Dimensioning, Fits and Geometric Tolerancing

Introduction

Engineering drawing is a language for communicating the geometry, size, function, and manufacturing requirements of a component. A drawing is not complete merely because its shape is recognizable. It must also state how large each feature may be, how accurately features must be located and oriented, and how parts are expected to assemble and operate. Dimensioning, fits, limits, and geometric dimensioning and tolerancing (GD&T) provide this information.

A dimension is a numerical statement of size or location. A tolerance defines the permitted variation in that dimension. A fit describes the relationship between mating features, usually a hole and a shaft. GD&T adds a symbolic system for controlling form, orientation, location, and runout in relation to theoretically exact references called datums.

The central design problem is balance. Excessively tight tolerances increase machining, inspection, and rejection costs. Excessively loose tolerances may produce leakage, vibration, misalignment, excessive wear, or assembly failure. Effective tolerancing therefore begins with function and proceeds through manufacturing and inspection considerations.

Learning Objectives

After studying this chapter, the student should be able to:

• distinguish size dimensions, location dimensions, limits, allowances, and tolerances;
• apply functional and manufacturing principles to dimensioning;
• calculate unilateral, bilateral, and limit tolerances;
• analyse tolerance accumulation in linear chains;
• select clearance, transition, and interference fits;
• use hole-basis and shaft-basis fit systems;
• interpret fundamental GD&T symbols, feature control frames, and datums;
• select datum references and geometric controls according to function;
• evaluate manufacturability, inspection capability, cost, and risk;
• prepare and assess a toleranced engineering drawing.

1. Functional Dimensioning

1.1 Dimensions as design requirements

A dimension may specify:

1. Feature size, such as a hole diameter, shaft diameter, slot width, or plate thickness.
2. Feature location, such as the distance between hole centres.
3. Feature orientation, such as an angle or a perpendicular relationship.
4. Geometric form, such as flatness or straightness.
5. Surface relationship, such as concentricity-related runout or parallelism.

Dimensions should communicate the design intent rather than simply describe how the designer happened to construct the model. A dimension is functional when its value and tolerance are derived from the way the component operates, assembles, or interfaces with another component.

For example, the position of a bearing seat is functionally important because it determines shaft alignment. A cosmetic external radius may be less critical and may receive a comparatively broad tolerance.

1.2 Dimensioning principles

Good dimensioning follows several principles:

• Dimension from functional surfaces or axes whenever possible.
• Avoid dimensioning from features that are themselves poorly controlled.
• Place each dimension where its meaning is unambiguous.
• Avoid unnecessary repetition of the same dimension.
• Do not use a dimension that can be obtained by adding or subtracting other dimensions unless it is functionally required.
• Give tolerances on all dimensions, either individually or through a stated general tolerance.
• Use basic dimensions for theoretically exact locations when a geometric tolerance controls the variation.
• Do not use the drawing to imply greater accuracy than the process or inspection method can support.

A dimensioning scheme based on a chain of unrelated dimensions can create accumulated error. A baseline scheme, in which several features are located from one functional datum, often gives better control and simpler inspection.

1.3 Size dimensions and location dimensions

A size dimension describes the magnitude of a feature. Examples include ⌀25 mm, 12 mm thickness, and R6 mm. A location dimension identifies where a feature is placed relative to another feature or datum. For a hole pattern, the hole diameter is a size dimension, while the coordinates of its centre are location dimensions.

The drawing should distinguish dimensions that control assembly from those that merely assist manufacturing. A manufacturing dimension may be replaced by a direct functional dimension if this reduces ambiguity.

1.4 General tolerances

When many dimensions have similar manufacturing requirements, a drawing may state a general tolerance, such as “Unless otherwise specified, ±0.1 mm.” This reduces clutter, but it must be appropriate for the manufacturing process. General tolerances should not be used to conceal critical requirements. Important interfaces, sealing surfaces, bearing seats, and locating features normally require individually specified tolerances.

2. Limits, Tolerance, and Allowance

2.1 Basic definitions

The basic size is the theoretical size from which limits are derived. The upper limit is the maximum permitted size, and the lower limit is the minimum permitted size. The tolerance is the total permitted variation.

where T is tolerance, U is the upper limit, and L is the lower limit. All three quantities must have the same units. The formula applies to both internal and external features.

For a shaft specified as 24.98–25.00 mm:

The shaft tolerance is therefore 0.02 mm.

A unilateral tolerance varies in one direction from the nominal size, for example 25.00 +0.02/−0.00 mm. A bilateral tolerance allows variation in both directions, for example 25.00 ±0.02 mm. A limit dimension directly states the permitted maximum and minimum sizes.

The allowance is the intentional minimum clearance or maximum interference between mating parts. Unlike tolerance, which describes variation in one feature, allowance describes the relationship between two mating features.

2.2 Hole and shaft terminology

For a hole and shaft assembly:

• Maximum clearance = maximum hole size − minimum shaft size.
• Minimum clearance = minimum hole size − maximum shaft size.
• Maximum interference = maximum shaft size − minimum hole size.
• Minimum interference = minimum shaft size − maximum hole size.

A clearance fit has clearance in every permissible condition. An interference fit has interference in every permissible condition. A transition fit may produce either small clearance or small interference, depending on actual sizes.

2.3 Tolerance zones

In a limit system, a tolerance zone is the interval between the upper and lower limits. Its position relative to the basic size determines whether the tolerance is unilateral, bilateral, or offset. For a shaft, the tolerance zone may lie below, above, or across the basic size. For a hole, the same principle applies.

The terms “hole” and “shaft” refer to internal and external features respectively; they do not imply that the component must literally be cylindrical. The system can be extended to slots, tabs, and other mating features.

3. Fits and Fit Systems

3.1 Functional selection of a fit

Fit selection should begin with the operating requirement:

• Clearance fit: parts must assemble freely, permit sliding, or allow lubrication.
• Transition fit: accurate location is required, but occasional assembly and disassembly may be necessary.
• Interference fit: torque or force must be transmitted, or relative movement must be prevented.

Other considerations include temperature, materials, surface finish, lubrication, assembly force, service loading, corrosion, and repair requirements. Thermal expansion can change a fit substantially. If a steel shaft and housing operate at different temperatures, the clearance may increase or decrease according to their coefficients of thermal expansion.

3.2 Hole-basis and shaft-basis systems

In the hole-basis system, the hole is held at a standard tolerance position and different shaft tolerances are selected to obtain the required fit. The common reference is an H hole, whose lower deviation is zero in the ISO system.

In the shaft-basis system, the shaft is held at a standard position and different hole tolerances are selected. This is useful when a shaft is produced by a fixed process, such as a standard ground bar, or when several components must fit one common shaft.

The hole-basis system is widely used because drills, reamers, and boring tools often make it economical to standardize hole sizes while varying shaft dimensions.

3.3 ISO fit notation

ISO fit notation combines a letter and a grade, for example H7, h6, or H7/g6. The letter identifies the position of the tolerance zone relative to the basic size; the grade identifies the tolerance magnitude. Uppercase letters conventionally denote holes and lowercase letters denote shafts.

The numerical grade is related to a standard tolerance unit. In the ISO system, the standard tolerance unit i, in micrometres, is commonly represented for a nominal size range by:

where D is the geometric mean of the nominal size range in millimetres and i is in micrometres. This relationship is used within the ISO system’s specified size ranges; it is not a universal manufacturing law. Standard tolerance grades are multiples of this unit according to the applicable standard.

A complete fit should be selected from the current applicable standard rather than calculated from memory. Standard tables account for size ranges, fundamental deviations, and grade values.

3.4 Worked fit example

An assembly uses a hole with limits 25.000–25.021 mm and a shaft with limits 24.980–24.993 mm.

Maximum clearance occurs with the largest hole and smallest shaft:

Minimum clearance occurs with the smallest hole and largest shaft:

Since both clearances are positive, the assembly is a clearance fit. The clearance allowance, or minimum clearance, is 0.007 mm, and the total clearance variation is 0.034 mm.

4. Tolerance Accumulation

4.1 Linear tolerance chains

Tolerance accumulation occurs when several dimensions contribute to a final functional dimension. A chain may be analysed by the worst-case method or by a statistical method.

For a simple additive chain, the worst-case resultant tolerance is:

where T_i is the tolerance magnitude of each contributing dimension. The absolute values are used because worst-case variation assumes that every dimension simultaneously deviates in the direction that produces the largest result.

If a closing dimension is calculated as a sum and difference of dimensions, nominal values are added algebraically, while tolerance magnitudes are added for the worst-case limit.

4.2 Worked tolerance-chain example

Three dimensions locate a shoulder: A = 40 ±0.10 mm, B = 25 ±0.05 mm, and C = 15 ±0.05 mm. Suppose the closing dimension is:

Nominally:

The worst-case tolerance is:

Therefore, X may range from −0.20 mm to +0.20 mm. The result reveals a design concern: a nominal zero closing dimension with a possible negative or positive gap is unlikely to be functionally acceptable. The designer should revise the datum structure, redistribute tolerances, or define the functional gap directly.

4.3 Worst-case and statistical methods

The worst-case method guarantees assembly if every component lies within its specified limits, but it may produce unnecessarily tight individual tolerances. A statistical method considers the distribution of actual variation. If independent, centred, random variations are reasonably represented by standard deviations σ_i, the root-sum-square estimate is:

This formula assumes independence and random variation. It does not guarantee that all assemblies will meet the requirement, and it is inappropriate when variations are correlated, distributions are strongly non-normal, or process centring is not controlled. Statistical tolerancing must therefore be supported by process data and an explicitly accepted risk level.

4.4 Improving tolerance chains

Tolerance accumulation can be reduced by:

• dimensioning from a common functional datum;
• eliminating unnecessary intermediate dimensions;
• using locating features rather than relying on accumulated edge distances;
• tightening only dimensions that affect the function;
• redesigning the assembly to absorb variation;
• using adjustable, compliant, or self-aligning features;
• applying GD&T with datum references instead of independent coordinate tolerances.

5. Geometric Dimensioning and Tolerancing

5.1 Purpose and scope

GD&T controls the allowable variation of geometry. It separates size requirements from geometric requirements and provides a consistent relationship between features and datums. A feature may have the correct size but still be unacceptable because it is tilted, displaced, bowed, or out of position.

The main control groups are:

Terminology and symbols should follow the governing standard adopted by the organization, such as ASME Y14.5 or ISO 1101. These standards are related but not identical; a drawing must identify the applicable interpretation where ambiguity is possible.

5.2 Datums and datum reference frames

A datum is a theoretically exact reference. A physical datum feature is the actual surface or feature used to establish that reference during manufacture or inspection. A datum reference frame commonly consists of:

• a primary datum that constrains the greatest number of degrees of freedom;
• a secondary datum that constrains additional motion;
• a tertiary datum that completes orientation and location.

The familiar three-two-one locating principle illustrates this arrangement: a primary plane can establish three contact constraints, a secondary plane two, and a tertiary plane one. The actual number and nature of contacts depend on the feature geometry and standard interpretation.

Datum selection should reflect assembly function. The primary datum is often the surface that rests on a mating component or establishes the principal orientation. The secondary datum may locate a side or axis, and the tertiary datum may establish clocking or a final coordinate direction.

A datum should also be stable, accessible, manufacturable, inspectable, and representative of how the component is used. Selecting a convenient but functionally irrelevant edge can create misleading inspection results.

5.3 Form controls

Form controls generally do not require a datum.

• Straightness limits how much a line element or derived median line may deviate from a perfect straight line.
• Flatness limits a surface to a zone between two parallel planes.
• Circularity limits each circular element to a zone between two concentric circles.
• Cylindricity controls the entire cylindrical surface within two coaxial cylinders.

Form tolerances are especially useful when a surface must seal, slide, or support a bearing. Size alone does not guarantee form. For example, a cylindrical shaft can remain within diameter limits while being slightly bowed.

5.4 Orientation controls

Orientation controls require a datum because orientation is meaningful only relative to a reference.

• Parallelism controls the orientation of a surface, line, or feature relative to a datum.
• Perpendicularity controls a 90° relationship.
• Angularity controls an orientation at a specified basic angle other than 0° or 90°.

Orientation controls do not, by themselves, establish the exact location of a feature. A hole may be perpendicular to a surface but still be displaced from its intended position. Location controls or dimensions are then needed.

5.5 Position tolerance

The position control is one of the most useful GD&T controls for holes and patterns. A basic dimension defines the theoretically exact location, while the feature control frame defines the permissible positional zone.

For a cylindrical feature, a position tolerance often creates a cylindrical tolerance zone around the true position. If a hole has a position tolerance of ⌀0.20 mm, its axis must lie within a cylinder of diameter 0.20 mm centred on the true position, subject to the applicable modifiers and datum references.

The radial displacement corresponding to a diametral position tolerance is half the stated diameter. Thus, ⌀0.20 mm permits a maximum radial axis displacement of 0.10 mm when evaluated at the stated condition.

5.6 MMC, LMC, and bonus tolerance

The maximum material condition (MMC) is the condition in which a feature contains the greatest amount of material. For a shaft, MMC is the largest permitted diameter. For a hole, MMC is the smallest permitted diameter. The least material condition (LMC) is the opposite limit.

When a geometric tolerance is specified with the MMC modifier, permissible geometric variation may increase as the feature departs from MMC. The additional amount is called bonus tolerance. For a hole, if the MMC size is 10.00 mm, the actual hole is 10.15 mm, and the position tolerance at MMC is ⌀0.20 mm, the available bonus tolerance is 0.15 mm, giving a total positional tolerance of:

This relationship assumes the MMC modifier is explicitly specified and that the feature and datum rules of the governing standard apply. MMC is valuable for functional gaging because it protects assembly at the virtual condition while allowing economical size variation.

5.7 Profile controls

Profile controls regulate a line or surface relative to a theoretically exact profile. They can control form, orientation, and location simultaneously. Profile is particularly useful for contoured castings, aerodynamic surfaces, sealing profiles, and complex moulded parts.

A profile tolerance may be unequal about the true profile if the standard and drawing specify an appropriate offset. The designer must state the intended relationship clearly; otherwise inspection interpretation may differ.

5.8 Runout controls

Circular runout controls variation at individual circular sections as a part rotates about a datum axis. Total runout controls the cumulative variation over the entire surface as the part rotates. Runout is useful for rotating shafts, bearing seats, brake discs, and pulley surfaces.

Runout can simultaneously reflect errors of form, orientation, and coaxial relationship. It should not be used merely as a substitute for a required position or cylindricity control; the selected control should correspond to the actual functional requirement.

6. Dimensioning, Manufacturability, and Inspection

Tolerance design is a cross-functional activity. Designers, manufacturing engineers, quality engineers, toolmakers, and inspectors should agree on critical characteristics before release.

6.1 Process capability

A process should not routinely be assigned a tolerance narrower than it can economically produce. Capability indices are often used to compare process variation with specification limits. For a stable, approximately normal process:

and, accounting for process centring:

USL and LSL are the upper and lower specification limits, μ is the process mean, and σ is the process standard deviation. These indices are meaningful only when the process is stable and the data and assumptions are appropriate. A high index does not prove that the process is stable or that the measurement system is adequate.

6.2 Measurement and inspection

Every tolerance must be measurable. A coordinate measuring machine may be appropriate for complex profiles, while a plug gauge, ring gauge, micrometer, bore gauge, or functional fixture may be faster and less costly for production inspection.

Measurement uncertainty should be small relative to the tolerance being assessed. Gauge repeatability and reproducibility studies help determine whether variation comes from the part or from the measurement system. Inspection fixtures should reproduce the datum reference frame and loading conditions specified by the drawing.

6.3 Cost and risk

Tighter tolerances can require precision machinery, additional operations, temperature-controlled inspection, special tooling, and greater scrap control. The correct question is not “What is the smallest tolerance possible?” but “What tolerance is necessary for function, safety, interchangeability, and life?”

Safety-critical characteristics may require traceability, documented approval, validated processes, and regulatory compliance. Drawings should identify critical, key, or special characteristics according to the organization’s quality system. A tolerance must never be relaxed without evaluating its effect on safety and performance.

7. Worked Application: Pump Shaft and Bearing Housing

The following is an illustrative case.

Background

A small centrifugal pump uses a rotating steel shaft supported by a bearing installed in an aluminium housing. The shaft must rotate freely, maintain alignment, and transmit torque through a separate keyed coupling. The bearing outer ring must be securely located in the housing, while replacement during maintenance should remain possible.

Problem

An initial drawing specified only nominal diameters: 25 mm for the shaft seat and 52 mm for the housing bore. Production reported variable noise, occasional bearing creep, and difficult assembly. Inspection also showed that the bearing seat location varied relative to the mounting face.

Analysis

The nominal dimensions did not define the required fits. The shaft-bearing interface required a controlled transition or light interference condition according to bearing and loading requirements. The housing-bearing interface required a controlled fit that prevented outer-ring rotation but permitted service removal. In addition, the shaft seat needed adequate cylindricity and runout relative to the bearing journal axis.

The mounting face was selected as the primary datum because it seats against the pump casing. A radial locating surface was selected as the secondary datum, and a keying or clocking feature was selected as the tertiary datum. This datum reference frame represented assembly conditions more accurately than an arbitrary outside edge.

Approach and solution

The designer first obtained the bearing manufacturer’s recommended seat limits and selected an appropriate standard fit rather than inventing a new tolerance. The shaft journal and housing bore were then specified using standardized fit notation and explicit material and temperature assumptions.

The shaft drawing included:

• a size tolerance for the bearing journal;
• a cylindricity control for the journal surface;
• a runout control relative to the shaft datum axis for adjacent rotating features;
• a surface-finish requirement suitable for the bearing seat;
• a datum axis established from the functional journal.

The housing drawing included:

• the bearing-bore fit;
• perpendicularity of the bore axis to the mounting datum surface;
• position or profile control for mounting holes relative to the datum reference frame;
• a controlled shoulder location to establish bearing axial position.

A tolerance-chain review confirmed that the bearing shoulder, housing shoulder, and casing interface could not accumulate enough variation to preload the bearing excessively. Inspection was planned with a bore gauge and functional datum fixture for the housing, and a roundness/runout instrument for the shaft.

Outcome

The revised design separated size, form, orientation, and location requirements. Assembly became repeatable, bearing creep was eliminated within the intended operating conditions, and inspection personnel could reproduce the drawing’s datum scheme. Some nonfunctional external dimensions were assigned broader general tolerances, reducing machining cost without reducing pump performance.

Learning points

1. Nominal dimensions alone do not define a functional assembly.
2. Fit selection must consider load, temperature, material, lubrication, and maintenance.
3. Datums should represent assembly and inspection conditions.
4. Form and runout may be as important as diameter for rotating components.
5. A tolerance that cannot be inspected consistently is an incomplete requirement.

8. Best Practices and Common Errors

Best practices

• Start with functional requirements and failure modes.
• Identify interfaces, locating surfaces, and replaceable components.
• Use standard fits and tolerance grades where possible.
• Apply the least restrictive tolerance that satisfies function.
• Use basic dimensions with GD&T for theoretically exact locations.
• Select datums according to assembly sequence and inspection setup.
• Check tolerance chains before releasing the drawing.
• Confirm that manufacturing and inspection equipment can achieve the requirements.
• State the governing GD&T standard and units.
• Review critical characteristics with manufacturing and quality personnel.

Common errors

• Repeating dimensions that can conflict with one another.
• Dimensioning from an irrelevant edge instead of a functional datum.
• Applying tight size tolerances when a geometric control is the actual need.
• Using concentricity or symmetry when position or runout better describes function.
• Omitting a tolerance from a critical dimension.
• Treating a general tolerance as suitable for every feature.
• Assuming that MMC bonus tolerance exists when no MMC modifier is shown.
• Using statistical tolerancing without evidence of stable, independent processes.
• Ignoring thermal expansion and assembly temperature.
• Specifying precision beyond the capability of the measurement system.

9. Contemporary Developments

Model-based definition and digital product-definition systems increasingly place dimensions, tolerances, datum structures, and inspection characteristics directly in three-dimensional CAD models. This can reduce drawing ambiguity, but only when annotations follow a controlled standard and manufacturing systems interpret them consistently.

Digital inspection systems can automatically compare measured point clouds with nominal geometry. Artificial intelligence may assist in identifying abnormal process trends, optimizing tolerance allocation, or detecting recurring inspection patterns. Such tools do not replace engineering judgement: training data, measurement uncertainty, traceability, cybersecurity, and human approval remain necessary.

Additive manufacturing creates additional challenges because anisotropy, support removal, thermal distortion, and surface roughness may vary by build orientation. Tolerances should therefore be linked to a validated process capability rather than copied from conventional machining practice.

Chapter Summary

Dimensioning communicates size, location, and functional intent. Limits define maximum and minimum permissible sizes; tolerance is the difference between those limits, while allowance describes the intended relationship between mating features. Clearance, transition, and interference fits are selected from functional requirements and may be organized through hole-basis or shaft-basis systems.

Tolerance accumulation must be evaluated, especially in linear chains. Worst-case analysis adds individual tolerance magnitudes and provides a limit guarantee; statistical analysis can be less conservative but requires valid assumptions and process evidence. GD&T controls form, orientation, location, profile, and runout in relation to functional datums. Position, MMC, bonus tolerance, and datum reference frames are particularly important for interchangeable manufactured parts.

Good tolerancing balances function, manufacturability, inspection capability, cost, safety, and lifecycle requirements. The best drawing is not the one with the smallest tolerances, but the one that communicates necessary requirements precisely and economically.

Key Terms

Basic size: The theoretical size from which limits are derived.

Upper limit: The maximum permitted size of a feature.

Lower limit: The minimum permitted size of a feature.

Tolerance: The total permitted variation between upper and lower limits.

Allowance: The intentional minimum clearance or maximum interference between mating features.

Clearance fit: A fit having positive clearance in all permissible conditions.

Transition fit: A fit that may produce either small clearance or small interference.

Interference fit: A fit having interference in all permissible conditions.

Hole-basis system: A fit system in which the hole tolerance position is held as the reference.

Shaft-basis system: A fit system in which the shaft tolerance position is held as the reference.

Datum: A theoretically exact reference used to establish relationships and measurements.

Datum feature: An actual physical feature used to establish a datum.

Feature control frame: A symbolic GD&T indication stating a geometric characteristic, tolerance, and datum references.

Form control: A control of shape that generally does not require a datum.

Position tolerance: A control defining the allowable location of a feature relative to true position.

MMC: Maximum material condition, representing the condition with the greatest amount of material.

Bonus tolerance: Additional geometric tolerance permitted as a feature departs from MMC.

Runout: Variation of a surface during rotation about a datum axis.

Tolerance chain: A sequence of dimensions whose variations affect a resultant functional dimension.

Process capability: The ability of a stable process to produce output within specified limits.

Review Questions

Short Answer Questions

1. Define tolerance and allowance, and distinguish between them.
2. What is the difference between a clearance fit and an interference fit?
3. Why are datums important in GD&T?
4. State the purpose of a position tolerance.
5. What is bonus tolerance under an MMC requirement?

Long Answer Questions

1. Explain the principles of functional dimensioning and discuss how they reduce manufacturing and assembly problems.
2. Compare hole-basis and shaft-basis systems, including situations in which each may be preferred.
3. Explain form, orientation, location, profile, and runout controls with suitable engineering examples.
4. Discuss worst-case and statistical tolerance accumulation, including the assumptions and limitations of each method.
5. Describe a systematic method for selecting datums and tolerances for a machined housing.

Analytical / Application Questions

1. A hole is 30.000–30.025 mm and a shaft is 29.980–29.995 mm. Calculate the maximum and minimum clearance and identify the fit.
2. A closing dimension is affected by three independent dimensions with tolerances of ±0.08 mm, ±0.05 mm, and ±0.03 mm. Determine the worst-case tolerance and explain one design method for reducing it.
3. A hole has a position tolerance of ⌀0.20 mm at MMC. Its MMC size is 12.00 mm, and its measured size is 12.12 mm. Calculate the available total position tolerance and explain the functional benefit of the MMC modifier.

Multiple Choice Questions with Answers

Question 1

A hole has limits of 25.000 mm and 25.021 mm. What is its tolerance?

A. 0.002 mm

B. 0.021 mm

C. 0.041 mm

D. 25.021 mm

Correct Answer: B. 0.021 mm

Question 2

A hole is 25.000–25.021 mm and a shaft is 24.980–24.993 mm. What is the minimum clearance?

A. 0.007 mm

B. 0.013 mm

C. 0.028 mm

D. 0.041 mm

Correct Answer: A. 0.007 mm

Question 3

Which fit provides positive clearance in every permissible condition?

A. Interference fit

B. Transition fit

C. Clearance fit

D. Press fit only

Correct Answer: C. Clearance fit

Question 4

In a hole-basis system, which feature is normally held at the standard reference position?

A. The hole

B. The shaft

C. The datum surface

D. The surface finish

Correct Answer: A. The hole

Question 5

For dimensions with tolerances of ±0.10 mm, ±0.05 mm, and ±0.05 mm, what is the worst-case accumulated tolerance?

A. ±0.05 mm

B. ±0.10 mm

C. ±0.15 mm

D. ±0.20 mm

Correct Answer: D. ±0.20 mm

Question 6

Which GD&T control primarily specifies the allowable location of a hole axis relative to true position?

A. Flatness

B. Position

C. Circularity

D. Parallelism

Correct Answer: B. Position

Question 7

Which control generally does not require a datum?

A. Perpendicularity

B. Position

C. Flatness

D. Runout

Correct Answer: C. Flatness

Question 8

For a hole, maximum material condition is its:

A. Largest permitted diameter

B. Smallest permitted diameter

C. Average measured diameter

D. Basic diameter plus position tolerance

Correct Answer: B. Smallest permitted diameter

Question 9

A hole has a position tolerance of ⌀0.20 mm at MMC. Its MMC size is 10.00 mm and actual size is 10.15 mm. What is the total available position tolerance?

A. ⌀0.05 mm

B. ⌀0.20 mm

C. ⌀0.35 mm

D. ⌀0.50 mm

Correct Answer: C. ⌀0.35 mm

Question 10

Which datum should normally be selected as primary for a component surface that seats against the mating assembly?

A. A random outside edge

B. The functional seating surface

C. The surface with the largest area only

D. The least accessible surface

Correct Answer: B. The functional seating surface