MACHING FACILITY LAB MANUAL MECH 200

Transcription

1 MACHING FACILITY LAB MANUAL MECH 200 October 2014 DEPARTMENT OF MECHANICAL ENGINEERING RODNEY KATZ REV 3

2 1 OBJECTIVES To expose students to the basic workings and procedures required to produce precision parts conforming to the specifications on engineering drawings using a manual milling machine and a manual lathe. The parts must be machined to the tolerances stated on the drawings without being test fitted to their mating parts, i.e. the brass bushing must press fit into the pillow block without deformation and/or excessive force. All parts will be assembled at the end of the Lab to produce a functioning Rotor Assembly. This exercise is intended to replicate a real world manufacturing condition in which various parts are produced from many different sources and a final assembly must be attained without having to rework the parts. To accomplish the above, students will appreciate the relevance of producing quality drawings which convey all the necessary details. Some tolerances required in this machining lab are relatively tight and will require particular attention to detail. Most parts can easily be machined to a tolerance of ±0.004 (0.1mm) with the machining tools used in the shop. The following example will give some physical size relevance to tolerances and dimensions to be used in the machining of the Rotor Assembly parts: o Average human hair = (0.04mm) thick o Average sheet of paper = ( 0.10mm) thick Some positioning and diameter tolerances required in this machining lab will be which is about 1 / 3 the thickness of an average human hair. This lab will also give the student an appreciation of the care, time and cost required to produce parts with tight tolerances. Therefore in the design process tight tolerances should be kept to a minimum and only used when necessary. Lab Safety Students must be familiar with and conform to the Machining/Design Facility Use Policy in Appendix A i

3 TABLE OF CONTENTS 1 OBJECTIVES... I 2 MANUAL LATHE LATHE SAFETY PROCEDURES USE AND CARE OF THE MILLING MACHINE GENERAL TECHNIQUES FOR TURNING ON A MANUAL LATHE MANUAL MILLING MACHINE MILLING MACHINE SAFETY PROCEDURES USE AND CARE OF THE MILLING MACHINE HOW TO CHANGE A MILLING TOOL REMOVING THE TOOL LOADING A TOOL GENERAL TECHNIQUES USED FOR MILLING THE PROJECT ALUMINUM ROTOR TURNED ON THE LATHE TURNING ALUMINUM ROTOR DRILLING THE SHAFT HOLE CUTTING OFF THE ROTOR FACING THE ROTOR TO FINISHED LENGTH BORING THE RECESS IN THE ROTOR BRASS BUSHING TURNED ON THE LATHE DRILLING AND REAMING THE BUSHING BORE CUTTING THE BRASH BUSHING OFF FACING THE BUSHING TO FINISHED LENGTH PILLOW BLOCKS ON THE MILLING MACHINE ii

4 4.3.1 SETTING THE X-Y DATUM CORNER OF THE VISE PREPARATION OF STOCK FOR PILLOW BLOCKS MILLING OF PILLOW BLOCKS BORING THE BUSHING HOLE MILLING THE SIDE RECESSES DRILLING SCREW CLEARANCE HOLES CNC MACHINING OF THE BASE PLATE WORKS CITED REVISION HISTORY APPENDIX A: MACHINING & DESIGN FACILITY USE POLICY A 7.1 SAFETY... A 7.2 FACILITY DRESS CODE... A 7.3 GENERAL... B 7.4 MECHANICAL ENGINEERING MACHINING FACILITY STANDARDS... B iii

5 TABLE OF FIGURES FIGURE 1: MANUAL LATHE [1]... 1 FIGURE 2: MAXIMUM PROTRUSION FROM THE CHUCK WITHOUT THE END SUPPORTED... 4 FIGURE 3: CORRECT TOOL POSITIONING ON A LATHE... 5 FIGURE 4: MILLING MACHINE USED IN THIS LAB IS CALLED A BRIDGEPORT STYLE KNEE MILL... 6 FIGURE 5: CORRECT METHOD FOR MEASURING DRILL DIAMETER WITH A CALIPER... 9 FIGURE 6: VISE CLAMPING OF PARTS IN SERIES AND PARALLEL FIGURE 7: FEATURES OF THE ROTOR FIGURE 8: MACHINING STEPS FOR ALUMINUM ROTOR FIGURE 9: CORRECT DRILL DEPTH FOR THE CENTER DRILL FIGURE 10: CUTOFF TOOL POSITIONING FIGURE 11: FACING THE ROTOR FIGURE 12: BORING TOOL SETUP ON LEFT AND ROTOR WITH FINISHED BORE ON RIGHT FIGURE 13: TURNING OF BRASS BUSHING FIGURE 14: REAMER USED FOR PRECISION DRILLING FIGURE 15: MILL AXES OF MOTION FIGURE 16: DATUM CORNER OF VISE AND THE X-Y COORDINATES FIGURE 17: LEFT DISPLAYS SETTING X DATUM AND RIGHT THE Y DATUM FIGURE 18: STEPS FOR MILLING PILLOW BLOCKS FIGURE 19: TOP VIEW OF CLIMB MILLING AND CONVENTIONAL MILLING FIGURE 20: VISE CLAMPING WITH ALIGNMENT USING MAGNETS FIGURE 21: AFTER PILLOW BLOCK HAS 0.5 HOLE MILLED FIGURE 22: CUTTER COMPENSATION FIGURE 23: STEPS FOR MILLING SIDE RECESSES IN PILLOW BLOCK iv

6 2 MANUAL LATHE FIGURE 1: MANUAL LATHE [1] 1

7 2.1 LATHE SAFETY PROCEDURES Only one student to operate the machine at any one time. Multiple people operating a machine at once can cause confusion and inadvertent operations which can endanger the other operator. Non-operating members of the group can watch, advise the operator and add coolant to the work piece if required. Lathe operator and observers must always stand to the side of the chuck, out of the line of rotation. Always remove the chuck key from the lathe chuck immediately after use and replace it in the chuck key holder (on the back splash guard). Do not ever leave the chuck key in the lathe chuck while your hand is not holding it. If a chuck key is left in the chuck and the lathe is turned on the results can be very serious. Always ensure the work piece is held securely in the chuck. Ask if uncertain. Always wait for the lathe chuck to come to a complete stop before touching the chuck or work piece. Never remove swarf (long stringy cuttings) from the lathe tool or work piece with your fingers. These can cause nasty cuts to your hands and fingers. Use the long nosed pliers, a dental pick and/or air gun to remove the swarf and cuttings. Do not allow an accumulation of swarf in the vicinity of the chuck and the work area. Back out of the work and remove it to the under tray or scrap bucket. Remove the lathe tool when drilling or using the tailstock. Also remove any drills from the drill chuck or the pointed live center when they are not being used. Always stop the lathe while changing tools. Ask the instructor before using sandpaper or a hand file on the lathe. 2.2 USE AND CARE OF THE MILLING MACHINE Refer to Figure 1 and familiarize yourself with the names and parts of the lathe. Oil the lathe first. Use the lubrication injector pump located on the apron of the machine, two shots required Only change lathe speeds when the lathe is off. When changing speeds using the gears, always first turn the chuck by hand ensuring the gears are properly engaged before switching the lathe back on. 2

8 Do not machine excessively close to the chuck. Keep the cutting tool tip a minimum of 1/8 away from the chuck. Ensure that sufficient stock is held in the chuck to prevent the work piece from being pulled out of the chuck while being machined. Use caution when using the long nosed pliers to remove swarf from around the work piece and cutting tool; do not knock pliers against the cutting tool or chuck. Use caution when placing any metal tools near the lathe cutting tools that are not in use. The lathe cutting tools used in this shop are expensive tungsten carbide inserts which have very sharp brittle tips and can be damaged easily if knocked against other metal objects. Therefore, do not place the chuck key on the headstock ledge; return it immediately to its designated holder on the back panel. Do not allow any tools or measuring instruments to protrude from the lathe headstock ledge, as they could accidentally drop onto the rotating chuck. 2.3 GENERAL TECHNIQUES FOR TURNING ON A MANUAL LATHE Pay close attention to the job at hand and the details. Failure to do so will often result in a finished part not conforming to specification. This is often only recognized at the completion of the part or worse yet in the final assembly resulting in a time consuming re-make or rework of the part. There is no Undo command in machining Removal, cutting or machining of material on a lathe with a lathe tool is referred to as turning. Always clean the chuck jaws with a shop cloth before installing the work to prevent eccentric chucking and indenting of the work piece by previous cuttings. Always ensure the work piece is rotating at full speed when engaging the cutting tool into the work piece or exiting the cutting tool from the work piece. Do not stop the chuck rotation with the cutting tool in the work piece or when it is touching the work piece. Always move the lathe tool to its cutting position off of the work piece then proceed with the cut into the work piece. Feeding in or out the X axis, determines the diameter of the work piece. Feeding in the carriage in the Z direction determines the length of the part. 3

9 Have the least amount of material protruding from the chuck as possible in order to machine the part. Rigidity is the key factor to achieving a good machined finish on the part. FIGURE 2: MAXIMUM PROTRUSION FROM THE CHUCK WITHOUT THE END SUPPORTED A general rule: Do not have more than 2 times the diameter of the work protruding from the chuck, and a minimum length of one times the diameter held in the chuck, as seen in Figure 2. If more of the work piece is to protrude from the chuck, a live center must be used to support the end, consult the instructor for additional guidance. The cutting tool must be centered with respect to the center of the spindle, seen below in Figure 3. When the tool tip is set to the spindle center height, a cut depth of translates to a diameter change of The digital readouts (DRO s) on the lathes are set to read in diameter (DIA). 4

10 FIGURE 3: CORRECT TOOL POSITIONING ON A LATHE Backlash is the play or slack between the driving screw element and the driven nut element that occurs when an overshoot and short backup is made while turning an axis into position. To eliminate backlash while turning into a desired position, the turning wheel must be backed out approx. half a turn from the original input direction and then repositioned again to the desired position. A small initial cut and measurement must always be made on the diameter of the X axis and another on the Z axis to establish a datum point from which the diameter and length can be set. This is a crucial measurement as all subsequent measurements will be based on these initial measurements. When measuring the diameter of the part in the chuck, move the carriage out of the way to allow unconfined access to the part. Use two hands when feeding during a cut. This will result in more control and will provide a uniform finish on the work piece. 5

11 3 MANUAL MILLING MACHINE FIGURE 4: MILLING MACHINE USED IN THIS LAB IS CALLED A BRIDGEPORT STYLE KNEE MILL 6

12 3.1 MILLING MACHINE SAFETY PROCEDURES Only one student to operate the machine at any one time. Multiple people working on a machine cause confusion and inadvertent operations which can endanger the other operator. Non-operating members of the group can watch, advise the operator and can add coolant to the work piece (part being machined) if required. Always shut-off the Mill before removing parts from the vise or measuring parts in the vise. Immediately and gently apply the break to stop the spindle rotation after switching off the motor, do not let the spindle coast to a halt. This ensures the cutter is stationary when the operator needs to handle or measure the work. Remove the draw bar wrench immediately after use and replace it on the provided peg. Always check to ensure the draw bar wrench is not on top of the mill prior to switching on the motor. If the cutter will not release easily from the collet after loosening, use a cloth around the cutter to protect your hands and fingers while removing the cutter. Do not use fingers to clear away chips. Use the air gun, but with caution and consideration for others. If you are uncertain about the set-up for machining your part ask the instructor. 3.2 USE AND CARE OF THE MILLING MACHINE Refer to Figure 4 to become familiar with the names and parts of the Manual Knee Mill. Oil the Mill first using the hydraulic oiler on the side of the machine before use (one pump is sufficient). Change the speed of the Mill only while the motor is running. This is due to the infinitely variable speed drive belt and pulley configuration (similar to that used in an infinitely variable speed snowmobile transmission.) When changing the machine speed between high and low the machine must be off. This leaver is located on the upper right hand side of the machine. Ensure the Way Lock Levers are loose when moving any of the X, Y or Z axes. These levers can be tightened if required to prevent movement. The compressed air can be used to clean the Mill but do not blow directly into the slides of the machine. 7

13 Coolant can be used liberally on the machine; any excess coolant sprayed on the floor must be cleaned up immediately to prevent a slipping hazard. All machines must be thoroughly cleaned and excess coolant dried off after use. There should be no visible chips on the vise, or milling table. In between the milling table slots should be cleaned with compressed air. There are five different metal recycling bins in the shop. Be sure you are placing the correct metal scrap into the appropriate bin or YOU will have to spend your personal time separating out the metal scraps! Note: there are two aluminum recycling bins one for shavings and the other for solid pieces. If the machine is making a strange noise, vibrating, or is not cutting as it should always stop and check for the cause or ask the instructor for assistance. Do not proceed with machining until the problem is solved. Never use a milling cutter in a drill cut. 3.3 HOW TO CHANGE A MILLING TOOL When removing cutting tools or the drill chuck from the collet, place the plastic tray below the tool. This prevents the tools and the vise from being damaged when they are tapped out, and accidentally dropped onto the mill. Always place tools on the plastic trays on the mill table. This prevents the steel tools from dinging the precision ground mill table. Do not place the collets on the plastic trays; instead return immediately to their home on the work bench REMOVING THE TOOL Apply the machine brake and turn the wrench ½ a turn to loosen the drawbar bolt on top of the machine. This will loosen the draw bar which protrudes down the center of the machine and secures the collet. Place your hand below the tool and tap the top of the drawbar with a rubber mallet this will cause the tool to come out of the machine. If the tool does not release right away then keep one hand below the tool and with the other loosen the bolt a little more and tap the drawbar again with the mallet. Once the tool is removed, continue to loosen the bolt by hand until the collet drops out. 8

14 3.3.2 LOADING A TOOL Place collet into the machine with one hand and hand tighten the drawbar bolt with the other hand until the collet is fully engaged with the machine draw bar. Place the tool into the collet and continue to hand tighten the bolt. If the tool does not fit into the collet, slightly loosen the bolt to allow the tool entry into the collet. Place hand on the milling machine brake and tighten the drawbar bolt with the wrench between 1 / 4 to 1 / 3 of a turn, MAXIMUM past finger tight. 3.4 GENERAL TECHNIQUES USED FOR MILLING Pay close attention to the job at hand and the details. Failure to do so will often result in a finished part not conforming to specifications. This is often only recognized at the completion of the part or worse yet in the final assembly resulting in a time consuming remaking or reworking of the part. Note: There is no Undo command in machining Ensure the vise jaws and machine base are thoroughly clean before installing parts (use the air-gun or shop towels if necessary). A tiny metal chip left sandwiched between the part and the vise jaw or parallels could result in a part not being square and can also leave indentations in the part. Always check the diameter of the drill with a caliper to verify it is the correct size. Previous users may have incorrectly replaced the drill in the drill index. The accurate method of measuring a drill is to measure across the cutting flutes tips using the broad section of the dial caliper as shown in Figure 6. FIGURE 5: CORRECT METHOD FOR MEASURING DRILL DIAMETER WITH A CALIPER 9

15 De-burr and remove all sharp corners of parts with a file after milling or cutting. This will ensure parts sit properly when re-installed in the vise, also for safety and cosmetic reasons. Only clamp one part at time. If it is necessary to clamp more than one part at a time to improve efficiency, only clamp in series, not in parallel as seen in Figure 6. Parts clamped in parallel cannot be held with even force and can cause one part to loosen during milling. Parts clamped in series Parts clamped in parallel - Recommended - - Not Recommended - FIGURE 6: VISE CLAMPING OF PARTS IN SERIES AND PARALLEL Most parts clamped in the vise only require the vise handle to be tightened approx. 1 / 4 of a turn past finger tight. This exerts a clamping force of approx. 2000lb on the part. Always ensure the cutter is rotating when bringing it into contact with the work piece. This prevents the cutter edges from being damaged. When making a finish cut in one axis always lock the opposite axis table using the locking handles. This will prevent any drift and chatter occurring in the opposite axis. Remember to unlock the handles after. Before removing the finished part from the vise, measure it to ensure that it is accurate and meets specifications. If additional machining is required and the part has been removed from the vise it can be difficult to achieve repeatable alignment resulting in parts not meeting specification. Scribe an X in the upper left corner of the part, in order to allow reinstallation in the vice with the same orientation when additional machining is required. 10

16 4 THE PROJECT 4.1 ALUMINUM ROTOR TURNED ON THE LATHE The Rotor will be machined from Aluminum 6061-T6, 1 1 / 2 diameter bar stock. Each piece is a minimum of 2 long to ensure that a sufficient amount of material can be held in the chuck for safety and rigidity TURNING ALUMINUM ROTOR The features of the rotor and associated names are displayed below in Figure 7. FIGURE 7: FEATURES OF THE ROTOR Set the lathe to 1075 rpm or 860 rpm, gear speed combo A-3. Place the aluminum designated lathe tool in the quick-change tool holder. See Figure 8 for the machining steps of the aluminum rotor. Place the 1 1 / 2 diameter aluminum bar in the chuck with approx. 1 1 / 2 protruding. Make a face cut of and set the Digital Read Out (DRO) on the Z to This is the datum point for the length (Z) of the part. Make a small skim cut (approx long in the Z axis) on the diameter of the work piece, and move the lathe tool back off the part in the Z axis not moving the position of the X axis. 11

17 STEP 1: Initial facing cut and set Z datum to zero STEP 2: Skim cut and set X to measured diameter value STEP 3: Turn OD to and face a depth of STEP 4: Rough stock removal: turn OD to and face STEP 5: Rough stock removal: Turn OD to and face STEP 6: Rough stock removal: turn OD to and face STEP 7: STEP 8: STEP 9: Final diameter stock removal. Final shoulder face cut in Z to Chamfer both outside edges turn od to a final diameter of a width of and a final using the chamfer tool and face diameter in X of FIGURE 8: MACHINING STEPS FOR ALUMINUM ROTOR 12

18 Measure the diameter of this cut with the dial calipers, and input this value into the DRO for the X axis. Turn the diameter to ±0.005 and to a length of Refer to Figure 8 for the steps to turn the boss to diameter by long. Only turn to ±0.010 in length (Z axis) for the rough cuts. The final length cut of the boss will be made using a facing cut by positioning the Z axis at ±0.005 and feeding into X to ± Remove the tool from the quick-change tool holder and replace with the chamfering tool and lightly chamfer the two corners as required. Note: These corners are only cosmetic chamfers, and therefore do not need to be accurate DRILLING THE SHAFT HOLE A center drill is always used in a lathe drilling operation. When a center drill hole is not used, the drill could deflect to the side resulting in an off center hole. Insert the center drill chuck into the tail stock and drill a hole in the aluminum work piece to the depth shown in Figure 9 (half way up the second taper). Replace the center drill with a 1 / 4 diameter drill and clear any remaining chips from the rotor. Drill a ¼ hole approx. 1 1 / 4 deep, backing out every 3 / 8 to clear the cuttings and inject coolant down the hole. All holes should be deburred, to do this insert the countersink tool in the drill chuck, gently bringing it into contact with the part. Rotate the chuck by hand. This will remove the burr at the entrance of the hole and create a small chamfer. FIGURE 9: CORRECT DRILL DEPTH FOR THE CENTER DRILL 13

19 4.1.3 CUTTING OFF THE ROTOR Insert the cut-off tool into the tool holder and align its front right tip to the front face of the part as shown in Figure 10. Make sure to not touch the tool tip to the part without the machine moving. Use a piece of square metal to achieve proper alignment. Move the Z carriage forward to approx. Z=1.050 and feed the cut-off tool into the work at a medium, steady pace ensuring coolant is being injected liberally into the cut-off groove. Once the cut-off tool penetrates to the drilled hole the part will simply fall away. Do not attempt to catch it. FIGURE 10: CUTOFF TOOL POSITIONING FACING THE ROTOR TO FINISHED LENGTH Remove the bar stock from the chuck and insert the rotor part as shown in Figure 11. Shim stock (brass foil) can be wrapped around the part in order to prevent the hard jaws of the chuck from indenting the part. Insert the regular lathe tool (diamond shaped) into tool holder and face the part, removing as little material as possible. Back the tool out in the X axis without moving the Z carriage. Measure the total length of the part and input this value into the Z DRO. Move the Z carriage to 1.00 and face the part. This will produce the 1.00 finished length of the part. 14

20 FIGURE 11: FACING THE ROTOR Insert the chamfering tool and turn a small cosmetic chamfer on the part BORING THE RECESS IN THE ROTOR Insert the boring tool into the tool holder. Take a brass shim and measure it with a caliper. Place the brass shim on the face of the rotor and very lightly touch the tip of the boring tool to the front face of the part near the center with the lathe turned off, see Figure 12. Set the DRO in Z to the thickness of the shim. Move the tip of the boring tool out in the X axis approx. 1/8 beyond the center hole and bore in the Z axis to a maximum depth of Repeat this operation increasing the diameter of the bore by approx per cut. After the 2nd cut, back out the boring tool in the Z axis, ensuring not to move the X axis from its last cut. Measure the internal diameter of the bored hole, and input this value in X DRO. Continue boring out the recess in increments of approx until a diameter of ±0.005 is achieved. Return the tip of the boring tool to the center of the part X = at a depth of Z = ±0.005 and feed the tool out to a diameter of Retract the tool in the Z, shown in Figure 12. The tool is only taken to diameter so it does not contact the inner diameter wall, which would produce chatter marks. 15

21 The internal chamfer on the bore diameter can be achieved by feeding the boring tool in at a 45 degree angle. (Internal chamfers cannot be turned using the regular lathe tool). FIGURE 12: BORING TOOL SETUP ON LEFT AND ROTOR WITH FINISHED BORE ON RIGHT 4.2 BRASS BUSHING TURNED ON THE LATHE The brass bushing will be machined from Brass 3 / 4 diameter bar stock. The stock piece must be a minimum of 1 1 / 2 long to ensure that a sufficient amount of material can be held in the chuck for safety and rigidity. Note: The brass bar stock is diameter therefore the 0.75 Nom. diameter section of the bushing is already to size and does not require machining. (Nom. is short for nominal which means: leave the pre-sized stock at its original size or as it comes from the supplier). Keeping nominal sizes in mind and using when feasible will save time and expense in designing and manufacturing parts. Using the diamond shaped lathe tool face the work piece and set the DRO to Z= Make a small skim cut (approx long) on the diameter of the work piece and move the lathe tool back off the part in the Z axis without moving the position of the X axis. Measure the diameter of this cut with the calipers and input this value into the DRO for the X axis. Turn the shoulder of the bushing to ±0.005 diameter and deep in approx diameter increments, as shown in Figure

22 STEP 1: Initial facing cut and set Z datum to zero STEP 2: Skim cut and set X to measured diameter value. STEP 3: Turn OD to.650 and face a depth of.440 STEP 4: STEP 5: STEP 6: Turn OD to.510 and face Turn OD to.505 and face Final diameter stock removal Measure diameter with Measure diameter with Turn od to a final diameter of micrometer and re-input into micrometer again and reinput, if and face DRO. necessary. STEP 7: Turn down step on leading edge to OD of and to a depth of STEP 8: STEP 9: Final shoulder face cut in Z to Chamfer both outside edges a width of and a final using the chamfer tool diameter in X of FIGURE 13: TURNING OF BRASS BUSHING 17

23 In order to obtain the high tolerance on the bushing O.D. (0.5020, , ) a micrometer must be used to measure the O.D. Input this micrometer measured diameter into the DRO. Turn the bushing down to diameter and measure it again using the micrometer, if it reads different to the DRO reading then update the DRO with this latest measurement. Make a cut to O.503 diameter and measure again with a micrometer. Now cut diameter to the required size , , and check the size using the micrometer. Position the tool at Z = and feed in the X axis to a diameter of This will face cut a clean square shoulder and produce an undercut at the junction of the flange and the shoulder. Turn the small reduced diameter of x 0.07 depth from the end of the part. This reduced diameter is designed into the part to allow for ease of initial insertion of the bushing into the pillow block bore. Insert the chamfering tool. Cut the small chamfers on the front edge and the shoulder edge DRILLING AND REAMING THE BUSHING BORE Refer to the Section 4.1.2, Drilling the Shaft Hole for initial drilling then Section Boring the Bushing Hole for creating the precision hole with a reamer. As this is a precision hole of ± it must be reamed to attain the tolerances required. A hole of approx diameter is drilled to a depth of 0.750, drilling in increments of approx. 1 / 4 deep and retracting to clear the cuttings (this is called peck drilling). FIGURE 14: REAMER USED FOR PRECISION DRILLING 18

24 Insert the diameter reamer into the drill chuck and change the lathe speed to 275 or 220 rpm depending on the lathe being used. Note: More cutting flutes on the tool require slower rotational speeds of the machine. While applying coolant, slowly feed the reamer into the drilled hole until the reamer bottoms out. Retract slowly. Do not lock the tailstock CUTTING THE BRASH BUSHING OFF It is important that all the necessary operations are performed on the working side of the part prior to it being separated from the initial stock piece. It is often very difficult to hold the part in this orientation again and maintain concentricity. Refer to Cutting Off the Rotor. Cut the bushing off longer than stated in the drawing, to a length of ± This extra length will allow a small amount of material to be removed for a facing cut. The cut-off tool might not produce a flat smooth face on the part FACING THE BUSHING TO FINISHED LENGTH Refer to Facing the Rotor to Finished Length. This method is repeated only using the brass bushing Face the bushing to a length of and chamfer O.D. using the chamfering tool and lightly chamfer the I.D. using the countersink tool in the drill chuck. The completed part should now conform to the drawing. 19

25 4.3 PILLOW BLOCKS ON THE MILLING MACHINE SETTING THE X-Y DATUM CORNER OF THE VISE Instructions for setting the Digital Read Out (DRO) systems are located on the individual machines. Note: All rotary dials on the machines and dimensions are in inches. FIGURE 15: MILL AXES OF MOTION The Mill uses an XYZ Cartesian plane axis system as displayed in Figure 15. The directions refer to the relative movement of the cutting tool, not the milling table. The milling machine vise must first be initialized to obtain a datum corner. This is usually the top left corner of the vise back jaw as shown in Figure 16. Note: The top left corner is commonly used as the machining datum; therefore it is also useful to dimension parts on the drawings from this corner. 20

26 FIGURE 16: DATUM CORNER OF VISE AND THE X-Y COORDINATES Install the 1 / 2 collet into the Mill spindle and install the diameter probe Edge Finder into the collet with approx. 1 total protruding. Note: The Edge Finder probe is diameter therefore a radius of is used to set the X and Y positions with respect to the edge of the vise. An Edge Finder centripetal probe will be used to accurately locate the datum corner of the vise with respect to the center of the Mill spindle, seen in Figure 17. Open the vise up and clamp a sample piece of material approx. ¾ up the jaws of the vice. It is very important to zero the machine with material clamped in the vice, otherwise Y axis positioning will be off approximately when parts are clamped. Turn the Mill on, setting the speed to approx RPM. Position the Edge Finder as shown in Figure 17 on the left and move the Y table slowly towards the Edge Finder until the Edge Finder probe is barely touching the edge of the vise. Continue slowly moving the Y table in the same direction until the Edge Finder probe flicks to the side (running eccentric with respect to the body). This position will be Y = , set the DRO to Y Repeat this operation to confirm that the correct position has been obtained. 21

27 FIGURE 17: LEFT DISPLAYS SETTING X DATUM AND RIGHT THE Y DATUM Move the X table with respect Edge Finder shown in Figure 17 on the right, and repeat the above two steps. This position will be X= , input this position to the DRO. Note: There are other methods to locate datum edges, enquire with the shop instructor for more information PREPARATION OF STOCK FOR PILLOW BLOCKS The pillow blocks will be made from aluminum 6061-T6 bar stock 1 / 2 x 2. Cut one piece 3 3 / 8 ± 1 / 16 long using the Metal Cutting Chop Saw. Remove all burrs using a file and deburring tool MILLING OF PILLOW BLOCKS SQUARING-UP BLOCKS Install the 1 / 2 wide parallels in the vise and place the work piece on top of the parallels. Lightly clamp the work piece and hit it with the rubber mallet to ensure it is well seated on the parallels, then tighten up the vise. A second hit with the mallet may be necessary to ensure good seating of the part. With the machine turned on set the manual mill to approx rpm. 22

28 Use a 1 / 2 diameter two flute, HSS (high speed steel) milling cutter to end mill the top face of the aluminum block as shown Figure 18, Step 1. Move the work piece under the cutter and slowly move it up using the Z axis crank handle until the cutter contacts. Set the Z dial to 0, then raise the table approx (one full revolution = ) for the first cut, this will be a plunge mill. Traverse the table back and forward to remove all the material on this plane. Remove an additional of material in the Z for a finishing cut. Remove the work piece from the vise and de-burr edges. Replace the work piece in the vise with the last machined side facing down. Remove approx of material in the Z axis in two cuts. Move the work piece in the X axis approx. 3 away from the cutter. Do not move the Z axis from its last cutting position and measure the height of the work piece using a caliper then reenter the Z datum as measured. Crank the table up the required amount and mill the work piece to its finished height of ± This completes Step 2 in Figure 18. Always check the work piece to ensure that it is square and the correct dimension has been obtained before proceeding to the next step. Place the work piece in the vise as shown in Figure 18, Step 3 with the bottom of the milling cutter protruding approx. 3/8 below the work piece. This will reduce tool deflection. Using the Y axis table side mill the part removing a maximum of per pass. Make the last cut a climb mill removing less than.005 of material using a slow steady feed rate. This will produce a superior finish. Climb milling is used on manual milling machines only when machining soft metals and plastics. Do not use climb milling when milling steel, conventional milling is used when milling steel on a manual milling machine. Climb milling is used predominantly in CNC machining on all metals and materials, this is due to a negligible amount of backlash on these machines. Note: Backlash is the play between the driving screw and driven nut of the machine. Remove the part and de-burr the last cut edge. Insert the work piece with the opposite end (unfinished end) protruding approx. 1 / 2. Side mill this edge removing the least amount of material to obtain a completely finished edge making the last cut a climb mill removing less than Total length of part should measure approx. 3 1 / 4 long. This completes Step 3. 23

29 Outline of pillow blocks in bar stock STEP 1: End milling 1 st edge.500 STEP 2: End milling of 2 nd edge STEP 3: Side milling using climb milling for finishing cut STEP 4: Scribe line thru center and cut with band saw STEP 5: End mill the pillow blocks individually FIGURE 18: STEPS FOR MILLING PILLOW BLOCKS 24

30 Note: Climb milling is when the work piece travels with the direction of the cutter rotation. Conventional milling is when the work piece travels against the rotation of the cutter, shown in Figure 19. FIGURE 19: TOP VIEW OF CLIMB MILLING AND CONVENTIONAL MILLING Remove the part from the vise and scribe a line dividing the part into two equal sections lengthwise. Using the Band Saw cut the part in two through this line. Consult the instructor on the safe and correct use of the Band Saw prior to use. Place one of the previously cut pieces in the vise protruding approx. 1/2 with the rough cut edge facing up as shown in Figure 18, Step 5. Face mill this piece to a height of ± Repeat this step for the 2 nd piece. De-burr with a file and check to ensure the part is square BORING THE BUSHING HOLE When a precise diameter hole is to be plunge bored with an end mill or reamer, a hole must first be drilled approx. 85% of the diameter of the finished hole size. Precision diameter holes can be bored using various techniques: Reaming Plunging into the work with a calibrated diameter end mill The center hole of the bushing was created using a reaming tool and the pillow block hole will be plunged into with a calibrated end mill tool. Clamp one block in the vise as shown in Figure 20 butting the block up to the magnet on the left side of the back jaw. The magnet acts as the position stop for the X axis.) Note: The hole boring operation will be done while the pillow blocks 25

31 are in a rectangular shape (prior to removing the material on the side) because this allows a more accommodating shape when clamping the part in the vise. FIGURE 20: VISE CLAMPING WITH ALIGNMENT USING MAGNETS Do not use excessive force when clamping as the vise is capable of exerting thousands of pounds of force on the part which can force the back jaw ( Y datum) backwards up to (This will happen on even the best vises). This will result in the final milled hole position of ± to be out of tolerance, ultimately causing the rotor assembly to bind. Insert the drill chuck in the spindle and then load a 7/16 diameter drill into the drill chuck. Turn the mill on and set the speed to approx rpm. Position X:0.875, Y: ensuring the table locks are engaged. Remove the part and repeat the drilling process for the 2 nd block. Insert the designated 1 / 2 diameter end mill into the collet. Turn on the mill and set the speed to approx rpm. Plunge the cutter through the drilled hole using the knee Z feed. Repeat for the 2 nd block. The finished product appears in Figure 21. FIGURE 21: AFTER PILLOW BLOCK HAS 0.5 HOLE MILLED The Instructor will check the hole height position relative to the base using the dial indicator installed on the height gauge. 26

32 4.3.5 MILLING THE SIDE RECESSES In order to mill the side recesses of the pillow blocks a cutter radius offset will be used as shown in Figure 22. The cutter radius offset, also commonly referred to as cutter compensation, is used to compensate for the cutting tool radius and must be offset from the cut line. Milling the side recesses in the pillow blocks will use a combination of side milling and end milling. Lines will be scribed on the blocks to give a visual reference when milling this step. As the student becomes more proficient with cutter tool offsets the scribing of visual references will not be necessary. Using the height gauge on the surface plate with the scriber tip, scribe lines in the position as shown in Figure 23, Step 1. Place the work piece in the vise vertically and ensure the cutter will not make contact with the vise. While the spindle is rotating, bring the tip of the cutter lightly into contact with the top of the block using the Z crank handle. Move off the work in the XY plane and zero the Z. Using a 1 / 2 diameter end mill cutter the radius offset will be The initial cut will be cutting along the Y axis. The roughing cut in the X should be a depth of therefore the initial X position should be: Starting Position = Cut Depth Cutter Compensation FIGURE 22: CUTTER COMPENSATION Starting Position = = Move to X: 0.100, Z: and lock the X axis. Cut completely through the width (0.5 ) of the pillow block as shown in Figure 23, Step 2. Increment the Z with the cutter to the side of the block. In this case do not plunge the cutter into the block. Remove approx vertically in Z with each cut until the depth of approx is reached. 27

33 Now make a finishing cut using climb milling which will result in a superior finish on the side. As shown in Figure 23, Step 3 moves to the final position of X: and Z: Now adjust the X position and complete the second recess. Step 1: Scribed lines for milling side recesses Step 2: 1st cut to rough out material at X:0.100 Step 3: Position of cutter for clean-up cut showing cutter offset position Step 4: Position of cutter for clean-up cut showing cutter offset position FIGURE 23: STEPS FOR MILLING SIDE RECESSES IN PILLOW BLOCK DRILLING SCREW CLEARANCE HOLES A general rule for determining screw clearance holes: Drill is approx. 5% larger than the outer diameter of the screw. For example, #10 screw = O.D x 1.05 = As there is no diameter drill select the next larger size = diameter (#7 drill). See the Common Tap and Clearance Drill Sizes chart located in the design lab for more information. 28

34 Install the drill chuck into the spindle. Using a #7 drill (0.201 diameter) to make loose clearance holes into the pillow blocks. Note: Ensure that the parallels under the part are set to the side as far as possible to avoid drilling into them. Turn the machine on and change the speed to approx rpm. Note: A tool offset is not used when drilling holes as holes are only point positions with the drill being centered to the machine spindle. 4.4 CNC MACHINING OF THE BASE PLATE The base plate machining will be a demonstration of CNC (computer numerical control) machining by the shop instructor. This demonstration will replicate a production method of machining the base plate. All milling edges, faces and drilled holes will be machined using a fixture plate and a single machine set-up. The base plate will be machined from a piece of 1 / 4 x 2.5 extruded aluminum cut to approx long. Initially two diameter holes will be drilled through the plate in the positions shown in the drawing. These two holes will serve as the machining fixture holes and hold the base plate in place during the CNC milling operation. Note: since fixture holes were incorporated into the design the work piece did not need to be clamped to a vise during machining. These simple holes allow full access to five sides of the work piece without having to remove and replace the work into the machine vise. This exponentially saves machining time! The CNC machine will cut out the outside contour first and then mill a deep pocket. This pocket is to create a flat surface for the pillow blocks to mate to in order to assure alignment. Aluminum extrusion does not often come perfectly flat; instead it can contain a slight convex or concave surface. Four tap drill holes will be drilled into the base plate in the positions indicated on the drawing using a #20 drill. (See Tap Drill Chart on the Design Lab walls for the selection of tap drill sizes). Note: Using CAD software Hole Wizard tool often results in components being over engineered. For example calling for 80% thread engagement when only 60% is required. Simple errors like this greatly increase the cost of machining. When designing a part first decide the appropriate fit required then select the drill needed from the chart. These holes will be tapped (internally threaded) using a #10-32 tap. All holes and edges are to be de-burred to assure a good mating surface of pillow block and base plate and also to prevent a person from cutting themselves while assembling components. 29

35 5 WORKS CITED [1] Dorian Tool Catalog, REVISION HISTORY Revision #: Date: Author: 1 October 11, 2002 Rodney Katz 2 October 06, 2014 Travis McKay & Jana Strain 3 October 15, 2014 Rodney Katz 30

36 7 APPENDIX A: MACHINING & DESIGN FACILITY USE POLICY 7.1 SAFETY Safe working procedures must be adhered to al all times. Familiarization with the document: Department of Mechanical Engineering Basic Safety Regulations for Instructors and Students is required. A copy is on hand in the Facility as well as at: When entering the shop for machining the first action is to sign into the Machine Equipment Sign in Book. Safety glasses must be worn at all times while using any tools and equipment or observing others machining Rushing is the main cause of accidents. Care and attention must be exercised so as not to cause injury to yourself or others. Any equipment or area requiring attention or which may cause a hazardous situation must be addressed immediately or reported to the Shop Supervisor. Shop personnel must be consulted before using any tool or method considered unsafe or with which a user is not familiar. Users are encouraged to ask questions at any time. 7.2 FACILITY DRESS CODE No open toe footwear is permitted No sleeveless shirts are permitted; at minimum a T-shirt is required. Long sleeves are recommended to avoid metal chips from irritating or burning the skin. All loose jewelry and rings must be removed before using moving equipment. Including earrings and necklaces because they can be pulled into the machine. Long hair must be tied back and up above the neck line, then constrained. Any loose hair is a major risk to personal safety; please see the shop walls for stories of fatal incidents that occurred as a result of long loose hair. A

37 7.3 GENERAL Care must be exercised so as not to cause damage or undue wear and tear to the facility. This includes protecting and maintaining equipment and fixtures as instructed by lab instructors and supervisors. Users of equipment must clean all areas of work and equipment after use to the level at which it was found. Machine tools and equipment used for the projects are to be thoroughly cleaned after use. Workbenches and the areas surrounding the equipment must be swept and vacuumed after use. Hand tools taken from the racks must be placed back following their use. All tools or materials borrowed from the Design Facility must be signed out with consent of the equipment must be swept and vacuumed after use. Hand tools taken facility personnel. 7.4 MECHANICAL ENGINEERING MACHINING FACILITY STANDARDS Drawings must be made for all work being performed in the Design Facility and submitted to the Facility personnel prior to commencing with any work. Only course related or approved projects can be worked on in the Design Facility. Machine Tools, equipment, and supplies in Room B111 are for use by the Design Facility Personnel only. Please consult first with the Facility personnel if you require supplies or tools from Room B111. B