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:

Another practical, but rarely used and optional feature of the CNC system is the definition of special zones that the tool can enter (allowed) or those that the tool cannot enter (disallowed) :

The definition of custom limits for a three-axis machining center is specified by diagonally opposed coordinate points, consisting of three axes, and resulting in a box - rectangular areas for CNC lathes are based on the same principle. For any machine, the specially defined zone establishes the required boundary. Control system parameter determines whether the selected zone will be protected internally (inside the boundary) or externally (outside the boundary). For example, parameter 1300 , bit #0 is used for this purpose on Fanuc 16-18-21 controls (additional parameter settings may also apply).

The programming format for the G22 command is:

G22 = Stored stroke limits activated                 ... defined zone

XYZ = Start point of the limited area                  ... measured from machine zero

IJK = End point of the limited area                     ... measured from machine zero

The active units of measurement are used as input values. G23 cancels the stored stroke check and is programmed by itself in a block. No more checking will be performed after the G23 command. There are two important conditions to be satisfied when specifying the G22 corner values:

The shaded area in the illustration above identifies the prohibited zone.

G21

G17 G23 G40 G80

G22 X-150.0 Y-75.0 K-100.0 I-280.0 J-175.0 K-125.0        (STROKE CHECK ON)

G90 G54 G00 X.. Y.. S.. M03

…

<machining with stored stroke check active>

...

G23                                                                                (STROKE CHECK OFF)

Can you tell how large zone has been selected for protection in the program above? It should be easy: 130 mm along X-axis, 100 mm along the Y-axis, and 25 mm along the Z-axis. Just take the difference between X-I, Y-J, and Z-K amounts in the G22 statement. Before any programmed tool motion attempts to enter the forbidden zone, the control system issues an alarm and stops further program processing before the tool enters the prohibited zone. The most common use of this feature is to program a protective zone around fixtures, during multi-part setups and other undesirable items that may be in the way of toolpath (even part of the current work may be defined as prohibited).

There is a rather good reason why this apparently powerful control feature has not been commonly used. The main reason is that it's just not powerful enough ; mainly when working with tool length and radius offsets. Neither offset is evaluated during the stroke check, because all the command does is following the XYZ motions. Also, in practice, it is not always easy to actually establish the zone that is to be protected by the program, particularly when programming away from the machine.

G23 cancellation command stands on its own - it does not accept any arguments and must be programmed in a separate block. One final word of caution:

Copyright © 2006 Industrial Press Inc.