Separating The Use Of Geometry And Wear Offsets
Many current-model turning centers have two sets of offsets: Geometry offsets are used to assign program zero during setup, and wear offsets are used to make sizing adjustments during the production run. When users view these offsets on the display screen, they look very similar.
Many current-model turning centers have two sets of offsets: Geometry offsets are used to assign program zero during setup, and wear offsets are used to make sizing adjustments during the production run.
When users view these offsets on the display screen, they look very similar. Each will have the same number of offsets (32, 99, etc.) and four registers (X, Z, R and T).
Turret index and offset specification are done with a four-digit T word (T0101, for instance). The first two digits of the T word specify the turret station number and the geometry offset number. The second two digits specify the wear offset number.
When an offset is invoked, say T0101, the control will add the value in the geometry offset to the value in the wear offset and use the result as the total offset. If a value of -10.0276 is in the X register of the geometry offset and a value of (+) 0.001 is in the X register of the wear offset, the total offset will be -10.0266.
So, it really doesn’t matter into which kind of offset you enter a given value. If you want to make a sizing adjustment, you could enter it into the geometry offset; if you want to enter a program-zero assignment value, you could enter it into a wear offset (assuming the wear offsets do not have a maximum entry value on your machine).
Though these things are possible, I urge you to separate the use of offsets. Use geometry offsets solely for program-zero assignment during setup. Use wear offsets solely for the purpose of workpiece sizing during the production run.
While these may seem to be standard practices there are times when (in my opinion) offsets are used somewhat inappropriately. Here are two examples:
Initial sizing on the first workpiece. The setup workers have just finished making the setup, and they’re running the first workpiece hoping that it will pass inspection. They might be using trial machining techniques to ensure that new tools just placed in the turret will machine the workpiece to size. Tool number two, the finish-turning tool, has just completed its machining operation and they find that it has machined a 2-inch diameter that is 0.003-inch oversize. What should they do?
Before answering, let me ask two more questions. What caused the 0.003-inch deviation? Did it have anything to do with tool wear?
Though this initial deviation has more to do with program-zero assignment (possibly an inaccurate touch off) than tool wear, most setup people will modify the wear offset (reducing it by 0.003 inch). But do remember, they can just as easily reduce the geometry offset by 0.003 inch and the machine will behave in exactly the same manner.
What is the advantage of making the initial adjustments in the geometry offsets? For very small lots there may not be any. But with larger lots, finishing tools will eventually wear out and be replaced. During the tool’s life, it’s likely that several sizing adjustments have been made to accommodate tool wear. When the cutting tool is replaced, the operator must also remember to reset its wear offset. To what value will it be reset? If the initial adjustment is done in the wear offset, the operator must remember its initial setting (-0.003 in the example above). But if the initial adjustment is done in the geometry offset, they can simply reset the wear offset to zero. (You may be questioning if the operators can precisely change or index an insert in such a manner that it is in exactly the same position as the previous insert. But even if they cannot, they must still know the initial wear-offset setting, regardless of whether trial machining will be done when the tool is replaced.)
So again, I recommend that setup people make initial adjustments in geometry offsets so that the values of wear offsets will be zero when the production run begins.
Tool nose radius compensation offset entries. The R and T registers are related to tool nose radius compensation. R specifies the radius of the cutting tool and T is a code number that specifies the tool type (T2 specifies a boring bar, and T3 specifies a turning tool). Again, there are R and T registers in both the wear and geometry offset pages.
First of all, be sure your setup people are not entering duplicate values in both wear and geometry offsets (I’ve often seen this mistake). If, for example, they enter a value of 0.0312 (for a 1/32-inch tool nose radius) in both R registers, most controls will add them together and use the total (0.0624 in our case). Worse, if they enter the T value in both registers—like T3 for a turning tool—most controls will interpret the T word as T6 (not a turning tool). Note that there are some parameter settings that deal with these issues, so some controls may behave differently than others in this regard.
While the R and T registers have nothing to do with program-zero assignment, I recommend entering tool nose radius compensation values into geometry offsets (leaving the R and T registers of the wear offset at zero). There are applications when as a cutting tool dulls, its radius gets smaller such as a button tool that machines a ball shape on the workpiece. Trying to deal with this problem with the X and Z registers will never render the desired results. Entering the amount of tool wear in the R register of the wear offset will correct the problem.