Profile tolerance: surface and line, and how to use them well

What profile does

Profile tolerance defines a boundary around a true profile. The true profile is the theoretically exact shape, defined by basic dimensions, a CAD model or a combination of both. The tolerance zone is the space between two boundaries offset from that true profile.

The feature must lie inside the zone. Because the zone has a shape, a size and a position, profile can control form, orientation and location at the same time. That makes it one of the most powerful controls in GD&T, and one of the easiest to misuse.

Profile is common on curved covers, sealing faces, cam tracks, connector shells, castings and moulded parts. It is also useful on a complex edge where a set of plus or minus dimensions would be difficult to read and impossible to inspect.

Surface profile and line profile

Profile of a surface applies to the entire surface. The zone is two surfaces offset from the true surface, and every point on the real surface must lie between them. It is the control to use when the whole form matters.

Profile of a line applies to each cross-section separately. The zone is two lines offset from the true line, and each section is checked on its own. It does not control how the sections relate to each other along the length. A part can pass every line section and still twist or wave between them.

Line profile is useful for a varying cross-section, such as an extrusion or a rolled edge, or as a refinement on a surface where the section shape is the critical feature. It is not a cheaper substitute for surface profile when the whole surface must be controlled.

The zone and its default disposition

Unless the drawing says otherwise, the profile zone is bilateral and equally disposed around the true profile. A tolerance of 0.4 mm means 0.2 mm on each side of the true profile. That is the default in both ISO 1101 and ASME Y14.5.

Sometimes the function is not symmetric. A sealing surface may need more material on one side, or a clearance may only exist in one direction. In that case the drawing has to state an unequal disposition. ISO 1101 uses a modifier for this; ASME uses a similar unequal disposition callout. The exact syntax matters, so follow the standard named on the drawing.

A unilateral profile is a special case of unequal disposition where the whole zone sits on one side of the true profile. It is not the default, and it should not be inferred from a note that says the surface may only move inward.

If the control wraps around an edge or a section, use the all-around symbol and make the extent clear. A profile frame on one view may be read as applying only to the visible edge. The all-around symbol removes that ambiguity.

Profile with and without datums

A profile callout with no datum references controls form only. The zone can float in location and orientation, so the surface can be the right shape and still be in the wrong place. That is sometimes enough for a cosmetic surface, but it is rarely enough for a mating feature.

Add datums and the zone is fixed in space. Profile then controls location as well as form and orientation. A profile callout with three datums is a complete location control for a complex surface, and it can replace a stack of linear dimensions.

The datum order still matters. Profile measured from a different primary datum can accept a different part. The inspection alignment should follow the frame, not the convenience of the CMM operator.

Two-tier profile callouts

A two-tier or composite profile callout separates the location requirement from the form requirement. The upper tier uses datums and a larger zone to locate the surface. The lower tier uses a smaller zone, often without datums, to refine the form within that location.

This is useful when a surface must be in the right place and also smooth. A single tight profile zone would force the process to hold location and form at the same tight value. A two-tier callout lets the supplier locate the surface to a workable band and then control the local shape more closely.

The lower tier must be smaller than the upper tier, otherwise it adds nothing. The datums in each tier should be read carefully. A lower tier without datums is a form refinement, not a second location requirement.

When profile is the right control

Use profile when the true shape is not a simple plane, cylinder or line. A curved cover, a cam profile, a seal groove or a complex edge is a natural fit. Use it when form, orientation and location need to be controlled together and a stack of linear dimensions would be ambiguous.

Do not use profile for a simple flat face that only needs to be flat. Flatness is clearer and easier to inspect. Do not use it for a hole pattern that needs position. Position is the better model for a cylindrical zone around an axis.

Profile is also useful for a part made from a 3D model, because the model is the true profile. The drawing can reference the model and apply a profile zone to the surfaces that matter. That is cleaner than trying to dimension a free-form surface with coordinates.

Inspecting a profile

A profile tolerance needs a measurement that covers the surface, not a handful of points chosen by the inspector. A CMM scan, a laser scan or a structured light scan can compare the real surface with the true profile. The report should state the point density and the alignment.

A few points can miss a local bulge or a dip between them. For a sealing surface, the gaps between points are where a leak path can start. For a cosmetic surface, a low point may be visible even if the measured points pass.

The inspection plan should also state how the true profile is defined. If it comes from a CAD model, record the model revision. If it comes from basic dimensions, record the table or the formula. A profile result without a controlled true profile is not evidence of conformity.

• Use a measurement method that covers the full surface.
• Record the model or basic dimension revision.
• State the datum alignment for each tier.
• Check the point density against the smallest feature.
• Report the maximum deviation and its location, not just a pass or fail.

Drawing rules that prevent disputes

Show the true profile with basic dimensions or a model reference. Put the profile frame on the surface or on a leader that clearly points to it. If the control applies all around a section, use the all-around symbol and make the extent clear.

State the disposition if it is not bilateral and equal. State the datums in the order that matches the function. If a two-tier callout is used, make the upper and lower zones visibly different and check that the lower zone is smaller.

Finally, check that the process can hold the zone. A profile tolerance on a casting is not the same as a profile tolerance on a machined surface. The supplier needs to know whether the surface is used as cast, machined or coated, because each route has a different variation.