Never Change A CNC Program To Size A Workpiece

Has the following ever happened to you? You’re machining a 2. 0-inch diameter on a CNC turning center.


Facebook Share Icon LinkedIn Share Icon Twitter Share Icon Share by EMail icon Print Icon

Has the following ever happened to you? You’re machining a 2.0-inch diameter on a CNC turning center. After machining, you measure this diameter and find it to be 2.002 inches. What do you do? Maybe a better question is: What do your operators do?

This oversize condition can be corrected by changing the command in the program that sends the finish turning tool to the 2-inch diameter. The X coordinate in this command (X2.0), could be reduced by 0.002 inch (making it 1.998 inches). When the tool machines the next time, it will machine the 2.0-inch diameter correctly.

However, this is not the way your operators should be making sizing adjustments. If the program is saved to the DNC system, the programmed coordinates will no longer be mean values of tolerance bands. The next time the job is run, the setup person will not know to what dimensions each cutting tool will machine.

All cutting tools, including cutting tools that are used from job to job, must be sized in every job. If sizing is done properly, with recommended methods, cutting tools that machine properly in one job will continue to machine properly in the next.

Sizing adjustments must be done while the machine sits idle. Since sizing may have to be done several times for each finishing tool, the machine will sit idle many times during the production run.

Always make sizing adjustments with offsets. This is the obvious way to make sizing adjustments. In the example given above, an offset (a wear or geometry offset) will be reduced by 0.002 inch. The programmed coordinates will remain at mean values. Cutting tools that machine properly in one job will continue to machine properly in the next. Sizing adjustments can be made while the machine is running, regardless of how many times a sizing adjustment must be made for a given finishing tool.

The example given above (sizing a 2.0-inch diameter) emphasizes a very common application for sizing with offsets and you may be pretty sure that your people are handling sizing adjustments properly. So let’s consider a more unique application: Your lathe program is turning a long diameter. At the chuck end there is good support for the workpiece but at the other end, there is no support. As the cutting tool begins machining the long diameter, tool pressure causes the workpiece to push away from the cutting tool’s cutting edge. As the cutting tool gets closer to the chuck end, the workpiece will push away less and less. For this reason, you find that the long diameter is tapered, smaller in diameter at the chuck end.

Though the same principles apply, I’m surprised at how many people handle this application with program changes: The operator will modify the X axis starting position (or ending position) of the taper. Once again, the mean value will no longer be part of the program, sizing will be inconsistent from job to job, the machine will sit idle while the sizing adjustment is made, and, since the tool pressure will increase as the cutting tool dulls, it is likely that several sizing adjustments must be made during each tool’s life.

Consider a grooving tool that machines two grooves, one in an area with good support (close to the chuck or tailstock) and another in an area with weak support (in the middle of the workpiece). The groove in the weakly-supported area will be larger in diameter than the groove in the well-supported area. Again, do your operators modify the program in order to get both grooves to come out on size? Remember, as the grooving tool wears, tool pressure increases. It may be necessary to make several such sizing adjustments during the grooving tool’s life.

I repeat: Always make sizing adjustments with offsets. While some applications require a little more programming ingenuity to handle with offsets, the benefits easily justify the effort. With the applications just mentioned (tapered diameter and two grooves), sizing should be done with two separate offsets. In the tapered diameter application, one offset will control the chuck end of the diameter and the second offset will control the other end. In the grooving application, one offset controls the groove with good support and another offset controls the groove with poor support.

I’ve only shown a couple of examples, but rest assured there is always a way to handle sizing adjustments with offsets.