# Blind holes

Non-through holes: usable bore and thread depth, drill-point geometry, remaining wall, chip evacuation and inspection requirements.

Reviewed: 2026-11-01

Tags: parts-and-design, holes, drilling, machining

## Define the functional depth

Specify the usable full-diameter depth separately from the deepest drill-point position. A blind hole stops within the part.

In the ideal 10.0 mm drill example, the conical point extends **3.004 mm** at 118° or **2.071 mm** at 135° beyond the full-diameter cylinder. Add the applicable point length when checking the deepest material removal and remaining bottom wall. Confirm the actual tool and bottom geometry.

Protolabs' threaded-hole guidance explicitly discusses points modelled at blind-hole bottoms: they may represent a drilled pilot point, serve a design function or provide space for threading chips. That distinguishes a bottom feature from usable thread or full-diameter bore. The source describes Protolabs' service, not a universal drawing convention. [Protolabs threaded-hole guidance](https://www.protolabs.com/en-gb/services/cnc-machining/threaded-holes-guidelines/)

State what the hole must do: locate a pin, provide a fluid pocket, receive a fastener or support another feature. The required inspection and bottom geometry follow from that function. A fastener that enters a hole is not proof that the specified thread engagement or seating condition has been achieved.

## Dimensions and acceptance fields

| Field | Meaning to preserve |
| --- | --- |
| Diameter and tolerance | Required bore size, with any finishing operation identified |
| Reference face and axis | Datum for depth, position and orientation |
| Full-diameter depth | Usable cylindrical length before the bottom transition |
| Bottom shape and total depth | Conical point, flat floor or another required profile |
| Thread requirement | Designation/class and minimum complete usable thread depth |
| Remaining material | Required ligament to the opposite face or nearby feature |

Mark whether a depth refers to the cylindrical portion or the deepest point. Resolve that explicitly between the drawing, model, quotation and manufacturing plan rather than expecting a supplier to infer the function. A flat-bottom requirement is a separate geometric requirement; it should not be assumed from a blind-hole label.

For stepped or intersecting holes, specify each depth from an unambiguous datum and review the remaining wall at the actual nearest feature. The outside part thickness alone may not identify the limiting ligament.

## Original drill-point calculation

Assume an ideal conical drill point with hole diameter **D**, included point angle **θ** and axial point length **h**. Elementary geometry gives

`h = (D / 2) / tan(θ / 2)`.

For an **assumed 10.0 mm diameter**:

| Assumed included angle | Ideal point length |
| --- | ---: |
| 118° | 3.004 mm |
| 135° | 2.071 mm |

These are original geometric examples, not a statement that either angle is required or supplied for every hole. Actual tool geometry and generated bottom profile must be confirmed.

If **20.0 mm full-diameter depth** is required, the ideal deepest point is approximately **23.004 mm** or **22.071 mm** from the same entry face. In an assumed 25.0 mm thick block, the corresponding ideal residual thickness is **1.996 mm** or **2.929 mm**. A 20 mm command interpreted as tool-tip depth would not provide the same 20 mm cylindrical bore.

This calculation excludes diameter/depth tolerances, tool-point details, face variation, runout and nearby features. It is not proof of an acceptable minimum wall, pressure resistance or machining instruction. Use worst-case accepted geometry when a minimum remaining ligament matters.

## Thread depth is not drill depth

Separate complete usable thread, incomplete thread/runout, tool lead and bottom clearance. The required pilot geometry and travel depend on the actual thread-making method and tool. A bottoming designation does not remove the need to check the tool's generated profile and available clearance.

Protolabs says its cited service CNC-cuts threads with a thread mill and shows thread depth on the quotation. Its stated service depth guidance is therefore evidence about that process offering, not a universal tapping limit. Confirm how the quoted feature satisfies the drawing instead of equating modelled hole depth with complete thread depth. [Protolabs process and quotation basis](https://www.protolabs.com/en-gb/services/cnc-machining/threaded-holes-guidelines/)

For an assembly, establish fastener penetration, washers/stack thickness, entry chamfer and required engagement together. Check that the fastener can clamp the intended stack without contacting the hole bottom first. Thread fit, engagement and bottom clearance answer different questions.

## Chip evacuation and process planning

Sandvik Coromant identifies coolant supply as affecting chip evacuation, thread quality and tool life in tapping, with internal supply preferred particularly for long-chipping materials and deeper holes. These are toolmaker recommendations to apply to the selected tool/material system, not a generic coolant setting or assurance that a blind hole will clear itself. [Sandvik Coromant tapping operation tips](https://www.sandvik.coromant.com/en-gb/knowledge/threading/tapping/operation-tips)

Plan how chips and cutting fluid leave the feature and how the hole is cleaned afterward. Retained chips can interfere with subsequent gauging, seating or assembly. Define cleanliness acceptance where the component's function requires it, including access for cleaning and inspection.

Haas' **G83 normal peck-drilling** documentation separately defines Z hole-bottom position, incremental peck depth and the R plane, and describes how control settings affect chip-clearing motion. It demonstrates why a process cycle has more inputs than final depth alone. These are Haas-control mechanics, not portable settings for another machine or a requirement that every blind hole be peck drilled. [Haas G83 documentation](https://legacy-aem.haascnc.com/content/haascnc/en/service/codes-settings.type=gcode.machine=mill.value=G83.html)

Select drilling, boring, reaming, milling and threading operations against the actual tolerance, material, access and bottom requirement. Verify tool reach and collision clearance separately from cutting length. This reference establishes no universal depth-to-diameter limit, speed, feed or peck increment.

## Inspection and release

Identify the measurement method for each functional requirement. A depth measurement contacting the point is different from evidence of full-diameter bore depth; a thread gauge does not by itself certify the surrounding wall or bottom clearance. Agree how inaccessible features are accepted before manufacture.

Inspect and record diameter, relevant depth definitions, location/orientation, bottom profile where required, complete thread depth and cleanliness against the drawing. Preserve which revision and datum were used. Any pressure, fatigue, sealing or fastener-strength requirement needs its own design and qualification basis beyond the hole geometry.

## Source scope

The cited Protolabs, Sandvik Coromant and Haas pages are live references without separately verified technical revision dates. Their manufacturing guidance is bounded to the described service, tooling or control. Original calculations above use explicitly assumed geometry; they are not supplier capability claims.