041

Navigate to OFFSET SETTING screen and verify the tool nose radius value in the geometry offset register (typically R value for turning or radius value for milling). Compare this value against the smallest internal radius or corner in the programmed path.

Check the program geometry where the alarm occurs. Calculate minimum allowable feature size: internal radius must be greater than tool radius, and corner angles should allow tool clearance. For 90-degree internal corners, tool radius should be smaller than both approach and departure move lengths.

If tool size cannot be reduced, modify the part program to add radius breaks or chamfers at sharp corners, increase internal radii, or split the operation into rough and finish passes with appropriate tool sizes.

Check Parameter 5004 (interference check for G41/G42). If set to 0, interference checking is disabled. Recommended setting is 1 to enable protection. Verify Parameter 5002 bit settings for compensation behavior during interference conditions.

Disabling interference checking (Parameter 5004=0) will allow program execution but may cause part scrapping or tool breakage due to excessive cutting.

Identify the exact N-block number where alarm 041 occurs. Review the three blocks before and after this location for acute angles, sharp corners, or near-parallel moves that change direction by small amounts.

Check Parameter 5003 (compensation mode selection). Bit 0 controls inside/outside corner behavior. Bit 1 controls circular/linear compensation at corners. Try adjusting these settings to change how the control handles corner transitions.

Modify the program by adding transition moves or circular interpolation (G02/G03) with appropriate radii at sharp corners. Alternatively, cancel compensation (G40) before the problem area, execute the tight geometry without compensation, then reactivate G41/G42.

For turning operations with tool nose radius compensation (G41/G42), verify the tool type code in the offset register matches the actual tool geometry (type 0-9). Incorrect tool type causes improper vector calculation at corners.

Verify the D code (milling) or T code offset number (turning) specified in the G41/G42 block corresponds to a valid offset register with non-zero radius value. Navigate to OFFSET SETTING screen and confirm the offset number and radius entry.

Check that the G41/G42 activation move (startup block) has sufficient length. The move distance should be at least 1.5 times the tool radius. If the startup move is too short, insert an additional linear move to provide adequate compensation approach distance.

Verify G41/G42 is not called while already active with a different offset number. Ensure G40 is programmed to cancel compensation before reactivating with different offset. Check for missing G40 before tool changes or offset switches.