11-12: GD&T

Why use GD&T? #

Limitations of conventional tolerancing #

Example: four pins need to make a clearance fit with four holes

Tolerance limits on pin and hole spacing need to be specified

  • (Left) Tolerance zones for centers of holes
  • (Right) What if a pin is positioned at the extreme edges of both tolerance zones?
    • Case 1 is extreme along $x$
    • Case 2 is extreme along both $x$ and $y$
  • In conventional tolerancing, tolerance zones are inherently one-dimensional
  • In two- or three-dimensional designs, we risk accepting non-functional parts if each dimension is considered in isolation
  • Options: tighten tolerances, enlarge clearance, or use…
  • GD&T: standard graphical language, ASME Y14.5, that allows tolerances to be unambiguously defined on drawings
    • Allows different features to be related to each other (3D)
    • Specifies how measurements are set up and made with datums

Datums #

Theoretical datums #

  • Theoretical datums are defined on drawings using features of the component to be manufactured
  • Datums can be
    • Planes (e.g. flat surfaces of the component) i.e after facing operations
    • Axes (e.g. axis of a hole or cylindrical feature) i.e when turning
  • Every datum is given a letter on the drawing which uniquely identifies it

Example: three perpendicular datum planes:

Datums in measurement #

  • Real manufactured objects deviate (even if slightly) from the ideal geometry
    • Surfaces not perfect planes
    • Axes not perfectly straight, etc
  • So, we need a procedure to interpret measurements from a component to establish a “best fit” for the datum plane or axis
    • Use a physical “datum simulator” like a rigid, flat surface (e.g. granite table) to rest against the component
    • Measure multiple points $(x,y,z)$ with CMM or optical metrology and fit the plane or axis datum in software (e.g. use least-squares regression – advanced software available for this)
  • The number of datums needed to define a given tolerance depends on the geometry of the component and the type of tolerance

Example: Physical Planar Datum Simulators #

  • In measurement, we place a flat surface against the component as a datum simulator
    • Needs to be at least $\approx 10$ times smoother than the target surface
    • We measure wrt this datum rather than the part’s features
  • For any given dimension specified in GD&T, datums are defined with an order of preference. During measurement:
    • First plane makes three-point contact with surface
    • Second plane makes two-point contact
    • Third plane: one-point contact

Introductory examples #

Example: hole in a block #

Surfaces are not smooth in a real part, so we measure the hole center from the datums $A,B,C$

Example: hole spacing in plate #

Four pins need to make a clearance fit with four holes – tolerance limits on pin and hole spacing need to be specified

Center positions #

MMC: Maximum Material Condition #

  • Use when want clearance
  • MMC means least “play” is available between the components
  • Bonus tolerance is added if components are not in MMC.
  • Example: if actual size of hole is .252" rather than .250", size of tolerance zone increases from .006" to .008" diameter

LMC: Least Material Condition #

  • Use if want interference
  • Or for, e.g., holes very close to the edge of a part
  • Bonus tolerance now added if more material is left on component

Feature Control Frames #

  • (Left) Geometric characteristic: symbol – see more below
  • (Middle) Size of the tolerance zone – either a linear dimension or a diameter of a tolerance zone, depending on the type of tolerance
  • (Right) Datum reference letters, if applicable
    • Noted in the order in which they are to be established during measurement.

Range of GD&T symbols #

Categories of Tolerance #

Form Tolerances #

Straightness #

1 Straightness of an edge, or a line on a surface (top) #

  • Tolerance defined as the maximum distance between the closest two parallel lines including all points on the edge under consideration
    • Single dimensional value (no diameter symbol, Ø)
  • Controls bowing, waisting, and barreling of cylindrical features

2. Straightness of an axis (bottom) #

  • Cylindrical tolerance zone must fit inside this diameter
    • Needs diameter symbol, Ø
  • Compute axis position by forming an equidistant set by bisecting pairs of measured points on surface of the cylindrical feature
  • Matters because we are generally trying to mate one cylindrical feature with another
    • e.g. peg and hole
  • Note that a cylindrical feature can have a straight axis without having straight edges, as would be the case when a feature exhibits waisting or barreling.

Flatness #

  • 2D version of straightness – applies only to planar feature
  • To measure, we sample a series points on the surface (physical edge)
    • Can be accomplished with optical interferometry or the entire surface in one scan, or, approximately, by stylus profilometry – e.g. by running a dial gage across the surface multiple times and measuring the needle deflection
  • Tolerance zone is defined as the maximum allowable spacing between the closest two planes that enclose all points on the manufactured surface
    • Tells us nothing about relationship with any other surface
      • Not used, e.g. , to control thickness uniformity of a plate
  • Disadvantage of using multiple linear measurements to check flatness is that the relative locations of these measurements are not known, so checking the flatness tolerance against the exact definition described above (maximum distance between two parallel planes) is then not strictly possible

Circularity (Roundness) #

  • Controls out-of-roundness within any plane perpendicular to the axis of the cylinder
  • The tolerance value specifies the maximum allowable difference between radii of two concentric circles that are as close together as possible and that enclose all points of the manufactured circumference
    • Center position of circles is fit to measurement data to give minimal difference in radii (minimum zone circle)
      • To test this tolerance strictly, one would have to measure the shape of the circumference with stylus, and then use a data-fitting algorithm to identify the two circles with the smallest difference in radii that enclose all points
    • How far from perfectly circular any particular circumference of a cylindrical feature is allowed to be.
  • In many machine shops, an approximate measure of circularity is often obtained by placing the component in a V-block (right), and rotating it while a dial gage stylus rests on the upper surface.
    • The peak-to-peak, $\Delta d$, deflection of the gage needle is taken as an estimate of out-of-roundness.

  • When a circularity tolerance is applied to a cylindrical feature, we require the tolerance to be independently met at all points along its axis.
  • When we consider all longitudinal positions simultaneously, our tolerance is one of cylindricity:

Cylindricity #

  • ‘3D version’ of circularity
  • All points on surface of cylindrical feature must lie between two concentric cylinders separated by no more than the tolerance value
    • Axial position and orientation of cylinders is fit to measurement data to give minimal difference between radii (MZC: minimum zone cylinder)
    • Considers all points on the surface of the feature simultaneously

Summary #

  • The range of acceptable material positions is contained by the tolerance zone:
    • 2D region for straightness/circularity
    • 3D region for flatness/cylindricity

Profile #

  • Specify the allowable deviation of a line or surface from a perfect profile
    • Can be bilateral (equal or unequal), or unilateral, shown above
    • Can be specified with or without a datum reference
  • Line profile tolerance example
    • Any line trace along the profile and parallel to its edges must satisfy the tolerance
    • Every point along a line tracing the surface of the toleranced feature must lie within a band whose width is given by the tolerance zone size.
    • The tolerance is defined between two endpoints that are labeled using letters
      • $X \iff Y$ in the example below
      • Can be (but does not need to be) referenced to one or more datums
    • Unless otherwise stated, the tolerance band is equilateral around the nominal position of the line.

Surface profile tolerance #

All points on the indicated surface must lie within the tolerance zone, considered simultaneously

Profile tolerances: with vs without datum #

Yellow shows looser tolerance zone without datums; just says that the line’s/surface’s shape has to fit the tolerance – not that that surface itself has to be constrained by it’s to fit with other parts

Unilateral vs Bilateral #

Orientation tolerances #

While form tolerances dictate the required “quality” of a single feature, and profile tolerances may or may not be anchored to a particular datum or datums, orientation tolerances inherently require the use of datums, because they are about relating one feature to another. We need to establish a datum to represent one feature before we can determine how the second feature relates to it. Orientation tolerances are as follows.

Parallelism #

  • Can be applied to surfaces and axes
    • One of the features is assigned a datum letter, and the other feature is referenced to it
  • Surface parallelism: when the non-datum feature is a plane, the tolerance zone tells us the maximum allowable distance between two planes which are:
    1. Parallel to the established datum
    2. As close together as possible
    3. Enclose all points on the referenced surface
  • As with flatness, though, a parallelism tolerance makes no statement about how the distance between the two features should be controlled/where the tolerance zone lies
    • That distance can be controlled by a separate dimensional tolerance as shown on the left side
    • E.x Two surfaces could be parallel but the wrong distance apart
  • Note that a parallelism tolerance is quite different from a flatness tolerance in that the planes being used to check a parallelism tolerance must lie parallel to a specified datum; this requirement does not exist for a flatness tolerance

Axis #

When the toleranced feature is an axis, we specify a cylindrical tolerance zone with a particular diameter — this tolerance zone is, however, constrained to be parallel to the datum, which differs from a simple straightness tolerance.

Establishing an axis datum #

  • If the axis datum is the first datum being established: find best-fit center-line for points measured on the surface of the cylindrical feature (e.g. by CMM)
    • Best-fit could be found by minimizing, e.g. sum of squared differences from surface points to axis
  • If other datum(s) have been previously established: the axis datum is also constrained to be perpendicular to previous datum(s)
    • Fitting process incorporates this constraint

Checking an axis tolerance #

  • Measure multiple points on the surface of the cylindrical manufactured feature
  • Find the effective position of the axis at all points along its length
    • Find “median position” between measured surface points
    • Manufactured axis will not be perfectly straight
  • Ask whether all points along the manufactured axis fit within a cylindrical tolerance zone of the specified diameter that has the prescribed relationship to the given datum:
    • Tolerance zone may be parallel, perpendicular, concentric, etc. relative to datum
    • Tolerance zone can take the most favorable possible position for meeting the tolerance
    • Applies along the whole length of the toleranced feature

Perpendicularity #

  • Perpendicularity tolerances are very similar conceptually to parallelism tolerances, but the tolerance feature and datum lie at 90˚ to each other rather than parallel
  • Can be applied to surfaces and axes
  • Surface perpendicularity: all points must lie between two planes, separated by the tolerance value and perpendicular to the referenced datum

Axes #

Axis perpendicularity: all points on the axis must lie within a cylinder with the diameter of the tolerance zone and perpendicular to the referenced datum

Angularity #

  • Traditional (non-GD&T) approach
    • Angular tolerance is specified as a number of degrees
    • Tolerance zone is wedge- shaped
  • GD&T approach – requires that all points on the tolerance feature lie between two planes that are:
    1. At the specified angle from the given datum, and
    2. Separated by no more than the size of the tolerance zone An angularity tolerance in GD&T
  • Note that an angularity tolerance of this kind is rather different from a “traditionally” defined angular tolerance, which would place a range on the effective angle between two features

Note that an angularity tolerance of this kind is rather different from a “traditionally” defined angular tolerance, which would place a range on the effective angle between two features (as shown in the left above). In the traditional approach, the tolerance zone gets wider as the distance from the intersection point between the two features increases. Depending on what the component is supposed to do in use, one might argue that either the traditional approach or the GD&T approach would be the more useful way of tolerancing an angled feature. For example, if the component is intended to serve as a wedge to set the angle between two flat components, the traditional tolerancing approach might work best. On the other hand, if the component is supposed to be a mirror on to which a plane-wave of light is incident, we might rather use the GD&T approach so that the local angle of the surface is kept within certain bounds all the way along its length. The designer needs to think carefully about exactly what manufacturing defect is to be avoided

Location #

Concentricity #

  • This tolerance is useful, for example, when designing rotating machinery, in which multiple components may need to be placed on a shaft without resulting in out-of-balance loads.
  • Concentricity relates two axes
  • One datum axis and one toleranced cylindrical feature
  • All points on the axis of the tolerance feature must lie within a cylindrical tolerance zone centered on the datum axis

Symmetry #

  • Relates two planar features
  • All median points lying mid-way between the two surfaces of the toleranced feature must lie within the tolerance zone
  • Tolerance zone is centered on the datum feature
  • Tolerance zone defined by two planes

In some components, one feature is intended to be centered relative to another, and a symmetry tolerance defines how far those two features can deviate from symmetry. Here when we say “feature” we refer to opposing pairs of surfaces with equal size — a particular type of feature known as a feature of size. The opposite sides of the slot above constitute a feature of size, as do the opposite outside faces of the component itself. As shown above, one feature is specified as a datum (by labeling one side of the feature with a lettered symbol). The other feature is labeled with its nominal dimension and also with a feature control frame that contains the symmetry symbol, the size of the tolerance zone, and the relevant datum. The tolerance zone tells us how far the midplane of the toleranced feature can deviate relative to the midplane of the datum feature (which would be established by measuring points on both sides of the feature — i.e., the height of the component in the example

Runout #

Runout tolerances differ from both circularity/cylindricity and concentricity tolerances in that they constrain peak-to-peak deviation of the surface of one feature when it is rotating about a datum axis. (No fitting of bounding circles or cylinders or of effective central axes is required.) Runout tolerances are thus helpful for tolerancing components that must rotate relative to other components while maintaining a certain amount of clearance — for example, a shaft turning within a cylindrical cavity. Runout is also important for ensuring cutting tool performance — in a milling tool or drill for example, limiting runout enables clean cuts to be made, as the tool will not periodically collide with the workpiece.

Circular runout #

  • Runout considers how the surface profile of an object varies as it rotates about a specified axis
    • Useful for specifying performance of rotating machinery, cutting tools etc.
  • Circular runout:
    • Imagine placing a dial gage on the surface of a cylindrical feature
    • Peak-to-peak variation of the reading as it rotates is circular runout
    • Circular runout tolerance must not be exceeded at any location along the axis of the feature

A circular runout tolerance limits the peak-to-peak deviation of points on any given circumference of a cylindrical feature, when it rotates about the specified datum axis. In the example shown on above, for example, circular runout could be measured by clamping the component in a chuck to establish datum A, then rotating the component with a dial gage in contact with the toleranced feature. The peak-to-peak movement of the indicator would need to be less than the tolerance specified. A circular runout tolerance must be satisfied independently at any circumference on the cylindrical feature to which it applies (not just the location at which the tolerance arrow appears to point).

Planar features #

  • Can also apply to planar features perpendicular to specified datum axis
  • Runout tolerance must not be exceeded at any radial location

Cylindrical, or total, runout #

  • Total runout is more restrictive than circular runout
  • Imagine taking dial gage readings at many locations along length of feature
    • Gage readings referenced to the rotation axis (axis = 0)
  • Peak-to-peak variation of all readings taken together must not exceed tolerance value
    • This is unlike circular runout, where each axial location is independent

This is the “3D” version of circular runout: the datum is established, and the component rotated, and the total peak-to-peak variation across all axial positions is found (e.g. by scanning a dial gage along the component as it rotates). Total runout will usually be larger than circular runout; the example below illustrates why:

Total runout for planar features #

  • Total runout can be applied to a planar feature perpendicular to the datum axis
  • Tolerance value must not be exceeded when considering overall peak-to-peak positional variation of all radial locations together
  • Often, a rotating component will be mounted at two locations (e.g. on two bearings at opposite ends of a shaft). Then, a runout tolerance will be specified relative to both of those datums using the convention illustrated below. The runout using datums A and B in this example is likely to be different from the runout that we would measure using only one of the datums, because the rotational axis established could change position as more points on the component’s surface are included in the fitting process.

Multiple datums #

  • It is common for rotating components to be held in bearings at both ends
  • Associate a datum feature with each end of the component
  • Rotation axis for evaluating runout can be based on these two datums together
    • Fit the axis to points measured along both datums
    • Reflects operation of component more accurately

Range of GD&T symbols #

Examples #

Perpendicularity #

  • Add perpendicularity tolerances to show:
    • 40-high left-hand edge, perpendicular to datum A, tolerance zone 0.2 in size
    • Hole axis perpendicular to datum A, tolerance zone 0.2 dia at MMC

Center Position #

Symmetry #