CNC Deep Hole Drilling: Design, Tooling and Inspection Guide

CNC deep hole drilling becomes difficult long before a hole looks unusually deep on a drawing. As the drill moves farther from the entry surface, chip evacuation becomes less reliable, coolant has a harder time reaching the cutting edges, tool deflection increases and small alignment errors can grow into meaningful position or straightness error.

For a buyer, the result is more than a slow drilling cycle. An unsuitable hole design can cause broken drills, trapped chips, rough walls, tapered diameters, off-center exits, internal burrs and parts that are difficult to clean or inspect. These risks increase when the hole is small, blind, intersected, tightly toleranced or machined in stainless steel, titanium and other demanding materials.

This guide explains how CNC deep hole drilling works, how depth-to-diameter ratio affects process selection, when peck drilling or through-tool coolant is appropriate, how engineers can design more manufacturable holes and how a supplier should inspect the finished result.

What Is CNC Deep Hole Drilling?

A deep hole has a large depth compared with its diameter. The relationship is normally expressed as a depth-to-diameter ratio, written as L/D or D × diameter.

For example:

• A 10 mm diameter hole that is 30 mm deep has a 3:1 L/D ratio.

• A 10 mm diameter hole that is 100 mm deep has a 10:1 L/D ratio.

• A 4 mm diameter hole that is 120 mm deep has a 30:1 L/D ratio.

There is no single ratio at which every hole becomes “deep.” Machine builders, drill manufacturers and production engineers may use different categories. In general machining, a hole beyond approximately 3×D already requires greater attention to chip removal. At higher ratios, dedicated long drills, pilot holes, internal coolant or specialized deep-hole processes become increasingly important.

The challenge depends on more than ratio. A 12×D hole in free-machining aluminum is not the same as a 12×D hole in titanium. Diameter, tolerance, material, entry geometry, exit condition, machine capability and production volume must all be considered.

Why Deep Holes Are Difficult to Machine

Chip Evacuation

The drill flutes must carry chips from the cutting point to the hole entrance. In a shallow hole, the distance is short and coolant can reach the cutting zone easily. In a deep hole, chips travel along a confined path while new chips continue to form.

If chips become too long, pack in the flute or weld to the tool, torque and heat rise quickly. The drill may rub the hole wall, damage the surface or break below the entry. Recovering a broken tool from a valuable part can be difficult or impossible.

Deep-hole drilling therefore depends on both chip formation and chip evacuation. Our separate CNC chip control guide explains the wider relationship between chip shape, tool geometry, feed and coolant.

Coolant Delivery

External flood coolant may not penetrate effectively to the tip of a long drill. The visible flow at the hole entrance does not prove that the cutting edges are being cooled or that chips are being transported out.

Through-tool coolant delivers fluid through internal passages close to the cutting zone. The system must provide suitable pressure, flow and filtration for the tool diameter and passage size. Pressure helps coolant reach the cut, while flow volume carries chips away. More pressure alone cannot correct an unsuitable flute, poor chip shape or blocked passage.

Tool Deflection and Hole Drift

A long drill is more flexible than a short drill. Entry error, spindle runout, uneven cutting forces, material variation or an interrupted feature can push it away from the intended axis. The hole may begin within position tolerance but drift as depth increases.

This is why entry preparation, a rigid holder, low runout and the correct pilot strategy matter. Simply slowing the feed does not necessarily improve straightness; an underfed drill may rub, form poor chips and wander more.

Heat

The cutting zone is enclosed and difficult to observe. Heat can accelerate tool wear, change chip behavior and affect diameter. In stainless steel and titanium, heat management is especially important because these materials can concentrate heat at the cutting edge.

Limited Process Visibility

The machine operator cannot directly see the drill tip or chips at the bottom of the hole. Spindle load, coolant flow, sound, chip appearance and tool-life data become important process signals. A stable deep-hole operation must be validated rather than judged only from the first completed part.

Understanding Depth-to-Diameter Ratio

L/D ratio is a useful starting point, not a complete specification.

These ranges are not universal limits. Modern tool families can cover different ratios, and the manufacturer's instructions for the exact drill always take priority. Sandvik Coromant, for example, offers purpose-designed tools for deep holes up to 30×D in suitable applications.

When reviewing a drawing, calculate ratio using the full cutting depth, including drill-point allowance where relevant. A blind hole specified with a full-diameter depth may require a deeper drilled cavity to account for the conical point.

Deep Hole Drilling Methods

Conventional Twist Drilling

A standard twist drill can make relatively shallow holes efficiently. It may use external coolant and a simple drilling cycle. As depth increases, flute capacity, rigidity and coolant access become limiting factors.

Long general-purpose drills should not automatically be treated as deep-hole drills. A purpose-designed tool may have a different point geometry, margin, coating, flute profile and internal coolant passage.

Peck Drilling

Peck drilling advances in increments and periodically retracts or partially retracts the tool. The movement can break chips and create room for coolant or chips to travel.

Two common strategies are:

• Full-retract pecking: the drill retracts far enough to clear the hole. It can improve evacuation but adds cycle time and repeated re-entry.

• High-speed or chip-breaking pecking: the drill retracts a small distance to break the chip without leaving the hole completely.

Pecking is useful in some applications, but it is not a universal deep-hole solution. Excessive pecking increases cycle time and may rub the hole or repeatedly shock the cutting edge. Some modern through-coolant carbide drills are designed to drill continuously without pecking.

Haas notes in its high-speed peck drilling guidance that peck strategy depends on drill type, coolant and material. The correct cycle should follow the drill manufacturer's application data rather than a fixed shop rule.

Through-Coolant Carbide Drilling

Solid-carbide deep-hole drills combine rigidity, precise geometry and internal coolant delivery. A short pilot drill is often used first so the long tool enters on-axis. Depending on the tool family, the long drill may enter the pilot at reduced speed, begin coolant flow and then accelerate to the recommended cutting data.

Important controls include:

• Pilot diameter and tolerance.

• Pilot depth and point geometry.

• Alignment between pilot and long drill.

• Holder quality and tool runout.

• Coolant cleanliness, pressure and flow.

• Controlled entry and withdrawal procedures.

• Tool-specific speed and feed.

Do not start a long flexible drill at full speed against an unprepared surface unless the toolmaker explicitly approves that procedure.

Gun Drilling

Gun drilling is a dedicated deep-hole process that uses a long, single-lip tool with internal coolant and an external chip channel. Guide support helps the tool produce long, straight holes with controlled diameter and finish.

It is commonly considered for high L/D ratios, demanding straightness or production volumes that justify specialized equipment. A guide bushing or accurately prepared pilot may be part of the process, depending on the machine and tooling system.

Gun drilling can produce excellent results, but it requires appropriate equipment, filtration, setup and process knowledge. It should be evaluated early when the drawing contains a very long precision bore rather than treated as a rescue operation after conventional drilling fails.

BTA and Ejector Drilling

BTA-style systems are used for larger-diameter deep holes and high material-removal rates. Coolant flows through the annular space around the tool, while chips return through an internal tube. Ejector systems use a related double-tube flow arrangement.

These methods are more common in dedicated deep-hole machines and larger industrial components than in ordinary prototype machining centers. They may be appropriate for hydraulic cylinders, energy equipment, shafts and other long bores.

Trepanning

Trepanning removes an annular ring and leaves a central core rather than converting the complete hole volume into chips. For a large deep hole, this can reduce power and material removal. It requires suitable geometry, tool support and a plan for the recovered core.

Electrical Discharge Machining

EDM may be considered when the material is very hard, the hole is extremely small or conventional cutting access is unsuitable. Hole-drilling EDM is often used to create starter holes or small passages in conductive materials.

EDM has different speed, surface and recast-layer considerations. It should be selected because it fits the requirement, not because the drawing omitted enough information for a conventional process review.

Pilot Holes and Entry Conditions

A pilot hole guides a long drill during entry. Its geometry should be matched to the deep-hole tool rather than chosen as a generic pre-drill.

The pilot normally needs:

• A compatible diameter and tolerance.

• Enough depth to support stable alignment.

• A bottom or point form recommended by the tool supplier.

• Good position and perpendicularity to the intended axis.

• A clean, burr-free entrance.

An oversized or misaligned pilot may allow the long drill to move before it is fully supported. An undersized pilot can rub the margins or prevent entry.

Flat and Perpendicular Entry

A flat surface perpendicular to the hole axis gives the cutting edges balanced engagement. Angled, curved, cast or uneven entries apply force to one side first and can deflect the tool.

Where function permits, add a spotface or perpendicular starting pad. If the entry must be angled, identify it on the drawing so the supplier can choose a pilot, milling operation or tool designed for that condition.

Inclined or Curved Exit

When a drill exits an inclined surface, one cutting edge breaks through before the other. The asymmetric force can damage the edge, enlarge the exit or create a heavy burr. Reduce feed before breakthrough when the tooling guidance calls for it and provide support where practical.

Blind Holes, Through Holes and Hole Bottoms

Blind-Hole Depth

A standard drill leaves a conical bottom. Drawings must distinguish between:

• Full-diameter usable depth.

• Total depth to the drill point.

• Thread depth.

• Tap-drill depth.

• Required bottom clearance.

If a mating pin needs 40 mm of cylindrical engagement, specifying a 40 mm total drilled depth may not provide 40 mm of full diameter. The drill-point allowance, chip space and inspection access must be considered.

Flat-Bottom Requirements

A flat-bottom hole may require a specialized drill, end mill, boring tool or secondary operation. “Flat” should be defined with a functional tolerance if it matters. A visual flat bottom and a tightly controlled perpendicular floor are different requirements.

Breakthrough

Through holes need exit clearance and a plan for the breakthrough disc or burr. Some indexable drills can eject a disc at high speed; Sandvik Coromant recommends enclosing the machine in its drilling safety guidance.

The part and fixture must also support the exit area. A thin unsupported wall can deform as the drill breaks through.

Intersecting Holes and Internal Burrs

Cross holes and internal passages create some of the hardest deep-hole problems. The drill experiences interrupted cutting at the intersection. Chips can catch in the opening, and a burr can remain where ordinary visual inspection cannot reach.

The drawing should identify:

• Every intersection.

• Which passage is drilled first if sequence matters.

• Whether an internal burr is permitted.

• The required edge break at the intersection.

• Cleanliness and loose-particle limits.

• How the result will be inspected.

Possible deburring methods include controlled brushing, abrasive-flow processes, thermal deburring, electrochemical deburring or purpose-designed cutting tools. The correct method depends on material, geometry, tolerance and cleanliness needs.

Avoid the vague note “remove all burrs” when the intersection is inaccessible. State the functional acceptance criterion and agree on a verification method.

Tool Runout, Holders and Machine Alignment

Runout causes one cutting edge to work harder than the other. In a deep hole, the effect can reduce tool life, enlarge the diameter and contribute to drift.

A stable setup may require:

• A precision collet, hydraulic chuck or shrink-fit holder.

• Clean tool and holder interfaces.

• Short practical stick-out.

• Measured spindle and tool runout.

• Verified machine alignment.

• A rigid workholding setup.

• Balanced cutting data for the tool and material.

The longest available drill is not necessarily the best choice. Use only the length required for the feature, because unnecessary overhang reduces rigidity.

Coolant Pressure, Flow and Filtration

Deep-hole drilling needs a coolant system, not just a pressure number.

Pressure

Pressure helps force coolant through the tool and into the cutting zone. Small internal passages can create high pressure with relatively low flow.

Flow

Flow carries heat and chips out of the hole. A system can show adequate gauge pressure yet provide insufficient chip-transport volume.

Filtration

Fine tool passages can be blocked by dirty coolant. Filtration should suit the orifice size and toolmaker's requirements. Coolant concentration and condition also affect lubrication, corrosion and tool life.

Delivery Timing

Coolant should be established before the deep drilling cut begins when the process requires it. Interrupting flow while the tool is buried can allow chips to pack and heat to rise.

Haas describes how through-spindle coolant can improve chip removal and permit single-pass deep drilling with suitable tooling. Actual performance still depends on tool passage size, material and application data.

Material-Specific Considerations

Aluminum

Aluminum can produce high chip volume and long ductile chips. Some grades are adhesive and can form built-up edge. Polished flutes, sharp geometry, generous chip space and suitable lubrication help prevent packing.

Deep aluminum holes can look easy because cutting forces are low, but chip volume can overwhelm a small flute. Cosmetic surfaces near the entrance and exit also need protection from chips.

Carbon and Alloy Steel

Steel behavior varies widely with grade, hardness and heat treatment. Stable chip breaking and appropriate coatings support reliable drilling. Hard inclusions, scale or interrupted entry can damage the drill.

Provide the exact alloy and condition rather than only “steel.” A process developed for annealed material may not transfer to hardened stock.

Stainless Steel

Austenitic stainless steels can work-harden and produce tough chips. The drill should cut continuously rather than dwell and rub. Coolant delivery, feed, geometry and tool condition are critical.

If a drilling cycle repeatedly re-enters a work-hardened surface, tool wear may accelerate. Process changes must be based on the specific drill and grade.

Titanium

Titanium has low thermal conductivity and a strong tendency to concentrate heat at the cutting edge. Deep titanium holes require conservative, validated data, effective coolant and careful tool-life control. Tool failure can occur quickly after wear reaches an unstable stage.

Nickel Alloys

Nickel-based alloys combine high strength, heat and work-hardening behavior. Tool geometry, carbide grade, coolant and engagement should be selected for the exact alloy. A qualified process and early tool replacement may be more economical than running to sudden failure.

Cast Iron

Cast iron often creates short, abrasive chips. Evacuation may be easier than with a ductile material, but abrasive wear and fine particles affect tooling, filtration and machine cleanliness.

Engineering Plastics

Plastics may soften, expand or smear under heat. A deep plastic hole can close slightly after drilling or accumulate stringy chips. Sharp tools, controlled temperature and allowances for material relaxation may be needed.

Hygroscopic plastics should be conditioned appropriately before final measurement. Thin-walled plastic features can also distort under clamping force.

Common Deep-Hole Defects and Their Causes

Oversize Diameter

Possible causes include tool runout, damaged margins, chip recutting, excessive vibration, unsuitable pilot size or spindle misalignment.

Undersize Diameter

Tool wear, thermal behavior, material recovery or an unsuitable tool can produce an undersize result. Plastics and some metals may change after the cut or after unclamping.

Taper

Diameter can change from entrance to bottom because of tool wear, heat, deflection or chip packing. Measure at relevant depths rather than checking only the entry.

Hole Drift

The exit or internal axis moves away from the intended line. Entry condition, pilot alignment, drill flexibility, runout and material variation are common contributors.

Poor Straightness

A hole may meet entry and exit position while its internal axis curves between them. Straightness must be specified and measured separately when function requires it.

Rough Surface or Scoring

Chips trapped between the margin and wall can score the bore. Built-up edge, worn tools, vibration or inadequate coolant can also reduce finish.

Exit Burrs

High feed at breakthrough, unsupported material or an unsuitable point geometry can create a heavy burr. An angled exit makes the problem more difficult.

Internal Burrs at Cross Holes

Interrupted cutting leaves material at passage intersections. The burr may be invisible from the outside and can break loose during service.

Broken Tool in the Hole

Packed chips, blocked coolant, excessive runout, wear, incorrect feed or an unstable peck cycle can cause failure. The response should include containment and root-cause review, not simply installation of another identical drill.

How Deep Holes Are Inspected

The inspection plan should match the functional requirement. One gauge rarely verifies every characteristic.

Diameter

Depending on size and depth, diameter may be checked with:

• Pin or plug gauges.

• Air gauges.

• Bore gauges.

• Internal micrometers.

• Coordinate measuring probes with suitable reach.

• Specialized bore-measurement systems.

A go/no-go plug may confirm size at accessible regions but not reveal taper or local damage along the complete depth.

Position

The hole entrance and exit can be measured on a CMM or with dedicated fixtures. For a blind hole, accessible datum strategy and probe reach matter.

Position tolerance controls location relative to datums. It does not automatically control straightness of the entire internal axis unless the specification and verification method address that need.

Straightness and Drift

Straightness can be evaluated with specialized probes, borescopes, air-gauge systems, ultrasonic or other application-specific methods. Destructive sectioning may be used during process development when non-destructive access is limited.

For critical parts, agree on the method before production. A requirement that cannot be measured with available equipment creates commercial and quality risk.

Surface Finish

A conventional stylus may not reach a small deep bore. Replica methods, specialized long-reach instruments, optical systems or qualified process evidence may be needed.

Specify surface roughness only where it supports function. An unnecessarily fine finish can require reaming, honing or another secondary process.

Internal Burrs and Cleanliness

Borescopes can inspect accessible passages and intersections. Flushing, particle counting, filter-patch testing or gravimetric methods may be specified for hydraulic, medical or fluid-control components.

The cleaning standard should define what is measured, the extraction method and the acceptance limit. “Clean” is not an objective inspection requirement by itself.

Leak and Flow Testing

Pressure decay, helium, bubble, hydraulic or flow testing may be appropriate for internal passages. A leak test confirms sealing performance, while a flow test can reveal blockage or restriction. Neither replaces dimensional inspection when diameter and position are also critical.

Designing Deep Holes for Manufacturability

Reduce L/D Ratio Where Possible

Increase the diameter, shorten the depth or drill from two sides if function allows. A modest design change can replace specialized tooling with a more reliable process.

Two-sided drilling creates an alignment and intersection challenge, so it is not automatically better. Define how the passages may meet and whether a step or mismatch is permitted.

Use Standard Diameters

Standard drill sizes are easier to source and replace. A nonstandard diameter may require custom tooling, reaming or boring. If the size is not functionally critical, choose a common value and apply a realistic tolerance.

Provide a Stable Entry Surface

Add a perpendicular pad or spotface when the surrounding geometry is angled or curved. The pad must be large enough for the pilot or drill diameter and should not create an unwanted stress concentration.

Allow Tool and Holder Access

Check the complete drill and holder envelope, not only the hole diameter. Nearby walls, bosses and fixture surfaces can prevent a rigid holder from reaching the axis.

Avoid Unnecessary Blind Depth

Extra depth increases cycle time, tool exposure and chip-evacuation distance. Provide only the depth needed for flow, engagement or assembly, plus necessary manufacturing allowance.

Separate Functional Requirements

State diameter, position, straightness, surface finish and cleanliness separately. Do not assume a tight diameter automatically delivers a straight, accurately located or clean hole.

Define the Exit and Intersections

Show whether the hole breaks through a flat, angled or curved surface and identify every cross passage. Add internal burr and cleanliness requirements where they matter.

Avoid Ultra-Tight Tolerance Along the Entire Depth Unless Necessary

A tight bore tolerance may require drilling followed by reaming, boring, honing or another process. Apply the strict limit only to the region that locates, seals or guides the mating component.

Discuss Critical Holes Before Design Release

A supplier can compare conventional drilling, long carbide drilling, gun drilling, EDM and multi-sided access before the geometry is frozen. Early DFM review is much cheaper than recovering a broken tool or redesigning a finished assembly.

How Deep Hole Requirements Affect Cost

Deep holes increase cost through several mechanisms:

• Long or specialized cutting tools.

• Pilot drilling and extra tool changes.

• Slower, validated entry and exit cycles.

• High-pressure coolant and fine filtration.

• More conservative tool-life limits.

• Additional setups or dedicated equipment.

• Internal deburring and cleaning.

• Long-reach or specialized inspection.

• Greater scrap risk if failure occurs late in the process.

Quantity also changes the best method. A prototype may justify a flexible machining-center process, while a repeated production part may justify custom drills, gun drilling or a dedicated fixture.

Do not compare quotations only by drilling cycle time. Confirm whether internal deburring, cleaning, straightness verification, tool-breakage containment and inspection reporting are included.

What to Include in a Deep Hole Drilling RFQ

Send the supplier enough information to choose and quote the process correctly:

• Native 3D CAD model and controlled 2D drawing.

• Exact material grade, condition and hardness.

• Hole diameter and tolerance.

• Full-diameter depth and total depth.

• Blind or through condition.

• Entry and exit surface geometry.

• Hole position and datum scheme.

• Straightness, roundness or cylindricity requirements.

• Surface roughness where functional.

• Cross-hole and internal intersection details.

• Internal burr and edge-break limits.

• Cleanliness, leak or flow-test requirements.

• Inspection method and reporting requirements.

• Prototype quantity, production quantity and annual demand.

• Mating components or a description of hole function.

Use the broader CNC machining RFQ checklist to prepare the rest of the quotation package.

Copy-and-Paste RFQ Template

Please quote CNC deep hole drilling for the attached model and drawing. Material: [grade, condition and hardness]. Hole diameter: [value and tolerance]. Full-diameter depth: [value]. Total depth: [value]. L/D ratio: [value]. Entry surface: [flat, angled or curved]. Exit condition: [blind, flat breakthrough, angled breakthrough or cross hole]. Critical requirements: [position, straightness, surface finish, burr, cleanliness, leak or flow]. Quantity: [prototype and production quantities]. Please identify the proposed drilling method, pilot requirement, internal-deburring method, inspection plan and any DFM changes that could improve reliability or reduce cost.

Questions to Ask a CNC Supplier

1. What drilling method do you recommend for this L/D ratio and material?

2. Will the process use a pilot hole and through-tool coolant?

3. Is peck drilling necessary for the selected tool?

4. How will tool runout and hole drift be controlled?

5. How will chips be removed from the full depth?

6. How will internal cross-hole burrs be removed and verified?

7. Can the requested diameter, position and straightness all be measured?

8. What happens if a drill breaks during production?

9. How is coolant filtration maintained for the tool passages?

10. Would a diameter, depth or entry-surface change reduce risk or cost?

Frequently Asked Questions

What depth is considered a deep hole in CNC machining?

There is no universal threshold. Many general machining discussions begin treating holes beyond about 3×D as deep enough to require closer chip-evacuation control. Specialized deep-hole tools and processes cover much higher ratios. Material, diameter, tolerance and coolant capability matter as much as ratio.

What does 10×D drilling mean?

It means the drilling depth is ten times the hole diameter. A 6 mm diameter hole drilled 60 mm deep is a 10×D hole.

Is peck drilling always required for a deep hole?

No. Pecking helps some tools and materials break or clear chips, but modern through-coolant carbide drills may be designed for continuous drilling. Excessive pecking can increase cycle time and tool wear. Follow the specific toolmaker's instructions.

Why is a pilot hole used before a long drill?

The pilot supports and aligns the long drill during entry. It reduces the risk of wandering or unstable engagement. Its diameter, depth and geometry must match the deep-hole tool.

Can a standard extra-long drill make a precision deep hole?

Sometimes, but length alone does not make a drill suitable. Precision deep-hole tools may use special points, margins, polished flutes, coatings and internal coolant. The holder, machine and entry procedure are equally important.

How straight can a CNC deep hole be?

Achievable straightness depends on L/D ratio, diameter, material, process, entry condition, tooling, machine alignment and measurement method. A supplier should review the actual drawing rather than promise one universal value.

What is the difference between hole position and straightness?

Position controls where the hole axis is located relative to datums. Straightness controls how much the axis or surface may deviate from a straight line. A hole can meet entry position but curve internally, so critical drawings may need both requirements.

How are internal cross-hole burrs removed?

Options include special brushes, cutting tools, abrasive flow, thermal deburring and electrochemical processes. Access, material, edge requirement and cleanliness determine the method. Borescope or cleanliness testing may be used for verification.

Does higher coolant pressure always improve deep drilling?

No. Pressure helps delivery, but chip transport also needs adequate flow. Passage size, filtration, coolant condition, tool geometry and chip shape all matter. Excess pressure cannot repair a blocked tool or unsuitable process.

Why did a deep-hole drill break?

Common causes include chip packing, coolant loss, excessive runout, worn edges, incorrect feed, poor pilot alignment, unstable entry and material variation. The broken tool is the result; the process should be investigated before drilling the next part.

How should a blind-hole depth be specified?

State whether the dimension is full-diameter depth or total depth to the drill point. Also identify thread depth, bottom shape and required clearance. This prevents the supplier from interpreting a conical drill bottom as usable cylindrical depth.

Can a deep hole be drilled from both ends?

Yes, if the part permits two-sided access. However, the two axes may not meet perfectly. The drawing should define allowable mismatch, step, burr and flow restriction at the intersection.

How are very small deep holes inspected?

Methods may include pin gauges, air gauges, borescopes, optical systems, flow testing or specialized probes. Some characteristics may require process qualification or destructive validation because normal instruments cannot reach the full depth.

What information most improves a deep-hole quotation?

The exact material, hole diameter, full-diameter depth, entry and exit conditions, cross-hole geometry, tolerance, straightness, finish, burr, cleanliness, test requirements and quantity are the most useful inputs.

Final Takeaway

CNC deep hole drilling is a complete process, not merely a longer drilling cycle. Reliable results depend on selecting the correct method for the depth-to-diameter ratio, guiding the tool at entry, controlling runout, delivering filtered coolant to the cutting zone, forming manageable chips and verifying the internal feature with an appropriate inspection plan.

Designers can reduce risk by using standard diameters, practical depths, stable entry surfaces, clear bottom definitions and realistic tolerances. Cross holes, angled exits, inaccessible burrs and cleanliness requirements should be discussed before the design is released.

For a deep-hole component, send your 3D model, drawing, material, quantity and critical bore requirements through the AluPrototype request-a-quote page. Our engineering team can review drilling method, tool access, chip evacuation, inspection and DFM options before machining begins.