Threaded Holes: Depth, Drill Size and How to Call Them Out

The anatomy of a threaded hole

A threaded hole is made in two operations, and confusing them is where most of the trouble starts.

First, a hole is drilled. Its diameter is smaller than the thread’s major diameter — the nominal size you see in the callout. This is the tap drill.

Then the hole is tapped. The tap cuts or forms the thread into the wall of the drilled hole. The material it removes becomes the space between the thread crests.

Three diameters describe the finished thread:

Diameter	What it is
Major diameter	The outside diameter of the thread — the nominal size, such as 6 mm for M6
Pitch diameter	The diameter where the thread flanks are equally thick and the width of the groove matches the width of the ridge; this is what governs the fit
Minor diameter	The diameter at the bottom of the thread grooves — close to the tap drill size

The tap drill is chosen so that the finished thread is about 75% of full thread depth. That figure is a compromise, not a maximum: a 100% thread needs a drill so close to the pitch diameter that the tap has almost no room to cut, which raises the torque and the risk of breaking the tap, and it adds very little to the strength of the joint.

The tap drill is not the thread diameter

This is the first thing that catches people out. An M6 thread does not start from a 6 mm hole.

For metric threads there is a working rule that covers most cases:

Tap drill = major diameter − pitch

Thread	Pitch	Tap drill
M3	0.5	2.5 mm
M4	0.7	3.3 mm
M5	0.8	4.2 mm
M6	1.0	5.0 mm
M8	1.25	6.8 mm
M10	1.5	8.5 mm
M12	1.75	10.2 mm
M16	2.0	14.0 mm
M20	2.5	17.5 mm

For inch threads the same idea applies in a different form: tap drill ≈ major diameter − (1 ÷ threads per inch). A 1/4-20 thread starts from a hole around 0.201 in, which is the #7 drill — again, notably smaller than the 0.250 in nominal size.

Two practical notes on this table.

The chart is more reliable than the rule. Published tap drill charts round to the nearest available drill size and account for the exact thread form. Where a thread is critical, the chart is the reference; the rule is for checking.

In difficult materials the drill is often opened up slightly. Tapping stainless steel, titanium or a hard alloy is much easier with a marginally larger tap drill, which reduces the thread engagement from 75% towards 65% and lowers the torque considerably. The joint loses a little strength and the tap is far less likely to break — usually a good trade, and a decision the shop can make if the thread’s function is known.

The three depths that get confused

This is the second and more expensive confusion, because it happens on drawings rather than in the head.

Term	What it means
Thread depth	How far the usable, full-form thread extends into the hole
Drill depth	How deep the drilled hole goes — always deeper than the thread
Full thread	The portion of the thread at full form, as opposed to the incomplete threads at the tap’s lead

The hole has to be deeper than the thread because a tap cannot cut full thread to the bottom of a hole. The tap has a chamfered lead at its tip — the first few threads of the tap are tapered to help it start — and the threads cut by that lead are incomplete. So the usable thread ends before the hole does.

Different tap types have different lead lengths. A taper tap has a long lead and needs the most clearance at the bottom; a plug tap has a moderate lead; a bottoming tap has a very short lead and can cut closer to the bottom, but is harder to start and is normally used only after a plug tap has opened the hole. That is the subject of the comparison on tap types.

How deep to drill

The rule of thumb that covers most work:

Drill depth ≈ thread depth + half the thread diameter

For an M6 thread required to a depth of 12 mm, that suggests drilling to about 15 mm. The allowance absorbs the tap’s lead and leaves room for chips to clear, which matters in a blind hole where the chips have nowhere to go.

Where the allowance should be increased:

• Hard or galling materials — stainless, titanium, hardened steel — where the tap loads up and the risk of breaking it at the bottom of a hole is high
• A taper tap rather than a plug tap, because the lead is longer
• A blind hole with limited chip clearance, where swarf packs at the bottom and effectively shortens the hole
• A thread that has to run close to a blind bottom, where the functional requirement leaves no room for a generous lead

Where it can be reduced:

• A through hole, where the tap exits and the lead is irrelevant
• A thread that does not need to be full depth, where the drawing can simply state a shallower requirement

The important point for a drawing is that the drill depth is the shop’s decision, not the designer’s. What the design needs is a defined thread depth — the length of usable thread. How much deeper to drill to achieve it depends on the tap, the material and the swarf behaviour, and it is better left to the shop than fixed on the drawing.

How deep does the thread actually need to be?

Here is the part that most drawings get wrong by defaulting to “as deep as possible”.

The load in a threaded joint is not carried evenly along the engaged threads. It is concentrated in the first few, with each successive thread carrying less. The consequence is that a thread engagement of roughly one diameter approaches full strength in steel, and about 1.5 diameters is safely full. Beyond that, adding depth adds very little to the strength of the joint.

What extra depth does add:

• Cycle time — drilling deeper takes longer, and tapping deeper takes longer still
• Tool cost — a longer tap or a longer drill, and more wear per hole
• Risk — the deeper the tap goes, the higher the chance of it breaking, and a broken tap in a part is usually a scrapped part
• Chip management — a deeper blind hole is harder to clear

So a drawing that asks for a thread twice as deep as it needs has bought nothing and paid for it on every part. Where the joint requires more strength, the productive changes are a larger thread, a stronger fastener material or a longer engagement in a weaker parent material — not simply more depth of the same thread.

The material changes the answer

The engagement needed to develop a fastener’s strength depends on the relative strength of the two materials. Where the parent metal is weaker than the bolt, more thread is needed to transfer the same load.

Parent material	Typical engagement for full strength
Steel	Around 1 to 1.5 × the thread diameter
Cast iron	Around 1.5 ×
Aluminium	Around 2 ×
Brass	Around 2 ×
Plastics	2 to 3 ×, or a threaded insert
Very soft or thin materials	Threaded insert rather than a tapped thread

Two consequences follow. First, the same drawing produces different thread depths depending on the material, which is a reason to state the material and let the depth be advised rather than fixed arbitrarily. Second, in plastics and very soft materials a tapped thread is often the wrong answer entirely — the threads strip under load or under repeated assembly, and a threaded insert distributes the load into the parent material properly. The grades we run and how each behaves at the tap are on the materials page, and the inserts themselves are covered under threaded inserts.

Blind holes, through holes and chip clearance

A through hole is the simplest case. The tap exits the far side, so the lead is irrelevant, chip clearance is straightforward, and depth control is not an issue. Where a design can use a through hole, it should — it is easier to make, easier to clean and easier to verify. On a turned part a through hole is usually drilled on the axis in the same cycle, which is covered on the CNC turning page.

A blind hole is where the difficulties live. The chips have to come back out of the hole they were cut in, and in a deep hole with a small diameter they can pack at the bottom, which both shortens the usable thread and raises the torque. The countermeasures are a deeper drill, a spiral-flute tap that lifts chips out rather than pushing them ahead, and frequent withdrawal to clear.

Where a blind hole has to hold a defined thread depth, the drawing statement that helps most is not the depth of the drill but the minimum depth of usable thread, along with a note of how close the hole is allowed to come to a wall or a cavity on the far side. That lets the shop choose an allowance it can actually achieve.

How to call out a thread on a drawing

A complete thread callout carries four things:

Element	Example	What it controls
Thread designation and size	M6 × 1.0	The nominal diameter and pitch
Tolerance class	6H	The fit of the thread
Depth	⤓ 12	How deep the usable thread goes
Through or blind	THRU, or a depth figure	Whether the tap exits the part

Written out, a callout looks like M6 × 1.0 — 6H — ⤓ 12. For inch threads the designation carries the series and the class, as in 1/4-20 UNC — 2B.

Three habits worth adopting:

State the thread depth, not the drill depth. The drill depth is a process decision. Where the design needs a minimum thread, say so, and let the shop provide the allowance.

State the tolerance class. A callout without a class leaves the fit open — and the class is what determines whether a fastener screws in with the right feel, or is loose, or will not start. Classes and designations are set out on the thread standards page.

Say whether the hole is through or blind. Where it is blind, say whether it may break through into a cavity on the far side. That single note can be the difference between a feasible part and one that has to be redesigned, and it is the kind of thing that belongs on the drawing rather than in a conversation after the first article.

The mistakes that cost the most

Giving a thread depth without saying whether the hole is through. On a part with a cavity behind the hole, the difference matters enormously.

Specifying the drill depth instead of the thread depth. The shop then has to work backwards and may not achieve the thread the design needs.

Calling out a thread without its class. The fit is left undefined, and a 6H and a 6G thread are not the same part.

Making threads deeper than the load requires. Extra depth buys no strength beyond about 1.5 diameters in steel, and costs time, tooling and tap-breakage risk on every hole.

Using a tapped thread in a soft material where an insert is needed. The thread strips and the part fails in service rather than in the shop.

Leaving a deep, small-diameter blind hole to the general tolerance. Depth on a blind hole is difficult to measure and difficult to hold, and where it matters it needs to be stated and planned for. The same applies to position: where a tapped hole has to relate to a face or another hole, that relationship is not controlled by the general tolerance block.

What to put on the drawing

Instead of	Write
M6	M6 × 1.0 — 6H — ⤓ 12, THRU or blind
M6, 15 deep	M6 — 6H — ⤓ 12 blind; the drill allowance is the shop’s
Tap drill 5.0	Nothing — the tap drill follows from the thread and the material
Thread as deep as possible	State the required thread depth
Deep blind hole	State the minimum usable thread and whether break-through is allowed
Thread in aluminium or plastic	State the material and the load; engagement or an insert may change

The two lines that prevent most of the rework are the thread depth and whether the hole is through or blind. Everything else about the hole — the tap drill, the drill allowance, the tap type — follows from those two plus the material, and is better decided by the shop than specified on the drawing. Precision features are held to ±0.01 mm with ISO 2768-m as the general block, and drawing conventions we can read are on the drawing requirements page. Send the drawing with the quantity, and the quote comes back within 24 hours with DFM feedback, including a note where a thread depth or a blind-hole requirement is adding cost without adding strength. Orders start at 50 pieces per style and material, samples from a single piece in 5–10 days, and every batch ships with a material certificate (MTR) tracing the grade to its mill heat plus pre-shipment photos.