325

Review the NC program and identify the sequence number referenced in the alarm. Locate the shape program (subprogram) called by the multiple repetitive cycle (G70-G76 for turning, G71-G73 for milling).

Examine the shape program line-by-line for prohibited commands: M-codes (especially M00-M09, M98/M99), T-codes with offset changes, G04 dwell, G10 programmable data setting, G50/G92 coordinate system setting, G54-G59 work coordinate selection, or any canned cycles (G70-G89).

Remove all prohibited commands from the shape program. Move spindle, coolant, and tool change commands to the main program before the repetitive cycle call. Ensure the shape program contains only G00, G01, G02, G03 motion commands defining the finishing geometry.

Do not include feedrate changes (F-code) that drastically differ from the cycle's programmed feedrate, as some controllers restrict this.

Verify parameter 5101 bit 0 (OGC) and parameter 5102 settings for G-code system compatibility. Check parameter 14880-14889 (multiple repetitive cycle settings) to confirm shape program restrictions for your specific FANUC series and software version.

Verify the multiple repetitive cycle syntax in the main program. For G71 type A (turning), confirm P-address specifies the start sequence number and Q-address specifies the end sequence number of the shape program. For G70-G73, check that the shape program is properly defined between these sequence numbers.

Check if the shape program contains M98 subprogram calls. Remove any subprogram calls from within the shape program and flatten the geometry into a single continuous profile definition. Subprogram nesting is not supported within multiple repetitive cycle shape definitions on most FANUC 0i/16i/18i systems.

Verify the shape program does not contain M99 return command within its body (only at the end if structured as a separate subprogram). Ensure proper program flow with correct sequence number ordering (N-numbers) between P and Q addresses.

Check parameter 5143 bit 3 (MCL) which controls whether multiple repetitive cycles allow certain extended commands. If available on your system, toggle this parameter and test. Always create a parameter backup before modification via SYSTEM > PARAM > [Write Enable] > PWE parameter setting.

Changing parameter 5143 may affect other cycle behaviors. Document original value before modification.

Review the shape program for G00 rapid traverse commands. Some multiple repetitive cycles (particularly G71/G72) require only G01/G02/G03 feed moves in the profile definition. Replace G00 with G01 at appropriate feedrate if the geometry requires linear positioning.

Verify that only the axes controlled by the repetitive cycle are programmed in the shape program. For G71 turning cycle, ensure only X and Z axes are commanded. Check parameter 1006-1008 (axis configuration) and parameter 1020 (number of controlled axes) via SYSTEM > PARAM > [Parameter Number Search].