🔧️ DESIGN FOR MANUFACTURABILITY · DEEP HOLES

Design for Deep Hole Drilling
(DFM)

Deep holes are defined by length-to-diameter (L/D) ratio, not absolute depth. Get the L/D, the hole geometry, and the material right at the drawing board and you cut per-hole cost 30–60%. Get them wrong and you are locked into gundrilling, BTA, or rework for the life of the part. These are the design rules that make deep holes manufacturable.

≤3:1Max L/D, standard drillPeck drilling to 5–10:1

Ø1mmPractical gundrill minimumBelow Ø3mm is risky

IT9–IT10Tolerance as-drilledIT7–IT8 w/ fine boring

≥1.5 × DEdge distance / wall2 × D for tapped holes

CLASSIFICATION

What Counts as a Deep Hole?

In machining terms a “deep hole” is any hole where depth exceeds three times the diameter (L/D > 3:1). On standard machining centers, conventional drilling loses effectiveness quickly beyond this point — chips cannot evacuate, coolant cannot reach the cut, and the tool starts to deflect. Most precision shops treat L/D > 5:1 as genuinely challenging, and L/D ≥ 10:1 as the point where specialized deep hole processes — gundrilling, BTA, or ejector drilling — become mandatory.

L/D Ratio	Classification	Recommended Method	Relative Cost Factor
< 3:1	Conventional hole	Standard twist drill	0.5×
3:1–5:1	Moderately deep	Peck drilling / extended-length drill	1.0× (baseline)
5:1–10:1	Deep hole	Modified twist drill / gundrill	1.3–1.8×
10:1–50:1	Deep hole	Gundrilling (single-lip) or BTA	2–5×
50:1–100:1	Very deep hole	BTA or ejector drilling	5–10×
> 100:1	Extreme deep hole	BTA / ejector with specialized support	10×+

💡 Cost escalates in steps, not a line: a 10 mm hole at 5×D costs about the same as at 2×D, but the same hole at 10×D costs 2–3× more, and at 50×D it costs 5–10× more. Beyond L/D > 30, specialized deep hole methods are no longer optional.

COST DRIVERS

Why L/D Drives Cost More Than Diameter

Machining time plus tooling typically account for 70–85% of total hole cost, and both scale with depth, not diameter. Studies of machining cost confirm that modifying hole diameter has little effect on cost when the same drill type is used, while every millimeter of depth directly raises process cost. That is why the first DFM question is always: can this hole be shorter?

L/D Ratio	Method	Cost Impact
≤ 3:1	Standard drilling	Baseline
3:1–5:1	Peck drilling	+10–20%
5:1–10:1	Peck drilling, extended drills	+30–80%
10:1–30:1	Gundrilling or BTA	+200–500%
> 30:1	Specialized gundrilling / EDM	+500% or more

Tolerance is the second multiplier

Moving from ±0.1 mm to ±0.025 mm can raise hole cost 2.5–4×; tolerances below ±0.005 mm can multiply cost more than 15×. Reaming, boring, and honing add another 3–5× of finishing cost on top of the drilled hole. Apply tight tolerances only where parts actually mate.

⚠️ Tooling is the hidden line item: gundrills are job-specific tools and at low volumes the tooling cost is typically passed straight to the customer. A custom solid carbide gundrill can cost more than $100 versus under $30 for an HSS drill — and carbide is frequently the only viable option above roughly 15×D. Standard diameters keep you on off-the-shelf tooling.

CHECKLIST

The Deep Hole Design Checklist

Nine rules, in priority order. Every rule traces directly to a machining cost or quality risk.

Minimize L/D ratio

Reduce depth or increase diameter first. A hole at L/D 50 costs 2–4× more than one at L/D 10; at L/D 100 it costs 5–10× more.

Prefer through holes

The tool exits completely, chips evacuate freely, and depth control is eliminated. Through holes are significantly cheaper than blind holes of equal depth.

Use standard diameters

Custom diameters need custom tooling with premium pricing and long lead times. Standard sizes are off the shelf; minimize the number of different sizes per part.

Account for the drill tip cone

Gundrills and BTA drills leave a conical bottom: roughly 0.3×D for a 118° point, 0.35×D for 135°, 0.25×D for 90°. Call out the full-diameter depth, not the cone tip — a “15 mm” blind bore with a 118° point is 15 mm to the shoulder plus ~3 mm of cone on a Ø10 mm hole. Flat-bottom specs add 2–3× cycle time and may need a special tool.

Keep edge distance & spacing

≥1.5 × D from hole center to edge (2 × D for tapped), ≥2 × D center-to-center between same-diameter holes. Thin walls let the drill deflect.

Make entry & exit perpendicular

Drills must enter and exit at 90°. Angled starts cause drill walk, deflection, and premature tool failure. Spot-face or bushing any angled entry.

Step diameters downward

Larger diameter near the surface, decreasing with depth. Keep each step change ≤50% of the larger diameter and each step length > its own diameter.

Avoid intersecting holes

A drill crossing a cavity or cross-hole follows the path of least resistance and wanders on re-entry. If unavoidable, keep ≥2 drill diameters of support material.

Limit thread engagement

Engagement beyond 1.5 × the nominal diameter adds no strength, only cost and tap-breakage risk. Cap tap depth near 3 × D and chamfer the entry.

REDESIGN

Minimize L/D Ratio — Design Alternatives

If a deep hole is functionally unavoidable, redesign to reduce the effective L/D before accepting the machining penalty. All four strategies below are free to specify at the drawing stage and each can halve machining cost.

🔧 Step-down (two-stage) holesDrill a larger diameter to the section needing the tight tolerance, then drill the small precise hole only at the bottom where it is required.

↔ Machine from both sidesSplit a through hole in half — each tool runs at half the L/D, bringing the job back inside standard machine capability.

🔗 Two-part assemblySplit the long hole across two components and join them. The effective L/D of each drilled half drops sharply.

🛠 Counterbore + bushingReplace a long precision bore with a clearance hole plus precision counterbores at each end to seat bushings or bearings.

🎯 Larger diameterWhere load allows, increasing D while holding L lowers the L/D ratio and often allows a standard machine and twist drill.

📝 Core it, if castingFor large or deep holes in cast parts, a cored hole saves material and rough machining — but plan a finish pass, since cores hold only loose tolerance.

💡 Design tip: if the deep hole survives review, question the next-most-expensive feature — the tolerance. A step-down or counterbored design often shrinks the tight-tolerance zone from the full hole length to two short local regions, which is where the real money is.

HOLE FEATURE RULES

Hole Feature Design Rules

Entry & Exit Geometry

Drill entry and exit surfaces should be perpendicular (90°) to the drill axis. If the tip contacts a slanted or non-planar surface it will wander because its axis is not perpendicular.
If an angled entry is unavoidable, add a spot face or starting bushing to give the drill a flat, stable start surface. A pilot hole 1–2 diameters deep works the same way.
The exit surface matters too: exit burrs are uneven around the circumference on non-perpendicular surfaces, making deburring difficult and risking drill damage at breakout.
Keep the entry zone simple — avoid cross-holes or keyways near the entry, and provide clearance for a drill bushing fixture where protrusions surround the hole.

Through vs. Blind Holes

Prefer through holes — the tool exits completely, improving chip evacuation and coolant flow and eliminating precise depth control. Secondary ops (reaming, threading) are easier on through holes.
Design blind holes 25% deeper than the functional depth to accommodate chip accumulation and the conical drill point.
A standard drill leaves a conical bottom at its tip angle (118° or 135°). Flat bottoms require an end mill, adding 2–3× cycle time — only specify when functionally required.
For blind bored holes in turning, provide tool relief at the bottom — a minimum of about 3% of the hole diameter to simplify honing, reaming, and grinding.

Stepped (Multi-Diameter) Holes

Diameter should decrease with hole depth — larger diameter nearer the surface. Avoid interior steps with increased diameter, which require a boring bar.
Diameter difference between adjacent steps should not exceed 50% of the larger diameter.
Minimum axial length of each step should generally be greater than the step diameter.
Consider combination step tools to collapse multiple operations into one tool change.
Keep any single bored surface below L/D 4:1–5:1 (up to 8:1 with a carbide boring bar) to limit bar deflection.

Intersecting & Cross Holes

Avoid intersecting deep holes with cavities or other holes. When a drill intersects a cavity it follows the path of least resistance and may wander significantly when it re-enters material.
If intersection is unavoidable, ensure the drill-through material thickness is at least 2 drill diameters so the first hole acts as a bushing to support the drill through the exit.
Prefer an on-center intersection over a scalloped design — it minimizes load unbalance and burr formation.
Plan deburring: exit burrs will be uneven around the circumference and require a secondary operation.

⚠️ Common mistake: partial holes. If a large portion of the hole axis is outside the material, the drill wanders. Keep at least 75% of the hole circumference within material, and never let the hole axis intersect a part edge.

TOLERANCE & STRAIGHTNESS

Tolerance & Straightness vs. Cost

The most common DFM mistake on deep holes is over-specification. Specify the roughest operation and the widest tolerance that still meets function. Deep hole drilling alone typically holds IT9–IT10 at Ra 2–6.3 μm; fine boring, rolling, and honing climb toward IT7–IT8 and Ra 0.1–0.8 μm — and each step adds cost.

Operation	Tolerance (IT)	Ra (μm)	Notes
Drilling / nesting (rough)	IT9–IT10	6.3–12.5	Rough pass only
Gundrill / BTA as-drilled	IT8–IT10	1.6–6.3	Typical commercial deep hole
Fine boring	IT8–IT9	1.6–3.2	Adds roundness control
Rolling / burnishing	IT8–IT9	0.2–0.4	Adds compressive residual stress
Honing	IT5–IT7	0.1–0.4	Best finish; does not fix drift

💡 Prefer runout over straightness: circular runout or total indicator runout (TIR) is the most practical way to control straightness and concentricity together. Concentricity alone does not control roundness — a hole can be perfectly concentric yet egg-shaped. Holding 0.003 in. size/runout over 6 in. of length is routine; holding it over 120 in. is a different problem entirely. Rough drilling typically allows about 0.001 in. of runout per inch of depth.

⚠️ Specify critical zones: if bore concentricity matters only near the ends, say so on the drawing — it significantly reduces cost. Straightness on a deep hole typically lands at 0.1–0.15 mm per 1000 mm; below that you are paying for a special process. Loosening a countersink tolerance or dropping a global profile callout can cut inspection cost 3–5× on individual features.

MATERIALS

Material Selection Notes

Raw material is usually the smallest part of machined cost — machinability is the hidden multiplier. A cheap, hard-to-machine alloy is often more expensive overall than a pricier free-machining grade, and the effect compounds in deep holes where chip evacuation and tool wear dominate.

Material	Machinability vs. C360 brass	Cost multiplier vs. 6061-T6	Deep-hole notes
6061-T6 aluminum	~90%	1.0× (baseline)	Best per-dollar deep hole performance
1018 carbon steel	~70%	1.1–1.2×	Good baseline; carbon steel runs ~30–50% over aluminum
4140 alloy steel (annealed)	~65%	1.3–1.6×	Machines well annealed; above ~HRC 50, grinding replaces drilling
303 stainless	~55%	1.5–1.8×	Free-machining grade, chosen over 304/316 for deep holes
316 stainless	~45%	1.8–2.2×	Work-hardens fast; slow speeds, ~20% more coolant, ~15% more machining hours
Ti-6Al-4V	~20%	4.0–7.0×	Slow speeds, work hardening, low feed = rubbing risk

⚠️ Work hardening: austenitic stainless (304/316) and titanium harden if the tool dwells or rubs, leaving the hole wall harder than the cutting edge. Deep holes in these materials need a constant aggressive feed, sharp positive-rake carbide with TiAlN coating, and high-pressure coolant — never let the tool idle in the cut.

💡 Don’t over-specify material: 316L specified for “corrosion resistance” on an indoor part with no moisture exposure adds roughly 40–60% machining cost for an unneeded property. Stainless adds 100–150% over aluminum; a hardened alloy adds more on top of that. Match the grade to the actual service environment.

METHOD SELECTION

L/D vs. Method Selection

Match the process to the L/D ratio and the diameter — the cheapest method that holds the hole wins. Gundrilling is most cost-effective from about Ø1 mm to Ø50 mm; above roughly Ø50–60 mm, BTA and ejector take over.

L/D Ratio	Recommended Method	Notes
5:1–10:1	High-performance twist drill, through-coolant	Peck drilling cycles (G73/G83)
10:1–20:1	Special deep-hole drills, high-pressure through-coolant	CNC machining center capable
20:1–100:1	Standard gundrilling machine	Ø1–50 mm sweet spot
100:1–200:1	High-performance gundrilling machine	Tool whip becomes a real issue
200:1–400:1	Specialist purpose-built machine	Multiple tool changes typical

💡 The 40:1 threshold: at roughly L/D 40:1, purpose-built deep hole machines gain a significant advantage over gundrills run on lathes or machining centers because tool whip dominates. Counter-rotation — part and tool spinning in opposite directions — reduces runout by about half and is the route to the best straightness on long bores.

⚠️ Pilot holes: gundrilling on a lathe needs a pilot hole 1–2 diameters deep and roughly 0.0005–0.001 in. larger than the drill. Position the drill in the hole before starting rotation, and keep fewer than 40 drill diameters unsupported.

🎯

D < 15mm→ Gundrill

⚖

D 15–30mm→ Compare methods

⚡

D 30–150mm→ BTA / ejector

🏭

D > 150mm→ BTA or trepan

REDESIGN EXAMPLES

Before/After Redesign Examples

Four concrete changes that turn an expensive deep hole into a manufacturable one.

Example 1Deep blind hole → through hole

BeforeØ10 mm blind, 120 mm deep (L/D 12:1), flat bottom required

AfterØ10 mm through hole, conical bottom, thread depth limited to 1.5 × D

Savings+25% blind-depth allowance eliminated, depth-control op removed, no flat-bottom tool

Example 2Full-length precision bore → counterbores + bushing

BeforeOne long Ø20 mm precision bore, 400 mm (L/D 20:1), ±0.01 mm over full length

AfterØ25 mm clearance hole plus precision counterbores at each end to seat bushings

SavingsTight-tolerance zone shrinks from 400 mm to two short counterbores; standard tooling

Example 3One-end drill → drill from both sides

BeforeØ15 mm × 600 mm drilled from one end (L/D 40:1)

AfterDrilled from both ends, 300 mm each (L/D 20:1), meeting on center

SavingsEffective L/D halved; standard gundrill machine holds the hole

Example 4Custom diameter → standard diameter

BeforeØ13.4 mm custom gundrill, special order

AfterØ13.0 mm or Ø13.5 mm standard tool

SavingsOff-the-shelf tooling, shorter lead time, lower cost per edge

RULES OF THUMB

DFM Rules of Thumb

Rule	Guideline
Deep hole definition	L/D > 3:1; specialized processes mandatory ≥ 10:1
Standard drilling maximum	L/D ≤ 3:1; peck drilling to 5–10:1
Blind hole depth allowance	+25% beyond functional depth (chips + cone)
Edge distance (center to edge)	≥ 1.5 × D; 2 × D for tapped holes
Hole-to-hole spacing	≥ 2 × D center-to-center
Thread engagement	max 1.5 × D (no strength gain beyond)
Tap depth	≤ 3 × D
Cone clearance below thread	3–5 pitch lengths past the last full thread
Stepped-hole step change	≤ 50% of the larger diameter
Partial holes	≥ 75% of circumference within material
Cross-hole support thickness	≥ 2 drill diameters
Boring bar L/D	≤ 4:1–5:1; to 8:1 with carbide bar
Internal coolant	40–100+ bar beyond ~8:1
Straightness (typical)	0.1–0.15 mm per 1000 mm
Tolerance as-drilled	IT9–IT10; finish operations to IT7–IT8

✅ The one-line rule: design for the shortest possible hole, the standard diameter, the through configuration, and the loosest tolerance that still functions — in that order of priority.

COMMON MISTAKES

Common DFM Mistakes

⚠️ Flat-bottom blind holes: a standard drill leaves a 118° or 135° conical bottom. A flat-bottom spec adds 2–3× cycle time and may require a special tool. Unless the flat bottom is a functional sealing surface, accept the standard cone.

⚠️ Over-tolerancing: tightening from ±0.1 mm to ±0.025 mm can raise cost 2.5–4×. Reserve tight tolerances for critical mating surfaces and use commercial tolerances everywhere else.

⚠️ Deep threads: engagement beyond 1.5 × D adds no strength and increases tap-breakage risk in a hole you cannot easily recover. Cap tap depth near 3 × D, chamfer the thread entry, and specify thread depth and drill depth separately on blind holes.

⚠️ Trying to break the rules without a plan: never attempt L/D > 5:1 with a standard twist drill on production parts — chips cannot evacuate, heat cannot dissipate, and the axis will deviate. A 0.1° angular error produces about 1.75 mm of deviation over 1000 mm of depth.

Design for Deep Hole Drilling
(DFM)

What Counts as a Deep Hole?

Why L/D Drives Cost More Than Diameter

Tolerance is the second multiplier

The Deep Hole Design Checklist

Minimize L/D Ratio — Design Alternatives

Hole Feature Design Rules

Entry & Exit Geometry

Through vs. Blind Holes

Stepped (Multi-Diameter) Holes

Intersecting & Cross Holes

Tolerance & Straightness vs. Cost

Material Selection Notes

L/D vs. Method Selection

Before/After Redesign Examples

DFM Rules of Thumb

Common DFM Mistakes

Key Safety Points

Keep Reading

Design for Deep Hole Drilling(DFM)

What Counts as a Deep Hole?

Why L/D Drives Cost More Than Diameter

Tolerance is the second multiplier

The Deep Hole Design Checklist

Minimize L/D Ratio — Design Alternatives

Hole Feature Design Rules

Entry & Exit Geometry

Through vs. Blind Holes

Stepped (Multi-Diameter) Holes

Intersecting & Cross Holes

Tolerance & Straightness vs. Cost

Material Selection Notes

L/D vs. Method Selection

Before/After Redesign Examples

DFM Rules of Thumb

Common DFM Mistakes

Key Safety Points

Keep Reading

Design for Deep Hole Drilling
(DFM)