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:

Of course, the words 'rarely' and 'seldom' are very subjective and rather relative. A preparatory command listed here as 'seldom used' may be used daily by some programmers. The opposite is true as well - commands not listed in this chapter are considered common - or at least more common - yet, some programmers may not use them at all.

In this conclusion of the 'special' G-codes subject, just a few brief notes relating to those G-codes that could be listed here but were not:

Tool Length Offset Negative - G44

It is virtually impossible to consider G44 without considering the related command G43. Let's look at their standard definitions first:

The G44 command is (almost) never used in daily CNC programming. Think of the G44 command as the exact opposite of G43 command, and at the same time think of some reasonable and practical applications for this command - most likely, you will find none. In order to use G44 over G43, there must be a benefit that is not found in the G43 application - then the G44 may be justified..

Tool Length Offset Cancel - G49

This is one command that asks a simple question - to use it or not to use it ? It has its firm adherents and its equally determined opponents - both camps claim that their approach is better. Without prejudice, let me state this - you programmers in both camps are right - up to a point, at least. In that respect, G49 becomes a rather strange command, perhaps even a bit foggy. Its single purpose is also a simple purpose - to cancel the tool length offset , initialized by the G43 (or G44) command, usually programmed at the beginning of each tool. So what is all the fuss about?

A lot depends on the part program itself - how it is written, particularly in terms of its structure. Program structure determines the order and placement of various commands and functions within the program body at the most convenient locations, particularly before and after the many machining sequences. In my CNC Programming Handbook , I have promoted a program structure that has been proven to work for the majority of programming situations. Here is its generic format:

G21

G17 G40 G80 T01

M06

G90 G54 G00 X.. Y.. S.. M03 T02

G43 Z2.0 H01 M08

G01 Z-... F…

<... machining commands ...>

G00 Z2.0 M09

G28 Z2.0 M05

M01

No G49 at all. Why? Because the program structure is designed to allow its omission. What is a seldom known fact is that the G28 (machine zero return) command automatically cancels the tool length offset. This statement should satisfy the opponents of programming G49. I plead guilty here.

Like a coin with two sides, there are also two sides of this argument, and fair is fair. If you wish to include the G49 in the part program, why not? Go for it. The above structure can be modified in two places, just by adding the G49 command:

N1 G21

N2 G17 G40 G49 G80 T01 (G49 USED)

N3 M06

N4 G90 G54 G00 X.. Y.. S.. M03 T02

N5 G43 Z2.0 H01 M08

N6 G01 Z-5.0 F…

<... machining commands ...>

N27 00 Z2.0 M09

N28 G49 G28 Z2.0 M05 (G49 USED)

N29 M01

If that is not much ado about nothing , then what is? While both approaches are very acceptable, and the program structure is followed - where is the catch? There is none - providing the structure is followed! The most important part of the program structure is the call of G43, before the machining sequences take over. Now consider this - what will happen if the G43 block is forgotten, simply missing for the next tool. It should not happen, but what if it does happen? There are two possibilities:

Possibility #1 ... G49 is used in the program

Possibility #2 ... G49 is not used in the program

Going from one tool to another within a single program always means repeating many commands, even if they are modal. This is a very worthwhile practice and saves many headaches later. So, here is a program structure for two tools, where G49 is used, but G43 is 'forgotten' for the second tool:

(=== G49 IS USED IN THE PROGRAM ===)

N1 G21

N2 G17 G40 G49 G80 T01 (G49 USED)

N3 M06

N4 G90 G54 G00 X.. Y.. S.. M03 T02

N5 G43 Z2.0 H01 M08

N6 G01 Z-5.0 F…

<... machining commands for T01 ...>

N27 G00 Z2.0 M09

N28 G49 G28 Z2.0 M05 (G49 USED)

N29 M01

N30 T02

N31 M06

N32 G90 G54 G00 X.. Y.. S.. M03 T03

<... missing G43 block … > (N33 G43 Z2.0 H02 M08 missing )

N34 G01 Z-5.0 F…

<... machining commands for T02 ...>

N52 G00 Z2.0 M09

N53 G49 G28 Z2.0 M05 (G49 USED)

N54 M01

Apart from a relatively minor problem of losing the coolant function, the consequences of the G43 omission for the second tool are far more severe. This is what will happen (correct setup is assumed) for Possibility #1 (G49 is used in the program):

G49 IS Programmed

The first tool will machine the part just fine. Then, the next tool - T02 - is brought into the spindle and moves to the first XY location. So far, all goes as planned. The block after N32 should be G43 block, etc., - but that block is missing! There will be no alarm, no message - no notification whatsoever - in fact, there will be no warning . The control system will simply interpret the Z-axis motion in block N34 as originating from machine zero - there is no tool to be considered, there is no tool length to be considered. Because of that, the point at the spindle gage line (spindle reference point at machine zero) will act as the tool tip and will try to move to the Z-5.0 location. That may not present a problem, if the spindle were empty . Of course, that is not the case at all - the spindle is not empty - there is a real tool - set and designated as T02 - and this tool has a length that reaches far below the spindle gage line. Situations such as this one provide good reasons for real worries, because without an alert reaction of the CNC operator, a disaster is ready to strike.

G49 IS NOT Programmed

What about the other alternative - the one where G49 is not included in the program? Is it a better alternative? Does it solve the problem? Should you prefer it?

Evaluate the following program - it is the same one as above, but no G49 is programmed.

(=== G49 IS NOT USED IN THE PROGRAM ===)

N1 G21

N2 G17 G40 G80 T01

N3 M06

N4 G90 G54 G00 X.. Y.. S.. M03 T02

N5 G43 Z2.0 H01 M08

N6 G01 Z-5.0 F…

<... machining commands for T01 ...>

N27 G00 Z2.0 M09

N28 G28 Z2.0 M05

N29 M01

N30 T02

N31 M06

N32 G90 G54 G00 X.. Y.. S.. M03 T03

<... missing G43 block … > (N33 G43 Z2.0 H02 M08 missing)

N34 G01 Z-5.0 F…

<... machining commands for T02 ...>

N52 G00 Z2.0 M09

N53 G28 Z2.0 M05

N54 M01

To answer the earlier questions - yes, this is a better alternative to the previous version, and no, it does not solve the problem. Whether you should prefer this version largely depends on the major consideration, described next. Don't make too many assumptions here and don't think that all is clear - the situation is still potentially dangerous, but a lot less dangerous than in the previous example. How much is less? Actually 50% less - and here is why.

Again, the first tool will perform flawlessly, as before. This time, there is no G49 tool length cancellation transferred to the next tool (T02), so the current tool length will still be in effect. In this case, the tool length offset for the tool T02 will be exactly the same as the tool length offset for tool T01. Not exactly an ideal situation, but a situation that has a chance to succeed.

The benefit of not programming the G49 is based on the rather dubious chance of 50/50 in case of a program error. If the actual physical length of T02 is shorter the actual physical length of T01, no collision will take place - and no machining will take place either. Of course, this is not the expected activity, but at least it is an activity that does no harm. Corrections to the program still have to made, but under friendly overall conditions.

If the program does include G49 and the situation is equal to the one described, the potential for a

collision is much greater. Please, do not make the mistake of thinking that 50/50 chance is better - it

is not. Both examples create problems and are potentially dangerous situations. The focus of this section

was to come to a single conclusion:

As you see from the demonstration, even an apparently insignificant missing of a single G-code often

makes a great difference in the final results. So what is the moral of this section … ?

Conclusion

Other G-codes can be added to this chapter, depending on the exact interpretation of the term 'seldom used G-codes' . In my CNC Programming Handbook , subtitled A Comprehensive Guide to Practical CNC Programming , most G-codes were explained in great detail, such as coordinate rotation G68 and G69, data input G10, scaling commands G50 and G51. Also included were some G-codes that are not used very often or not used any more, such as position compensation codes G45 through G48. Fanuc Macro B related G-codes G65 through G67 and the whole subject of macros are covered in a separate book, Fanuc CNC Custom Macros , with the subtitle Programming Resources for Fanuc Custom B Users . Both books have been published by Industrial Press, Inc., New York, NY, USA.

In this handbook, a special chapter has been set aside for the plane selection commands G17 through G19, containing many details, techniques and special applications.