Limits, fits and tolerances; GD&T basics

Why it matters

No machine makes two parts exactly the same size, so every drawing must say how much variation is acceptable and how mating parts should behave together: free running, locating, or pressed. Limits and fits make mass-produced parts interchangeable, and GD&T controls form, orientation and position, which size limits alone cannot. Getting this right decides whether a bearing seat, gear bore or dowel pin works on the first assembly or ends up as scrap.

Key ideas

Size terms

• Basic (nominal) size: the size from which limits are set, e.g. Ø50 mm.
• Limits: the maximum and minimum permissible sizes.
• Tolerance: the difference between the upper and lower limits. It is always positive and has no sign.
• Deviation: limit minus basic size. Upper deviation (ES for holes, es for shafts) and lower deviation (EI for holes, ei for shafts). Deviations carry a sign.
• Fundamental deviation: the deviation closest to the zero line. It fixes the position of the tolerance zone and is shown by a letter (capital for holes, small for shafts).
• Allowance: the intentional difference between the maximum material limits of mating parts (minimum hole minus maximum shaft). It is the tightest condition of the fit: positive for clearance, negative for interference.

Fits

• Clearance fit: the smallest hole is larger than or equal to the largest shaft, so there is always clearance (or zero). Example: H7/g6 (location with small running clearance), H8/f7 (running fit).
• Interference fit: the largest hole is smaller than the smallest shaft, so there is always interference. Example: H7/p6, H7/s6 (press fits for bushes and gears).
• Transition fit: the tolerance zones overlap, so an assembled pair may have small clearance or small interference. Example: H7/k6, H7/n6 (location of gears, pulleys and couplings on keyed shafts).

Hole-basis and shaft-basis systems

• Hole-basis: the hole is always an H hole (lower deviation EI = 0, so the minimum hole size equals the basic size). Different fits are obtained by changing the shaft letter. This is the preferred system because holes are made with fixed-size tools (drills, reamers) and checked with fixed plug gauges.
• Shaft-basis: the shaft is always an h shaft (upper deviation es = 0, so the maximum shaft size equals the basic size), and the hole letter changes. Used where one bright-drawn shaft carries several parts with different fits.

ISO / IS 919 system

• A tolerance is written as a letter plus a grade number: in Ø50 H7/g6, H7 is the hole and g6 the shaft.
• There are 20 international tolerance grades IT01, IT0, IT1 … IT18. A smaller number means a tighter tolerance. Roughly: IT01–IT4 for gauges, IT5–IT7 for precision fits, IT8–IT11 for general machining, IT12–IT18 for rough work.
• Tolerance grades IT5 to IT16 are multiples of the standard tolerance unit i, which grows with size because larger parts are harder to hold to the same absolute accuracy.
• The diameter steps in the tables (e.g. 18–30, 30–50, 50–80 mm) are used with the geometric mean of the step as D.
• Fundamental deviations are given by empirical formulas in the standard. Take exact values from the IS 919 / ISO 286 tables in your data book; the formulas reproduce them to within rounding.

GD&T basics

• Size limits control only size. GD&T adds control of geometry through a feature control frame: symbol, tolerance value (with Ø if the zone is cylindrical), material modifier, then datum references in order of precedence (primary, secondary, tertiary).
• Characteristic groups: form (straightness, flatness, circularity, cylindricity, no datum needed); orientation (parallelism, perpendicularity, angularity); location (position, and in older standards concentricity and symmetry); runout (circular and total runout); profile (of a line, of a surface).
• Datums: theoretically exact planes, axes or points simulated by inspection equipment (surface plate, mandrel). The 3-2-1 principle: the primary datum is contacted at three points, the secondary at two, the tertiary at one, removing all six degrees of freedom.
• Basic dimensions (boxed) give the exact true position; the tolerance comes from the frame, not from ± values.
• Material conditions: MMC is the condition with most material (smallest hole, largest shaft); LMC has least material (largest hole, smallest shaft); RFS means the geometric tolerance applies whatever the size.
• Bonus tolerance: when a position tolerance is specified at MMC, the tolerance grows by the amount the feature departs from MMC. This lets functional parts pass and is the basis of fixed functional gauges.
• Virtual condition: the worst-case boundary of size plus geometry. For a hole at MMC it is MMC size minus the geometric tolerance; for a shaft it is MMC size plus the geometric tolerance. Mating parts assemble if the hole's virtual condition is at least the shaft's.
• Envelope principle (Rule #1, ASME): a feature of size at MMC must have perfect form, so form errors must fit inside the size tolerance unless stated otherwise.

Formulas

Tolerance = Upper limit − Lower limit = ES − EI (hole) = es − ei (shaft)

• Limits and deviations in mm or μm. Tolerance is always positive.

Maximum clearance = Hole_max − Shaft_min Minimum clearance (allowance) = Hole_min − Shaft_max

• A negative result means interference. For an interference fit, maximum interference = Shaft_max − Hole_min.
• Clearance fit if Hole_min ≥ Shaft_max; interference fit if Hole_max ≤ Shaft_min; otherwise transition.

i = 0.45·∛D + 0.001·D

• i = standard tolerance unit (μm); D = geometric mean of the diameter step (mm), D = √(D₁·D₂). Applies to sizes up to 500 mm.

IT5 = 7i, IT6 = 10i, IT7 = 16i, IT8 = 25i, IT9 = 40i, IT10 = 64i, IT11 = 100i

• From IT6 onward each grade is about 1.6 times the previous one (the R5 preferred-number series).

Shaft fundamental deviations (upper deviation es, μm, D in mm), as given in IS 919 tables: d: es = −16·D^0.44 e: es = −11·D^0.41 f: es = −5.5·D^0.41 g: es = −2.5·D^0.34 h: es = 0

• For holes in the hole-basis system, H has EI = 0. Other shaft letters (k, n, p, s …) are read from the data book.

Bonus tolerance = |Actual size − MMC size| (for a modifier at MMC) Virtual condition (hole) = MMC size − geometric tolerance at MMC Virtual condition (shaft) = MMC size + geometric tolerance at MMC

Worked examples

Example 1 (standard): classifying a fit. Given: hole Ø50 mm with limits +0.05 / 0.00 mm, shaft Ø50 mm with limits 0.00 / −0.05 mm.

1. Hole limits: Hole_max = 50.05 mm, Hole_min = 50.00 mm. Hole tolerance = 0.05 mm.
2. Shaft limits: Shaft_max = 50.00 mm, Shaft_min = 49.95 mm. Shaft tolerance = 0.05 mm.
3. Maximum clearance = Hole_max − Shaft_min = 50.05 − 49.95 = 0.10 mm.
4. Minimum clearance = Hole_min − Shaft_max = 50.00 − 50.00 = 0.00 mm.
5. Since Hole_min ≥ Shaft_max, there is never interference. This is a clearance fit with maximum clearance 0.10 mm and zero allowance (a sliding fit, not a transition fit).

Example 2 (GATE level): limits of Ø50 H7/g6 from the formulas. Given: Ø50 mm lies in the 30–50 mm step. Use i = 0.45·∛D + 0.001·D, IT7 = 16i, IT6 = 10i, and for g: es = −2.5·D^0.34.

1. D = √(30 × 50) = 38.73 mm.
2. i = 0.45 × 38.73^(1/3) + 0.001 × 38.73 = 0.45 × 3.383 + 0.0387 = 1.561 μm.
3. IT7 = 16 × 1.561 = 24.98 μm ≈ 25 μm. IT6 = 10 × 1.561 = 15.6 μm ≈ 16 μm.
4. Hole H7: EI = 0, ES = +25 μm. Hole limits: 50.000 to 50.025 mm.
5. Shaft g: es = −2.5 × 38.73^0.34 = −8.67 μm ≈ −9 μm. ei = es − IT6 = −9 − 16 = −25 μm. Shaft limits: 49.975 to 49.991 mm.
6. Maximum clearance = 50.025 − 49.975 = 0.050 mm. Minimum clearance = 50.000 − 49.991 = 0.009 mm.
7. Result: hole 50.000/50.025 mm, shaft 49.975/49.991 mm; clearance fit with clearance 9 μm to 50 μm. These agree with the ISO 286 table values.

Example 3 (GD&T bonus tolerance). Given: hole Ø20 +0.10/0 mm with position tolerance Ø0.20 mm at MMC. A produced hole measures Ø20.08 mm.

1. MMC of hole = 20.00 mm (smallest hole).
2. Bonus = 20.08 − 20.00 = 0.08 mm.
3. Allowed position tolerance = 0.20 + 0.08 = Ø0.28 mm.
4. Virtual condition = 20.00 − 0.20 = Ø19.80 mm. Any mating pin whose virtual condition is at most Ø19.80 mm will always assemble, and a fixed Ø19.80 mm functional pin gauge checks size and position together.

Common mistakes

• Calling a fit "transition" when the minimum clearance is exactly zero. Zero allowance with no possible interference is still a clearance fit.
• Mixing the direction of subtraction: maximum clearance uses the largest hole and the smallest shaft; minimum clearance uses the smallest hole and the largest shaft.
• Writing tolerance with a sign, or giving a "range" when the tolerance (a single number) is asked.
• Using the nominal size instead of the geometric mean of the diameter step in the formula for i.
• Forgetting that i is in micrometres while D is in millimetres.
• Swapping MMC and LMC for holes: the MMC of a hole is its smallest size.
• Assuming GD&T bonus tolerance applies when the frame says RFS (no modifier).

For GATE ME

Expect numericals on: limits and clearance or interference from given deviations; deciding the type of fit; computing IT grades and fundamental deviations from the standard tolerance unit formula (always use the geometric mean of the step); and, often in the same question, designing GO/NO-GO gauges for the computed limits (see the gauges topic). Conceptual MCQs test hole-basis versus shaft-basis, MMC/LMC, and which GD&T characteristics need a datum. Practise rounding to whole micrometres the way the tables do.

Quick check

1. A hole is 25.000/25.021 mm and a shaft is 25.022/25.035 mm. What type of fit is this?
2. What is the MMC size of a hole Ø12 +0.018/0 mm?
3. In the hole-basis system, which deviation of the hole is zero?
4. Using i = 0.45·∛D + 0.001·D, roughly how many times larger is IT8 than IT7?
5. Does flatness need a datum reference?

Answers: 1. Interference fit (smallest shaft 25.022 mm exceeds largest hole 25.021 mm). 2. Ø12.000 mm. 3. The lower deviation EI = 0. 4. 25/16 ≈ 1.56 times. 5. No, it is a form tolerance and never references a datum.