285

Identify the N-block number displayed with the alarm and locate that line in your part program.

Check for prohibited commands within the look-ahead section: work coordinate changes (G54-G59), tool length offset changes (G43/G44), coordinate system rotation (G68), or mirror image (G51.1) commands mixed with motion blocks.

Separate incompatible commands by inserting a G09 (exact stop) or M00 (program stop) before the problematic command to force buffer flush.

Adding exact stops will reduce machining speed but ensures proper command execution

Re-run the program from several blocks before the alarm point to verify the correction.

Review the program section before the alarm for active high-speed modes (G05.1, G08 P1) or AI nano smoothing commands.

Check if canned cycles (G81, G83, etc.) or subprogram calls appear after high-speed mode activation without proper cancellation.

Cancel high-speed mode with G05.1 Q0 or G08 P0 before the canned cycle or subprogram call, then re-enable it afterward if needed.

Verify parameter settings for look-ahead (19500 series) to ensure proper high-speed mode configuration for your machine capabilities.

Incorrect look-ahead parameters can cause instability or reduce surface finish quality

Examine the NC code for blocks with 4 or more axes commanded simultaneously, especially if mixing linear (XYZ) with rotary (ABC) axes in complex interpolation.

Check for drastic feed rate changes (F codes) or very short move segments (less than 0.001mm) that may overload the look-ahead processor.

Simplify the toolpath by reducing simultaneous axis moves, smoothing out feed rate transitions, or increasing minimum segment length in your CAM post-processor tolerance settings.

If using a CAM system, increase the chord tolerance and reduce the number of output segments for curved surfaces to prevent micro-segmentation.

Increasing tolerance may slightly affect surface finish on tight radii