Form Tolerances

Form tolerances are the family of GD&T controls that govern a single feature’s own shape — how straight an edge is, how flat a surface, how round a circle, how cylindrical a bore or a shaft. They are the purest of the geometric tolerance families: where the orientation, position and runout controls relate one feature to another or to a datum, a form tolerance judges a feature on its own terms, with no datum reference in its call-out, because a surface can be flat without reference to anything else. This entry sets out the four — straightness, flatness, roundness and cylindricity — what each controls, the zone it allows, and what each asks of machining and measurement.

Form, not finish

Form tolerances sit at a boundary a machinist must not confuse: the feature’s shape at the scale of the whole surface, and the texture of its surface at the scale of the tool’s marks. A flat face can be very smooth — its surface finish excellent — and still be bowed, its overall shape wrong; a rough face can still lie within two close parallel planes. Form tolerances govern the first, the macro-geometry, judged over the feature’s full extent, and that decides how they are measured: a surface plate and an indicator sweep the whole face for flatness, where a roughness meter would tell nothing. Form is the feature’s truth of shape; finish is the truth of its texture, and the drawing states each separately.

Straightness

Straightness is the form control of a line, and it has two meanings the drawing keeps apart. On a flat surface, it keeps every line element of the surface — a line drawn across the face — within two parallel straight lines a stated distance apart, the control where one line on a face must be true, such as a surface that locates a slide or a seal along a narrow path. Called out on an axis, it means something stronger and commoner in machining: the axis of a shaft or long bore must lie within a cylindrical zone of the stated diameter along its whole length, controlling a shaft’s bow or a long bore’s wander. Axis straightness is the machining meaning of “not banana-shaped”: a bar turned between centres can be round at every cross-section and still bow, and this tolerance catches the bow. A straightness of a line element is measured with a straightedge and feeler, or a dial swept along the line; straightness of an axis by rotating the part on its ends and indicating the middle, or on a CMM.

Flatness

Flatness controls a whole surface, keeping it within two parallel planes a stated distance apart; it is the form tolerance a machinist meets most often, on faces that must seal, sit flush or provide a datum. The zone is a slab: the entire surface must lie between two imaginary parallel planes of any orientation, and every point of the face must fall within the slab’s thickness. Flatness carries no datum — the surface is judged against itself — and its call-out is a parallelogram symbol with a tolerance value, standing alone in its control frame. Machining flatness is largely the art of not making it worse: the machine’s face pass can be true, yet the part leaves the machine bowed if clamping distorted it or released stress moved it, so the face is machined with the part held without bending and unclamped before it is judged. Measuring flatness is done on a surface plate, sweeping an indicator across the face in a grid and taking the spread of readings as the slab’s thickness — one of the fundamental measurements of measuring a feature.

Roundness

Roundness — circularity in GD&T, roundness in shop speech — controls a single circular cross-section of a cylindrical feature, keeping it within two concentric circles a stated radial distance apart. Its zone is an annulus: at every point around the circumference, at one cross-section, the surface must fall between a pair of concentric circles whose radial separation is the tolerance. Roundness is judged one cross-section at a time: it does not limit whether the diameter changes along the length, which is a matter of size and straightness. A turned or ground diameter can differ at each end and still be round at every section. Roundness is what a lathe produces when the work runs true, and what grinding holds when the wheel cuts a true circle; it is destroyed by a chuck gripping the part out of round, by three-jaw pressure distorting a thin ring, or by untrue centres. Precise measurement needs a roundness machine that rotates the part about its axis and plots a stylus’s trace; a V-block and indicator give an approximation that misses some lobes of error, and the tolerance tells whether the approximation suffices.

Cylindricity

Cylindricity is the most demanding of the four, combining roundness and straightness into one control of the whole surface of a cylinder. Its zone is the space between two coaxial cylinders a stated radial distance apart, and the entire surface — at every cross-section, over the whole length — must fall within it. Cylindricity therefore controls roundness and axis straightness and taper and diameter variation all at once: a feature can pass roundness at every section and still fail cylindricity if its diameter changes along its length, because the two coaxial cylinders must contain the whole surface. It is used where a whole cylindrical surface must work together — a bore a piston must seal along its full travel, a journal that must sit in a bearing along its length. Cylindricity is rarely specified and never cheap: it demands grinding or honing with the work held without distortion, and measurement over the full length on a roundness machine or CMM, so the drawing uses it only where the function truly asks.

Form in the cut

The four form tolerances ask different things of the machine, but the machinist reads them by one question: what keeps this feature true to its own ideal shape? Straightness of an axis asks how the part is held and cut so it does not bow; flatness asks how the face is cut and released so it does not spring; roundness asks how the work runs in chuck, centres or steady so every cross-section is a true circle; cylindricity asks all of it together, the whole cylindrical surface held in one close zone. Every answer returns to the same foundations: a rigid machine, a part held without distortion, a cut that does not move the work, and the repeatability to make the next part as true as the first. Form tolerances are the drawing’s way of saying a feature must be shaped right, not just sized right, and the machinist who reads the GD&T language reads in each one a requirement that setup, cut and measurement all meet — shape held true to itself, from first pass to final check.