GD&T - Geometric Dimensioning & Tolerancing

Every feature on a part has a size, a shape, an angle and a location. Geometric Dimensioning and Tolerancing (GD&T) gives each of those its own control and defines an exact zone the real feature must fit inside. When you know what zone a symbol makes, you know what to measure, what to measure it from, and what a passing part looks like.

What You Will Be Able to Do

• Name the 12 geometric characteristics and their five categories.
• Describe the tolerance zone each one makes and say when it needs a datum.
• Say how each characteristic is usually checked.
• Work out what a basic dimension, a position callout and a title-block tolerance each control on the same feature.
• Explain Rule #1, a projected zone, and why a round zone is not the same as a square one.

Which Edition Governs the Drawing

ASME Y14.5-2018, reaffirmed in 2024, is the current US edition. It is on stabilized maintenance, and there is no newer edition. It lists 12 geometric characteristics.

The 2009 edition listed 14. The 2018 edition removed concentricity and symmetry because they were hard to inspect and often misused. Position covers most of what they did, and runout or profile covers the rest. The 2009 edition is still widely used, so you will still see those two symbols. The drawing's title block or notes say which edition governs. If a drawing cites the 2009 edition, its symbols mean what that edition says. Some companies draw to ISO rules, which look similar but differ in places. If a drawing names no standard, ask before you interpret it.

The 12 Characteristics at a Glance

Two habits make everything below easier. First, the number in the frame is the total width of the zone, not a plus-or-minus value. A zone 0.010 wide is 0.005 each side of center. Second, the controls nest. Form is usually the tightest, then orientation, then location. A position zone also limits tilt, and a parallelism zone also limits flatness, so a tighter callout on the same feature only refines the looser one.

Form: Shape With No Reference

Form controls compare a feature to its own perfect shape. They never use a datum, because they say nothing about where the feature sits.

Flatness and straightness differ in what they cover. Flatness controls a whole surface. Straightness controls one line at a time on that surface, or the axis of a cylinder. Circularity and cylindricity differ the same way. Circularity tests each cross-section on its own, so a tapered pin can pass. Cylindricity tests the whole surface at once, so it includes circularity and straightness and also catches taper.

Setting a part on a surface plate and sweeping the top face does not check flatness. That checks parallelism to the bottom face, because any warp in the bottom tilts the reading. A micrometer also has limits on round parts. A shape with three lobes can read the same diameter all the way around and still be out of round.

Orientation: Angle to a Datum

Orientation controls hold a feature at an angle to a datum, so a datum is always required. They control angle only, not location. The zone keeps its angle to the datum but can slide anywhere the feature's other dimensions allow.

On a surface, the zone is two parallel planes. On an axis with a Ø in front of the number, the zone is a cylinder, so the whole axis must stay inside it from end to end.

Location: Position

Position is the most common callout you will read. It sets a zone centered on the exact location given by basic dimensions from the datums. The axis of a hole or pin gets a cylinder, shown with Ø. The center plane of a slot or tab gets two parallel planes, with no Ø. Position applies to features of size, and it almost always references datums. The rare exceptions are special cases such as a pattern controlled only to itself.

Position is reported as a diameter, so the math has one extra step. Find how far the axis is from its true location, then double it.

1. Take the X and Y errors. Say the hole is 0.003 off in X and 0.004 off in Y.
2. Find the straight-line distance. Square each, add them, and take the square root: 0.000009 + 0.000016 = 0.000025, and the square root is 0.005.
3. Double it. The position reads 0.010.

That hole needs a zone of at least Ø 0.010. It fails a Ø 0.008 zone, even though each error looks small on its own. A CMM does this math, builds the datum frame first, and checks the axis along its length. A functional gauge can also check position when the frame uses (M).

Round Zones Versus Square Zones

A plus-or-minus location of +/- 0.005 in X and Y makes a square zone 0.010 on each side. A Ø 0.010 cylinder fits inside that square and touches its sides. A hole in the corner of the square is 0.0071 from center (0.005 x 1.414), so the square accepts it and the cylinder rejects it. At the same number, the cylinder is the tighter of the two.

Now look at it from the mating part. A bolt does not care which direction a hole is off. If 0.0071 works in the corner, it works in every direction. A round zone of Ø 0.0141 reaches the same corners and has about 57 percent more area than the square. That is why a round zone suits round parts: it accepts every hole that will work the same way in every direction.

Profile: With and Without Datums

Profile controls a shape of any kind, including curves. Basic dimensions define the true shape, and the zone follows it. The number is the total width, split evenly on both sides unless a (U) modifier says otherwise.

• Profile of a line makes a 2D zone that applies to each cross-section by itself, like two offset lines on a slice through the part.
• Profile of a surface makes a 3D zone of two offset surfaces, and the entire surface must lie between them at once.

The datums decide how much it controls.

Profile is checked with a CMM scan. Profile of a line can also be checked on an optical comparator against an overlay.

Runout: Rotating Parts

Runout controls surfaces that spin around a datum axis, so a datum is always required. It is read as full indicator movement (FIM), the difference between the highest and lowest reading.

• Circular runout checks one cross-section at a time. Rotate the part a full turn with the indicator at one spot, then move and start again. Each circle is judged alone.
• Total runout checks the whole surface at once. Sweep the indicator along the surface while the part rotates, and do not reset it. The full sweep must stay inside the tolerance.

Because of that, total runout catches out-of-round, bow, taper and axis offset together, while circular runout can miss taper and bow. On a face, circular runout catches wobble at each radius, and total runout also catches a dished or coned face. Runout takes no (M) or (L). To check it, rotate the part on its datum diameters, between centers, in a collet or in V-blocks, and do not rotate it on the surface being measured.

Basic Dimensions and the Title Block

A basic dimension is a number in a box. It is theoretically exact. It has no tolerance of its own, the title block does not apply to it, and you never add a plus-or-minus to it. The tolerance comes only from the feature control frame that uses it.

Here is how the pieces divide up on one drawing. The title block says +/- 0.005. A hole is dimensioned Ø 0.500 with no tolerance beside it, located by boxed dimensions of 1.500 and 0.750, with a frame of position Ø 0.010 to A, B and C. The part's overall length is 4.000.

The frame overrides the title block for the characteristic it controls, here location. It does not touch anything else, and the title block still governs size and any feature with no frame.

Rule #1 in Plain Words

Rule #1 says a feature of size must have perfect form when it is at its maximum material condition (MMC), the size with the most material: the largest shaft or the smallest hole. A shaft of Ø 0.500 +/- 0.002 must fit inside a perfect Ø 0.502 cylinder. At 0.502, it must be perfectly straight and round. At 0.498, it can bow up to 0.004 and still fit the envelope.

So size limits also limit form, even with no form symbol on the drawing. Rule #1 applies to each feature by itself. It does not control how one feature relates to another, such as a hole to a face. That takes a geometric control.

Modifiers in the Frame

(P) modifies the tolerance zone. It is not a datum modifier and never appears after a datum letter. It is common on threaded and press-fit holes, because a bolt follows the tilt of its hole. Say a thread 0.500 deep leans 0.002 over its depth. About 0.750 above the surface, the bolt has moved another 0.003, right where it passes through the mating part. A zone inside the hole would never see that. So the frame projects the zone above the surface by a stated height, usually the thickness of the mating part.

Common Mistakes

If a callout is unclear, ask engineering and get the answer in writing. A guess can scrap a whole job.

Check Your Understanding

1. A hole reads 0.004 off in X and 0.003 off in Y. The frame is position Ø 0.008 with no modifier. Does it pass?

No. The straight-line error is 0.005, so the position reads 0.010, which is over 0.008. Neither error looks large alone, but the zone is round and the distance is what counts.

2. The title block says +/- 0.010. A hole has boxed location dimensions and a position frame of Ø 0.006. A coworker says the location can be off by 0.010. Are they right?

No. Boxed dimensions take no title-block tolerance. The position frame controls location, so the zone is Ø 0.006. The title block may still control the hole's size if the size has no tolerance of its own.

3. A shaft passes circular runout at three sections, but fails total runout. How can that happen?

Each circle was fine on its own, but the circles do not line up along the length. Taper or bow shifts the readings from section to section. Total runout never resets the indicator, so it catches the change.

4. A curved surface has profile of a surface 0.008 with no datums. Another drawing shows the same callout to A, B and C. What is different?

The first controls shape only, and the zone can float to fit the part. The second also fixes the surface's angle and location relative to the datums, so it is much harder to meet.

Key Takeaways

• The 2018 edition has 12 characteristics and the 2009 edition had 14. The drawing says which governs.
• The frame's number is the full width of a zone, and the symbol tells you the zone's shape.
• Form never takes a datum, orientation and runout always do, position nearly always does, and profile may or may not.
• Basic dimensions are exact. The frame overrides the title block only for what the frame controls.
• At the same number, a round zone is tighter than a square one, but it treats every direction alike, which suits round parts.
• Rule #1 means perfect form at MMC. (P) moves a zone above the surface and is not a datum modifier.