Teaching CNC Mill

General note: try to sprinkle tidbits throughout training! You don’t have to get too deep into the details before you need them.

Safety

  • Clothes should be relatively fitted to your body–no loose or flowy clothing
  • Nothing dangling off clothes–sweatshirt tassels, lanyards, etc
  • No jewelry!
  • Keep hands away from:
    • Spindle while on
    • Table–lots of torque! Crushing hazard!
    • Watch when holding endmills–they are super sharp. Much sharper than drill bits.
  • Safety glasses!
  • Where is the E-Stop?

5 step checklist:

  • 5 step checklist, if you do everything correctly in the right order, will prevent you from crashing the machine
  • Perform full five step checklist each time you change your setup

Step 1: Simulate in the CAM software

  • CAM software is what we use to produce the g-code that the machines run off of
  • We won’t be going over the CAM today, but there is a CAM training! Checkout the libcal if you’re interested in working on these machines independently
  • What are we looking for in the CAM, according to the 5 step checklist? The datum point and where the first tool approaches the part
    • What is a datum point?
      • The point of reference for the machine on your part
      • Different on each part
      • Check in the CAM for where the datum point is in each axis, X, Y, and Z
    • Why do we check for where the tool approaches the part?
      • Good idea to have an idea of where that tool will approach so we can catch major issues before we begin to cut. If the tool is supposed to approach in the front right corner of the part but it approaches in the back left corner, you know you’ve done something wrong.
    • Simulate so you have some understanding of what the toolpaths are supposed to do

Step 2: Set your tools

  • Get the tools from the CAM software–beware of tool numbers!
    • Tool 1: ½” Flat End Mill (FEM)
    • Tool 3: 3/16” Flat End Mill (FEM)
  • Prototraks use the ‘master tool’ method–this is a reference tool that all of the tools use
  • We begin by going into Setup Mode
    • Go into Tool Table
    • Review how to put tools into the machine
      • Hold on the chuck, with your hand splayed so that if you drop it, you don’t smash your hand with the sharp part
      • Clean the collet taper and the inside of the machine taper with your hand real quick
      • Each collet has a keyway–find the key in the machine with the keyway, push up, and briefly but firmly hit the ‘in’ button
        • Don’t hold it for too long! If the tool starts to spin you are done
        • If you hold it too long the tool can get stuck and even eventually break the quil
    • Put the master tool into the quil
    • Review ‘jog’ mode
      • Slow down the feed rate to 50
      • Change to negative if you want to move down
      • Always watch the tool as it’s moving
      • EXIT JOGMODE as soon as you are done with jog mode!
      • Don’t ever jog all the way into something–always finish with the quil
    • Show setting reference tool to back of vise
    • Show on control (don’t have to demonstrate) that you have to put the diameter into the tools
    • Clear out tool table
    • STUDENTS DO: set reference tool and tools 1 and 3

Step 3: Set your X, Y, and Z work offsets

Set X and Y Work Offsets:

  • Go into DRO mode
  • Explain Fine vs Coarse motion
  • Explain X, Y, and Z axes
    • Like taking a piece of paper with coordinate geometry axes on it and laying it down flat, with Z coming out of the paper
  • Explain putting part into vise
    • What are parallels?
      • Parallel!
      • Precision ground–don’t mix and match from set to set
      • Today we need the highest parallels
    • Place part on parallels with cut side down, in the center of the vise
    • Ensure there is >1.32” sticking up out of vise at it’s shortest point
    • Tighten vise down with gold handle nice and tight
  • Students DO: Set up stock in vise
  • Edge-finding
    • What is edge finding? …finding edges
    • Edgefinders run at 1,200 RPM
    • Demonstrate setting spindle speed
    • Demonstrate edgefinding on the X axis
      • Start with edgefinder kicked out
      • Edgefind one side–demonstrate kickout!
      • Come up on Z
      • Set X to zero
      • Go over and edgefind other side
      • Come up
      • Divide x value by 2
      • Travel to that value
      • Set X to zero
    • Sabotage
  • Students DO: Set X and Y offsets

Set Z Work Offset:

  • What is the Z offset? The height difference between where you set your tools and your datum point
  • We set Z offset using one of the tools from our program
  • We may as well use tool 1! Change to tool 1
  • Change tool number in control to tool 1
  • Bring tool to top of part–aka the datum point– using quil and set Z to zero
  • Students DO: Set Z offset

Step 4: Simulate in control

  • We simulate in control to:
    • Make sure we’ve uploaded the right program
    • Make sure the entire program runs in the control–sometimes a control will dislike a particular line of gcode–it would suck to discover that halfway through running the part!
  • Go into ‘Program In/Out’ mode
  • Program we’re looking for is CNC Training Op1
  • Go into ‘Setup’ Mode
  • ‘Verify Part’
  • Adjust dimensions to match your actual stock to get an accurate picture
  • Hit ‘Make part’
  • ‘Verify Part’ again
  • Make sure:
    • Tool is coming down in the same spot as in the CAM software
    • Part looks the same as in CAM software

Step 5: Check Distance to Go

  • Remember when we said in the beginning that if you did each of these steps correctly and in the right order, you couldn’t crash the machine?
  • That’s this step!!
  • We are ready to run, with one caveat
  • Go into ‘Run’ mode
  • Hit go
    • Whenever there is green text, make sure to actively and deliberately read and respond to the green text
    • Confirm that we have the half inch tool in the spindle
    • Start spindle
    • Hit go
    • STOP before it reaches the part
      • Turn off spindle
      • Confirm that the tool is where the control thinks it is by comparing the Z value to the physical measurement between the tip of the tool and the datum point–in this case the top of the part
      • Use the special rules we have that have thousands of an inch one one side
    • Start coolant
      • Mist coolant
      • Use accessory button
      • Point mist flow at bottom of tool
      • Tighten mist down all the way so it’s just air
      • Release a little bit until you can see the tiniest bit of mist
    • Make sure quil is locked
    • Restart spindle (MENTOR NOTE: ALWAYS WATCH TO CONFIRM THAT THEY RESTART THE SPINDLE BEFORE HITTING GO! THEY FORGET. A LOT.)
    • Use remote button to press go and watch it cut!
    • Keep that remote button in your hand in case you want to pause it
    • If anything goes horribly wrong, bop the E-Stop

Second Op!

  • Watch simulation together
  • Explain how part goes into vise now
  • Still the highest parallels
  • Note where the datum point is! It’s at the bottom of the part!
  • They don’t have to reset tool table because all the tools are the same
  • STUDENTS DO: Set X and Y and reconvene when ready to set Z

Setting Z to bottom of part:

  • Set to top of parallels!
  • Be very careful–you SHOULD NOT move the table while the tool is down! It’s a good way to break your tool.
  • Check to see if you can reach the parallel; if not, bring the tool up, move your table, and try again.
  • Set Z to top of parallel

When you check the distance to go, you have to check the distance to the parallels!!

NOTE: If the bandsaw cut is horrible, have them stop the operation before the second tool cuts. They can run the setup for the last toolpath and just run it 5 times instead of 4.

Ops 3, 4, 5, & 6 :

  • Lower parallels, so that almost the whole cube is inside the vise
  • Use a bump stop so you only have to set X, Y, and Z once
  • You only have to check your distance to go once!
  • Datum point is center center top!

Related Articles

Responses

This site uses Akismet to reduce spam. Learn how your comment data is processed.