machining process.pptx

Introduction machining processes.

General Design rules for machining.

Dimensional Tolerances and surface roughness.

Design For machining.

Ease –redesigning of components for machining ease with suitable examples.

General design recommendations for machined parts

1. MACHINING PROCESSES Dr.M . Bala Theja,M.Tech,Ph.D Associate Professor Department of Mechanical Engineering

2. CONTENTS Introduction machining processes. General Design rules for machining. Dimensional Tolerances and surface roughness. Design For machining. Ease –redesigning of components for machining ease with suitable examples. General design recommendations for machined parts.

3. INTRODUCTION Machining is the manufacturing process by which parts can be produced to the desired dimensions and surface finish from a blank by gradual removal of the excess material in the form of chips with the help of a sharp cutting tool. Almost 90% of the all engineering components are subjected to some kind of machining during manufacture for semi finishing operations. It is very important to design those parts in such a way that would lead to the increase in efficiency of the machining process, enhancement of the tool life and reduction of the overall cost of machining. To achieve these targets, a brief knowledge of various machining processes is required.

4. CLASSIFICATION OF MACHINING EROSION

5. DFM for economic production Manufacturing cost is the key for economic success of the product . Economic success depends on the profit margin on each unit sale and the volume of the units sold . Profit margin and the sales volume depends on product quality . Successful design ensures high product quality while minimising the manufacturing cost. DFM helps you to reduce the manufacturing cost without sacrificing the product quality through the following: Simplicity of the product Standard materials and components Standard design of the product Specify liberal tolerances Use most machinable materials available in local market. Avoid secondary operations or finishing operations

6. DESIGN RULES FOR MACHINING EASE 1. The amount of machining should be reduced , as far as possible, by assigning size tolerances only for fits between mating surfaces ; all other elements should have free dimensions. Parts may be obtained without any machining if precise methods of blank manufacture are applied.

7. 2. Convenient and reliable locating surfaces should be provided to set up work piece for machining. Whenever possible, the measurement datum should be made to coincide with the set-up datum surface by proper dimensioning of the part drawing. 3. There should be sufficient rigidity of work piece so as to eliminate significant deformation in the process of machining. 4. Provisions should be made for conveniently advancing rigid, high- production cutting tools to the surface being machined . Difference in height between adjacent, rough and machined surfaces should be sufficient, making adjustment for the machining allowances, to enable the cutting tools to clear the rough surface in its overtravel.

8. 5. clearance recesses: Dimension A should be provided to allow overtravel of cutting tool whenever it is necessary.

9. 6.Parts should be designed so that several work pieces can be set up to be machined simultaneously , as shown in figure. The following considerations are important for elementary surfaces of machine parts:

10. 7. External surfaces of revolution , upset heads, flanges and shoulders should be extensively applied to reduce machining and to save metal. 8 . It is advisable to retain the centre holes on the finished components (shafts and similar parts ) that were machined between centres. 9. The elements of the shank design should be unified , whenever possible, so that the same multiple tool set-up can be employed in machining them, as illustrated in Figure.

11. 10 . –A It is a good practice to provide a spherical convex surface with a flat end surfaced. 10-B Minimize the use of different machine for a single part. Use single machine as far as possible 11. Holes: (a) through holes are to be used , wherever possible, because such holes are much more simple to machine than blind holes. The form of blind holes should correspond to the design of the tool to be employed in machining for example, with the reamer or counter bore.

12. (b) Holes should not be located closer to a certain minimum distance from an adjacent wall of the part: A ≥ D/2 + R. This distance for holes accommodating fastening bolts should be A ≥ D n /2 + R. where D n is the diameter of a circle circumscribing the nut.

13. (c) Center distances of holes should be specified, by considering the possibility of using multi spindle drilling heads . For this purpose, the location and sizes of the holes in flanges have to be unified. The number of holes and their location in a flange should be designed so that the holes can be drilled three or four spindle heads with subsequent indexing. (d) Holes to be drilled should have their top and bottom surface square to the hole axis to prevent drill breakage. (e) When several holes are located along the same axis, it is good practice to reduce the diameter of each consequent hole by an amount exceeding the machining allowance for the preceding hole. This will enable a set-up to be used in which all the holes are bored simulatenously . (f) In drilling at the bottom of a slot, their diameter should be less by 0.5-1mm than the slot width.

14. In stepped holes, maximum accuracy should be specified for the through step. Either a blind hole or a through hole should be provided on the axis in the design of concave spherical surfaces to avoid zero cutting speeds at the axis fig(a), thus preventing damage to the tool point. It is advisable to avoid recesses in holes that are to be machined on single or multiple spindle drilling machines since they complicate machining operations. Machined recesses should also be avoided by using cored recesses fig(b).

15. Threads: (a) It is advisable to use an entering chamfer on threaded holes. (b) The number of incomplete threads cut with a tap in a blind hole with no recess should be equal to three for grey iron casting and five for steel parts (c) A neck at the end of a thread is not required for milled threads. (d) Preferred thread standards should pertain, not only to the machine under consideration, but to all the threads used in the plant or branch of industry. Small diameter threads(6mm and less) should be avoided if they are cut.

16. 13. Flat surfaces: (a) The outline of a machined flat surface should ensure , as far as possible, uniform and impact less chip removal. (b) The size of a machined flat surface should be in accordance with the sizes of standard milling cutters, i.e., the width of the surfaces should be unified to suit the standard services of face mill diameters or the widths of plain milling cutters. (c) If no elements are provided for cutting tool overtravel, the transition surfaces should correspond in size and form to the cutting tool (See below figs)

17. 14. FORMED SURFACES: The radii of concave and convex surfaces should correspond to those of standard convex and concave milling cutters. 15. SLOTS AND RECESSES: Whenever possible, through slots should be employed. If through machining is possible, the end of the slot should correspond to the radius of the cutter The width and depth of slots should be specified according to the sizes of standard side milling, viz. end mills. The corner radii at the bottom of recess should be the constraint for all around recess and should correspond to the size

18. DIMENSIONAL TOLERANCE AND SURFACE ROUGHNESS FOR MACHINING PROCESSES

19. REDESIGN OF A PART FOR EASY MACHINING EXAMPLE: The following figure shows the initial design of the shaft support bracket, which is bolted to a housing to support a rotating shaft. Accurate machining is needed for the bore with high tolerance in locating the bore relative to the dowel.

20. REDESIGN OF A PART FOR EASY MACHINING ANALYSIS: Initial design had the following features that are difficult to machine: Different diameters for the dowels and bolt holes, which requires tool change and loss of time The bore and oil hole are long relative to their diameter, which require long processing steps. The is no obvious features on the outer surface to fix the part and prevent rotation during machining.

21. REDESIGN OF A PART FOR EASY MACHINING SOLUTION: For easy machining, the part was redesigned as shown in Fig. 7.18: The dowels and bolt holes have the same diameter. The center of the bore has a larger diameter than the ends to reduce length to be machined. The length of the oil hole is reduced. Flat surfaces were cast on outer surfaces for ease of location while machining.

22. REDESIGN OF A PART FOR EASY MACHINING CONCLUSION: These changes reduced the machining time from 173 to 119 seconds, (33%). Quality is also better and higher tolerances are possible.

23. MACHINING OPERATIONS PERFORMED ON LATHE

24. DESIGN RECOMMENDATIONS FOR TURNING A. STOCK SIZE AND SHAPE 1. The largest diameter of the component should be taken as the diameter of the bar stock in order to conserve material and save machining time. 2. Standard sizes and shapes of bar stock should be used in preference to special diameters and shapes. B. BASIC PART SHAPE COMPLEXITY 1. Keep the design of parts as simple as possible to reduce the number of tool stations and gauging processes required. 2. Use standard tools as much as possible by specifying standard, common sizes of holes, screw threads, knurls, slots, and so on.

25. DESIGN RECOMMENDATIONS FOR TURNING C. AVOIDING SECONDARY OPERATIONS 1. The part should be complete when cut off from the bar material. 2. Secondary operations such as slots and flats should be small and performed when the part is held in the pickoff attachment. 3. Internal surfaces and screw threads should be located at one end so that they can be performed before cutoff and without the need for rechucking

26. DESIGN RECOMMENDATIONS FOR TURNING

27. DESIGN RECOMMENDATIONS FOR TURNING D. EXTERNAL FORMS 1. The length of the formed area should not exceed two and half times the minimum WP diameter (Fig. Next slide). 2. Sidewalls of grooves and other surfaces that are perpendicular to the axis of the WP should have a slight draft of 1/2° or more to prevent tool marks when the tool is withdrawn (Fig. Next slide). 3. When turning from square or hexagonal stock, the turned diameter is the distance between two opposite flats of the stock. It is advisable to design turned parts to be about 0.25 mm or smaller than the bar stock size. 4. Avoid deep narrow grooves and sharp corners.

28. DESIGN RECOMMENDATIONS FOR TURNING

29. DESIGN RECOMMENDATIONS FOR TURNING E. UNDERCUTS 1. Avoid angular undercuts and use undercuts obtainable with traverse or axial tool movements. 2. External grooves are machined more economically than internal recesses. F. HOLES The bottom shape of blind holes should be that made by a standard drill point(Fig. Next slide). G. SCREW THREADS 1. Avoid the formations of burrs in threaded parts (Fig. Next slide).

30. DESIGN RECOMMENDATIONS FOR TURNING

31. DESIGN RECOMMENDATIONS FOR TURNING H. KNURLS 1. Knurled width should be narrow (≤WP diameter). 2. Specify the approximate number of teeth per inch, type of knurl, general size, and use of knurl. I. SHARP CORNERS 1. Avoid sharp corners (external and internal) as they cause weakness or more costly fabrication of form tools. 2. Provide a commercial corner break of 0.4 mm by 45°. 3. An internal sharp corner can be made by providing an undercut at the corner

32. DESIGN RECOMMENDATIONS FOR TURNING

33. DESIGN RECOMMENDATIONS FOR TURNING J. SPHERICAL ENDS Design the radius of the spherical end to be larger than the radius of the adjoining cylindrical surface

34. DESIGN RECOMMENDATIONS FOR TURNING K. SLOTS AND FLATS Slots are produced with a concave surface at the bottom or end (milling cutter radius)

35. DESIGN RECOMMENDATIONS FOR TURNING L. MARKING 1. Position impression marking so that roller marking tools can be used.

36. DRILLING OPERATIONS

37. DRILLING OPERATIONS

38. DESIGN RECOMMENDATIONS FOR DRILLING A. DRILLING 1. The drill entry surface should be perpendicular to the drill bit to avoid starting problems and to ensure proper location. 2. The exit surface of the drill should be perpendicular to the axis of the drill to avoid drill breakage when leaving the hole .

39. DESIGN RECOMMENDATIONS FOR DRILLING 3. For straightness requirements, avoid interrupted cuts to avoid drill deflection and breakage (Fig). 4. Use standard drill sizes whenever possible. 5. Through holes are preferable than blind holes , as they provide easier clearance for tools and chips. 6. Blind holes should not have flat bottoms because they require a secondary machining operation and cause problems during reaming.

40. DESIGN RECOMMENDATIONS FOR DRILLING 7. Avoid deep holes (over three times diameter) because of chip clearance problems and the possibility of straightness errors (Figure). 8. Avoid designing parts with very small holes if they are not truly necessary (3 mm is the desirable minimum diameter). 9. If large holes are required, it is desirable to have cored holes (casting) in the WP before drilling.

41. DESIGN RECOMMENDATIONS FOR DRILLING 10. If the part requires several drilled holes, dimension them from the same surface to simplify fixturing .

42. DESIGN RECOMMENDATIONS FOR DRILLING 11. Rectangular rather than angular coordinates should be used to designate hole locations (Figure). 12. Design parts so that all can be drilled from one side or from the fewest number of sides.

43. DESIGN RECOMMENDATIONS FOR DRILLING 13. Design parts so that there is a room for the drill bushing near the surface where the drilled hole to be started (Figure). 14. Standardize the size of holes, fasteners, and screw threads as much as possible.

44. DESIGN RECOMMENDATIONS FOR DRILLING 15. For multiple-drilling operations, the designer should bear in mind that there are limitations as to how closely two simultaneously drilled holes can be spaced (for 6 mm diameter or less, spacing should not be less than 19 mm center to center).

45. DESIGN RECOMMENDATIONS FOR REAMING 1. Even when using guide bushing, do not depend on reaming to correct location or alignment discrepancies unless the discrepancies are very small. 2. Avoid intersecting drilled and reamed holes to prevent tool breakage and burr removal problems (Figure). 3. If blind holes require reaming, increase the drilled depth to provide room for chips (Figure).

46. DESIGN RECOMMENDATIONS FOR BORING During boring, avoid designing holes with interrupted surfaces, as they cause out-of roundness errors and tool wear. 2. Avoid designing holes with a depth-to-diameter ratio of over 4:1 or 5:1 to avoid inaccuracies caused by boring-bar deflection. This ratio becomes 8:1 for carbide boring bars. 3. For larger depth-to-diameter ratios, consider the use of stepped diameters to limit the depth of a bored surface.

47. DESIGN RECOMMENDATIONS FOR BORING 4. Use through holes whenever possible. 5. If the hole must be blind, allow the rough hole to be deeper than the bored hole by ¼ hole diameter. 6. Use boring only when the accuracy requirements are essential. 7. Do not specify bored-hole tolerances unless necessary. 8. The bored part must be rigid so that deflection or vibrations caused by the cutting forces are reduced.

48. MILLING OPERATIONS

49. DESIGN RECOMMENDATIONS FOR MILLING 1. Sharp inside and outside corners should be avoided. 2. The part should be easily clamped. 3. Machined surfaces should be accessible. 4. Easily machined material should be specified. 5. Design should be as simple as possible.

50. ADDITIONAL RECOMMENDATIONS FOR MILLING 1. The product design should permit the use of standard cutter shapes and sizes rather than special ones

51. ADDITIONAL RECOMMENDATIONS FOR MILLING 2. The product design should permit manufacturing preference as much as possible to determine the radius where two milled surfaces intersect or where profile milling is involved

52. ADDITIONAL RECOMMENDATIONS FOR MILLING 3. When small flat surface is required, the product design should permit the use of spot facing, which is quicker than face milling

53. ADDITIONAL RECOMMENDATIONS FOR MILLING 4. When spot faces are specified for casting, provide a low boss for the surface to be machined.

54. ADDITIONAL RECOMMENDATIONS FOR MILLING 5. When the outside surfaces intersect and a sharp corner is not desirable, the product design should allow a bevel or chamfer rather than rounding

55. ADDITIONAL RECOMMENDATIONS FOR MILLING 6. When form-milling or machining rails, do not blend the formed surface to an existing milled surface

56. ADDITIONAL RECOMMENDATIONS FOR MILLING 7. Keyway design should permit the keyway cutter to travel parallel to the center axis of the shaft and form its own radius at the end

57. ADDITIONAL RECOMMENDATIONS FOR MILLING 8. A design that requires the milling of surfaces adjacent to a shoulder should provide clearance to the cutter path (Fig). 9. A product design that avoids the necessity of milling at parting lines, fl ash areas, and weldments will generally extend the cutter life.

58. ADDITIONAL RECOMMENDATIONS FOR MILLING 10. For more economical machining, the product design should allow staking so that a milled surface can be incorporated into a number of parts in one gang milling operation

59. ADDITIONAL RECOMMENDATIONS FOR MILLING 11. The most economical designs are those that require the minimum number of operations. 12. The product design should provide clearance to allow the use of larger-size cutters rather than small-size ones to permit high removal rates. 13. In end-milling slots, the depth should not exceed the diameter of the cutter (fig)

60. ADDITIONAL RECOMMENDATIONS FOR MILLING

61. DESIGN RECOMMENDATIONS FOR SHAPING, PLANING AND SLOTING 1. It is preferable to put machined surfaces in the same plane to reduce the number of operations required. 2. Avoid multiple surfaces that are not parallel to the direction of tool reciprocation, which would need additional setups. 3. Avoid contoured surfaces unless a tracer attachment is available and then specify gentle contours and generous radii as much as possible. 4. Design parts so that they can be easily clamped to the worktable and are rigid enough to withstand defl ection during machining

62. DESIGN RECOMMENDATIONS FOR SHAPING, PLANING AND SLOTING

63. DESIGN RECOMMENDATIONS FOR SHAPING, PLANING AND SLOTING 5. With shapers and slotters , it is possible to cut to within 6 mm of an obstruction or the end of a blind hole. If possible, allow a relived portion at the end of the machined surface.

64. DESIGN RECOMMENDATIONS FOR SHAPING, PLANING AND SLOTING 6. For thin, flat WPs that require surface machining, allow sufficient stock for a stress-relieving operation between rough and finish machining or, if possible, rough machine equal amounts from both sides to allow 0.4 mm for finish machining on both sides. 7. The minimum size of hole in which a keyway or a slot can be machined with a slotter or a shaper is about 25.54 mm. 8. Because of the lack of rigidity of long cutting tool extensions, it is not feasible to machine a slot longer than four times the hole diameter.

65. DESIGN RECOMMENDATIONS FOR SHAPING, PLANING AND SLOTING

66. DESIGN RECOMMENDATIONS FOR THREAD CUTTING Provide a space (1.5–19 mm) for the thread cutting tool Keep the thread as short as possible, which machines quicker and provides longer tool life.

67. DESIGN RECOMMENDATIONS FOR THREAD CUTTING 3. Allow chip clearance space when cutting internal threads (through holes are best) 4. Include a chamfer at the top and the end of external threads and a countersink at the top and the end of internal threads.

68. DESIGN RECOMMENDATIONS FOR THREAD CUTTING 5. Consider the use of a reduced height thread form, which machines more easily 6. The surface of the starting thread must be flat and perpendicular to the thread’s center axis.

69. DESIGN RECOMMENDATIONS FOR THREAD CUTTING 7. Avoid slots, cross holes, and fl ats that intersect with the cut threads. 8. When cross holes are unavoidable, consider countersinking of such cross holes. 9. Do not specify closer tolerances than required (class 2 is commonly satisfactory). 10. Ground threads should be provided with corners of 0.25 mm at the root. 11. The length of center less ground threads should be larger than the thread diameter.

70. DESIGN RECOMMENDATIONS FOR THREAD CUTTING 12. Coarse threads are more economical to produce and assemble faster than fine threads. 13. Tubular parts must have a wall thickness that withstands the cutting forces.