD axis.
Through-holes at least vent chips out the far side. Blind holes trap chips and coolant at the floor. That is why a 5xD through-hole in aluminum is routine, and a 5xD blind Ø2 mm in 304 is a different job.
NIST manufacturing pages (2026) will not hand you a magic L/D. They will treat the process you name as part of the spec. If the print says “drill” and the ratio says gun drill, the spec is already split.
On CNC milling plates, holes are often pecks from the same 3-axis setup. On CNC turning, on-center holes can run deeper because the drill sits on the spindle axis. Neither setup makes a 20xD Ø1.5 mm hole “free.”
L/D also limits inspection. A CMM probe that cannot reach the floor cannot prove ±0.02 mm at the floor. Ballooned FAI for a deep hole needs a method that matches the depth: pins, a bore gauge at named planes, or a note that only the entry is held. If the hole is datum B in an ASME Y14.5-2018 frame, a wandering deep cylinder is a wandering frame. Keep datum bores in a friendlier band, or name the process that keeps B straight.
Write L/D in the RFQ as one line for the worst hole. Example: “Worst hole Ø4 x 28 mm full diameter, blind, L/D = 7, 6061-T6.” That line prices pecks, coolant, and risk. A pretty pocket on the same drawing does not.
Through vs blind, and why the drill point steals depth
A twist drill ends in a point. The full diameter does not start at the tip. If you need Ø6 mm for 20 mm of engagement, the tip goes deeper than 20 mm. If you dimension only “20 mm deep” with no note, the shop will guess whether you meant full diameter or tip.
Write it: Ø6 through, or Ø6 x 20 mm full diameter, 118° point allowed below. For flat-bottom holes, say mill or end-mill plunge, not drill.
Blind holes need a chip well or extra depth below a thread. If an M6x1 needs 12 mm of usable thread, the tap drill must go deeper than 12 mm, and the full-diameter drill deeper still. Missing that stack is the usual “thread gauge stops short” fail.
Point geometry cheats you in numbers. A 118° point on Ø6 mm adds about 1.8 mm of tip below full diameter. A 135° point adds less. If the wall behind the hole is only 22 mm thick and you asked for 20 mm full diameter plus a 118° point, you break through. Call through, or call a flat mill, or shorten full-diameter depth.
When you send the RFQ, list the worst L/D hole on the part in one line. That hole often sets the process, not the pretty pocket on the same drawing.
Through vs blind is also a burr and coolant story. Through-holes throw a far-side burr into a pocket or a mating face. Say whether you mill the exit, brush it, or accept it. Blind holes pack chips. Peck cycles, dwells, and coolant-through tools are how shops stay in the 3-5xD blind band. They still do not make 12xD Ø2 mm blind a standard 3-axis drill.
Default CNC hole depth to diameter ratio bands
These are typical process bands for CNC hole depth to diameter ratio, not a guarantee from any one factory. Material and diameter move the edges.
| Hole type | Typical L/D band | Process you are implying | Watch-out |
|---|---|---|---|
| Through, aluminum 6061-T6 | about 4-8xD | Twist drill, peck as needed | Exit burr, wander on thin entry |
| Through, 304 / 316 | about 3-6xD | Peck, good coolant, sharp point | Work-hardening if you rub |
| Blind, any metal | closer to 3-5xD | Peck, chip-clear dwells | Packed chips, broken tools |
| Very deep (over 10xD) | Named deep-hole | Gun drill, special coolant-through | Must be on the print |
| Milled / interpolated hole | Depth vs mill stick-out | End mill, not a drill | Finish and roundness |
| Tapped hole | Usable thread about 1.5-3xD | Tap drill deeper than thread | Blind taps need chip room |
Bottom line: if you stay in the twist-drill band and you dimension full-diameter depth, most shops can quote a mill or lathe cycle. If you leave the band, name the process.
Diameter splits that same table. Use this second band chart when the hole is small or the material is gummy.
| Diameter | Material | Through band | Blind band | What to write on the PDF |
|---|---|---|---|---|
| ≥ Ø6 mm | 6061-T6 | 5-8xD routine | 4-6xD | Twist drill, peck if >6xD |
| ≥ Ø6 mm | 304 / 316 | 4-6xD | 3-5xD | Peck, do not rub the floor |
| Ø3-6 mm | 6061-T6 | 4-6xD | 3-5xD | Peck, watch walk at entry |
| Ø3-6 mm | 304 / 316 | 3-5xD | 3-4xD | Sharp point, coolant, named pecks |
| Ø2-3 mm | any | 3-5xD | 3-4xD | Fragile; expect extra time |
| < Ø2 mm | any | Treat as special | Treat as special | Often mill, EDM, or Swiss |
| Any Ø, >10xD | any | Named process | Named process | Gun drill or coolant-through plus method |
The Aluminum Association listings (2026) describe 6061-T6 as a widely machined alloy. It still packs chips in a blind 8xD Ø3 mm hole. “Aluminum is easy” is not an L/D waiver.
Call geometry the way ASME Y14.5-2018 expects: a diameter, a depth, and a note for the point or flat. If the hole also carries position to A-B-C, the depth callout and the position frame are two balloons. Size at the mouth does not prove size at 7xD.
7075-T6 drills well but is more notch-sensitive at intersections. 304 work-hardens if you dwell and rub. POM and other plastics melt and then undersize. Each material moves you toward the conservative side of the band, it does not invent a new physics.
Small diameters, cross holes, and Swiss vs mill
Below about Ø2-3 mm, L/D gets nasty fast. The drill is fragile and walk shows up as oval entry. Swiss CNC machining helps when the hole is on a slender shaft and the bushing keeps the work stiff. It does not make a 12xD Ø1 mm cross hole trivial.
Cross holes that break into a bore need a burr plan. Say whether you mill the intersection, brush it, or accept a remaining burr.
Coolant-through tools and peck cycles extend the comfortable band. They still do not turn “Ø1.8 x 40 mm blind” into a standard 3-axis drill without extra time.
For aluminum parts, through-holes in plates are the friendly case. Stainless and titanium are not. Rubbing at the bottom of a blind hole is how you lose the next tool.
Entry faces matter. A drill starting on a steep 5-axis wall, a mill radius, or a thin web will walk. Spot or mill a flat, or start from a boss. If datum A is that face, a walked entry also walks the hole’s position frame.
Interpolated holes (helical mill) trade drill L/D for mill stick-out. A Ø8 mm hole 12 mm deep in 6061-T6 is a normal helical mill. A Ø8 mm hole 80 mm deep is not. Use interpolation when you need a flat bottom, a non-standard diameter, or a better finish than a drill, and when stick-out still allows a stiff mill.
Threads, coating, and inspection of deep holes
Taps follow the drilled hole. A wandered L/D drill will throw a tap out of pitch or break it. Keep usable thread in a modest multiple of diameter unless you specify a thread mill.
Coating changes diameter. Type II 5-25 µm on a tight hole is a different size after anodizing. Deep coated holes are also hard to rinse. If the hole is a precision bore, mask it or measure after finish, and say which.
Inspection of a 12xD hole is not a caliper job. Use pins, a bore gauge at stated depths, or accept that a CMM probe may not reach the floor. If you cannot inspect the bottom, do not hold ±0.02 mm there.
On the PDF, show diameter, full-diameter depth, and through vs blind. STEP must match those depths. Cosmetic holes in CAD are often modeled shallow.
Worked RFQ hole stack, 6061-T6 manifold, qty 40, raw FAI then Type II:
- Ø8H7 through 18 mm plate: L/D ≈ 2.2, twist drill plus ream. Datum B. Balloon size and perpendicularity to A. Measure after mask or before coat, as the print says.
- Four M6x1-6H through: L/D of tap drill is short. Balloon class with a plug. Position Ø0.2(M)|A|B|C|.
- Ø4 x 28 mm full diameter, blind, 118° point allowed below: L/D = 7. This is above the cozy blind band. Write peck / coolant-through on the note. Balloon size at 5 mm and at 25 mm depth. Do not accept a mouth-only pin.
- M5x0.8 x 10 mm usable thread, blind: tap drill deeper than 10 mm, full-diameter drill deeper still, chip well at the floor. One “M5 x 10 deep” note is not that stack.
FAI method list for those holes: bore gauge or CMM for H7, plug for threads, pin or two-depth bore check for Ø4. If balloon 10 fails at 25 mm depth, recut the peck cycle. Do not release 39 more pieces with the same short full-diameter.
How to inspect hole L/D on first article
Ballooned FAI is how you find out whether the L/D you wrote is the L/D you received. A mouth-only pin check is not an inspection of a 7xD hole. Write depths on the balloon list, then use a tool that can get there.
Method by band:
| L/D band | Typical method on FAI | What “pass” means | Do not do |
|---|---|---|---|
| ≤3xD through | Pin, plug, or CMM at mid-plate | Size and position in the stated zone | Caliper across a burr |
| 4-6xD twist-drill | Pin or bore gauge at entry and mid | Full diameter to the stated depth | Tip-depth only |
| Blind 3-5xD | Depth mic plus pin to full diameter | Floor is chip-clear, diameter holds | “Looks deep” on a photo |
| ~7-10xD peck / coolant-through | Bore check at two or three named planes | No bell-mouth, no packed floor | CMM probe that cannot reach |
| >10xD named deep-hole | Process record plus gauges at named depths | Straightness and size as specified | Treat as a standard drill |
If the hole is datum B, those named planes are how you build the cylinder. ASME Y14.5-2018 does not let you pick the easy mouth and call it B when the assembly uses the full bore. Record alignment: A plane, B axis from the stated depths, C clocking, then position of the rest of the pattern.
Worked actuals for the Ø4 x 28 mm blind hole (L/D = 7). Limit: Ø4.00-4.05 mm full diameter to 28 mm, 118° point allowed below. FAI actuals: 4.02 mm at 5 mm depth, 4.04 mm at 25 mm depth, full-diameter depth 28.2 mm. Pass. If 25 mm depth reads 3.92 mm, fail. Recut with a longer peck or a coolant-through drill. A deviation that says “mouth is fine” is how 39 more sensors will not seat.
Threads on a deep stack need their own rows. GO plug for class, depth mic for usable thread, and a note if the tap hit packed chips. Coating thickness on a deep hole is a poor balloon unless you can measure it. Prefer mask-and-measure-raw for H7, and a coated coupon or a significant surface for Type II 5-25 µm.
Put the method column on the RFQ so the shop prices time. “Inspect Ø4 at 5 mm and 25 mm” is a quote input. “Inspect holes” is not. If the shop cannot reach 25 mm with the gauge they named, change the method or the requirement before you freeze the lot.
FAQ
What CNC hole depth to diameter ratio is safe for twist drills?
About 4-6xD is the usual comfortable band for standard twist drills, with pecks as you approach the high end. Deeper needs a named cycle, not a silent default. Through-holes in 6061-T6 can sit toward 8xD. Blind holes and 304 sit toward 3-5xD. Small diameters shrink the band further. Put the worst hole’s L/D on the RFQ line so the quote includes pecks or gun drill instead of a broken Ø2 mm tool.
How deep can a blind CNC hole be?
Keep blind holes closer to 3-5xD unless you name a deep-hole method. Chips have nowhere to go. Small diameters make that worse. A 5xD blind Ø8 mm in aluminum is ordinary with pecks. A 5xD blind Ø2 mm in 304 is a risk. If you need more depth, write coolant-through, gun drill, or mill-from-both-sides. Dimension full-diameter depth so the point does not steal the floor you thought you had.
Why is my hole short of full diameter at the bottom?
The drill point is using part of the depth. Dimension full-diameter depth separately, or call a flat-bottom mill. A 118° point on Ø6 mm eats about 1.8 mm. If FAI only measured tip depth, the report can pass while a pin stops short of the engagement you need. Balloon full diameter at a stated depth. On the STEP, model the full cylinder to that depth, not a cosmetic dent.
Can I treat hole L/D the same in aluminum and stainless?
No. Stainless work-hardens and wants a more conservative ratio, sharper tools, and real pecks. Aluminum is more forgiving, not unlimited. 6061-T6 still packs chips in a blind 8xD Ø3 mm hole. 304 / 316 will glaze and then walk if you rub the floor. Move stainless toward the low end of the band table, and do not use “aluminum is easy” as a waiver on a mixed-material drawing.
How should I dimension a tapped blind hole?
Give usable thread depth, tap drill depth greater than that, and full-diameter drill depth greater still, plus a note if a thread mill is required. One “M6 x 12 deep” note is not a stack. Usable thread for M6 is often about 1.5-3xD. The tap drill must clear chips below that. Balloon the thread class with a plug, and balloon drill depth with a pin or depth mic. If the hole is also positioned to A-B-C, that is a third balloon.
When do I need gun drilling?
When L/D is beyond what a twist drill and peck cycle can hold on that diameter, often around 10xD and up, or when straightness through a long bore is the function. Name it on the drawing. A silent 15xD Ø5 mm hole will be quoted as hope or as a padded “special.” If that bore is datum B, gun drill (or an equivalent named process) is how B stays a cylinder. Inspect at named depths, not only at the mouth.
Set CNC hole depth to diameter ratio on the print: full-diameter depth, through vs blind, and a named process if you leave the twist-drill band. Send the STEP and PDF with that worst hole called out through the contact page so the quote matches the drill, not a guessed gun-drill job.
