Haas Mini Mill & Super Mini Mill 2

How to start, set up, run and look after the two Haas vertical mills in the shop.

Download the PDF (print version)

About this guide

This guide covers the two Haas vertical mills in the shop: the Mini Mill and the Super Mini Mill 2. Both use the same Haas control, so one set of steps works on either machine. Figures below are Haas catalog values for the base models; confirm them against each machine's serial plate.

Mini Mill Super Mini Mill 2
Travels X × Y × Z 16" × 12" × 10" 20" × 16" × 14"
Spindle 40 taper, 6,000 rpm 40 taper, 10,000 rpm
Tool changer 10-tool umbrella (standard) Confirm on machine
Shop extras seen in photos Tool cart with offset tags Tool cart with offset tags, probe

Who reads what:

  • Students: Safety rules, Know the machine, Student operating steps, and the Quick cards.
  • Students writing programs: Fusion to machine, and Hand-written G-code.
  • Instructor: Instructor maintenance, and the To confirm list at the end.

The steps assume the Haas Next Generation Control (NGC). The 2018 decals on the machines suggest NGC, but this needs a look at the screen to confirm.

Safety rules

No student runs either mill until the instructor has signed them off on this section. These are draft shop rules; edit them to match school policy.

Before you touch the machine

  • Safety glasses on. Long hair tied back. No gloves, loose sleeves, lanyards, rings or dangling jewelry.
  • Closed-toe shoes. No headphones.
  • One operator at the control. Everyone else stays behind the operator.
  • Know where the red EMERGENCY STOP button is before you press anything else.

While the machine runs

  • Doors closed whenever the spindle turns or a program runs. Never defeat a door interlock.
  • Never reach into the enclosure while anything is moving. Wait for the spindle to stop completely.
  • Stay at the control with a hand near FEED HOLD for the whole program. Never leave a running machine.
  • If something sounds, looks or smells wrong, press FEED HOLD. If there is danger to a person or the machine, press EMERGENCY STOP. Then get the instructor.

Tools, chips and coolant

  • Cutting tools are sharp even when still. Hold a tool holder by its body, not by the cutter. Use a rag for large cutters.
  • Never clear chips by hand or with compressed air aimed at yourself or others. Use a brush or the chip hook.
  • Coolant on the floor is a slip hazard. Wipe it up straight away.
  • Only machine materials the instructor has approved. The decal on the machine prohibits ceramics; ask before cutting anything other than aluminum, steel, brass or machinable plastic.

Which stop to use

Button What it does When to use it
FEED HOLD Stops axis motion; the spindle keeps turning. CYCLE START resumes. Anything you want to pause and check
RESET Stops the program, spindle and coolant; clears alarms The run is over or wrong and you want to start again
EMERGENCY STOP Stops all motion and shuts off the servos Danger to a person or an imminent crash

Know the machine

A vertical mill moves a part under a spinning cutter along three axes. Stand at the control, facing the doors:

Axis What moves Positive direction, as the tool sees the part
X Table, left and right Tool moves right across the part
Y Table, toward and away from you Tool moves toward the back of the part
Z Spindle head, up and down Tool moves up, away from the part

Two zero points matter. Machine zero (home) is fixed by the machine and found at power-up. Part zero is a point you choose on your part; the machine stores it as work offset G54. Your Fusion setup and the machine must agree on where part zero is.

Two offsets make a program run in the right place. The work offset (G54) tells the machine where the part is in X and Y. The tool length offset (H number) tells it how long each tool is, so every tool reaches the same Z height.

The control panel at a glance

The panel has well over a hundred keys, but they sort into eight groups, and a first job uses about two dozen of them. Learn the groups before the keys.

Function keysJog keysOverride keys Display keysCursor keysLetter keys Mode keysNumber keysOutside the keypad, always in reach Start up and set offsetsMove an axis by handSlow down or speed up a run Choose what the screen showsMove around menus and programsType program words and names Pick a mode first, every timeType values, then confirm The keys that belong to a modesit in the row to its right EMERGENCY STOP, CYCLE START, FEED HOLD, the jog handle, POWER ON and POWER OFF, the USB port RESET, POWER UP, PART ZERO SET+X, -X, +Y, -Y, +Z, -ZFEEDRATE, SPINDLE, 5% RAPID POSITION, OFFSET, ALARMS, SETTINGArrows, HOME, END, PAGE UP / DOWNA to Z, SHIFT, EOB 0 to 9, CANCEL, ENTER EDIT, MEMORY, MDI,HANDLE JOG, LIST PROGRAM
A schematic of the Haas keypad. Positions are approximate; check them against the real control.

Read it in this order: choose a mode on the right, use the display keys to see what you need, then act with the function, jog or number keys. If a key seems to do nothing, the machine is usually in the wrong mode.

Three habits make the panel manageable:

  • Mode first. HANDLE JOG to move by hand, MDI for a one-line command, MEMORY to run a program, EDIT to change one, LIST PROGRAM to choose one.
  • The screen tells you the mode. The current mode is shown at the top left of the display. Check it before pressing CYCLE START.
  • Ignore the rest for now. Keys not named in this guide are for features you will not use in your first projects.

Keys you will use

Group Keys What they are for
Power POWER ON, POWER OFF, EMERGENCY STOP Starting and stopping the machine
Start-up RESET, POWER UP Clearing alarms; homing all axes
Modes HANDLE JOG, MDI, MEMORY, EDIT, LIST PROGRAM Moving by hand; one-line commands; running, editing and choosing programs
Displays POSITION, OFFSET, CURRENT COMMANDS, ALARMS Where the machine is; offsets; tool table; alarm text
Setup TOOL OFFSET MEASURE, NEXT TOOL, TOOL RELEASE, PART ZERO SET, ATC FWD, ATC REV Measuring tools, loading tools, setting part zero
Running CYCLE START, FEED HOLD, GRAPHICS, SINGLE BLOCK, 5% RAPID, 25% RAPID, FEEDRATE −10% / +10% Starting, dry-running on screen, pausing and slowing a program

Tool carts and yellow tags

Each mill has a cart of tool holders. A yellow tag under each holder gives its tool number, a description and an H value, for example a 5/16" drill tagged T14 with H 6.1037. The Super Mini Mill 2 cart also holds a probe.

  • A tool always goes back in its own tagged slot.
  • The tool number on the tag must match the tool number in your program.
  • Never swap a cutter in a holder without telling the instructor. The H value on the tag is then wrong.

Student operating steps

Every job follows the same eight stages, in this order. Key names are in capitals as printed on the control.

1. Power up

  1. Check the area: doors closed, nothing loose on the table, no tools left inside.
  2. Check that shop air is on. A low-air icon on the screen means the machine will not run until pressure is restored.
  3. Press POWER ON and wait for the control to finish starting.
  4. Turn the EMERGENCY STOP button clockwise to release it, then press RESET to clear alarms.
  5. Open and close the door once if the screen shows a cycle-door icon.
  6. Check the table and spindle have a clear path, then press POWER UP. All axes move to home straight away. Stand clear.
  7. At the start of every school day, run the 20-minute warm-up program O09220 before anyone cuts. School policy is a daily warm-up, whatever the machine did the day before.

2. Hold the part

  1. Wipe the vise jaws, the parallels and the bottom of your stock. One chip under the part ruins the cut.
  2. Seat the stock on parallels with enough material above the jaws for your deepest cut.
  3. Tighten the vise firmly and tap the stock down with a soft mallet. Remove the vise handle.
  4. Check that the stock size and orientation match your Fusion setup.

3. Load tools

  1. Collect only the tools your program calls, from their tagged cart slots.
  2. Press MDI. Type T and the tool number, for example T3, then press ATC FWD. The machine brings that pocket to the spindle.
  3. Hold the tool by the holder body. Line up the two slots in the holder flange with the drive keys on the spindle.
  4. Press and hold TOOL RELEASE, push the holder up into the spindle, then let go of the button. Tug down gently to confirm it is clamped before you let go of the holder.
  5. Repeat for each tool.

The Super Mini Mill 2 may have a side-mount tool changer, which also needs each tool entered in the tool table under CURRENT COMMANDS. The instructor will show which changer each mill has.

4. Set tool length offsets

The H value for each tool must be in the control before you run. In this shop the value may come from the yellow tag or the probe; ask the instructor which. The manual touch-off method is:

  1. Bring the tool into the spindle. Press HANDLE JOG, then .1 for fast jogging.
  2. Jog X and Y until the tool is over the middle of the part. Jog Z down to about 1" above it.
  3. Press .0001 for slow jogging. Hold a slip of paper flat on the part and lower the tool until the paper just drags.
  4. Press OFFSET and choose the TOOL tab. Highlight the H (length) Geometry value on that tool's row.
  5. Press TOOL OFFSET MEASURE. Check the number changed. Press Y if the control asks you to confirm a large change.
  6. Press NEXT TOOL. The spindle moves up quickly and changes tools. Repeat for each tool.

5. Set part zero (G54)

  1. Load the pointer or edge finder the instructor specifies.
  2. Press HANDLE JOG, then .1. Jog Z to about 1" above the part, then switch to .001 and come down to about 0.2".
  3. Jog X and Y to your part zero. Use the same corner you picked in Fusion.
  4. Press OFFSET and choose the WORK tab. Move the cursor to the G54 X value.
  5. Press PART ZERO SET once to store X. Press it a second time to store Y.
  6. Stop there. A third press writes a Z value into G54 and can crash the tool into the part.

6. Load the program

This is the sequence posted on the Super Mini Mill 2.

  1. Plug your USB drive into the port on the side of the control.
  2. Press LIST PROGRAM. Arrow across to the USB tab (or MEMORY if the program is already on the machine).
  3. Arrow down to your file and press SELECT PROGRAM. The active program is marked with an asterisk.
  4. Press MEMORY. Check that the program name at the top of the screen is yours.

To keep a copy on the machine instead: highlight the file on the USB tab, press ENTER to tick it, press F2, choose Memory, and press ENTER. Only .nc files copy to memory.

7. Prove it out

No program cuts metal until it has passed both checks.

On screen

  1. In MEMORY mode press GRAPHICS, then CYCLE START. The program is drawn on screen and nothing moves.
  2. Check the shape, the size and the depth against your drawing. Press F2 to zoom.
  3. Fix any alarm before going further. Get the instructor's OK.

First real run

  1. Press MEMORY to leave graphics. Close the doors.
  2. Press 5% RAPID and turn on SINGLE BLOCK.
  3. Press POSITION and choose the DIST TO GO tab. It shows how far the machine will travel on the current line.
  4. Press CYCLE START once per line. Keep your other hand on FEED HOLD.
  5. Watch the first approach to the part. If the tool is 1" above the part and Dist To Go for Z reads more than 1", press FEED HOLD and get help.
  6. Once the first tool is cutting correctly, turn off SINGLE BLOCK. Raise rapids to 25% only when the instructor agrees.

8. Finish and shut down

  1. Wait for the spindle to stop and the program to end before opening the doors.
  2. Remove the part. Deburr sharp edges at the bench, not in the machine.
  3. Brush chips off the vise and table into the chip pan. Wipe the vise jaws.
  4. Return every tool holder to its tagged cart slot.
  5. Remove your USB drive. Tell the instructor about any alarm, odd noise or broken tool.
  6. Press POWER OFF only if the instructor asks. Otherwise leave the machine homed with doors closed.

Fusion to machine

A Fusion program runs correctly only when four things match the machine: part zero, tool numbers, units and the post processor.

In Fusion (Manufacture workspace)

  1. Setup. Set the stock to the real size of your material. Put the work coordinate origin on the corner and face where you will set G54 at the machine. Top of stock, back-left corner is the usual shop choice.
  2. Tools. Pick tools from the shop tool library so each tool number matches its yellow tag. Never invent a tool number.
  3. Toolpaths. Keep clearance and retract heights well above the vise and clamps.
  4. Simulate. Run the simulation with stock shown. Fix every red collision mark before posting.
  5. Post process. Choose the post that matches the control:
Control on the machine Fusion post to use Output file
Next Generation Control HAAS - Next Generation Control .nc
Older (classic) control HAAS (pre-NGC) .nc

Give the program a number and a short name with your initials. Save the .nc file to your USB drive.

Before you walk to the machine

Open the .nc file in a text editor and check five things:

At the machine

Follow stages 6 and 7 of the operating steps: load from USB, run in graphics, then single-block the first run at 5% rapid.

Common mismatches

What you see Likely cause
Graphics shows the part far off the table Fusion origin is not where G54 was set
Tool stops well above the part, or dives toward it Wrong H value, or the wrong tool in that pocket
Alarm as soon as the program starts Wrong post, or a tool number the machine does not have
Part is 25 times too big or too small Inch and metric mixed up
Rapids look slow and steady in a pre-NGC program That post outputs positioning moves as fast feed moves by default

Hand-written G-code

A mill program is a list of lines the machine reads top to bottom: set up safely, pick a tool, move, cut, retract, stop. Reading G-code lets you spot a bad Fusion program before it cuts.

Starter program

This cuts one straight slot 0.050" deep along X with a 1/2" end mill. Part zero is the top, back-left corner of the stock. It is a teaching example with gentle numbers for aluminum; prove it out in graphics like any other program.

%
O01001 (SLOT - YOUR INITIALS)
(T1 = 1/2 END MILL)
G20 G17 G40 G49 G80 G90 (SAFE START: INCH, XY PLANE, CANCEL COMP AND CYCLES, ABSOLUTE)
T1 M06 (LOAD TOOL 1)
G00 G54 X-0.5 Y-1.0 (RAPID TO START, LEFT OF THE PART)
S3000 M03 (SPINDLE ON CLOCKWISE, 3000 RPM)
G43 H01 Z1.0 (APPLY TOOL 1 LENGTH, STOP 1 INCH ABOVE PART)
M08 (COOLANT ON)
G00 Z0.1 (RAPID CLOSE TO THE SURFACE)
G01 Z-0.05 F10. (FEED DOWN TO DEPTH)
G01 X3.5 F20. (CUT THE SLOT)
G00 Z1.0 (RETRACT)
M09 (COOLANT OFF)
M05 (SPINDLE STOP)
G28 G91 Z0. (Z TO MACHINE HOME)
G28 G91 Y0. (TABLE FORWARD TO UNLOAD)
G90
M30 (END AND REWIND)
%

Codes worth knowing

Code Meaning
G00 Rapid move, not for cutting
G01 Straight cutting move at feed rate F
G02, G03 Arc clockwise, arc counter-clockwise
G20, G21 Inch, metric
G28 Return to machine home
G40, G41, G42 Cutter compensation off, left, right
G43 H__ Apply the length offset for that tool
G54 Use the first work offset (part zero)
G80, G81, G83 Cancel drill cycle, drill, peck drill
G90, G91 Absolute positions, incremental moves
M03, M05 Spindle on clockwise, spindle stop
M06 Tool change
M08, M09 Coolant on, off
M00, M01 Stop, optional stop
M30 End of program and rewind

Writing and editing at the control

  • New program: press LIST PROGRAM, then INSERT. Enter an O-number and, if you like, a file name and comment.
  • Edit: select the program, press EDIT, type a change, then use INSERT to add it, ALTER to replace the highlighted word, DELETE to remove it and UNDO to step back.
  • One-off commands: press MDI, type a line such as S1000 M03, then press CYCLE START. Nothing typed in MDI is saved as a program.
  • VPS templates: the control's Visual Programming System builds common features, such as engraving or bolt circles, from a fill-in form.

Decimal points matter. On a Haas, X2. means two inches; X2 without the point may be read as a much smaller move, depending on a machine setting. Always type the decimal point.

Quick cards

Four cards to print and post at each mill. Each is a short reminder for a student who has already been trained on the full steps above.

Card 1: Start-up

  1. Glasses on, hair back, no gloves.
  2. Doors closed, table clear, air on.
  3. POWER ON. Release EMERGENCY STOP. Press RESET.
  4. Cycle the door if asked.
  5. Path clear? Press POWER UP and stand back.
  6. First thing every day: run warm-up O09220.

Card 2: Set up

  1. Clean the vise. Seat the stock on parallels. Tighten. Handle off.
  2. Load each tool: MDI, type T and the number, ATC FWD, then TOOL RELEASE to seat it.
  3. Tool lengths: OFFSET, TOOL tab, TOOL OFFSET MEASURE, NEXT TOOL.
  4. Part zero: OFFSET, WORK tab, cursor on G54 X, PART ZERO SET twice. Never three times.

Card 3: Load and run

  1. LIST PROGRAM. Arrow to USB. Arrow to your file.
  2. SELECT PROGRAM, then MEMORY.
  3. GRAPHICS, then CYCLE START. Check the picture. Get the instructor's OK.
  4. MEMORY again. Doors closed.
  5. 5% RAPID and SINGLE BLOCK on. Watch Dist To Go.
  6. CYCLE START with a hand on FEED HOLD.

Card 4: Stop and clean up

If Then
You want to pause and look FEED HOLD
The run is wrong RESET, then get the instructor
Danger to a person or a crash is coming EMERGENCY STOP
An alarm appears Do not clear it. Read it, write it down, get the instructor

When finished: spindle stopped, part out, chips brushed into the pan, vise wiped, tools back in tagged slots, USB out.

Instructor maintenance

Most of the upkeep is a two-minute daily look and a weekly check of coolant and air; the rest is monthly or slower. Intervals below follow Haas's VMC Maintenance Schedule. The Haas site would not load the full page while this was written, so the table was assembled from search excerpts of it. Check it against the live page before treating it as final.

Schedule

Interval Task System
Daily Inspect the windows for damage Enclosure
Daily Check the door interlock works Enclosure
Weekly Clear chips from the tool changer Tool changer
Weekly Check coolant level Coolant
Weekly Check coolant concentration with a refractometer and log it Coolant
Weekly Check the spindle air regulator pressure Pneumatics
Monthly Check the axis lubrication reservoir and refill Axis lubrication
Monthly Check the spindle lubrication tank level Spindle lubrication
Monthly Clean the vector drive air vents and filter Electrical cabinet
Monthly Inspect and lubricate the way covers Enclosure
Monthly Umbrella changer: inspect motors and sensors; grease guide rails and extractor fingers Tool changer
Quarterly Side-mount changer: check cambox oil level Tool changer
Six months Drain and clean the coolant tank; replace coolant; clean the coolant filter Coolant
Six months Run the axis and spindle lubrication tests Lubrication
Six months Inspect air and lubrication hoses for cracks Pneumatics, lubrication
Six months Probe: check batteries and calibration Probe
Six months Side-mount changer: inspect arm plunger; clean and lubricate pocket plungers Tool changer
Annually Measure spindle drawbar force Spindle
Annually Clean the air purge solenoid Pneumatics
Annually Side-mount changer: grease cams; replace worn pocket parts Tool changer
As required Clean the coolant filter screen; clean and lightly oil the spindle taper; grease pull studs Coolant, spindle, tooling

In a student shop it is worth doing the weekly coolant and chip items daily, since many hands use the machine.

Daily walk-round for a student shop

These are shop practice, not Haas requirements.

When something stops the machine

Condition First things to check
Low-air icon or alarm Compressor running, shop air valve open, regulator pressure at the machine
Machine will not start a program Doors closed, EMERGENCY STOP released, RESET pressed, axes homed with POWER UP
Tool change stopped part-way Do not force the carousel. Read the alarm, then follow the tool changer recovery prompts on the control
Over-travel or travel-limit alarm Part zero or the Fusion origin is wrong; the program is asking for a move outside the machine's travels
Tool cuts air or cuts too deep Wrong H value for that tool, or the tool was changed in its holder
Poor finish, squealing Dull or chipped cutter, part loose in the vise, speeds and feeds too high

Press ALARMS for the alarm number and text, and look the number up in Haas's online alarm reference. For anything electrical, inside the cabinet, or involving the spindle or drawbar, call the Haas Factory Outlet rather than opening the machine.

To confirm in the shop

Eight details could not be read from the photos. Each one changes a line in this guide.

Sources

Pages opened and read for the procedures:

Pages found by search but not opened in full; details taken from search excerpts and due a re-check:

The safety rules, the starter program, the daily walk-round and the troubleshooting table are general machining practice written for this guide, not taken from a Haas document.