You know that machining centers have tool length compensation, cutter radius compensation and fixture offsets. Turning centers have geometry offsets, wear offsets and tool nose radius compensation.
You know that machining centers have tool length compensation, cutter radius compensation and fixture offsets. Turning centers have geometry offsets, wear offsets and tool nose radius compensation. However, there may be times when you don't agree with the methods by which they must be used. If you would like to change the way compensation types behave, or actually invent your own, custom macro B can help.
You have total access to all offsets (you can both read and write) from within a program when the control is equipped with custom macro B, or almost any version of parametric programming. This allows you to do things you may have thought impossible. Previous CNC Tech Talk columns gave some specific examples of how you can invent or modify compensation types. (See February 1995, May 1995, February 1996 and April 1998.)
This access to offsets from within programs has fantastic implications. Truly, when you see setup people and/or operators struggling with some compensation related function, recognize that you can probably help them by modifying the way your current compensation values are entered and handled.
Turning center controls, for example, have a nice wear offset table. The operator enters the small deviation between how the tool should be cutting and how it is actually cutting into the wear offset. Many machining centers, on the other hand, do not have wear offsets. To enter a small deviation, the operator must modify a very large value (commonly the tool length or cutter radius compensation value), a procedure more prone to error. With custom macro B, you can actually add a kind of wear offset function. For any tool that machines critical Z surfaces, for example, you can use a special offset in the offset table (we'll choose number ninety-nine for our example) as the tool's wear offset. Consider this command that plunges into a 0.5-inch deep pocket.
N050 G01 Z-[0.5 - #2099] F4.0
System variable #2099 contains the value of offset number ninety-nine. If its value is currently zero, the pocket will be machined to a 0.5 inch depth. But say the operator measures the pocket depth and determines that it is 0.002 inch too shallow. Instead of modifying the (very large and cumbersome) tool length compensation offset for this tool, the operator will instead enter -0.002 inch in offset number ninety-nine (or whatever offset you designate for the machining cutter's wear offset).blog comments powered by Disqus