PROTOTYPE DESIGN AND MANUFACTURING MANUAL

Transcription

1 PROTOTYPE DESIGN AND MANUFACTURING MANUAL University Of Victoria Department Of Mechanical Engineering Prototype Design and Manufacturing Machining Facility Victoria, BC, Canada Rodney Katz Senior Scientific Assistant R. KATZ OCTOBER 2009 REV 0 J. STRAIN JANUARY 2016 REV 0.1

2 EXECUTIVE SUMMARY This manual is meant to serve as a guide when designing and manufacturing prototypes at the University of Victoria, Mechanical Engineering Machining facility. Design topics covered include inherent alignment, components, materials types and stock sizes. Guides to creating engineering drawings with all of the required information specific to the manufacturing of an individual design are also included. Manufacturing information is given for lathe and milling machines. The operations covered include drilling, tapping, boring, grooving, parting, threading, turning, side and end milling. Reminders are given about machining fixture set up and techniques. Mistakes and oversights during machining can result in broken tools, ruined parts and damage to machines. This can be both costly in time and money. Unlike making CAD drawings, machining does not have an undo button and the students who use the machine shop need to think the entire process through before beginning. Simple understanding of machining steps and time spent mapping out the meticulous details of a project will result in students gaining a better comprehension of manufacturing as well as achieving more with the limited time available in the machine shop. Since there are numerous ways to machine a component, students should create a machining plan, discuss plans with shop staff and make revisions when necessary. Multiple resources including tap drill sizes, static O-ring selection charts, machine feed and speed guidelines for different materials and operations are included in the appendices.

3 TABLE OF CONTENTS 1 INTRODUCTION PART ONE: STEPS TO DESIGN PROTOTYPING TOP DOWN MACHINING ALIGNMENT Alternate Methods BEARINGS MOTOR MOUNTING O-RINGS PIPES AND TUBES Pipe and Fluid Fittings MATERIALS Stock Materials Aluminum Steel Plastics Delrin (acetal) PVC Plexiglas DRAWINGS Dimensioning Baseline Dimensions Ordinate Dimension Common Drawing Mistakes Desirable Drawing Tolerances ANILAM CNC MILLING MACHINE Drilling Pattern Pocket Cutting Profile Cutting Frame Pocket PART TWO: MANUFACTURING DRILLING AND TAPPING i

4 3.1.1 Drilling Drilling Plexiglas: Tapping LASER CUTTER AND ENGRAVER LATHE Lathe Tools Machining Operations Boring Grooving Parting-Off Threading Turning Chip Load MILLING Milling Tools Machining operations End Milling Side Milling Setup Methods for CNC Machine Circular Parts O-RINGS Steps For Creating Axial O-Rings Grooves Steps for Creating Radial O-Ring Grooves POSTS Important Notes for Posts Lathe Process for Machining Multiple Posts with Bosses PART THREE: CREATING A MACHINING PLAN TOOL DETERMINATION SAMPLE MACHINING PLAN CONCLUSION WORKS CITED APPENDIX A: TAP AND BODY DRILL SIZES... A 8 APPENDIX B: LATHE OPERATIONS SPEED AND FEED GUIDES... B 9 APPENDIX C: ISO INCH EXTERNAL THREADING GUIDELINES... C 10 APPENDIX D: MILLING OPERATIONS SPEED AND FEED GUIDES... D 11 APPENDIX E: STATIC O-RING SEALING GUIDE... E 12 APPENDIX F: FACE SEAL O-RING GUIDE... F ii

5 TABLE OF FIGURES FIGURE 1: MIXER DEVICE WITH POST AND PLATE METHOD... 1 FIGURE 2: FLATS ON ROUND PARTS USED FOR ALIGNMENT IN A VISE... 3 FIGURE 3: PLACING A CIRCULAR PART IN A FIXTURE WITH GROOVES FOR REALIGNMENT... 4 FIGURE 4: DOWEL PIN REMOVAL USING A THROUGH HOLE IN THE SHAFT... 5 FIGURE 5: MIXER DEVICE USED AS PROTOTYPE ASSEMBLY EXAMPLE... 6 FIGURE 6: MULTIPLE SETUPS USED WHEN A PART CANNOT BE TOP DOWN MACHINED... 7 FIGURE 7: POST WITH END BOSSES AND EXTRA HOLES IN OD... 8 FIGURE 8: ALIGNED PLATES AND POSTS ASSEMBLY... 8 FIGURE 9: THREE POST DESIGN WITH DIFFERENT SHAPED PLATES... 9 FIGURE 10: EXAMPLES OF HOW POSTS AND PLATE DESIGNS CAN BE USED FIGURE 11: PLATE ASSEMBLY USING SQUARE POSTS FIGURE 12: PLATE ASSEMBLY USING ANGLE BRACKETS FIGURE 13: PLATE ASSEMBLY USING WELDED ANGLE BRACKETS FIGURE 14: WELDED WINCH FRAME FIGURE 15: PLATE ASSEMBLY USING C-CHANNEL FOR POSTS FIGURE 16: MOTOR WITH BOSS AND BOLT HOLES FIGURE 17: O-RINGS FIGURE 18: AXIAL O-RING SEAL ON LEFT AND A RADIAL O-RING SEAL ON RIGHT FIGURE 19: O-RING AXIAL GLAND ON LEFT AND RADIAL GLAND ON RIGHT FIGURE 20: PLEXIGLAS BONDED BUTT JOINT FIGURE 21: EXAMPLE ENGINEERING DRAWING TITLE BLOCK FIGURE 22: BASELINE DIMENSIONING FIGURE 23: DIMENSION LINE SPACING INCORRECT ON LEFT AND CORRECT ON RIGHT FIGURE 24: ORDINATE DIMENSIONING FIGURE 25: ELEVATION VIEW WITH AND WITHOUT HIDDEN LINES FIGURE 26: SLOT DIMENSIONING FIGURE 27: EASY TO READ DRAWING WITH ORDINATE DIMENSIONS FIGURE 28: DRAWING BLOCK FOR STANDARD TOLERANCES FIGURE 29: ANILAM INPUT SCREEN FOR BOLT HOLE CIRCLE FIGURE 30: ANILAM INPUT SCREEN FOR RECTANGULAR POCKET FIGURE 31: ANILAM INPUT SCREEN FOR CIRCULAR POCKET iii

6 FIGURE 32: ANILAM INPUT SCREEN FOR RECTANGULAR PROFILE FIGURE 33: ANILAM INPUT SCREEN FOR CIRCULAR PROFILE FIGURE 34: ANILAM INPUT SCREEN FOR FRAME POCKET FIGURE 35: PERCENTAGE OF THREAD ENGAGEMENT EXAMPLES FIGURE 36: STANDARD NOMENCLATURE FOR SINGLE POINT CUTTING TOOLS [4] FIGURE 37: LATHE OPERATION ILLUSTRATED [5] FIGURE 38: BORING EXAMPLE AND TOOL TYPE [6] FIGURE 39: GROOVING EXAMPLE AND TOOL TYPE [2] FIGURE 40: PARTING-OFF SCHEMATIC [5] FIGURE 41: THREADING EXAMPLE AND TOOL TYPE [2] FIGURE 42: FACING EXAMPLE AND TOOL TYPE [2] FIGURE 43: END MILLING [7] FIGURE 44: SIDE MILLING [7] FIGURE 45: CNC FIXTURE PLATE SETUP IN MILLING VISE FIGURE 46: CIRCULAR PART FIXTURE SETUP FIGURE 47: CIRCULAR PART FIXTURE SETUP FOR MULTI-AXIAL FORCES FIGURE 48: AXIAL O-RING GROOVE FIGURE 49: RADIAL O-RING GROOVE FIGURE 50: ENGINEERING DRAWING OF A POST FIGURE 51: BACK SCREW ENGINEERING DRAWING [9] FIGURE 52: MACHINED 316 STAINLESS STEEL BACK SCREW LIST OF TABLES TABLE 1: CHARACTERISTICS OF MILD VERSUS STAINLESS STEEL TABLE 2: RECOMMENDED AVERAGE FEED RATES FOR TWO FLUTE HSS DRILLS [3] TABLE 3: SURFACE SPEED RECOMMENDATIONS FOR DRILLING USING HSS [3] TABLE 4: PARTING-OFF INTO A TUBE FEED RATE GUIDE USING 400 SFM [5] iv

7 LIST OF ACRONYMS AND SYMBOLS ACRONYM MEANING UNITS Δapx Radial infeed used in threading in φ Threading constant: 1 st pass=0.3, then φ =nap-1 ADR Axial Depth ratio compared to tool diameter in ap Cutting Depth in CAD Computer Aided Design D Diameter in BHD Bolt Hole Diameter f Feed Speed in/min fn Feed Rates used in Lathe Calculations in/rev fr Feed Rates used in Drilling Calculations in/rev ft Chip Load used in Milling Calculations in/tooth HSS High Speed Steel ID Inner Diameter In N Rotational speed rpm NA North American NPT National Pipe Thread nap Number of Passes used in threading # OD Outer Diameter in RD Radial Depth ratio compared to tool diameter in T Number of Teeth of the cutting tool # TPI Threads Per Inch TPI TYP Typical V Cutting Speed sfm v

8 1 INTRODUCTION The purpose of this manual is to present best practices for the design and manufacturing of prototype devices, low volume machined parts and assemblies. It is important to note that many of the methods and techniques outlined in the manual are specific to the University of Victoria Mechanical Machining Facility. Design methodology is a very broad subject and this manual only covers the basics. This manual is structured around the design and manufacturing of a single device which encompasses many typical characteristics of features found in mechanical engineering research apparatuses. Figure 1 displays this design, which is very efficient to machine, incorporates inherent alignment, uses stock material readily available in the machine shop and is familiar to the shop machinists. Examples of less effective designs of the same device are also included. These methods are often initially thought to be easier to fabricate but do not lend the same advantages listed above. FIGURE 1: MIXER DEVICE WITH POST AND PLATE METHOD 1

9 2 PART ONE: STEPS TO DESIGN Design of a device should always begin by communicating with the specific shop or facility where parts will be manufactured. While in the design phase, continually communicating with shop personnel will always lead to designs which are less expensive and more efficient to build. Whenever possible, design parts in inches. The rationale being the machine shop cutting tool and material inventory are in the imperial system. Designing in metric then converting to inches leads to odd dimensions thus complicating the design and machining process, resulting in a more costly and time consuming part. Always keep in mind stock material sizes when designing parts. This is paramount to achieving an economically feasible design. Often the stock material size will be sufficient to accommodate your design with little additional machining required. In Canada available stock material sizes are produced in the imperial system as most material comes from U.S. suppliers. The capabilities of the shop or facility need to be carefully considered in order to design economically feasible devices or equipment: Machinery and shop specific expertise, CNC milling, lathe capability, sheet metal capabilities, welding capabilities, heavy machining, precision grinding, water jet cutting, EDM, rapid prototyping, etc. Shop preferred manufacturing methods and materials. Machine tool (lathe, mill) capacity. What is the largest or smallest size workpieces and cutting tools that the shop machines can comfortably accommodate. Time line required to deliver parts. 2

10 2.1 PROTOTYPING Generally prototype parts should incorporate inherent alignment, the ability to be machined and reworked easily, use material stock sizes and avoid many components with tight tolerances, small tapped holes and other delicate features. Utilize as many offthe-shelf items as possible. These will save many hours of design and machining work, paying for themselves many times over. Often off-the-shelf components may not meet all the requirements but can be machined to accommodate the design requirements. Inherent alignment means parts automatically fit into place. This eliminates the need for post machining and hand tool modification in order to fit parts together. Bosses and other features should be incorporated in the design to assure alignment of final assemblies. Building a design to create the ability for unforeseen circumstances could mean adding extra holes and also elongating holes. When milling is required on round parts the fixture set up is extremely important. Figure 2 displays flats on round parts. This allows for the part to be replaced into a vise with a known orientation for post machining or modifications at a later date. FIGURE 2: FLATS ON ROUND PARTS USED FOR ALIGNMENT IN A VISE 3

11 Tabs or marks for realigning parts if they are going to be placed back in a machine for post machining operations as shown in Figure 3. This is often the case when the part needs holes aligned to each other from both ends. Another reason for alignment marks would be if the part needs to be oriented in a specific rotational angle at assembly time. FIGURE 3: PLACING A CIRCULAR PART IN A FIXTURE WITH GROOVES FOR REALIGNMENT Use an easy to machine material like aluminum, acetyl (Delrin) and PVC (plastic) wherever possible. Even though these materials may be twice or three times the cost of steel, their fabricating and machining costs will be drastically lower resulting in a less expensive part. Size parts with a consideration for material yield. If aluminum sheet comes in 48 X 96 sheets. If you require four pieces 12 ½ X 12 ½ this will result in much waste material. Re-consider the design to work with 12 X 12 pieces. Sheet metal does not consume material for cuts whereas plate material (3/16 and thicker) will consume approximately 3/16 per cut due to the sawing and clean- up process. Plate material is also supplied in 12 increments. Therefore if four 12 X 12 plates are required this will produce a large amount of excess material. Try to work the design with part sizes of X

12 When designing a hole for a press fit dowel pin, incorporate a smaller diameter through hole which can be used to push or knock the dowel pin out if required, as shown in Figure 4 below. If no through hole is present it will be very difficult to remove the dowel pin and removal methods will result in damaging the pin and possible also the hole. FIGURE 4: DOWEL PIN REMOVAL USING A THROUGH HOLE IN THE SHAFT Avoid welding parts together. Welding does not allow for major changes if required. Separating parts can be labor intensive and sometimes close to impossible. It is also very difficult to accurately align welded parts. Design the assembly of sufficient size to avoid working in confined spaces. Also avoid the use of tiny screws such as #2-56 and smaller. Try to keep the fastener thread type selection to a minimum. #10-32 is a very practical size for much of the metal work performed in the shop and is easily tapped. Use a courser thread when working with plastics, such as # Tapped holes #6-32 and larger should be drilled all the way through in materials up to ¾ thick if possible as opposed to holes drilled to specific depths. It is always easier to tap a through hole opposed to a blind hole (one that does not penetrate). Blind holes may only be tapped partially through. The mixer device shown in Figure 5 is the example prototype assembly used to discuss the key components that are noted on the diagram. 5

13 FIGURE 5: MIXER DEVICE USED AS PROTOTYPE ASSEMBLY EXAMPLE 2.2 TOP DOWN MACHINING Flat parts, e.g. top and bottom plate, machined using a manual or CNC mill should be designed such that machining is required on one or two sides only. This is called Top Down machining. Try to avoid having features machined in the sides of plates. The actual process of cutting material is relatively quick. It is the setup and positioning of material and parts that takes majority of the time. If a part can be setup once and then cut without rotating or repositioning the part, machining efficiency will increase exponentially. Figure 6 shows an example of a part which requires multiple setups to machine. This part will need to be repositioned in the vise five times to drill all the required holes in the sides, thus consuming much time and effort. The more often a part is repositioned (clamped) in the machine the greater the possibility of misalignment of the features. 6

14 The long length of this part creates problems of instability, resulting in material flex, and inaccurate hole positioning. The milling machine being used may not have the required travel in the Z-axis needed to drill the end holes, shown in the third setup of Figure 6. Remember the drill chuck is extends approximately three inches, the ¼ diameter drill extends 4 and the part on end extends approximately 6 high, resulting in a consumption of 13 of the milling machines Z axis travel. The part clamped on end will also accentuate the deviation of the hole positioning (0.1 degree off perpendicular on a 6 protruding clamped part in the vise will cause a positioning error of the drilled hole by ). Trying to ensure the part is clamped perpendicular by this amount or better is very time consuming. FIGURE 6: MULTIPLE SETUPS USED WHEN A PART CANNOT BE TOP DOWN MACHINED 7

15 2.3 ALIGNMENT Alignment of parts and features is one of the most important aspects of mechanical design. If parts are designed with alignment in mind at all times it will prevent much frustration and added cost in the final assembly. One basic method to align parts is to use posts with bosses on both ends. Figure 7 shows an example of a post which incorporates bosses to aid alignment. FIGURE 7: POST WITH END BOSSES AND EXTRA HOLES IN OD Incorporating a boss on each side of the post has the added advantage of allowing the post to be held in the lathe chuck so the critical length can be measured off the front face of the chuck jaws, also the Z datum. The procedure used in the shop for accurately machining this type of post design is very efficient. Figure 8 shows how posts with integral bosses are used in the assembly. FIGURE 8: ALIGNED PLATES AND POSTS ASSEMBLY 8

16 Once the parts are assembled the two plates will be aligned sufficiently in order to attain the desired alignment. This method allows the plates to be efficiently milled and drilled Top Down with one setup. No repositioning is required. The machining process for posts is in Part Two: Manufacturing, page 51. This method can be altered to suit different applications while still maintaining alignment of plate features (center and shaft holes, bearing bores etc.): Plates can be different shapes if required, e.g. Figure 9 Three posts can be used instead of four, e.g. Figure 9 Not all posts need to be the same diameter Plate thicknesses can be different Figure 10 shows different examples of how posts can be used on a variety of applications FIGURE 9: THREE POST DESIGN WITH DIFFERENT SHAPED PLATES 9

17 Car chassis Tapping Machine Table Submersible Chassis (fits in tube) Winch 3 post design FIGURE 10: EXAMPLES OF HOW POSTS AND PLATE DESIGNS CAN BE USED 10

18 2.3.1 ALTERNATE METHODS This section presents some of the alternatives to using round posts with bosses. The alternatives may appear easier to fabricate but are often much more time consuming to machine and assemble. The alternatives do not incorporate inherent alignment features. Figure 11 shows a design similar to the recommended method. The square posts are difficult to machine because multiple machining setups are required. FIGURE 11: PLATE ASSEMBLY USING SQUARE POSTS Figure 12 and Figure 13 show the two plate assembly with angle brackets. Angle brackets are appealing because they seem simple to machine (just cut to length and drill). However, often what appears simple to fabricate, can result in being difficult and cumbersome. The method in Figure 12 is very time consuming to machine as the top and bottom plates cannot be machine Top Down. A total of 64 holes must be drilled, half of these also need to be tapped in the sides of the plates. Tapping is much easier in a through hole and when there will not be issues of conflicting with other features. 11

19 FIGURE 12: PLATE ASSEMBLY USING ANGLE BRACKETS The second angle bracket method shown in Figure 13 uses welds. This assembly requires 16 welds. Considerable time is required to setup and weld. Proper alignment of the plates will be virtually impossible and often require some post machining or hand work. In terms of prototyping welding does not allow parts to be easily modified. FIGURE 13: PLATE ASSEMBLY USING WELDED ANGLE BRACKETS 12

20 Figure 14 shows a welded version of a winch frame. This winch would take a considerable amount of time and effort to construct due of the number of welds and the requirement that the frame be accurately aligned for bearings blocks. FIGURE 14: WELDED WINCH FRAME There is a time and place for welding but in most assemblies used in the Mechanical Engineering Department it is not appropriate. Welding of small aluminum parts is very difficult and should be avoided. Figure 15 below shows the two plate assembly using C-channels. This method is appears relatively quick to machine but has significant alignment limitations: C-channel comes in standard sizes therefore spacing of the plates has limited options. Spacers must be used to adjust plate spacing. The size of extruded C-channel is not always accurate and the C-channel sides are often not perpendicular. Ensuring the holes are drilled directly opposite one another in the C-channel is very difficult. Securely holding the C-channel parts in the vice for drilling is cumbersome. 13

21 FIGURE 15: PLATE ASSEMBLY USING C-CHANNEL FOR POSTS 2.4 BEARINGS Bearings of many varieties are often used in mechanical design and are of utmost importance to the functionality of an assembly. Machined features that accept bearings must usually be made to tighter tolerances than other features. If a bore hole for a bearing is too small requiring excess force to seat the bearing, it will often cause the bearing to run rough and lead to premature failure. If a bore hole is too loose, the bearing will slop around and reduce the alignment of the shaft. Always include tolerances in drawings for dimensions related to bearings. If possible have the bearings available at the time of machining. This will greatly help the machinist correctly size the bearing bore hole. 2.5 MOTOR MOUNTING Most small and midsize motors incorporate a boss and bolt holes on their face as shown in Figure 16. The motor s boss assures concentric alignment of the motorshaft to the mounting surface. Correct use of tolerances for the receiving bore of the boss is very 14

22 important. If possible have the motor available to the machinist to check the bore size and fit at time of machining. This will often avoid time consuming reworking of parts. When dimensioning the bolt hole pattern be sure to label the bolt hole diameter on the engineering drawing. Also label the angles if the bolt holes are not evenly spaced. FIGURE 16: MOTOR WITH BOSS AND BOLT HOLES 2.6 O-RINGS O-rings are one of the most common types of seals used. They are extremely efficient and very inexpensive. The machining processes required to accommodate O- rings is often simple if the part is designed with consideration. Sealing using O-rings allows for easy disassembly of the apparatus if modifications or cleaning are required. There are two types of O-ring sealing configurations, axial and radial. An axial O- ring seal is located on the face of a part. A radial O-ring seal is on the outer or inner wall of a part. Radial seals on small shafts can significantly decrease the strength of the shaft. In this case it is better to groove the inner diameter of the part that the shaft will fit into. 15

23 It is best to avoid the use of radial O-ring configurations when possible because they are more difficult to machine and require much tighter tolerances in all respects. The plexiglas O-ring container configuration in the sample mixer device shown in Figure 5 used an axial seal. Axial seals are easier to machine than a radial seals. If a radial seal were used, the inner diameter of the plexiglas container would have to be accurate and concentric. Stock tubular material is often not accurate or concentric and would therefore require additional machining. In order to attain an accurate and concentric ID on a tube it must be bored on a lathe which is very time consuming. For an axial seal only the ends of the container need to be machined which is a quick process. A radial seal is often more difficult to remove the end caps especially in oceanographic instruments as seen in the schematic comparison of axial and radial O-rings FIGURE 17: O-RINGS in Figure 18 below. FIGURE 18: AXIAL O-RING SEAL ON LEFT AND A RADIAL O-RING SEAL ON RIGHT 16

24 The groove in which the O-Ring sits is called the gland and is shown in Figure 19. Appendix E and F show tables for gland sizes for different O-rings. The machining process for O-ring glands is in Part Two: Manufacturing, page 46. FIGURE 19: O-RING AXIAL GLAND ON LEFT AND RADIAL GLAND ON RIGHT 2.7 PIPES AND TUBES Pipe sizes are based on nominal inner diameters, not outer diameters (i.e. a ¾ schedule 40 pipe will have an OD of ). The nominal inner diameter of pipe usually does not match the physical inner diameter. This is due to the different wall thicknesses which are referred to as schedule sizes (e.g. schedule 40 or schedule 80). Different pipe materials also have different OD sizes (e.g. ¾ copper pipe has an O.D. of vs. ¾ steel and aluminum pipe both having an OD of ). Tube sizes are referred to and based on the actual physical OD (i.e. 1 tube is physically 1.00 O.D). Pipe is often less expensive than tube therefore it is used when larger quantities are required in the design or when fluid transport is required. Tube is used when a specific diameter is required. 17

25 2.7.1 PIPE AND FLUID FITTINGS National Pipe Thread (NTP) and ISO fittings are the most common fluid fittings used in the shop. NPT fittings are tapered to produce an effective friction seal when screwed into the mating fitting. NPT fittings are not used in thin material or sheet metal because a minimum of four threads must be engaged to produce a reliable seal. ISO fittings have straight threads and incorporate an O-ring at the base to create a seal. The mating surface for these O-rings must always be spot-faced to produce a reliable seal and include machined marks concentric with the O-ring seal. See the offset hole in the top cap of Figure 5. If a spot face is not made then any striations or any scratches in the plastic plate would allow a leak. Whenever O-rings are used any machining marks or scratches must be concentric with the O-ring. 2.8 MATERIALS This section lists some of the more common materials used in the Mechanical Engineering Machine Shop. Consult McMaster-Carr [1] for more detailed information on the material sizes, characteristics and cost STOCK MATERIALS When designing keep in mind the standard sizes of stock materials. In most cases stock materials do not have accurate sizes or geometric tolerances (perpendicular sides, parallelism, etc.). An example exception is precision ground steel rod which is ground to tight tolerances. If high precision alignment is required the stock material must often be machined on the significant mating surfaces. Aluminum plate has good surface flatness 18

26 as opposed to aluminum extrusion and is approximately twice the price. Use of aluminum plate can often reduce the amount of machining required paying for itself in the final result ALUMINUM Aluminum is most often the material of choice in the Mechanical Engineering Machining Facility. Aluminum characteristics and advantages: Lightweight Large size selection Good strength Good corrosion resistance Easy to machine Clean to work Good esthetics High heat conductivity Easily recyclable Readily available Difficult to weld properly Can be anodized to achieve a very highly corrosion resistant surface, reduced friction and also colored surfaces STEEL Mild steel is not used extensively in the Mechanical Engineering Machining facility. It is generally used for shafts, heavy welded structures, axels etc. Stainless steel is used only when necessary because it takes approximately five times longer to machine than the same part out of aluminum would. Machining stainless requires different tools and cutting techniques. Before stainless and mild steel are easy to weld. TABLE 1: CHARACTERISTICS OF MILD VERSUS STAINLESS STEEL Mild Steel High strength Heavy Corrodes easily causing rust Certain types of steel prove difficult to machine Low cost Considerably more costly to machine than aluminum Stainless Steel High strength and temperature resistance Very heavy Very good corrosion resistance Costly to machine Expensive Great esthetics 19

27 2.8.4 PLASTICS DELRIN (ACETAL) Delrin is often used as a replacement for aluminum parts, due to its excellent machinability. Try to implement it into designs when possible. One major advantage being that it does not need any coating to be corrosion proof. It also produces very esthetically pleasing parts due its sheen and color. Delrin has the following characteristics: Excellent machinability Corrosion proof Good relative strength Lightweight Tough and wear resistant Very low friction coefficient Solvent and fuel resistant White or black in colour Commonly available in round rod/bar, sheet, and plate o Some applications of Delrin: are bushings for low speed applications, wear pads, fluid fittings, gears, pulleys and idlers Delrin cannot easily be bonded to itself or other materials PVC Good corrosion resistance Easy to machine Lightweight Can be bonded easily. A mechanical interconnectivity of the two parts is always required when bonding PVC. It is not advisable to butt joint PVC. Not recommended for wear applications due to high friction coefficient. 20

28 2.8.5 PLEXIGLAS Lightweight Optically clear Brittle Scratches easily Low operating temperature band Commonly available in sheet, tube and solid round Bonds to itself very easily Plexiglas can be bent using heat. o Bending Plexiglas is not recommended for prototype design because changes and adjustments cannot be made. o Accuracy is difficult to achieve Plexiglas can be easily bonded together with a butt joint resulting in relatively strong bond, as shown in Figure 20. The surfaces must be smooth and flat before bonding and this can be done by milling or routing. FIGURE 20: PLEXIGLAS BONDED BUTT JOINT 21

29 2.9 DRAWINGS Try to always include an assembly view with a set of submitted drawings. This will help the shop understand the purpose of the parts and where extra care should be taken when machining. If tolerances or dimensions were omitted in a drawing it will often allow the shop to make an informed judgment when ambiguous. Dimension drawing features according to the shop preferred method or specific CNC mill that will be used. Make sure the drawing scale is noted. If dimensions need to be checked or are missing they can be measured off the drawing. When prototyping, printing drawings with a 1:1 scale can be useful to see the effects of changes on the part. General information should be included in the drawing title block. An example title block is shown in Figure 21. Details to include: scale, quantity, material, part #, contact info, tolerances FIGURE 21: EXAMPLE ENGINEERING DRAWING TITLE BLOCK DIMENSIONING Mark the origin of a part based on the origin that will be used when machining. The top left corner of the part is considered the origin of square parts. The origin of circular parts is the center of the circle. TYP is used to state that all the features of this type will be the same, unless otherwise noted. Hole depths must be noted. For connecting parts a hole should be threaded on one part only, the other part will have a clearance hole. 22

30 BASELINE DIMENSIONS Baseline dimensions cause drawings too appear cluttered and hard to read as shown below in Figure 22. Figure 22 also has the dimension lines touching the part. FIGURE 22: BASELINE DIMENSIONING Figure 23 shows a close up of the mistake from Figure 22 on the left and the correct use of dimension line spacing on the right. FIGURE 23: DIMENSION LINE SPACING INCORRECT ON LEFT AND CORRECT ON RIGHT 23

31 ORDINATE DIMENSION Use ordinate dimensioning to make drawings easier to read. Figure 24 displays ordinate dimensions, however the drawing appears crowded because the features are all dimensioned on two sides. Draw ordinate lines on the side of the part that is closest to the detail they are showing the position of, in this case the lower and far left features should have been dimensioned on the bottom and left side as shown in Figure 27. FIGURE 24: ORDINATE DIMENSIONING COMMON DRAWING MISTAKES First angle projection used instead of third angle projection, the NA standard. Too many decimals places. Dimensions referenced from wrong side of part edge and baseline method used. Font to big or too small (should be 12 pt. 14 pt.). Arrow heads too big. 24

32 Too many hidden lines make drawing difficult to interpret as shown in Figure 25. Elevation view of part should be shown without hidden lines. Use section views to display details..250 NOM.250 NOM FIGURE 25: ELEVATION VIEW WITH AND WITHOUT HIDDEN LINES Too much information on one drawing sheet. Instead use more than one drawing sheet to show part more clearly. Slots dimensioned to center points instead of the ends as shown in Figure 26. Remember to include the center of the slot when ordinate dimensioning. FIGURE 26: SLOT DIMENSIONING DESIRABLE DRAWING Using the shop specific preferred dimensioning style, taking care to ensure that the drawing is easy to read and that all features are properly dimensioned will help to speed up the machining process. Figure 27 is the best and most clear version of the part compared to Figure 22 and Figure 24. The center position of the slot is dimensioned and the width and total length are shown. 25

33 FIGURE 27: EASY TO READ DRAWING WITH ORDINATE DIMENSIONS TOLERANCES Tolerances are a very important aspect of drawings which are often overlooked and are not given the attention required. All dimensions should have an associated tolerance. Standard tolerances, based on number of decimal places, for the entire drawing should be displayed in the title block, as shown in Figure 28. If certain dimensions can accommodate a wider tolerance then remove the appropriate decimals. When FIGURE 28: DRAWING BLOCK FOR STANDARD TOLERANCES needed, add tolerances to individual dimensions to highlight the precision required. 26

34 2.10 ANILAM CNC MILLING MACHINE The CNC Milling machines used extensively in the Mechanical Engineering Machine Shop utilize an Anilam control system. Figure 29 to Figure 34 show a variety of input screens of canned cycles that are used for conversational programming. A canned cycle is a set of machine operations initiated by a single line of code. It uses a fill in the blank type interface. Use the figures shown below to determine the appropriate method to dimension part features which will be CNC milled. The zeros represent the features that must be included and dimensioned on engineering drawings DRILLING PATTERN When drilling holes in a circular pattern, as shown in Figure 29, the origin of the part is at the center of the circle. There should be a bolt hole diameter (BHD) dimensioned on the drawing along with starting angles. FIGURE 29: ANILAM INPUT SCREEN FOR BOLT HOLE CIRCLE For linear hole patterns the starting hole position must be known and the x and y increments to the following holes. It is important to use simple increment spacing whenever possible such as xinc= 3.0 & yinc= -0.5 versus xinc= & yinc=

35 POCKET CUTTING Pocket cutting is used to mill out all of the material inside of the shape to a specified depth. The center of the feature must be dimensioned for both circular and rectangular pockets. Figure 30 displays the rectangular pocket requirements including length, width and an optional corner radius. Having a corner radius will help to ease deburring. Figure 31 displays the circular pocket and the diameter is the only additional required input. FIGURE 30: ANILAM INPUT SCREEN FOR RECTANGULAR POCKET FIGURE 31: ANILAM INPUT SCREEN FOR CIRCULAR POCKET 28

36 PROFILE CUTTING Profile cutting is used when the CNC mill cuts the outline of the shape. Both circular and rectangular profiles can be cut and are shown in Figure 32 and Figure 33 respectively. The input requirements are the same as with pocket cutting. The only additional requirement is to determine if the pocket will be cut from the inside or outside of the shape. Profiles are used for milling the outside contours, slots and holes. The best surface finish is achieved on parts when the cutter has space to ramp in and out of the cut. FIGURE 32: ANILAM INPUT SCREEN FOR RECTANGULAR PROFILE FIGURE 33: ANILAM INPUT SCREEN FOR CIRCULAR PROFILE 29

37 FRAME POCKET A frame pocket is when a CNC mill cuts a rectangular groove. This can have any radius on the corners and is commonly used for cutting rectangular O-ring grooves. The pattern incorporates the length and width of both the island and frame, as well as the center position. These parameters are displayed in Figure 34. FIGURE 34: ANILAM INPUT SCREEN FOR FRAME POCKET 30

38 3 PART TWO: MANUFACTURING To create working components from engineering drawings requires an understanding of machine capabilities, operations and tool setups. First order of operations is chosen, and then tool types and machining fixtures can be determined. Details of cut depths, machine feeds and speeds are calculated before beginning. The speed and feed rates of a machine are dependent on the type, composition and thermal conductivity of the material for both the workpiece and tool, stiffness of workpiece and machine, tool wear, depth of cut and efficiency of cutting fluid [2]. Tool manufactures provide recommendations about the maximum feed rate, units of [in/rev] or [in/tooth], and peripheral velocity of tool, which is often expressed in North America as surface feet per minute [sfm] [3]. Peripheral velocity is based on the tool diameter when drilling and milling, but for the lathe the diameter is based on the workpiece because that is the spinning component. 3.1 DRILLING AND TAPPING DRILLING A center hole should be drilled to ensure the drill enters the workpiece with correct alignment. Use anytime there is a chance the drill bit may glance off the material or when holes need to be precisely positioned. Stub drills offer better rigidity and are recommended when working with harder materials. Drilling deeper holes tend to result in heat accumulation around the drill which can cause softening or even permanent dulling of the drill [2]. The drills used in the shop are 31

39 mostly made of high speed steel (HHS) with some cobalt drills used for harder materials such as titanium. Peck drilling is the practice of drilling a short distance, then withdrawing the drill to reduce the chip packing [3]. The cutting edges of a drill can be fractured by feeding into the workpiece too quickly and thus overloading the drill [3]. TABLE 2: RECOMMENDED AVERAGE FEED RATES FOR TWO FLUTE HSS DRILLS [3] Drill Diameter [in] Recommended Feed, fr [in./rev] under 1/8 up to /8 to 1/ to /4 to 1/ to /2 to to and over to Equations 1 and 2 are used to determine the ideal machine rpm (N) and feed speed (f). Recommend feed rates (fr) for HSS drills are provided Table 2and cutting speeds (V) are provided in Table 3. Sample calculations can be found in Section 4.2: Sample Machining Plan on page 57. N = 12V πd f = Nf r (1) (2) TABLE 3: SURFACE SPEED RECOMMENDATIONS FOR DRILLING USING A HSS DRILL [3] Material HHS: Recommended Speed, V [surface ft/min] Aluminum 200 Copper 100 Stainless Steel 40 Stainless Steel (Hardened) 20 Steel: Low Carbon 60 Steel: High Carbon 30 Plastics Titanium alloys 20 Wood

40 DRILLING PLEXIGLAS: Plexiglas will often to crack when the drill bit exits through the other side of the part. To prevent this, slow down the drill feed for the last 1/16 while drill bit exits the material. This heats the Plexiglas to make the last 1/16 more pliable to prevent cracking. Use extra care when drilling holes greater than 5/16 diameter TAPPING Taps are used to cut internal threads. The various types of taps used in the shop are: Spiral point taps Bottoming Tap Dies NPT taps Spiral point taps are the most commonly used. The first 3 to 4 threads on these taps are partial therefore they do not cut full threads for the complete length of engagement. If this is required a bottoming tap must be used following a spiral point tap. Bottoming taps are used to cut threads to the bottom of a blind hole. A bottoming tap does not have a tapered cutting edge therefore a spiral point tap must be used first. Do not use a bottoming tap to cut threads in an unthreaded hole. The only exception is tapping soft plastics. Use a bottoming tap only when thread depth is critical, e.g. 1/2 plate requiring 3/8 thread depth. A tap drill bit is the specific sized drill bit for a certain tap. For example a #6 drill is used to create the initial hole for a 1/4-20 tap. A complete list of tap and clearance drill sizes can be found in Appendix A: Tap and Body Drill Sizes. 33

41 The percentage of thread refers to the amount of thread in terms of the total thread depth, from crest to root. Use a larger tap drill bit to lower the thread percent and vice versa. Decreasing the thread percent minimizes the torque on the tap and dramatically helps to avoid breaking the tap. It also speeds up the threading procedure. Percentage of thread will vary depending on material. Steels require a lower percentage of thread and plastics will need more. FIGURE 35: PERCENTAGE OF THREAD ENGAGEMENT EXAMPLES Imperial screws are called out using the screw size and the threads per inch (TPI). Metric threads are specified by the OD and the distance between the threads. NPT Threads: National Pipe Thread (NPT) are tapered threads for sealing fluids. A die is used to cut external threads. Maximum depth of tapped holes should not exceed 3 X diameter of tap. Usually twice the tap diameter is all that is required to provide maximum holding force. 34

42 3.2 LASER CUTTER AND ENGRAVER 35

43 3.3 LATHE LATHE TOOLS Lathe operations use single point cutting tools and standard nomenclature is displayed below in Figure 36. The peripheral velocity is based on the diametric location of cutter contact. For turning and radial grooving this will be the outer diameter of the workpiece. Boring and axial grooving will be calculated using the larger outer diameter of the cutting tool. For large boring operations this can require multiple machine speed reductions as the internal diameter is increased. FIGURE 36: STANDARD NOMENCLATURE FOR SINGLE POINT CUTTING TOOLS [4] Tool positioning is extremely important and makes the difference between cutting or pushing material, superior surface finish or tool damage. External operations require the tool positioned at the center line of the workpiece or slightly below. For internal operations the tool needs to be placed at the centerline or slightly above. 36

44 3.3.2 MACHINING OPERATIONS The advantage of using a lathe is concentricity of various features as displayed in Figure 37. The five main operations used in the machine shop are outlined below. FIGURE 37: LATHE OPERATION ILLUSTRATED [5] Lathes often have set speeds; therefore the rpm of the machine should be adjusted for the specific cutting conditions. Machine speeds should be lower for roughing cuts and deep cuts, and faster for finishing cuts. The most common rpm setting for the lathes in Prototype Design and Manufacturing Machining Facility is setting A3, which ranges between rpm depending on the lathe. If cutting large diameter (D) or tough materials the speeds and feeds will need to be calculated and adjusted accordingly. Equations 3 and 4 govern the rotational speed (N) and feed rate (f) for lathe operations using single point cutters. Tool and workpiece piece material are used to determine the required surface feed per minute and inches per revolution. Recommended feed rates 37

45 and cutting speeds for boring, grooving, threading and turning are found in Appendix B. Sample calculations can be found in Section 4.2: Sample Machining Plan on pages 56 and BORING N = 12V πd workpiece (3) f = Nf n (4) Boring is used to create internal features. The depth of cut, feed and workpiece material determine the load on the boring bar [5]. There is risk of vibration caused by friction or tool deflection therefore the largest possible tool diameter with the shortest holder should be used for improved rigidity. An example is shown below in Figure 38. FIGURE 38: BORING EXAMPLE AND TOOL TYPE [6] GROOVING Grooving is used to create radial O-rings and other concentric slots. An example and schematic drawing are shown below in Figure 39. Grooving creates high cutting forces and therefore set up and tool rigidity is key. Machine RPM should be reduced. 38

46 FIGURE 39: GROOVING EXAMPLE AND TOOL TYPE [2] PARTING-OFF Parting-off is characterized by using a tool to completely remove one end of the workpiece from the stock material, as shown in Figure 40. It is preferable to part off into an air space, this can be done by drilling a hole. The parting tool can skate so never part off into an angled hole. FIGURE 40: PARTING-OFF SCHEMATIC [5] To save material and reduce cutting forces the narrowest tool possible should be used. Table 4 displays the feed rates to be used in Equation 4, based on a starting cutting speed of 400 sfm. Most parting tools in the shop are 2mm, however it is important to measure tools prior to using them to ensure the correct machine settings are being used. 39

47 TABLE 4: PARTING-OFF INTO A TUBE FEED RATE GUIDE USING 400 SFM [5] Component Wall Thickness Insert Width Feed Rate [in] [mm] [in/rev] < < < < < < < < THREADING Threading is done with a small tool and requires using an automatic feed setting for precision and accuracy. Specifications and settings differ per machine and most external threading operations will require multiple passes to achieve the desired depth. Non-CNC lathes use radial infeed to make cuts [5] and an example and schematic shown in Figure 41. The insert tip is exposed to high temperatures and will wear on both sides of the flank. There is a risk of vibration and the chips produced are stiff and V-shaped [5]. FIGURE 41: THREADING EXAMPLE AND TOOL TYPE [2] 40

48 Threading with radial infeed uses a method that decreases the depth of cut at each pass. This allows for deeper cuts to be taken initially and then must be reduced as more surface area of the tool become engaged with the workpiece. The chip being removed on each pass has a constant area. The cut depth ( apx ) for each pass (nap) is shown in Equation 5, where φ is a constant. The total depth of thread (ap) is determined using the TPI and Equation 6. Alternatively a chart displayed in Appendix can be used to determine a cutting sequence. Sample calculations can be on page 56. a p apx = nap 1 φ (5) a p = 1 (6) TPI TURNING Rotational workpiece machine motion combined with the linear movement of the tool constitute lathe turning. Cutting conditions are determined by cutting speed, feed rate and depth of cut. The defining factor is work hardness [2]. Harder workpiece materials require slower cutting speeds and the opposite is true for harder tools. An example and schematic drawing are shown below in Figure 42. FIGURE 42: FACING EXAMPLE AND TOOL TYPE [2] 41

49 3.3.3 CHIP LOAD Cutting tool material and the hardness of the workpiece material are the basis of chip load. Good chip forming, breaking and evacuation are key to maintaining high quality production and surface finish [5]. Chips should never turn blue or brown when using HHS tools. Although carbide cutters will produce a number of chip colors, black chips mean the cutting conditions need adjustment [2]. Chip color is a good indication of cutting condition limits. The effective entering angle is dependent on the nose radius of the tool as shown below in and should be as close to 90 as possible. 42

50 3.4 MILLING MILLING TOOLS Drills and end mills are the most common tools used in the shops milling machines. End mills material can be made of HHS or carbide. Carbide tools are tougher and can remove more material than a HHS end mill. If large amounts of material must be removed or surface finish is important, than a roughing tool should be used followed by a finishing tool. Serrated flute end mills can remove three times as much material as plain, helical fluted, end mills [2]. Feed rates should be reduced when using frail or thin workpieces. Guidelines for machine speeds when using the manual mills are found on the shop bulletin boards MACHINING OPERATIONS Peripheral velocity when milling is based on the tool diameter (D). Cutting speed (V) and feed rate (fr) are based on the tool and workpiece material, cutter size, number of cutter teeth and desired cut depth as a percentage of the tool diameter. Equations 7 and 8 are used to determine the ideal machine rpm (N) and feed rates (f). Appendix D is a compilation of the material types most commonly used in the machine shop as well as tool information for a many sizes of HSS and carbide end mills [7]. Sample calculations can be found in Section 4.2: Sample Machining Plan on page 58. N = 12V πd f = Nf t #teeth (7) (8) 43

51 END MILLING End milling produces a flat surface perpendicular to the axis of the cutter as shown below in Figure 43. Precision shapes and holes can be created using milling machines equipped with end mills. When end milling the entire cutter can be fully engaged and the axial depth ratio (AD) determines the machine feed and speed settings. During end milling the radial depth ratio (RD) is equal to the tool diameter. FIGURE 43: END MILLING [7] SIDE MILLING Side milling produces a machined surface that is parallel to the axis of the cutter as shown below in Figure 44. The axial depth ratio of the cutter is limited to 1.5 times the cutter diameter. The radial depth ratio determines the machine feed and speed settings. FIGURE 44: SIDE MILLING [7] 44

52 3.4.3 SETUP METHODS FOR CNC MACHINE Flat parts are often machined on a CNC mill using a fixture plate, shown in Figure 45. If the part does not have any features in its ends or sides only one setup is required, also called top-down machining. The advantages include that the outside of the part can be machined in one step and precise copies of the same part can be rapidly machined. FIGURE 45: CNC FIXTURE PLATE SETUP IN MILLING VISE CIRCULAR PARTS When the milling forces will be in the Z-axis only a circular part can be held to a fixture plate using a single, central bolt and washer, shown in Figure 46. This would occur when drilling. If radial forces are applied the part can rotate and cause damage to both the part and cutting tool. FIGURE 46: CIRCULAR PART FIXTURE SETUP 45

53 In other cases where lateral and radial cutting forces will be applied to the part a jig can be used. Figure 47 shows an example of a very simple, effective circular holding jig which is commonly used in the shop. The scratch marks on the part and jig allow the part to be replaced into the mill in the correct orientation for post machining operations or modifications. FIGURE 47: CIRCULAR PART FIXTURE SETUP FOR MULTI-AXIAL FORCES 3.5 O-RINGS O-ring types and uses are dependent on the application. Static seal O-rings are the most commonly used in undergraduate prototype design and guidelines for choosing the correct O-ring are found in both Appendix E and Appendix F. In a truly static seal, the mating gland parts are not subject to relative movement (except for small thermal expansion or separation by fluid pressure). Examples of static seals are: a seal under a bolt head or rivet, a seal at a pipe or tubing connection, a seal under a cover plate, plug or similar arrangement or, in general, the equivalent of a flat gasket [8]. 46

54 3.5.1 STEPS FOR CREATING AXIAL O-RINGS GROOVES FIGURE 48: AXIAL O-RING GROOVE 1. Determine the width of the tool being used. Using the following formula, determine the X position for the OD of the O-ring groove and Reduce machine RPM. (O-ring O.D.) (2)(Tool Width) = X (1.750) (2)(0.0525) = Work piece MUST be rotating for steps 2 and 3. Using the right side of the tool, establish the tool position on the OD of the work piece and enter the OD of the work piece into X on the digital read-out (e.g ). 47

55 3. Using the tip of the tool, establish the tool position on the front face of the work piece by touching off lightly. Enter into Z on the digital read out. Touch off the tool where the O-ring groove will be located. The score mark created from the tool will disappear when the O-ring groove is cut. 4. Steps 4 and 5 will be rough cuts. Rough cuts are usually smaller than the final tolerance. This is performed to improve surface finish and tolerances. Move tool in X axis to and then move tool in Z axis to Move tool in X axis out to This final rough cut. 6. Perform the finishing cut. Move X to 1.580, next move Z in to and then move X out to This should be done in one fluid motion. The tool should never become stationary on the workpiece when performing any cuts. This can cause chatter and excessive heat generation and when machining plastic it will create a poor surface finish and the seal may leak. 48

56 3.5.2 STEPS FOR CREATING RADIAL O-RING GROOVES FIGURE 49: RADIAL O-RING GROOVE 1. Determine the width of the tool being used, e.g Use the following formula to determine the final Z position for the O-ring groove width. (Groove width) (Tool Width) + (Z distance from datum surface) = Z (0.145) (0.0525) + (0.25) = Work piece MUST be rotating for steps 2 and 3. Using the left side of the tool, establish the tool position on the end of the work piece and enter the width of the tool into Z on the digital read-out, e.g This established the right side of the tool as zero in the Z axis. 49

57 3. Using the tip of the tool, establish the tool position on the O.D. of the work piece and enter the O.D. of the work piece into X on the digital read out. e.g Touch off the tool where the O-ring groove will be located. The score mark created from the tool will disappear when the O-ring groove is cut. 4. Steps 4 and 5 will be rough cuts. Rough cuts are usually smaller than the final tolerance. Move tool in Z axis to and then move tool in X axis to Move tool in Z axis to This is the final rough cut. 6. Preform the finishing cut in one fluid motion. Move Z to , next move X in to and then move Z to The tool should never become stationary on the workpiece, this can cause chatter, poor surface finish and the seal may leak 50

58 3.6 POSTS The best practice for dimensioning a post drawing when using the machining method outlined in Section is shown in Figure 50. The zero datum position is the base of the left boss. This is done because the critical dimension for this part is and not the overall length of 4.0. If alignment is very critical, e.g. top and bottom plates must be aligned within ±0.003, then the outer diameter of the post must be machined first to maintain concentricity throughout the machining process. Stock material is often not perfectly round. Machining the full outer diameter length is rarely required. FIGURE 50: ENGINEERING DRAWING OF A POST IMPORTANT NOTES FOR POSTS The overall length need not to be machined as accurately as the critical length between the bosses, shown in Step 9. When turning the boss in Step 2 it can be beneficial to leave an extra-long boss. This gives the chuck jaws more surface area to clamp when turning with the live center. After Step 9 this extra length can be faced off easily. 51

59 3.6.2 LATHE PROCESS FOR MACHINING MULTIPLE POSTS WITH BOSSES Step 1 Face first end of post and set Z-axis to zero on lathe digital readout Step 2 Turn boss to required diameter and approximate depth. Step 3 Centre drill Step 4 Drill end to tap depth Step 5 Tap. Repeat steps 1-5 for all posts Step 6 Zero tool against chuck using shim (make sure to account for shim thickness) 52

60 Step 7 Face opposite end of post to approximately the total length Step 8 Centre drill. Repeat steps 7 and 8 for all identical posts Step 9 Turn second boss with live center (Z = critical length of post) Step 10 Drill boss of opposite end to tap depth Step 11 Tap second end Step 12 Chamfer all sharp edges 53

61 4 PART THREE: CREATING A MACHINING PLAN The order of operations during machining can have variability. It is important to minimize the number of different fixture set ups and tool changes as well as maximize the amount of rigidity in the fixture setup. Rigidity is the key factor to both safety and surface finish. Alignment, concentricity and squaring of a part become more increasingly difficult to achieve with each new fixture set up. It is also extremely important to note tool compensation requirements, tight tolerances, rough and finishing cut depths, and specialized surface finishes, such as an O-rings, on the machining plan. Having a predetermined plan will also allow students to collect all required tools before beginning machining, thus significantly speed up the machining process. Rigidity is achieved using a lathe by holding the workpiece within the chuck at least one diameter deep. Shorter pieces will have to be held using a custom fixture plate. The workpiece should also not protrude out of the chuck more than a two diameter equivalent. Longer protrusions require the use of a live center to maintain rigidity and alignment. On a milling machine parts can be clamped firmly into the vise. Circular parts require flats or a custom fixture plate to achieve alignment and rigidity. Thin, delicate and/or odd shaped work pieces can be rigidly held by drilling holes and then having adjacent threaded holes on a custom fixture plate. Fixture plates that are made of different materials than the workpiece should milled and drilled before attaching the work to prevent cutter deflection. 4.1 TOOL DETERMINATION Once the fixture set up is determined, the tools required can be chosen. It is ideal to select the largest diameter tool to be able to complete the desired cutting operation 54

62 because smaller tools are less rigid and more fragile. Most of the shop drills and mills are made of high speed steel. These will work well for the majority of workpiece materials except steel or titanium, which would require cobalt coated drills and carbide cutters. All operations requiring the same tool within a fixture set up should be completed before changing the tool. Precision holes require center drilling and may also require sequentially stepping the drill size up to ensure an acceptable chip load. 4.2 SAMPLE MACHINING PLAN FIGURE 51: BACK SCREW ENGINEERING DRAWING [9] Figure 51 displays an engineering drawing [9] of a part that was to be made out of 316 stainless steel. This part required work on both the lathe and milling machine. A total of 25 steps were used to complete the part and are listed below. The feeds and speeds were calculated and displayed for each tool set up. 55

63 1) Rewrite Section B-B numbers and set the zero datum point from threaded end. 2) Place 1 stainless round in lathe with approximately 0.8 protruding from the chuck. 3) Use carbide turning tool and set speed and feed. Rough cuts of 0.05 and finishing % of ideal machine rpm was used to adjust for unideal cutting conditions. N = 12V πd = π 1in.6 = 630 rpm f = Nf n = 630rpm in = 3.78 in/min rev 4) Turn OD to and face to establish X and Z datum points. 5) Turn down the OD of the end to and deep. This will allow the part to easily thread into the connecting piece. 6) Change to the grooving tool and create a slot between Z= and that has an OD of This allows for space to turn the machine off when using auto feed for threading, Step 9. 40% of theoretical used to account for tool condition. N = 12V πd =.4 = 904 rpm π 0.998in f = Nf n = 904rpm in = in/min rev 7) Change to threading tool and set speed and feed based on a 28 TPI. Eight passes will be done and the depth of each radial cut is determined below. The initial cut depth is and then reduces to a final depth of cut of The feed input of the lathe is a preset and will be different for each lathe. The rpm was reduced by 25% to account for a worn tool insert and machine safety when using the automatic feed setting. N = 12V = 0.25 = 180rpm πd π 0.941in a p = 1 TPI = 1 28 = a p apx 1 = nap φ =. 3 = apx 2 = = apx 3 = = apx 4 = = apx 5 = = apx 6 = = apx 7 = = apx 8 = = ) Zero tool by touching on the end of the workpiece with the left hand side of the tool. 9) Complete multiple passes, with excess coolant, until thread depth matches required depth. Use magnifying glass to check threads. 56

64 10) Using the drill chuck, begin by center drilling. Then peck drill to a depth of 0.8 using the following drills and machine speeds. Since drilling is performed using the hand wheel, feed rates are not calculated. 1 st ) #35: N = 12V = 12 40ft/min = 1388 rpm πd π 0.11in 2 nd ) ¼ : N = 12 40ft/min π 0.25in = 611 rpm 3 rd ) 3/8 : N = 12 40ft/min π 0.375in 4 th ) 29/64 : N = 12 40ft/min π 0.453in = 407 rpm = 337 rpm 11) Change to boring tool and set speed and feed. Rough cuts of and finishing N = 12V πd = = 744 rpm π 0.846in f = Nf n = 744rpm in = 2.98 in/min rev 12) Zero tool on end and bore ID of to a minimum depth of ) Turn an ID of to a depth of and then take a finishing cut along the back to the final depth of and out to X= ) Go to X= and Z= and cut inner chamfer using cross slide. 15) Change to parting tool and set speed and feed. The sfm was reduced by 50% to account for cutting into stainless steel using a universal parting-off insert. The wall thickness is equal to ( )/2=0.251 so using Table 4 a feed of in/rev was used. N = 12V πd = sfm π 0.846in.5 = 900 rpm f = Nf n = 900rpm = 2.7in. min 16) Place a long plastic tube in the drill chuck to prevent the workpiece from falling when cut off. 17) Zero right hand side of parting tool in Z with a square piece of stock and part off between Z= and This will allow for slipping. 18) Create a fixture plate to hold the Back Screw in the lathe again without crushing the threads. 19) Place turning tool back in using the same speed as above and take down to overall size of ) Place boring tool back in lathe and create a small inner chamfer to prevent snags and soften inner edge. 21) Create a fixture plate to hold the workpiece in the mill. The OD should be 1 with a step of at a depth of

65 22) Use dial indicator on milling machine to center the circle and set the X and Y datum to zero at the center of the circle. 23) Place Back Screw into the fixture plate and load a carbide 3/16 three flute milling cutter into the chuck. Set machine speed and feed. Since the total cut depth is approximately 75% diameter of the cutter, the lowest cutting speed value will be used in the calculations. N = 12V πd = sfm π in = 2037rpm f = Nf t T = 2037rpm in tooth 3 teeth = 1.22in/min 24) Zero the tool on the surface of the workpiece and end mill the hexagon profile and inner slot. Taking rough cuts and finishing cuts. 25) Remove part and deburr all rough and sharp edges. The resulting part is seen below in Figure 52. FIGURE 52: MACHINED 316 STAINLESS STEEL BACK SCREW 5 CONCLUSION Following the design principles and suggestions outlined will help students create lean prototypes that can be easily manufactured and modified. Students who create a meticulous and thorough machining plan prior to gaining access to the machine shop make a more efficient use of both time and resources. Plans will help avoid mistakes and also aid in better finish, alignment, squaring and concentricity of prototypes. The application of theoretical understanding of machining principles will result in greater comprehension of the design and manufacturing process for students. 58

66 6 WORKS CITED [1] McMaster-Carr, [Online]. Available: [Accessed ]. [2] Fox Valley Technical College, "Machine Tool Technician Program," Wisconsin, [3] University of Flordia, "Department of Mechanical & Aerospace Engineering," [Online]. Available: Drilling%20and%20Milling%20Speeds%20and%20Feeds.pdf. [Accessed ]. [4] T. Baumeister, "Marks' Standard Handbook for Mechanical Engineers E8," New York, Mc-Graw-Hill, 1978, pp to [5] Sandvik Coromant, "Cutting Tools," [Online]. Available: [Accessed ]. [6] Sherline Product Inc., "SHERLINE Lathe Operating Instructions," [Online]. Available: [Accessed ]. [7] Niagara Cutter, "Comprehensive Solutions to Cutting Challenged," [Online]. Available: [Accessed ]. [8] Parker, "Parker O-Ring Handbook ORD 5700," [Online]. Available: Ring%20Division%20Literature/ORD% pdf. [Accessed ]. [9] R. Harirforoush, Back Screw RFS5, Victoria: University of Victoria Mechanical Engineering, [10] Plastics International, [Online]. Available: [Accessed ]. [11] J. Strain, "Achieving Optimal Workflow Efficiency during Machining," Victoria,

67 7 APPENDIX A: TAP AND BODY DRILL SIZES TAP TAP DRILL CLEARANCE DRILL NOM SIZE-T.P.I DRILL # DEC EQU TIGHT/PRECISION CLEARANCE MEDIUM CLEARANCE LOOSE CLEARANCE DRILL # DEC EQU DRILL # DEC EQU DRILL # DEC EQU / / (MM) / /4-28 7/ / (MM) / / / / (MM) / / / / / / /8-24 R / / / / / / / / / / / / / /2-13 7/ / (MM) / / / / (MM) / **** FOR METRIC AND NTP TAP SIZES, PLEASE SEE THE SHOP REFERENCE MATERIALS NOTE: THESE TAP DRILL AND CLEARANCE DRILL SIZES OUTLINED IN THE TABLE ARE SUFFICIENT FOR MOST WORK CONDUCTED IN THE UVIC MECHANICAL ENGINEERING MACHINING FACILITY. FOR CRITICAL OR HIGH STRESS APPLICATIONS CONSULT SHOP SUPERVISOR BEFORE SELECTING A TAP OR CLEARANCE DRILL. A

68 8 APPENDIX B: LATHE OPERATIONS SPEED AND FEED GUIDES [2] [5] [10] B

69 9 APPENDIX C: ISO INCH EXTERNAL THREADING GUIDELINES [5] C

70 10 APPENDIX D: MILLING OPERATIONS SPEED AND FEED GUIDES [7] D

71 11 APPENDIX E: STATIC O-RING SEALING GUIDE [8] E

72 12 APPENDIX F: FACE SEAL O-RING GUIDE [8] F