GD&T is the drawing language that states what a feature must do, not just where a coordinate puts it. This guide covers the full ASME Y14.5-2018 symbol set, feature control frame anatomy, datums, MMC/LMC/RFS modifiers, bonus tolerance, composite position, three worked examples, inspection methods, and the case against coordinate tolerancing.
It is written for engineers and buyers who quote drawings and then have to agree with a supplier about conformance. Symbol glyphs are named in words where a browser may not render them.
What GD&T Is and What It Replaces
GD&T is a symbolic language that defines geometry by function. A feature control frame replaces stacked plus/minus dimensions with a tolerance zone of stated shape, the control that applies, and the datums fixing the part in space. The zone matches how the part assembles and how it is inspected.
Coordinate tolerancing looks simpler and often costs more. A hole at ±0.1 mm in X and Y gets a square 0.2 mm zone with 0.04 mm² of area against 0.0314 mm² for a Ø0.2 mm cylinder, so it accepts a 0.141 mm diagonal offset the cylindrical zone would reject, and says nothing about the hole axis.
How to Read a Feature Control Frame
Read left to right: the geometric characteristic symbol, the tolerance zone size and shape with any material condition modifier, then the primary, secondary and tertiary datums. Every compartment is a separate requirement, and the frame applies to the feature its leader touches or to the feature of size it sits under.
Take position, Ø0.25 (M), A, B, C:
- Position states the control; the zone location comes from basic dimensions.
- Ø0.25 (M) is a 0.25 mm cylindrical zone at maximum material condition, so it grows as the hole grows.
- A, B, C set the datum reference frame the inspector must build first.
Basic dimensions are boxed numbers with no tolerance of their own, because the referencing profile, position or angularity frame absorbs all their variation. A drawing full of boxed dimensions is not untoleranced; the tolerances live in the frames.
Two leader conventions extend a frame: all around wraps a profile control around an outline; all over applies it to every surface.
The Full ASME Y14.5-2018 Symbol Set, by Category
Twelve symbols remain in ASME Y14.5-2018, in five categories: four form, three orientation, one location, two profile and two runout. Concentricity and symmetry, both location controls in Y14.5-2009, were removed in 2018, so a print that still calls them out works to an older edition.
Form controls: no datum reference
Form tolerances compare a feature to itself, so a datum reference in a form frame is an error.
| Symbol | Tolerance zone | What it controls | Practical note |
|---|---|---|---|
| Straightness (straight line) | Parallel lines, or a cylinder for an axis with Ø | Line elements, or the derived median line of a feature | Indicator on V-blocks reads it; below 0.01 mm needs a capable turning process. |
| Flatness (parallelogram) | Two parallel planes, value apart, no datum | Every point of a surface at once | Default for sealing faces; plate and 0.001 mm indicator, optical flat above 0.002 mm. |
| Circularity (circle) | Two concentric circles in one cross-section | Each circular element independently along the axis | A two-point micrometer cannot prove it; three-point check or roundness machine, typically 0.005 to 0.02 mm. |
| Cylindricity (circle between lines) | Two coaxial cylinders, radial gap equal to the value | Roundness, taper and straightness of the whole cylinder | Most expensive form control; reserve it for seal journals and bearing seats. |
Orientation controls: datum required
Orientation frames reference at least one datum, fixing the zone in orientation while its location may float.
| Symbol | Tolerance zone | What it controls | Practical note |
|---|---|---|---|
| Perpendicularity (right angle) | Parallel planes at 90 degrees to the datum, or a cylinder with Ø | Squareness of a face or axis to a datum | Granite square and indicator beats a CMM for most floor checks. |
| Parallelism (two slanted lines) | Parallel planes or a cylinder, parallel to the datum | Thickness variation and orientation to a datum | Replaces a tight ± thickness where stack height matters, and flattens the surface too. |
| Angularity (angle) | Parallel planes or a cylinder at the basic angle | Angle and orientation to a datum | The angle must be basic; sine bar or CMM. Never pair it with a ± angle on one face. |
Location control: position
Position is the only location symbol left, and it carries basic dimensions, datum precedence and modifiers at once.
| Symbol | Tolerance zone | What it controls | Practical note |
|---|---|---|---|
| Position (circle with crosshairs) | Cylinder (Ø) or parallel planes centered on true position from basic dimensions | Location and orientation of a feature of size, with (M) or (L) bonus | Cheapest way to locate holes; at MMC a functional gauge checks size and location together. A CNC milling plate gets one frame per pattern. |
| Concentricity (removed in 2018) | Coaxial cylinders about the datum axis, applied to median points | Median points of opposing surface elements | Do not use on new prints: slow to verify, poor match to function. Use position at MMC or runout. |
| Symmetry (removed in 2018) | Parallel planes centered on the datum plane | Median points of opposing elements | Same history; use position on a basic center plane, or profile of a surface. |
Profile controls
Profile controls size, form, orientation and location of shapes no other symbol can describe.
| Symbol | Tolerance zone | What it controls | Practical note |
|---|---|---|---|
| Profile of a line (arc) | Parallel lines offset from the true profile, each normal to it | Form of one line element or a 2D section | For cams, airfoils and extrusions; optical comparator or CMM scan. Without datums it controls form only. |
| Profile of a surface (half circle) | Surfaces offset from the true profile, equal split unless modified | Form, orientation, location and size against basic dimensions | One frame can replace position, angularity and flatness; add all-around or all-over for coverage. |
Runout controls
Runout compares a rotating surface to a datum axis and is always RFS: no MMC or LMC modifier applies.
| Symbol | Tolerance zone | What it controls | Practical note |
|---|---|---|---|
| Circular runout (single arrow) | Concentric circles about the datum axis, per cross-section | Circularity plus coaxiality of each element | Centers or V-blocks with an indicator; a bent or conical part can still pass. |
| Total runout (double arrow) | Coaxial cylinders about the datum axis, whole surface | Coaxiality, cylindricity, taper and face squareness | Must be at least any circular runout on the same feature; below 0.02 mm needs grinding. |
Modifiers: MMC, LMC, RFS, Free State, Projected Zone
MMC adds tolerance as a feature departs from maximum material, LMC as it departs from least material, and RFS is the default with no symbol. Free state, projected zone and tangent plane change where and when the requirement applies. A modifier never changes what is controlled, only how much tolerance is available.
| Modifier | Notation | Effect | When to use it |
|---|---|---|---|
| MMC | (M) | Adds bonus tolerance as the feature departs from maximum material | Clearance holes and fastener patterns checked with functional pins |
| LMC | (L) | Adds bonus as the feature departs from least material | Thin walls where the risk is too little material, such as a bore near an edge |
| RFS | no symbol | Holds the stated tolerance whatever the size | Press-fit dowels, bearing seats, and the Rule 2 default |
| Free state | (F) | Applies the requirement with the part unclamped | Sheet metal and thin rings that deflect, and would otherwise be clamped straight |
| Projected zone | (P) plus height | Extends the zone a stated distance above the surface | Threaded inserts and studs, so an angled hole cannot push the stud out of position |
| Tangent plane | (T) | Contact on the high points only | Gasket faces where only the peaks touch the mating part |
| Unequal profile | (U) plus value | Sets how much profile tolerance lies outside the true profile | Castings and machined pads, for example profile 0.3 (U) 0.1 |
Datums and the Datum Reference Frame
A datum is a theoretically exact plane, axis or point established by a simulator such as a surface plate, chuck or mandrel. The datum features remove six degrees of freedom: the primary three, the secondary two, the tertiary one. The inspector must build the frame the drawing specifies.
On a prismatic part that is the 3-2-1 rule. Datum A stops translation along Z and rotation about X and Y, datum B stops translation along X and rotation about Z, datum C stops translation along Y.
- Reference features that survive to the finished part. A datum on a surface that gets machined away forces the inspector to guess.
- Match precedence to the assembly. The primary datum should be the face that seats on the mating part.
- Use datum targets on castings. Three points marked A1, A2 and A3 give a repeatable seat a rough surface cannot.
- Never datum a centerline. It has no physical feature to build a simulator from.
Bonus Tolerance Worked Example: 4-Hole Pattern at MMC
Bonus tolerance is the extra geometric tolerance a feature earns as it departs from MMC. It equals actual mating size minus MMC size, added to the stated tolerance. A hole at MMC gets the stated zone; at LMC it gets the zone plus the size range.
The example is a 10 mm plate with four holes for M8 bolts: 4x Ø9.0 +0.3/0, position Ø0.25 (M) to A, B, C.
- MMC and LMC. For a hole, MMC is the smallest size, so MMC is Ø9.0 and LMC is Ø9.3.
- Zone at MMC. Ø0.25, allowing 0.125 mm of radial offset.
- Bonus. Actual size minus 9.0, so Ø9.15 earns 0.15 mm.
- Total zone. Ø0.40 at Ø9.15, allowing 0.20 mm radial offset.
- Virtual condition. 9.0 minus 0.25 gives Ø8.75, the boundary the hole never violates, so an Ø8.75 gauge pin must pass.
| Actual hole | Bonus | Total zone | Max radial offset |
|---|---|---|---|
| Ø9.00 (MMC) | 0.00 | Ø0.25 | 0.125 |
| Ø9.10 | 0.10 | Ø0.35 | 0.175 |
| Ø9.20 | 0.20 | Ø0.45 | 0.225 |
| Ø9.30 (LMC) | 0.30 | Ø0.55 | 0.275 |
Check the fastener before releasing the print: for a fixed fastener the minimum hole is fastener diameter plus position tolerance, so 8.0 plus 0.25 gives 8.25, well under the 9.0 minimum hole. That 0.75 mm is why bonus tolerance is safe here, because even at MMC the bolt fits.
Composite Position vs Two Single Segments
A composite frame has one position symbol and two tolerance rows. The top row locates the pattern to the datums. The bottom row controls hole-to-hole spacing and orientation inside the pattern, unlocated to datums it omits. Two single segments are independent requirements that may use different datum sets.
| Aspect | Composite frame | Two single segments |
|---|---|---|
| Bottom row | Spacing and orientation only, not located to omitted datums | Independent requirement that also locates each hole |
| Datum references | Repeat the top row in order, dropping from the right | Free to differ, including none |
| Typical use | Bolt circles where spacing is tight but location may float | Patterns located to one datum set and spaced to another |
The common callout is position Ø0.5 (M) to A, B, C over Ø0.15 (M) to A, B, C. The top row lets the pattern shift 0.25 mm radially, matching cover clearance; the bottom row holds every hole within 0.075 mm of its neighbors, matching insert pitch. A shifted pattern passes the bottom row and fails the top.
Worked Example: Profile of a Surface on a Casting
Profile of a surface on a casting controls the as-cast skin against a true profile built from basic dimensions, with a bilateral zone split equally unless (U) shifts it. It states how much stock the foundry may leave for machining.
An investment-cast A356-T6 housing, 180 mm across, with a machined face and bore, needs three frames:
- As-cast skin: profile 0.8 all over, no datums. Holds the skin to the true profile and keeps wall thickness consistent, without locating it in the datum frame.
- Machined pad: profile 0.3 (U) 0.1 to A, B, C. 0.1 mm outside the true profile, 0.2 mm inside, so the pad may stand proud but not thin the wall beneath.
- 8x Ø9.0 +0.3/0 position Ø0.3 (M) to A, B, C with projected zone (P) 12. The projected height clears the 12 mm stud bosses.
The stock budget is where profile pays: with 2.0 mm of nominal stock and a 0.8 mm as-cast profile, the worst case leaves 1.2 mm before cleanup. A foundry outside that band ships an un-machinable part, and the as-cast frame makes that the foundry’s problem.
Inspection splits in two: scan the as-cast skin with structured light or laser against CAD, and check the machined pad on a CMM at about 1 mm point spacing, with uncertainty at or below 10 percent of the 0.3 mm tolerance. Datum targets A1 to A3 give the CMM a repeatable seat.
Worked Example: Runout on a Shaft
Runout compares a rotating surface to a datum axis. Circular runout checks each cross-section independently; total runout checks the whole surface at once. Both are always RFS, both need a datum axis, and the value must be smaller than the size tolerance of the feature it controls.
The example is a 320 mm steel shaft with bearing journals at Ø40 ±0.008, a gear seat at Ø60, a seal journal at Ø35 and a flange. Datum axis A-B comes from both journals, the standard way to control a shaft in two bearings.
- Gear seat Ø60: circular runout 0.020 to A-B. The press-fit gear needs concentricity at each section, not taper.
- Seal journal Ø35: circular runout 0.012 to A-B. Inside the 0.016 mm size tolerance, as the standard requires, and tight enough for the lip seal.
- Flange face: total runout 0.025 to A-B. Controls squareness to the axis and flatness together, which stops a bolted coupling wobbling.
Run the consistency check on every shaft print. Total runout must be at least as large as circular runout on the same feature, because it includes taper and straightness. A print calling total 0.015 and circular 0.020 is self-contradictory and will be disputed at goods-in.
Process follows tolerance. Turning holds 0.020 mm on a 320 mm shaft; 0.012 mm on the seal journal usually means grinding it and both bearing seats in one setup. Inspect between centers or on V-blocks with a 0.001 mm indicator, rotating 360 degrees; total runout adds an axial traverse.
GD&T vs Coordinate Tolerancing
Coordinate tolerancing gives a rectangular zone and relies on implied datums. GD&T states the zone shape and datum frame explicitly, which changes which parts are accepted, how gauges are designed, how stack-ups are calculated, and how much the supplier must guess.
| Aspect | Plus/minus tolerancing | GD&T |
|---|---|---|
| Zone shape | Square, so the diagonal allows 41 percent more deviation | Cylindrical or parallel-plane zone matched to function |
| Datum | Implied by dimension origin | Explicit, in precedence order, with a simulator per feature |
| Bonus | None, the tolerance is fixed | Available through MMC and LMC |
| Stack-up | Worst-case arithmetic on every dimension | Zones combine as boundaries, often allowing looser individual tolerances |
| Inspection | Each dimension measured separately | Functional gauging at MMC checks size and location in one pass |
| Disputes | Frequent, because function was never stated | Rare, because requirement and inspection method are one statement |
| Best use | Simple parts with no assembly stack | Anything that assembles, rotates, seals or locates |
Cost runs both ways. Frames can add CMM time and need functional gauges, but they usually relax individual tolerances because the zone matches function. A precision machining supplier working to ASME prints inspects to the frame, not the coordinate table, which is worth checking when you qualify a shop.
Inspection Methods by Symbol
Every control has a fast shop-floor method and a reference method: the first holds the process, the second decides conformance in a dispute. Plan both per frame, because the method decides whether the part passes and what the gauge has to be.
| Control | Shop-floor method | Reference method |
|---|---|---|
| Straightness, surface | Straightedge and feeler gauge, or plate and indicator | CMM line scan |
| Straightness, axis | V-blocks and indicator, full rotation | CMM median line |
| Flatness | Plate and indicator, optical flat for lapped faces | CMM plane fit |
| Circularity | V-block and indicator, three-point check | Roundness machine or CMM circle fit |
| Cylindricity | Roundness machine with axial traverse | CMM helical scan |
| Perpendicularity | Granite square and indicator | CMM with a datum frame |
| Parallelism | Plate, height gauge and indicator | CMM |
| Angularity | Sine bar with gauge blocks | CMM |
| Position at MMC | Functional gauge with virtual-condition pins | CMM |
| Position RFS | No fixed gauge applies | CMM or laser tracker |
| Profile of a surface | Profile projector, or a check fixture for repeat parts | CMM scan or structured light against CAD |
| Runout | Centers or V-blocks with a 0.001 mm indicator | CMM with a rotary table |
Whatever the method, the quality assurance plan should name it per frame and state the measurement uncertainty, because a 0.005 mm CMM claiming a 0.01 mm tolerance measures its own error as much as the part. Gauge R&R at or below 10 percent of tolerance is the target; above 30 percent is rejected.
Drawing Review Checklist Before You Send an RFQ
Most quoting disputes come from five habits: missing datums, form tolerances stacked on size tolerances, MMC where no bonus is wanted, profile frames that contradict each other, and tolerances tighter than the process can hold. Ten minutes of review prevents all five.
- State the standard and edition on the print; ASME Y14.5-2018 and ISO 1101 are not interchangeable.
- Check every datum feature exists on the finished part and is reachable by a simulator.
- Keep form tolerances smaller than the size tolerance they refine, or Rule 1 is contradicted.
- Verify runout and profile values sit inside the size band of the features they control.
- Choose MMC or RFS deliberately; MMC on a press-fit bore gives away tolerance the fit needs.
- Check the casting stock budget, since as-cast profile plus allowance must leave cleanup material.
- Reserve sub-0.01 mm tolerances for the features that need them; grinding a whole part for one bore is the classic cost mistake. See CNC machining cost.
- Confirm material and heat treatment first, since residual stress moves a tight frame after machining. 6061 vs 7075 aluminum shows two alloys of similar strength with different thin-wall behavior.
FAQ
Is concentricity still legal under ASME Y14.5-2018?
No. Concentricity and symmetry were removed in 2018, so a drawing that still uses them invokes Y14.5-2009 or earlier. For a rotating part, use circular or total runout to a datum axis. For a clearance fit, position at MMC is cheaper to inspect and closer to the function.
What is the difference between circular runout and total runout?
Circular runout checks each cross-section independently as the part rotates, catching eccentricity and out-of-round there. Total runout checks the entire surface while the indicator traverses along the axis, so it also catches taper, barrel shape and bending, and is always the larger value.
When should I use MMC instead of RFS?
MMC suits assembly clearance, such as a bolt hole pattern, because a larger hole tolerates more positional error without hurting the joint. RFS suits location that matters regardless of size, such as a press-fit dowel or bearing bore. MMC on a fit needing concentricity gives away tolerance you need.
Do I need GD&T on a simple part?
Not necessarily. A part with one tolerance and no mating feature is fully defined by coordinate dimensions, and frames only add inspection cost. GD&T earns its place when a part assembles, rotates, seals, or has a stack-up where variation direction matters.
What if my drawing says ASME but the shop works to ISO?
The defaults differ. ASME applies the envelope requirement through Rule 1, so size limits also control form. ISO 1101 applies the independency principle unless (E) invokes the envelope requirement, so a part made to the ISO default can pass size and still exceed an ASME form limit.
Does GD&T increase machining cost?
Not by itself. Cost follows tolerance value and the number of separately inspected features, not the presence of a frame. GD&T often lowers cost because MMC bonus and functional gauging accept parts a coordinate table would reject, and one profile frame can replace four dimensions.
YC Prime Precision is an ISO 9001-certified contract manufacturer in Qingdao, China, with 90,000 m² of plant, 3- and 5-axis CNC milling and turning to ±0.005 mm, investment and low-pressure casting, and CMM inspection with certificates on request. If you have a drawing with frames to quote, state the standard and edition on the print and send it for an instant quote.
