MEAM.Design - Machining - TL-1 CNC Lathe

TL-1 CNC Lathe Guide

Welcome to a quick start guide to the Haas TL-1 lathe. This step-by-step guide will walk you through the machine start-up, setting offsets, and loading your program into the machine.

1. Obtain permission.

You will need to have a Machining Work Permit approved by a full-time member of the shop staff prior to working on the TL-1.

2. Save G-code for your machining operations onto a USB Flash drive as a .txt file.

3. Have all of the stock, tooling, and fixtures you will need to machine your part(s) on hand.

4. Start up the TL-1.

  • Before turning the TL-1 on, you must move the tailstock and carriage out of the way, both for your own safety and convenience. Both should be moved as far to the right as possible, with about two inches left between the tailstock and carriage.
  • Press the green <POWER ON> button on the upper-left corner of the machine's control panel.
  • Wait for the machine to boot up. This process will take a few seconds.
  • If an alarm screen reading "ALARM - SERVOS OFF" appears, press the orange <RESET> button to clear the alarm.

5. Set door-hold override.

  • In the DISPLAY section of the console (top-center), select the <SETNG/GRAPH> button.
  • Press the <WRITE/ENTER> button to navigate to the "PROGRAM" tab.
  • Press the ↓ (down arrow) to scroll to option 51, titled "DOOR HOLD OVERRIDE".
  • Press the → (right arrow) until the override is set to "ON".
  • Press <WRITE/ENTER>, at which point the display will prompt you that you're entering a less safe work mode.
    • Press <Y> to confirm.

6. Re-home the machine.

  • Ensure that the tailstock is cleared by moving it to the far right.
  • Press the <MDI/DNC> button, then <PRGRM CONVRS>, and <POWER UP/RESTART>.
  • The machine will go through a calibration cycle and establish a machine-zero reference point. When it has finished, the carriage will be in the lower right corner nearest the control panel.
  • The machine will prompt you to install Tool #1 and start to beep.
  • Press the <RESET> button to clear this message.

7. Set tool offsets.

A note regarding Z: You will be independently zeroing all of the tools to a known, repeatable surface, rather than to the part. We will be zeroing to 2.0000" away from the face of the chuck, using a 2" height offset gage. This is for safety so the Z-zero will clear the chuck jaws.
  • Press the <OFFSET> button once to enter the tool geometry page.
  • From here you will zero your tools in the X and Z axes.
    • To control the axes via the scroll wheel, push the <HAND JOG> button and the corresponding X+ or Z+ directional button. The resolution of the axes' movements can be set using the buttons on the right side of the control panel. A single click on the wheel can move an axis 0.1 to 0.0001 inches.
    • To control the axes via the hand wheels, push <HAND JOG>, <SHIFT>, and then the corresponding X+ or Z+ button; the screen will now display "XZ MANUAL JOG".
    • Note that the spindle can be turned on at any time while in the offset page by typing a number and pushing the spindle <FWD> button; press <STOP> to turn it off.
  • To zero the each tool, you first have to make sure that the tools are cutting at the correct height.
    • Load a piece of sacrificial stock into the chuck, and face a small section. Change the tool height if necessary, and repeat until the tool is on center.
    • Left-handed cutters can be checked visually by loading a center in the tailstock.
  • To set a tool offset in Z:
    • Place the height gage on the chuck face.
      • NOTE: You can also place the gage on any other repeatable surface to set tool length offsets, but there must be a conductive path for the height gage to function properly.
    • Select a value for the jog rate and jog the tool over until it nearly contacts the height gage.
    • Press the <.001> button and position the tool until the red indicator light turns on. Retract the tool until the indicator light just turns off.
    • Press the <.0001> button and repeat the previous step. After the indicator light turns off, remove the height gage and move the tool back .0001". This is to prevent the tool from scratching the tip of the height gage.
    • Navigate to the Z offset of the tool and press the <Z FACE MESUR> button.
    • Repeat this process for all tools.
      • NOTE: Left-handed cutters can be zeroed using two 1-2-3 blocks to position the height offset gage facing left. Depending on how this is done, you should end up 1.0000" away from the chuck face. This can be fixed by re-positioning the tool one inch over and pressing <Z FACE MESUR> again.
  • To set a tool offset in X:
    • Load a sacrificial piece of stock into the chuck.
    • Take a light turning pass to create a qualified surface. Do not change the position in X after taking this cut.
    • Measure the diameter of the stock with a micrometer and take note of this value.
    • Navigate to the X offset of the tool and press <X DIA MEASUR>.
    • Input the measured value of the stock and press <WRITE/ENTER>.
      • NOTE: You will want to check this by commanding the machine to move to an X position to take a light turning pass. Then, measure the diameter and confirm that the value matches the X position. Press <MDI DNC> and use the following code to position the tool in X:
      G54 T1 X(Desired Position).
    • Repeat this process for all tools.
      • NOTE: Boring tools can be checked by running the spindle in reverse and cutting on the opposite side of the stock. Enter a negative diameter after pressing <X DIA MESUR>.

8. Establish the X-Z origin of your part.

  • Press the <OFFSET> button until the lower pane is highlighted.
  • Use the cursor keys to highlight the X or Z entry in your coordinate system.
    • Unless you have a reason to do otherwise, use the G54 coordinate system; this is the default for our machine. This is the coordinate system that the machine will use to run your CAM file; if this is incorrect, then your part will be completely wrong and you risk crashing the machine.
  • Input an X or Z offset and press <F1> to set a zero into that register.
  • NOTE: It is generally sufficient to leave the work offset as zero and use the tool offsets, unless you are using special fixturing or need a particular zero.

9. Load your G-code into active memory.

  • Insert your USB drive into the side of the control panel.
  • Press the <LIST PROG> button.
    • You will see two tabs: one that says "MEMORY", and one that says "USB DEVICE".
    • Press the → (right arrow) to navigate to the "USB DEVICE" tab.
    • Press <WRITE/ENTER> to select the program.
    • Press <F2>. The machine will prompt you to save the program to either "MEMORY" or "USB DEVICE".
    • Select "MEMORY" and press <WRITE/ENTER> to paste the program to the machine's memory.
  • To navigate to your file, press the <MEM> button and you should see your program in the left side pane.
    • NOTE: Your G-code should be double-checked by an authorized individual. Make sure to check the X and Z positions at the start of the program and when there are tool changes. A suggested starting point is (X8.0, Z5.0) to clear your part and allow easy tool changes, depending on your part dimensions.
  • To make edits to your code on the machine, press the <EDIT> button and navigate to the proper line.
  • Input the correct code and use the four buttons to the right of the <EDIT> button as needed.

10. Simulate and run your code.

You may not operate the Haas without supervision from an authorized individual—this individual will tell you everything you need to know.
  • While in the edit mode, press the <CYCLE START> button to simulate your program on the display.
  • Press the <MEM> button to navigate to your program.
  • Run your program by pressing <CYCLE START>. The spindle will start and the tool post will begin moving.
    • NOTE: It is a good idea to start by "cutting air". You can do this by removing your stock or setting a positive Z work offset that clears your part.
The TL-1 has been known to attack its operator if it is not shown enough respect, so beware!