CNC Knowledge

Why Are Blind Holes in Machining Essential?

A blind hole stops short of breaking through the far wall. That single geometric choice changes stiffness, sealing, chip control, and tool life. This page is for engineers and buyers who need to know when blind holes in machining are the right call, and how to troubleshoot one that has gone wrong.

Get Instant Quote Talk to an Engineer

Thread depth vs drill depthFlat-bottom vs conicalChip evacuationSealing faces

Blind holes in machining on a 5-axis CNC machined engine part

On this page

1
Blind hole problems: symptom, cause, fix
2
What makes blind holes in machining essential
3
Drill depth, thread depth, and usable depth
4
When a through hole beats blind holes in machining
5
Tooling and cutting data for blind holes
6
How to inspect and verify a blind hole
7
A repeatable sequence for blind holes

Troubleshooting table

Match the symptom you see on the part to the most likely cause before you change the program.

Symptom	Likely cause	What to do
Drill breaks at the bottom	Chip packing in a deep blind hole	Peck drill, retract fully, add through-coolant
Thread feels loose or strips	Thread cut into the drill cone, not full diameter	Add 2-3 thread pitches to drill depth
Hole depth drifts on the floor	Drill point angle left out of the program	Program to the cylindrical depth, not the tip
Bottom is domed, not flat	Standard 118° or 140° drill point	Use a flat-bottom or end mill for the seat
Wall bulges after tapping	Too little material between hole and OD	Keep 1× diameter of wall or move the hole
Coolant weeps past a plug	Seat not flat, or burr left at the cone	Face the seat, deburr, check Ra 1.6-3.2 μm
Tapping torque spikes	Chips left in the hole before the tap	Blow out and inspect; use form taps in ductile stock

Why the geometry matters

A blind hole ends inside the material. There is no exit, so the far wall stays intact. That wall carries load, holds pressure, and keeps chips and fluid from crossing to the other side of the part. On a hydraulic manifold, a through hole would leak. On a mold plate, it would leave a witness mark on the opposite face.

The trade is chip evacuation. A through hole lets chips fall out the bottom. A blind hole traps them. Deep blind holes in aluminum or 316 stainless are where most breakages happen, and the usual culprit is a chip ball at the bottom of the hole rather than a worn tool.

Blind holes in machining also set the datum for depth. A drilled tip has a conical end. If the drawing calls out a depth, ask whether that depth is to the shoulder of the cylinder or to the point. The difference is roughly 0.3 × diameter for a 118° point, which is often more than the tolerance on the depth itself.

1
StrengthThe far wall stays continuous, so bending and hoop stress paths are not cut.
2
SealingA flat seat at the bottom gives a plug or O-ring something to bear against.
3
Depth controlDrill point angle is a real dimension, not a rounding error.

Depth rules

Drill depth, thread depth, and usable depth

Three depths get confused on the same drawing. Drilled depth is the total depth from the surface to the tip. Usable depth is where the hole is at full diameter. Thread depth is how far the tap reaches. A standard tap cannot cut full threads into the drill cone, so thread depth must always be less than usable depth.

A practical rule: drill 2-3 thread pitches deeper than the required thread depth, and keep usable depth at least that deep. In 6061 aluminum, M6 × 1.0 tapped 12 mm deep usually needs a drilled depth near 16 mm. In 17-4PH stainless the same callout may need more, because the material pushes the tap and chips pack harder.

For a flat-bottom blind hole, a standard twist drill will not do. Spot with a stub drill, then step down with a flat-bottom end mill or a 180° spotting tool. Flat-bottom geometry is what makes a hydraulic seat seal. It also removes the cone that a tap cannot cut into.

When not to use one

Chip evacuation is the main reason to go through. If the hole is deeper than about 3 × diameter and the material is gummy, a through hole removes most of the risk. Deep small holes in copper, 304 stainless, or titanium are far easier when chips have somewhere to fall.

Cross-drilled lubrication passages are another case. A through hole lets you push coolant from one end and flush the other. Blind passages trap debris and are hard to clean. If the part is a manifold with intersecting bores, plan the through holes first so chips do not lodge in downstream cavities.

Weight and stiffness matter too. A deep blind hole removes material only where you need it and leaves the rest of the section stiff. A through hole removes a full column of material and can lower the natural frequency of a bracket or housing. Know which one you are trading.

1
Go throughDepth over 3 × diameter, gummy material, or a flushing path.
2
Go blindLeak path must be blocked, or the far face must stay clean.

Tooling and parameters

Peck drilling is the default for blind holes in machining. On a 6 mm carbide drill in 6061-T6, a peck of 0.5-1.0 × diameter with full retraction clears chips. In 316L stainless, drop to 0.3-0.5 × diameter and slow the feed. Through-coolant helps most when the pressure is high enough to push chips back up the flutes.

For flat-bottom seats, a two-tool sequence works well. Spot and drill to within 0.5 mm of final depth, then finish with a flat-bottom end mill at 0.02-0.05 mm per tooth. Leave 0.1 mm for the finish pass on a sealing seat so the surface lands near Ra 1.6-3.2 μm.

Thread milling is worth considering on large or awkward threads. It cuts a full thread form without a tap, and it does not care much about the drill cone. On a 4,000 mm part with a deep M20 thread, thread milling is often the safer route than a long tap.

Quality checks

Check depth before you tap. A depth micrometer or a pin gauge on the shoulder gives you the number that matters. Do not trust the drill tip as a depth reference. On a tight callout, measure the usable depth from the surface to where the hole goes full diameter.

Look at the bottom. A borescope or a quick air blow will show a chip ball or a smeared cone. If a thread feels rough, back the tap out and inspect before you force it. A broken tap in a blind hole is one of the more expensive ways to lose a part.

On sealing seats, check flatness and finish. A seat that is domed will not seal, no matter how much torque the plug gets. For a fluid path, a light dye check or a pressure test on the assembly will reveal a leak that a visual check misses.

Step by step

Use this order on the floor. Each step removes a failure mode before it starts.

1
1. Confirm the depth definitionAsk whether the drawing depth is to the tip or the shoulder. Add 0.3 × diameter for a 118° point if it is to the shoulder.
2
2. Spot the locationUse a stub spot drill at 1,200-2,000 rpm in aluminum. Keep the spot shallow, 0.5-1.0 mm, so the drill does not wander.
3
3. Peck drill with full retractionPeck 0.5-1.0 × diameter in aluminum, 0.3-0.5 × diameter in stainless. Retract fully so chips clear the flutes.
4
4. Leave room for the tapDrill 2-3 thread pitches deeper than the required thread depth. Never tap into the cone.
5
5. Flat-bottom the seat if neededStep down with a flat-bottom end mill. Leave 0.1 mm for the finish pass to reach Ra 1.6-3.2 μm.
6
6. Clean before threadingBlow out and inspect the hole. Any chip left behind will spike tapping torque and can break the tap.
7
7. Tap or thread millUse a form tap in ductile stock. On large deep threads, thread milling avoids the long-tap risk.
8
8. Verify depth and finishMeasure usable depth with a pin gauge. Check the seat with a borescope before the part leaves the machine.

FAQs

Blind holes in machining: common questions

How much deeper should I drill than the thread?

Add 2-3 thread pitches to the required thread depth. For an M6 × 1.0 tapped 12 mm deep, a drilled depth around 16 mm gives the tap room to cut full threads without hitting the cone.

In harder or gummier stock, add a little more. The tap still needs clearance for chips.

Can a blind hole be drilled with a standard 118° drill?

Yes, but the bottom will be conical. If the drawing needs a flat seat for a plug, O-ring, or dowel, follow the drill with a flat-bottom end mill.

A 180° spotting tool also works for shallow seats. The point is that a standard drill leaves a cone a tap cannot fully cut into.

Why does my tap break at the bottom of a blind hole?

Usually a chip ball sits at the bottom and the tap hits it. The torque spikes and the tap snaps.

Blow out the hole before tapping, use a spiral-flute tap, and drill deep enough that the tap is not cutting in the cone.

When should I use a through hole instead?

When depth is more than about 3 × diameter, or the material is gummy, or the hole is a fluid passage that needs flushing.

A through hole removes most chip-evacuation risk. It also removes material that may have been carrying stiffness.

How do I check the depth of a blind hole?

Use a depth micrometer or a pin gauge on the shoulder. Measure to where the hole goes full diameter, not to the drill tip.