MEAM.Design - Machining - Haas Mini Mill

Haas Mini Mill Guide

Welcome to a quick start guide to the Haas Mini Mill. This step-by-step guide will walk you through the machine start-up, configuration, and pre-machining workflow.

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 Haas.

2. Save G-code for your machining operations onto a USB Flash drive as a .txt file. PLEASE CHECK YOUR COORDINATE SYSTEMS!!! This is the most important thing to check for in your G-code. The machine has six coordinate systems, spanning from G54 to G59. These are meant to be used if you are setting up multiple fixtures. However, to make life easy, please define all your operations within the G54 coordinate system. This means that when you save the G-code, YOU MUST REPLACE ALL INSTANCES OF G53, G55, G56, G57, G58, AND G59 WITH G54. This is is what happens when you don't!

NOTE: Your USB drive must be formatted as either a FAT or FAT16 file system.

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

4. Start up the Haas Mini Mill.

  • Press the green Power On button on the upper-left corner of the machine's console.
  • Wait for the machine to boot up. This process takes approximately 90 seconds.
  • If an Alarm screen reading "102 SERVOS OFF" appears:
    • Press the big red Reset button.
    • The screen should then say "NO ALARM".

5. Set door-hold override.

  • In the Display section of the console (top-center), select the Setting Graph button.
  • Press Page Down to advance to the next screen of the machine settings window.
  • Press the ↓ (down arrow) until you get to row number 51, titled "DOOR HOLD OVERRIDE". (NOTE: the rows are not in numerical order).
  • Press the → (right arrow) until the override is set to "ON"
  • Press Write | Enter, which is on the bottom-right corner of the console.
  • Press the Y button when prompted to confirm that you wish to enable the door hold override.

6. Re-home the machine.

  • Ensure that the machine's vise is empty (except for a vice-stop if one has been pre-installed).
  • If there is a tool in the spindle:
    • Firmly hold onto the tool holder and press the Tool Release button (approximately one foot above the spindle, inside the machine), holding it down for about one second. A burst of compressed air will blow away loose chips and release the tool holder from the spindle.
    • CAUTION: Tools are often heavier than they appear!
  • Press the Power Up | Restart button.
  • The machine will go through a calibration cycle, zeroing all three axes and inserting Tool #1 into the spindle.

7. Load tool carousel.

Prior to loading each tool, ensure that the taper of the tool holder is free of all debris.
After re-homing, the tool changer is ready to have Tool #1 loaded.
  • To load Tool #1 into the spindle, align the two slots on the tool holder with the corresponding posts on the spindle.
  • Insert the tool holder into the spindle, holding it approximately 1 inch below full insertion.
  • Press the Tool Release button (approximately one foot above the spindle, inside the machine), and hold it for about one second. A burst of compressed air will blow away any loose chips. Firmly press the aligned tool holder into the spindle, release the Tool Release button, and the tool will be sucked into position. Ensure the tool is secure before carefully letting go of the tool holder.
  • To insert another tool, you must CHANGE TO A DIFFERENT TOOL NUMBER:
    • Enter MDI (Manual Data Input) mode by pressing the MDI DNC button on the touch pad.
    • Use the Delete button to delete any existing code that has been entered.
    • Type "M06 TX" (where X is the tool number you wish to set the spindle to), then press Write | Enter.
    • Hit the green ''Cycle Start" button in the lower-left corner of the machine console. The machine will place the existing tool in the carousel and move to location X in the carousel. If a tool was already loaded into position X, it will be loaded into the spindle, and you will have to remove it to install a different tool.
  • At this point, repeat all of the above steps to insert the remaining tools into the spindle.

8. Set tool height offsets.

A note regarding Z: You will be independently zeroing all of the tools to a known, repeatable surface (typically the bed), rather than to the part. This provides numerous benefits, including the ability to utilize the same tools for multiple part setups, with different part Z-zero heights. Furthermore, this process allows any tool to be replaced without impacting the Z offsets of the other tools, as they are all set independently.
Using a Digital Height Gage, you must set all of the tool length offsets for your tools. The Gage is 2.0000 inches tall, but you should always verify this.
  • Use the CHANGE TO A DIFFERENT TOOL NUMBER procedure listed above to change to the desired tool. Typically, it is easiest to start with Tool #1, and set the Z-Zero of each of the tools sequentially.
  • Hit Offset to enter into the offset registry.
  • Place the height gage on the mill's bed (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).
  • Press the Hand Jog button, and then the .01 increment button. Select the Z axis by pressing either +Z or Z, and use the rotating dial to bring the tool down NEAR (but not yet touching) the top of the height gage. You might also need to jog in the X and Y axes, using the same procedure, substituting the +X/-X or +Y/-Y buttons accordingly.
  • Place the handle jog into the .001 increment by pressing the .001 button.
  • Lower the tool until it contacts the top of the gage. The red indicator light on the gage will tell you when the tool is in contact. Back off until the indicator light just turns off.
  • Select the .0001 increment by pressing the .0001 button and repeat the zeroing process.
  • Ensure that the cursor on the screen highlights the length offset for the current tool, and press the Tool Offset Measure button to set the Tool Length Offset register for that tool.
  • Repeat this process for all of the tools that have been inserted into the machine. Be consistent in your methodology.
  • Now, all of the tools have been zero'd 2.0000 inches above the bed of the machine.

9. Establish the X-Y origin of your part.

  • Mount your work to the table (via the vise or other means). Make sure it is VERY secure.
  • Using the procedures listed above, insert the digital edge-finder into a tool holder, and load that holder into the spindle.
  • Use the same hand-jog operations from Part 8 to locate the X-Axis of your machining operation. Raise the spindle, and compensate for the radius of the edge-finder!
  • Hit the Offset button twice to enter into the Work Zero Offset menu.
  • Page down (or up) until you see the G54 register (or the G55 register if your G-code is based in G55).
  • Place the cursor on the X register, and press Part Zero Set. This has now set the X-zero location for your part.
  • Repeat the same procedure to set the Y-axis.

10. Establish the Z-zero of your part.

A second note regarding Z: Recall that we set the tools relative to a known surface. In this step, we are going to determine the offset between that surface and the Z-zero height of our part.
  • Load one of your pre-set tools, Tool X, into the spindle.
  • Place the digital height gage onto the Z-Zero plane of your part (based on the settings in your G-code). NOTE: The height gage relies on the conductivity of the work surface to complete a circuit, thus indicating when the tool comes in contact with the gage. If you are machining any non-metal, you must create a conductive "bridge" in order to use the height gage.
  • Follow the same procedure defined in part 8 to locate Tool #X exactly 2.0000 inches above the Z-zero height.
  • Hit the Offset" button twice to enter into the Work Zero Offset'' Menu.
  • Page down (or up) until you see the G54 register (or the G55 register if your G-code is based in G55).
  • Move the cursor to the Z entry and type 0.000, then press F1 to set a zero into that register.
  • Note the "Z-Position" listed in the lowest row of the machine's screen.
  • Type this number (which is usually negative), and then press Write | Enter.
  • The G54 (or G55) Work Zero Offset in Z should now match the current "Z Position".
  • Press Offset to view the Tool Offset Registry.
  • Remember the Offset Length for Tool #X.
  • Press Offset again to return to the Work Zero Offset screen.
  • Move to the G54 (or G55) Z registry, and type the negative of the Offset Length for Tool #X that you just committed to memory. Press Write | Enter.
  • Type -2.0. Press Write | Enter, and the Z-Zero will be properly set to your part's Z-zero height. This step accounts for the height of the gage.

11. Load your G-code into active memory.

  • Insert your USB drive (formatted as either a FAT or FAT16 file system) into the machine.
  • Press List Prog.
  • Use the ↓ (down arrow) to scroll down the left column until "Floppy" is selected.
  • Press F4.
  • Press the → (right arrow), then the ↓ (down arrow) to scroll through the files saved on the floppy disk.
  • Once the desired file is highlighted, press Write | Enter to copy the file.
  • Press the ← (left arrow), then press the ↓ (down arrow) to scroll down the left column until "Hard Drive" is selected.
  • Press F4.
  • Press the → (right arrow).
  • Press F2 to paste the file into the hard drive.
  • The machine will say "Processing" for approximately 30 seconds. NOTE: If the machine processes for longer than 2 minutes, you will need to power-cycle the machine, set the door-hold override, and re-home the axes, then try again. Fortunately, you will not need to reset any of the tool data.
  • Once the file is ready, the screen will say "Done".
  • Press End to advance to the file most recently pasted into the hard drive. This should be your program.
  • Press Select Program to open your code.
  • Hitting Currnt Comds will show the G-code being executed by the Haas in real-time. You can use the scrolling arrows to view the tool's current position in the machine's different coordinate systems.

12. 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.

The contents of this page were derived, in part, from Stanford's HAAS Mini Mill User's Manual.