Every dimension specified on a workpiece drawing has a tolerance—either explicitly specified with a tolerance band or implied in some manner. Explicit tolerances are specified in different ways (plus or minus a value, plus one value or minus another, or high limit and low limit).
Every dimension specified on a workpiece drawing has a tolerance—either explicitly specified with a tolerance band or implied in some manner. Explicit tolerances are specified in different ways (plus or minus a value, plus one value or minus another, or high limit and low limit). Implicit tolerances are usually related to a dimension’s number of decimal places. They are specified with a note somewhere on the blueprint.
A programmer must determine and specify the mean value of the tolerance band as the coordinate included in each programmed command. This will ensure consistency throughout the program and among programs. Everyone working with the program will know that programmed coordinates specify mean values. When using cutting tools (and offsets) from one job to the next, the setup person can rest assured, knowing that if a cutting tool machines dimensions to size in one job, it will continue to do so in the next.
I know CNC setup people and operators who also use the mean value of every tolerance band as the target value when machining workpieces. For a turned diameter machined on a turning center, let’s say a dimension is specified as 1.000 ±0.0005. The mean value, of course, is 1.000. If a workpiece has just been machined and this diameter comes out to 1.0004—and, assuming the operator wants to make a sizing adjustment—he or she will reduce the offset for the finish turning tool by 0.0004. With the next workpiece machined, the 1.000-inch diameter will come out precisely to its mean value (again, 1.000).
With small lots and large tolerances, targeting the mean value will work just fine. But with large lots, and especially with smaller tolerances, targeting the mean value has a major limitation.
As you know, every cutting tool used on a metalcutting CNC machine will wear as it machines workpieces. As a tool wears, a small amount of material will be worn away from its cutting edge(s). Tool wear will cause the cutting tool to remove less material from the workpiece, which changes the dimension(s) machined by the tool.
This is especially troublesome with turning centers because they use many single-point cutting tools. External diameters will grow as a finish turning tool wears, and internal diameters will shrink as a finish boring bar wears.
When you target the mean value, you’re only working with half the tolerance band. Again, if the tolerance is quite large, targeting the mean value may not present a problem. A cutting tool may last for its entire life without any of the dimensions it machines getting close to a tolerance limit.
But with small tolerances, the CNC operator may have to make sizing adjustments (to offsets) several times during the life of a cutting tool. This, of course, can be quite distracting, especially if the operator is expected to do other things during the CNC cycle.
If your operators are currently targeting the mean value for every tolerance band, you can actually double the amount of time (and number of workpieces) between sizing adjustments. Instead of targeting the mean value, have the operators target a value that is close to the high or low limit, whichever will allow the cutting tool to machine for a longer period of time before a sizing adjustment is needed. I recommend targeting a value that is within about 20 percent of the limit.
For example, let’s take a look at the 1.000 ±0.0005 turned diameter. You know that this diameter will grow as the finish turning tool wears. So, I recommend having the operator target a value of 0.9996 when he or she makes a sizing adjustment (0.9996 is right at 20 percent of 0.0005, which, when subtracted from 1.000, brings the dimension to its 0.9995 low limit). This will allow the tool to machine workpieces until the 1.000 diameter grows to 1.0004 (within 20 percent of the high limit). Then a sizing adjustment will be made.
Another way to determine how close the target dimension should be to the tolerance limit involves finding out when operators are making sizing adjustments. Have them balance the sizing adjustment. In the example above, if they are only allowing the 1.000 diameter to grow to 1.0003 before they make a sizing adjustment back to the mean value, have them target a value of 0.9997.
While this may sound like an obvious way to handle sizing adjustments (if you currently use it), I’m amazed at how many operators target the mean value for every dimension they machine, regardless of the tolerance bands they must hold. If you leave operators on their own to determine target values, they’re probably targeting mean values. Production run documentation must specify the target value for every dimension that requires sizing adjustments.blog comments powered by Disqus