Understanding Engineering Drawing Tolerances and Their Effect on CAD

One shape in the model, a range on the drawing

Every real part differs a little from every other. A drawing says how much difference is acceptable, feature by feature. A CAD model is a single exact shape. That mismatch is the whole subject of this guide: each tolerance on the drawing is information the model's geometry cannot hold by itself, so somebody has to decide what value to model and where the tolerance goes.

Limit, plus/minus and general tolerances

Limit dimensions

A limit dimension states both limits directly, such as 12.05 over 11.95. In ASME Y14.5 the upper limit sits above the lower when the two are stacked, and the lower limit comes first when they are written on one line. Nothing has to be calculated, which is one reason limit dimensions appear on critical sizes. To work through limits for your own values, use the limit dimensions tool.

Plus/minus tolerances

A plus/minus tolerance states a nominal value and the allowed deviations from it.

• Equal bilateral: 12 ±0.05, limits 11.95 and 12.05.
• Unequal bilateral: 12 +0.10/−0.05, limits 11.95 and 12.10.
• Unilateral: 12 +0.10/0, all of the allowed variation on one side of nominal.

The nominal value is a reference point. It need not be in the middle of the zone, and with fit tolerances it can lie outside the zone altogether. That matters as soon as a model is built from the drawing.

General tolerances

A dimension with no tolerance of its own takes the general tolerance from the title block or a note. ISO 2768-1 defines classes for linear and angular dimensions without individual tolerance indications: f (fine), m (medium), c (coarse) and v (very coarse), with the permitted deviation growing with the size of the dimension. A note such as “ISO 2768-m” selects a class, and a combined note such as “ISO 2768-mK” adds a general geometrical tolerance class (H, K or L) defined in ISO 2768-2; check which standard and edition the drawing invokes. Drawings to ASME practice more often carry a company tolerance block keyed to decimal places, with one value for X.X and a tighter one for X.XX.

Either way, the general tolerance belongs to every untoleranced dimension on the sheet. It has to be read from the title block, not assumed, and a drawing that has no general tolerance and an untoleranced dimension has a question in it.

What a size means: two-point, envelope and Rule #1

ISO 14405-1 sets the default size of a feature of size as a two-point size: every local measurement across the feature must fall within the limits. Under the ISO default, the independency principle of ISO 8015, a size tolerance does not control form unless a modifier says so. The envelope requirement, a circled E after the tolerance, adds that control. ASME Y14.5 starts from the other default. Its Rule #1 says the limits of size of a regular feature of size also control its form, so at maximum material condition the feature must have perfect form. The same “Ø20 ±0.02” therefore means different things on an ISO drawing and an ASME drawing, and the model shows neither.

GD&T at a conceptual level

Geometric dimensioning and tolerancing, defined in ASME Y14.5 and in ISO 1101 with its related GPS standards, controls form, orientation, location, profile and runout. Each control defines a tolerance zone, and most of them place that zone relative to datums.

Feature control frames

A feature control frame is a row of compartments, read left to right. The first holds the geometric characteristic symbol: position, flatness, perpendicularity, profile and so on. The second holds the tolerance value, with a diameter symbol when the zone is cylindrical, and an optional material condition modifier for maximum or least material condition. The rest hold the datum references, in order of precedence.

A position control of Ø0.2 at maximum material condition to datums A, B and C means that the axis of each hole must lie inside a cylinder 0.2 in diameter, centered on its true position in the A, B, C frame. As the hole departs from its maximum material size (gets larger), the allowed zone grows by the same amount. True position is set by basic dimensions, shown in boxes: theoretically exact values whose tolerance lives in the frame, not on the dimension.

Two consequences follow for anyone modeling from the drawing. Features located this way belong at their basic dimensions in the model. And a cylindrical position zone is larger than the square zone that ±X and ±Y coordinate tolerances give: the circle through the corners of the square has π/2, about 1.57 times, the square's area. That extra usable tolerance is one reason position tolerancing is preferred for hole patterns.

Datums

Datum features are physical surfaces or features named with datum letters on the drawing. The datum reference frame they establish, in order of precedence, is where measurement starts for every control that references them. In a CAD model, datums are only faces and axes. Their letters, their order and their meaning are not in the geometry unless they are added as annotations. The guide to verifying CAD against a drawing shows how to measure a model in the datum frame.

The two systems are close, not identical. ASME Y14.5-2018 removed the concentricity and symmetry characteristics, which ISO 1101 retains, and the defaults for size differ as described above. Read the drawing's standard note before interpreting a frame.

Fits at a conceptual level

A fit describes how two mating features of the same nominal size relate once both tolerances apply. ISO 286-1 builds each tolerance class from two parts. A fundamental deviation, written as a letter (capitals for holes, lower case for shafts), places the zone relative to the nominal size. A standard tolerance grade (an IT grade), written as the number after the letter, sets the zone's width for the size range. H7 is a hole tolerance class; H7/g6 is a fit.

• Clearance fit: the hole is never smaller than the shaft. H7/g6 is a common close sliding fit.
• Transition fit: depending on actual sizes there may be a small clearance or a small interference. H7/k6 is a common locating example.
• Interference fit: the shaft is never smaller than the hole, and the parts are pressed or shrunk together. H7/p6 is a common locational interference fit.

In the hole-basis system the hole is H, whose lower deviation is zero, so the hole's zone starts at the nominal size and goes up. In the shaft-basis system the shaft is h, whose upper deviation is zero. The fit calculator gives the clearance or interference from hole and shaft limits you enter; the limits for a designation come from the tables of ISO 286-2, which this guide does not repeat.

Nominal versus mean-of-tolerance modeling

Most CAD models are built at nominal values, the numbers printed on the drawing. That is simple and traceable, because every model dimension equals a drawing dimension. It breaks down when the tolerance is not symmetric about nominal:

• A pocket depth of 5 +0.2/0 modeled at 5.0 sits at its lower limit, and a toolpath cut to the model aims at the edge of the zone.
• A Ø20 H7 bore modeled at 20.000 sits at the bottom of its zone, which is its maximum material size.
• A Ø20 g6 shaft modeled at 20.000 is outside its zone entirely, because both g6 limits are below the nominal size.
• An interference fit modeled at nominal on both parts gives two cylinders of the same diameter. An assembly interference check then reports nothing, although the drawn parts must interfere.

Mean-of-tolerance modeling, also called mid-limit modeling, builds each feature at the center of its zone: 5.1 for the pocket, and the midpoint of the H7 limits for the bore. Machinists often aim at the middle of the zone, and a model at the mean lets CAM, simulation and inspection programs aim there too. The cost is that model values no longer equal drawing values, so anyone comparing the two must know which convention was used and how values were rounded.

Neither convention is right for every use. The convention has to be chosen on purpose, stated on the model or in its record, and applied to every feature. A model with some features at nominal and some at the mean is the worst case, because it looks like either and is neither.

When several toleranced dimensions add up to one result, such as a gap or an overall length, the result's variation is a stack-up. Worst-case analysis adds the tolerances. Statistical methods such as root sum square assume variations that are independent, centered and roughly normal, with each tolerance taken as the same multiple of its standard deviation (often 3σ), and they are reliable only with several contributors. Try a chain of your own dimensions with the tolerance stack-up tool.

What a CAD model can and cannot carry

ISO 10303-242, STEP AP242, is the application protocol built to carry exact geometry together with the tolerances, datums and notes attached to it. Older protocols such as AP203 and AP214 are mostly used for geometry alone. Whether tolerances survive an exchange depends on both the sending and the receiving system, so check what arrived instead of assuming it.

3D annotations at a general level

3D annotations are the non-geometric data attached to a 3D model: dimensions, tolerances, datums, feature control frames, notes, surface finish and material. ASME Y14.41 sets out practices for digital product definition data, in which an annotated model supplements or replaces the drawing; ISO 16792 is the ISO counterpart.

These annotations come in two forms. Graphic annotation, also called presentation, is displayed for a person to read, much like a drawing placed in 3D. Semantic annotation, also called representation, is machine-readable data linked to the faces it controls, which CAM, inspection programming and tolerance analysis software can use. A model can show a feature control frame on screen with no semantic link to any face, and a receiving system then sees only a picture of text.

When a drawing and an annotated model both exist, the organization has to say which one governs, and many drawings carry a note that settles it. Without one, a model built from a PDF drawing is a derivative: the drawing remains the definition, and tolerances that exist only on the drawing must travel with the model as recorded requirements.