6.1 Flatness & Straightness Controls for Surfaces & Features of Size

ASME GDTP Technologist Y14.5-2009

Track your progress as you read

Finished sections get a check mark.

1 Chapter 1: Scope, Certification Logistics, Fundamental Rules & General Dimensioning

1.1 ASME GDTP Technologist Exam Scope, Prometric Logistics, & Certification Rules 1.2 Fundamental Rules of ASME Y14.5-2009 (Rules a through p) 1.3 Engineering Drawing Standards, Drawing Units, & Basic vs. Toleranced Dimensions 1.4 Dimensioning Features: Diameters, Radii, Chamfers, Countersinks, Counterbores, Spotfaces, Keyseats & Slots 1.5 Application of Dimensions & Location of Features: Lines, Leaders, Reference Dimensions, Rectangular vs. Polar Coordinates

2 Chapter 2: Features, Limits of Size, & Material Condition Principles

2.1 Features, Features of Size, & Limits of Size 2.2 Rule #1 (Taylor Principle / Envelope Rule), Its Exceptions & Overrides 2.3 Material Condition Concepts: MMC, LMC, & RFS Calculations

3 Chapter 3: General Tolerancing & Symbology

3.1 Direct Tolerancing, Limit Dimensioning, & Angular Tolerancing 3.2 The 14 Geometric Characteristic Symbols, Feature Control Frames, & Special Modifiers 3.3 Screw Threads, Gears & Splines, Angular Surfaces, Tapers & Statistical Tolerancing 3.4 Feature Control Frame Placement, Combined Frames, Tolerance Zone Definition & Tabulated Tolerances

4 Chapter 4: Datum Reference Frames & Degrees of Freedom

4.1 Theoretical Datums, Datum Feature Simulators, & Physical Datum Features 4.2 Degrees of Freedom Constraint & The 3-2-1 Datum Precedence System 4.3 Planar, Cylindrical, & Width Datum Feature Establishment

5 Chapter 5: Advanced Datum Applications: Targets, Boundary Modifiers, Customized Frames & Restrained Condition

5.1 Datum Target Points, Lines, Areas, & Movable Datum Simulators 5.2 Material Boundary Modifiers (RMB, MMB, LMB) & Datum Shift Calculations 5.3 Functional Datum Feature Selection, Multiple Datum Reference Frames & Simultaneous vs. Separate Requirements 5.4 Rotational Constraint About a Datum Axis or Point & Customized Datum Reference Frames 5.5 Irregular & Complex Datum Features, Mathematically Defined Surfaces, Restrained Condition & Datum Feature Controls

6 Chapter 6: Form Tolerances

6.1 Flatness & Straightness Controls for Surfaces & Features of Size 6.2 Circularity & Cylindricity Controls, Differences, & Inspection

7 Chapter 7: Orientation Tolerances

7.1 Parallelism Controls for Planar Surfaces & Cylindrical Features of Size 7.2 Perpendicularity & Angularity Tolerances with Basic Angles & Tangent Plane

8 Chapter 8: Location: Position Fundamentals & Calculations

8.1 Position Tolerancing Fundamentals, True Position, & Coordinate Conversions 8.2 Bonus Tolerance & Virtual Condition Calculations for Internal & External Features 8.3 Projected Tolerance Zones (Ⓟ Modifier) & Fixed vs. Floating Fastener Formulas 8.4 Zero Positional and Orientation Tolerancing at MMC and at LMC 8.5 Surface vs. Axis Interpretation of Position & the Boundary Concept for Slots, Tabs & Noncircular Features

9 Chapter 9: Location: Patterns, Composite Controls, Coaxial & Symmetrical Relationships, and Functional Gaging

9.1 Hole & Slot Patterns, Multi-Segment Frames, & Composite Position Tolerancing 9.2 Functional Gaging Principles & Inspection Verification of Position 9.3 Coaxial Holes, Counterbored Holes, Non-Parallel Axes, Spherical Features & Bidirectional Position 9.4 Concentricity & Symmetry Tolerances Under ASME Y14.5-2009 9.5 LMC Applied to Position: Wall Thickness, Breakout Protection & Boundary Calculations

10 Chapter 10: Profile Tolerances

10.1 Profile of a Line & Profile of a Surface Fundamentals & Basic Geometry 10.2 Bilateral, Unilateral, & Unequally Disposed Profile Boundaries (Ⓤ Modifier) 10.3 Composite Profile Tolerances vs. Multiple Single-Segment Profile Controls 10.4 Profile Verification, Coplanarity Controls, & Non-Rigid Parts 10.5 Profile Applications: Conicity, Extruded and Irregular Shapes, and Profile-Controlled Datum Features 10.6 Modifier Rules for Profile & Combined Controls (Profile with Position, Orientation and Runout)

11 Chapter 11: Runout Tolerances & Comparative Control Analysis

11.1 Circular Runout vs. Total Runout Interpretation & Dial Indicator Verification 11.2 Comparative Analysis: Runout vs. Form, Orientation, & Concentricity Controls

6.1 Flatness & Straightness Controls for Surfaces & Features of Size

Key Takeaways Explain This Topic AI

Form tolerances (straightness, flatness, circularity, and cylindricity) are intrinsic geometric controls that NEVER reference datums; specifying a datum reference in any form feature control frame is an invalid syntax error.

Surface flatness and surface straightness refine the Rule #1 boundary and must specify a tolerance value smaller than the feature's size tolerance, operating without material condition modifiers.

When flatness or straightness is associated with a feature of size dimension (and preceded by ⌀ for cylindrical features), the control governs the derived median plane or derived median line, explicitly overriding Rule #1.

When applied to a feature of size at MMC (Ⓜ modifier), form controls permit bonus tolerance as the feature departs from MMC toward LMC, establishing a constant virtual condition boundary (MMC + tolerance for external features; MMC - tolerance for internal features).

Last updated: September 2026

6.1 Flatness & Straightness Controls for Surfaces & Features of Size

Quick Answer: In ASME Y14.5-2009 , form controls—comprising straightness , flatness , circularity , and cylindricity —are intrinsic geometric controls that never utilize datums . Placing a datum reference in a form feature control frame is an invalid syntax error. Surface flatness (Section 5.4.2) and surface straightness (Section 5.4.1) control physical surface elements, refine the Rule #1 envelope, must specify a tolerance smaller than the size tolerance, and strictly forbid material condition modifiers (Ⓜ or Ⓛ). In contrast, when flatness or straightness is associated with a feature of size (Sections 5.4.1.2 and 5.4.2.1), the control applies to the derived median plane (DMP) or derived median line (DML) , explicitly overrides Rule #1 , permits the Ⓜ modifier, generates bonus tolerance , and creates a fixed virtual condition boundary.

Fundamental Rules Governing Form Tolerances (ASME Y14.5-2009 Section 5)

Geometric dimensioning and tolerancing organizes geometric controls into five distinct families: form, orientation, profile, runout, and location. Form tolerances occupy the very base of this geometric hierarchy because form represents the intrinsic shape of an individual feature in isolation, completely decoupled from any external coordinate framework.

The Absolute Datum Prohibition Rule

The most fundamental rule governing all form tolerances under ASME Y14.5-2009 is: Form controls NEVER reference datums.

A datum establishes a reference relationship (location or orientation) between two or more features. Because form controls govern only the shape of a single feature relative to its own ideal geometry, referencing a datum is theoretically meaningless and constitutes a severe syntax error on an engineering drawing.

If a planar surface control references a datum (e.g., [ Flatness | 0.1 | A ] ), it is an invalid callout; the control should be specified as perpendicularity , parallelism , or angularity (orientation) or profile of a surface .

If a cylindrical axis control references a datum (e.g., [ Straightness | Ø 0.2 | A ] ), it is invalid; the control is properly specified as parallelism , perpendicularity , position , or runout .

Relationship to Rule #1 (Envelope Principle)

Under ASME Y14.5-2009 Section 2.7.1, Rule #1 dictates that where only a tolerance of size is specified, the limits of size of an individual feature of size prescribe the extent to which variations in its geometric form—as well as its size—are allowed. Rule #1 establishes two fundamental boundaries:

Perfect form at MMC : The surface or surfaces of a regular feature of size shall not extend beyond a boundary (envelope) of perfect form at maximum material condition (MMC). At MMC, zero form variation is permitted.

Form error allowed at LMC : As the actual local size of the feature departs from MMC toward least material condition (LMC), form variations (straightness, flatness, circularity, cylindricity) are permitted up to the maximum limit of the size tolerance.

Consequently, when a form control is applied to a surface , it serves strictly as a refinement of Rule #1 . For a surface form control to be meaningful, the specified form tolerance must be less than the total size tolerance . If a sheet metal plate has a thickness of 10.0 ± 0.4 mm 10.0 \pm 0.4\text{ mm} 10.0 ± 0.4 mm (total size tolerance of 0.8 mm 0.8\text{ mm} 0.8 mm ), specifying a surface flatness tolerance of 1.0 mm 1.0\text{ mm} 1.0 mm is redundant and technically incorrect because Rule #1 already limits the surface form variation to 0.8 mm 0.8\text{ mm} 0.8 mm . FORM CONTROL & RULE #1 RELATIONSHIPS

SURFACE FORM (Refines Rule #1) FEATURE OF SIZE FORM (Overrides Rule #1)
┌────────────────────────────────┐ ┌────────────────────────────────────────┐
│ • Controls physical surface │ │ • Controls derived median plane/line │
│ • Tolerance < Size Tolerance │ │ • Tolerance CAN exceed Size Tolerance │
│ • Perfect form at MMC upheld │ │ • Rule #1 perfect form at MMC WAIVED │
│ • Modifiers (Ⓜ/Ⓛ) FORBIDDEN │ │ • Modifiers (Ⓜ/Ⓛ) PERMITTED │
│ • Datums FORBIDDEN │ │ • Datums FORBIDDEN │
└────────────────────────────────┘ └────────────────────────────────────────┘
Surface Flatness (ASME Y14.5-2009 Section 5.4.2)

Flatness is the condition of a surface having all elements in one plane. When applied as a surface control, flatness ensures that a physical planar surface does not exhibit excessive waviness, bow, dish, or twist.

Tolerance Zone Definition

The tolerance zone for surface flatness is bounded by two parallel planes separated by the specified tolerance value t t t .

The tolerance planes are not constrained in location or orientation relative to any datum reference frame. They are free to float, translate, and tilt in 3D space to best contain the surface.

All extracted points of the actual surface must lie simultaneously between these two parallel planes.

Surface flatness is a 3D surface control (unlike surface straightness, which is 2D line-element-based).

Drawing Callout & Syntactical Placement

For surface flatness, the feature control frame is placed:

Attached to the surface via a leader line pointing directly to the physical surface.

Attached to an extension line extending from the surface, visibly offset and separated from any size dimension.

On a leader line pointing to the surface in an isometric or 3D view.

Because surface flatness applies to a physical surface (which has no size), material condition modifiers (Ⓜ or Ⓛ) are strictly prohibited . An MMC symbol inside a surface flatness frame is an invalid callout.

Flatness Applied to a Feature of Size (ASME Y14.5-2009 Section 5.4.2.1)

Section 5.4.2.1 of ASME Y14.5-2009 permits flatness to be applied to a regular feature of size consisting of two parallel opposed planar surfaces (such as a plate thickness, tab width, or slot width).

Placement & The Controlled Entity

When flatness is applied to a feature of size:

The feature control frame is placed directly associated with the size dimension (e.g., positioned directly beneath the size dimension or attached to the dimension line).

Controlled Entity : The control applies to the derived median plane (DMP) , NOT the physical surfaces! The derived median plane is the mathematically constructed mid-surface formed by the centers of all opposed line segments bounded by the actual surfaces.

Explicit Override of Rule #1

Applying flatness to a feature of size represents one of the official exceptions to Rule #1 . When specified:

The requirement of perfect form at MMC is completely waived . The derived median plane is permitted to bow, curl, or warp beyond the MMC envelope of the feature.

The individual opposed surfaces must still satisfy the cross-sectional actual local size limits at all locations.

The specified flatness tolerance can be greater than the size tolerance .

Material Condition Modifiers & Virtual Condition Calculations

Because a feature of size has measurable material mass, flatness of a feature of size may be specified Regardless of Feature Size (RFS) (the default per Rule #2) or with the Maximum Material Condition (Ⓜ) or Least Material Condition (Ⓛ) modifier.

When the Ⓜ modifier is applied:

The specified tolerance applies when the feature of size is produced at its Maximum Material Condition (MMC) .

As the actual mating size departs from MMC toward LMC, bonus tolerance is added directly to the flatness tolerance: Bonus Tolerance = ∣ Actual Mating Size − MMC ∣ \text{Bonus Tolerance} = |\text{Actual Mating Size} - \text{MMC}| Bonus Tolerance = ∣ Actual Mating Size − MMC ∣ Total Permissible Flatness = Specified Flatness + Bonus Tolerance \text{Total Permissible Flatness} = \text{Specified Flatness} + \text{Bonus Tolerance} Total Permissible Flatness = Specified Flatness + Bonus Tolerance

The control generates an unyielding worst-case outer boundary known as the Virtual Condition (VC) :

For an external feature of size (e.g., plate or tab thickness): V C external = MMC + Flatness Tolerance at MMC VC_{\text{external}} = \text{MMC} + \text{Flatness Tolerance at MMC} V C external = MMC + Flatness Tolerance at MMC

For an internal feature of size (e.g., slot or groove): V C internal = MMC − Flatness Tolerance at MMC VC_{\text{internal}} = \text{MMC} - \text{Flatness Tolerance at MMC} V C internal = MMC − Flatness Tolerance at MMC

Worked Calculation: Derived Median Plane Flatness at MMC

A mounting plate is dimensioned with a thickness of 12.00 ± 0.20 mm 12.00 \pm 0.20\text{ mm} 12.00 ± 0.20 mm (Limits: 11.80 − 12.20 mm 11.80 - 12.20\text{ mm} 11.80 − 12.20 mm ; MMC = 12.20 mm \text{MMC} = 12.20\text{ mm} MMC = 12.20 mm , LMC = 11.80 mm \text{LMC} = 11.80\text{ mm} LMC = 11.80 mm ). Directly under the thickness dimension, the feature control frame specifies [ Flatness | 0.15 Ⓜ ] .

Virtual Condition : V C = MMC + Flatness at MMC = 12.20 mm + 0.15 mm = 12.35 mm VC = \text{MMC} + \text{Flatness at MMC} = 12.20\text{ mm} + 0.15\text{ mm} = 12.35\text{ mm} V C = MMC + Flatness at MMC = 12.20 mm + 0.15 mm = 12.35 mm A functional receiver gage with two parallel plates spaced at 12.35 mm 12.35\text{ mm} 12.35 mm can accept the part.

If produced at MMC ( 12.20 mm 12.20\text{ mm} 12.20 mm ) : Bonus = 0 mm ⟹ Permissible DMP Flatness = 0.15 mm \text{Bonus} = 0\text{ mm} \implies \text{Permissible DMP Flatness} = 0.15\text{ mm} Bonus = 0 mm ⟹ Permissible DMP Flatness = 0.15 mm

If produced at an actual mating size of 12.05 mm 12.05\text{ mm} 12.05 mm : Bonus = 12.20 mm − 12.05 mm = 0.15 mm \text{Bonus} = 12.20\text{ mm} - 12.05\text{ mm} = 0.15\text{ mm} Bonus = 12.20 mm − 12.05 mm = 0.15 mm Total Permissible DMP Flatness = 0.15 mm + 0.15 mm = 0.30 mm \text{Total Permissible DMP Flatness} = 0.15\text{ mm} + 0.15\text{ mm} = 0.30\text{ mm} Total Permissible DMP Flatness = 0.15 mm + 0.15 mm = 0.30 mm

If produced at LMC ( 11.80 mm 11.80\text{ mm} 11.80 mm ) : Bonus = 12.20 mm − 11.80 mm = 0.40 mm \text{Bonus} = 12.20\text{ mm} - 11.80\text{ mm} = 0.40\text{ mm} Bonus = 12.20 mm − 11.80 mm = 0.40 mm Total Permissible DMP Flatness = 0.15 mm + 0.40 mm = 0.55 mm \text{Total Permissible DMP Flatness} = 0.15\text{ mm} + 0.40\text{ mm} = 0.55\text{ mm} Total Permissible DMP Flatness = 0.15 mm + 0.40 mm = 0.55 mm

Surface Straightness (ASME Y14.5-2009 Section 5.4.1)

Straightness is a condition where an element of a surface, or an axis, is a straight line. When applied to a surface, straightness controls individual longitudinal line elements.

Tolerance Zone Definition

The tolerance zone for surface straightness is a 2D zone bounded by two parallel lines separated by the specified tolerance value t t t .

The control is evaluated line element by line element independently . Each longitudinal line element must lie between its own pair of parallel lines.

Straightness does NOT control form from one line element to the next (waviness, dish, or twist across lines is not constrained by straightness; that requires flatness).

View Orientation Requirement : The feature control frame must be attached in the view where the controlled elements appear as a line (e.g., the side or elevation view of a cylinder or flat bar).

No Diameter Symbol : Because the tolerance zone consists of two parallel lines, the diameter symbol (⌀) is strictly prohibited .

No Modifiers : Like surface flatness, surface straightness refines Rule #1, applies to physical surface lines, and never permits datums or material condition modifiers (Ⓜ or Ⓛ) .

Straightness of a Feature of Size / Axis (ASME Y14.5-2009 Section 5.4.1.2)

When straightness is applied to a cylindrical feature of size (such as a pin, shaft, or hole):

Placement : The feature control frame is associated directly with the size dimension (placed under the dimension, attached to the dimension line, or attached to the leader).

Controlled Entity : It controls the derived median line (DML) of the feature (commonly referred to as axis straightness). The derived median line is formed by the centers of all cross-sectional discs taken perpendicular to the axis.

The Diameter Symbol (⌀) Requirement : Because the tolerance zone for a cylindrical feature is a cylindrical volume , the tolerance value in the feature control frame MUST be preceded by the diameter symbol (⌀) . Omitting ⌀ is a critical drawing error.

Rule #1 Override : Attaching straightness to a feature of size explicitly overrides Rule #1 perfect form at MMC. The pin or bore may bow beyond its MMC boundary.

Virtual Condition & Bonus Tolerance for Axis Straightness

Like feature-of-size flatness, axis straightness may be specified RFS or at MMC (Ⓜ). When specified with Ⓜ: Virtual Condition (External Pin) = MMC + Straightness Tolerance at MMC \text{Virtual Condition (External Pin)} = \text{MMC} + \text{Straightness Tolerance at MMC} Virtual Condition (External Pin) = MMC + Straightness Tolerance at MMC Virtual Condition (Internal Hole) = MMC − Straightness Tolerance at MMC \text{Virtual Condition (Internal Hole)} = \text{MMC} - \text{Straightness Tolerance at MMC} Virtual Condition (Internal Hole) = MMC − Straightness Tolerance at MMC Bonus Tolerance = ∣ Actual Local Size / Mating Size − MMC ∣ \text{Bonus Tolerance} = |\text{Actual Local Size / Mating Size} - \text{MMC}| Bonus Tolerance = ∣ Actual Local Size / Mating Size − MMC ∣ Total Permissible Axis Straightness = Specified Tolerance + Bonus \text{Total Permissible Axis Straightness} = \text{Specified Tolerance} + \text{Bonus} Total Permissible Axis Straightness = Specified Tolerance + Bonus

Worked Calculation: External Pin Axis Straightness

A shaft is dimensioned Ø20.00 ± 0.10 with [ Straightness | Ø 0.05 Ⓜ ] directly below the diameter callout.

MMC = ∅ 20.10 mm \text{MMC} = \varnothing 20.10\text{ mm} MMC = ∅ 20.10 mm ; LMC = ∅ 19.90 mm \text{LMC} = \varnothing 19.90\text{ mm} LMC = ∅ 19.90 mm .

Virtual condition: V C = 20.10 mm + 0.05 mm = ∅ 20.15 mm VC = 20.10\text{ mm} + 0.05\text{ mm} = \varnothing 20.15\text{ mm} V C = 20.10 mm + 0.05 mm = ∅ 20.15 mm .

If the shaft is manufactured at an actual mating size of ∅ 19.95 mm \varnothing 19.95\text{ mm} ∅ 19.95 mm :

Bonus = 20.10 mm − 19.95 mm = 0.15 mm \text{Bonus} = 20.10\text{ mm} - 19.95\text{ mm} = 0.15\text{ mm} Bonus = 20.10 mm − 19.95 mm = 0.15 mm .

Total Permissible Straightness = ∅ 0.05 mm + 0.15 mm = ∅ 0.20 mm \text{Total Permissible Straightness} = \varnothing 0.05\text{ mm} + 0.15\text{ mm} = \varnothing 0.20\text{ mm} Total Permissible Straightness = ∅ 0.05 mm + 0.15 mm = ∅ 0.20 mm .

The actual derived median line may have up to ∅ 0.20 mm \varnothing 0.20\text{ mm} ∅ 0.20 mm of bow, provided the mating envelope does not exceed the ∅ 20.15 mm \varnothing 20.15\text{ mm} ∅ 20.15 mm virtual condition boundary and local diameters remain between ∅ 19.90 \varnothing 19.90 ∅ 19.90 and ∅ 20.10 mm \varnothing 20.10\text{ mm} ∅ 20.10 mm .

Surface Form vs. Feature of Size Form: Master Comparison Table

Attribute / Parameter Surface Flatness (5.4.2) FOS Flatness (5.4.2.1) Surface Straightness (5.4.1) FOS Straightness (5.4.1.2)

Controlled Entity Physical surface points Derived Median Plane (DMP) Individual surface line elements Derived Median Line (DML)

Tolerance Zone Geometry Two parallel planes ( t t t ) Two parallel planes ( t t t ) Two parallel lines ( t t t ) Cylindrical zone (⌀ t t t )

Drawing Placement On surface or extension line Directly with size dimension On surface in line view Directly with size dimension

Diameter Symbol (⌀) Prohibited Prohibited Prohibited Mandatory (for cylinders)
Datum References Strictly Prohibited Strictly Prohibited Strictly Prohibited Strictly Prohibited

Material Condition (Ⓜ/Ⓛ) Strictly Prohibited Permitted (RFS default) Strictly Prohibited Permitted (RFS default)

Rule #1 Relationship Refines Rule #1 ( t < size tol t < \text{size tol} t < size tol ) Overrides Rule #1 ( t t t can exceed tol) Refines Rule #1 ( t < size tol t < \text{size tol} t < size tol ) Overrides Rule #1 ( t t t can exceed tol)

Virtual Condition Created? No (Inner/Outer bounds only) Yes : V C = MMC ± t VC = \text{MMC} \pm t V C = MMC ± t No Yes : V C = MMC ± t VC = \text{MMC} \pm t V C = MMC ± t

Bonus Tolerance Possible? No Yes (if Ⓜ or Ⓛ specified) No Yes (if Ⓜ or Ⓛ specified)
Common Exam Traps: Flatness & Straightness

Trap 1: The "Datum Reference" Syntax Error : A question presents an FCF such as [ Flatness | 0.05 | A ] or [ Straightness | Ø 0.1 | A | B ] . Examinees often analyze the numbers without noticing the callout is completely illegal. Form controls NEVER use datums.

Trap 2: Missing or Erroneous Diameter Symbol (⌀) : For surface straightness, adding a ⌀ symbol is an error (the zone is 2D parallel lines). For cylindrical feature-of-size straightness (axis straightness), omitting ⌀ is an error (the zone is a cylinder).

Trap 3: Assuming Surface Flatness Overrides Rule #1 : Surface flatness cannot allow a feature to violate its MMC envelope. Only flatness applied to a feature of size overrides Rule #1.

Trap 4: Incorrect Sign in Virtual Condition Formulas : For external features (pins/tabs), virtual condition is MMC + tolerance \text{MMC} + \text{tolerance} MMC + tolerance . For internal features (holes/slots), virtual condition is MMC − tolerance \text{MMC} - \text{tolerance} MMC − tolerance . Subtracting on external features or adding on internal features is a classic distractor.

Trap 5: Confusing Line Elements with Surface Extent : Surface straightness controls only individual line elements independently. A surface can pass surface straightness on every single element while being severely twisted or dished across its width.