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:

Fanuc controls provide several features that can be considered together under the general description special cutting modes . The term 'cutting mode' refers to the status of the control selected for the cutting toolpath. Combined to a table, there are five cutting modes available:

All commands in the G61 to G64 series belong to the same modal G-code group, so one mode cancels another mode. Only one special cutting mode can be in effect at any moment, and all modal commands are cancelled by each other - or brought to normal cutting mode by programming G64.

Exact Stop Check G09 - G61

Commands G09 and G61 are used for the same purpose - to control the positioning accuracy at the end of cutting motions (at sharp corners). The difference between the two commands is modality:

G09 - Exact stop check ... non-modal - effective for one block only
G61 - Exact stop check mode ... modal - remains effective until canceled

Either command can be used to control how the cutting tool approaches the programmed end point. When used in the program, the control system provides a slight deceleration before reaching the contour end point. Both G09 and G61 will cause the control system to check if the cutting tool is positioned exactly where it should be. When the position is confirmed, the next program block will be processed. The illustration shows (greatly exaggerated) the effect of normal cutting and cutting with exact check programmed. Use only when necessary!

Once the exact position has been reached, the control system will automatically accelerate at the beginning of the next block. Exact check (single or modal) is normally programmed for linear motion (G01) as well as circular motions (G02 and G03). It is most effective at sharp corners (intersections), not at tangencies (blend radius), particularly when fast cutting feedrate is used.

A simple 75 _ 50 mm rectangle has four corners, but only three may require the use of exact check command - there is no corner cutting at the beginning and at the end:

Expect a very short delay at each corner, while the G61 command remains in effect. The modal mode G61 is canceled by G62, G63 or G64 commands and no other values are required in the block.

Automatic Corner Override - G62

G62 is another not very common G-code that may come useful under the right circumstances. It is defined as automatic corner override command. The main purpose of G62 is to control the federate for inside corners (sharp inner corners) , when the cutter radius offset is in effect. G62 will force an adjustment to the feedrate, resulting in an improved quality of the surface finish and improves the tool life at the same time. Once activated in the program, the override of inner corners is automatic, until another cutting mode is used (G61, G63, or G64). There are no other values programmed with G62. In terms of contour change, see illustration for the possibilities. There are four types of inner corners that are supported by the G62 command - listed in the direction of cutting motion:

Inner corner between a line and another line ... Line-Line transition
Inner corner between a line and an arc ... Line-Arc transition
Inner corner between an arc and a line ... Arc-Line transition
Inner corner between an arc and another arc ... Arc-Arc transition

Tapping Mode - G63

Feedrate override switch and the feedhold button are not active in the tapping mode G63. In tapping mode, the tool does not decelerate at the contour change point - the next block is processed immediately. There are no other values programmed with G63.

In practical usage, this command can be used when a tapping sequence needs to be programmed the long way - without the benefit of cycles (G74 or G84). Such a sequence will include standard G00 and G01 commands, which can be manipulated during machining operation. G63 command prevents such manipulation, eliminating source of a possible problem. A typical programming example when this mode will be very useful is when the tapping requires different feedrate on the way in than on the way out. This technique is often employed for very small and fine threads, usually less than 0.5 mm pitch. In the example, 0.35 mm pitch will be used, at 700 r/min. The requirement is 80% of the feedrate in, 120% of the normal feedrate out, so G84 cycle cannot be used. Illustration is not necessary.

G90 G54 G00 X50.0 Y60.0 S800 M03 (HOLE LOCATION)

G43 Z4.0 H03 M08 (START POINT AT X50.0 Y60.0 Z4.0)

G63 (TAPPING MODE BECOMES EFFECTIVE)

G01 Z-12.0 F224.0 M05 (FEED-IN AT 80 PERCENT OF FEEDRATE)

Z5.0 F336.0 M04 (FEED-OUT AT 120 PERCENT OF FEEDRATE)

G64 (NORMAL CUTTING MODE - G63 MODE CANCELED)

M05 …

Standard tapping feedrate is 800 r/min _ 0.35 pitch = 280 mm/min . To feed-in at 80%, the federate will be 224 mm/min, and to feed-out at 120%, the feedrate will be 336 mm/min.

Normal Cutting Mode - G64

This is the mode that is used in programming the most often. If you never use other modes listed in this chapter, you may not even need G64. When the power is supplied to the control system, the control starts in the state of 'normal cutting mode' . Normal cutting mode means there are no special conditions required to accommodate single direction positioning, stop check, corner override, or tapping modes. In this case, there is no need to include G64 in the CNC program, unless one of the special cutting mode is used or the programmer chooses to include it. In that case, the G64 should always be included at the program start, along with other initialization commands:

G21

G17 G40 G64 G80 (CUTTING MODE AT THE START)

...

G61 (EXACT STOP CHECK MODE IN EFFECT)

...

<machining uses the exact stop check mode>

...

G64 (CUTTING MODE CANCELS G61 - NORMAL MODE)

...

Including the cancellation at the beginning (G64), the program is guaranteed to start in the normal cutting mode. G64 also cancels all other modal commands (G61, G62, and G63).