M5 tap drill: 4.2 mm, and what the number alone does not tell you
The short answer: 4.2 mm
The metric coarse thread M5 has a pitch of 0.8 mm. The tap drill for a cut thread is 4.2 mm according to DIN 336 and ISO 2306. That is exactly the workshop rule of nominal diameter minus pitch: 5 mm − 0.8 mm = 4.2 mm. Unlike M8 or M12, the rule works here without any rounding.
| Quantity | Value | Source |
|---|---|---|
| Pitch P | 0.8 mm | DIN 13-1, coarse thread |
| Tap drill, cut thread | 4.2 mm | DIN 336 |
| Tap drill, formed thread | 4.55 … 4.6 mm | d − 0.55 · P, check the tool maker’s data |
| Minor diameter of nut D₁ (min) | 4.134 mm | ISO 965-1 |
| Minor diameter of nut D₁ (max, 6H) | 4.334 mm | ISO 965-1 |
| Clearance hole, medium | 5.5 mm | ISO 273 |
| 90° countersink | about 5.8 mm | rule of thumb d + P |
All M5 dimensions including stress area and engagement lengths are on the M5 thread page (in German).
If the number was all you needed, you can stop here. If you have ever snapped an M5 tap in a blind hole, keep reading, because the cause is almost never the diameter itself.
Why 4.2 and not 4.0 or 4.3
An internal thread 6H allows a minor diameter between 4.134 and 4.334 mm. Whatever the drill leaves inside that band is within the standard. A twist drill usually cuts a few hundredths oversize, so a 4.2 mm drill typically ends up at 4.22 to 4.25 mm, close to the middle of the band.
| Drill | Thread engagement (calculated) | Hole inside 6H band? |
|---|---|---|
| 4.0 mm | about 96 % | no, too small |
| 4.1 mm | about 87 % | just below the middle |
| 4.2 mm | about 77 % | yes, centred |
| 4.3 mm | about 67 % | yes, at the upper edge |
| 4.5 mm | about 48 % | no, too large |
Engagement as (d − drill) / (1.299 · P), relative to the full theoretical profile height. Drills that cut oversize shift every row down a little.
The 4.0 mm drill is the classic mistake. It looks like a round number and is lying around in plenty of drill boxes. The tap then has to remove material that does not belong to the thread, the torque rises sharply, and in a blind hole packed with chips that is quickly enough to break an M5 tap. A broken tap in a finished part costs more than any box of drills.
The other direction is less harmful than people think. More engagement adds very little strength, because the outer flank regions carry little of the load. In a properly designed bolted joint the bolt fails first. A 4.3 mm drill is therefore a deliberate choice in tough materials, not a bodge. At 4.5 mm you are outside the standard, though, and the thread strips the first time someone uses a torque wrench.
How deep the hole has to be in a blind hole
A tap does not cut the full profile from its very tip. At the front sits the chamfer, two to three threads long on blind-hole taps (form C). Those threads do not produce a load-bearing thread. On top of that comes the point of the twist drill, which at a 118° point angle is about 0.3 · d long. For a blind hole the calculation goes like this:
Drill depth (full diameter) ≈ usable thread depth + chamfer + clearance
Chamfer form C: 2.5 threads × 0.8 mm ≈ 2.0 mm
Clearance: ≈ 1.0 mm
Drill point 118°: 0.3 × 4.2 mm ≈ 1.3 mm (added below)
Example aluminium, 11 mm thread engagement:
11 + 2.0 + 1.0 = 14 mm full diameter, about 15.3 mm to the tip
The 11 mm in the example is not arbitrary. For a property class 8.8 bolt in aluminium you allow roughly 2.2 · d, in low-strength steel about the nominal diameter, so 5 mm, in cast iron around 7.5 mm. Make the engagement too short in a soft material and the thread strips, however clean the hole is. The values per material are also on the page for the M5 8.8 tightening torque (in German).
Thread forming, fine thread and thread inserts
The 4.2 mm only applies to a cut coarse thread. As soon as the process or the pitch changes, so does the hole, and not by a few hundredths.
| Version | Tap drill | Note |
|---|---|---|
| M5, cut | 4.2 mm | standard value to DIN 336 |
| M5, formed | 4.55 … 4.6 mm | displaces instead of cutting, the forming tap’s own chart applies |
| M5 x 0.5, cut | 4.5 mm | fine thread, d − P |
| Wire thread insert M5 | 5.2 mm | with the matching insert tap, maker’s data |
M5 x 0.5 has its own page: M5 x 0.5 thread (in German).
With thread forming the wrong drill is the most expensive mistake. A forming tap in a 4.2 mm hole has to displace far too much material and breaks easily. Formed threads pay off in ductile materials such as wrought aluminium alloys or structural steel, because no chips are produced and the grain flow is kept. In grey cast iron or brittle brass they do not work.
Material and workshop practice
The diameter stays the same, but the material decides how comfortably the tap works. A few values that keep turning up in tool makers’ charts:
- Aluminium: 4.2 mm, spiral-flute tap for blind holes, plenty of lubricant. If the material smears, a better tool grade helps more than a larger hole.
- Stainless steel (e.g. 1.4301): work-hardens. A 4.25 or 4.3 mm drill lowers the cutting torque noticeably and stays within the 6H band.
- Grey cast iron: 4.2 mm, dry or with air, straight-flute tap. The short chips rarely cause trouble here.
- Structural steel S235: 4.2 mm, the easy case.
As an order of magnitude for HSS in structural steel: drill at about 25 m/min, which at 4.2 mm is roughly 1900 rpm, and tap much slower at about 10 m/min, a little over 600 rpm. The feed when tapping is the pitch, 0.8 mm per revolution, and nothing else. Without synchronised spindle control you need a floating tap holder. Exact values for tool and material come from the cutting data calculator. And lightly countersink the hole first, otherwise the first thread throws up a burr that spoils the seating of the bolt.
Where it goes wrong in practice
Most problems with M5 threads are not diameter problems. When a thread strips or a tap breaks, check these points, roughly in this order:
- Blind hole drilled too shallow, the tap bottoms out or runs into its own chips.
- 4.0 mm drill grabbed from the wrong box instead of 4.2.
- Forming tap in a hole sized for a cut thread.
- Engagement in aluminium designed by the steel rule, 5 mm instead of about 11 mm.
- Bolt tightened by feel. For M5 8.8 that is only about 6 Nm, or 60 N of hand force on a 100 mm spanner. How much friction matters there is covered in the article on tightening torque and preload.
Frequently asked questions
What drill size do I use for an M5 thread?
For a cut coarse thread M5 x 0.8 a 4.2 mm twist drill to DIN 336. For a formed thread 4.55 to 4.6 mm according to the tool maker, and for the fine thread M5 x 0.5 a 4.5 mm drill.
Can I pre-drill M5 with 4 mm?
Better not. 4.0 mm is below the smallest permitted minor diameter of 4.134 mm. The tap then has to remove extra material, the cutting torque rises sharply, and especially in blind holes an M5 tap breaks easily.
How deep do I drill for an M5 blind hole?
Usable thread depth plus about 2 mm for the tap chamfer plus roughly 1 mm clearance, measured to the end of the full-diameter section. The drill point adds about 1.3 mm. For 11 mm of thread in aluminium that is about 14 mm of full-diameter depth.
What clearance hole does an M5 bolt need?
ISO 273 gives 5.3 mm for the fine series, 5.5 mm for the medium series and 5.8 mm for the coarse series. The medium series is the usual default for parts without special positional requirements.