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:

I n the earlier section describing the G27 command, a small example of the G92 command was presented. On the lathes, the most common equivalent command is G50. Both these commands are considered obsolete by any modern standards - they have been replaced by the much more flexible work offsets G54-G59. The reason there is at least a miniature version of these commands described here, came from the many requests to cover this feature for the users who still work with older controls.

All machines that support work offsets also support G92, mainly for the compatibility with older programs. This statement - while correct - also requires a word of caution first:

Yes, it is possible to mix work offsets with position register commands in the same program, but it can cause more headaches than it's worth. The most common definition for G92/G50 is position register command . What does it really mean? Keep in mind these commands are dated before any work offsets existed, although the G43 command for tool length offset was already available. While work offset is always measured from machine zero to part zero along an axis (usually as a negative dimension), position register is measured from part zero to machine zero (usually as a positive dimension). That is an important difference, but not really the major difference between the two methods of coordinate setting. The major difference is in the respective applications of both command types:

• Position register G92/G50 is set in the program for each tool

…actual dimensions for each axis must be known during program development

• Work offsets G54-G59 are set at the machine and only called by the program

…actual dimensions are not known during program development

• Tool length offset G43 is set in the program for both G92 and G54-G56 (mill controls only)

... actual dimensions are not known during programming

In summary, there is only one - and only one - reason for either G92 or G50 command in the program:

G92 X195.0 Y88.0 Z20.0 (POSITION REGISTER COMMAND - THREE AXES SELECTED)

In this block, the programmed data 'tell' the control that the tool current position is located 195 mm from the part zero along the X-axis, 88 mm along the Y-axis, and 20 mm along the Z-axis.

The major problem with position register commands is the fact that for most setups, the programmer has no way of knowing where exactly the tool is located. In order to make this feature work, several rather elaborate methods have been devised, to shorten the setup time. Programmers soon found out that it is easier to leave the G92 block in the program empty and let the operator to fill-in the data, based on actual setup. However, this method had only been possible when software based CNC systems replaced the hardwired NC systems. Of course, work offsets have solved this problem for all but those users who still have no choice but to program in the very old fashioned way.

G92 Position Register for Milling

Some older CNC lathes also accept G92 as the position register command, but generally G92 is used for milling, while G50 is used for turning. The best way to illustrate the G92 command is to use it in a program with two tools and follow its settings from one tool to the next. The illustration below shows top and front setup of a simple part. Note the arrow directions and the dimensions required by setup.

A suitable spot drill and a _ 5 mm drill will be programmed to machine the two holes shown. The first tool - spot drill - starts from machine zero. This position is a normal start for any first tool, because the machine has to be zeroed for every setup at startup. When the tool is located at machine zero, the CNC operator must set the part zero exactly 300 mm along the X-axis and 200 mm along the Y-axis. These are the main conditions of G92 command - this is how G92 works!

Based on extensive experience of many users, this setup task is virtually impossible to do at the machine, with any degree of precision - at least in a reasonable time frame. However, that was - and still is, if necessary - the main drawback of G92.

The following programming example is based on the provided setup, including both tools, with appropriate comments:

N1 G21

N2 G17 G40 G80 G90 T01

N3 M06 (SPOT DRILL)

N4 G92 X300.0 Y200.0 Z0 S1200 M03 T02 (CURRENT TOOL AT MACHINE ZERO)

N5 G00 X20.0 Y15.0 (FIRST HOLE LOCATION)

N6 G43 Z10.0 H01 M08 (TOOL 10 MM ABOVE WORK)

N7 G92 Z10.0 (CURRENT TOOL POSITION REGISTERED)

N8 G99 G82 R2.0 Z-2.75 P200 F120.0 (SPOT DRILL AT CURRENT LOCATION)

N9 X80.0 Y45.0 (SECOND HOLE LOCATION)

N10 G80 Z10.0 M09 (CYCLE COMPLETED)

N11 G28 Z10.0 M05 (ONLY Z-AXIS TO MACHINE ZERO)

N12 M01

After the first tool in the program (T01 is the spot drill in the example) completes the machining operation, the location of th T01 is critical within G92 environment and must always be known. Based on the program developed so far, the tool T01 is located at X80.0 Y45.0, when block N12 is processed. The tool T01 is also located at machine zero in the Z-axis.

The illustration at right shows the current tool position of T02, which replaced tool T01 during automatic tool change.

Following the normal rules, G92 command data must contain the current tool location - as it relates to part zero. In this programming example, the second tool T02 is located exactly at the same XY position as the previous tool T01, so no special programming effort is necessary. If G92 for the X and Y coordinates is used in the program, its values will be:

G92 X80.0 Y45.0 Z0 (CORRECT BUT UNNECESSARY SETTING)

The remainder of the program can now be written, considering the settings described so far:

N13 T02

N14 M06 (5 MM DRILL)

N15 G90 G92 Z0 (CANCEL Z-AXIS SETTING)

N16 G00 G43 X80.0 Y45.0 Z10.0 H02 M08 (MOVE TO SECOND HOLE 10 MM ABOVE)

N17 G92 Z10.0 S1350 M03 (CURRENT TOOL POSITION REGISTERED)

N18 G99 G81 R2.0 Z-12.5 F150.0 (DRILL AT CURRENT LOCATION)

N19 X20.0 Y15.0 (FIRST HOLE LOCATION)

N20 G80 Z10.0 M09 (CYCLE COMPLETED)

N21 G28 Z10.0 M05 (ONLY Z-AXIS TO MACHINE ZERO)

N22 G28 X20.0 Y15.0 (=> WHAT IS THE G92 AT THIS BLOCK?)

N23 M30

Of course, the comment in block N22 is unnecessary, but included here anyway - what is the current tool position? Since the current tool T02 is located at machine zero, it means it is located 300 mm and 200 mm respectively, along the X and Y axes - from part zero. The Z-axis is the original setting as determined by the tool length.

G50 Position Register for Turning

The G50 command shares most programming features with its G92 cousin - its definition, its purpose, and its method of programming. The only visible difference in the program is the axes designation as X and Z rather than X, Y and Z. Although an obsolete command, many older programs do contain this type of tool setting and still use it. The part programmer should convert the program to the modern method, which is very easy - just eliminate the G50 X.. Z.. reference. For those who still need to work with the G50 position register, here is an example that should make its use clearer.

To illustrate the G50 concept, a simple drawing shown at right will be used for the example. For actual machining, three typical and unique tools will be selected, to show the various G50 relationships:

T01 = 80 _ Turning tool

T02 = _ 18 mm Drill

T04 = _ 16 mm Boring bar

For simplicity (and better clarity), only the necessary toolpath will be covered in the program. Facing and center-drilling operations have been skipped. Spindle speeds and cutting feedrates are only reasonable and not important at this time.

Tool Change Position

During tool change, it is quite common on a CNC lathe to move the current tool to a safe position away from the part, but not necessarily to machine zero. A variation on the same topic will be a tool change at machine zero in the X-axis only - but close to the part in the Z-axis. The main reason is that the X-axis travel is much shorter than the Z-axis travel on most machines. Also, this method adds to the safety aspects of the automatic tool change process by adding additional clearance. This is also the programming method used in the examples provided in this chapter.

The above safety message applies to any type of lathe programming, not just when the G50 is used.

Initial Data

Unlike the modern programming method, using G50 means using several dimensions known to the part programmer. These dimensions relate to the CNC lathe itself, as well as to all tools used in the program. The schematic illustrations on the next page show dimensional data for the CNC lathe used for this example, with attached chuck, jaws and turret without and with tools. The dimensions used are realistic but not to scale , and are always known from the data supplied by the lathe manufacturer.

The first piece of the 'puzzle' defines the fixed machine dimensions provided by the manufacturer, when the empty tool turret is located at machine zero. If the Z-dimension is given to the chuck face, just add the width of the standard jaws for all related calculations. The width of the part is included in the illustration as part of the current setup, not part of the machine specifications.

When the cutting tools are mounted in the turret, their d imensions must also be known to the CNC programmer. This is the program section that makes the G50 programming method very inconvenient and perhaps even hard in some opinions (by today's standards).

As there are three tools used by the program, the critical dimensions of each tool must be known before the actual program can be written. The illustration above shows the critical dimensions for tool T01 (turning tool) that are important to the overall setup and related program development.

The remaining two illustrations that follow show the equivalent critical dimensions - also known when the program is written - for the other two tools used by the program. Note that the data for all three tools listed are dimensioned from machine zero, and their X/Z dimensions are always known.

From the CNC programmer's viewpoint, once the individual tool dimensions are known relative to the provided machine and part dimensions, the program using the position register command G50 can be written and used for tool change at any reasonable location.

Tool Change Position

It is not necessary to return to machine zero after each tool has completed its work. The travel can be unnecessarily long, particularly along the Z-axis. That means the programmer has to select a tool change position for each tool. The basic rule (as defined earlier) is to make sure that the minimum clearance is applied to the longest tool. If the longest tool has enough clearance, every other tool will have even more clearance.

For the purposes of comparison, this example will be presented in two stages - in the first stage, each tool change will be at machine zero (easier but less efficient), the second stage will show how the tool change can be done close to the part in Z-axis (the shorter X-axis will still be done at machine zero position).

Tool Change at Machine Zero

In this case, the longest tool length is not important, as machine zero position is a fair distance from the part. The following program is listed in the order of described tools - T01, T02, T04:

N1 G21 (METRIC UNITS)

N2 T0100 (TOOL 01 LOCATED AT MACHINE ZERO)

N3 G50 X160.0 Z303.0 (O.D. TOOL TIP POSITION FROM PART ZERO)

N4 G96 S120 M03 (SPINDLE SPEED AND ROTATION)

N5 G00 G42 X52.0 Z3.0 T0101 M08 (CHAMFER START POINT)

N6 G01 X58.0 Z-1.0 F0.125 (FRONT CHAMFER)

N7 Z-25.0 F0.3 (OUTSIDE DIAMETER CUTTING)

N8 X63.0 (FACE CUTTING)

N9 X67.0 Z-27.0 F0.125 (REAR CHAMFER)

N10 U5.0 F0.5 (CLEARANCE RETRACT)

N11 G00 G40 X160.0 Z303.0 T0100 (RETURN TO THE MACHINE ZERO POSITION)

N12 G27 X160.0 Z303.0 (CHECK IF THE TOOL IS AT MACHINE ZERO)

N13 M01 (OPTIONAL STOP)

N14 T0200 (TOOL 02 LOCATED AT MACHINE ZERO)

N15 G50 X160.0 Z263.0 (DRILL TIP POSITION FROM PART ZERO)

N16 G97 S900 M03 (SPINDLE SPEED AND ROTATION)

N17 G00 X0 Z5.0 T0202 M08 (START LOCATION FOR DRILLING)

N18 G01 Z-47.0 F0.375 (END LOCATION FOR DRILLING)

N19 G00 Z5.0 (RETURN BACK TO START LOCATION)

N20 X160.0 Z263.0 T0200 (RETURN TO THE MACHINE ZERO POSITION)

N21 G27 X160.0 Z303.0 (CHECK IF THE TOOL IS AT MACHINE ZERO)

N22 M01 (OPTIONAL STOP)

N23 T0400 (TOOL 04 LOCATED AT MACHINE ZERO)

N24 G50 X182.0 Z267.0 (BORING BAR TIP POSITION FROM PART ZERO)

N25 G96 S110 M03 (SPINDLE SPEED AND ROTATION)

N26 G00 G41 X30.0 Z3.0 T0404 M08 (CHAMFER START POINT)

N27 G01 X22.0 Z-1.0 F0.125 (FRONT CHAMFER)

N28 Z-42.0 F0.25 (INSIDE DIAMETER CUTTING)

N29 U-5.0 (CLEARANCE RETRACT)

N30 G00 Z3.0 (RETRACT FROM THE HOLE)

N31 G40 X182.0 Z267.0 T0400 (RETURN TO THE MACHINE ZERO POSITION)

N32 G27 X182.0 Z267.0 (CHECK IF THE TOOL IS AT MACHINE ZERO)

N33 M30 (END OF PROGRAM)

Note the inclusion of G27 command - it checks if the current tool position is actually at machine zero. In a way, the command in this program is redundant, but at least it brings some piece of mind - for example, if there is an error in the data input (data entry error). The G27 command has been described earlier in this chapter.

Tool Change Close to the Part

When the tool change takes place close to the part, the longest tool length is important. In the example used, the longest tool is the drill, with 47 mm overhang. The programmer selects any suitable clearance - for the example, 50 mm Z-clearance will used for the longest tool (T02). That means a very special care must be taken to program the G50 coordinates for all other tools. When the G50 method was the only method available to establish the current tool position, this particular reason was the weakest point of the whole concept. CNC programmers often resorted to the method of returning all tools to machine zero when each operation was completed. Convenience won over efficiency.

As the tool does not return back to the machine zero position, there is no need for the G27 command in this version. Although only the Z-clearance is shown, X-clearance will work the same way.

The last program will not change in any way that relates to the toolpath and cutting conditions. Only the G50 will change, based on the current tool position. Watch the underlined settings carefully - even when combined with the illustrations, this subject may take a while to fully understand. The most difficult part of this programming method is to determine the G50 position of the next tool, relative to the position of the current tool. For safety reasons, tool change position of any tool must be at least 50 mm away from the front face of part, that is from Z0. The result is a guarantee that no tool will be located behind the chuck during tool change, causing a possible collision.

In a summary, each tool will make a tool change at the exact location of the longest tool. However, because the length of each tool is different, the G50 Z-setting will also be different to maintain this minimum clearance position.

The calculation of the G50 at the tool change position of any tool considers the known settings:

For the first tool, the formula can be used with exact dimensions:

G50 = 303 _ 263 _ 50 = 90 = G50 X.. Z90.0

The longest tool (T02) total distance is 263 mm, and the clearance from Z0 for that tool is 50 mm. The program for the first tool still originates at machine zero, but terminates at a Z90.0 tool change position:

N1 G21 (METRIC UNITS)

N2 T0100 (TOOL 01 LOCATED AT MACHINE ZERO)

N3 G50 X160.0 Z303.0 (O.D. TOOL TIP POSITION FROM PART ZERO)

N4 G96 S120 M03 (SPINDLE SPEED AND ROTATION)

N5 G00 G42 X52.0 Z3.0 T0101 M08 (CHAMFER START POINT)

N6 G01 X58.0 Z-1.0 F0.125 (FRONT CHAMFER)

N7 Z-25.0 F0.3 (OUTSIDE DIAMETER CUTTING)

N8 X63.0 (FACE CUTTING)

N9 X67.0 Z-27.0 F0.125 (REAR CHAMFER)

N10 U5.0 F0.5 (CLEARANCE RETRACT)

N11 G00 G40 X160.0 Z90.0 T0100 (RETURN TO THE TOOL CHANGE POSITION)

N12 M01 (OPTIONAL STOP)

The second tool - T02 - is also the longest tool, therefore its G50 Z.. must be G50 Z50.0. The formula listed above applies equally for this tool as well:

G50 = 263 _ 263 _ 50 = 50 = G50 X.. Z50.0

The program listing for the second tool shows the setting at the program beginning (block N14) and the return motion block N19, using the same coordinates.

N13 T0200 (TOOL 02 LOCATED AT TOOL CHANGE POSITION)

N14 G50 X160.0 Z50.0 (DRILL TIP POSITION FROM PART ZERO)

N15 G97 S900 M03 (SPINDLE SPEED AND ROTATION)

N16 G00 X0 Z5.0 T0202 M08 (START LOCATION FOR DRILLING)

N17 G01 Z-47.0 F0.375 (END LOCATION FOR DRILLING)

N18 G00 Z5.0 (RETURN BACK TO START LOCATION)

N19 X160.0 Z50.0 T0200 (RETURN TO THE TOOL CHANGE POSITION)

N20 M01 (OPTIONAL STOP)

When the original drawing was presented and three tools had been selected, there was a good reason for such a selection. In terms of the program structure, every first tool of the program represents program formatting at beginning (of the first tool), every second tool represents the formatting for all tools between the first one and the last one (the second tool), and the third tool represents the last tool format.

When this method is applied to the G50 X.. Z.. position register command, the original intent remains the same - the G50 for any middle tool (all tools after the first and before the last) will start and end at the same position - see above illustration.

The last tool (see program and illustration on the next page) is always treated somewhat differently, and programmer's preferences may not work here very well. When the last tool has completed all machining, the programmer may choose to return the tool to the tool change position, as any previous tool - this is a wrong decision . Returning the tool to a position other than machine zero means inconsistency between the position of the last tool for one part, and the position of the first tool for the next part. Since the program is written in such a way that the first tool starts from machine zero, the last tool must return to the same position - that means to machine zero. The suggestion is simple:

Based on the explanation for programming the first and last tool, the boring bar (T04) - the last tool from the example - can be programmed.

N21 T0400 (TOOL 04 LOCATED AT TOOL CHANGE POSITION)

N22 G50 X182.0 Z54.0 (BORING BAR TIP POSITION FROM PART ZERO)

N23 G96 S110 M03 (SPINDLE SPEED AND ROTATION)

N24 G00 G41 X30.0 Z3.0 T0404 M08 (CHAMFER START POINT)

N25 G01 X22.0 Z-1.0 F0.125 (FRONT CHAMFER)

N26 Z-42.0 F0.25 (INSIDE DIAMETER CUTTING)

N27 U-5.0 (CLEARANCE RETRACT)

N28 G00 Z3.0 (RETRACT FROM THE HOLE)

N29 G40 X182.0 Z267.0 T0400 (RETURN TO THE MACHINE ZERO POSITION)

N30 G27 X182.0 Z267.0 (CHECK IF THE TOOL IS AT MACHINE ZERO)

N31 M30 (END OF PROGRAM)

Only the last tool returns to the machine zero position, so the G27 command is justified, if required.

Conversion of G50 to Geometry Offset

Although the word 'conversion' in the title may seem a bit overstated (there is no actual conversion), how do we change a program listing that contains G50 to the modern method of programming, using Geometry and Wear offsets? Simple - take the G50 and its related blocks out of the program altogether. Here is the same program as listed above, but using the modern method - no G50 at all . Study it carefully, particularly the tool position at the end of each tool - it offers a reasonable position to provide a clearance for the tool change, considering all tools.

N1 G21 (METRIC UNITS)

N2 T0100 (TOOL 01 LOCATED AT MACHINE ZERO)

N3 G96 S120 M03 (SPINDLE SPEED AND ROTATION)

N4 G00 G42 X52.0 Z3.0 T0101 M08 (CHAMFER START POINT)

N5 G01 X58.0 Z-1.0 F0.125 (FRONT CHAMFER)

N6 Z-25.0 F0.3 (OUTSIDE DIAMETER CUTTING)

N7 X63.0 (FACE CUTTING)

N8 X67.0 Z-27.0 F0.125 (REAR CHAMFER)

N9 U5.0 F0.5 (CLEARANCE RETRACT)

N10 G00 G40 X150.0 Z100.0 T0100 (RETURN TO A SAFE TOOL CHANGE POSITION)

N11 M01 (OPTIONAL STOP)

N12 T0200 (TOOL 02 LOCATED AT TOOL CHANGE POSITION)

N13 G97 S900 M03 (SPINDLE SPEED AND ROTATION)

N14 G00 X0 Z5.0 T0202 M08 (START LOCATION FOR DRILLING)

N15 G01 Z-47.0 F0.375 (END LOCATION FOR DRILLING)

N16 G00 Z5.0 (RETURN BACK TO START LOCATION)

N17 X150.0 Z50.0 T0200 (RETURN TO A SAFE TOOL CHANGE POSITION)

N18 M01 (OPTIONAL STOP)

N19 T0400 (TOOL 04 LOCATED AT MACHINE ZERO)

N20 G96 S110 M03 (SPINDLE SPEED AND ROTATION)

N21 G00 G41 X30.0 Z3.0 T0404 M08 (CHAMFER START POINT)

N22 G01 X22.0 Z-1.0 F0.125 (FRONT CHAMFER)

N23 Z-42.0 F0.25 (INSIDE DIAMETER CUTTING)

N24 U-5.0 (CLEARANCE RETRACT)

N25 G00 Z3.0 (RETRACT FROM THE HOLE)

N26 G40 G28 U0 W0 T0400 (RETURN TO THE MACHINE ZERO POSITION)

N27 M30 (END OF PROGRAM)

Summary

In a summary, the G50 command is very impractical and inefficient but it reflect the progress of its time - yes, it was a great progress, in spite of the appearances. Its main disadvantage is quite obvious - many dimensions must be known to the part programmer at the time of program development, which creates a situation not always practical or even possible. Repeating a tool is often very difficult and the whole concept is prone to many errors. Yet, millions of parts have been machined with the G50 used in the program.