All parts and features have some variation from ideal size, and this variation is controlled by the designer through the application of dimensional tolerances. The system of limits and fits allows the designer to quickly tolerance parts that fit together with a predetermined clearance or interference. Limits of size refer to the two tolerances or deviations applied to a dimension that set the upper and lower limits for that dimension. These tolerances are meant to be applied to nominal parts that were designed ‘line to line’ (without clearance when nominal size) in assemblies. The standards governing limits and fits are specific to cylindrical features and parts (holes and shafts), but these fits can also be applied to non-cylindrical features and parts like rectangular slides and pockets. When selecting fits, one must consider the loading, speed, length of engagement, temperature, and lubrication conditions of the assembly. The designer is free to use the standard fits or specify different tolerance combinations to achieve the desired result.

RECOMMENDED RESOURCES

•Oberg, Jones, Horton, Ryffel, Machinery’s Handbook, 28th Ed., Industrial Press, New York, NY, 2008

•ANSI B4.1: “Preferred Limits and Fits for Cylindrical Parts”

•ISO 286: “ISO System of Limits and Fits”

TYPES OF FITS AND THEIR LIMITS

Fits refer to the amount of clearance or interference between mating parts. There are three basic types of fits: clearance fits, transition fits (chance of either clearance or interference), and interference fits. Each fit specifies two sets of tolerances, or limits of size: one for the hole or external feature, and one for the shaft or internal feature. These tolerances are applied to the nominal feature size when parts are designed ‘line to line’ (without clearance at nominal size), and can be either positive or negative. Tolerance designations are represented by a class letter followed by a tolerance grade number. The hole or internal feature’s tolerance class is represented by a capital letter, and the shaft or external feature’s tolerance class is represented by a lowercase letter. The larger the grade number, the wider the tolerance range. On part drawings, tolerances are given using the class letter and grade number designation, the numerical tolerances themselves, or both. For example, a hole and pin are designed nominally ‘line to line’ and the designer wishes to apply a press fit to the joint. The pin is a commercial item with an m6 tolerance. The designer would then need to find out what tolerance designation to apply to the hole. This will be solved in the next few paragraphs.

ANSI B4.1 governs preferred limits and fits in inch units. The ANSI system uses descriptive two-letter designations to represent fits. Each type of ANSI fit has a series of possible grades, each represented by a number. The grade indicates the degree of tightness of the fit. ANSI fit grades are not the same as tolerance grades. A graphical representation of the ANSI standard fits is shown in Figure 3-1. ISO 286 governs preferred limits and fits in metric units. The ISO system of fits specifies preferred tolerance combinations for each fit type. Table 3-1 lists some commonly used fits, their typical use, and their graded tolerance designations from both the ANSI and ISO standards. Revisiting the example with the m6 tolerance pin, it can be seen from Table 3-1 that a locational interference fit joint can have a tolerance combination of H7/p6. Because the pin has an m6 tolerance rather than the standard p6, some calculation will be required to adjust the tolerances. That will be discussed further in the next paragraph.

Figure 3-1: Graphical Representation of ANSI Standard Fits

Tolerance grades, or limits of size, are graduated based on the size of the feature being toleranced. Larger features will have larger tolerance ranges. Standard ANSI tolerance grades and their numerical values are shown in Table 3-2. IT tolerance grades and their values are given in Table 3-3. The graded tolerance values corresponding to a given fit letter and grade number combination are normally obtained either through the use of charts or are built in to drafting (CAD) software. Some selections from these charts are provided in Tables 3-5 through 3-10. To use the tolerance charts, the designer must look up first the value corresponding to the letter designation. The tolerance values are then located on the letter designation chart at the intersection of the feature size row and number designation column.

Again revisiting the example with the m6 pin, the numerical limits of size for each tolerance designation can be found using Tables 3-5 through 3-10. First look up the limits of size for the diameter of the hole and pin, assuming that they are the standard locational interference fit tolerances of H7/ p6. If the pin diameter is 0.25 inch, the chart limits of size values for H7 in that size are +0.0006 / −0. For p6, the limits of size are +0.001 / +0.0006. Calculate the maximum and minimum interference between an H7 hole and a p6 pin using those limits: 0.001 / 0. For more information on performing tolerance analysis, please refer to Section 3.3. Now apply these interference values to the m6 pin and its limits of size to get the target tolerances for the locational interference fit hole. Use the tables to find the limits of size for the m6 pin with 0.25 inch diameter: +0.00059 /+0.00024. Because the least calculated interference should be 0, the upper limit for the hole to fit this oversized pin should be +0.00024. The upper limit of interference is 0.001, so the lower limit for the hole should be −0.00041.

If the designer prefers to use a tolerance designation instead of numerical values for the hole, a standard designation should be sought for limits of size of +0.00024/ −0.00041 for a diameter of 0.25 inches. Using the tables, the closest designation to those limits of size is K7 for that size of hole. Designation K7 at 0.25 inches diameter has limits of size of +0.0001 / −0.0005. A K7 hole combined with an m6 pin in that size will result in a fit that allows between 0.00014 and 0.00109 inches of interference in the joint. The standard fit allows between 0 and 0.001, so this modified fit should work acceptably. The advantage of using the system of limits and fits is that once a fit is calculated, the designations are easily remembered and reused. A standard dowel pin has an m6 designation, so the designer can easily remember (or record) that a K7 hole will yield a satisfactory interference fit. Numerical values need not be recalled once a fit is defined. When the designer has control over the tolerances applied to both parts, using standard fit designations can speed the process.

When using force fits, the pressure required to assemble the parts can be estimated using pressure factors. The stress resulting from force fits should be calculated for a more accurate result. It is essential that the elastic limit of the parts in a force fit assembly not be exceeded because that would result in a loosening of the fit. Consult the recommended resources for calculation guidance.

Table 3-1: Commonly Used Limits and Fits

Table 3-2: Selected ANSI Tolerance Grades

Table 3-3: Selected International Tolerance (IT) Grades

MACHINING TOLERANCES

Choice of tolerances should always take into account the manufacturing process capability as well as functional requirements. Every machining process has a tolerance capability. This can vary by machine and machinist. Some machining tolerances are given in ANSI B4.1. Table 3-4 illustrates some typical tolerance grades achieved by various machining processes. The values shown are intended only as a guide and vary depending on machine tool and operator. Tables 3-2 and 3-3 provide the numerical values for the tolerance grades as a function of part size.

Table 3-4: Manufacturing Process Average Tolerance Grades

LIMITS OF SIZE DATA

Tables 3-5 through 3-10 contain some of the more commonly encountered limits of size.

Table 3-5: Selected Limits of Size, Holes (Inch)

Table 3-6: Selected Limits of Size, Shafts (Inch)

Table 3-7: Additional Selected Limits of Size (Inch)

Table 3-8: Selected Limits of Size, Holes (Metric)

Table 3-9: Selected Limits of Size, Shafts (Metric)

Table 3-10: Additional Selected Limits of Size (Metric)

CRITICAL CONSIDERATIONS: Limits, Fits, and Tolerance Grades

•Factors like long engagement lengths, temperature, and lubrication will affect fit.

•Standard fits are an excellent starting point, but are no substitute for careful analysis of tolerances.

•In a force fit assembly, the elastic limit of the parts must not be exceeded. Calculate the resultant stresses for all force fits to ensure proper grip.

BEST PRACTICES: Limits, Fits, and Tolerance Grades

•When choosing tolerances for holes, an H designation is preferred.

•Use the most generous grades and tolerances possible to ease manufacture.

•Standard fits can be used to calculate the total clearance or interference for a desired result. When designing around an item with given limits of size, those values can be applied to calculate the limits of size for the mating part.

Section 3.2

TOLERANCES ON DRAWINGS, AND GD&T

Choosing tolerances and representing those values on drawings are critical steps of the design process. Choosing and analyzing tolerances is addressed in Sections 3.1 and 3.3 of this chapter. Communicating the desired tolerances and design intent can be simplified using implied tolerances, as well as Geometric Dimensioning and Tolerancing (GD&T).

RECOMMENDED RESOURCES

•L. Foster, Geo-Metrics III, Addison-Wesley Publishing Company, New York, NY, 1994

•Oberg, Jones, Horton, Ryffel, Machinery’s Handbook, 28th Ed., Industrial Press, New York, NY, 2008

•ANSI Y14.5M: “Dimensioning and Tolerancing”

•ANSI B4.1: “Preferred Limits and Fits for Cylindrical Parts”

IMPLIED TOLERANCES

To simplify drawings, most drawing title blocks contain a list of implied tolerance values. These tolerance values are applied to all dimensions unless otherwise specified. Tables 3-11 and 3-12 give some commonly used implied tolerances, but any tolerances may be applied to a drawing as implied tolerances. Wider tolerances generally reduce manufacturing cost, so generous implied tolerances are preferred if possible.

Table 3-11: Common Implied Tolerances (Inch)

Table 3-12: Common Implied Tolerances (Metric)

GEOMETRIC DIMENSIONING AND TOLERANCING (GD&T)

The use of Geometric Dimensioning and Tolerancing (GD&T) is the subject of many excellent books. GD&T allows the user to specify tolerances and relationships based on physical features and can yield drawings that are truer to the design intent that traditional Cartesian tolerancing. This section will serve as a basic introduction to the subject. Refer to the recommended resources for a full treatment of the proper use of GD&T and its symbols.

Datums

GD&T uses datums and a system of symbols to communicate the relationships between and tolerances of part features and surfaces. Datums are theoretically exact points, axes, or planes that are used as references to define the location and orientation of features on a part. Their typical appearance is illustrated in Figure 3-2. Although datums are usually associated with physical features, they are theoretical and have no tolerance or deviation from ideal even if the actual feature deviates. Datums should be selected to represent the function and mating relationship of a part. When selecting datums, it is helpful to use the following procedure:

1.Select datum A to be the primary constraining surface to contact the mating part when this part is placed into an assembly. This is the primary functional datum. For convenience, this surface is often a flat plane. Often this will be the bottom surface of a part, or a side surface if the part attaches on its side.

2.Select datum B to be the second constraining feature to locate the part to another part when the part is placed into an assembly. This datum is often a dowel hole or other locating feature. This is the secondary functional datum.

3.Select datum C to be the third constraining feature (if there is one) to contact the mating part when this part is placed into an assembly. This is the tertiary functional datum. This is often a slotted hole for a dowel pin. When all three datums are in use to constrain the part, it should not be able to move or rotate. It should be fully constrained.

Figure 3-2: Datum Callouts

It is possible to have more than three datums on a part, and it is also possible to have only one or two datums on a part. The typical case uses three datums. Datums can be patterns of features, such as a pair of dowel holes. In a case where datum A is a planar surface and datum B is a pair of holes, datum C is rarely needed to fully define the part because datum B can be used for location and orientation purposes. Orientation can be related to the imaginary line between the two holes in the pattern defining datum B, and location can be related to the center of either hole.

Symbols

Geometric characteristic symbols are used to specify feature and surface characteristics like orientation, location, shape, symmetry, and runout. These symbols are used as part of a feature control frame represented by a rectangle. This feature control frame contains the geometric characteristic symbol, a total tolerance, any modifiers, and the datums referenced in their order of significance. Figure 3-3 illustrates a typical feature control frame and its contents.

Table 3-13 provides geometric symbols governed by ANSI Y14.5M, which is the unified U.S. standard for both inch and metric units. For a complete coverage of ISO standards governing GD&T, the following standards are required:

•ISO 129: Technical Drawings General Principles

•ISO 2768: General Geometrical Tolerances

•ISO 8015: Fundamental Tolerance Principle

•ISO 406: Linear and Angular Dimensions

•ISO 5459: Datums and Datum Systems

•ISO 2692: Maximum Material Principle

•ISO 2692: Least Material Principle

•ISO 1101: Tolerances of Form, Orientation, Location and Run-Out

•ISO 5458: Positional Tolerancing

•ISO 3040: Cones

•ISO 1660: Profiles

•ISO 10578: Projected Tolerance Zones

•ISO 10579: Non-Rigid Parts

•ISO 7083: Symbols Proportions

When tolerances of position or profile reference datums, the two are related using “basic” dimensions. These dimensions have their value enclosed in a box. Basic dimensions are interpreted as nominal dimensions with no tolerance. The tolerance governing the feature’s position(s) and orientation(s) is applied through the feature control frame attached to the feature that is being positioned using the basic dimension.

Figure 3-3: Feature Control Frame

The following are descriptions of the most commonly used geometric symbols (Table 3-13) and their interpretation:

Straightness is a specification applied mainly to cylindrical features, and less commonly to flat features like rectangular bars. In the case of a cylindrical feature, it defines a tolerance zone within which the longitudinal elements of the feature must lie. Straightness is a tolerance of form, not position, and therefore does not reference any datums. Figure 3-4 demonstrates the straightness callout and its measurement.

Table 3-13: ANSI and ISO Geometric Symbols

Figure 3-4: Straightness Callout and Interpretation

Flatness is a specification applied to flat surfaces. It defines a tolerance zone between two parallel planes. All elements of the actual surface must fall within these two parallel planes. Flatness is a tolerance of form, not position. As a result, it does not reference any datums, and the planes defining the tolerance zone do not need to be parallel to any datums. Figure 3-5 illustrates the flatness callout and its measurement.

Figure 3-5: Flatness Callout and Interpretation

Circularity is a specification applied to cylindrical, conical, or spherical surfaces. On a cylindrical feature, it defines a circular tolerance zone on a plane perpendicular to the axis of the cylinder. An infinite number of planes can be assumed. The feature surface at each planar cross section must fall within the tolerance zone. This tolerance does not define the relationship between the cross sections at different planes. Circularity is a tolerance of form, not position, and therefore does not reference any datums. Figure 3-6 illustrates circularity tolerance for a conical feature.

Figure 3-6: Circularity Callout and Interpretation

Cylindricity is a specification applied to a cylindrical feature. It defines a cylindrical tolerance zone with a straight axis around the cylinder, within which all points on the feature’s surface must lie. Cylindricity is a tolerance of form, not position. As a result, it does not reference any datums. Figure 3-7 illustrates the cylindricity callout and meaning.

Figure 3-7: Cylindricity Callout and Interpretation

Angularity is a specification applied to a flat surface, axis, or midline of a feature. It defines a tolerance zone between two parallel planes at the specified angle from a datum. The angle will be given as a basic dimension. All points on the surface must fall between the tolerance planes. Angularity is a tolerance of orientation relative to a datum. Figure 3-8 illustrates angularity tolerance.

Figure 3-8: Angularity Callout and Interpretation

Perpendicularity is a specification applied to a flat surface, axis, or midline of a feature. It defines a tolerance zone between two parallel planes perpendicular to a datum. All points on the surface must fall between the tolerance planes. Perpendicularity is a tolerance of orientation relative to a datum. Figure 3-9 illustrates perpendicularity tolerance.

Parallelism is a specification applied to a flat surface, axis, or midline of a feature. It defines a tolerance zone between two parallel planes parallel to a datum. All points on the surface must fall between the tolerance planes. Parallelism is a tolerance of orientation to a datum. Figure 3-10 shows the parallelism callout and its meaning.

Figure 3-9: Perpendicularity Callout and Interpretation

Figure 3-10: Parallelism Callout and Interpretation

Concentricity is a specification applied to cylindrical or spherical features. It defines a tolerance zone about the axis of the feature (or center point, in the case of a sphere) within which all center points of the feature must lie. Concentricity is a tolerance of location relative to a datum axis or center point. An illustration of this is shown in Figure 3-11.

Figure 3-11: Concentricity Callout and Interpretation

Circular runout is a specification applied to cylindrical features, or features with round cross section. It defines a circular tolerance zone on a plane perpendicular to the datum axis within which all elements of the feature surface intersecting that plane must lie. An infinite number of planes can be assumed. Circular runout, unlike total runout, does not relate measurements at each section to one another. The part will be rotated about the datum in order to measure runout. Circular runout is a functional tolerance that relates the circular form at each cross section to one or more (concentric) datum axes. Figure 3-12 illustrates circular runout and its measurement.

Figure 3-12: Circular Runout Callout and Interpretation

Total runout is a specification applied to cylindrical features. It defines a cylindrical tolerance zone parallel to the datum axis within which all elements of the feature surface must lie. The part will be rotated about the datum in order to measure runout. Total runout is a functional tolerance that relates the cylindrical form to one or more (concentric) datum axes. Figure 3-13 illustrates total runout and its measurement. This specification is particularly useful when dimensioning rotating shafts that carry components like bearings or gears that are sensitive to misalignment.

Figure 3-13: Total Runout Callout and Interpretation

Profile of a surface is a specification applied to surfaces. The surfaces can be of complex shape and must be fully defined using basic dimensions. Profile of a surface defines a tolerance zone centered on the nominal surface and following the surface shape. All points on the surface must fall within the two boundary planes. Unilateral tolerancing is possible, so consult the recommended resources for more information. Profile of a surface is a tolerance of form that may or may not reference datums. When datums are referenced, the profile form and relative position are both controlled. This specification is very powerful in that regard. Figure 3-14 illustrates this callout.

Figure 3-14: Profile of a Surface Callout and Interpretation

Position is a specification applied to center points, midplanes, or axes of features. It is most commonly applied to holes and hole patterns. Position specification defines a tolerance zone around the feature’s nominal center. This tolerance zone is cylindrical in the case of hole features, and rectangular in the case of flat features. The center, midplane, or axis of the feature must lie within the tolerance zone. Position tolerance can be applied to groups of identical features and, in such a case, the tolerance zone is set up for each individual feature in the pattern. Position is a tolerance of location relative to one or more datums. Basic dimensions must be used to provide nominal location for the features bearing position tolerances. Figure 3-15 illustrates a typical position callout for holes, and Figure 3-16 shows some possible variations allowable within position tolerance zones. Compound tolerance frames are an advanced technique that may be used to control position of features within a pattern while allowing a separate tolerance to control the location of the pattern center relative to the datums. This powerful technique is illustrated in the recommended resources as well as in Chapter 4 of this book.

Figure 3-15: Position Callout and Tolerance Zones

Figure 3-16: Position Tolerance Zones and Allowable Variation of a Hole Axis

Modifiers

Tolerance modifiers include maximum material condition, minimum material condition, and regardless of feature size. Modifers may not be added to runout, concentricity, or symmetry specifications. Maximum material condition (MMC) is the condition in which a feature is at the limit of size corresponding to the maximum material left on the part. For a hole, MMC corresponds to the smallest hole within the stated limits of size. For an external diameter, MMC corresponds to the largest diameter within the stated limits of size. Least material condition (LMC) is the condition in which a feature is at the limit of size corresponding to the least material left on the part. LMC for a hole is the largest hole within the limits of size, and for an external diameter is the smallest diameter within the limits of size.

MMC and LMC are used to modify a tolerance or datum reference based on the size of the feature as produced, rather than its theoretical size. Regardless of feature size (RFS) indicates that the tolerance or datum reference applies to a nominal feature and not to the feature as produced. RFS is assumed in all cases unless otherwise stated. MMC is commonly used, whereas LMC is seldom used. When the MMC modifier is present, the tolerance is read as “tolerance when feature is at maximum material condition.” The use of MMC permits additional tolerance when the considered feature, as produced, departs from its maximum material condition. Consult the recommended resources and Section 3.3 for guidance on the proper use of modifiers.

CRITICAL CONSIDERATIONS: Tolerances on Drawings and GD&T

•All dimensions on a drawing must have tolerances specified, either implied or explicit.

•Dimensions and tolerances should convey design intent and functional relationships between features and surfaces.

•Analyze all critical tolerances to ensure proper fit and function.

BEST PRACTICES: Tolerances on Drawings and GD&T

•Use standard symbols when applicable rather than notes. Standard symbols have clear and universal meaning, whereas notes may be misunderstood.

•Specify the loosest tolerances possible to save cost and enable a choice of manufacturing methods. This may require explicit tolerances that are looser than the drawing’s implied tolerances in some cases.

•When checking drawings, a useful technique with paper drawings is to use a highlighting marker for checked dimensions and a red pen to make changes. The title block should also be checked, including any implied tolerance information.

•Apply position tolerance to all holes, and dimension their locations with basic dimensions.

•Threaded features and tapped holes are normally dimensioned with the modifier “Regardless of Feature Size (RFS),” and the tolerance is applied to the axis of the thread derived from the pitch cylinder. Exceptions to this practice must be noted on the drawing.

•When applicable, apply the modifier “Maximum Material Condition (MMC)” to allow more deviation when parts to be fit together are not produced at the maximum material condition limits of size. This can save cost by allowing more deviation while ensuring proper fit.

Section 3.3

TOLERANCE STACK-UPS

Written by Charles Gillis, RE.

Every dimension on every feature on every mechanical component has variation. The allowable variation is specified by the designer through tolerances associated with each dimension. Understanding the effects of these variations on the assembly and assigning appropriate tolerances to dimensions requires performing tolerance stack-ups. Sometimes referred to as tolerance analysis or tolerance assignment, performing stack-ups bring together understanding of manufacturing processes and dimensioning standards (e.g. ASME Y14.5) to meet the assembly’s functional requirements; they are a critical element of good design practice.

The choice of tolerance is as important as any other design choice. Tolerances must not be chosen arbitrarily, but rather with good understanding of assembly requirements, manufacturing process capabilities, and cost. Good designs allow the largest tolerances possible to achieve the functional requirements. Manufacturing methods evolve and improve over time, and larger tolerances give manufacturers greater flexibility to choose methods: part routing, machine tool choice, setups, etc. Overly restrictive tolerances tie the hands of manufacturers and drive costs up. Excessive precision may meet the functional requirements, but is a very poor design choice.

Tolerance stack-up calculations are performed during the design phase to understand sources of variation within a physical assembly, for sensitivity analysis, and to verify that the design intent has been captured on dimensional specifications (detail drawings). Performing stack-up calculations allows designers to assign tolerances based on manufacturing capability, to determine assembly process capability, and to implement process control. This section presents the reasons and methods for conducting tolerance stack-up calculations, including several different mathematical approaches and the appropriateness of each approach. The purpose is to enable the reader to understand the effects of tolerance stack-ups on design choices, ultimately enabling better design choices.

RECOMMENDED RESOURCES

•D. Madsen and D. Madsen, Geometric Dimensioning and Tolerancing, 8th Edition, Goodheart-Willcox, Tinley Park, Il, 2009

•A. Newmann and S. Newmann, GeoTol Pro - A Practical Guide to Geometric Tolerancing per ASME Y14.5-2009, Society of Manufacturing Engineers, Dearborn, MI, 2009

•ASME Y14.5 - 2009: Dimensioning and Tolerancing

DESIGN PRACTICE

Good design practice involves an iterative process:

1.Determine which component dimensions contribute to critical assembly dimensions (the tolerance stack-up chain).

2.Assign preliminary tolerances.

3.Analyze the assembly tolerances.

4.Determine fitness of design, iterate as necessary.

Component dimensions are “in-specification” (in spec) if they are manufactured within their specified tolerances. The combined effect of the individual variations in an assembly may not be in spec, even if the components are. It is sometimes discovered through tolerance analysis that a concept will not achieve the assembly tolerance needed.

When a tolerance stack-up shows the assembly to be “out-of-spec,” the designer reduces and/or re-distributes component dimension tolerances using some of the following methods:

1.Redesign the assembly to reduce the number of components in the stack-up chain, or utilize features that can be produced through inherently more precise processes.

2.Change the component dimensioning scheme to better represent assembly method, apply different geometric controls, or reduce the number of dimensions in the stack-up chain.

3.Eliminate fits from the stack-up chain.

4.Utilize precision locating methods (see Chapter 4) to reduce variation introduced by fits.

5.Reassign / reduce component dimension tolerances.

THE TOLERANCE STACK-UP CHAIN

The first step in a tolerance stack-up is to determine the chain of dimensions contributing to the stack-up. Consider the assembly of components in Figure 3-17. In order for the components to be assembled, it is necessary for the tab of the left component to fit within the slot of the right component. The detail drawings illustrating relevant dimensions are shown in Figure 3-18. The designer is interested in the allowable variation on the size of the lower gap of the tab / slot features, as well as the upper gap of the tab / slot features. Two stack-up calculations are required to determine that positive, non-zero gap distances exist on both the top and bottom clearances.

For chains involving only a few dimensions, it may be tempting to take shortcuts. However, an organized approach is the best approach in determining the tolerance stack-up chain. The procedure is as follows:

1.Understand the assembly. Analyzing unfamiliar designs may require some time to get oriented.

2.Gather the detail component drawings, which may be in process.

3.Make an assembly sketch. Hand-drawn is best, as it is often helpful to illustrate gaps and clearances, show components at extreme positions and orientations, and show other dimensions out of scale.

4.Choose a sign convention (e.g., positive up, positive to the right).

Figure 3-17: Sample Assembly for Analysis

Figure 3-18: Detail Drawings of Component Parts

5.Determine which dimension needs to be solved. This requires a good understanding of the problem in order to convert a design concern into a specific dimension that must be discovered. The concern being addressed by the analysis may require that several stack-ups be evaluated. A stack-up to determine if a retaining ring will fit within its groove would seek to calculate the clearance gap dimension (groove width – ring thickness) and ensure it is positive. More complicated problems can be properly defined and understood with the aid of the sketch.

6.Draw the assembly dimension and label it ‘A’ for assembly. The assembly dimension is the unknown dimension you’re solving for. It should be the only dimension that is not obtained from the component detail drawings.

7.Identify contributing dimensions. Determine which dimensions on the component detail drawings contribute to the size, position, and / or orientation of the assembly dimension sought. These dimensions may be given with bilateral equal or unequal tolerances, unilateral tolerances, limit tolerances, title block tolerances, or geometric controls. Draw the other dimensions on the assembly sketch per the detail drawings. Label them.

8.Make each dimension into a vector by assigning an origin and destination. The choice of origin and destination is arbitrary, but it is important that this convention be maintained once it is chosen. The vector is illustrated with an arrowhead on the destination’s extension line and an origin symbol (circle) on the origin’s extension line.

9.Chain all the dimensions together head-to-tail. Ensure the chain of dimensions forms a complete loop with the destination of the final dimension connecting to the origin of the first. The term “loop” is used even if the vectors may all be one-dimensional (e.g.. all dimensions are up / down, or all dimensions are left / right). Although components are three-dimensional, and specifications made properly using GD&T fully define the component in 3D, tolerance analyses are generally 2D or even 1D problems. Depending on the assembly, the designer determines in steps 1 through 3 whether the stack-up problem is 1D, 2D, or 3D. The simplification to a 2D or 1D problem does not omit any information or oversimplify the analysis — it is done when the problem is, at its core, a 2D or a 1D problem. The vast majority of tolerance stack-up problems within machine design are 1D. In other fields, 2D and 3D analyses may be required more often. The rest of this section focuses on techniques for 1D stack-ups.

10.Write the stack-up equation. Write out the tolerance stack-up equation as the algebraic sum of dimensions, following the positive / negative sign convention. Set the sum equal to 0. Re-arrange the equation to solve for assembly dimension A.

A tolerance stack-up chain drawing clearly shows how component dimensions relate to one another and contribute to assembly dimensions. Understanding this relationship allows the design engineer to meet the functionality and cost goals. The creation of the stack-up chain drawing is the first step in analysis or assignment and is best begun when the design of the overall assembly scheme is still preliminary.

The simplified stack-up chain drawing is shown in Figure 3-19. Each dimension has a marked origin and destination, i.e., a “from” denoted by the circular origin symbol and a “to” denoted by an arrow. Each “from” connects to the next “to.” The assembly dimension connects the first “to” to the last “from.” A clearance dimension is included for each fit.

Figure 3-19: Stack-Up Chain Drawing

The stack-up equation is first written by summing the dimensions using the sign convention (“up” arrows positive, “down” arrows negative):

+G − H − A + F + E + B − C − D = 0

Re-arranging to solve for the assembly dimension A:

A = B − C − D + E + F + G − H

The assembly dimension A contains both dimensions with positive signs (positive contributors) and negative signs (negative contributors).

The stack-up equation must be created before any calculations can be done. Some tolerance stack-up problems are very simple and can be solved with simple arithmetic without the need to write the stack-up equation. These are sometimes done mentally, or written on scrap paper that is not maintained as part of the engineering records, resulting in a loss of important engineering analysis. The step-by-step process illustrated here assures that a standard methodology is followed, ensuring a commonality of approach regardless of the complexity of the problem. This method is appropriate for both simple problems and complex stack-ups involving dozens of dimensions. It also allows checking and review by other engineers seeking to verify correctness of analysis, to issue engineering changes, or to diagnose problems encountered downstream.

PRELIMINARY TOLERANCE ASSIGNMENT

Assigning small tolerances requires producing high-precision components that increase cost. The designer must be careful not to exceed the capabilities of the manufacturing process (see Section 3.1), or to exceed cost targets. When assembly variation is sufficiently controlled by limiting allowable component variation, interchangeability is achieved. Interchangeability has many benefits to the assembly process, maintenance, and field service, but it requires careful planning.

Interchangeability may be required if a firm uses globally-sourced components and its products are installed, sold, used, or serviced globally; for example if its strategy is to be able to build-to-print from anywhere any time, and ship parts to any field location. Replacement parts and serviceable parts often need to be completely interchangeable as machining-to-fit is not an option. Interchangeable parts enable lower-skilled technicians or users to service, repair, and / or replace parts without precision assembly setup procedures. Whenever it is reasonable to assume that the component in question will be exchanged for an equivalent one, designing for interchangeability should be considered.

When interchangeability is not required, or when assembly variation cannot be adequately controlled by tolerance assignment alone, several design options are available, each requiring greater skill during the assembly process:

•Setup at assembly: Adjustability is designed into the assembly, assembly instructions are provided by the design engineer, and final setup dimensions and assembly tolerances are clearly indicated. Standard shop inspection tools, portable coordinate measuring machines, or custom-designed gages may be used to achieve the assembly accuracy required.

•Assembly fixturing: Similar to setup at assembly, though fixtures are used to hold some or all components in relationship to one another during the assembly process. Many modular fixturing systems are available, or custom fixturing may be required.

•Assembly of matched sets: Components are segregated by the measurements of critical dimensions. Assemblers match small components with large ones, for example — to achieve a tighter assembly variation. The stack-up guides the assembly planner in creating assembly instructions. Ball bearings are produced as matched sets of inner / outer races and balls.

•Machining at assembly: After the components are assembled, critical dimensions are achieved by finish machining features that were only roughed in initially. Dowel pins or other permanent fitting methods are often used to lock in the critical assembly dimensions, either by preventing disassembly or by ensuring repeatable re-assembly.

Even though the assembly’s dimensional needs have been met, the task of tolerance assignment is not necessarily complete. Consider an example of seven dimensions contributing to a tolerance stack-up chain. One approach is to assign the same tolerance to each dimension in the chain, such that the total assembly tolerance is achieved. This may not be optimal because features that are simple to produce with precision could have smaller tolerances assigned, and features made using more difficult or costly operations may require larger tolerances. A second approach seeks to match each contributing dimension tolerance to the manufacturing capabilities used to produce it. Section 3.1 provides guidelines for common manufacturing processes. Good partnerships between design engineers (function, design, dimensioning) and machine shop / manufacturing personnel (process capability and cost) can prove extremely valuable. Alternative approaches to tolerance assignment incorporate manufacturing vs. tolerance cost information and sensitivity analysis to assign tolerances based on multiplicative effects of their contributions to the assembly tolerance and cost. Analysis gives just one answer, but assignment has no unique solution.

ANALYSIS AND ASSIGNMENT METHODS

Tolerance analysis and tolerance assignment are two sides of the same coin, the only difference being which dimensions are considered inputs and which are outputs. For either approach, four methods of calculation are common:

•Worst-case

•Statistical

•Combined

•Monte Carlo

Worst-Case Method

The most common method of tolerance stack-up for machine design engineers is the worst-case method. The tolerance stack-up calculation is performed twice, resulting in the maximum assembly dimension on the first pass and the minimum value on the second pass. Using this method gives the maximum possible contribution to the final result from each source of variation. Benefits to this method are its simplicity and speed. It leaves the smallest tolerances available for assignment. If the designer is more interested in reducing risk than in accurate predictions, worst-case is the method to use.

Writing all dimensions in the chain in limits-of-fit format provides simple and efficient bookkeeping. This is a shorthand way of writing what are actually two equations, and they are each evaluated. The calculation is performed twice. The maximum value of the assembly dimension, Amax, is obtained by adding the maximum (top value) of all positive contributors and subtracting the minimum (bottom value) of all negative contributors. Amin is the sum of all minimum (bottom value) positive contributors minus all maximum (top value) negative contributors.

Here is what the two equations look like when separated:

A_max = B_max − C_min − D_min + E_max + F_max + G_max − H_min

A_min = B_min − C_max − D_max + E_min + F_min + G_min − H_max

Calculating the example stack-up from Figures 3-17 through 3-19:

This calculation has revealed that the gap in question can obtain a negative value — meaning an interference is possible. If this design were still preliminary, the designer could address this problem by adjusting assigned tolerances.

Worst-case analysis is appropriate when the number of components produced is relatively small, and when inspection is used on every component to eliminate components whose dimensions fall outside the specification limits. When components are screened, the designer can assume that component dimensions will be produced in-spec. Worst-case analysis is also used when no quality inspection data are available to allow more conservative prediction of the produced component dimensions.

One drawback of the worst-case analysis is that it is unlikely that the actual measured assembly dimension will take on the calculated minimum or maximum value. It is more likely to be near the middle of the range, as component dimensions produced near their upper limits cancel out the effect of dimensions produced near their lower limits. This drawback becomes more pronounced when more dimensions are included in the stack-up chain.

The stack-up equation can also be used to solve a tolerance assignment problem containing a single unknown. When the assembly dimension is known, and only one dimension needs to have its dimensional limits assigned, the separated worst-case equations can be re-arranged to solve for the final tolerance to assign. For example, when the limits of dimension B are desired,

B_max = A_max + C_min + D_min − E_max − F_max − G_max + H_min

B_min = A_min + C_max + D_max − E_min − F_min − G_min + H_max

The stack-up equation used for analysis must be separated before it can be re-arranged for use in assignment. This is because of the way the analysis equation is derived: dimension A reflects the total variation of all dimensions. Using this equation for assignment may reveal that there is not enough tolerance left to give to dimension B and other assignment changes must be made. This is indicated by a meaningless result showing a minimum value for dimension B greater than its maximum value. Often, an assignment problem requires assigning tolerances to several dimensions, and the analysis equation cannot be re-arranged to solve for the missing dimension. In this case, an iterative approach is used.

Statistical Method

The statistical stack-up method shifts the focus from the possible to the probable. The resulting predictions of assembly dimensions are more realistic provided the data and/or assumptions are realistic. Statistical stack-ups also leave larger tolerances available for assignment. The analysis gives likely values and ranges depending on confidence intervals. The analysis is not a guarantee of conformance to specs because some outliers may exist. Assembly yield rates or defect rates can be predicted.

When a large number of dimensions contribute to a stack-up, the result is typically distributed according to a normal distribution. Even though individual components will be fully screened at inspection, statistical methods predict the likely assembly dimensions more accurately than the more conservative worst-case method.

Statistical stack-up calculations are appropriate when it is known or can be assumed that the contributing dimensions follow a normal distribution. When a dimension follows a normal distribution, most of the values are clustered around the mean value. It is also possible for a dimension to attain a value outside its specification limits, though with low probability. If no quality inspection reports exist for a component being designed, but data for analogous components and manufacturing processes shows a normal distribution, statistical methods may also be applied.

For large production runs, Statistical Process Control (SPC) is typically used to control the manufacturing process and ensure dimensions are under control. SPC controls the process, not the component. Sample components are inspected at intervals and used to determine whether the process is in control. Inspection is not used to determine which components fall within specifications and which do not on a part-by-part basis. Under these conditions, a normal distribution of dimensions typically results. This will typically be true of commodity hardware components like screws.

Using Variables with a Normal Statistical Distribution

The normal distribution for a given dimension is described by two parameters: the mean (μ) and standard deviation (σ). The mean indicates the average value, and the standard deviation is a measure of the variation within the sample. A larger standard deviation indicates more dispersed values of the dimension. Stacking up dimensions described by a normal distribution results in an assembly dimension with a normal distribution. This distribution can then be compared to assembly spec limits to determine the likelihood of a given assembly being out-of-spec, or the percentage of assemblies that will be produced out-of-spec (defect rate).

For the stack-up equation derived in the previous section,

Assembly mean: μA = μB − μC − μD + μE + μF + μG − μH

Assembly standard deviation:

Note that the mean values sum algebraically to the assembly mean whereas the standard deviations combine as the square root of the sum of the squares of the standard deviations. Note also that standard deviations all add as positive terms under the radical. A statistical stack-up using all normally-distributed dimensions is often called the Root Sum of Squares (RSS) method.

For a tolerance assignment problem where an assembly dimension is known, and all dimensions are prescribed but one, the analysis stack-up equation can be rearranged as it was in the worst-case example. If dimension B is desired,

Dimension mean: μB = μA + μC + μD − μE − μF − μG + μH

Dimension standard deviation:

As with the worst-cast stack-up, most assignment problems will require simultaneous assignment of tolerances to several dimensions and an iterative approach. If the calculation of the dimension standard deviation results in a negative number under the square root sign, the assignment problem can not be solved with the tolerances currently chosen. There is insufficient variation remaining to be assigned to dimension B.

Using the Standard Normal

The property of the normal curve that is most useful to machine designers is that the area under the curve, bounded between lower and upper points ZL and ZU on the Z-axis, represents the percentage of all Z’s that will be between ZL and ZU. The total area under the normal distribution curve is always equal to 1, or 100%. Calculating the area under a given normal distribution curve can be tedious, so a transformation of variables is used to take advantage of tabulated values.

The standard normal is simply a normal distribution curve with μ = 0 and σ = 1. The area under the standard normal curve is pictured in Figure 3-20 and tabulated in Table 3-14. The values indicate the area under the curve to the left of Z. The table is read by finding the value of Z by summing the column and row headers and locating the area at the intersection. The area under the curve to the left of Z = −1.25 is 0.10565, or 10.565% of the population. This percentage is found at the intersections of row “−1.2” and column “−0.05” corresponding to the value of −1.25.

Figure 3-20: Standard Normal Curve

Because the curve is symmetric, the table only gives the area under the curve for half the curve: from the left up through Z = 0. To calculate the area for positive values of Z, use the identity:

Area(Z) = 1 − Area(−Z)

The following example demonstrates how to use the table to determine what percentage of assemblies fall between the upper and lower spec limits of AUSL = 0.35 and ALSL = 0. First, calculate the assembly mean and standard deviation:

μA	=	μB − μC − μD + μE + μF + μG − μH
	=	1.735 − 8.5 − 3.175 + 2.66 + 0.51 + 8.5 − 1.5625
μA	=	0.17

Table 3-14: Area Under the Standard Normal Curve

To calculate the values for Z we will look up in the table:

The area under the normal curve between ALSL and AUSL is the area under the curve to the left of ZUSL minus the area under the curve to the left of ZLSL, ^or:

=	Area(3.911) − Area(−3.694)
=	[1 − Area(−3.911)] − Area(−3.694)
=	(1−0.00005)−0.00011
=	0.99984

According to this sample calculation, 99.984% of assemblies will be in-spec, and 0.016% out-of-spec. The standard normal table can also be used to determine spec limits for a given desired defect rate.

Modeling the Distribution

Performing an accurate analysis using the statistical method requires knowledge of the dimensions of the produced parts. This is not always available, and assumptions must be made. Given upper and lower specification limits (USL, LSL), what will be the mean (μ) and standard deviation (σ) of the population? These values can be assumed outright when their meaning is fully understood.

Often the mean and standard deviation are assumed by way of other measures. The process capability index (Cpk) is used as an indicator of how well a manufacturing process is capable of producing dimensions on-target between the spec limits. The terms Cpl and Cpu are the lower and upper process capability indices, respectively.

A Cpk of 1.0 with a mean (μ) on target (halfway between the specification limits) corresponds to a standard deviation (σ) of one-sixth of the tolerance range (USL − LSL), or 99.73% of dimensions in-spec. Larger values of Cpk indicate greater control over the process and incur greater manufacturing expense: smaller values, less control at less cost. A centered process with Cpk of 2.0 represents a Six Sigma process, a goal of many corporate quality programs using SPC, and may be assumed by the design engineer purchasing components from reputable and reliable companies. A smaller assumption on Cpf would be more conservative.

However, knowing Cpk alone is not enough to select both μ and σ When the terms Cpl and Cpu are equal, the μ is on target and centered between the spec limits. They need not be equal. A larger upper process capability index occurs when the mean is shifted closer to the LSL; a larger lower process capability index means the mean is shifted toward the USL. When Cpl and Cpu are known or can be estimated, μ and σ can be calculated:

Подняться наверх