Carbide Drill Diameter Tolerance: How to Choose m7, h7 or h8

The drill catalogue lists the same diameter in two or three versions, one marked m7, one h7, sometimes one h8, and the drawing only says the hole must be H7 or H8. Someone has to pick the drill class before the RFQ goes out, and a wrong guess shows up later as oversize holes, a long drill that rubs in its own pilot, or a reamer left with the wrong amount of stock.

Choose a carbide drill’s diameter tolerance, m7, h7 or h8, from the hole class on the drawing and from what the hole becomes next: a finished hole, a pilot or a pre-hole.

If a new drill already cuts oversize, start with oversized holes from a new carbide drill; the full field list is in the solid carbide drill RFQ checklist, and holder and stickout effects are in carbide drill stickout, runout and toolholders.

What m7, h7 and h8 mean on a drill

ISO 286-1 defines the code system, and ISO 286-2 tabulates the limit deviations for each class. A tolerance class is a letter plus a number, and each part does a different job.

The letter sets the position

The letter is the fundamental deviation: where the tolerance zone sits relative to the nominal size. For external features, which ISO 286 calls shafts, the letter h puts the upper limit exactly at nominal, so the whole zone is at or below nominal. The letter m puts the lower limit above nominal, so the whole zone is oversize. A drill body is an external feature, so its diameter is given a lowercase shaft class.

The number sets the width

The number is the standard tolerance grade, IT7 or IT8. A higher number means a wider band. At a given nominal size, h7 and m7 are exactly the same width, because both are IT7; they only sit in different places. An h8 drill is allowed a wider spread than either.

Lowercase is the drill, uppercase is the hole

Uppercase letters are hole classes. H7 and H8 put the lower limit of the hole at nominal and the zone above it. The drawing tells you the hole class; the drill class is a separate decision about the tool, and the two are easy to confuse on a quick read of a catalogue or an RFQ.

ISO 286 limits for m7, h7 and h8 drills

The table lists the upper and lower limit deviations from ISO 286-2 for the size ranges most solid carbide drills fall into, with the H7 and H8 hole classes alongside for comparison. Values are in micrometres (µm), where one micrometre is one thousandth of a millimetre. Each range is “over” the lower size and up to and including the upper size.

Source: ISO 286-2, limit deviations for shafts (h, m) and holes (H). The figures above were cross-checked against published reproductions of the ISO 286-2 tables. For sizes outside these ranges, or for a formal contract, read the values from the current edition of the standard itself.

A worked example: a 12 mm drill in m7 may measure from 12.007 to 12.025 mm; the same drill in h7 from 11.982 to 12.000 mm; in h8 from 11.973 to 12.000 mm. An H7 hole at 12 mm is 12.000 to 12.018 mm.

How each class sits against an H7 or H8 hole

Putting the drill band next to the hole band shows what each class asks of the process.

• m7 drill. The whole band is above nominal, and in every range in the table its upper limit falls between the H7 and H8 upper limits. An m7 drill starts inside an H8 hole zone. Against H7, a drill near the top of its m7 band is already larger than the hole allows before any cutting effect is added, so m7 alone does not promise an H7 hole.
• h7 or h8 drill. The whole band is at or below nominal, so the drill itself sits outside, and just under, an H-class hole zone. The hole reaches H7 or H8 only if the process opens it slightly relative to the drill, or it is left undersize for a following operation (see sizing the reamer band for an H7 hole).
• h8 compared with h7. Same position, wider spread. Two h8 drills of the same nominal size can differ more from each other than two h7 drills, which matters when several spindles or several stations must drill the same hole.

This is why the drill class should be chosen from the hole class and the route, not from habit or catalogue default.

Which drill tolerance class to choose

Choose m7 when the hole should land on the plus side

Use m7 when the drilled hole is itself the finished H-class hole with a generous enough band, commonly H8 or wider, and the process is stable enough to add little on top of the drill size. It is also the usual choice for a pilot drill, because the pilot hole should come out slightly larger than the drill that follows it. Catalogue solid carbide drills made to DIN 6537 are commonly listed with an m7 cutting diameter and an h6 shank (DIN 6535 HB), so an h7 or h8 drill is usually something to ask for rather than assume.

Choose h7 when the hole must not grow

Use h7 when the drawing or the next operation penalises oversize more than undersize: a hole that will be tapped or reamed with a set allowance, a hole whose upper limit is close to nominal, or a long drill that must pass through an m7 pilot hole without contacting its walls.

Choose h8 when the band can be wider

Use h8 for holes with open tolerances, clearance holes and general drilling where the drill class is not the limiting factor. It is common on general-purpose drills. Do not expect an h8 drill to hold a hole that needs an IT7 spread, since the drill’s own variation is already wider than IT7.

When the drill makes a pre-hole for a reamer

Drill makers’ technical guides generally put the best drilled hole at about H8 under favourable conditions, so an H7 callout normally needs a finishing step after the drill. For a pre-hole, the nominal drill diameter is set from the reaming allowance and the reamer type, and the class then keeps that allowance consistent from drill to drill. Pick the class that keeps the pre-hole inside the allowance window after the process adds its own oversize; the PCD reamer allowance and pre-hole size guide explains how the window is set.

Why the hole still misses when the drill is in tolerance

A drill measured inside m7, h7 or h8 only proves the tool. The hole adds its own effects, and the direction depends on the setup and the material:

• Runout at the cutting point from the holder, collet or spindle usually opens the hole beyond the drill diameter. See stickout, runout and toolholders.
• Point symmetry and entry. An unequal lip or a sloped entry surface can make the drill cut to one side. Pilot hole and entry control covers this.
• Material behaviour. Some materials spring back or shrink after cutting and can leave the hole close to, or below, the drill size; others let the margins burnish or smear the wall.
• Heat and coolant. Temperature at the cut and at measurement changes both part and tool size.
• Back taper and regrinding. Drills are normally ground with a slight back taper, so diameter is specified at the point. Each regrind shortens the drill and can move the new point diameter toward the low end of its class or below it, depending on the taper and the amount removed. Check the diameter after regrinding, not only on new tools.

If the hole moves while the drill is in class, work through the oversize-hole diagnosis before changing the class.

How to state drill tolerance on an RFQ

A diameter with no class, or a standard number with no class, leaves the maker to guess. State the following in the RFQ or on the tool drawing:

• nominal diameter and the class, written together, for example “Ø12 m7”, and the point or length at which the diameter is measured;
• the hole class and limits from the part drawing, and whether the drill makes the finished hole, a pilot hole or a pre-hole;
• for pre-holes, the next operation and its allowance; for pilots, the class of the drill that follows;
• material, depth, holder and coolant method, because these decide how far the hole departs from the drill;
• how the drill diameter will be inspected and reported, and whether reground drills must return to the same class.

If the hole class is tighter than any drill class can carry through your process, say so. The answer may be a different route, such as drill and ream, rather than a tighter drill; see choosing a hole machining route.

Frequently Asked Questions

What is the difference between m7 and h7 on a drill?

Both are IT7, so they have the same band width. An h7 drill sits at or below nominal diameter; an m7 drill sits entirely above nominal. The values for each size range are given in ISO 286-2.

Will an h7 drill make an H7 hole?

Not by itself. The drill class describes the tool, while the hole depends on runout, point symmetry, material, heat and wear. An h7 drill is below the H7 hole zone, so the hole reaches H7 only if the process opens it slightly and consistently.

Why are pilot drills often m7?

A pilot hole should be slightly larger than the drill that follows, so the longer drill can enter without rubbing on the pilot wall. An m7 pilot with an h7 follow-on drill keeps the pilot on the plus side and the long drill on the minus side of nominal.

Is h8 good enough for a carbide drill?

For open-tolerance and clearance holes, usually yes. For holes that need an IT7 spread, or several spindles drilling the same hole, h8 allows more variation between drills than h7 or m7, so specify the tighter class.

Next step

Read the hole class from the part drawing, decide whether the drill makes the finished hole, a pilot or a pre-hole, and then choose m7, h7 or h8 and write it next to the diameter on the RFQ.

Related reading
- Field list: Solid carbide drill RFQ checklist
- Pilot drilling: When to pilot drill before a carbide drill
- Geometry: Solid carbide drill geometry
- Special tools: Replacing a special cutting tool from a sample

Product
- Solid carbide drill · Combination drill-reamer · Drawing-based custom cutting tools. Discuss Your Tooling Requirements

Send Your Drawing
Send the part drawing with the hole class, material, depth, holder and coolant details, and whether the hole is finished by the drill, for an XRZ engineering review of the drill diameter and tolerance class. Quick RFQ: Custom cutting tool RFQ.

---