Lesson 6 The Key Operation Procedures

Lesson 6 The Key Operation Procedures Step-by-step procedures can keep you from having to memorize every function that you must perform on your CNC machining center. You will soon memorize procedures for task that you perform on a regular basis but written procedures will always help you perform lesser used tasks. While you have been introduced to the various buttons and switches on a typical machining center, it is unlikely that you have memorized them all. It is also unlikely that you know the appropriate order by which you should press buttons and activate switches to do anything on the machine. For example, think of what it takes to perform one of the most basic tasks a setup person or operator must do to power up the machine. Just because you know the related buttons and switches, does not mean you know the step-by-step procedure needed to turn on a CNC machining center. The procedure for a given machining center might look something like:? Step 1: Turn on the main breaker (in back of the machine).? Step 2: Press the power on button on the control panel.? Step 3: Press the hydraulic system on button on the machine panel.? Step 4: Follow the procedure to do a manual zero return. With such a procedure, turning on the machine is not a t all difficult. While you should still know the function of the related buttons and switches, this procedure provides you with sequential order (steps) you need. And similar procedures for other important tasks will be just as easy to follow (if you have them). Admittedly, the most often used procedures will be soon memorized and because most experienced setup people and operators have them memorized, they haven t written them down. And unfortunately, most companies don t have a written set of procedures for their CNC machines. Though this may be the case, nothing stops you from developing a written set of procedures for yourself. While you ll need the help of an experienced person, you can easily develop a set of procedures that will help you (and others) remember the steps necessary to do just about anything on the machine. We divide the procedures needed to run a CNC machining center into five categories: Manual procedures Setup procedures Manual data input (MDI) procedures Program editing procedures Program operation procedures Here are specific procedures that we recommend you write down in each category: Manual procedures: To power up the machine To do a manual zero return To manually start the spindle To manually jog the axes To use the handwheel To manually load and remove cutting tools in the spindle Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page1

Setup procedures: To load tools into the automatic tool changer magazine To set or reset the relative position display To enter and modify tool offsets To enter and modify fixture offsets To measure program zero assignment values To measure tool length compensation values MDI procedures: To use MDI to change tools To use MDI to start the spindle To use MDI to do a zero return Program editing procedures: To enter a program through the keyboard To load a program from a DNC system To save a program to a DNC system To see a directory of programs To delete a program To call up a program (make it the active program) To search within a program To alter a word in a program To delete a word in a program To insert a word in a program Program operation procedures: To run a verified program To cancel the cycle To verify programs To re-run tools The goal with any step-by-step procedure is to keep you from having to memorize anything. But you must, of course, understand when and why to perform each procedure. We ll be addressing the logic for using these procedures throughout this text. Again, whenever you come across a task for which we have not supplied a step-by-step procedure, get someone to help you. As they demonstrate what it takes to perform the tasks, write down in step-by-step fashion what they do. The next time you must perform the procedure, you ll have the needed step-by-step instructions for doing so and you won t have to ask again. Figure 6.1 shows a form you can use to create your own procedures. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page2

Procedure name: Machine: Description: Procedure: Notes: 1) 2) 3) 4) 5) 6) 7) 8) 9) 10) 11) 12) 13) 14) 15) 16) Figure 6.1 Procedure form The next two pages provide you with a quick reference for one popular Fanuc control model. But if you have other Fanuc controls, or if you have machining centers with controls that are not made by Fanuc, make your own quick reference sheet or operation handbook. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page3

To power-up the machine: The Key Operation Procedures Fanuc 16M and 18M Quick Reference For Key Procedures Required before doing anything else on the machine. 1. Turn on main breaker (Usually located at rear of machine). 2. Press control power on button. 3. Press machine ready or hydraulic on button. (not necessary on some machines.) Be sure that emergency stop button is not locked in. 4. Follow sequence to do a manual zero return. (All Fanuc controls require that you do a manual zero return as part of the power-up procedure.) To manually jog the axes: Required when taking measurements on the machine, when performing manual machining operations, and in general, whenever you must move an axis. 2. Place axis selector switch to desired axis (X, Y, or Z). 3. Place the jog feedrate switch to the desired motion rate. 4. Using the plus or minus buttons or joystick, move the axis in the desired direction and amount. Jogging the machine does not provide precise positioning. Use the handwheel when more precise positioning is needed. To load tools into the ATC magazine Required during setup and when tools must be replaced during a production run. 2. Go to the tool changer and rotate it to the desired position. 3. Load the tool into the desired position by unclamping a lever or simply snapping it into position. 4. Continue rotating magazine and loading tools for all tools to load. Machines vary when it comes to how the ATC magazine is loaded. If you have problems, consult your machine tool builder s operation manual. To enter and modify fixture offsets Required during setup to enter program zero assignment values. 1. The mode switch can be in any position. 2. Press the key labeled offset/setting. 3. Press the soft key under fixture offset (if needed). 4. Using the cursor control up and down arrow keys, position the cursor to the fixture offset register to enter. 5. Type the value of the offset and press input. 6. Repeat steps four and five for all axes. To do a manual zero return: Required right after power up. The zero return position in at least one axis is also the tool change position for most machines. The machine must be at this position prior to running a program. 1. Place mode switch to zero return. 2. Using the axis select switch select the X axis. 3. Using the minus direction push button or joystick, move the machine about two to three inches in the minus direction. 4. Using the plus direction push button or joystick, hold plus until zero return origin indicator light comes on. 5. Repeat steps 2-4 for all other axes. To use the handwheel Required when precise axis motion is needed - as when measuring program zero assignment values and tool length compensation values. 1. Place mode switch to handwheel. 2. Place axis select switch to desired position (X, Y, Z, or B/C). 3. Place handwheel rate switch to desired position (X1, X10, or X100). 4. Using handwheel rotate plus or minus to cause desired motion. Use the relative position display when taking measurements. To set or reset the relative position display Required when taking measurements on the machine. To reset (set to zero) 1. Mode switch can be in any position. 2. Pr ess the key labeled position until the relative display screen is shown. 3. Type the letter address of the axis you wish to reset (X, Y, or Z). That letter will start flashing on the axis display. 4. Press the soft key under origin. To set to a specific value 1. Mode switch can be in any position. 2. Press the key labeled position until the relative display screen is shown. 3. Type the letter address for the axis you wish to set and type its value. 4. Press the soft key under preset. To manually start the spindle: Required whenever you use a conventional edge-finder to measure program zero assignment values or when you will be performing manual milling operations. 2. Select the desired direction (forward or reverse) with the appropriate switch. 3. If available, select the desired speed in rpm with the appropriate switch. 4. Press the spindle on button. 5. To stop spindle, press the spindle stop button. Not all machines have manual controls for the spindle. This procedure will only work for those that do. You can also use the MDI procedure to start the spindle. Some machines allow you to manually start and stop the spindle, but not select speed or direction. To manually load and remove tools in the spindle Required when you want to inspect the cutting tool. 2) If the machine has an air-blow switch, be sure it is turned off. 3. If there is already a tool in the spindle, hold the tool with one hand and press the unclamp button with the other. The tool will drop out of the spindle so be ready. 4. To load a tool into the spindle, place the tool into the spindle with one hand and press the clamp button with the other. With most machining centers, a tool holder will only fit into the spindle in one orientation. To enter and modify tool offsets Required during setup to enter initial offset values and when trial machining. Required during a production run when sizing is needed. 1. The mode sw itch can be in any position. 2. Press the key labeled offset/setting. 3. Press the soft key under wear (if needed). 4. Using the cursor control up and down arrow keys, position the cursor to the offset number to enter. 5. Type the value of the offset and press input. You can overwrite the current offset setting by pressing the soft key under input or you can modify its current value by your entry by pressing the soft key under input + Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page4

Fanuc 16M and 18M Quick Reference For Key Procedures To use MDI to change tools Required whenever a manual tool change is needed as when measuring tool length compensation values on the machine. 1. Place the mode switch to MDI. MDI appears at the top of the display screen. 3. Type T and the number of the tool you wish to load into the spindle. 4. Press the EOB key and press the soft key under insert. 5. Press the start key or cycle start button (Tool rotates into waiting position.) 6. Type M06, the EOB key, and press the soft key under insert. 7. Press the start key or cycle start button (Tool change takes place). To enter a program using the keyboard A program must reside in the machine s memory before it can be run. This is one way to load a program but it is time consuming. 1. Place the mode switch to edit. 3. Type the letter O and the program number of the program to be entered. 4. Press the soft key under insert. 5. Press the EOB key and press the soft key under insert. 6. Typing one command at a time and ending each command with the EOB key, enter the balance of the program. To see a directory of programs Required when you want to know which programs are in the machine. 1. Place the mode switch to edit. 3. Press the soft key under program again. To search within a program Required when you must edit a program. 2. Press the extreme left soft key until program appears at the bottom of the screen then press the soft key under program. 3. Press the reset key to return the program to the beginning (not always required). 4. Type the word you wish to search to. 5. Press soft key under fwd search. The control will find the first occurrence of the word you typed. Other important procedures: To measure program zero assignment values To measure tool length compensation values To verify programs To re-run tools To use MDI to activate the spindle Required whenever a manual tool change is needed as when measuring tool length compensation values on the machine. 1. Place the mode switch to MDI. MDI appears at the top of the display screen. (example: S500 = 500 rpm) 3. Press the EOB key and press the soft key under insert. 4. Type M03 for forward or M04 for reverse, press the EOB key, and press the soft key under insert. 5. Press start key or cycle start button. (spindle starts) 6. To stop spindle, type M05, the EOB key, and press the soft key under insert. Then press start key or cycle start. To load a program from a DNC system Required during setup to load the program/s needed for the job. 1. Place the mode switch to edit. 3. Be sure the DNC system is connected the machine. 4. Type O (letter, not zero) and the program number to be loaded. 5. Press the soft key under read. 6. Go to the DNC system and send the program. To delete a program Required when you re finished using a program. 3. Type letter O and the program number to be deleted. 4. Press the soft key under delete. To alter a word in a program 3. Search to the word to be altered. 4. Type the new word. 5. Press soft key under alter. To insert a word in a program 3. Search to the word just prior to the word you want to insert. 4. Type the word you wish to insert. 5. Press soft key under insert. To use MDI to do a zero return The zero return position in at least one axis is usually the tool change position. The machine must be at this position when the program is activated. This procedure is faster than the manual procedure. 1. Place the mode switch to MDI. MDI appears at the top of the display screen. 3. Check that the machine can go straight home with no interference. 4. Type G91 G28 X0 Y0 Z0, press the EOB key and then press the soft key under insert. 5. Press start key or cycle start button. You can omit axes that you don t want to zero return. To save a program to a DNC system Required after program verification if changes have been made to the program. 1. Get the DNC system ready to receive a program. 2. Place mode switch to edit. 3. Press the key labeled program until 4. Type the letter O and the program number of the program to be sent. 5. Press the soft key under punch. To call up a program (make it the active program) Required when you want to work on another program in the control. 3. Type the letter O and the program to be searched to. 4. Press the soft key under fwd search. To delete a word in a program Required when you must edit a program. 3. Search to the word to be deleted. 4. Press the soft key under delete. To run a verified program Required during a production run. 1. Load part into setup. 2. Send the machine to its starting point (usually the tool change position). 3. Place the mode switch to edit. 4. Press the key labeled program until 5. Press the reset key (check the active program number). 6. Check position of all conditional switches (dry run, etc.). 7. Place the mode switch to memory or auto. 8. Place the feedrate override switch to 100 per cent. 9. Press cycle start button. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page5

Key points for Lesson Six: The Key Operation Procedures Running a CNC machining center requires little more than following a series of procedures. The trick is knowing when and why to perform a given procedure. Writing down procedures will keep you from having to ask someone for help every time you need to perform the procedure. Write down a procedure for every task you must perform on your machining center. Copyright 2011, CNC Concepts, Inc. Machining Center Setup and Operation Page6