Engineering Drawing and GD&T Basics: Fits, Tolerances and Position
An engineering drawing is a contract between the designer and the manufacturer. It must say not only what shape and size a part has, but how much each feature may vary and still work. Dimensions with plus-minus tolerances control size; geometric dimensioning and tolerancing (GD&T) controls form, orientation and location relative to datums. This article covers the projection system used in India, standard limits and fits, tolerance stack-up, and the core GD&T ideas with numerical examples.
Orthographic Projection
A part is shown in two or more views, typically front, top and side. In first angle projection, the top view is placed below the front view and the left-side view is placed to the right of the front view. In third angle projection, the top view is placed above and the right-side view to the right. Indian standard practice (SP 46) and much of Europe use first angle; the USA uses third angle. The projection symbol, a truncated cone in two views, must appear in the title block so there is no confusion.
| Line type | Use |
|---|---|
| Continuous thick | Visible outlines and edges |
| Continuous thin | Dimension lines, extension lines, hatching |
| Dashed thin | Hidden edges |
| Chain thin (long dash, dot) | Centre lines, axes of symmetry |
| Chain thick at ends and changes | Cutting planes for sections |
Limits and Fits
In the ISO system a hole is written with a capital letter and a shaft with a small letter, followed by an IT grade number. The letter sets the position of the tolerance zone relative to the basic size and the number sets its width. In the hole-basis system the hole is H (lower deviation zero) and the shaft letter is chosen to get the desired fit.
Basic size 25 mm (size range over 18 up to 30 mm) H7 hole: +0.021 / 0 -> 25.000 to 25.021 g6 shaft: -0.007 / -0.020 -> 24.980 to 24.993 p6 shaft: +0.035 / +0.022 -> 25.022 to 25.035 25 H7/g6: Maximum clearance = 25.021 - 24.980 = 0.041 mm Minimum clearance = 25.000 - 24.993 = 0.007 mm (sliding fit) 25 H7/p6: Maximum interference = 25.035 - 25.000 = 0.035 mm Minimum interference = 25.022 - 25.021 = 0.001 mm (light press fit)
| Fit | Type | Typical application |
|---|---|---|
| H7/g6 | Close running clearance | Sliding gears, precise guides, spigots |
| H7/h6 | Locational clearance | Parts that must locate accurately but assemble freely |
| H7/k6 | Transition | Gears and pulleys on shafts with keys |
| H7/p6 | Light interference | Bushes pressed into housings |
Tolerance Stack-Up
When several toleranced dimensions add up to an overall dimension, their variations accumulate. Three spacers 20 plus-minus 0.1, 30 plus-minus 0.1 and 15 plus-minus 0.05 mm are stacked on a shaft.
Nominal total = 20 + 30 + 15 = 65 mm
Worst case: +/- (0.1 + 0.1 + 0.05) = +/- 0.25 mm
Statistical (root sum square):
+/- sqrt(0.1^2 + 0.1^2 + 0.05^2) = +/- 0.15 mmWorst case guarantees every assembly fits but forces tight, costly part tolerances. Root sum square assumes variations are random and independent, so extremes rarely combine; it is used in high-volume production where a very small reject rate is acceptable.
GD&T: Symbols, Datums and the Feature Control Frame
GD&T uses a feature control frame: a box containing the geometric symbol, the tolerance value (with a diameter sign if the zone is cylindrical), any material condition modifier, and the datum references in order of priority. Datums A, B and C are real features on the part, such as a flat base and two edges, that set up the reference frame for measurement.
| Category | Characteristics | Datum needed |
|---|---|---|
| Form | Flatness, straightness, circularity, cylindricity | No |
| Orientation | Perpendicularity, parallelism, angularity | Yes |
| Location | Position, concentricity, symmetry | Yes |
| Runout | Circular runout, total runout | Yes |
| Profile | Profile of a line, profile of a surface | Optional |
The ASME Y14.5 standard (2018 edition) removed concentricity and symmetry, recommending position, runout or profile instead; ISO GPS standards still include them. Check which standard your drawing follows.
Worked Example: Position Tolerance with MMC Bonus
A hole is dimensioned diameter 10.0 to 10.2 mm, with a position tolerance of diameter 0.2 at maximum material condition (MMC) relative to datums A, B and C. For a hole, MMC is the smallest size, 10.0 mm.
Measured hole centre is off by 0.06 mm in X and 0.08 mm in Y. Actual position error (diametral) = 2 * sqrt(0.06^2 + 0.08^2) = 2 * 0.10 = 0.20 mm If the hole measures 10.0 (at MMC): allowed = 0.2 -> 0.20 OK, just on the limit If the hole measures 10.15: allowed = 0.2 + 0.15 = 0.35 -> OK with margin If the hole measures 10.2 (at LMC): allowed = 0.2 + 0.2 = 0.40 Virtual condition = MMC - position tolerance = 10.0 - 0.2 = 9.8 mm
The extra tolerance as the hole grows is the bonus tolerance. It reflects the real function: a larger hole can be further off position and still accept the mating bolt. The virtual condition of 9.8 mm is the worst-case boundary, so a fixed pin of 9.8 mm, or a functional gauge with pins of that size, will always pass a good part.
Common Mistakes
- Mixing first and third angle conventions, which mirrors the views and causes wrong parts.
- Chain dimensioning features that must relate to each other, which stacks tolerances unnecessarily.
- Specifying tight tolerances everywhere instead of only on functional features.
- Listing datums in the wrong order; the primary datum is the one the part rests on first.
- Forgetting that a plus-minus location tolerance creates a square zone, while a diameter position tolerance creates a round zone about 57 percent larger in area.
Summary
Projection standards arrange views, ISO limits and fits define clearance and interference precisely, stack-up analysis tells you how tolerances combine, and GD&T controls form and location relative to datums. With position at MMC, bonus tolerance and virtual condition, drawings can match the real function of a part and allow the widest economical manufacturing tolerance.