Machinery's Handbook, 31st Edition
Allowances and Tolerances 641 When unilateral tolerances are used, one of the following three methods should be used to express them: 1) Specify, limiting dimensions only as
Diameter of hole: 2.250, 2.252 Diameter of shaft: 2.249, 2.247 2) One limiting size may be specified with its tolerances as
Diameter of hole: 2.250 + 0.002, –0.000 Diameter of shaft: 2.249 + 0.000, –0.002 3) The nominal size may be specified for both parts, with a notation showing both allow ance and tolerance, as Diameter of hole: 2 1 ⁄ 4 + 0.002, – 0.000 Diameter of shaft: 2 1 ⁄ 4 – 0.001, – 0.003 Bilateral tolerances should be specified as such, usually with plus and minus tolerances of equal amount. An example of the expression of bilateral tolerances is 2 ± 0.001 or 2 Application of Tolerances.— According to common practice, tolerances are applied in such a way as to show the permissible amount of dimensional variation in the direction that is less dangerous. When a variation in either direction is equally dangerous, a bilat- eral tolerance should be given. When a variation in one direction is more dangerous than a variation in another, a unilateral tolerance should be given in the less dangerous direction. For nonmating surfaces, or atmospheric fits, the tolerances may be bilateral or unilat eral, depending entirely upon the nature of the variations that develop in manufacture. On mating surfaces, with few exceptions, the tolerances should be unilateral. Where tolerances are required on the distances between holes, usually they should be bilateral, as variation in either direction is normally equally dangerous. The variation in the distance between shafts carrying gears, however, should always be unilateral and plus; otherwise, the gears might run too tight. A slight increase in the backlash between gears is seldom of much importance. +0.001 –0.001 One exception to the use of unilateral tolerances on mating surfaces occurs when tapers are involved; either bilateral or unilateral tolerances may then prove advisable, depending upon conditions. These tolerances should be determined in the same manner as the toler ances on the distances between holes. When a variation either in or out of the position of the mating taper surfaces is equally dangerous, the tolerances should be bilateral. When a variation in one direction is of less danger than a variation in the opposite direction, the tolerance should be unilateral and in the less dangerous direction. Locating Tolerance Dimensions.— Only one dimension in the same straight line can be controlled within fixed limits. That dimension is the distance between the cutting surface of the tool and the locating or registering surface of the part being machined. Therefore, it is incorrect to locate any point or surface with tolerances from more than one point in the same straight line. Every part of a mechanism must be located in each plane. Every operating part must be located with proper operating allowances. After such requirements of location are met, all other surfaces should have liberal clearances. Dimensions should be given between those points or surfaces that it is essential to hold in a specific relation to each other. This restric tion applies particularly to those surfaces in each plane that control the location of other component parts. Many dimensions are relatively unimportant in this respect. It is good practice to establish a common locating point in each plane and give, as far as possible, all such dimensions from these common locating points. The locating points on the drawing, the locating or registering points used for machining the surfaces and the locating points for measuring should all be identical.
Copyright 2020, Industrial Press, Inc.
ebooks.industrialpress.com
Made with FlippingBook - Share PDF online