Machining Technology

The engine lathe is one of the most versatile and oldest machine tools in the machining field. The principal operation of the engine lathe is to rigidly hold and rotate a workpiece against a cutting tool. The tool travels along the outside of the workpiece to shave off material and produce cylindrical parts.

Speed

The standard formula for used for lathe operations: RPM = 3.82 X CS / D where CS = cutting speed in surface feet per minute and D = diameter of the workpiece.

Feed

Feed rates for lathe operations are given in IPR (inches per revolution), or FPR (feed per revolution in inches). For example, the feed rate of 0.002 IPR (or FPR) means that every time the spindle makes one revolution, the cutting tool advances 0.002" across the surface of the work.

Time

Calculate time per cut = L / (RPM X IPR) where L is the length of the workpiece

Project 1

Before machining, I always write some notes on the drawing to make it more understanding and easier for me to make a plan.

Step Shaft

Facing and turning are two of the most common lathe operations. Facing is cutting across the end of a workpiece to machine the end flat, while turning is reducing the outside diameter of a workpiece. Avoiding excessive tool overhang provides a rigid setup and eliminates chatter or vibration. Follow these steps to machine turning operations:

Project 2

short Shaft

Use the same operations as project 1. Note that the tolerance for the diameters is now 0.005 instead of 0.015.

Project 3

Long Shaft

Use the same operations as project 2. Note that the tolerance for the diameters is now 0.002 instead of 0.005.

Project 4

Angle Shaft

Shouldering combines turning and facing to create a step where two different diameters meet. The compound rest can be positioned to machine to angular shoulder or taper.

Project 5

Turning Between Centers

  1. Tools:
    1. Center drill
    2. Inserted carbide roughing tool
    3. Inserted carbide finishing tool
    4. Grooving tool
    5. Chamfering tool
    6. Bump type knurling tool
    7. External thread cutting tool

  2. Dimension: 0.9” OD X 5.12” L

  3. RPM:
    • Roughing: 250 RPM
    • Finish: 750 RPM
    • Grooving: 80 RPM
    • Threading: 80 RPM
    • Knurling: 80 RPM
    • Filing/Sanding: 160 RPM

  4. Material: cold roll steel or mild steel

  5. Operations:
    1. Deburring
    2. Facing
    3. Roughing
    4. Finishing
    5. Shoulder Lengths
    6. Undercutting
    7. Threading
    8. Knurling
    9. Filing/Sanding

      1. Turning
        1. Facing both ends

        2. Center drilling both ends
          Use the tailstock to see if the center drill is center.
          ID = 0.25

        3. Measure the overall length of the workpiece with the height gage

        4. Use Lathe Center for roughing and finish
          The main advantage of working between centers is that work can be easily removed, turned end for end, and reinstalled with a very high level of repeatability, or accuracy. Diameters machined from each end will maintain concentricity and have very little runout because the centers accurately locate the work in the same position each time.

        5. Roughing side 1:
          Leave the OD 0.020 for finish

          Shoulder length 1:
          OD = 0.9 + 0.020 = 0.920
          L = 3.25

          Shoulder length 2:
          OD = 0.750 + 0.020 = 0.770
          L = 2.50

          Shoulder length 3:
          OD = 0.625 + 0.020 = 0.645
          L = 1.50

          Shoulder length 4:
          OD = 0.500 + 0.020 = 0.520
          L = 1.0

        6. Roughing side 2:

          Shoulder length 5:
          OD = 0.750 + 0.020 = 0.770
          L = 3.25

          Shoulder length 6:
          OD = 0.500 + 0.020 = 0.520
          L = 4.37

        7. Use the height gage to measure the all lengths

        8. Finish side 1:
          Wait for the part to completely cool after the roughing operation.

          Shoulder length 4:
          OD = 0.9
          L = 3.25

          Shoulder length 3:
          OD = 0.750
          L = 2.50

          Shoulder length 2:
          OD = 0.625
          L = 1.50

          Shoulder length 1:
          OD = 0.500
          L = 1.0

        9. Finish side 2:

          Shoulder length 5:
          OD = 0.750
          L = 3.25

          Shoulder length 6:
          OD = 0.500
          L = 4.37

        10. Use the height gage to measure the all lengths

        11. Finish Grooving Side 1:
          Reduce the RPM for the grooving operation. This undercut is a narrow groove that provides a space for the threading tool to stop after the half-nut lever is disengaged without damaging the threads.

          Groove 1: 0.600

        12. Finish Grooving Side 2:

          Groove 2: 0.600
          Groove 3: 0.37

        13. Chamfer Side 1:

          2 X 0.03 x 45 degrees
          0.06 x 45 degrees

        14. Chamfer Side 2:

          2 X 0.03 x 45 degrees
          0.06 x 45 degrees

        15. Threading ¾-16 UNF-2A

        16. Threading ½-13 UNC-2A

Project 6

  1. Tools:
    1. Center drill
    2. Inserted carbide roughing tool
    3. Inserted carbide finishing tool
    4. Grooving tool
    5. Chamfering tool
    6. External thread cutting tool
    7. 0.500” drill
    8. 0.750” drill
    9. Boring bar
    10. Internal grooving tool
    11. Internal thread cutting tool

  2. Dimension: 1.950” OD X 4.30” L

  3. RPM:
    • Roughing: 250 RPM
    • Finish: 750 RPM
    • Grooving: 80 RPM
    • Threading: 80 RPM
    • Filing/Sanding: 160 RPM

  4. Material: cold roll steel or mild steel

  5. Operations:
    The lathe project will require two setups.

    The first setup for the following external operations:
    1. Deburring
    2. Facing
    3. Roughing
    4. Finishing
    5. Shoulder Lengths
    6. Undercutting
    7. External Threading
    8. Filing/Sanding
    9. Drilling

    10. The second setup will use soft jaws for the following internal operations:
    11. Boring
    12. Undercutting
    13. Internal threading

      1. Turning
        1. Facing both ends

        2. Indicate and center drilling both ends

        3. Measure the overall length of the workpiece with the height gage

        4. Use Lathe Center for roughing and finish

        5. Roughing side 2:
          Leave the OD 0.020 for finish

          Shoulder length 4:
          OD = 1.950 + 0.020 = 1.970
          L = 0.80

        6. Roughing side 1:

          Shoulder length 1:
          OD = 1.700 + 0.020= 1.720
          L = 0.80

          Shoulder length 2:
          OD = 1.450 + 0.020 = 1.470
          L = 1.30

          Shoulder length 3:
          OD = 1.000 + 0.020 = 1.020
          L = 2.800

        7. Use the height gage to measure the all lengths

        8. Finish side 2:
          Wait for the part to completely cool after the roughing operation.

          Shoulder length 4:
          OD = 1.950
          L = 0.80

        9. Finish side 1:

          Shoulder length 1:
          OD = 1.700
          L = 0.80

          Shoulder length 2:
          OD = 1.450
          L = 1.30

          Shoulder length 3:
          OD = 1.000
          L = 2.800

        10. Use the height gage to measure the all lengths

        11. Finish Grooving Side 1:
          Reduce the RPM for the grooving operation.

          0.750
          0.200 wide: 2.800 – 3.00
          3.00 – 0.120 (tool’s tip) = 2.880

        12. Finish Grooving Side 2:

          1.250
          0.200 wide: 1.30 – 1.500
          1.500 – 0.120 (tool’s tips) = 1.38

        13. Use the height gage to measure these shoulder lengths
          Distance between two grooves: 2.800 – 1.500 = 1.300

        14. Chamfer
          0.09 X 45 degrees

        15. Threading 1.000-8 UNC-2A

        16. Filing/Sanding
          Run the spindle at about 160 RPM.
      2. Determine thread data for 1-8 UNC-2A

        Major diameter:
        Max = 0.9980
        Min = 0.9830

        Pitch diameter:
        Max = 0.9168
        Min = 0.9100

        Wire thread gage:
        Use wire size 0.072
        M = E + constant = 0.9100 + 0.10775 = 1.01775

      3. Peck Drilling
        Some lathes may have graduations on the tailstock quill or hand wheel.
        A lower RPM will allow you to clear and buildup of chips.
        Peck drilling is the process of clearing the drill from the part to clear out chips.

        1. Center drilling 0.440
        2. Spot drilling 0.500
        3. Twist drilling 0.720
      4. Clamping workpiece with soft jaw inserts
        Soft jaws will be placed between the workpiece and the jaws of the chuck to prevent marking the part during machining.

      5. Boring
        Bore the hole for a 1.250 -12 UNF-2B:
        Minor diameter = 1.160

        • Rigidity is a prime concern when boring, so use the largest boring bar as possible.
        • The longer a boring bar hangs over the tool holder the more it will flex causing unwanted chatter.
        • If chatter occurs, increase the feed rate and reduce spindle speed.
        • The boring bar should be setup as rigid as possible.
        • Zero the tool on the face of the of the part.
        • Take a check cut, measure, and put that dimension in the DRO.
        • Use a telescoping gage and a micrometer to measure the bore size.

        Rough internal shoulder lengths:
        Length 1:
        ID = 0.75 - 0.010 = 0.730
        L = 2.3

        Length 2:
        ID = 0.900 - 0.020 = 0.880
        L = 2.20

        Length 3:
        ID = 1.160 - 0.020 = 1.140
        L = 1.15

        Finish internal shoulder lengths:
        Length 1:
        ID = 0.75
        L = 2.3

        Length 2:
        ID = 0.900
        L = 2.20

        Length 3:
        ID = 1.160
        L = 1.15

        Internal Grooving
        Reduce the RPM for the grooving operation. To machine an undercut for a thread relief, use an internal grooving bar.

        ID = 1.40
        0.300 wide = 0.850 - 1.15

        Chamfering
        0.06 X 45 degrees

      6. Internal Threading
        1. Applying a coating of layout fluid to the workpiece diameter can make it easier to make a light touch.
        2. To machine an undercut for a thread relief, use an internal grooving bar.
        3. Flipping the tool, and reversing the direction of the threading operation to avoid crashing while threading internally into a blind hole.
        4. Choose a threading bar as short as possible, still having proper clearance.
        5. Be very careful when internal threading to a blind shoulder, and slow down the RPM.
        6. When necessary, in between cuts, stop the machine and remove chips.
        7. Take a scratch cut, shut the machine down, and check pitch with a thread pitch gage.

        Determine thread data for 1.250 -12 UNF-2B

        Minor diameter:
        Max = 1.178
        Min = 1.160

        Pitch diameter:
        Max = 1.2039
        Min = 1.1959