Machining on the HAAS in the RPL

This page contains stuff that used to be on the SDMTutorialNotes page about how to operate the HAAS.

-- AlanAsbeck - 23 May 2006

Updated helpful photos in "changing a tool" section.

-- SeungBum? - 18 July 2006

Contents:

General Comments:

Notes on dealing with wax blocks:

• Keep metal bottom of attacher mechanism clean—rest it on a paper towel when you put it down. Blow it off with air before attaching to HAAS.
• The pedal on the floor releases the locking mechanism. To place a wax block down, first position the metal holes over the pegs in the HAAS. Then push the foot pedal to open the locking mechanism, and lower the wax block the rest of the way down. Release the pedal.

Planing on the HAAS

How to plane a wax block: (make it smooth on top)

1. There are different instructions depending on if your block is above or below ~180mm. The different instructions for >180mm are marked "For tall blocks:" below.
2. Push “Offset”. Scroll up to where the G55 line is (the G55 coordinate system). DON’T CHANGE the x and y values ever. (If you ever change these numbers by accident, there is a program called "Numbers" on the HAAS that contains them). We will here change the Z coordinate to be the height of our wax block after it is planed. First figure out the height of your wax block, either by looking at what is written on the surface of it, or measuring it yourself with calipers. We will be planing off 2mm of wax at a time, so we should type in a height that is 2mm less than the current (original) height of our wax block. To type in the new desired number, highlight the Z entry and type in “-NN.” using the keypad, where NN is the height of your wax block. Be sure you have a period at the end! Push “F1” to change the value. So, suppose our wax block is height 64. We want to change the Z offset to “-62.”
   • Tall blocks: Change the offset to "0."
3. Push “List Prog” to select the planing program. Highlight Program #1002, “Wide Plane”. Push “Select Prog” to select it.
4. Push “Edit” to change program. The 7th line says “G01 Znn. F2000. ;” where nn = a number. Highlight the Znn entry. Change this to "Z0." by typing in "Z0." then pushing "Alter" to replace the entry in the program. (Again include the period after it!) If it is already Z0., then just leave it.
   • Tall blocks: Change the value to "Znn." where nn = desired height of block after planing. For example, if your block is currently height 190 and you want to plane it to remove 2mm, type in "Z188."
5. Push “Mem” to be able to run programs in general. Then, when you are in the Mem screen, we have to check a bunch of stuff before running the program. In particular:
   • SPIND = spindle speed. For planing we want to use a spindle speed of 60%. Push the +10% or -10% buttons until the screen reads 60%. In general, you can push “100% Spindle” to set the speed to 100% if anything is displayed on the screen. If it is 100% no notification will show on the screen.
   • FEED RATE = how fast it moves when it is actually cutting the part. Set this in accordance with your bit size. For planing things, set it to 100% for the initial passes and 60% for the final pass if you want a better surface finish.
   • RAPID = how fast it moves through the air between cuts. Set this to 5% for starters, then you can increase it to up to 25% or 50% later. (100% is way too fast).
   • Push “Single Block” to make “SINGBK” display on the screen. This means that it will only execute one line of code each time you push the green start button. Keep it in SINGBK mode to see what’s going on, until it has gotten a ways into the program, then you can push it again to turn it off. Try hitting the "single block" button a few times, it will toggle the mode on and off as indicated by "SINGBK" turning on and off on the screen.
   • Push “Reset” to highlight the first line of the program. This is IMPORTANT because it will start stepping through the program at whatever line is highlighted.
   • Make sure the AIR HOSES are where you want them to be. If it will switch a tool, make sure they are back and won’t run into the grey tool housing. Then after the tool switches, you should point them at the mill bit again, during one of the Single Block stops. If it is not switching a tool, make sure they are pointed at the tool tip.
   • Close doors of HAAS.
6. Finally, we can push the green “Cycle Start” start button to begin stepping through the code. Keep your hand over the “Feed hold” button to stop the machine at any time. Push the emergency stop button to stop everything immediately, including braking the spindle. The “Reset” button stops the tool and spindle, but more slowly. The “Feed hold” button stops the translation but the spindle continues. You can push this at any time to pause in the middle of a program, and then push the start button to resume where you left off.
7. You usually will have to do multiple planing passes on a wax block. To change the offset easily between passes, push "Ofset", then when the G55 Z entry is highlighted (as it should be), type in a positive number e.g. "2." and push "Write/Enter". This will add the number to the current value. We want to use a positive number because a less-negative Z offset corresponds to a lower block height. Again, be sure you have a period after the number or it will add e.g. 0.002 instead of 2.0. Plane off 2mm at a time at most.

Running a real program:

1. Go to the “Ofset” menu. Go to line G55, and change the Z entry to “-nn.”, where nn = the actual height of your planed wax block in mm. YOU MUST HAVE A NEGATIVE NUMBER HERE, and you must have a DECIMAL POINT! If you just enter -115, the Haas thinks you mean 0.115mm! Not good! The nn value you will have is the last height you used when planing your block as described above.
2. Transfer program from computer to HAAS:
   • Push “MDI DNC” twice to select DNC mode. It will say “waiting for DNC”.
   • Log on to the computer in there using name, password both = “biomim”. Use SecureFX or other method to transfer the .ptp files from chewie.
   • Open the “sdnc” program. Go to Communicate -> Download -> To HAAS. Choose your .ptp file.
   • Plug in the cable from the HAAS to the computer. It will stretch across the floor.
   • Push “Connect”, then “Transmit”. This will transfer the program into the HAAS memory. If the program is larger than the memory, it will transfer the rest as it finishes the early parts of the program. Leave everything on and plugged in so it can do this.
3. If you get an alarm on the HAAS when transferring the program (the lights will flash and it will say something on the screen), push “Alarm Mesgs” to see the alarm. Push “Reset” to clear the alarms. An alarm at this step usually indicates an RS232 error. In this case, quit the downloader program, then go to the Haas and hit RESET, then MDI DNC twice. Then try to send the program again.
4. Back on the HAAS, it will display the program on screen. DON’T PUSH RESET or it will clear the memory, and you’ll have to transfer it over again.
5. Once the program starts loading onto the Haas, you're ready to start machining. Before starting, always check the following:
   • Make sure "SINGLE BLOCK" mode is on. Leave it on until the mill has started cutting into the wax, then you can turn it off.
   • Move the AIR HOSES if there will be a tool change. Be sure to move them back after the tool change!
   • Set the RAPID speed to 5%
   • Set the SPINDLE SPEED to either 100%, or up to ~130% for 1/32" or smaller bits.
   • The FEED RATE should be the correct value for the mill bit you are using (or less to start with): 1/4” = 200%; 1/8" = 100%; 1/16” = 40%; 1/32” = 20%. You can always make the feed rate less than this if you want.

1. Step through the program by hitting the Start button to run each line. Keep your hand over the Feed Stop button, ready to hit it if anything looks funny. In one of the early lines in the program, it will say “Z10”. Make sure at this point that the tip of the cutter is actually 1cm above the wax block. Any errors you will likely get will all be Z-offset errors. This is a very important step to make sure you do not have an offset error.
2. Once you're sure everything's ok, you can turn off Single Block mode and let it run. Can change Rapid speed to 25% or 50%.
3. As you are stepping through the program, you can push “Curnt Comds” to see a different view of the program. The up/down arrows give you different coordinate systems on the bottom. The “Work” system is best, because the z-coordinate is the height above the wax block surface, which is useful for debugging. (+) = above block, (-) = into block.
4. If you want to check the status of the part later, you can do the following:
   1. push feed hold.
   2. push “Coolant” which will stop the air.
   3. push “Stop”, which is next to the “CW”, “CCW”, and “Spindle” buttons.
      This will stop everything so you can open the door and check on things. To restart the program, do the following in this order:
   4. push “Coolnt” to restart the air flow.
   5. Push “CW” to start the spindle.
   6. push the green start button to resume the program.

Summary of what to do on HAAS:

Planing: Regular-height blocks:

1. Push OFSET: On G55 line, set to "-NN.", push "F1" to change.
2. Push "List Prog", Highlight Program #1002, “Wide Plane”. Push “Select Prog” to select it.
3. Push “Edit”. The 7th line says “G01 Znn. F2000. ;” Highlight the Znn entry. Type in "Z0." , push "Alter"
4. Push “Mem”. Check the following:
   • SPIND = spindle speed: Set to 100%.
   • FEED RATE: set it to 100% for the initial passes and 60% for the final pass if you want a better surface finish.
   • RAPID: Set to 5% for starters, then you can increase it to 25% or 50% later.
   • “SINGBK” should be displayed on the screen. Turn it off once you're into the program.
   • Push “Reset” to highlight the first line of the program.
   • Make sure the AIR HOSES are where you want them to be. If it will switch a tool, make sure they are back. Then after the tool switches, you should point them at the mill bit again, during one of the Single Block stops.
   • Close doors of HAAS.

Planing: Tall blocks:

1. Push OFSET: On G55 line, set to "0.", push "F1" to change.
2. Push "List Prog", Highlight Program #1002, “Wide Plane”. Push “Select Prog” to select it.
3. Push “Edit”. The 7th line says “G01 Znn. F2000. ;” Highlight the Znn entry. Type in "ZNN.", e.g. "Z182." , push "Alter"
4. Push “Mem”. Check the following:
   • SPIND = spindle speed: Set to 100%.
   • FEED RATE: set it to 100% for the initial passes and 60% for the final pass if you want a better surface finish.
   • RAPID: Set to 5% for starters, then you can increase it to 25% or 50% later.
   • “SINGBK” should be displayed on the screen. Turn it off once you're into the program.
   • Push “Reset” to highlight the first line of the program.
   • Make sure the AIR HOSES are where you want them to be. If it will switch a tool, make sure they are back. Then after the tool switches, you should point them at the mill bit again, during one of the Single Block stops.
   • Close doors of HAAS.

Running a real program:

1. “Ofset” : Line G55, change the Z entry to “-nn.”, "F1" to change. MUST BE NEGATIVE, must have a DECIMAL POINT!
2. Transfer program from computer to HAAS:
   • Push “MDI DNC” twice to select DNC mode: “waiting for DNC”.
   • SecureFX to transfer .ptp files from chewie.
   • “sdnc” program: Communicate -> Download -> To HAAS. Choose your .ptp file.
   • Push “Connect”, then “Transmit”.
     
3. Back on the HAAS, check the following:
   • DON’T PUSH RESET or it will clear the memory
   • "SINGLE BLOCK" mode should be on.
   • Check the AIR HOSES
     • Be sure to move them back if there is a tool change!
   • RAPID speed to 5%, can increase to 50% later
   • SPINDLE SPEED to 100% for most bits, or up to ~120% for 1/32" or smaller bits.
   • FEED RATE: Start at 10% then increase once program starts: 1/4” = 200%; 1/8" = 100%; 1/16” = 40%; 1/32” = 20%.
     
4. When it says “Z10”., make sure it's 1cm above the wax block.
5. Once program is going, turn off Single Block mode, change Rapid speed to 25% or 50%.
6. Can push “Curnt Comds”, then up/down arrows to get to “Work” system. There the z-coordinate is the height above the wax block surface.
   
7. Pausing the HAAS:
   1. Wait until mill bit is in air.
   2. Push "Feed hold".
   3. Push “Coolant” which will stop the air.
   4. Push “Stop”, which is next to the “CW”, “CCW”, and “Spindle” buttons.
      To restart the program:
   5. Push “Coolnt” to restart the air flow.
   6. Push “CW” to start the spindle.
   7. Push green Start button.

Cleaning up the HAAS

After using the Haas, you must do a quick clean-up. Use the compressed air to spray the chips off the mounting block, the slide covers, the tool changer, the inside of the doors, and the back and side walls. Basically we want to keep all surfaces fairly clean (except for the bottom where all the chips are). Every few weeks the chips must be emptied out from the Haas. This can be done by sliding open the side panels and scooping the chips out into a garbage bag.

Changing a tool on the HAAS

Removing a broken tool

• Switch to the tool you want to use. Do this either by running the first part of a program that switches to that tool, or execute the following in MDI mode: "T# M06" where # is the tool number, for example "T5 M06". If you are in MDI mode, BE SURE YOU'RE IN SINGBK MODE!!!
• Put the HAAS in Handle Jog Mode.

Hit the "Tool Release" button inside the HAAS next to the spindle (on the front bottom right of the spindle housing, see picture at right). This will release the tool chuck--be sure you are holding onto it when you do this!!
Put the chuck into the big metal hexagonal tube-like thing that Tom has on his desk (see picture at right). It is hexagonal on the outside, cylindrical on the inside, and has two bumps sticking up. The tool chuck will fit nicely into it.
Use a 1" wrench to loosen (unscrew) the chuck holding in the mill bit (wrench is shown in picture at right). You may have to hold the hexagonal metal thing on its side in order to get good leverage. Take out the old or broken mill bit.

Installing a new tool

• With the chuck still in the hexagonal metal thing, put in a new mill bit.
• Tighten the chuck--but you don't need to overtighten it! Also, be very careful when moving the wrench around the newly-installed bit, don't smack the wrench into it and break it by accident.
• Remove the chuck from the hexagonal metal thing.
• Clean off the conical part of the chuck with a paper towel, and clean off the inside of the conical tube inside the HAAS that the chuck fits into.
• On the HAAS, push "MDI/DNC", then "Orient Spindle" which is in the same row as "MDI/DNC". This will align the spindle appropriately.
• On the chuck, you will notice that there is a lip with two cut-out sections on it. One of these cut-out sections has a little square with rounded corners indented into it while the other one does not. The side with the indented-rounded-square should be on the left side as you are facing the HAAS--it should be towards the tool changer rack in the HAAS.
• With the chuck oriented as such, put the chuck into the socket for it on the HAAS and push the "Tool Release" button. This will suck the chuck into the spindle and keep it there.

Setting the height of a tool

This must be done after you change a tool, or can also be done for an existing tool if you want to re-set the height (length) of it.

• Clean off the metal surfaces that are on the palette-aligner thing. Make sure they're really clean, or this will make the tool height wrong.

Take the RED metal palette on the shelves where we store the blocks (see picture at right). It has a cylinder on top of it (leave the cylinder on top). Clean the circles on the bottom where it mounts into the HAAS.

• Put in the HAAS with the cylinder on the right-hand side, with the "0 degree" marking in front towards you.
• Clean the end of the newly-installed mill bit if it is dirty, and dust off the top of the cylinder on the red palette.
• On the HAAS, push "Ofset", then go to the G55 line. Set the Z-Offset to 0 by highlighting the Z value, typing "0." on the number pad, and pressing "F1".
• Push "MDI/DNC" to go into MDI mode.
• PUSH "SINGBK" to put it in Single Block mode!!!!!
• Execute the following lines in MDI mode. Usually they are already typed in, so to execute them you just scroll down to them using the wheel and push the green Start button once for each line (since you're in SINGBK mode). If you need to edit one of the lines, it's like editing a program, highlight an entry and type in the new text and push "Alter". I don't know how to add a new line or new entry. Anyway, here are the lines you should execute:

G55 ;
G91 G28 Z0. ;
G90 ;

• Push "POSIT". This displays the Coordinate systems. Check to make sure both the Machine, Work coordinate systems have Z values of 0. If they aren't 0, you did something wrong (I don't know what, I've never seen other values)
• Push "Handle Jog" on the HAAS. We are going to lower the mill bit so it touches the top of the cylinder. Use handle jog mode (adjusting X,Y,Z) to lower the tool so it is directly over the cylinder on the red palette, just a little bit above the surface. Position it above a spot on the cylinder that is flat and does not have "divots" from other tools running into the cylinder in the past. Put the handle jog on the smallest step size (0.001) and very slowly and gently lower the mill bit until it touches the top of the cylinder. Usually using the scroll wheel on the HAAS is the easiest way to lower down the mill bit. When it does touch the top of the cylinder, a red LED will come on on the side of the cylinder.
• When the red LED comes on, move the mill bit up and down one click (0.001) to verify that when you raise up the mill bit, the light turns off, and when you move it back down again the light turns on. If the mill bit or the cylinder are dusty, it will behave abnormally (i.e. the light won't turn on and off appropriately) and you will have to clean them off and try again.
• Leave the mill bit one click (0.001) above where the red light comes on.
• Push "OFSET".
• Using the 'Page Up','Page Down', and Arrows, NOT THE DIAL scroll to the Tool #s page. It lists all the tools and their offsets. Highlight the number under the "Geometry" column (the Z values) using the arrow keys for the tool currently in the spindle. (The tool number for this tool will be highlighted in the far left column).
• Push "Tool Ofset Measur" which is under the "F1" button to measure the Z number.
• With this newly-measured Z value highlighted, type in "-72.657" on the keypad and push "Write/Enter" to add this value to the newly-measured Z value. This "-72.657" value is the distance from the bottom of the palette mounting system to the bottom of a wax block, I think. If you ever forget this number, it can be found in program #0001, "Numbers" (i.e. push "List Prog" and scroll to #0001 and edit it).
• Push Handle Jog again, and move the bit up and off the cylinder by pushing the Z up arrow.

That's it!

Codes for HAAS

If you need to understand what the HAAS is doing when it executes those various Gnn Mnn commands at the beginning and ends of the program, look at the table below:

• MillGandMCard.pdf: Codes for running the HAAS, acquired from http://www.haascnc.com/

RS232 Setting for HAAS

The HAAS communicates with the HAAS using a simple RS232 connection. The pinout for the DB25 connector is available on the HAAS manual, which can be accessed by pressing "Help Calc" on the HAAS.

Data bits: 7
Parity: Even
Protocol: ASCII (as opposed to Xmodem)
Line speed: 38400
Stop bits: 1
Handshaking: Xon/Xoff (No hardware handshaking)
Block Delay: 0 msec
EOB: CR+LF
Char Code: ASCII (as opposed to EIA)
-- SalomonTrujillo - 30 Jul 2007

-- AlanAsbeck - 23 May 2006