309 Chapter 8 Position Tolerancing Fundamentals Copyright Goodheart-Willcox Co., Inc. threaded hole and the clearance hole depends on the clearance between the hole and the fastener. The difference in diameter between the clear- ance hole and the fastener is the total amount of posi- tion tolerance that may be split between the threaded hole and the clearance hole. When evenly divided, the two features may move equal distances on oppo- site sides of the true position, just as the fi gure shows. Example Calculation Problem: Required: Calculate the position tolerance for a fi xed fastener application. Given information: Specifi ed hole diameter: .296″ ±.003″ Fastener diameter: .250″ MMC Solution: T = (H – F)/2 T = (.293″ – .250″)/2 T = .043″/2 T = .0215″ Just as for a fl oating fastener condition, the solu- tion of a fi xed fastener problem requires that at least two parameters be known. The fi xed fastener for- mula can be easily used to solve for a hole size when the fastener and a preselected tolerance are known. Simple mathematics is used to solve for the hole size. T = (H – F)/2 2T = H – F 2T + F = H – F + F 2T + F = H H = 2T + F Additional Tolerance (Bonus Tolerance) The previously explained formulas, when used for calculating position tolerances, result in a numer- ical value that is based on a fastener passing through the holes. Position tolerances may also be calculated for the purpose of protecting the edge distance or spacing between holes. The calculated value is typ- ically the amount of tolerance shown in the feature control frame. Depending on the design function, the tolerance will be specifi ed as applicable RFS, at MMC, or at LMC. When applicable RFS, no material condition modifi er is shown. When the tolerance is applica- ble at MMC or LMC, the feature control frame will include the appropriate MMC or LMC material con- dition modifi er. When the MMC modifi er is shown, the tol- erance value in the feature control frame applies when the controlled feature is produced at the MMC size. At any size other than MMC, the allowable tolerance zone is increased. The allowable increase in the tolerance is directly related to the depar- ture of the controlled feature from its MMC size. The allowable increase in the tolerance is known as additional tolerance, sometimes called bonus tolerance in industry. The allowable position tolerance for a produced feature is equal to the specifi ed position tolerance plus the applicable additional tolerance. When using the surface (boundary) method, the amount of addi- tional tolerance depends on the actual produced size of the feature. When using the axis method, the size of the unrelated actual mating envelope is used to calculate additional tolerance. The size of the unre- lated actual mating envelope for a hole is the size of an inscribing cylinder. Therefore, the size of the unrelated actual mating envelope is affected by fea- ture size and form variations. Because the form of each feature shown in the following illustrations is drawn without variation, the size of the hole and the size of the unrelated actual mating envelope are the same. It is possible to calculate the allowable additional tolerance for all of the possible produced sizes, but the exact allow- able additional tolerance for a particular feature is unknown until the feature is produced. T = H – F 2 T is the position tolerance applied to both parts Tolerance zone (T) H – F Basic dimension True position True position Axis of clearance hole Axis of threaded hole Datum features can remain aligned Goodheart-Willcox Publisher Figure 8-17. With the shown fi xed fastener formula, the difference in diameter between the clearance hole and the fastener is divided evenly between the position tolerances for the two parts.