The more commonly used method today is to input these values into the OFFSET/ GEOMETRY register for each tool (Figure 2-30). Follow these steps to input the measured tool offset value.
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 the X-axis direction.
3. Measure the distance along the Z-axis from the cut surface to the desired zero point.
4. Use this value to input the Z-axis offset for the desired tool number with the following procedure:
a) Press the OFFSET/SETTING function button.
b) Press the OFFSET soft key.
c) Use one of the search methods or use the cursor keys to move the cursor to the offset number to be set.
d) Use the alphanumeric keypad to select the letter address Z.e) Use the alphanumeric keypad to key in the value of the measurement taken.
f) Press the MEASURE soft key.
Figure 2-30 Turning Center OFFSET/GEOMETRY Display Screen Courtesy FANUC FA America
Input the difference between measured value and the coordinate as the offset value.
Measure the X-Axis Offset
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 just cut on the workpiece.
4. Follow the same procedure for setting the X offset value as stated above (steps 4. a–f) to input the diameter measured in step 3.
Apply this method for all of the remaining tools used in the program. The offset values are automatically calculated and set.
Turning Center Tool Sensor Measuring
On most modern machines, 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 and Tool Tip Orientation “T”. Review the Operator Manual specific to your machine for exact procedures.
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.
• Press the OFFSET soft key. The screen display shown in Figure 2-31 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.
Example 1: The Absolute System
After machining the workpiece shown in Figure 2-32, if the measured external diameter exceeds the value of tolerance (for example, 1.003), enter the offset with a negative sign assigned to the value –.003 in the wear offset by following these steps.
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+
Figure 2-31 OFFSET/WEAR Display Screen Courtesy FANUC FA America
Figure 2-32 Example of a Machined Workpiece Used for Adjusting Wear Offsets Courtesy FANUC FA America
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.
3. Press U
4. Key in –.002 (on the screen)
5. 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
3. Press W
4. Key in –.006 (on the screen)
5. Press INPUT (Z–.014)
TOOL PATH VERIFICATION OF THE PROGRAM
Конец ознакомительного фрагмента.
Текст предоставлен ООО «ЛитРес».
Прочитайте эту книгу целиком, купив полную легальную версию на ЛитРес.
Безопасно