set to ON, the CNC operator has the option to walk around the machine, check if the right tool is ready for tool change and - if necessary - make corrections before the ‘wrong’ tool is actually brought into the spindle.
This is only a small example of how program structure may affect setup. Programmer’s cooperation should not be difficult to secure.
Single Block mode is NOT functional for tapping or threading operations
Block Skip
Block Skip switch is another operation panel feature that requires support in the program. Part program that contains a forward slash symbol (
Some controls use description ‘Block Delete’ instead of the more accurate ‘Block Skip’. Keep in mind that no blocks in the program will actually be deleted - they will be only skipped - they will be bypassed and ignored during program processing when Block Skip switch is ON.
The most common (and often the only) use of block skip function in the part program is as the first character in the block, for example,
/ N76 G91 G28 X0 Y0
... where the XY machine zero return motion can be skipped, if desired.
Some controls allow block skip function in the middle of a block, for example,
N132 S800 M03 / S1200
Be extra careful in such situations and think twice.
In this case, the spindle will rotate at 800 r/min if the block skip switch is ON and 1200 r/min if the switch is OFF. If the control system supports this feature, the actual order of commands in the program is very important - with two conflicting commands - S800 and S1200, it is the latter one that will be processed. Make sure to check if your control system supports this feature.
Note that the placement of M03 function is in front of the slash - the spindle rotation clockwise is common to both situations.
Common Program errors with Block Skip
The problems encountered with block skip function can happen because of the operator’s error:
▪Not activating the Block Skip switch at all
▪Activating the Block Skip switch too late, after the program started processing block with slash
▪Switching to Block Skip switch OFF before all skipped program blocks have been processed
Problems can also be caused by two program errors:
▪Incorrect block skip symbol (/) application
▪Missing modal settings
Of the two problems, missing modal settings are the most common. This is definitely a program error, but a keen operator should be able to detect it. Knowledge of what modal commands are is important, as is the knowledge of what is the effect of various M-functions, particularly M00 and M01 functions.
In part programming, modal commands and functions are those that can be programmed only once and remain active without being repeated in each block. Most - but not all - G-codes are modal. Certain machine functions are also modal. For example, once the spindle speed rotation M03 or M04 is established, it remains in effect.
For both modal G-codes and M-functions, each remains active until either changed (cancelled) by another command or function. As an example, take M03 - spindle rotation CW function. Spindle rotation CW can be cancelled by M04 (rotation CCW function) or M05 (spindle stop function). For G-codes, it is similar. For example, as only one motion command can be active at any given time, it means that commands G00, G01, G02, G03 as well as any other motion command (such as fixed cycles) will cancel each other.
The following example shows the error caused by incorrect use of modal commands in the part program:
| N1 G21 | |
| N2 G17 G40 G80 G90 T01 | |
| N3 M06 | (T01 WORKING) |
| N4 G54 G00 X75.0 Y125.0 S1000 M03 | |
| N5 G43 Z25.0 H01 M08 | |
| N6 G99 G81 R2.0 Z-4.6 P200 F150.0 | |
| ... | |
| ... | |
| N23 G80 Z25.0 M09 | |
| N24 G28 Z25.0 M05 | |
| / N25 G91 G28 X0 Y0 | |
| N26 M01 | |
| N27 T02 | |
| N28 M06 | (T02 WORKING) |
| N29 G54 G00 X75.0 Y125.0 S1200 M03 | |
| ... |
Evaluate the example and see where the problem is. The program structure is not the best, but the program will work well if the block N25 is skipped. Being able to do such an evaluation is part of being a skilled CNC machine operator.
Overall, the program looks OK and will perform well with Block Skip switch turned ON. In this case, the G90 absolute mode programmed in block N2 remains in effect through the whole program and block N25 will be skipped. If the Block Skip switch is turned OFF, all blocks will be processed, including block N25. This block includes optional return to machine zero in both X and Y axes, using G91 incremental method. As there is no G90 repeated for the next tool, the control will remain in incremental mode and the program will cause many problems. The correct block N29 should be:
N29 G90 G54 G00 X75.0 Y125.0 S1200 M03
Further examples in the chapter ‘Trial Cuts’ show the proper usage of block skip to avoid problems related to modal values and other activities.
During program run, make sure the Block Skip mode is selected before the program processes the first block preceded by the slash
Regardless of whether the block skip function is or is not used in the program, the normal setting