Machine Designers Reference. J. Marrs
limits and fits are specific to cylindrical features and parts (holes and shafts), but these fits can also be applied to non-cylindrical features and parts like rectangular slides and pockets. When selecting fits, one must consider the loading, speed, length of engagement, temperature, and lubrication conditions of the assembly. The designer is free to use the standard fits or specify different tolerance combinations to achieve the desired result.
•Oberg, Jones, Horton, Ryffel, Machinery’s Handbook, 28th Ed., Industrial Press, New York, NY, 2008
•ANSI B4.1: “Preferred Limits and Fits for Cylindrical Parts”
•ISO 286: “ISO System of Limits and Fits”
TYPES OF FITS AND THEIR LIMITS
Fits refer to the amount of clearance or interference between mating parts. There are three basic types of fits: clearance fits, transition fits (chance of either clearance or interference), and interference fits. Each fit specifies two sets of tolerances, or limits of size: one for the hole or external feature, and one for the shaft or internal feature. These tolerances are applied to the nominal feature size when parts are designed ‘line to line’ (without clearance at nominal size), and can be either positive or negative. Tolerance designations are represented by a class letter followed by a tolerance grade number. The hole or internal feature’s tolerance class is represented by a capital letter, and the shaft or external feature’s tolerance class is represented by a lowercase letter. The larger the grade number, the wider the tolerance range. On part drawings, tolerances are given using the class letter and grade number designation, the numerical tolerances themselves, or both. For example, a hole and pin are designed nominally ‘line to line’ and the designer wishes to apply a press fit to the joint. The pin is a commercial item with an m6 tolerance. The designer would then need to find out what tolerance designation to apply to the hole. This will be solved in the next few paragraphs.
ANSI B4.1 governs preferred limits and fits in inch units. The ANSI system uses descriptive two-letter designations to represent fits. Each type of ANSI fit has a series of possible grades, each represented by a number. The grade indicates the degree of tightness of the fit. ANSI fit grades are not the same as tolerance grades. A graphical representation of the ANSI standard fits is shown in Figure 3-1. ISO 286 governs preferred limits and fits in metric units. The ISO system of fits specifies preferred tolerance combinations for each fit type. Table 3-1 lists some commonly used fits, their typical use, and their graded tolerance designations from both the ANSI and ISO standards. Revisiting the example with the m6 tolerance pin, it can be seen from Table 3-1 that a locational interference fit joint can have a tolerance combination of H7/p6. Because the pin has an m6 tolerance rather than the standard p6, some calculation will be required to adjust the tolerances. That will be discussed further in the next paragraph.
Figure 3-1: Graphical Representation of ANSI Standard Fits
Tolerance grades, or limits of size, are graduated based on the size of the feature being toleranced. Larger features will have larger tolerance ranges. Standard ANSI tolerance grades and their numerical values are shown in Table 3-2. IT tolerance grades and their values are given in Table 3-3. The graded tolerance values corresponding to a given fit letter and grade number combination are normally obtained either through the use of charts or are built in to drafting (CAD) software. Some selections from these charts are provided in Tables 3-5 through 3-10. To use the tolerance charts, the designer must look up first the value corresponding to the letter designation. The tolerance values are then located on the letter designation chart at the intersection of the feature size row and number designation column.
Again revisiting the example with the m6 pin, the numerical limits of size for each tolerance designation can be found using Tables 3-5 through 3-10. First look up the limits of size for the diameter of the hole and pin, assuming that they are the standard locational interference fit tolerances of H7/ p6. If the pin diameter is 0.25 inch, the chart limits of size values for H7 in that size are +0.0006 / −0. For p6, the limits of size are +0.001 / +0.0006. Calculate the maximum and minimum interference between an H7 hole and a p6 pin using those limits: 0.001 / 0. For more information on performing tolerance analysis, please refer to Section 3.3. Now apply these interference values to the m6 pin and its limits of size to get the target tolerances for the locational interference fit hole. Use the tables to find the limits of size for the m6 pin with 0.25 inch diameter: +0.00059 /+0.00024. Because the least calculated interference should be 0, the upper limit for the hole to fit this oversized pin should be +0.00024. The upper limit of interference is 0.001, so the lower limit for the hole should be −0.00041.
If the designer prefers to use a tolerance designation instead of numerical values for the hole, a standard designation should be sought for limits of size of +0.00024/ −0.00041 for a diameter of 0.25 inches. Using the tables, the closest designation to those limits of size is K7 for that size of hole. Designation K7 at 0.25 inches diameter has limits of size of +0.0001 / −0.0005. A K7 hole combined with an m6 pin in that size will result in a fit that allows between 0.00014 and 0.00109 inches of interference in the joint. The standard fit allows between 0 and 0.001, so this modified fit should work acceptably. The advantage of using the system of limits and fits is that once a fit is calculated, the designations are easily remembered and reused. A standard dowel pin has an m6 designation, so the designer can easily remember (or record) that a K7 hole will yield a satisfactory interference fit. Numerical values need not be recalled once a fit is defined. When the designer has control over the tolerances applied to both parts, using standard fit designations can speed the process.
When using force fits, the pressure required to assemble the parts can be estimated using pressure factors. The stress resulting from force fits should be calculated for a more accurate result. It is essential that the elastic limit of the parts in a force fit assembly not be exceeded because that would result in a loosening of the fit. Consult the recommended resources for calculation guidance.
Table 3-1: Commonly Used Limits and Fits
Table 3-2: Selected ANSI Tolerance Grades
Table 3-3: Selected International Tolerance (IT) Grades
MACHINING TOLERANCES
Choice of tolerances should always take into account the manufacturing process capability as well as functional requirements. Every machining process has a tolerance capability. This can vary by machine and machinist. Some machining tolerances are given in ANSI B4.1. Table 3-4 illustrates some typical tolerance grades achieved by various machining processes. The values shown are intended only as a guide and vary depending on machine tool and operator. Tables 3-2 and 3-3