All current model CNC controls allow offsets to be changed during the execution of the CNC program. That is, operators can change an offset during a production run while the machine is running. For example, if a turning center operator determines that the diameter of a workpiece is growing close to its high limit, the operator can change the related offset while the machine is running the next workpiece. If the operator happens to make the change prior to the tool change for the tool being modified, the change will take effect in the very next workpiece. If not, it will take effect in the workpiece after that. This is true of both machining centers as well as turning centers.
Note that most current model controls do not allow the operator to change the program that’s being executed while it’s being executed (with most controls, you cannot change the program that’s running while it’s running). Remember that there is a feature called background edit, but it only works with other programs on most controls (you can change another program while a program is running).
Since offsets can be changed while the machine is running, they should always be your method of choice for handling sizing problems. If they are, the task of holding size can always be off-line. Again, the machine can be productive while offsets are being changed.
Though this is the case, there are still many programmers who handle sizing problems by expecting the operator to change the program. One classic example is related to tool pressure when turning a critical diameter on a turning center. If one end of the diameter is better supported than the other, the workpiece will tend to push away from the tool as it machines, inducing a taper on the diameter. While this is a problem that can be handled easily with a second offset for the turning tool (in essence, each end of the diameter has its own offset), there are many programmers who will have the operator change the program to eliminate the taper. While both methods work, again, the machine must be down while the program is being changed. And it’s likely that as this turning tool dulls, the amount of taper on the diameter will change, meaning it may be necessary to adjust for the taper on the diameter several times during the tool’s life.
There will be other times when you may be tempted to handle sizing problems with program changes. In last month’s CNC Tech Talk column we discussed one—milling two pockets having different rigidity in the setup on a machining center. Other times include turning or boring two critical diameters on a turning center (possibly one is close to the tailstock with good, stout support, and the other is in the middle of the workpiece), machining two grooves on a turning center (again, possibly one is in an area of good support and the other is not), and turning long shafts on a turning center (possibly the part pushes away in the middle). Again, if you’re trying to minimize tool offset changing time during the production run, you should handle all sizing problems with offset changes as opposed to program changes. Though it may take a little more ingenuity, there will always be a way to do so.
Note that we’re talking about a problem caused by a difference in tool pressure from one time the tool machines to another, which is indicative of a lack of rigidity in your workholding setup. If you have this problem on a regular basis, it should be taken as a signal that you should improve the design of your setups.blog comments powered by Disqus