Programming this operation, when it’s required, can improve productivity.
It is common practice to use trial machining techniques to size-in cutting tools that machine surfaces with small tolerances. This involves adjusting the cutting tool’s wear offset during setup in such a way that the tool will leave excess material on the machined surface and the workpiece attributes will meet their target dimensions. This will enable the cutting tools to last for an extended period of time (possibly their entire lives) before a sizing adjustment is required.
After the first workpiece is machined, the machine is stopped and the setup person measures the machined surface and adjusts the offset by an amount that will bring the surface to its target value. Then the tool is rerun. When the tool cuts this second time, the workpiece dimensions should be very close to their target. Any deviation will be related to the tool pressure difference when machining the trial-machining stock versus the actual amount of stock left for machining.
While the concept of trial machining is not difficult to understand, trial machining itself does require manual intervention from the person running the machine. Anything that can be done to simplify and streamline the process will, in turn, improve productivity.
Trial machining is only required when a new cutting tool machines a critical surface for the first time—finishing tools machining small tolerances. Once the machine is in production, the vast majority of machining cycles will not require trial machining. Therefore, if we’re going to program the trial machining operation, we must provide a way for the setup person or operator to specify whether or not it is required.
An easy way to do this is to use the block delete function (specified by the slash code [/] in a program). The operator will turn on the block delete switch when trial machining is not required, and the machine will skip any trial machining commands. Conversely, he will turn off the block delete switch when trial machining must be done.
Following is an example for sizing-in critical diameters on a turned workpiece. Tool No. 1 is the rough turning tool, and tool No. 2 is the finish turning tool. Both tools are sized-in together, ensuring that the appropriate amount of finishing stock is left on all diameters (in this case, 0.04 inch) and that tool pressure does not affect the sizing adjustment. In this example, the trial machining is performed first in an area of raw material that eventually will be removed from the workpiece. This prevents removing too much material and having to scrap the workpiece. The raw material stock diameter is 3.0 inches, and the depth-of-cut for the roughing tool is 0.15 inch.
/G10 P1 U0.01 (Increase roughing offset by 0.01)
/N005 T0101 M41
/N010 G96 S400 M03
/N015 G00 X2.7 Z0.1 M08 (Tool will machine to 0.15 depth)
/N020 G01 Z-0.3 F0.015 (Machine enough to take measurement)
/N030 G00 X5.0 Z5.0 (Move to turret index position)
/N035 M00 (Stop for measurement; diameter should be 2.7)
/N040 T0101 (Ensure that offset change is instated)
/N045 G00 X2.7 Z0.1 M08
/N050 G01 Z-0.3 (Ensure that diameter is truly 2.7)
/N055 G00 X5.0 Z5.0
/N060 T0202 M42 (Index to finishing tool)
/N065 G96 S500 M03
/N070 G00 X2.62 Z0.1 M08 (Tool will machine 0.04 depth)
/N075 G01 Z-0.3 F0.008
N085 G00 X5.0 Z5.0
/N090 M00 (Stop for measurement; target is 2.62)
/N095 T0101 M41 (Actual machining starts here)
The G10 close to the beginning increases the rough turning tool’s offset by 0.01 inch, ensuring that this tool does not machine too deep on the first try. The roughing tool is then commanded to machine a small amount of material (at the tool’s required depth-of-cut) and is retracted to the turret index position. The machine stops, and the operator measures the diameter. Since the diameter will be slightly more than 2.7 inches, he adjusts offset No. 1 accordingly. Once the cycle is restarted, the roughing tool will machine again, ensuring that the diameter is 2.7 inches.
The finishing tool then machines 0.080-inch more from the workpiece, retracts to the turret index position and stops. The operator measures, and, if the diameter is not precisely 2.62 inches, adjusts accordingly. Machining of the actual part then begins. The roughing tool will leave precisely 0.04 inch (on the side), and the finishing tool will machine precisely to programmed diameters.
Be sure to include a message after each program stop (M00) to specify the size that the operator is shooting for. Also, the entire series of trial machining commands could be placed in a subprogram so that only one command (the calling M98 command) need be in the main program. This also makes a pretty good application for a custom macro if you must perform trial machining operations on a series of similar workpieces.
These subjects are the building blocks of training newcomers on a specific CNC machine tool.
Take a closer look at these reference position commands.
A custom-macro-based system can predict when a tool will become dull.