8.4 Zero Positional and Orientation Tolerancing at MMC and at LMC

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

8.4 Zero Positional and Orientation Tolerancing at MMC and at LMC

Key Takeaways Explain This Topic AI

ASME Y14.5-2009 para. 2.8.3 makes a zero tolerance at MMC totally dependent on the unrelated actual mating envelope: at the MMC limit of size no position or orientation tolerance is allowed and the feature must be at true position or perfect in orientation.

Converting to zero at MMC moves the geometric tolerance into the size tolerance, so the MMC size becomes the former virtual condition and the functional gage pin diameter is unchanged.

Zero tolerancing accepts parts that a conventional callout would reject for undersize, because any hole whose mating envelope clears the virtual condition boundary is now within the size limits.

Para. 2.8.5 mirrors the concept at LMC, where the tolerance depends on the actual minimum material envelope and the feature must be at true position when produced at its LMC limit.

Zero tolerancing is appropriate only where assembly clearance is the sole functional requirement, because it greatly enlarges the stated size range while the LMC limit must still be set for function.

Last updated: September 2026

8.4 Zero Positional and Orientation Tolerancing at MMC and at LMC

Quick Answer: Para. 2.8.3 defines the effect of zero tolerance at MMC : the tolerance becomes totally dependent on the size of the unrelated actual mating envelope of the considered feature. No tolerance of position or orientation is allowed if the feature is produced at its MMC limit of size — at MMC it must be located at true position, or be perfect in orientation , as applicable. Para. 2.8.5 gives the mirror image for zero tolerance at LMC , where the tolerance depends on the actual minimum material envelope . The design payoff is that zero tolerancing converts unusable size tolerance into usable position tolerance without changing the virtual condition, which is why it is the standard treatment for clearance holes whose only requirement is assembly.

The Problem Zero Tolerancing Solves

Consider a clearance hole for an M8 fastener, sized ⌀8.40 – ⌀8.70 with ⌖ | ⌀0.4 Ⓜ | A | B | C .

MMC = ⌀8.40, so the virtual condition is 8.40 − 0.40 = ∅ 8.00 8.40 - 0.40 = \varnothing 8.00 8.40 − 0.40 = ∅ 8.00 .

A hole produced at ⌀8.50 earns 0.10 bonus and may be off position by ⌀0.50.

But now imagine a hole produced at ⌀8.35 — undersize. It is rejected for size , even though its actual mating boundary might sit perfectly at ⌀8.00 and the fastener would assemble without complaint.

The size limit is doing work the function never asked for. Zero tolerancing removes that artificial rejection.

The Zero-at-MMC Conversion

Where a tolerance of position or orientation is applied on a zero tolerance at MMC basis, the tolerance is totally dependent on the size of the unrelated actual mating envelope of the considered feature. No tolerance of position or orientation is allowed if the feature is produced at its MMC limit of size; and in this case, it must be located at true position or be perfect in orientation, as applicable. (Para. 2.8.3)

The conversion is mechanical. Move the geometric tolerance into the size tolerance so the virtual condition is unchanged:

Conventional Zero at MMC
Size ⌀8.40 – ⌀8.70 ⌀8.00 – ⌀8.70
Position ⌖ ⌀0.4 Ⓜ A B C ⌖ ⌀0 Ⓜ A B C
MMC ⌀8.40 ⌀8.00
Virtual condition 8.40 − 0.40 = ⌀8.00 8.00 − 0 = ⌀8.00
Functional gage pin ⌀8.00 ⌀8.00 — identical
Hole at ⌀8.40 0 bonus → ⌀0.4 total 0.40 bonus → ⌀0.40 total
Hole at ⌀8.70 0.30 bonus → ⌀0.7 total 0.70 bonus → ⌀0.70 total

Hole at ⌀8.20 REJECTED for size ACCEPTED , 0.20 bonus → ⌀0.20 total ZERO TOLERANCE AT MMC — TOTAL TOLERANCE vs. SIZE

total position tol
⌀0.70 ┤ ● (hole at 8.70)
│ ●
⌀0.40 ┤ ● (8.40)
│ ●
⌀0.20 ┤ ● (8.20)
│ ●
⌀0.00 ┤ ● (8.00 = MMC: must be at TRUE POSITION)
└──┬─────┬──────┬────────┬────────┬────────┬──► actual mating size
8.00 8.20 8.40 8.55 8.70

Every point on that line has the same inner boundary of ⌀8.00 . The gage never changes; only the accept/reject decision at the small end of the size range does.

The Trade the Exam Tests

Zero tolerancing is not free. It transfers the entire burden onto the size dimension :

At exactly MMC the hole must be perfectly located — an impossible manufacturing target, so in practice the shop must run the process away from MMC .

The size tolerance appears enormous (⌀8.00 – ⌀8.70), which can alarm a reviewer who does not read the feature control frame.

It is appropriate only where assembly clearance is the sole requirement . If minimum edge distance, wall thickness, or a bearing fit also matters, the enlarged size range is dangerous — the ⌀8.70 end is still governed by the LMC limit, so the designer must set that limit for function, not for convenience.

Zero Tolerance at LMC (Para. 2.8.5)

Where a tolerance of position or orientation is applied on a zero tolerance at LMC basis, the tolerance is totally dependent on the size of the actual minimum material envelope of the considered feature. No tolerance of position or orientation is allowed if the feature is produced at its LMC limit of size; and in this case, it must be located at true position or be perfect in orientation, as applicable.

Same mechanism, opposite direction. Zero at LMC protects minimum wall thickness or minimum stock : at LMC the feature is at its worst case for material, so it must be perfectly located; as the feature moves toward MMC, material is regained and tolerance is released.

Zero Orientation Tolerance at MMC (Para. 6.4.4)

The orientation section carries its own application of the same idea. Para. 6.4.4, Application of Zero Tolerance at MMC , applies zero perpendicularity, parallelism, or angularity at MMC to a feature of size — most commonly a perpendicularity refinement on a hole already located by position . The interpretation matches para. 2.8.3: at MMC the feature must be perfect in orientation , and tolerance accrues only as the feature departs from MMC.

Application Paragraph Depends On At the Stated Limit
Zero position or orientation at MMC 2.8.3 Unrelated actual mating envelope True position / perfect orientation
Zero position or orientation at LMC 2.8.5 Actual minimum material envelope True position / perfect orientation
Zero orientation at MMC on a FOS 6.4.4 Unrelated actual mating envelope Perfect orientation

Zero position at MMC for symmetry 7.7.1.1 Unrelated actual mating envelope Symmetrical boundaries of perfect form

Trap: candidates read ⌖ | ⌀0 Ⓜ | A | B | C and conclude the drawing demands perfection. It does not. It demands perfection only at MMC , a size the process is expected never to produce. The real requirement is the virtual condition boundary , which is exactly the MMC size itself.