Position tolerance and bonus tolerance, with a worked hole example

What position tolerance controls

Position is a location control. It defines a zone around the theoretically exact location of a feature and requires the feature axis or centre plane to stay inside it. The exact location comes from basic dimensions measured from a datum reference frame.

For a round hole with a diameter symbol in the tolerance cell, the zone is a cylinder. The axis of the hole must lie within that cylinder over the full depth of the feature. For a slot or a rectangular feature, the zone is usually two parallel planes or a rectangular box, depending on the symbol.

Position does not control the size of the hole. Size is controlled by the limit dimensions. Position does not control surface finish or material. It controls location, and it can also limit orientation because the zone has a direction.

Reading the callout

An illustrative callout is a hole dimension of 8.00 to 8.20 mm with a frame that reads: position, diameter 0.20, M, datum A, datum B, datum C. The diameter symbol means a cylindrical zone. The 0.20 is the zone diameter at maximum material condition. The M means the tolerance can grow as the hole grows.

The datums are the origin. A is the primary face, B and C locate the hole in the other two directions. The basic dimensions from B and C define the true position. There is no plus or minus on those basic dimensions because the zone carries the variation.

If the M is missing, the callout is regardless of feature size. The 0.20 mm zone applies whether the hole is 8.00 or 8.20 mm. That is the safer default when the function does not depend on clearance.

Some drawings add a projected tolerance zone for a hole that receives a stud or a pressed pin. The zone is projected above the surface by a stated height, so the axis is controlled where the mating part actually sits. Without the projection, a hole can pass at the surface and still cause the stud to bind at the top of the stack.

The bonus tolerance arithmetic

Bonus tolerance is the difference between the actual size and the size at the stated material condition. For a hole at MMC, MMC is the smallest permitted diameter. If the hole is made larger, the axis can move further and still leave the same clearance for the fastener.

The table below uses the illustrative callout above. The size limits and the stated position tolerance are assumed for the example. The arithmetic is the point, not the particular numbers.

When LMC is the right modifier

The L modifier works in the opposite direction. For a hole, least material condition is the largest permitted diameter. The position tolerance is smallest at that size and grows as the hole gets smaller.

This is useful when a minimum wall or a minimum distance to an edge is the concern. At the largest hole, the wall is thinnest, so the location needs the tightest control. As the hole shrinks, there is more material left and more room for location variation.

The same logic applies to a pin or a boss, where the roles of maximum and least material are reversed. The important step is to decide which condition represents the worst case for the function, then apply the modifier that protects it.

Datum shift is a separate allowance

Bonus tolerance applies to the toleranced feature. Datum shift applies to a datum feature referenced at a material boundary. If datum B is a hole referenced at M, the datum feature can move within the clearance between the hole and its simulator. That movement shifts the whole datum reference frame.

Datum shift and bonus can both apply on the same callout, and they are not the same thing. Bonus comes from the size of the toleranced hole. Datum shift comes from the size of the datum hole and the clearance to the gauge or mandrel.

The distinction matters at inspection. A functional gauge naturally includes both effects. A CMM calculation has to apply them separately and in the right order. If the drawing invokes a datum boundary, the inspection plan should say how the shift is handled.

How to inspect a position callout

A functional gauge is the simplest method when the callout is at MMC. The gauge pin or gauge feature is made to the virtual condition boundary, which combines the maximum material size with the geometrical tolerance. For the illustrative hole, the virtual condition is 8.00 minus 0.20, or 7.80 mm. A pin of that size checks the combined effect in one pass.

A CMM measures the axis and the size separately, then calculates the available bonus. The axis result must be compared with the total allowed zone, not the stated zone. The alignment must follow the datum order on the drawing, or the result is from a different reference frame.

For a critical feature, check the gauge repeatability before accepting the result. A position callout at the edge of the process can produce a pass or fail decision that depends more on the fixture than on the part.

• Confirm the modifier before calculating any bonus.
• Measure size and axis at the same cross-sections.
• Apply the datum order from the frame.
• Compare the axis result with the total allowed zone.
• Record the method and the alignment in the report.

Common errors

The first error is adding bonus when the frame has no modifier. Without M or L, there is no bonus. The second is adding the bonus to the size tolerance. That lets a hole exceed its size limit, which the standard does not permit. The third is applying the bonus twice, once in the CMM report and again in a spreadsheet.

The fourth is ignoring datum shift when the datum is referenced at a boundary. The fifth is using a position callout without basic dimensions, which leaves the true position undefined. The sixth is assuming that MMC is the default. It is not. The modifier has to be on the drawing.

A seventh error is a zone that is larger than the clearance the assembly actually has. Bonus can make a hole pass a drawing that will not accept the fastener at the worst case. The tolerance stack should start from the function, not from the inspection result.

Position or coordinate tolerance?

Use position when the feature has a functional location and the zone shape should match the clearance. A round hole with a round zone is a better model of a fastener than a square plus or minus box. Use position with M when the hole only needs to accept a pin and the size can vary.

Use a coordinate tolerance for a simple feature where the location is not critical and the general tolerance is enough. Use profile for a curved surface or an edge that needs form as well as location. Use runout for a rotating surface.

The choice should be visible in the drawing and in the inspection plan. A position callout with the wrong modifier, or a basic dimension that nobody checks, is more expensive than a simple coordinate tolerance because it looks rigorous without being functional.

If the drawing is a legacy coordinate scheme, do not convert it to position without recalculating the zone. A square plus or minus box and a cylindrical position zone accept different parts, even when the numbers look similar.