Machining Technology

Conventional, or manual, milling machines are primarily used to machine flat and angled surfaces by feeding a workpiece into a rotating cutting tool to remove material. They are also commonly used to position work more accurately for the same type of holemaking operations than can be accomplished with a drill press. By combining these operations, components can be machined to countless desired shapes.

Speeds and Feeds for Milling Operations

Calculating spindle RPM for milling operations is the same as calculating RPM for drill press operations. Use the standard formula RPM = 3.82 X CS / D where CS = cutting speed in surface feet per minute and D = diameter of the cutting tool. Milling machines also use IPM (inches per minute) for power quill feed settings. To calculate IPM, the following formula is used: IPM = FPT X N X RPM, where FPT = feed per tooth, N = number of teeth, or flutes, of the cutting tool, and RPM = spindle RPM.

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.

Square

Squaring a workpiece means machining the sides of a workpiece perpendicular and parallel to each other. Before beginning, take a few minutes to check the alignment of the machine head and the milling vise. If the head is not trammed and the vise is not aligned, it may be impossible to create a "square" block. A small workpiece like this can be machined using the face of an endmill. I always face off the workpiece before do other operations. The end can be machined by peripheral milling using an endmill. Use the quill to position the endmill vertically. Remember to bring the quill stop against the micrometer adjusting nut and lock the quill. Set depth of cut using the X-axis and then lock it in place to prevent movement during the milling pass. Set a "0" on the DRO to establish a reference position, then machine roughing passes within about 0.010" to 0.020" of final size using DRO to set cut depth. Next, I create a flat reference surface which will then be used position the work as other surfaces are machined. Using the largest surface will minimize any setup errors when machining other sides of the block. If a smaller surface is used to orient the block for cutting a larger surface, any setup error will be multiplied. The less the quill is extended, the more rigid the machine setup. Lock the saddle before milling. If the surface is rougher than desired, decrease the feed rate until an acceptable finish is reached. Spindle speed may also be increased about 10%-20% when taking light finishing cuts to improve surface finish. Remember to check for parallelism between sides by measuring near the four corners. Whenever possible, measure the workpiece while it is still mounted in the vise. This keeps the machined surface on the same plane, which eliminates setup errors that can be caused by repositioning the work.

Project 2

Step Block

Project 3

123 Block

Holemaking operations are performed on the vertical milling machine. The work can be precisely moved using the table and saddle movements to align the work with the spindle. The digital readout (DRO) can also be used to create precise spacing between hole locations or between edges and hole locations. It is a good practice to lock both saddle and the table before creating holes to ensure that neither moves during the actual machining operation.

When the location of a hole from a reference edge is more critical, an edge finder can be used to very accurately find a reference edge. Carefully move the table to bring the edge finder in contact with the edge of the workpiece. Continue to slowly move the table. Notice that the tip will begin to run more true as the workpiece pushed the tip into alignment with the shank. When the tip "kicks," the position of the center of the edge finder (and the machine spindle) is one-half of the edge finders tip diameter from the edge of the workpiece. Every time you remove the workpiece from the workholding device, make sure that you know the reference '0" position from the edge of the workpiece so you can reestablish the coordinate locations from the same edge. Follow these steps to machine holemaking operations:

Project 4

Clamp

A pocket is an internal part feature machined into the surface of a workpiece. Pocket location and size can be controlled by using the DRO to monitor table and saddle movements. Follow these steps to machine a pocket:

Project 5

  1. Tools:
    1. 4-flute HSS endmill ½
    2. ngle block or V-block

  2. Dimension: 1.490”W X 1.875”L X 0.990”H

  3. RPM: 500

  4. Material: cold roll steel or mild steel

  5. Milling Operations:
    1. Debur the block
    2. Square the block
    3. Cut the center slot
    4. Cut the step
    5. Mill the angle

      1. Machine Setup
        • Use parallels to raise the workpiece in the vise.
        • Load the workpiece into the vise.
        • Tighten the vise.
        • Assure there is no debris on the arbor and the spindle.
        • Load a tool into the spindle.
      2. Square the block
        • Determine the Feeds and Speeds for the squaring operation.
        • Set the Feeds and Speeds on the milling machine.
        • Face off before square the block.
        • Remove the necessary amount of material to square the top of the part.
        • Use a micrometer to check for taper in the squared part.
        • Use a micrometer to check for parallelism in the squared part.
        • Fix a tapered part.
        • If the horizontal spindle surface grinder is used for the finish, leave extra 0.005 for the dimensions.
      3. Cut the center slot
        • Determine the depth of cut (no more than half the diameter of the cutting tool).
        • Divide the length of the workpiece in half: 1.875 / 2 = 0.9375
        • Depth: 0.990 – 0.187 = 0.803 or 0.187 deep
      4. Cut the step
        • Determine the step’s location on the X-axis: 1.490 – 0.375 = 1.115 or 0.375 wide
        • Determine the depth’s location on the Z-axis: 0.990 – 0.375 = 0.615 or 0.375 deep
      5. Angular milling
        • Use V-block or angle block to mill the angular part 45 degree and 0.250 depth.
        • 0.990 – 0.250 = 0.740 or 0.250 deep

Project 6

  1. Tools:
    1. Roughing 4-flute HSS endmill:5/8
    2. Finishing 4-flute HSS endmill:1/2
    3. Center drill #1 and #3
    4. Chamfer endmill
    5. HSS twist drill
    6. Tap drill #7
    7. Boring Head

  2. Dimension: 1.875”W X 2.50”L X 1.375”H

  3. RPM: 500

  4. Material: cold roll steel or mild steel

  5. Milling Operations:
    1. Deburr the block
    2. Square the block
    3. Cut the first step
    4. Cut the second step
    5. Cut the center slot
    6. Center drill
    7. Tap drill
    8. Drill a thru hole
    9. Bore the 0.750" hole
    10. Countersink

      1. Machine Setup
        • Use parallels to raise the workpiece in the vise.
        • Load the workpiece into the vise.
        • Tighten the vise.
        • Assure there is no debris on the arbor and the spindle.
        • Load a tool into the spindle.

      2. Square the block
        • Determine the Feeds and Speeds for the squaring operation.
        • Set the Feeds and Speeds on the milling machine.
        • Face off before square the block.
        • Remove the necessary amount of material to square the top of the part.
        • Use a micrometer to check for taper in the squared part.
        • Use a micrometer to check for parallelism in the squared part.
        • Fix a tapered part.
        • If the horizontal spindle surface grinder is used for the finish, leave extra 0.005 for the dimensions.

      3. Cut the first step
        • Determine the step’s location on the X-axis: 1.50 or 1.00 wide
        • Determine the depth’s location on the Z-axis: 0.750 or 0.625 deep

      4. Cut the second step
        • Determine the step’s location on the X-axis: 1.00 or 0.50 wide
        • Determine the depth’s location on the Z-axis: 1.125 or 0.250 deep

      5. Cut the center slot
        • Divide the length of the workpiece in half: 1.875 / 2 = 0.9375
        • Depth: 1.000 or 0375 deep

      6. Center drilling
        • Use an edge finder to locate four holes.
        • Center drill each of the 4 holes on the part. Use ¼ of the normal RPM. A center drill is used to create a more positive starting point for a twist drill.

        • Use center drill # 1 for:
        • 1st hole: X = 0.125, Y = 0.250
          2nd hole: X = 0.812, Y = 1.687

        • Use center drill # 3 for:
        • 3rd hole: X = 0.500, Y = 0.937
          4th hole: X = 2.000, Y = 0.500

      7. Drill the two holes:
        • Use drill size 0.123
        • 1st hole: X = 0.125, Y = 0.250, Z = 0.50
          2nd hole: X = 0.812, Y = 1.687, Z = 0.50

        • The depth stop on the mill quill can be used to set the depth.
        • Use peck drilling to clear chips from the point.
        • Use a gage pin to check the full-diameter depth of a hole.

      8. Tap drill
        • Use drill size 0.2010 for tap 0.250-20 UNC-2B
        • 3rd hole: X = 0.500, Y = 0.937, Z = 0.70

        • Drill the tapped hole.
        • The depth stop on the mill quill can be used to set the depth.
        • Use peck drilling to clear chips from the point.
        • Use a gage pin to check the full-diameter depth of a hole.

        • Countersink bored hole: 0.03 X 45 degree
        • Use ¼ of the drilling RPM.

        • Determine the correct tap drill size.
        • Use oil.
        • Start tapping the hole using a dead center and a taper tap.
        • Continue tapping the hole with a plug tap.
        • Finish tapping the hole with a bottoming tap.
        • When tapping, advance the tap about one half to one full turn at a time. The tap should then be backed out by half a turn before continuing. This helps break the chip being formed as it cuts. Not backing the tap up will often cause the tap to bind in the hole and break.

      9. Drill and bore a thru hole
        • Use drill size 0.710
        • Use 250 RPM for drilling.
        • 4th hole: X = 2.000, Y = 0.500

        • Calculate and set an appropriate spindle speed. Because boring bars are less rigid than other holemaking tools, spindle speeds will need to be reduced by one-fourth to one-third of the calculated RPM for a drill of the same diameter as the diameter to be bored. This will help reduce excessive vibration and chatter.
        • Machine a check cut with the boring bar.
        • Use a dial indicator to adjust the boring bar.
        • Bore hole to final size.

        • Countersink bored hole: 0.03 X 45 degree
        • Use ¼ of the drilling RPM.

      10. Backside of the part
        • Load countersink and locate hole to be countersunk: 0.03 X 45 degree
        • Use ¼ of the drilling RPM.