Thomas Industrial Library

Every CNC programmer and most of CNC machine operators have a simple chart of all common G-commands (G-codes) and M-functions (M-codes), usually tucked away somewhere under the lid of their tool box or they have them posted on any convenient machine side or cork board. This chapter covers most of those G-codes that are either uncommon, seldom used, special, or outright mysterious. Keep in mind that machine manufacturers often add G-codes and M-codes of their own. These special codes or functions cannot be covered in a general publication, such as this handbook.

Miscellaneous functions (M-functions) are not covered here at all, as they are often very much dependent on the machine tool manufacturer - for that reason, they are not part of this chapter. The situation is much different with various G-codes, some standard, some optional - they are covered here.

These special and less frequently used G-codes are as important as those used on a daily basis, even if only as accepting them for possible future use. Programmers often forget that there are many preparatory commands available that are not used very frequently. In this chapter, the focus will be on those G-codes that may sometimes become the key to solving a particular problem or achieving a particular programming goal. Some of these preparatory G-codes have a direct relationship with each other, in which case, all related commands will be considered together and explained together.

Divided into seven groups, seventeen preparatory commands covered in this chapter are:

Seldom used command G60 can be very practical if the machine tool suffers from a problem called backlash . Backlash is the result of wearing out the machine slides over a period of time. For that reason, the backlash problem is associated with older machines or machines that were exposed to some heavy duty machining, misuse and even some abuse. Virtually every control system offers a feature called backlash compensation - this is not a programmable feature, rather it is aimed at service technicians as it relates to the system parameter settings, sometimes combined with physical adjustments. Whether the backlash is compensated by software or by some physical means, it may not be enough to provide the optimum machining conditions for older machines. For that purpose, the control offers one special command - G60 - called the uni-directional approach or single direction positioning .

The command G60 belongs to the G-code Group 00 , which means it is a one-shot command (used only in the block that includes it).

How to use G60? As its purpose is tool positioning - not cutting - it replaces the G00 rapid motion command. Its most common uses are applied to fixed cycles where the distance between hole positions is extremely critical. In fixed cycles, G60 has no effect on the Z-axis motions. Also, in fixed cycles that contain shift from the center (G76 and G87), the single direction positioning does not apply to the shift. Absolute or incremental mode can be used with G60 the same way as with the G00. If mirror image is used, the positioning direction does not change. For the example shown, system parameter setting for the direction is X+Y+, and the amount of overrun as 1 mm (X+1.0 and Y+1.0).