ASME Y14.5-2018 Dimensioning & Tolerancing Best Practices

Table of Contents

1. Introduction — Why ASME Y14.5 Matters

ASME Y14.5-2018 is the authoritative American National Standard for dimensioning and tolerancing in engineering drawings and digital product definitions. It establishes the symbols, rules, definitions, requirements, defaults, and recommended practices that engineers use to communicate geometric requirements — size, form, orientation, location, and profile — from design through manufacturing and inspection.

The 2018 revision (which supersedes ASME Y14.5-2009) made several key changes: the concentricity and symmetry symbols were eliminated (other characteristics now provide more direct and unambiguous control), profile tolerancing for location is emphasized over plus/minus tolerancing, and model-based definition (MBD) support was expanded throughout.

The language of the standard is precise: "shall" means mandatory, "should" means recommended, and "may" means permissible. Understanding this distinction is the first step to correctly applying GD&T.

2. Fundamental Rules of Dimensioning

Section 4 of the standard establishes fundamental rules that govern every dimension and tolerance on an engineering drawing. Violating any of these is a non-conformance to the standard.

Dimensioning Application Rules

• Dimension lines shall not be centerlines, extension lines, phantom lines, or outlines of the object.
• Extension lines start with a short visible gap from the part outline and extend beyond the outermost dimension line. They are drawn perpendicular to dimension lines.
• Leaders terminate in an arrowhead (to an edge) or a dot (within a surface outline). Leaders should be inclined straight lines with a short horizontal portion at the note/dimension midheight.
• Overall dimensions: When an overall dimension is specified, one intermediate dimension is omitted or identified as reference.
• Dimensions should be placed outside the outline of a view unless directness of application provides clarity.

3. Units, Notation, and Tolerance Expression

Millimeter Dimensioning (Section 4.3.1)

• Dimension less than 1 mm ? leading zero is required (e.g., 0.5, not .5)
• Whole-number dimension ? no decimal point, no trailing zero (e.g., 25, not 25.0)
• Dimension with decimal fraction ? no trailing zero (e.g., 25.5, not 25.50) — except in bilateral tolerances where matching decimal places are required
• No commas or spaces to separate digit groups

Inch Dimensioning (Section 4.3.2)

• Express to the same number of decimal places as the tolerance
• In bilateral tolerancing, the dimension and both tolerance values have the same decimal places
• In limit dimensioning, if either limit has decimal digits, the other shall have matching trailing zeros (e.g., 1.250 / 1.000)

Tolerance Expression (Section 5.3)

Tolerances may be expressed as:

• Limit dimensioning — high limit above low limit (or low–high on a single line with a dash)
• Plus and minus (bilateral) — dimension ± tolerance
• Unilateral — variation in one direction only; the zero value carries the sign of the nonzero value
• Geometric tolerance via feature control frame
• General tolerance note or tolerance block referencing all unspecified dimensions

Single Limit Tolerances

MIN or MAX is placed after a dimension when the other limit is determined by the design context (e.g., depth of a blind hole may have only a MIN). Use this only when the intent is clear and the unspecified limit approaches zero or infinity without detriment.

4. Limits of Size and the Envelope Principle (Rule #1)

Section 5.8 establishes how size limits control form for regular features of size — cylindrical surfaces, spherical surfaces, circular elements, and sets of two opposed parallel surfaces.

When Rule #1 Does NOT Apply

The envelope principle is overridden in these cases:

• Stock items (bars, sheets, tubing, structural shapes) governed by industry standards — surface texture governs in the as-furnished condition
• Features with the free state modifier (nonrigid parts)
• When a form tolerance (straightness or flatness) is applied directly to a feature of size — this allows the feature to exceed the MMC envelope in form
• When the independency symbol (?) is applied — form becomes uncontrolled by size, requiring a supplementary form tolerance
• When average diameter is specified (for flexible parts)

Relationship Between Individual Features (Section 5.8.3)

Limits of size do not control orientation or location relationships between individual features. Features shown perpendicular, coaxial, or symmetrical must be adequately toleranced with orientation/location/profile controls. Do not rely on size tolerances alone for functional relationships.

5. Material Condition Modifiers — RFS, MMC, LMC (Rule #2)

Rule #2: The Default (Section 5.9.1)

Surface Method vs. Axis Method

When a geometric tolerance is applied at MMC or LMC, two interpretation methods exist:

• Surface method (default and preferred): The feature's surface shall not violate the virtual condition (VC) boundary. This is the more conservative and physically meaningful interpretation.
• Axis method: The feature's derived axis, center plane, or center point shall not violate the tolerance zone. This method carries risks when there are form deviations on the feature.

Geometric Characteristics That Cannot Use MMC/LMC

The following cannot be modified by MMC or LMC: circular runout, total runout, orientation tolerances applied to a surface, profile of a line, profile of a surface, circularity, and cylindricity. These apply RFS only.

6. Datum Reference Frames

Section 7 establishes the datum system — the backbone of GD&T. A datum reference frame (DRF) consists of three mutually perpendicular planes and three mutually perpendicular axes at their intersections. Together they define a coordinate system from which measurements are taken.

Six Degrees of Freedom

Every part has six degrees of freedom: three translational (X, Y, Z) and three rotational (u, v, w). Datum features constrain these degrees of freedom based on their geometry:

Order of Precedence

Datum feature references in a feature control frame are listed left to right in order of precedence: primary, secondary, tertiary. The primary datum constrains the most degrees of freedom; the tertiary completes the constraint. This order directly determines how the part is fixtured for inspection.

True Geometric Counterpart

A true geometric counterpart is the theoretically perfect boundary used to establish a simulated datum from a physical datum feature. In practice, this is represented by a gage surface, fixture element, or mathematical simulation. It has perfect form and basic orientation relative to other datum references in the same frame.

Temporary vs. Permanent Datum Features

In-process features (e.g., machining references on a casting) may serve as temporary datum features to establish permanent datums. Permanent datum features should be surfaces or diameters that are not appreciably changed by subsequent processing operations.

Datum Targets

When a full surface cannot serve as a reliable datum feature (e.g., a rough casting or warped surface), datum targets are used. They designate specific points, lines, or areas on the feature. Target types include:

• Datum target point — contact at a specific point (used in sets of three for a primary plane)
• Datum target line — contact along a line
• Datum target area — contact over a defined area (shape and size specified in the upper half of the datum target symbol)

7. Feature Control Frames and Symbology

Feature Control Frame Anatomy

The feature control frame (FCF) is the primary method for specifying geometric tolerances. It consists of compartments read left to right:

Fourteen Geometric Characteristic Symbols

ASME Y14.5-2018 defines 14 geometric characteristics (the concentricity and symmetry symbols were removed in the 2018 edition):

Feature Control Frame Placement

An FCF is related to a considered feature by:

• Placing it below or beside a leader-directed note or dimension pertaining to the feature
• Attaching a leader from the frame pointing to the feature or extension line
• Attaching a side, corner, or end of the frame to an extension line from the feature

Key Modifying Symbols

8. Form Tolerances (Section 8)

Form tolerances control the shape of individual features without any datum reference. They are the only tolerances in GD&T that do not require datums. Form tolerances are always RFS — MMC and LMC do not apply when form tolerances are applied to a surface.

Straightness

Controls the straightness of a surface element (2D, on a line element) or a derived median line (3D, on a cylindrical feature of size). When applied to a flat surface, each line element in the indicated direction must lie within a tolerance zone of two parallel lines separated by the tolerance value. When applied to a cylinder axis (derived median line), the axis must lie within a cylindrical zone of diameter equal to the tolerance value.

Flatness

Controls all elements of a surface within a tolerance zone of two parallel planes. Flatness is always applied to surfaces, never to features of size (unless the derived median plane is specified explicitly). The flatness tolerance must be less than the size tolerance of the feature it controls.

Circularity (Roundness)

For a cylinder or cone: all points of each circular cross-section must lie within an annular zone (two concentric circles) in the plane of that cross-section. The zone width equals the circularity tolerance. For a sphere: all points of any circular cross-section must lie within the annular zone. Circularity is always RFS.

Cylindricity

The most complex form control — all points of a cylindrical surface must lie within a tolerance zone of two coaxial cylinders. Cylindricity simultaneously controls circularity, straightness, and taper of the cylinder. Like all form tolerances, it requires no datum.

Nonrigid Parts — Free State and Restrained

Flexible parts (sheet metal, rubber seals, thin-walled parts) may be inspected in the free state (gravity only) or the restrained condition (simulating assembly loads). The ? free state modifier in the FCF specifies that the tolerance applies in the unrestrained condition. Notes on the drawing should specify any restraint forces required for inspection.

9. Orientation Tolerances (Section 9)

Orientation tolerances — angularity, parallelism, and perpendicularity — control the angular relationship between features. All orientation tolerances require at least one datum reference. They also inherently control flatness (for surface features) or straightness (for axes) within the orientation tolerance zone.

Tangent Plane Modifier

When the tangent plane modifier ? is added to an orientation tolerance, the zone is established by the high points of the surface (the tangent plane) rather than all surface elements. This is useful for mating surfaces where only the tangent plane orientation matters, not the form of the surface itself.

Zero Orientation at MMC

A zero orientation tolerance at MMC can be used to establish a boundary of perfect form at MMC for controlling the relationship between features. For example, specifying perpendicularity at 0 ? relative to a datum controls both the axis deviation and the virtual condition of the feature simultaneously, eliminating the tolerance zone when the feature is at MMC.

10. Location Tolerances — Position (Section 10)

Positional tolerancing is the most widely used GD&T control. It defines the allowable variation in the location of a feature of size (holes, pins, slots, bosses) from its true position — the theoretically exact location established by basic dimensions.

Positional Tolerancing Fundamentals

The tolerance zone for a cylindrical feature (hole, pin) is typically a cylinder of diameter equal to the positional tolerance value, oriented perpendicular to the datum plane and centered on the true position. For a feature at RFS, the axis of the unrelated AME must lie within this cylinder.

Fixed vs. Floating Fastener Formulas

When applying positional tolerances for fastener clearance holes, use the appropriate formula:

• Floating fastener (bolt through clearance holes in both parts): T = H - F, where T = positional tolerance diameter, H = minimum hole diameter, F = maximum fastener diameter. Each part gets the same tolerance: T per part = (H - F) / 2 if split equally.
• Fixed fastener (stud or press-fit in one part): T = H - F, where the full tolerance is applied to the clearance hole only, or split as T1 + T2 = H - F.

Projected Tolerance Zone

When a threaded insert, dowel pin, or stud can cause interference with a mating part outside the toleranced part, the tolerance zone is projected above the part surface by the minimum projection height. This ensures the fastener's functional length stays within the positional constraint, preventing interference in assembly.

Composite Positional Tolerancing

A composite feature control frame for position contains a single position symbol followed by two (or more) segments. The upper segment controls the pattern location relative to datums (PLTZF — Pattern Locating Tolerance Zone Framework). The lower segment controls only the feature-to-feature relationship within the pattern (FRTZF — Feature Relating Tolerance Zone Framework) — orientation to the datums is maintained but not location.

Bidirectional Positional Tolerancing

When different tolerances are needed in X and Y directions, bidirectional positional tolerancing uses two separate feature control frames — one per direction — or the polar coordinate method. The tolerance zone becomes a rectangle rather than a cylinder. This is appropriate for slots or elongated holes where assembly requirements differ by direction.

Coaxial Feature Controls

Coaxiality (the condition where two or more feature axes are coincident with a datum axis) is now controlled by positional tolerancing or profile of a surface rather than the deprecated concentricity symbol. Position RFS controls the axis of the AME; profile of a surface controls all surface elements directly. Position at MMC/LMC allows bonus tolerance as size departs from the stated material condition.

Symmetrical Relationships

The symmetry symbol was removed in ASME Y14.5-2018. Symmetrical relationships are now controlled by positional tolerancing or profile of a surface applied to the feature's derived median plane or axis. This provides clearer, more directly verifiable requirements.

11. Profile Tolerances (Section 11)

Profile tolerances are the most versatile tool in GD&T — they can control form, orientation, location, and size simultaneously with a single control. ASME Y14.5-2018 emphasizes profile as the preferred method for location tolerances applied to surfaces.

Profile of a Surface vs. Profile of a Line

• Profile of a surface — controls all surface elements in three dimensions. The tolerance zone is two boundaries (inner and outer) that are uniform offsets of the true profile surface. This is the primary profile control for 3D surfaces.
• Profile of a line — controls surface elements in two dimensions (cross-sections in the indicated view only). Used as a refinement when only a specific cross-section matters, or for extruded/prismatic features with a profile refinement in one plane.

Tolerance Zone Disposition

Composite Profile Tolerancing

Like composite position, composite profile has a single profile symbol with multiple segments. The upper segment establishes the profile location and orientation relative to datums. The lower segment controls only the form and orientation of the profile (not its location relative to datums). This is powerful for complex curved surfaces where tight form control is needed independent of where the feature is located.

Dynamic Profile Tolerance Modifier (New in 2018)

The dynamic profile modifier controls the form of a feature independent of its size. When applied in a composite profile frame, it allows the lower segment to control form only — the feature can grow or shrink in size while maintaining the specified form refinement. This is particularly useful for controlling the cross-sectional shape of extruded features or surfaces of revolution where size varies by design intent.

Application Range — All Around, All Over, Between

• All around — profile applies to all surfaces visible in the view indicated (shown by a circle at the bend of the leader)
• All over — profile applies to all surfaces of the part (shown by two concentric circles)
• Between — profile applies between two designated points/features on the part

12. Runout Tolerances (Section 12)

Runout tolerances control surfaces of revolution — cylinders, cones, and face surfaces — relative to a datum axis. They are always applied RFS and always require a datum axis reference. Runout is typically used for rotating parts (shafts, bearing journals, pulleys).

Circular Runout

Controls each individual circular cross-section independently. As the part is rotated 360° about the datum axis, the full indicator movement (FIM) at any single circular cross-section must not exceed the runout tolerance. Circular runout controls a combination of out-of-roundness and eccentricity — it does not directly control the axis of the feature.

Total Runout

Controls all surface elements simultaneously across the entire surface. As the part is rotated and the indicator moved along the full length of the surface, the total FIM must not exceed the tolerance. Total runout controls cylindricity (form), coaxiality, and taper simultaneously. It is a more comprehensive and tighter control than circular runout.

Runout vs. Cylindricity vs. Coaxiality

13. Top Best Practices for Engineering Drawings

• 1
  Apply GD&T from function, not manufacturing convenience. Datum features and tolerance values should reflect how the part works in assembly — what mates with what, what must rotate, what must seal. Datum selection based on manufacturing process leads to inspection-unfriendly parts and parts that pass inspection but fail in assembly.
• 2
  Use basic dimensions with feature control frames instead of plus/minus for features of size location. Plus/minus tolerancing on locating dimensions creates non-cylindrical tolerance zones (square zones for bolt patterns) that are more restrictive than needed for round fastener heads. Position with basic dimensions gives circular zones and maximizes the acceptable part yield.
• 3
  Choose profile of a surface for complex surfaces and surface-to-surface relationships. Profile simultaneously controls size, form, orientation, and location. It eliminates the tolerance accumulation that arises from chaining multiple direct tolerances. Profile referenced to a common datum reference frame is the preferred location control in the 2018 edition.
• 4
  Specify datum features in functional order of precedence. Primary datum should be the largest, most stable surface (typically the mounting face). Secondary and tertiary datums should correspond to functional interfaces. Maintain the same datum reference frame across related features to avoid tolerance accumulation from frame switching.
• 5
  Apply MMC modifier where clearance assembly is the functional requirement. When parts assemble with clearance fits, MMC on positional tolerances captures bonus tolerance when the feature is smaller than MMC — allowing looser production control when the feature naturally has more clearance. Zero position at MMC is particularly effective when virtual condition must be exactly at nominal.
• 6
  Avoid unnecessary tight tolerances. Tighter tolerances increase cost non-linearly. Use tolerance stackup analysis (worst-case or statistical) to determine the minimum required tolerances for assembly. Statistical tolerancing (Section 5.18) with SPC can justify larger individual tolerances when the manufacturing process is demonstrated to be capable.
• 7
  Use composite tolerancing to separate location from form/orientation control. Composite position or composite profile allows a wide location tolerance for assembly and a tight form/orientation tolerance for fit or function. This avoids the cost of holding tight location tolerances on a whole pattern when only the internal pattern relationship matters.
• 8
  Always add the standard reference on your drawing. Any engineering document based on ASME Y14.5-2018 shall note this fact on the document. Use the full designation: "ASME Y14.5-2018" — not "ASME Y14.5" or "per GD&T standard." This prevents ambiguity when the 2009 and 2018 editions differ.
• 9
  Replace concentricity and symmetry with position or profile. Both symbols were eliminated in the 2018 edition due to the difficulty of measuring the derived median point/plane required. Use position (for axis control) or profile of a surface (for surface control) instead — these have well-defined measurement procedures and consistent interpretation.
• 10
  Use projected tolerance zones for threaded inserts, press-fit pins, and studs. The interference risk for these features occurs outside the part boundary, where the fastener or pin protrudes. A projected tolerance zone extends the positional zone above the surface by the minimum engagement length, ensuring the mating part sees correct alignment.
• 11
  Apply datum targets for castings, forgings, and large or flexible parts. Full surface datums are unreliable when surfaces are rough, non-flat, or functionally contact only at specific points. Datum targets define the exact contact points used for fixturing, creating repeatable datum establishment between design, manufacturing, and inspection.
• 12
  For plated or coated parts, explicitly state whether limits apply before or after processing. Section 5.4.1 requires the drawing or referenced document to specify this. A note such as "DIMENSIONAL LIMITS APPLY AFTER PLATING" eliminates ambiguity and prevents scrap due to coating thickness misinterpretation.

14. Common Mistakes to Avoid