Programming of CNC Machines. Ken Evans
Press the OPRT soft key.
4. Press the rightmost (continuous-menu key) soft key two times.
5. Press the F OUTPUT soft key.
6. Select F SET or P SET to identify the File name or Program name respectively.
7. Use the keypad to enter the desired program number, preceded by the letter address O, and then press the EXEC soft key.
The program will be saved to the selected offline location media.
8. To save all programs stored in memory, use the same steps above Press O–9999.
A Program is Deleted from Memory
To delete a program from the controller memory, follow these steps:
1. Enter the EDIT mode.
2. Press the PRGRM soft key.
3. Press the DIR soft key.
The program directory will be displayed.
4. Press the OPRT soft key.
5. The screen with one of the soft keys labeled DELETE will be displayed.
6. Enter the program file number (preceded by the letter address O) that you wish to delete.
7. Press the DELETE soft key.
8. Press the EXEC soft key.
The file is deleted.
MDI OPERATIONS
You may input small programs via the keypad at the control. The size of the program, which is limited to 10 lines on the control described in this book, is determined by the parameter setting from the manufacturer. Small programs provide 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 data to be executed by using the methods described later in the section Program Editing Functions.
For the program number, the control assumes O0000 and the data may be entered. Each block ends with the end-of-block (EOB) character (;) so that individual blocks of information can be kept separately. For example:
N1 G50 S1000;
4. Press the EOB function key to insert the semicolon at the end of each line.
5. Press the INSERT key.
6. Press CYCLE START to execute the program information.
If you make a typographical error while entering a given block, you can eliminate it by pressing the CAN key to cancel the error and then reenter the correct value.
You may execute the MDI program as you do with automatic operation. 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.
You can erase an entire program created in MDI mode by the following step:
1. Press the RESET key.
The program will also be erased when the last block of the program is executed by single–block operation.
To perform an individual MDI operation, use the methods described above. For the control described, the display screen is shown in Figure 2-27.
Example 1
1. Turn on the spindle at 500 RPM in the clockwise direction.
2. Key in the following command:
3. S500 M03
4. EOB
5. INSERT
6. CYCLE START
Figure 2-27 Program Screen in MDI Mode Courtesy FANUC FA America
Example 2
Use the following 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 commands:
1. T5 M6 (or T0500for a turning center)
2. EOB
3. INSERT
4. CYCLE START
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 or adjustments are needed, 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 Figure 2-28.
Two display screens are needed to handle the six offsets G54–G59. To display a desired page, follow either of these two methods.
Method 1
1. Press the PAGE UP or PAGE DOWN keys until the desired offset is shown.
2. Use the cursor move keys to select the offset number G54–G59 and axis desired.
Alternatively, you can input an offset number 01–06 and press the NO.SRH (number search) soft key. To change the coordinate values of the offsets, use the following method.
Method 2
1. Use the alphanumeric keypad to enter the new value for the offset.
2. Press the INPUT soft-key.
Figure 2-28 Work Coordinates Display Screen Courtesy FANUC FA America
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 new 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. In this procedure, which is called edge-finding, it is nearly always the perpendicular edges (secondary and tertiary datum) of the workpiece that are referenced.
Follow these steps for measuring Work Coordinate Offsets:
1. Position the machine to HOME.
2. Use the procedure above (steps 1–2) 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 either manually or by using MDI.
8. Manually position the tool tip edge to contact the workpiece zero surface along the X- or Y-axis.
9. Use the cursor keys and select X or Y; then input the value of