What Is a Hole Tolerance? (In Short)
On a technical drawing, a hole dimension rarely says just "Ø15"; next to it you'll find a code like H7 or H10. That code tells you how much bigger or smaller the hole is allowed to be. No machine can drill a hole at exactly 15.000 mm — there is always a small deviation. The tolerance is the accepted limit of that deviation.
The number (IT grade) in the code tells you the width of the tolerance: the smaller the number, the tighter the tolerance and the more precise the job. The letter tells you where the tolerance sits relative to the nominal size. For holes, the most common letter is H: with an H tolerance the hole can never be smaller than the target size — only larger, by up to the tolerance.
Example: Ø15 H10 → tolerance width 0.07 mm. The hole must be between 15.000 and 15.070 mm. If you measure 14.995 mm the hole is undersized (scrap or rework); at 15.080 the hole is oversized.
🔧 Hole Tolerance Calculator
Enter the hole diameter and the tolerance grade from the drawing; see the smallest and largest acceptable size for the hole.
—
📋 IT Tolerance Table (Holes 3–250 mm)
Values are in mm and show the width of the tolerance. When you use the calculator, the matching cell is highlighted in the table.
| Grade | 3–6 | 6–10 | 10–18 | 18–30 | 30–50 | 50–80 | 80–120 | 120–180 | 180–250 | Typical use |
|---|---|---|---|---|---|---|---|---|---|---|
| IT5 | 0.005 | 0.006 | 0.008 | 0.009 | 0.011 | 0.013 | 0.015 | 0.018 | 0.020 | Bearing seats, precision fits |
| IT6 | 0.008 | 0.009 | 0.011 | 0.013 | 0.016 | 0.019 | 0.022 | 0.025 | 0.029 | |
| IT7 | 0.012 | 0.015 | 0.018 | 0.021 | 0.025 | 0.030 | 0.035 | 0.040 | 0.046 | |
| IT8 | 0.018 | 0.022 | 0.027 | 0.033 | 0.039 | 0.046 | 0.054 | 0.063 | 0.072 | |
| IT9 | 0.030 | 0.036 | 0.043 | 0.052 | 0.062 | 0.074 | 0.087 | 0.100 | 0.115 | Holes for forming (fluteless) taps |
| IT10 | 0.048 | 0.058 | 0.070 | 0.084 | 0.100 | 0.120 | 0.140 | 0.160 | 0.185 | |
| IT11 | 0.075 | 0.090 | 0.110 | 0.130 | 0.160 | 0.190 | 0.220 | 0.250 | 0.290 | Standard tapping holes, standard drilled holes |
| IT12 | 0.120 | 0.150 | 0.180 | 0.210 | 0.250 | 0.300 | 0.350 | 0.400 | 0.460 | |
| IT13 | 0.180 | 0.220 | 0.270 | 0.330 | 0.390 | 0.460 | 0.540 | 0.630 | 0.720 |
Two rules to remember: the smaller the IT number, the more precise the job, and within the same IT grade the tolerance grows with hole size (Ø10 H7 has a tolerance of 0.015 mm, while Ø100 H7 has 0.035 mm).
How to Read Codes Like H7 and H10
This page works out the tolerance of a single hole. If the shaft going into it also carries a tolerance, the ISO 286 Hole and Shaft Fit Calculator tells you how much clearance or interference is left between the two.
Letter = position of the tolerance. Capital letters are used for holes. H is the most common and means "from zero upward": the lower limit of the hole is exactly the nominal size, the upper limit is nominal + tolerance width.
Number = width of the tolerance (IT grade). Read it from the table above.
Ø20 H7 example: From the table, the 18–30 mm column + IT7 → 0.021 mm. Because it is H: smallest 20.000 – largest 20.021 mm.
Letters other than H (F, G, JS, K, P...) shift the tolerance to different positions around the nominal and are mostly used for special fit situations (tight fits, press fits). In everyday shop work you will almost always see H on holes; if you see a different letter, check with whoever prepared the drawing or consult full tolerance tables.
Which process produces which hole?
A hole made with a standard drill is usually around IT12–IT13. IT9–IT10 takes a drill in good condition and careful parameters. IT7–IT8 cannot be held by drilling alone — the hole must be reamed or finish-bored afterwards. IT5–IT6 is grinding/honing territory.
Frequently Asked Questions
My hole is out of tolerance — what now?
If the hole is undersized, you're in luck: it can be brought to size by reaming, boring or re-machining. If the hole is oversized, material cannot be added back — in most cases the part is scrap. That's why the basic rule for precise holes is to approach the size from below.
Why does the tolerance of a tapping hole matter?
If the tap hole is too narrow, the tap strains and can break; if it's too wide, the thread engagement is loose and the bolt sits slack. IT11–IT13 is fine for standard taps; forming (fluteless) taps need a more precise hole (IT9–IT10). To calculate the drill size, use our Tapping Techniques and Tap Drill Size Calculator.
How do I know I'm within tolerance?
By measuring. For IT11 and above, calipers are usually enough; for IT7–IT10 use a three-point bore micrometer or a go/no-go plug gauge; IT5–IT6 requires precision measuring equipment. Remember that a caliper's own accuracy is around 0.02–0.03 mm — you cannot check a 0.021 mm tolerance with a caliper.