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:

Although included in the title, the G28 command is definitely not special - it is used on a daily basis, virtually in every CNC program. Still, it is described here, along with its related commands, to provide a single reference to all commands related to machine zero return. First, some definitions:

Primary Machine Zero Return - G28

The most common G-code of the four commands listed above is definitely the G28. To a large extent, G30 shares the same characteristics as G28, except it relates to a secondary machine zero, if available. For the record, machine zero is the position of all axes that always remains the same. Machine zero is the master origin of the machine - origin that is specified by the machine manufacturer. Machine zero always has the coordinates of X0Y0Z0. Normally, this position is never changed and is used as a reference point for other required measurements and adjustments, such as work offsets and tool length offset, for example. In order to measure work offset or tool length offset accurately, the measuring process must start from a common point - from a zero - machine zero, that is .

As a command, G28 is different than other G-codes, in the sense that it functions as two commands rolled into one . Once you understand this very basic concept, using G28 will be problem free. The following definition should shed some light on the 'two commands in one' statement:

The meaning of the definition should be clear - the tool motion will indeed terminate at machine zero, but it will take a break along the way - through another location - through an intermediate point. Consider the two G28 versions - one in absolute mode, the other in incremental mode (return along the Z-axis only is shown, where Z0 is the top of part):

G90 G28 Z20.0 ... the tool moves to the position 20 mm above part, then continues to machine zero

G91 G28 Z20.0 ... the tool moves by the distance of 20 mm, then continues to machine zero

This type of program input is also one of the most common. After all, in order to make an automatic tool change, the tool must be located at machine zero for the Z-axis (vertical machining centers) or for the Y-axis (horizontal machining centers). What makes this command sometimes hard to understand is that it does not seem to be necessary, it does not seem to have any purpose. In the two common examples above, that is true. Actually, if the Z-axis alone is used with G28, the motion to the intermediate point is practically useless. In case of two or three axes used simultaneously with G28, the situation is much different. The following example and illustration show the intended use of G28:

…

G90 G00 X14.4 Y9.0 (CURRENT POINT - XY)

Z2.0 (CURRENT POINT - Z)

G01 Z-13.3 F150.0

G28 X14.4 Y9.0 Z2.0 (INTERMEDIATE POINT)

...

Many programmers have wondered at the actual benefits of this command, as it saves only a single block of the program. There is a simple idea behind the G28 command - to bypass obstacles on the way to machine zero when moving two or more axes simultaneously. In a single axis machine zero return, there are no obstacles to consider, so the intermediate point is unnecessary, but it still must be programmed. The solution? The intermediate tool position will be the same as the current tool position.

The previous example will be used with a retract move added:

…

G90 G00 X14.4 Y9.0

Z2.0

G01 Z-13.3 F150.0

G00 Z2.0 (SAFE RETRACT)

G28 X14.4 Y9.0 Z2.0 (INTERMEDIATE POINT)

...

Some programmers prefer to use incremental zero return, with exactly the same effect:

…

G90 G00 X14.4 Y9.0

Z2.0

G01 Z-13.3 F150.0

G00 Z2.0 (SAFE RETRACT)

G91 G28 X0 Y0 Z0 (INTERMEDIATE POINT)

G90 … (REINSTATE ABSOLUTE MODE)

...

The two versions with the safe retract are preferred methods - the G90 method is favored over the G91 version, as there is no need to change the mode. Use G91 only if absolute position is unknown.

Keep in mind that X0Y0Z0 in absolute mode refer to part zero location, X0Y0Z0 in incremental mode refer to no motion , that is a motion that has a zero length. Zero motion during machine zero return applies only to the intermediate point - G91 G28 Z0 simply means that there will be no motion to the intermediate point and the tool will move to machine zero directly. Make sure to include G91 in the block. Both G90 and G91 examples will have the same effect - the Z-axis retract above part is very strongly recommended . The best way to see the effect of this often mysterious command is in the single block mode, where both parts of the zero return motion will be apparent.

Return from Machine Zero - G29

G29 is the virtual opposite of G28 - it's almost that simple. Practical usage of this command is very questionable. While G28 can be described as the return to machine zero from the current tool position through an intermediate point, the G29 is the return from the machine zero to the specified tool position through the last intermediate point . Of course the last intermediate point must be defined first, often for the previous tool. For example, here are all critical blocks for two tools:

… (TOOL 01 WORKING)

G90 G00 X50.0 Y30.0

Z2.0

G01 Z-15.0 F150.0 (TOOL IS BELOW THE PART)

G28 X50.0 Y30.0 Z2.0 (XY IS THE CURRENT POINT THROUGH Z2.0 FIRST)

...

M06 (TOOL 02 WORKING)

...

G90 G29 X75.0 Y40.0 Z2.0 (COORDINATES SPECIFY THE NEW TARGET LOCATION)

...

What will be actually happening at the machine? For the first tool T01, machining will take place at X50.0Y30.0, to the depth of Z-15.0. The tool retracts to Z2.0, and from this location, all three axes return to machine zero (for whatever reason). Now, the next tool T02 is working and G29 specifies target location of X75.0Y40.0 and Z2.0. How the tool will move there is the very purpose of G29. The control will use the last intermediate point (X50.0Y30.0Z2.0), moves the tool to this position first, then moves to the actual target of X75.0Y40.0Z2.0. Why? Honestly, beats me.

The difficulty is not much in the understanding of this command; the difficulty is mainly related to its application. It is much easier to understand a command that is used all the time (G28) when compared with a command that is practically never used (G29). Here is the simple conclusion:

Machine Zero Return Position Check - G27

Although listed first in the table, this G-code can only be truly understood if several other G-codes are understood first, particularly G90, G91, and G92 (or G50 on lathes).

Since the G27 command is listed in this chapter, it belongs to one of those commands seldom – if ever - used in CNC programs. First, its definition in the section title identifies this command as machine zero return position check . This command has no practical purpose in modern programming, but it can be useful to those programmers who still have to program G92 or G50 position registers for some very old control systems (those that do not support work offsets). Details about G92/G50 are described in the next section. For now, just accept the fact that G92 registers the specified XYZ coordinates as the current tool position from part zero - not from machine zero . Here is an example of a typical G27 use in incremental mode:

…

G90 (ABSOLUTE MODE)

G92 X300.0 Y200.0 Z100.0 (CURRENT TOOL LOCATION AT MACHINE ZERO)

G00 X20.0 Y15.0 Z2.0 (START LOCATION FOR CUTTING)

G01 Z-5.0 F120.0 (MACHINE TO ABSOLUTE DEPTH OF 5 MM)

G91 G01 X40.0 F150.0 (MACHINE PART IN INCREMENTAL MODE - CUT ¼)

Y30.0 (MACHINE PART IN INCREMENTAL MODE - CUT 2/4)

X-40.0 (MACHINE PART IN INCREMENTAL MODE - CUT ¾)

Y-30.0 (MACHINE PART IN INCREMENTAL MODE - CUT 4/4)

G00 Z7.0 (RETRACT BY 7 MM)

G27 X280.0 Y185.0 Z98.0 (CHECK IF THE MOTION TERMINATES AT MACHINE ZERO)

...

In the above program, look at the G27 block - it is of special interest. Once the machining has taken place, all axes will move to the position specified in the G27 block, which is the incremental motion to the machine zero, from the current tool position. The big question is - did all axes actually reached the machine zero? Well, upon the block completion, G27 will perform the check, and if the machine zero position has been reached, axes confirmation lights will turn on; if the machine zero position has not been reached, the control will issue an alarm, and no further program processing will be allowed.

Now, let's look at the above example more carefully - will the machine zero lights come on or will there be an alarm?

The best approach to understand G27 is to convert the whole program to absolute mode:

…

G90 (ABSOLUTE MODE)

G92 X300.0 Y200.0 Z100.0 (CURRENT TOOL LOCATION AT MACHINE ZERO)

G00 X20.0 Y15.0 Z2.0 (START LOCATION FOR CUTTING)

G01 Z-5.0 F120.0 (MACHINE TO ABSOLUTE DEPTH OF 5 MM)

G01 X60.0 F150.0 (MACHINE PART IN ABSOLUTE MODE - CUT ¼)

Y45.0 (MACHINE PART IN ABSOLUTE MODE - CUT 2/4)

X20.0 (MACHINE PART IN ABSOLUTE MODE - CUT ¾)

Y15.0 (MACHINE PART IN ABSOLUTE MODE - CUT 4/4)

G00 Z2.0 (RETRACT 2 MM ABOVE PART)

G27 X280.0 Y185.0 Z98.0 (CHECK IF THE MOTION TERMINATES AT MACHINE ZERO)

...

Write down the last positions of XY and Z - they are usually in two blocks, just before the G27 command - they are X20.0 Y15.0 Z2.0. Next, subtract each position from the respective axis in the G92:

X200.0 - 20.0 = X280.0 Y100.0 - 15.0 = Y185.0 Z100.0 - 2.0 = Z198.0

This example is correct, G27 will confirm that machine zero has been reached in all three axes.

Using G27

G27 should always be used in the G40 mode (cutter radius offset canceled), otherwise the tool will not be confirmed at machine zero. Also watch for cases when the machine lock switch is turned on, for example, during program verification. In this case, there will be no machine zero check performed. If you find a practical application for this command, you can use it for both mills and lathes with same logical approach. Programs written in incremental mode (G91) benefit the most from this G-code. Under normal situation, use G28 in order to return to machine zero - the position checking is already built in and it is a much more convenient way of programming.

Secondary Machine Zero Return - G30

Most vertical machines have only one machine zero. One machine zero is always the primary machine zero, as there is no other choice. Some horizontal machining centers - particularly those used with pallet changers - often need a secondary machine zero location, in order to align two independent pallets, for example. The applications for both G28 and G30 are exactly the same - in order to return to the primary machine zero, use G28; in order to return to the secondary machine zero, use G30. All other conditions listed under the G28 heading apply equally to G30. Third and fourth machine zero commands are also available on some controls, but rather rare.