• 1-888-TEC-EASE
  • Outside USA: 1-716-785-6015
Free Tec-Ease Mug GD&T Textbooks GD&T Training GD&T Public Seminars GD&T Computer Based Training GD&T Reference Material
Protect Your Boundaries with Profile
(In accordance with Y14.5M-1994 standard)

PDF of this Tip

Most holes will have both a size and position tolerance. This combination causes the hole to "act" larger and smaller than the actual size from a fit and shift stand point. The smallest the hole may act is called the inner boundary. The largest the hole may act is called the outer boundary. The inner boundary represents the closest the surface of the hole may ever get to the basic location relative to the referenced datums. This boundary often affects the fit of mating parts. The outer boundary represents the farthest the surface of the hole may ever get from the basic location relative to the referenced datums. This boundary often affects the shift or slop between mating parts. The dynamic tolerancing diagrams illustrated below show how the boundaries are affected when position and profile tolerances are applied to a hole. The solid area indicates all of the tolerance of both size and position (including bonus tolerance allowed by modifiers) allowed on the hole. The blue area in each example shows the allowable tolerance when position at RFS is used. The green areas show additional or bonus tolerance.

In this first example Regardless of Feature Size is implied. This is the most restrictive (expensive) control. Although the size may not be less than 9.8mm or greater than 10.2mm, the hole may act like 9.5mm to 10.5mm. Any holes made from 9.5mm to 9.8mm or from 10.2mm to 10.5mm should be rejected for size even though they may function.

By using the MMC modifier, a bonus is allowed that could permit the hole to be out of position by as much as 0.7mm. Although the inner boundary did not change, the outer boundary has grown to 10.9mm since a 10.2mm size hole may be out of position by as much as 0.7mm due to bonus tolerance. This could cause shift problems if this hole is being used to locate parts in an assembly.

By using the LMC modifier, a bonus is allowed that could once again permit the hole to be out of position by as much as 0.7mm. This time the outer boundary did not change from the first RFS example, but, the inner boundary could be as small as 9.1mm since a 9.8mm size hole may be out of position by as much as 0.7mm due to bonus tolerance. This could cause fit problems in an assembly.

Although historically profile of a surface has not been widely used to locate holes, it is acceptable and offers many advantages. When the size and locating dimensions are basic, profile controls both size and position. The green areas represent the additional tolerance realized if profile rather than position at RFS is used. The closer to 9.5mm or 10.5mm production makes the hole, the better the position of the hole must be. Production is given the greatest position allowance of 0.5mm if they produce holes at 10mm. This gives production the most possible tolerance while protecting both the inner and outer boundaries. It also encourages production to keep their process centered at 10mm. Designers often use position at MMC for holes because it provides bonus tolerance while assuring fit between mating parts. What they often miss is the resulting shift that may occur between mating parts. Using profile of a surface in this manner provides the most tolerance while protecting an assembly’s fit and shift.

Back to Tips Tip added Feb 1999