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 move keys 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 then 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
Tools length offsets can be measured by manually positioning the tool tip to contact the Workpiece Zero surface (Z-axis). This procedure is called “Touching-Off” and is nearly always the top most surface, primary datum of the workpiece. All tools used in the program must have their offsets recorded in the Offset register. If there is not a value in the offset register for a programmed tool, the control will not execute for that tool call, an alarm will occur, and the machine will stop. If a value of zero is in the offset register, the control will accept the zero offset and over travel will result. Conversely, if a value in the offset register is incorrect, the control will execute the tool call as if it was correct and the result could be a collision. For this reason, it is a good idea to delete tool offset data from the offset register when the tool for which it was intended is removed. To do this, input a value of zero for the tool offset register desired.
Figure 2-29 Machining Center OFFSET/GEOMETRY Display Screen Courtesy FANUC FA America
The following steps are needed for the tool offset measuring procedure:
1. Manually position the tool tip to contact the workpiece zero surface (Z-axis).
2. Press the POSITION function key.
3. Select the RELATIVE soft key.
4. Use the alphanumeric keypad and press Z and then INPUT to enter the axis to be measured. The axis should be blinking on the display screen and the soft key options PRESET and ORIGIN shown.
5. Press the ORIGIN soft key and then EXEC. The value in the RELATIVE position display will be changed to 0.0.
6. Press the OFFSET/SETTING function button and then press the OFFSET soft key to display the offset page for tool compensation.
7. Manually position the tool tip to contact the workpiece zero surface (Z-axis).
8. Use the arrow direction keys or the search method described above to position the cursor to the desired offset.
9. Use the alphanumeric keypad and press Z.
10. Press the INPUT soft key.
The relative Z value for the tool offset will be input to the offset register. Repeat for each tool used in the program.
Machining Center Tool Sensor Measuring
On most modern machines, a tool sensor is used as opposed to manually measuring each tool length. When this is the case, all of the programmed tools are manually or automatically positioned to contact the sensor for each tool axis, and the offset values are automatically input into the control. Review the operator manual specific to your machine for exact procedures.
ADJUSTING WEAR OFFSETS FOR MACHINING CENTERS
For machining centers, WEAR offset is assigned in the direction of the Z-axis for tool length compensation. Variations in the X- and Y-axes are compensated by adjusting the values in the (RADIUS) WEAR column. The method for inputting adjustment data is similar to adjusting wear offsets for turning centers.
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 control’s Work Coordinates offset page.
Measure the Z-Axis Work Coordinate
1. Identify the coordinate system G54–G59 to be used.
2. Manually position the cutting tool and make a cut on the face of the workpiece.
3. Without moving the Z-axis, stop the spindle and move the tool away from the part in the X-axis direction.
4. Identify the distance along the Z-axis from cut surface to the desired zero point.
5. Press the WORK soft key to display the WORK COORDINATES display screen.
6. Position the cursor to the desired workpiece offset to be set.
7. Use the letter address key Z to select the axis to be measured.
8. Use the value of the measurement taken to input the Z-axis work coordinate.
9. 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 the 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 the 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 above in Steps 6 and 7.
The work coordinate for the X-axis will be input.
TURNING CENTER TOOL OFFSETS
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 and the actual position of a tool 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 effect on the finished part where tapers and radii are turned. Refer to Part 3, Tool Nose Radius and Tip Orientation (T), for more details.