Lathe Stud

his part named “Stud” will have some profiling on the OD (Outside Diameter) and a 1/2-20 UNC external threads on both ends.

  • Select MODEto get to the control’s Main Menu.

To make the part, we are going to separate it into two sections as shown below. This is limitation is partly due to the geometry of the right-hand face tool that will be used for turning operation and partly due to threads on both sides.

Step 1 – Setting Raw Material

  • Calibrate the right-hand face tool (tool #1), the groove tool (tool #10), and the threading tool (tool #7) as specified in Setting Up Tools Tutorial.
  • Obtain 0.5” diameter aluminium stock from stock area, about 3.2” long.
  • Hold stock in 0.5” collet and secure collet on chuck using ratchet. About 1” stock should stick out from collet/chuck. Use a chuck key to secure collet firmly.
  • Select tool #1 by pressing tool # soft key then enter [1]and press Abs Set.
  • Press Spin Speed, enter [1000], and press Inc Setto set the spindle speed to 1000 revolutions per minute (RPM)

  • Turn on spindle and face part as demonstrated in Setting Up Tools Tutorial and set Z = 0 on faced side
  • Move tool away from part and turn off spindle
  • Unscrew collet to remove part and measure the length of the part. Write this dimension down as we’ll use it to dimension part to length.
  • Hold part again in collet with non-machined side facing away from the chuck.
  • Turn on spindle and touch off tool #1 on the side sticking out and set Z=0.
  • Since we want length of stud to be 3.125” long, subtract 3.125” from the measured length.
  • Press GO TO then press x coordinate key. Enter [0] and press Abs Set. Press z coordinate, enter the difference between the measured length and 3.125” and press Abs Set. We aim to cut-off excess material and dimension part as specified on part drawing.
  • Start Spindle and move tool to Z = -0.03, X = 0.55 by turning the hand wheels. Ensure jog keys are set to fine feed by pressing F key on the computer panel.
  • Turn the X hand wheel ONLY to face off part to X = 0. Turn hand wheel continuously at a slow rate.
  • Move tool away from part in +X direction to about X = 0.55 then make another 0.03” increment along –Z direction to about Z = -0.06. Turn the X hand wheel ONLY to face off part to X = 0. Turn hand wheel continuously at a slow rate. Repeat this to the set Z GO TO limit.
  • After last pass, press RETURN to exit GO TO function then press Z coordinate key and enter [0] and press Abs Set. This sets a new origin for the part.
  • Move tool away from part and stop the spindle.

Now we move on to the process of defining the part contour.

Since we are using stock with same diameter as the part, we only need to machine the thread major diameter, thread groove relief and the threads.

Step 2 – Thread major diameter

We need to turn the thread diameter to the specifications shown then machine the thread relief groove.

The contour sketch for the thread major diameter and the groove is shown below.

Follow these steps to machine the profile.

  1. Press GO TO, then press x coordinate key. Enter [0.49] and press Abs Set. Press z coordinate, enter [-0.5], and press Abs Set.
  2. Start Spindle and move tool to Z = 0.2, X = 0.5 by turning the hand wheels. Ensure jog keys are set to fine feed by pressing F key on the computer panel.
  3. Turn X hand wheel to the set GO TO limit i.e. X = 0.49”.
  4. Turn Z hand wheel to machine along the z direction to the set Z GO TO limit of Z = -0.5.
  5. Move tool away from part in +Z direction to about Z = 0.5 or until tool is clear off part in the Z direction.

Step 3 – Machining Chamfer

To machine the chamfer at the edge of Side A, we will use the TAPER function.

  1. Press GO TO, then press x coordinate key. Enter [0.48] and press Abs Set. Press z coordinate, enter [0], and press Abs Set.
  2. Start Spindle and move tool to Z = 0, X = 0.48 by turning the hand wheels. Ensure jog keys are set to fine feed by pressing F key on the computer panel.
  3. Press RETURN to exit GO TO function.
  4. Press DO ONE – TAPER then enter [45] to set chamfer angle to 45 degrees.
  5. Turn the X hand wheel clockwise to machine fillet. Turn hand wheel until tool clears the part.
  6. Press RETURN, move tool away from part, and stop the spindle

Using a micrometer, inspect the final diameter of side A. Make necessary adjustments as required.

Step 4 – Machining Groove

The groove is defined by points shown in the diagram below.

X BEGIN marks the beginning of groove from part surface while X END marks the depth of groove. Z1 and Z2 are the same as is Z4 and Z3 for a straight groove. To machine the groove, follow these steps.

  1. Load tool #10 on the tool holder and change the tool # to 10 on the terminal. Ensure you’ve already calibrate appropriate tool. For this tutorial, we’ll use a groove tool of width 0.094”. Confirm tool width using a caliper and recalibrate the tool if necessary.
  2. Press GO TO, then press x coordinate key. Enter [0.4] and press Abs Set. Press z coordinate, enter [-0.5], and press Abs Set.
  3. Start Spindle and move tool to Z = -0.5, X = 0.55 by turning the hand wheels. Ensure jog keys are set to fine feed by pressing F key on the computer panel.
  4. Turn X hand wheel to machine to the set GO TO limit i.e. X = 0.4”.
  5. Move tool away from part in +X direction to about X = 0.55 or until tool is clear off part in the Z direction.
  6. Press GO TO, then press x coordinate key. Enter [0.4] and press Abs Set. Press z coordinate, enter [-0.531], and press Abs Set. Repeat steps 3 to 5.
  7. Move tool away from part and turn off the spindle.

Step 5 – Machining Threads

We are going to make a threading program. Below is a chart showing thread characteristics.

  1. Press MODE – PROG – GO TO BEGIN – THREAD and enter the following specifications in order. If you press GO TO BEGIN and another program appears, erase the program.
  2. Press MODE – EDIT – ERASE PROG – YES then repeat aforementioned procedure.
  • Enter [0.5] for X BEGIN.
  • Enter [0.1] for Z BEGIN.
  • Enter [0.5] for X END.
  • Enter [-0.75] for Z END.
  • Enter [0.05] for PITCH. PITCH is given by 1/No. of threads per inch
  • Enter [0.003] to set DEPTH OF PASS.
  • Enter [2] for # OF SPRING PASSES. This is the number of iterations of final cut.
  • Press Abs Set to set PLUNGE ANGLE to the default setting of [29.5].
  • Enter [2] for outside thread.
  • Enter [1] for # OF STARTS.
  • Enter [500] to set RPM.
  • Enter [7] for TOOL #

Now we need to enter or confirm the current information in the tool library. Refer to Setting Up Tools Tutorial.

  1. Press MODE to return to control main menu
  2. Press SETUP
  3. Press REF POSN to confirm tool reference position is set to X = 4.000, Z = 4.000. NOTE: It’s very important that the reference position is set to avoid crashing tool into part and/or chuck.
  4. Press RETURN to exit REF POSN.
  5. Press TOOL PATH to view the tool path graphic. If there is a program error it will be displayed now.
  6. If everything is OK, press MODE to return to the Main Menu.

We need to modify the X coordinate setting for Tool #7. This will enable us to machine threads with accuracy by starting off with a larger pitch diameter.

  1. Press SETUP – TOOL TABLE to access the lathe tool table.
  2. Using the data down and data right soft keys, scroll to Tool #7 X Modifier cell and enter 0.01”. Press Abs Set.
  3. Press MODE to exit the tool table.

Step 6 – Running Program

  1. Press RUN to enter run mode.
  2. Press START to cue up the program from the beginning.
  3. Note – the prompt invites you to press GO when you are ready to execute the program. If you press GO now – the machine will move in rapid speed up to the part and will enthusiastically begin to execute the commands you have entered. But what if you have made a mistake? You could have a crackup and damage the tool, the part, or yourself. So let’s be safe – here is a mode you should use the first time you run a new program:
  4. Press TRAKING. This will allow you control the rate of program execution by moving the hand wheels.
  5. Follow the screen prompts;
  6. Put in TOOL #7.
  7. Turn the spindle on.
  8. Press TRAKING
  9. Z- Axis hand wheel is used for aggressive feed.
  10. X- Axis hand wheel is used for fine feed.
  11. Turn the x hand wheel to machine the threads. Continue turning until the program runs over and the tool retreats to the home reference position.

Step 7 – Measuring Pitch Diameter

We use the thread micrometer with appropriate anvils to measure the pitch diameter. The expected tolerance is 0.4619” – 0.4662”.

  • Secure the anvils on the thread micrometer with the wedged anvil on the stationary arm (anvil side) of the micrometer and the pointed anvil on the moving arm (spindle). Zero the thread micrometer.
  • To measure the pitch diameter, align the anvil with a crest and a trough on the same thread as shown below. The anvils should slide back and forth over the thread as to mimic a bolt of the similar thread specifications. Read off the measurement and repeat the reading again. Take an average of three readings to be the final pitch diameter. The pitch diameter is expected to be larger than the specified pitch diameter due to the X modifier.

  • Subtract the measured pitch diameter from the specified pitch diameter. Subtract this difference from tool #7 x modifier setting by accessing the tool table as mentioned at the end of step 5.
  • Rerun the program i.e. repeat step 6.
  • Measure the pitch diameter to inspect the pitch diameter specification. If the pitch dimeter is greater than required, repeat the above steps and rerun the program.
  • If the pitch diameter is within the given tolerance range, obtain a thread plug gage and confirm that the threads fit.

  • The GO (green) gages should fit while the NO GO (red) gages shouldn’t.
  • Once thread inspection is finished, remove the part from the collet and reinsert it with the non- machined side sticking out.
 

Step 8 – Setting Raw Material

  • Hold stock in 0.5” collet and secure collet on chuck using ratchet. About 1” stock should stick out from collet/chuck. Use a chuck key to secure collet firmly.
  • Select tool #1 by pressing tool # soft key then enter [1] and press Abs Set.
  • Press Spin Speed, enter [1000], and press Inc Set to set the spindle speed to 1000 revolutions per minute (RPM)
  • Turn on spindle and touch off part as demonstrated in Setting Up Tools Tutorial and set Z = 0 on faced side
  • Move tool away from part and turn off spindle 
  • REPEAT STEPS 2 to 7. For step 5, repeat only the last section on setting x modifier for tool #7.
  • Once you’ve inspected the second set of threads, your part is ready.

⬆︎