Rotating cutting tools can be held in at least two attitudes: parallel to the X or Z axes. The cutting tools can perform machining operations on faces (Z-axis work) or on diameters (X-axis work).
With some live tooling machines, each cutting tool is fixed on the X- and Z-axis center lines. The tool cannot move in the direction perpendicular to the XZ plane. These machines can only perform machining at the center of the workpiece in X.
More-sophisticated live tooling machines enable machining perpendicular to the XZ plane because they have a Y axis. While the Y axis often has limited travel (compared to the Y axis of a machining center), it increases machine capability. Now machining operations do not need to be centered on the workpiece.
One common frustration with Y-axis lathes is that each cutting tool requires calibration during setup. That’s because many machines’ live tooling tool stations are not perfectly aligned with one another. When the center of one is at the X-axis center, the others won’t be. Indeed, many sliding-headstock machines actually use the Y axis as the “tool changing mechanism.” The Y axis simply moves to change from one cutting tool to the next.
While there may be ways to permanently qualify and record the related center positions, many setup people go through a tedious process to calibrate every live tool along the Y axis for every setup. This procedure involves touching off an aligning pin (held in the tool station) on both sides of the workpiece and using the position displays to calculate the center of workpiece location for the tool station along the Y axis. With this value known (the Y-axis program-zero assignment value for the tool station), the setup person enters it into the appropriate geometry offset.
Here’s a custom macro to simplify the process.
O0001 (CROSS TOOL ALIGN Y AXIS)
N1 #121 = 1 (TOOL NUMBER TO CALIBRATE)
(SELECT TOOL AND JOG PIN TO ABOUT 0.25 ABOVE PART IN X.)
N3 #101 = #5003
N4 G01 Y[#101+0.4] F30.0
N6 #3006 = 100 (TOUCH X PLUS SIDE)
N7 #110 = #5003
N8 G01 Y[#101+0.4]
N12 #3006 = 100 (TOUCH X MINUS SIDE)
N16 #105 = [[#110+#111]/2]]
N18 #106 = #5023
N19 #[2300 + #121] = #106
Begin by placing a pin in the cutting tool holder. The pin can be the same diameter as the cutting tool you’ll be using.
Then, alter line N1 by entering the tool station number of the tool to be calibrated. Next, manually jog the machine so the pin is approximately centered on the workpiece in Y and about 0.2 inch above the workpiece in X.
Next, activate the program. The current Y position is stored in line N3. #5003 is the current position in the third axis, which is the Y axis for most turning centers.
The Y axis moves plus in line N4 to a position that clears the workpiece diameter. In line N5, the pin moves below center in X (U commands an incremental X movement).
In line N6, the machine stops and displays the message “TOUCH X PLUS SIDE.” Select
the handwheel mode and cautiously touch the pin to the workpiece in X. When finished, place the mode switch back to automatic and press the cycle start button.
Line N7 stores the current Y position (while the pin is touching), and then the pin moves clear and comes back to center in lines N8 through N10.
The process is repeated for the Y minus side in lines N11 through N15. In line N16, the true Y center line is calculated, and the Y axis moves to this position. In line N18, the current Y-axis position relative to the Y-axis zero return position is determined. Finally, in line N19, this value (Y-axis program-zero assignment value) is placed in the appropriate geometry offset.
This program can be improved. You may, for example, be able to have the custom macro automatically detect which live tool is in position (possibly by testing the current Y position after center is found). Also, this program is for relatively small parts (ranging to about 0.5 inch in diameter if a 0.25-inch-diameter pin is used). With a few modifications, it can work for larger part sizes.