501

Press OFFSET button and check work coordinate system offsets (G54-G59). Navigate to CURRENT screen to identify active work offset. Verify offset values against machine setup documentation, especially for the axis indicated in the alarm.

Check tool length offsets (OFFSET > TOOL GEOM or TOOL WEAR screens). Examine offset number called by active H-code or D-code for excessive negative values that would position axis beyond travel limit.

Review MDI or program line that triggered alarm. Calculate actual machine position by adding program coordinate + work offset + tool offset. Compare to negative stored stroke limit in parameter 1321 (axis n, negative side).

Correct erroneous offset values. Reset alarm (RESET button), return axis to safe position using MPG or JOG mode, then rerun program from safe point.

Ensure machine coordinate position is within travel limits before jogging. Use POS > MACHINE display to verify absolute position.

Navigate to SYSTEM > PARAM and set parameter write enable (PWE) bit 1 in parameter 3202 to 1 if modification is needed. Check parameter 1320 bits 0-7 to verify stored stroke check 1 is enabled for the affected axis (bit n must be 0 to enable axis n checking).

Parameter changes require machine builder authorization. Record original values before modification.

Access parameter 1321 (stored stroke check 1 negative limit). Verify the negative limit value for axis n matches machine mechanical travel limits per machine specifications. Typical format: parameter 1321+n contains negative side limit.

If using dual stroke check, verify parameter 1327 (stored stroke check 2 negative limit) and parameter 1326 bit settings. Check parameter 1815 (stroke check selection) to determine which stored stroke set is active.

After parameter verification/correction, power cycle the control (full power OFF/ON) to ensure parameters take effect. Re-establish reference position using zero return (G28) before operation.

Backup all parameters to memory card before power cycle using SYSTEM > PMC > FILE function.

Navigate to POSITION screen and check MACHINE coordinate display for the alarmed axis. Verify actual machine position against parameter 1321 negative limit. If position shows invalid data, reference point return was not completed.

Press RESET, then execute reference point return for all axes (AUTO mode, run G28 X0 Y0 Z0; or manual zero return using REF RETURN button). Confirm absolute position indicators illuminate on control panel.

Ensure no workpiece or fixturing obstructs axis travel to reference point. Use override controls if needed.

Review NC program in EDIT or PROGRAM screen. Search for G90 absolute positioning commands and verify calculated positions. Check for missing G54-G59 work coordinate calls or incorrect incremental G91 move sequences that accumulate beyond limits.

Use CUSTOM > PROGRAM CHECK or dry run with feedrate override at 0% and single block (SBL) active. Monitor POSITION screen machine coordinates to verify program stays within stored stroke limits before actual cutting.

Disable automatic tool changer and spindle during program verification to prevent collisions.