DFM: Hole Design

Holes are the most common machined feature, and the easiest to get wrong. This page covers which hole type to use, how small you can go, how deep, how to design blind and threaded holes, and the positioning rules that prevent distortion and scrap.

Hole Types at a Glance

Not all holes are equal. Each type serves a different purpose, requires a different tool, and has different cost and tolerance implications. Choose the simplest type that meets the functional requirement.

Hole Type	Process	Typical Tolerance	Cost Factor	Typical Application
Through Hole	Drilling	±0.1–0.25mm	1.0× (baseline)	General fastening, fluid passage, weight reduction
Blind Hole	Drilling (stopped)	±0.1–0.25mm depth ±0.5mm	1.1×	Threaded holes, dowel pins, set screws, hidden fasteners
Counterbore	Drill + end mill	±0.05–0.1mm (bore dia.)	1.3×	Socket head cap screws, dowels, bushings
Countersink	Countersink cutter	±1° angle, ±0.1mm dia.	1.2×	Flat-head screws, deburring, self-centering
Spot Face	End mill / face cutter	±0.05mm flatness	1.2×	Bearing seat, washer face on rough casting surface
Reamed Hole	Drill + ream	±0.005–0.02mm	1.5–2.0×	Locating pins, bearing bores, precision fits (H7)

Simplest is cheapest A through hole drilled in one operation is the lowest-cost hole. Every additional feature — depth stop, counterbore, countersink, reaming — adds a tool change, an operation, and cost. If a flat-head screw is not visible or functional, use a socket head cap screw in a counterbore (or even a through hole with a nut on the back) to save cost.

Minimum Hole Diameter by Process

Every hole-making process has a practical minimum diameter. Below these limits, tool deflection, breakage, and chip evacuation become problematic. The values below assume steel or aluminum. Harder materials (titanium, stainless) may require larger minimums.

Process	Min. Diameter	Max. Depth (L/D)	Achievable Tolerance	Surface Finish (Ra)	Relative Cost
Twist Drill (standard)	0.5mm (#80)	5–8×D	±0.05–0.15mm	1.6–6.3μm	1.0× (baseline)
Reaming	1.0mm	10–15×D	±0.005–0.02mm	0.4–1.6μm	1.5–2.0×
Boring (single-point)	3.0mm	Up to 50×D	±0.005–0.01mm	0.4–1.6μm	2.0–3.0×
Gun Drilling	2.0mm	Up to 100–150×D	±0.01–0.05mm	0.8–3.2μm	3.0–5.0×
BTA Deep Hole	6.0mm	Up to 150×D	±0.01–0.03mm	0.4–1.6μm	4.0–8.0×
Center Drill	0.5mm	1–2×D	±0.05mm	3.2–6.3μm	0.3× (spotting only)
EDM (small hole)	0.1mm	Up to 20–50×D	±0.005–0.02mm	0.8–3.2μm	5.0–10.0×

Small holes in hard materials Drills below 2mm in stainless steel or titanium are fragile. Expect higher breakage rates and slower feeds. For production runs, consider using carbide micro-drills with peck drilling cycles. For holes below 1mm in hard materials, wire EDM may be more economical despite the higher per-hole cost, because scrap from broken drills is eliminated.

Blind Hole Design

A blind hole does not break through the workpiece. It is more complex than a through hole because the drill must stop at a precise depth, the bottom has a conical shape from the drill point, and chips must evacuate upward through the flutes.

Bottom Geometry

Standard twist drills produce a conical bottom — this is not optional, it is inherent to the tool geometry. The drill point angle determines the shape of the cone.

Drill Point Angle	Material Application	Bottom Cone Depth	Notes
118°	General purpose (steel, aluminum, most materials)	~0.3×D	Standard point. Most common. Good chip formation in most materials.
135°	Hard materials (stainless, titanium, superalloys)	~0.35×D	Flatter point = thinner web = easier penetration in hard materials.
90°	Soft materials (aluminum, brass, plastics)	~0.25×D	Sharper point, reduces wandering in soft materials.
Flat bottom (end mill)	When a true flat bottom is required	0 (flat)	Requires an end mill or flat-bottom drill. Slower and more expensive. Use only when functionally necessary.

Depth Limitations

Depth Range	L/D Ratio	Method	Cost Impact
Shallow	≤ 3×D	Standard drilling, single pass	Baseline
Standard	3–5×D	Standard drilling, peck cycle	+10–20%
Deep	5–10×D	Peck drilling, extended-length drills, reduced feed	+30–80%
Very deep	10–30×D	Gun drilling or BTA system	+200–500%
Ultra-deep	> 30×D	Specialized gun drilling, EDM hole popping	+500%+

Depth callout matters When specifying a blind hole depth, you are specifying the depth of the full-diameter portion, not the tip of the drill cone. If you need a specific flat-bottom depth, say so — and expect an end mill operation (higher cost). If you call out "drill 15mm deep" with a 118-degree point on a 10mm drill, the actual hole is 15mm to the shoulder of the drill, but the point extends ~3mm deeper.

Chip Evacuation in Blind Holes

In a blind hole, chips have only one way out — back up through the flutes. This is the primary reason deep blind holes are expensive and slow. Design strategies to mitigate:

Design Approach	Benefit	When to Use
Through hole instead of blind	Chips exit the bottom. No peck cycle needed. Faster, cheaper.	Whenever the part design allows it. Always prefer through holes.
Reduce depth to ≤ 3×D	Chips evacuate easily in a single peck. No special tooling needed.	Standard fastener holes. M6 bolt only needs 9–12mm depth in aluminum.
Peck drilling cycle	Drill retracts periodically to clear chips. Prevents packing and breakage.	Any blind hole deeper than 3×D. Standard CNC programming practice.
Chip clearance groove	Enlarged area at the bottom gives chips space to accumulate without jamming.	When the hole must be blind and deep, and through-hole is not possible.

Threaded Holes

Threaded holes are the single most common hole feature in CNC machined parts. Getting the depth, clearance, and entry chamfer right prevents tap breakage, weak joints, and assembly problems.

Minimum Thread Depth by Material

The required thread engagement depth depends on the material being threaded. Softer materials need more engagement to develop full strength. Harder materials need less.

Material (Threaded)	Min. Thread Depth	Recommended Depth	Max. Useful Depth	Why
Aluminum (6061, 7075)	1.5×D	1.5–2.0×D	2.5×D	Soft — needs more threads to avoid stripping
Steel (mild, 4140)	1.0×D	1.0–1.5×D	1.5×D	Strong enough with standard engagement. Beyond 1.5×D adds no strength.
Stainless Steel (304, 316)	1.0×D	1.0–1.25×D	1.5×D	Strong. Deeper threads dramatically increase tapping time and tap wear.
Titanium (Ti6Al4V)	0.75×D	0.75–1.0×D	1.25×D	Very strong — deep threads waste machining time. Galling risk.
Brass / Bronze	1.5×D	1.5–2.0×D	2.5×D	Soft — strips easily. Consider helicoil for high-load joints.
Plastics (nylon, Delrin)	2.0×D	2.0–2.5×D	3.0×D	Very soft. Use coarse pitch. Consider self-tapping or inserts for repeated assembly.

D = nominal thread diameter. Example: M8 in aluminum needs minimum 12mm thread depth (1.5 × 8).

Bottom Clearance for Tapped Blind Holes

The tap cannot cut threads all the way to the bottom of a blind hole. You must provide clearance below the required thread depth.

Factor	Value	Explanation
Tap lead-in (chamfer)	2–3 pitch lengths	First 2– threads from the tap point are incomplete — they don't count as full engagement.
Bottoming tap uncut	1–2 pitch lengths	Even a bottoming tap leaves uncut material at the very bottom.
Total clearance below threads	3–5 pitch lengths	For M10x1.5: add 4.5–7.5mm below the last full thread.

Specify hole depth separately from thread depth Call out both values: thread depth and total drill depth. Example: M8x1.25-6H THRU 12, DRILL 18 DEEP. This gives the machinist clear instructions: drill to 18mm, thread to 12mm, leaving 6mm of clearance for the tap point. If you only call out "M8x1.25 DEEP 12", the machinist must guess the drill depth — and may drill too shallow, causing tap breakage.

Entry Chamfer

Feature	Specification	Purpose
Internal thread entry chamfer	0.5–1.0mm × 120° countersink	Prevents the first thread of the bolt from catching the sharp hole edge. Prevents cross-threading. Always add this.
External thread lead chamfer	0.5–1.0mm × 45°	Helps the bolt start into the nut. Standard practice.

Blind vs Through for Threaded Holes

Factor	Through Hole	Blind Hole
Cost	Lower — single drill + tap, no depth stop	Higher — requires depth control, peck cycle, clearance
Thread strength	Limited by part thickness	Controlled by specified depth
Chip evacuation	Chips exit the bottom — no issues	Chips pack at the bottom — can break taps
Assembly access	Bolt passes through — nut on other side	Bolt does not pass through — cleaner appearance
Sealing	Cannot seal (hole is open on both sides)	Can seal if bottom is plugged or closed

Deep Holes (L/D > 5)

When the hole depth exceeds 5 times the diameter (L/D > 5), the hole is classified as "deep." Deep holes are progressively more expensive because chip evacuation, coolant delivery, and tool rigidity all become challenging.

Deep Hole Methods

L/D Range	Recommended Method	Tool	Cost Factor	Key Consideration
5–8×D	Peck drilling (standard CNC)	Extended-length twist drill	1.2–1.5×	Reduce feed by 30–50% vs standard depth. Peck depth = 1–2×D.
8–15×D	Peck drilling or gundrill	Oil-hole drill or gundrill	1.5–3.0×	Coolant-through-tool is strongly recommended. Short pecks (0.5–1×D).
15–40×D	Gun drilling	Single-lip gundrill	3.0–5.0×	Dedicated gundrilling machine or special CNC setup. High-pressure coolant through the tool.
40–100×D	Gun drilling or BTA	BTA deep hole drill	4.0–8.0×	BTA system pulls chips out the exterior tube. Better for larger diameters (≥15mm).
> 100×D	Specialized gundrill / EDM	Custom gundrill or wire EDM	8.0–15.0×	Very few shops can do this. Lead time increases. Consider redesigning.

Cost escalation is exponential A 10mm hole that is 20mm deep (2×D) costs roughly the same as a 10mm hole that is 50mm deep (5×D). But a 10mm hole that is 100mm deep (10×D) costs 2–3× more. A 10mm hole that is 500mm deep (50×D) costs 5–10× more. If you don't need a deep hole, don't design one. If you do, consider whether a stepped or staged approach can achieve the same function at lower cost.

Gun Drilling vs BTA

Property	Gun Drilling	BTA (Boring and Trepanning Association)
Diameter range	1–50mm	15–200mm+
L/D capability	Up to 150×D	Up to 150×D
Coolant delivery	Through the drill's internal coolant hole	Around the outside of the drill tube (annular)
Chip removal	Chips exit through the flute (internal)	Chips exit through the drill tube (external)
Surface finish	Ra 0.8–3.2μm	Ra 0.4–1.6μm (better)
Best for	Small diameter deep holes, single-piece production	Larger diameter, higher volume, better surface finish

Hole Positioning

Where you place holes on a part affects machinability, part accuracy, and structural integrity. Holes too close to edges cause breakout. Holes too close to each other cause wall distortion. Holes in thin sections cause deflection during drilling.

Edge Distance Rules

Rule	Minimum Value	Why
Hole center to edge (general)	≥ 1.5×D	Prevents edge breakout during drilling and ensures the tool has sufficient material around the hole.
Hole center to edge (countersink / counterbore)	≥ 1.5×D + countersink radius	The larger diameter of the countersink must also clear the edge.
Hole center to edge (tapped hole)	≥ 2.0×D	Material around a tapped hole must resist the outward force during tapping. Closer than this and the wall bulges or cracks.
Hole center to edge (close-tolerance / reamed)	≥ 2.0×D	Thin walls deflect during reaming. You cannot hold tight tolerances if there is not enough surrounding material.

Hole Spacing Rules

Rule	Minimum Value	Why
Center-to-center (same diameter)	≥ 2.0×D	Prevents web between holes from collapsing. Ensures structural integrity.
Center-to-center (different diameters)	≥ (D1 + D2) / 2 + 1mm	The web between two different-sized holes must be at least 1mm (preferably 2mm+) to survive machining.
Staggered holes	≥ 1.5×D each direction	Even staggered holes need minimum edge distance in both axes.
Hole to machined feature (slot, pocket)	≥ 1.0mm wall (3mm preferred)	Thin walls between holes and pockets deflect during machining and cause out-of-tolerance features.

Distortion from nearby holes Drilling a hole relieves internal stress in the material. If holes are closely spaced, drilling one hole can cause the web between holes to warp or the adjacent hole to go out-of-round. This is especially true in castings, forgings, and heat-treated parts. Mitigation: (1) increase spacing, (2) rough-drill all holes first then finish to final size, (3) stress-relieve before final machining.

Common Mistakes

#	Mistake	What Happens	Correct Approach
1	Hole too close to edge	Material breaks out at the edge during drilling. Hole is incomplete, part is scrap.	Maintain ≥ 1.5×D from hole center to nearest edge. For tapped holes, ≥ 2.0×D.
2	Blind hole too shallow for thread depth	Tap bottoms out before reaching full thread depth. Incomplete threads = weak joint. Tap can break in the hole.	Hole depth = thread depth + 3–5 pitch lengths. For M8x1.25 deep 12mm: drill at least 16–18mm.
3	Not specifying thread depth and drill depth separately	Machinist must guess clearance. May drill too shallow (broken tap) or too deep (wasted cycle time).	Call out both: "M10x1.5-6H THRU 15, DRILL 22 DEEP". Never leave drill depth ambiguous.
4	Specifying a flat bottom when conical is acceptable	Requires an end mill operation instead of a drill. 2–3× longer cycle time for the hole.	Accept the drill-point cone unless a flat bottom is functionally required (e.g., a pressure seal seat, a locating pin seat).
5	Deep hole (L/D > 10) without considering gun drilling	Standard peck drilling produces an inaccurate, tapered hole. Tool breaks. Excessive cycle time.	For L/D > 10, specify gundrilling or accept wider tolerances. Discuss with the machinist before committing to the design.
6	Counterbore diameter too close to edge	The larger counterbore diameter breaks out at the edge even though the through-hole is fine.	Edge distance must account for the counterbore diameter, not just the through-hole diameter: ≥ 1.5×D_cbore.
7	Threaded hole in very thin wall	Wall bulges during tapping. Threads are incomplete or the wall cracks. No thread strength.	Minimum wall thickness around a tapped hole = 0.5×D (1.0×D preferred). Below this, use a nut plate or insert.
8	Holes clustered too close together	Web between holes collapses during machining. Distortion causes positional errors. Part scrap.	Center-to-center spacing ≥ 2.0×D for same-diameter holes. For different diameters, web thickness ≥ 2mm.
9	No entry chamfer on threaded hole	Bolt's first thread catches the sharp hole edge. Cross-threading, misalignment, damaged threads on assembly.	Always add a 120° countersink (0.5–1.0mm wide) at the thread entry. Costs pennies, prevents scrap.
10	Over-specifying reamed holes where drilled suffices	Reaming adds a tool change, a finishing pass, and tighter tolerance on the pre-drill. Cost increases 50–100% for no functional gain.	Use reaming only for locating pins, bearing bores, and precision fits (H7). For clearance holes and general fastening, a drilled hole is sufficient.

← Wall Thickness & Fillets

Tolerance Design →