Using Secondary Offsets On Machining Centers

Most machining center programs require but one offset per tool. When it comes to tool length compensation, for example, most applications require that you use one tool length compensation offset for each tool. The same is true for cutter radius compensation. Most tools require one cutter radius compensation offset per tool.

The primary offset number is usually quite easy to determine. Most programmers simply make it the same as the tool station number. Tool number five, for example, will use offset number five. Tool number six uses offset six, and so on. This logic makes it easy for the setup person and operator to know which offsets affect each tool.

You may know, however, that some controls have one offset value per tool. That is, the control manufacturer does not allow the programmer to specify tool length compensation values with the same offset number as cutter radius compensation values. With this kind of control, programmers commonly add a constant number (greater than the number of tools the machine can hold) to the tool station number to come up with the offset number used with cutter radius compensation. If the machine can hold 30 tools, for example, they’ll simply add 30 to the tool station number to come up with the cutter radius compensation offset number. Tool number five will use offset number five as the primary offset for tool length compensation and offset 35 as the primary offset for cutter radius compensation.

As stated, one offset per tool is usually sufficient. Once you instate tool length compensation, for example, it will be correct for all cutting movements the tool makes. The same is true for cutter radius compensation. There are times, however, when you may need more than one offset per tool. This is most commonly necessary when there are differences in tool pressure from one surface the tool machines to another. Consider the drawing.

Notice that there are two pockets that must be milled. One pocket, located at the base of the workpiece, has good, stout support. The other is right in the middle of a rather flimsy area of the workpiece. It is likely that the tool will push the workpiece away in this area while the pocket at the base of the workpiece will be machined in its normal fashion. It’s likely that the pocket in the flimsy area will be shallower than the pocket at the base of the workpiece.

This problem can be easily overcome with two tool length compensation offsets, one for the pocket in the flimsy area and another for the pocket at the base of the workpiece. This will give the setup person complete and individual control of each pocket.

Programming two offsets is actually quite easy. Simply instate the primary offset on the tool’s first Z-axis motion to the first pocket you wish to machine. When finished, retract in Z to a location that clears the second surface. Instate the secondary offset on the tool’s first Z-axis approach to the second surface. Pick a logical offset number, and make sure the setup person and operator know what you are doing.