Читать книгу Programming of CNC Machines - Ken Evans - Страница 11
ОглавлениеFigure 1 Common Operators Panel
1. To become familiar with common CNC Machine Operation Panel functions.
2. To become familiar with common Machine Control Panel functions.
3. To learn common operations performed at the Machine Control.
4. Learn how to use the Controls to input setup data including Tool and Work Offsets.
5. Learn how to use the Control to edit programs.
6. Examine some common cases of problem situations and learn how to solve them.
Every CNC Machine Tool has an Operation Panel and a Control Panel that are the interface between the Operator and or Programmer and the Machine Tool, sometimes referred to as the Human Interface (HMI). The Operator Panel is the method with which we physically manipulate the working components of the machine to do what we need and the Control Panel is where the program data are entered and stored. A thorough understanding of each is necessary for successful CNC Machine use. First, we will study and example of an Operation Panel.
Figure 2 Operation Panel Courtesy GE FANUC
The following descriptions for the above diagram represent the configuration for a common Operators Panel. Some differences do exist for each manufacturer Operation Panel, but they generally contain the same features. The illustration shows a panel for a two-axis lathe. The panel used for a mill would be essentially identical, except for the added keys for the additional axes. The user should consult the applicable manufacturer manual for detailed descriptions that match their needs. Please also note that the Handle (Pulse Generator) and the Rapid Traverse Override buttons are not shown in this view of the controller, although it is described in the text. Another common item not shown here are the switches used to change the chucking direction from external to internal and are specifically for lathes.
OPERATOR PANEL FEATURES FEEDRATE OVERRIDE
The Feedrate override dial allows control of the feedrate when the operator adjusts the position. At the 12:00 o’clock position the feed, during auto-cycle, will occur at 100% of the programmed value. This allows the control of the work feeds defined by the F-word in the program. The percentage of the value entered in the program can be increased or decreased. This feature offers the operator the control needed to fine tune feeds. It can also be used to control feedrates while using the manual jog mode function.
Figure 3 Feed Override
EMERGENCY STOP
The EMERGENCY STOP is the large, red, mushroom-shaped button used to stop machine function when an emergency situation occurs. Some example situations are: overloading of the machine, a clamping of the machined part has come loose, or incorrect data in the program or work or tool offsets have caused a collision (crash) between the tool and the workpiece. When this button is pressed, all program commanded feedrates and spindle revolutions are halted immediately. Recovery from an “E-Stop” condition requires resetting the program controller and Homing of the machine axes. To reset the EMERGENCY STOP button, turn it clockwise. It should “pop-out” of the depressed condition. Check the monitor for any alarm signals and take note of the Alarm # and description, and then eliminate the cause that forced the use of the EMERGENCY STOP button. Press the Reset button to clear all pending commands and Home the machine axes when no interference conditions are present.
Figure 4 Emergency Stop
PROGRAM PROTECT
When this key-switch is in the ON condition (vertical), it prohibits any program changes to be made. The condition does not affect work or tool offset adjustments. Some shops set this condition to ON, remove this key and allow only the programmer or set-up person access to the key. This is especially true in larger shops with multiple shifts and many workers. Some Quality programs like ISO9000 require that CNC program integrity is insured.
Figure 5 Program Protect Keyswithch
PROGRAM SOURCE
On some operator panels, a rotary switch referred to as Mode Select is used instead of buttons that are shown here. This switch includes both automatic (AUTO) and manual operation functions. The position of this switch determines whether the machine utilizes the automatic or the manual control. This switch can also be positioned to allow the entry of data into the control manually (Manual Data Input or MDI) or to make changes to the program through the EDIT mode. For this purpose, operator panel buttons are used to specify the control or operational mode.
Figure 6 Program Source
Note: When the buttons are pressed, they are active and remain so until another mode button is pressed. In some conditions, multiple Light Emitting Diodes (LED’s) may be lit simultaneously. The LED in the upper left corner of the button is lit when the mode is ON and active.
Auto
By pressing this button, the control mode enables the CNC commands stored in the memory to be executed for automatic operation. When the Cycle Start button is pressed, and this mode is active, automatic operation will occur.
Edit
By pressing this button, the program edit mode is selected. The EDIT mode enables the user to enter the part program to control memory, enter any changes to the program and transfer data from the program via RS232 interface to an offline storage device or check the program file memory and storage capacity.
Note: The RS232 interface is a 25-pin serial cable connector (in Figure 7) is located behind the flip-up door just below the Program Protect key switch. This connection is also used for DNC (Direct Numerical Control) program operations when the program is too large for the controller memory and is executed directly from a remote Personal Computer (PC).
Figure 7 RS232 Communications Interface Port
MDI-Manual Data Input
By pressing this button, the MANUAL DATA INPUT mode is selected. The MDI mode enables the automatic control of the machine, using information entered in the form of program blocks without interfering with the basic part program. This mode is often used during the machining of workpiece holding equipment such as soft-jaws and during setup. It corresponds to single moves (milling surfaces, drilling holes), descriptions of which need not be entered to memory storage. MDI mode can also be used during the execution of the program. For example, suppose the program is missing the command M03 S350; needed to turn on the spindle, clockwise, at 350 r/min and the End-Of-Block character (;). In order to correct this omission, press the SINGLE BLOCK button and then the MDI button. Using MDI, the user can enter functions M03 and S350 from the control panel keypad followed by the EOB character. Then, enter this command by pressing INPUT on the control panel. Press AUTO to reenter the program auto-cycle mode and then press CYCLE START to continue execution of the program from memory.
OPERATION SELECT
The following buttons are related to the automatic operation of the machine. Activating one of these buttons has an effect on the operation and is described on the next page:
Single Block
The execution of a SINGLE BLOCK (SINGL BLOCK) of information is initiated by pressing this button to turn it ON. Each time the CYCLE START button is pressed, only one block of information will be executed. This switch can also be used if you intend to check the initial performance of a new program on the machine or when the momentary interruption of a machine’s work is necessary.
Figure 8 Operation Selection Buttons
Block Delete
BLOCK DELETE (BLOCK DELET) is sometimes called Block Skip. When this button is pressed and is active simultaneously with the auto-cycle mode, the controller skips execution of the program blocks that are preceded by the slash (/) symbol and that end with the end of block (;) character. For instance, if a section of the part program or a particular block of the program is not presently needed, but you would like to keep this information for future use, then place the block skip symbol (/) at the beginning of each such block. The BLOCK DELET button is located on the control panel. If it is activated, then information contained in the blocks that are preceded by the symbol (/) will not be executed.
Example:
N100G01X2.810Y3.256
/N105X3.253Y2.864
/N110X3.800
(Blocks N105 and N110 will be skipped)
Notes: The symbol (/) should be placed at the beginning of the block. If it is not, then all the information contained in the block preceding the symbol (/) will be executed, while the information following this symbol will be omitted.
If the BLOCK DELET is in the OFF condition, all blocks, regardless of the symbol (/), will be executed.
When transferring the program to punched tape or external computer, all program information, regardless of symbol (/), is transferred.
Opt Stop-Optional Stop
When this button is pressed, the OPTIONAL STOP mode is active. The OPTIONAL STOP function interrupts the automatic cycle of the machine if the program word M01 appears in the program. Quite often, function M01 is placed in the program after the work of a particular tool is completed or before a tool change. This enables the operator to perform routine measurements directly on the machine and, if necessary, make adjustments and then rerun the same tool to correct inaccuracies.
Dry Run
By pressing the DRY RUN button during automatic cycle, all of the rapid and work feeds are changed to the rapid traverse feed set in the parameters instead of the programmed feed. Consult the manufacturer manual for specific directions on the use of this function.
DRY RUN is also used to check a new program on the machine without any work actually being performed by the tool. This is particularly useful on programs with long cycle times so the operator can progress through the program more quickly.
Caution: When using this function, it is NOT intended for metal cutting.
Prg Test-Program Test
This function is also known as MACHINE LOCK. Activating this mode inhibits axis movement on all of the axes. This button is used to check a new program on the machine through the controller. All movements of the tool are locked, while a program check is run on the computer and displayed on the screen. The operator can observe the position display on the screen and if any program errors are encountered, an alarm will be displayed. This function is especially useful for checking very large programs requiring a long cycle time to complete. This test is normally the first in a series (Program Test, Dry Run and Single Block) of preliminary actions to be executed before full auto cycle mode is attempted. For any program test, all offsets should be set first.
Axis Inhbt-Axis Inhibit
This function is identical to MACHINE LOCK for all axes. Activating this mode inhibits axis movement on all of the axes. A common situation would be to inhibit the axes to allow for internal checking of the program. Some controllers have additional buttons or switches that enable inhibiting of only one axis at a time. This function is especially useful when inhibiting the Z axis so that all X, Y movements can still be observed.
Figure 9 Execution Buttons
EXECUTION
These three buttons are related to automatic operation of the machine. The first button starts, the second temporarily stops automatic operation and the last key merely indicates when a program stop is encountered. Their specific functions are described below:
Cycle Start
The CYCLE START button is used to start automatic operation. Use this button in order to begin the execution of a program from memory. When the CYCLE START button is pressed, the LED located above this button goes on and the active program will be executed to the end.
Cycle Stop (Feed Hold)
Pressing the CYCLE STOP button during automatic operation will halt all feed movements of the machine. It will not stop the spindle r/min or affect the execution of tool changes on some machines. When the CYCLE STOP button is pressed, the LED located on the button goes on, and the LED located on the CYCLE START button goes off. When the CYCLE STOP button is pressed, all feeds are temporarily stopped; however, the spindle rotation is not affected. This button is used when minor problems are encountered, such as coolant flow direction or when checking DISTANCE-TO-GO during setup. When the problem is remedied, press CYCLE START again to resume automatic cycle operation. It is not recommended using this button to interrupt a cut because the spindle does not stop and damage to the tool or part may occur. When pressed during the execution of the tapping or threading cycle, CYCLE STOP will take effect after the thread pass or the tap is withdrawn. If the tap breaks during the tapping cycle, the only way to stop the machine is by pressing the RESET button on the controller or the EMERGENCY STOP button.
Prg Stop-Program Stop
When a Program Stop is commanded in the program by the program word M00, automatic operation is stopped and the LED on this button is turned on. This button does not have an ON/OFF function that affects the program stop condition. It is merely an LED indicator lamp to indicate when a program stop condition is active.
Figure 10 Operation Buttons
OPERATION
The keys in the Operation section of the control are used for manual operation of the machine during setup and initial startup. Their specific functions are described below:
Home
Pressing this button on and then pressing the X or Z (X, Y or Z for Machining Centers), buttons causes the machine to return to the Machine Zero position for each axis in relation to the machine coordinate system.
Jog
Pressing the JOG button activates a manual feed mode that allows the selection of manual feed movements along single axes X or Z (X, Y, or Z for machining centers). With the button activated, use the Axis/Direction buttons and the Speed/Multiply buttons to move the desired axis at the chosen feed rate (in/min). On some controls Speed/Multiply is a rotary type switch that activates this function.
INC Jog
Press this button (Incremental JOG) to activate the JOG mode in Incremental steps at feed as per selection using the Speed/Multiply buttons.
MPG-Manual Pulse Generator
Pressing this button activates the manual handle feed mode for the selected axis. This handle is known as the Manual Pulse Generator. Pressing the MPG button places the machine in the HANDLE mode. This mode enables manual control of axis movements (for X, Y or Z, or for rotational axes A, B or C) by use of the handle after activating their respective axis buttons. For instance, press MPG then press X and then use the handle to move to the desired position along the X axis. By turning the handle clockwise, you can move the tool in a positive direction with respect to the position of the coordinate system. By turning the handle counterclockwise, the tool is moved in a negative direction with respect to the position of the coordinate system. The handle contains 100 notches, each of which corresponds to an increment (distance to be moved). Turning the handle, you can feel the displacement from one notch to the next.
Figure 11 Manual Pulse Generator (MPG) Handle
To set the magnitude for the distance to be moved, press one of the Speed/Multiply buttons as described in more detail below.
Caution: If the handle is rotated quickly while the magnitude is set at X100 or X1K the tool will move at a rapid feed rate and a crash could occur!
Teach
This button activates the Teach-in Jog or Teach-in Handle mode. When this mode is used, the movements of the axes are recorded while in either Jog or Handle mode. Machine positions along the X, Y, and Z axes obtained by this manual operation are stored in memory as a program position and are used to create a program. These movements can then be executed just as with any program. Consult the manufacturer operator’s manual for detailed descriptions on its proper use. Not all controls have this feature.
Offset Mesur-Offset Measurment
When this button is pressed, the OFFSET MEASURE mode is selected and the position of the tool in relation to the coordinate system is written into the tool or work offset for the active axis.
SPEED/MULTIPLY
When INC JOG is selected from the Operation Mode buttons, the incremental step selected by the Speed/Multiply buttons determines the magnitude of the displacement along the chosen axis in the selected direction. When one of these buttons is pressed and released, the movement will be as follows:
X1 = a movement of .0001 inch or .0025 millimeters (mm)
X10 = a movement of .001 inch or .0254 mm
X100 = a movement of .010 inch or .254 mm
X1K = a movement of .100 inch or 2.54 mm
The buttons used to select the axis and the direction of movement are located on the mid to upper right part of the operator panel as shown in Figure 1 for this controller.
Figure 12 Speed/Multiply Buttons
For example, to displace the tool along the X axis in a positive direction by the value of .010 inch, follow these steps:
• Press the INC JOG button.
• Press the X100 button.
• Press the button X once.
Each time the button is pressed, a displacement of the selected value results.
If the JOG mode is selected when one of these buttons are activated and the selected axis button is pressed and held in, the movement will occur at feed as indicated by LOW, MEDL, MED, MEDH or HIGH. The operator can also use the % Traverse Feed override dial to further control this feed rate.
When the MPG Operation mode is selected, the incremental step selected by the Speed/Multiply buttons determines the magnitude of the movement along the chosen axis in the selected direction.
Each button setting corresponds with the scale of the Handle. One full revolution of the Handle (360°) corresponds to 100 units on the scale. On the button X1 the X means “times” the minimum increment.
When the button is pressed for:
X1, turning the handle by one unit corresponds to the movement of .0001 inch or .0025 mm.
X10, turning the handle by one unit corresponds to the movement of .001 inch or .0254 mm.
X100, turning the wheel by one unit corresponds to the movement of .01 inch or .254 mm.
X 1K, turning the wheel by one unit corresponds to the movement of .100 inch or 2.54 mm.
Usually, X1 is used when you are precisely dialing-in the zero of the workpiece and when you are determining the tool length offset.
In manual control, you must also use the AXIS/DIRECTION buttons to determine the axis of displacement.
For example: if you need to move the machine table, with respect to the tool by 1.00” along the X axis in a positive direction, follow these steps:
• Press MPG Operation mode button.
• Press the AXIS/DIRECTION button X+
• Press the SPEED/MULTIPLY button X10.
Turn the handle one full revolution (100 units) and then check the value of the displacement on the screen. It should indicate a movement of 1.00”.
LOW
X1
The button, LOW indicates feed rate at a LOW speed while in the JOG Operation mode. The button, labeled as LOW X1 indicates that turning the handle by one unit corresponds to the displacement of .0001 inch or .0025 mm while in the MPG Operation mode.
MEDL
X10
The button, MEDL indicates feed rate at a MEDIUM LOW speed while in the JOG Operation mode. The button, labeled as MEDL X10 indicates that turning the handle by one unit corresponds to the displacement of .001 inch or .0254 mm while in the MPG Operation mode.
MED X100
The button, MED indicates feed rate at a MEDIUM speed while in the JOG Operation mode. The button, labeled as MED X100 indicates that turning the handle by one unit corresponds to the displacement of .01 inch or .254 mm while in the MPG Operation mode.
MEDH
X1K
The button, MEDH indicates feed rate at a MEDIUM HIGH speed while in the JOG Operation mode. The button, labeled as MEDH X 1K indicates that turning the handle by one unit corresponds to the displacement of .100 inch or 2.54 mm while in the MPG Operation mode.
HIGH
This button is used to indicate the feed rate at a HIGH speed while in the JOG Operation mode.
SPDL DEC-Spindle Speed Decrease
Pressing this button causes the spindle speed to decrease.
SPDL 100%
Spindle override 100%: Sets an override of 100% for the spindle motor speed.
SPDL INC- Spindle Speed Increase
Pressing this button causes the spindle speed to increase.
Figure 13 Spindle Buttons
SPINDLE
These buttons are used exclusively during the manual operation of the machine for setup functions. The descriptions below explain their specific function:
SPDL CW-Spindle Rotation CW
By pressing this button while in one of the Operation modes; HOME, JOG, INC JOG or MPG the spindle will start rotation in the clockwise (CW) direction. The spindle r/min is adjusted by using the SPDL DEC, SPDL 100%, or SPDL INC buttons. The last r/min commanded in the program or used while in this mode is retained and will restart upon pressing the SPDL 100% button. When the machine is first started, there has been no value established for the r/min, so if one of these buttons is pressed while in the modes described above an alarm will result. An r/min must be input via MDI or by activating the program. From that point on, as long as the machine is not turned off, the r/min will be activated at the last commanded value when one of these buttons is pressed.
SPDL STOP-Spindle Stop
Pressing this button stops spindle motor rotation while in one of the Operation modes listed above. Pressing this button will NOT stop the spindle while in any of the Execution modes.
SPDL CCW-Spindle Rotation CCW
By pressing this button while in one of the Operation modes HOME, JOG, INC JOG or MPG the spindle will start rotation in the counterclockwise (CCW) direction. The spindle r/min is set by using the SPDL DEC, SPDL 100%, or SPDL INC buttons. The last r/min commanded in the program or used while in this mode is retained and will restart upon pressing the SPDL 100% button.
AXIS/DIRECTION
These buttons are used to select the Manual feed axis direction. Pressing these buttons executes movement along the selected axis in the selected direction by jog feed (or step feed) when the corresponding button is set to on in the jog feed mode (or step feed mode). The same is true for each of the axes where buttons are present.
Figure 14 Axis Direction Buttons
−X
When pressed, this button executes movement along the X axis in the negative direction with respect to the coordinate system.
+Z
When pressed, this button executes movement along the Z axis in the positive direction with respect to the coordinate system.
−Z
When pressed, this button executes movement along the Z axis in the minus direction with respect to the coordinate system.
+X
When pressed, this button executes movement along the X axis in the positive direction with respect to the coordinate system.
Note: The Y axis buttons for milling machines are not depicted in the operator panel in Figure 1. The following are their descriptions.
−Y
When pressed, this button executes movement along the Y axis in the negative direction with respect to the coordinate system.
+Y
When pressed, this button executes movement along the Y axis in the positive direction with respect to the coordinate system.
TRVRS-Rapid Traverse
Caution: When using this rapid traverse function be sure that all machine movements will not cause interference during motion!
Press this button to activate jog feed at a rapid traverse rate. Use this button to perform rapid movements along a previously chosen axis. For example, press the button TRVRS then the X positive button, the X axis will move at rapid traverse until the button is released.
Rapid Traverse Override (%)
(Not shown on this operator panel model)
Some operator panels include a % override dial or buttons that can be used to control the rapid feed rate. This switch or these buttons are used to reduce the rapid feed rate (G00). If it is positioned at 100, this corresponds to 100% of the rapid feed rate that the machine can generate. Buttons are commonly incremented in steps of 10, 25, 50 and 100%.
Figure 14b Rapid Traverse Override Buttons
In the above illustration, F0 corresponds with 10% (as determined by parameter).
COOLANT
During manual or automatic operation, these buttons may be used to activate or stop the flow of coolant.
CLNT ON-Coolant ON
When this button is pressed the supply of coolant is started.
CLNT OFF-Coolant OFF
When this button is pressed the supply of coolant is stopped.
CLNT AUTO-Coolant Auto Mode
This button is pressed to activate the automatic start and stoppage of coolant flow during program execution when called by program words M08 and M09 respectively.
Figure 16 Common Control Panel
CONTROL PANEL
The control panel described here is quite typical of the control panels used on CNC machines. The control panel switches and buttons may be distributed differently on the panel for each individual machine; however, the purpose and function of each switch and button remains the same. Some control panels are equipped with additional buttons or switches not shown here. Definitions and applications of these buttons or switches can be found in the manufacturer instruction manuals for the machines.
The control panel is located at the front of the machine and is equipped with a CRT and with various buttons and switches, as illustrated in Figure 16.
Two items not shown on this controller that are common on many modern controls are a 3.5 floppy disk and PCMCI (Portable Computer Memory Card Interface) slot. These are both used as a file storage medium and a method for file transfer. The floppies typically hold a maximum of 1.44 mega bytes (MB) of data while PCMCI cards range from 40MB to 200MB. The 1.44 MB floppy can store the equivalent of 3600 meters of paper tape. Both are widely used to store part programs offset data and NC parameter information. Because of emerging technologies in computer industry, the storage and data transfer medium described here are changing and improving rapidly and some controllers are now being equipped with a Universal Serial Bus (USB) drive interface.
A detailed description for the use of each button and the purpose of the particular sections of the control panel are presented in the following sections:
POWER-ON & POWER-OFF
These buttons are used to activate/deactivate the power to the control. The ON button is typically green in color and when it is ON, the key is lit. The OFF button is typically red in color and when the power is turned OFF to the control, the key is lit. At startup of the main power to the machine, the OFF button is lit.
Press theses buttons to turn CNC power ON and OFF.
Figure 17 On Button
Figure 18 Off Button
Notes: The control is always turned ON after the MAIN POWER switch is ON. The switch is located on the door of the control system and is typically at the back or side of the machine. The control is always turned OFF before the MAIN POWER switch is turned OFF.
CRT DISPLAY
This is the television-like screen on which all the program characters and data are shown. Sizes vary from around 9 inches to approximately 15 inches. Displays are color, monochrome or Liquid Crystal Displays (LCD).
Reset Key
Pressing this button resets or cancels an alarm and can be used for cancellation of an automatic operation. An alarm can only be cancelled if its cause has been eliminated.
Figure 19 Reset Button
When the reset button is pressed during automatic operation, all program commanded axis feeds and spindle revolutions are cancelled. The program will return to its starting block when this button is pressed.
Help Key
Pressing this key gives the operator help screens on how to operate the machine functions such as MDI key operation, or details related to an alarm that has occurred in the control.
Figure 20 Help Key
SOFT KEYS
The soft keys have numerous functions, depending on the applications selected with other keys. The specific functions of the soft keys are displayed at the bottom of the CRT screen as shown in Figure 21. The purpose of the soft keys is to minimize the use of dedicated keys on the control panel.
Figure 21 Controller Soft Keys
By use of the soft keys; the machine ORIGIN register can be reset, READ soft keys allow entering the program to memory from a punched tape or other storage medium, and the PUNCH soft key allows program readout from memory to a punched tape or other storage medium.
By pressing a soft key, the function selections that belong to it appear. These selection choices are called chapters. These selection soft keys are the first four rectangular keys under the CRT. By pressing one of the chapter selection soft keys, the screen for the selected chapter appears. If the soft key for a target chapter is not displayed, you must press the continuous menu key located at the right end of the soft keys (sometimes referred to as next-menu). In some cases, there are additional chapters that can be selected from within a chapter. When the desired screen is displayed, press the soft key under operation selection (OPRT) on the display for data to be manipulated. To reverse through the chapter selection soft keys, press the return menu key located at the left end of the soft keys.
The general screen display procedure is explained above; however, the actual display procedure varies from one screen to another. For details, see the description of individual operations.
Note: The operator should consult the manufacturer manual for more specific detailed instructions on the use of the soft keys.
Figure 22 Alpha-Numerical Keypad
ADDRESS AND NUMERIC KEYS (ALPHA-NUMERICAL KEYS)
This keypad of letters, numbers, and symbol characters is used to input data while writing or editing programs at the control. These keys are also used to enter numerical data and offsets into memory. Many of the keys are used in conjunction with other keys.
Shift Key
Because there is not enough space on the control for all keys necessary, some keys have two characters on them. When the letter or symbol indicated in the bottom right corner of the key is needed, the operator first presses the SHIFT key, which switches the key to that character. This sequence must be followed each time an alternate letter is needed. The shift key functions the same way as its equivalent on a computer keyboard.
On the display, a special character will be shown when a character indicated at the bottom right corner on the key can be entered.
Figure 23 Shift Key
Input Key
The INPUT key is used for MDI operation and to change the offsets. After the data are entered via the keypad the INPUT key is pressed. The data are entered into the offset register or the program for execution.
Figure 24 Input Key
Cancel Key
This key is used while inputting data in the MDI mode. It is essentially a destructive backspace key and can be used to correct an erroneous entry. Press this key to delete the last character or symbol input to the key input buffer. For instance, when the key input buffer displays:
Figure 25 Cancel Key
N5X12.00Z
and then the cancel key is pressed, the address Z is erased and
N5Xl2.00 is displayed.
EOB Key-End of Block Key
This is the END-OF-BLOCK key. When pressed while in the MDI mode the EOB character (;) is inserted into the program at the cursor location.
Note: The (;) symbol is never part of the program manuscript. The control system will automatically show the EOB character, for every “Enter” key used on a keyboard.
Figure 26 End of Block Symbol Key
PART PROGRAM EDIT KEYS
These keys are used to enter new program data (Insert), to make program changes (Alter), or to delete program data in memory (Delete). They are used while editing programs.
Figure 27 Program Edit Keys
FUNCTION KEYS
These buttons correspond to particular display modes (active mode).
By pressing any one of these buttons, the display will be switched to the corresponding screen. Then the soft keys may be used to display the needed data.
•Press the POS key to display the Position Screen.
•Press the PROG key to display the program list screen.
•Press the OFFSET/SETTING key to display the screen used to set offsets or adjust parameter settings.
•Press the SYSTEM key to display the system screen.
•Press the MESSAGE key to display the message screen.
•Press the GRAPH key to display the graphics screen.
Figure 28 Function Keys
CURSOR
This symbol is in the form of a blinking dash on the display, which is located below the position of a particular address while in one of the Edit modes. On many controls, the cursor highlights the whole word, for example X7.777
Cursor Move Keys (Navigation Keys)
In order to navigate through the program, there are four keys used to move the cursor.
Figure 29 Cursor Move Keys
The right pointing arrow key is used to move the cursor to the right or in the forward direction. When this key is pressed, the cursor moves only one space each press of the button, in the forward direction.
The left pointing arrow key is used to move the cursor to the left or, in the reverse direction. Just as with the prior described case, when this key is pressed, the cursor moves only one space each press of the button, in the reverse direction.
The downward pointing arrow key is used to move the cursor downward through the program in the forward direction. When this key is pressed, the cursor moves one full line downward in the forward direction, each time.
The upward pointing arrow key is used to move the cursor upward through the program in the reverse direction. When this key is pressed, the cursor moves one full line upward in the reverse direction each time.
Page-UP/DOWN Keys
Usually the length of the program exceeds what the height of the screen will display. The CURSOR move keys can be used to scroll through the program. When you press and hold the CURSOR button with the down or up arrow, the cursor will move through the program line-by-line. A more effective method to move a large amount is to use the two PAGE keys. Using these keys will advance in the direction selected by the number of lines the screen can display. The last block of a given page becomes the first block of the next page. Use the PAGE button with the arrow pointing up to change pages in the opposite direction.
Figure 30 Page Keys
Example:
O0001
N1G50X7.777 Z7.777 S1000
N2T0100M39
N3G96S600M03
In the above example, with the CURSOR resting below N then pressing the CURSOR button three times with the right-pointing arrow causes the cursor to be located below the letter (address) G.
By pressing the CURSOR button (with the arrow pointing up) repeatedly, the prompt will move to the first word of program O, which corresponds to the upper limit of cursor movement. Another fast way to return to the program head is to press the RESET key.
By pressing the CURSOR button once, with the arrow pointing down, the cursor will move down one line. If the cursor must be moved over a few or many words, you need not press the button repeatedly. Just press and hold this button down; the cursor automatically jumps one word at a time in the given direction. The PAGE keys allow for scrolling through long programs more effectively.
OPERATIONS PERFORMED AT THE CNC CONTROL
The following explanations are for operations considered routine for operators of CNC machine tools and are given in their sequence of use.
Please note that the following procedures are specific to the type controller depicted here (Fanuc 16 or 18 series). The procedures for another type control may be similar. Be sure to consult the manufacturer manuals specific to your machine tool operation and control panel.
The Machine is Turned on and Homed (Machine Zero)
Turn on the main power switch, and then press the ON Power button on the controller. Most modern machine tools will automatically start-up in the HOME mode. This means that before any automatic or manual operation may begin, it will be required to Home the machine first.
If the Operation selection LED, HOME, is not lit, press it now.
Using the Axis/Direction keys, press the direction necessary to HOME the machine. Note that many machine tools will have LED’s for each axis that are lit to indicate when an axis is HOMED.
Figure 31 Actual Position (Absolute) Screen
At machine start-up, a common screen displayed is ACTUAL POSITION (ABSOLUTE). If it is not displayed, press the function key labled POS then the soft key ABS. The displayed coordinate values represent the relationship between the Workpiece Zero and the Machine Zero (HOME). When the machine is HOME, press the soft key OPRT, then press ORIGIN and then press ALLEXE to zero each of the coordinate axes.
By pressing the soft keys, other display screens can be activated. For instance, when we press the button ABS (which corresponds to position), the digital counter appears on the screen for the X and Z axes, which is the absolute coordinate system for a given workpiece (for milling machines X, Y, and Z will be displayed). The position (POS) function is assigned four display screens and can be found by pressing the soft keys labeled; ABS, REL, ALL and OPRT. The first screen corresponds to a position change in the ABSOLUTE (ABS) system for X, Z, as illustrated. The second screen RELATIVE (REL) corresponds to position changes in the incremental system, U and W (for milling machines X, Y, and Z). The third, ALL gives representation of all four of the displays simultaneously on one screen as shown in Figure 32.
The values listed in the readout for MACHINE represent the distance from Machine Home position.
The DISTANCE TO GO readout is the most significant part of the third display. The coordinates in this quarter of the display of the screen correspond to the path that will be followed by the tool in order to complete the execution of a given block of information while under automatic operation.
Example:
N20G00Z0.
N22G01Z-12.000F.015
Figure 32 Position, Actual Position, Screen
Figure 33 Program Library Screen
When block N22 is first read by the control, the value Z-12.000 will appear under DISTANCE TO GO readout in the lower right corner of the screen. After moving a distance of 1 inch, the value of coordinate Z changes to Z-11.000, and so on. The other displays, “ABSOLUTE” and “RELATIVE” correspond to the first two display screens, but this time they are smaller so that all four may fit on one screen. All of the displays may be changed to read in millimeters, with respect to Machine Zero, by changing a machine parameter or by using a G-Code in the program.
A Program is Loaded From Memory
The program may be in the program directory but not activated for automatic operation. Follow these steps to activate a program.
1. Press the EDIT button to enter the EDIT mode.
2. Press the PROG function key.
3. Either the program contents or program file directory will be displayed.
4. Press the OPRT soft key.
5. Press the rightmost (continuous-menu key) soft key.
6. Use the keypad to enter the desired program number preceded by the letter address O.
7. Press the FSRH (forward search) and the EXEC soft keys.
The program will now be in the active status and ready to use for automatic operation.
An NC Program is Loaded Into Memory
Follow the steps below to load a program into the controller from an NC tape. Be sure that the input device is ready for reading (tape entry to tape reader if used).
1. Press the EDIT button on the operator’s panel to enter the Edit mode.
2. Press the PROG function key.
3. Either the program contents or program file directory will be displayed.
4. Press the OPRT soft key.
5. Press the rightmost (continuous-menu key) soft key.
6. Use the keypad to enter the desired program number to load preceded by the letter address O.
7. Press the READ soft key and then the EXEC soft key.
The program will be loaded into the controller’s memory.
A Program is Saved to an Offline Location
For example; an NC Tape, Floppy disc, PCMIA card, or PC hard disk connected via RS232.
Follow the steps below to save a program to an NC tape.
Be sure that the output device is ready for output.
If the NC tape output is EIA/ISO, it needs to be specified by using a parameter.
1. Press the EDIT button on the operator’s panel to enter the EDIT mode.
2. Press PROG function key.
Either the program contents or program file directory will be displayed.
3. Press the OPRT soft key.
4. Press the rightmost (continuous-menu key) soft key.
5. Use the keypad to enter the desired program number to save preceded by the letter address O.
6. To save all programs stored in memory Press –9999.
7. To save multiple programs at one time enter their program numbers separated by a coma i.e.: O1234, O1235.
8. Press the PUNCH and then EXEC soft keys.
The program will be saved to the offline location media.
A Program is Deleted From Memory
To delete a program for the controller memory, follow these steps:
1. Enter the EDIT mode.
2. Press the PRGRM soft key.
The program directory will be displayed.
3. Press the OPRT soft key.
The screen with soft keys labeled F SRH, READ, PUNCH, DELETE and OPRT will be displayed.
The program directory is displayed only while in the EDIT mode.
4. Press the DELETE soft key.
5. Enter the program file number (preceded by the letter address O) you wish to delete.
6. Press the EXEC soft key.
The file is deleted.
To delete all programs from memory use steps one through three, and then the following steps in place of the last three steps as above:
Caution: Be sure the program files you are deleting are backed up prior to executing these steps because they will not be recoverable!
O–9999
DELETE
EXEC
The operator may input small programs via the keypad at the control. The size of the program is limited to 10 lines on the control that is described in this book and is determined by the parameter setting from the manufacturer. It is an excellent method of executing simple commands like tool changes, controlling the spindle r/min and its rotation direction, etc. To enter the MDI mode of operations follow these steps:
1. Press the MDI button on the operator panel.
2. Press the PROGRAM function key.
3. Enter the desired program number preceded by the letter address O.
4. Enter the data to be executed by using the methods described later in PROGRAM EDITING FUNCTIONS.
As soon as the program number is entered, you can begin to enter program data. If a program number is not input, the control assumes O0000, and the data may be entered. Each block ends with end of block (EOB) character (;) so that individual blocks of information can be kept separately. For example: N1G50S1000;
5. Press the EOB function key to insert the semicolon at the end of each line.
6. Press the INSERT edit key.
7. Press CYCLE START to execute the program information.
If a typographical error is made while entering a given block, you can eliminate the error by pressing the CAN key to CANCEL the error and then reenter the correct value.
The MDI program may be executed just as with automatic operation and the same control functions apply except that an M30 (tape rewind) command does not return the control to the program head instead M99 is used to perform this function. Please refer to the machine tool manufacturer manual for specific instructions.
Erasure of an entire program created in MDI mode may be accomplished as follows:
1. Use the alphanumeric keypad to enter the address O.
2. Press the DELETE key on the MDI panel.
The same result may be accomplished by pressing the RESET key.
Also the program will be erased when execution of the last block of the program is completed by single–block operation.
To perform an individual MDI operation, use the methods described above. For the control described here use the display screen shown in Figure 34.
Example 1:
1. Turn on the spindle at 500 RPM in the clockwise direction.
2. Key in the following command:
3. S500M03
4. EOB
5. INPUT
6. CYCLE START
Figure 34 Program Screen in MDI Mode
Example 2:
Follow these directions to position tool number 5 to the active position on the turret (or to install tool 5 into the spindle on a milling machine).
Key in the following command:
1. T0500 (or T5M06 for a mill)
2. EOB
3. INPUT
4. CYCLE START
The codes listed along the bottom of the display pictured in Figure 34 are G-Codes that are active upon start up of the machine called defaults. They are also reinstated upon pressing of the RESET key.
MEASURING WORK OFFSETS, TURNING CENTER
It is necessary to establish a relationship between the machine coordinate system and the workpiece coordinate system. The following steps are necessary to input the measured values for the workpiece zero to the controls Work Coordinates offset page.
Measure the Z Axis Work Coordinate
1. Manually position the cutting tool and make a cut on the face of the workpiece.
2. Without moving the Z axis, stop the spindle and move the tool away from the part in X-axis direction.
3. Measure the distance along the Z axis from cut surface to the desired zero point.
4. Press the WORK soft key to display the WORK COORDINATES display screen.
5. Position the cursor to the desired Workpiece offset to be set.
6. Use the letter address key Z to select the axis to be measured
7. Use the value of the measurement taken to input the Z axis Work Coordinate
8. Press the MEASUR soft key.
The Work Coordinate for the Z axis will be input.
Measure the X Axis Work Coordinate
1. Manually position the cutting tool and make a cut along Z axis to create a diameter on the workpiece.
2. Without moving the X axis, stop the spindle and move the tool away from the part in Z axis direction.
3. Measure the diameter you just cut on the workpiece.
4. Use the value of the measurement taken to input the X axis Work Coordinate (enter the diameter).
5. Follow the same procedure for setting the Z axis Work Coordinate value as stated in steps six and seven above.
The Work Coordinate for the X axis will be input.
MEASURING WORK COORDINATE OFFSETS, MACHINING CENTER
Following is the procedure for setting the Work Offsets for each workpiece coordinate system G54 to G59. When the values are known you can:
1. Press the OFFSET/SETTING function key.
2. Press the WORK soft key.
The WORK COORDINATES setting screen is displayed as shown in the Figure 35. There are two display screens needed to handle the six offsets G54 to G59. To display a desired page, follow either of these two methods:
1. Press the PAGE up or PAGE down keys until the desired offset is shown.
2. Enter the offset number, G54 – G59.
3. Press the NO.SRH soft key.
Figure 35 Work Coordinates Display Screen
To change the coordinate values of the offsets, use the following method:
1. Use the arrow keys to position the CURSOR on the appropriate offset number.
2. Use the alphanumeric keypad to enter the new value for the offset.
3. Press the INPUT soft key.
Note: When the INPUT key is used to enter values, the amount entered will replace any amount in the register. When the +INPUT or -INPUT key is used, the existing amount in the offset register will be added or subtracted, whichever applies, by the amount entered into it.
Once the value is entered here, it is the Workpiece Zero or origin for the workpiece coordinate system.
To change an offset by a specific amount, use the alphanumeric keypad to enter the desired value then press the +INPUT soft key.
Measured Values
Work Offsets can be measured manually by positioning an edge-finding tool to contact with the workpiece zero-surface in both X and Y axes sequentially. This procedure is called Edge Finding and is nearly always the perpendicular edges (secondary and tertiary datum) of the workpiece that is referenced.
Follow these steps for Work Coordinate Offset measuring:
1. Position the machine to HOME.
2. Use the procedure above (steps 1 – 3) to find the WORK COORDINATES setting display screen.
3. Use the arrow keys to position the cursor on the offset you wish to use.
4. Press 0 INPUT for the X value.
5. Press 0 INPUT for the Y value.
6. Install an Edge-Finding tool into the spindle using MDI or manually.
7. Start the spindle RPM clockwise at approximately 1000 by using MDI or manually.
8. Manually position the tool tip edge to contact the workpiece zero-surface along the X or Y axis.
9. Use the alphanumeric keypad and press X or Y and then INPUT, to enter the axis to be measured.
The desired axis should be blinking on the display screen and the soft key options NO. SRH and MEASUR should be present.
10. Press the MEASUR soft key. The absolute position value will be input to the offset.
11. Manually retract the Edge-Finding tool and repeat the same operation for the remaining axis. In most cases, the operator will be required to input the difference between the value input and the Edge-Finder radius (typically 0.100 or 3mm) before automatic operation can be executed.
On Turning Centers, the tool offsets are measured in two directions: Z and X.
These values represent the difference between the reference position (Machine Home) of the tool turret used in programming and the actual position of a tools tip used as the programmed tool point. The amount of Tool Nose Radius is input on the OFFSET display screen where R is indicated for each tool. An incorrect value here will have an affect on the finished part where tapers and radii are turned. Refer to Part 3, Tool Nose Radius and Tip Orientation for more details.
Measured Values
If the position register commands (G50 for turning or G92 for milling) are used, the values for each tool that have been measured will be input into the program for each tool with the G50 or G92 command.
The more commonly used method today is to input these values into the OFFSET/GEOMETRY register for each tool (See Figure 37). Follow these steps for input of the measured tool offset value.
Figure 36 Offset Display Screen
Figure 37 Offset/Geometry Display Screen
Measure the Z Axis Offset
1. Manually position the cutting tool and make a cut on the face of the workpiece.
2. Without moving the Z axis, stop the spindle and move the tool away from the part in X axis direction.
3. Measure the distance along the Z axis from cut surface to the desired zero point. Use this value to input the Z axis offset for the desired tool number, with the following procedure:
4. Press the OFFSET/SETTING function key.
5. Press the OFFSET soft key until the required tool offset compensation display screen is found.
6. Use one of the search methods or use the cursor keys to move the cursor to the offset number to be set.
7. Use the alphanumeric keypad to select the letter address Z.
8. Use the alphanumeric keypad to key in value of the measurement taken.
9. Press the MEASURE soft key.
The difference between measured value and the coordinate will be input as the offset value.
Measure the X Axis Offset
1. Manually position the cutting tool and make a cut along Z axis to create a diameter on the workpiece.
2. Without moving the X axis, stop the spindle and move the tool away from the part in Z axis direction.
3. Measure the diameter just cut on the workpiece.
4. Follow the same procedure for setting the X offset value as stated above (steps 5 – 10).
Apply this method for all of the remaining tools used in the program. The offset values are automatically calculated and set.
Tool Sensor Measuring
On some newer machines, a method of tool-offset measurement exists where a tool sensor is used as opposed to machining the diameter and face of the material. In this case, all of the programmed tools are manually or automatically positioned to contact the sensor for each axis and the offset values are automatically input to the control. The operator still must manually enter Tool Nose Radius compensation values in the “R” column of the OFFSET/GEOMETRY register.
ADJUSTING WEAR-OFFSETS FOR TURNING CENTERS
Wear-Offsets are used to correct the dimensions of the workpiece that change because of cutting tool wear.
For a Turning Center, the X direction offset corresponds to the diameter, for example: if the X wear offset for a tool is .01, an incremental change of minus .01 refers to a decrease of the diameter by .01 and an incremental change of plus .01 refers to an increase of the diameter by .01.
To adjust the WEAR-offsets:
Press the OFFSET/SETTING button until the screen display shown in Figure 38 appears.
Examples of Adjusting Wear-Offsets
For the following examples, the operator should display the OFFSET screen for WEAR offsets and the cursor should be positioned to the tool and axis requiring adjustment.
Figure 38 Offset Display Screen for Wear-Offsets
Example 1: The Absolute System
If after machining the workpiece shown in Figure 39, the measured external diameter exceeds the value of tolerance (i.e. 1.003), enter the offset with a negative sign assigned to the value -.003 in the wear offset by following these steps.
Figure 39 Examples of a Machine Workpiece used for Adjusting Wear-Offsets
1. Press X
2. Key in -.003
3. Press INPUT
Then, after machining several more pieces, the diameter increases due to tool wear. If the measured diameter is 1.002, enter the offset as follows:
1. Press X
2. Key in -.005
3. Press INPUT
Please note that it was necessary to add a value of .002 into the Offset register to the previously entered value of .003. A similar approach is applicable in the direction of the Z axis.
If the measured length is 1.492, then the value of the offset entered is -.008.
1. Press Z
2. Key in -.008
3. Press INPUT
A new measured length of 1.494 gives an entered value of the offset of -.006.
1. Press Z
2. Key in -.014
3. Press INPUT
Example 2: The Incremental System
To gain a better understanding, let us examine identical cases when the incremental coordinate system is used. The measured value is = 1.003.
Offset: U
1. Key in -.003
2. Press INPUT
Following that, the diameter is = 1.002.
1. Press U
2. Key in -.002 (on the screen)
3. Press INPUT (X-.005)
And Z = 1.492
Offset: W
1. Key in -.008
2. Press INPUT
After machining a few pieces, Z = 1.94.
Offset: W
1. Press W
2. Key in -.006 (on the screen)
3. Press INPUT (Z-.014)
Tool Length Offsets “TLO” are called in the program by the H-word. The values input into the corresponding TLO# register are needed for proper positioning of the tool along the Z axis. Similarly, the Cutter Diameter Compensation “CDC” values are entered on the Offset display register under column “R” and are called in the program by the D-word. These compensations are important for proper radial (X, Y) positioning of the tool. If the values are known, the following sequence can be used to input them into the offset page. When the setup values are known, you may:
1. Press the OFFSET/SETTING function key.
2. Press the OFFSET soft key. It may be necessary to press this key several times until the desired offset display is present.
3. Use the arrow direction or page keys to position the cursor to the tool number to be set.
The search method may also be used by entering the tool number whose compensation is to be changed and the pressing the NO.SRH soft key.
Enter the numerical value of the offset (including sign) and press the INPUT soft key.
To add or subtract from an existing offset value key in the amount (a negative value to reduce the current value), then press the +INPUT soft key.
Diameter compensation values are input, as known, after measuring their actual size. Depending on the parameter setting for the specific machine used, the value is entered as either tool diameter or radius. Consult the appropriate manufacturer operation manual for exact conditions.
Measured Values
