How Should You Design Deep Holes and Small-Diameter Holes for CNC Machining?

Deep and small-diameter holes can look simple in CAD while creating disproportionate machining risk. As depth increases relative to diameter, drill rigidity decreases, chips travel farther before leaving the bore, and straightness becomes harder to control. Small drills add fragility and leave less margin for unstable entry geometry, restrictive tolerances, or obstructed tool access.

Good hole design starts with function, not an arbitrary diameter or depth. Identify whether the hole controls flow, fastener engagement, alignment, sealing, clearance, or another requirement. Then reserve tight specifications for the characteristics that protect that function.

The decisions below translate that intent into machinable geometry, clear drawing callouts, practical inspection criteria, and a complete CNC machining RFQ.

How Should You Classify Holes by Depth-to-Diameter Ratio?

Classify each drilled hole by dividing its required depth by its diameter. Depths up to about 3×D are preferred, 4–5×D are generally more manageable, and ratios approaching 8–10×D should trigger supplier review of tooling, chip evacuation, straightness, inspection, and process selection.

The ratio is a screening tool, not a universal capability statement. A 20 mm-deep hole with a 5 mm diameter is 4×D. At a 2 mm diameter, the same depth becomes 10×D and presents a very different drilling problem.

Material grade remains part of the decision. A hole in a readily machinable aluminum condition may not need the same cutting strategy as the same ratio in a material prone to greater tool wear or work hardening. A blind bore also retains chips differently from a through-hole.

Record the diameter, total drilled depth, usable full-diameter depth, through or blind condition, entry geometry, tolerance, surface finish, and functional purpose. These details let the supplier judge whether conventional CNC drilling is suitable or whether a dedicated deep-hole process¹ deserves consideration.

Example: A 3 mm hole at 24 mm depth has an 8×D ratio. Treat it as an exception requiring explicit review, not simply as an ordinary 24 mm-deep hole.

Should You Increase Hole Diameter Before Choosing Specialty Drilling?

Yes, if the hole cannot be shortened and its function permits a larger bore. Increasing diameter allows a stiffer tool, improves chip evacuation, and may move the feature from a high-risk aspect ratio into a range better suited to conventional CNC drilling.

Separate the modeled diameter from the minimum functional diameter. A flow passage needs a sufficient opening, a clearance hole must admit its fastener, and an alignment bore may require a defined fit. Those functions do not always demand one exact nonstandard drill size.

Before fixing the dimension, define:

• The minimum opening required by the function.
• The largest diameter that preserves wall thickness, sealing land, and assembly clearance.
• Whether a standard drill size² within that range is acceptable.
• Whether diameter, position, straightness, or surface finish controls acceptance.
• Whether reaming is permitted for a fitted bore.

A larger diameter lowers the depth-to-diameter ratio without changing the part depth. It can reduce reliance on a long, fragile tool and may simplify chip removal. Check the change against edge distance, adjacent passages, threaded features, pressure boundaries, and the remaining wall.

Scenario: A 20 mm-deep clearance passage is initially modeled at 3 mm diameter, giving a ratio above 6×D. If the assembly accepts a 4 mm standard hole, the ratio becomes 5×D. Conventional drilling may then be more practical, although material, entry geometry, tolerance, and wall thickness still require review.

Do not enlarge a bearing, sealing, metering, or precision alignment bore merely to simplify production. State the allowable functional range and invite the supplier to propose a standard diameter or staged operation within it.

When Is a Small-Diameter Hole Functionally Necessary?

A small-diameter hole is justified when flow, venting, metering, fastening, sensing, or assembly genuinely requires it. Holes below roughly 2.5–3 mm deserve deliberate review because drill fragility, chip evacuation, material behavior, depth, tolerance, surface finish, and inspection can dominate manufacturing risk.

Challenge a tiny hole before carrying it into the released drawing. Ask what would fail if its diameter increased, its depth decreased, or it became a larger passage. A feature retained only because it appeared in an early model may not justify its tooling and scrap exposure.

Use a functional review:

• Does diameter control flow, pressure response, venting, or fastening?
• Could a standard drill size meet the same requirement?
• Can depth remain near or below 3×D?
• Is the hole through or blind, and how can chips leave it?
• Is the entry flat and square to the drilling direction?
• Which tolerance or finish requirement is functional?
• What inspection method and frequency are required?

Name the exact material grade and condition³ rather than saying only “metal” or “plastic.” Material affects chip formation, heat, tool wear, and the drilling plan. Quantity and production intent matter as well: a prototype for design learning may need different verification from stable repeat production.

One common mistake is combining a diameter below 3 mm, depth above 8×D, tight position, and fine bore finish without identifying the controlling function. That combination removes process flexibility and may require specialized tooling and structured inspection. Classify each small hole as functional, assembly-related, or non-critical, then request DFM feedback on diameter, depth, tolerance, and finish before release.

How Should You Design Hole Entries and Blind-Hole Bottoms?

Provide a flat, stable entry surface square to the drilling direction whenever geometry permits. For blind holes, accept the normal drill-point form unless a flat region performs a defined function; angled entries and fully flat bottoms can require preparation or secondary machining.

A drill establishes its path at the entry. A flat surface normal to that path supports more balanced initial contact than an angled, curved, stepped, or interrupted surface. Unstable contact can encourage wandering before the tool is fully engaged, with greater consequences in a long bore.

If a non-square entry is unavoidable, show the acceptable finished geometry. A spot face may create a local surface perpendicular to the drilling direction, while pilot drilling may establish a path for a later operation. Unless the final part specifically requires one method, allow the supplier to choose the preparation rather than prescribing unsupported cutting parameters.

Does a blind hole need a flat bottom?

Usually only when the bottom locates a component, controls usable volume, provides clearance, or performs another defined function. A drilled blind hole naturally retains a conical drill-point region⁴. Calling out one depth without distinguishing full-diameter depth from drill-point depth creates room for conflicting interpretations.

Example: A pin must enter 12 mm into a blind bore, but the drawing says only “12 mm deep” and depicts a flat bottom. State the required full-diameter depth and whether extra drill-point depth is acceptable. If the pin bears against a flat area, define the necessary flat diameter and location rather than requiring the entire bottom to be precision-flat.

Use section views to expose hidden entries, adjacent cavities, breakthrough restrictions, sealing lands, wall thickness, and local finish requirements.

How Should Drilling Direction and Tool Access Be Arranged?

Arrange holes along as few accessible machining directions as the design permits, preferably principal axes with unobstructed drill-and-holder clearance. Side-entry, angled, or multi-face holes may require indexing, extra fixtures, or multi-axis positioning, increasing setup effort and cross-setup tolerance risk.

Tool access means more than an open line through the bore. The drill body, holder, fixture, clamps, and surrounding geometry all need clearance along the approach path. A hole may be visible in CAD yet remain inaccessible with a sufficiently short and rigid tool.

Review the arrangement diagnostically:

• Can several holes be produced from one orientation?
• Does a wall, boss, flange, or clamp obstruct the holder?
• Is the entry normal to the tool axis?
• Does an angled hole need fixed indexing or continuous multi-axis motion?
• Do opposite-face holes share a critical position or coaxial relationship?
• Can the part be held without concentrating force on a thin wall?

Features machined in one setup are generally easier to control relative to one another because they avoid datum transfer between reclampings⁵. This does not mean every multi-side component needs simultaneous five-axis machining. Fixed-angle holes may suit indexed positioning, while accessible orthogonal holes may suit separate controlled setups. The supplier should select the simplest arrangement that reaches every feature and protects the specified relationships.

Where positions accumulate through chained dimensions across several faces, tolerance stack-up may obscure the actual assembly requirement. Use functional datums and identify which cross-face relationships truly matter.

Provide the complete 3D model with section views for hidden approaches. Mark angled holes, obstructed entries, restricted clamping regions, and critical face-to-bore relationships so setup and inspection effort can be assessed during quotation.

Which Hole Characteristics Actually Need Tight Control?

Tightly control only the hole characteristics that protect function. Diameter may govern fit, position may govern assembly, straightness may govern alignment or flow, and surface finish may govern sealing or sliding. Restricting all four on a deep small bore can add avoidable machining and inspection risk.

A hole is not one specification. Size, form, orientation, location, and surface condition describe different aspects of performance. Applying the same restriction to all of them can force extra operations without improving the part.

Reaming may provide a controlled fitted diameter, but it does not automatically correct position, straightness, or every finish requirement. Likewise, a tighter plus-or-minus size does not describe how a bore relates to a mounting face or another hole. Use geometric dimensioning and tolerancing⁶ when location, orientation, or coaxiality protects function, with datums representing assembly and inspection.

Avoid a blanket fine-finish note on every bore. Deep-hole finish can require additional passes and measurement, so localize it to sealing, sliding, or other functional zones. If anodizing or plating affects a fitted bore, clarify whether the accepted dimension applies before or after finish buildup.

The RFQ should pair every critical characteristic with its acceptance limit, measurement condition, inspection frequency, and required report.

How Much Material Should Remain Around a Deep Hole?

Begin the design review with at least 1.5×D from the hole center to a nearby edge and at least 2×D for tapped holes. Treat these as conditional references because material grade, depth, wall support, spacing, clamping, and nearby functional surfaces can change feasibility.

Measure edge distance from the hole centerline to the nearest free edge, not from the bore wall. The remaining ligament⁷—the material between the hole and that edge—must tolerate drilling forces, tapping loads where applicable, clamping pressure, and the finished part’s service load.

The 1.5×D and 2×D references are starting points, not automatic acceptance rules. A shallow through-hole in a thick supported region differs from a high-aspect-ratio blind hole beside a tall thin wall. Closely spaced bores may also interact even when each appears acceptable in isolation.

Review these features together:

• Diameter, depth, and through or blind condition.
• Center-to-edge distance and actual remaining wall thickness.
• Center-to-center spacing between adjacent holes.
• Thread diameter and required engagement.
• Nearby pockets, counterbores, channels, and sealing lands.
• Material grade and condition.
• Available clamping and backing support.

Insufficient support can contribute to edge breakout, distortion, cracking, or damage to the wall between passages. Thin aluminum regions may also move under clamping or cutting pressure, so define the measurement condition if a wall or nearby bore is tolerance-critical.

Do not try to solve weak geometry with a blanket tight tolerance. Mark critical surrounding surfaces, minimum wall regions, permitted breakthrough, no-clamp areas, and required inspection. The supplier can then review workholding and drilling sequence against the complete model.

How Should Drilled Depth and Thread Depth Be Specified?

Specify full thread depth and total drilled depth as separate requirements. Where the joint permits, allow approximately three to five thread pitches of extra drilled depth for tap clearance, and avoid requesting more thread engagement than the assembly function and material require.

A blind threaded hole contains several depth zones: the full-diameter drilled region, usable full thread, incomplete thread near the bottom, and drill-point region. One depth callout cannot communicate them reliably.

The drawing should state:

• Thread standard, nominal size, pitch, and class where required.
• Minimum full-thread depth⁸ or functional engagement length.
• Total drilled depth, including permitted drill-point space.
• Bottom-clearance and breakthrough restrictions.
• Entry chamfer or countersink when function requires it.
• Thread inspection and reporting expectations.

Allowing approximately three to five thread pitches beyond the required thread depth is a supported design reference. It gives the tap room before the bottom of the drilled hole. That allowance remains conditional on available wall thickness, adjacent cavities, sealing boundaries, and whether extra depth would weaken a critical section.

Functional thread engagement around 1.5–2× the screw diameter may be sufficient in suitable applications, but material, loading, joint design, and applicable engineering requirements must govern the decision. Extra engagement is not automatically beneficial. A small thread, long engagement, and high drilled-hole ratio combine fragile tooling with difficult chip evacuation.

A note such as “M4 × 20 deep” is ambiguous because it may refer to thread depth, drill depth, or both. Replace it with separate full-thread and total-drill requirements and state whether breakthrough is prohibited. This gives the supplier a clear basis for drilling, tapping, clearance, and inspection.

How Should Intersecting Holes, Internal Burrs, and Inspection Be Defined?

Define where passages intersect, whether internal burrs are permitted, what flow or assembly clearance must remain, and how acceptance will be verified. Distinguish first-article, sampling, and production checks because inaccessible crossings can add deburring, cleaning, measurement, and reporting effort.

An intersecting passage creates an internal edge that may be unreachable from outside the part. Chips or burrs at the crossing can restrict flow, catch a wire or tube, contaminate a system, or prevent a component from passing. A general “deburr all edges” note does not define an achievable internal condition.

Pin gauges may help verify accessible bore size or clear passage. Borescope inspection⁹ may support visual review of an internal crossing. Neither method should be specified automatically; select it according to the characteristic and acceptance criterion.

Scenario: Two drilled channels form a manifold, but the drawing controls only their diameters. Add the required clear intersection, internal burr acceptance, cleaning condition, and first-article verification. If straightness matters, control it separately rather than assuming that an open passage proves alignment.

Burr direction also matters when a drill exits into a cavity, sealing face, or assembly surface. Identify the sensitive side so the supplier can plan drilling order and deburring access.

What Should a Hole-Specific CNC Machining RFQ Include?

Send both geometry and controlled specifications: a 3D model, current 2D drawing, exact material, quantity, production intent, hole table, critical tolerances, finish, inspection scope, revision, and delivery expectations. Confirm that the requested process is CNC machining rather than an unrelated sheet metal or molding process.

CNC machining removes material from stock by drilling, boring, reaming, milling, or turning. CNC turret punching¹⁰ and CNC punch press work use programmed punches on sheet metal. Metal stamping uses dedicated dies, sheet metal fabrication may combine cutting, punching, bending, welding, and finishing, and plastic injection molding forms polymers in a mold.

“CNC turret punching, CNC punch press, CNC-controlled stamping equipment, or metal stamping depending on the actual process” is not one standard process term. Clarify whether it means CNC turret punching, a CNC punch press, CNC-controlled stamping equipment, general metal stamping, or another process before comparing quotations.

Hole-specific RFQ approval checklist

• ☐ Current 3D CAD model showing complete geometry and approach space.
• ☐ Controlled 2D drawing with units, part number, active revision, and governing-document note.
• ☐ Exact material grade and condition, plus required material documentation.
• ☐ Quantity and prototype, pilot, or repeat-production intent.
• ☐ Hole table with identifier, diameter, total depth, usable depth, through or blind condition, and criticality.
• ☐ Thread standard, pitch, class where required, full-thread depth, drilled depth, and bottom restriction.
• ☐ Critical size, position, straightness, coaxiality, and surface-finish requirements.
• ☐ Functional datums and GD&T where feature relationships matter.
• ☐ Entry geometry, drill-point allowance, intersections, burr limits, and passage-clearance criteria.
• ☐ Finish, coating, cleaning, masking, and edge requirements where applicable.
• ☐ Inspection method, frequency, reporting scope, and acceptance criteria.
• ☐ Delivery expectations, partial-shipment needs, and revision stability.
• ☐ Permission to propose standard diameters, adjusted depths, or another suitable drilling process.

If the model and drawing conflict, identify the controlling document before quotation. Complete evidence lets the supplier assess tooling, setup, chip evacuation, inspection, cost, and schedule without filling gaps with conservative assumptions.

For a manufacturability recommendation or quotation, send the 3D model, controlled 2D drawing, material grade, quantity, prototype or production intent, hole table, critical tolerances, surface finish, inspection expectations, revision level, and delivery requirements. Flag every deep, small, blind, threaded, angled, or intersecting hole.

References