390

Locate the alarm block number in the program display and examine the G01 line for ,C or ,R notation.

Verify that the chamfer value after ,C or radius value after ,R is present and is a positive number (e.g., G01 X50. Y50. ,C5. not just ,C).

Check that the chamfer/radius value is not larger than the programmed move distance in either axis—the value must be smaller than the actual linear distance traveled.

Correct the value or remove the chamfer/radius command if not needed, then reset the alarm and restart the program from a safe position.

Always verify tool position before restarting after program edits to prevent crashes.

Identify the current G01 block with ,C or ,R and calculate the absolute move distance in X and Y (or other axes involved).

Verify that the chamfer value is less than both the current block move distance AND the next block move distance—chamfer connects two moves.

Reduce the chamfer/radius size to approximately 80% or less of the smallest move distance involved, or increase the programmed move distances.

Test the edited program in single block or dry run mode to confirm proper execution of the chamfer.

Use feedrate override and rapid override controls during initial test runs.

Check that ,C or ,R is only used in G01 linear interpolation blocks—chamfering is not valid with G02, G03, G00, or canned cycle commands.

Review if tool nose radius compensation (G41/G42) is active and creating interference—temporarily cancel compensation to test if this is the issue.

Canceling compensation requires safe positioning to avoid tool path deviation.

Verify that both the current and next blocks are in the same plane (G17, G18, or G19) and that chamfering is supported in the active plane per your control model.

Separate the chamfer into discrete moves (program the angled cut manually) if the automatic chamfer function cannot resolve the geometric conflict.