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 the current position related to the workpiece.
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, you 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.
MACHINING CENTER TOOL OFFSETS
Tool Length Offsets (TLO) are referenced in the program by words beginning with H. The values input into the corresponding T# (LENGTH) GEOM column are needed for to properly position the tool along the Z-axis. When adjustments are needed to compensate for wear, values are input into the WEAR column. Similarly, the Cutter Diameter Compensation (CDC) values are entered on the Offset display register into the (RADIUS) GEOM column and are referenced in the program words beginning with D. 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 button.
2. Press the OFFSET soft key to display a figure such as Figure 2-29.
3. Use the cursor
