Programming of CNC Machines. Ken Evans
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