Known restrictions

Offset

If the program continues with an offset after block search since it was not fully restarted on the contour, this offset remains valid up to program end and reset. When the program is restarted, the motion continues without offset.

Motion and technology in starting block

If an NC block intended for restart receives motion and technology commands (e.g. N100), only the remaining motion commands are actually executed. All technology commands are only simulated in block N100 (block search mode).

Programing Example

Motion and technology in starting block

N90 X90

N100 X100 S1000 M3 M111

N110 …

If technology commands also require to be executed in real motion, the operator may only continue to move in block search up to the end of block N90 with a covered distance of 100%. This refers to the above example.

Automatic restart

Please note the points below for automatic restart to the contour:

1. Axes are moved backward along a straight line. The starting movement is executed with rapid traverse values (G00). If obstacles occur on the straight line, the operator must carry out a manual repositioning before automatic restart to the contour.
2. If soft gantry is active, the starting movement is executed decoupled for slave axes, i.e. the axes only move in coupled mode after the approach block.
3. An axis swap is then permitted in block search and continues to permit return to the contour if the axes are requested by a request for positions by the interpolator (default setting, not with #CALL AX FAST).
4. Axes which are moved during block search and which are released before switch-over to read mode may not start automatically at the last known position.

In the example below, the B axis is not moved back to position 45 if automatic restart to the contour is selected. The Z axis is not moved either. The C axis is moved correctly to the contour.

Programing Example

Automatic restart

N00 X10 Y20

N10 #CALL AX [B, 4, 3]

N20 B45     (B axis is not considered)

N30 #PUT AX [B]

N40 Z100

N50 #PUT AX [Z]   (Z axis released, cannot be)
                  (restored)

N60 #PUT AX [X,Y]

N70 #CALL AX [X, 1, 1] [Y, 2, 0]     (exchange X/Y)
                                     (considered)

(-Continuation position-)

N100 X100 Y200              (Continue normal processing)

                            (after block search)

M30

If program processing is to continue to the continuation position after an abort using block search, the parameters can be obtained directly from the status data in the PLC (see Section Status data: Access via HLI) . If the block search parameters are specified directly based on the NC program, it must be taken into consideration that contour influencing functions, e.g. tool radius compensation and polynomial smoothing, affect the original target positions and block limits.

Attention

If a program only contains relative G91 positions in the block search section, different positions may be approached in the block search despite a restart of the same program.

It is recommended that at least one absolute position occurs in the block search section of the NC program.

Attention

A homing run G74 is omitted during block search. This may result in different follow-on positions or axis offsets compared to real processing.

Attention

A measurement block G100 {<axis><destination>} is replaced by a linear motion to the target position during block search.

G01 {<axis><destination>}

Therefore, the specified target position is approached as if the probe signal had not occurred during the measurement.

This may result in different follow-on positions of the axes compared to real processing.