Designing for machining round holes Introduction There are various machining processes available for making of round holes. The common processes are: drilling, reaming and boring. Drilling is a machining process used to create round holes in a work piece. Figure M3.3.1 shows the drilling operation. Figure M3.3.1: Drilling operation Reaming is a process used to enlarge the existing round hole to the required accurate size and smooth finish to the surface of the hole by using an end cutting tool. The tool used for reaming operation is called reamer. Figure M3.3.2 illustrates the reaming operation. Figure M3.3.2: Reaming operation Boring is a machining operation that enlarges an existing hole by removing metal with a rigidly mounted single-point cutting tool. This operation is carried out either by rotating the work piece of the tool on the center line of the hole or feeding the tool into the work parallel
to the axis of rotation. In this case, the rigidity of the spindle and the boring tool determines the accuracy of the cut. Application of hole machining processes Holes are produced by machining operation when other methods such as casting, forging, molding, extruding, stamping, etc. fails to produce the hole or doesn t produce with necessary size, accuracy or other functional requirements. When specific requirements such as accuracy of diameter, location, straightness, or direction are required in components, bored holes are recommended. Typical parts with bored holes include gearboxes, sewing-machine arms, bearings, hydraulic cylinders, pump housings, die sets for metal stamping, machine-tool frames and many other machine components. Suitable materials Since it is easy to use carbide, ceramic and diamond-tipped single point cutting tools in the hole boring process, it is possible to process difficult to machine materials. With such type of material, machine speed and feed must be reduced with reduced machinability. Design recommendations The best way to minimize the cost of hole machining operation is simply to avoid them. Creating the hole by other means like cast, mold or pierce which will satisfy the functional requirements of the part is recommended. Though drilling operation is a roughing operation, other surface finishing operation reaming or boring operation is not recommended unless it is specified. Drilling: The recommended design rules for drilled holes are as follows: The drill bit should be always perpendicular to the drilling surface. This avoids the starting problems and also helps in ensuring the proper location of the hole.(refer Figure M3.3.3)
Figure M3.3.3: Entrance and exit surface should be perpendicular to the drill bit. The axis of the drill should always perpendicular to the exit surface. This avoids breakage problems as the drill leaves the work. (Refer Figure M3.3.3) Interrupted cuts are to be avoided when straightness of hole is important. If at all necessary, it is advised to use a guide bush at each re-entry surface. If holes with intersecting openings are unavoidable, the center point of the drill must remain in the work piece throughout the cut.(refer Figure M3.3.4) Figure M3.3.4: Center point of the drill in the work throughout the cut For economic reason, it is always preferred to use standard drill sizes whenever possible. Extra cost will be added to the part for drill grinding if nonstandard drills are used. Through holes are preferable than blind holes. It provides clearance to the tool and chip in secondary operations like reaming, tapping, or honing. The drill bit always generates pointed holes in blind holes. Flat bottoms are costlier in blind holes as secondary operations are required.(refer Figure M3.3.5)
Figure M3.3.5: Use standard drill-point angles for bottoms Recommended depth of the hole is maximum 3 times that of the diameter of the hole. If it is more, it creates chip clearance problems and the possibility of deviations from straightness. Special tooling, equipment and techniques are used for deep hole drilling. For example, Gun barrel bored holes can be as deep as 5 times that of the hole diameter. Deeper holes are possible but can cause tool deflection and breakage problems. For deep, narrow holes, consider stepped diameters as shown in Figure M3.3.6. Figure M3.3.6: Avoid deep, narrow holes A minimum diameter about 3mm is preferred for hole drilling as small diameter drills are more prone to breakage. For large finished hole, cast in holes are preferred in the work piece prior to the drilling operations. This saves material and reduces the power required for drilling. If several drilled holes are to be made in the part, it is required to dimension them from the same surface to simplify fixturing. (Refer Figure M3.3.7)
Figure M3.3.7: Locate all holes from one surface in so far as possible. In the design and drawing of holes, rectangular coordinates are to be used than angular coordinate to designate the location of the hole. It will be easier for the machinist to use in laying out the part or a drill fixture. (Refer Figure M3.3.8) Figure M3.3.8: Rectangular coordinates are preferable to angular coordinates for showing hole locations in drawings. Design of parts should be such that all holes can be drilled from one side or from the few number of sides. This would simplify the tooling and minimize handling time. It is required to provide space for drill bushing close to the work piece surface to be drilled.(refer Figure M3.3.9)
Figure M3.3.9: Allow room for drill bushings close to the work piece surface to be drilled Standard size holes, fasteners, and other screw threads need to be used to minimize the number of drill spindles and drill changes. For multiple-drilling arrangements as a rule of thumb the spacing between the holes should not be less than 19 mm for small holes of 6-mm diameter or less. Although in some cases 13 mm is possible. Reaming The following design practices are recommended for reaming: 1. In the practice guide, bush is used for reaming operation when hole location is critical. But if the hole location or alignment is not proper, it is not advisable to depend on reaming to correct location or alignment discrepancies unless the discrepancies are very small. 2. Intersecting drilled and reamed holes are recommended to avoid if possible, to prevent tool breakage and burr-removal problems. (Refer Figure M3.3.10) Figure M3.3.10: Avoid intersecting drilled and reamed holes if at all possible
3. If a blind hole requires reaming, it is required to allocate for extra drilled depth to provide room for chips. (Refer Figure M3.3.11) Figure M3.3.11: Provide extra hole depth if blind holes are to be reamed. Boring Recommended design practice for boring are as follows: 1. Avoid designing holes with interrupted surfaces. Interrupted cuts tend to throw holes out of round and cause vibration and tool wear. 2. Designing of holes with a maximum depth-to-diameter ratio of 4:1 or 5:1 is recommended. With higher ratio, accuracy will be lost due to boring bar deflection. In exceptions, diameter ratios of 8:1 can be designed with carbide boring bars. It is recommended to use stepped diameters to limit the depth of the bored surface if deep holes are unavoidable.(refer Figure M3.3.12) Figure M3.3.12: Avoid deep, narrow holes 3. Blind holes are to be avoided. If blind holes are needed, then depth of the rough hole should be deeper than the bored portion by an amount equal to at least onefourth the hole diameter. (Figure M3.3.13)
Figure M3.3.13: Blind holes to be bored should be one-fourth diameter deeper than the final bored hole to allow space for chips. 4. Boring is more expensive than drilling and reaming. Recommended only if it is extremely necessary. 5. The part must be rigid enough to eliminate deflection or vibration which is generated as a result of cutting forces. Sufficient precaution need to be taken in the work piece and fixture design to avoid deflection of the part when it is clamped in the fixture. Otherwise machined surfaces will be off location when the part springs back from its clamped position. Dimensional factor The accuracy and straightness of drilled holes depends upon the correctness of drill sharpening. The play and lack of rigidity in the typical drill spindle also affect the accuracy and straightness of drilled holes. Drill bushing also affects the accuracy. Thermal coefficient of expansion of material to be drilled has influence on diameter close tolerance hole. For example: Aluminum which expands during drilling and then contracts on cooling.
Recommended tolerances Table M3.3.1 to M3.3.3 provides the recommended tolerances of drilled, reamed, and bored holes. Table M3.3.1: Recommended Tolerances for Diameters of Drilled Holes (Source: Design for Manufacturability Handbook by James G Bralla, 2nd Ed) Hole diameter, mm Recommended tolerance, mm 0 to 3 + 0.08, - 0.025 Over 3 6 + 0.10, - 0.025 Over 6 13 + 0.15, - 0.025 Over 13 25 + 0.20, - 0.05 Over 25 50 + 0.25, - 0.08 Over 50 100 + 0.30, - 0.1 Table M3.3.2: Recommended Tolerances for Diameters of Reamed Holes (Source: Design for Manufacturability Handbook by James G Bralla, 2nd Ed) Hole diameter, mm Recommended tolerances, mm 0 13 ± 0.013 to ± 0.025 Over 13 25 ± 0.025 Over 25 50 ± 0.05 Over 50 100 ± 0.08
Table M3.3.3: Recommended Tolerances for Diameters and Depths of Bored Holes (Source: Design for Manufacturability Handbook by James G Bralla, 2nd Ed) Hole diameter, mm Normal tolerance, mm Close tolerance, mm Precision production boring 0 19 ±0.025 ± 0.005 Over 19 25 ± 0.04 ± 0.005 Over 25 50 ± 0.05 ± 0.01 Over 50 100 ± 0.08 ± 0.02 Over 100 150 ± 0.1 ± 0.025 Over 150 300 ± 0.13 ± 0.05 Jig boring 0 25 ± 0.013 ± 0.0025 Over 25 ± 0.025 ± 0.005 Depth (blind or partially bored holes) Precision production boring ± 0.08 ± 0.013 Jig boring ± 0.025 ± 0.013