FANUC 31i-B J777: why an accepted G05.1 Q2 does not mean every block is smoothed
Separate J777 licensing, axis selection and block-level operation. PS5085 is not a dedicated missing-option test, and PS5421 can indicate a function conflict.
Contents
Mode entry is not block-level activity
Smooth interpolation reconstructs smooth curves from short segments while retaining portions that must follow the programmed polygonal path. Acceptance of G05.1 Q2 does not establish that every subsequent block is smoothed. This article covers Smooth Interpolation on 31i-B, not every G05.1 Q value or Nano Smoothing.
Scope and authorized addition
The 2013 FANUC catalogue assigns A02B-0327-J777 to 31i-B Smooth Interpolation. B-64484EN/03 §4.12 also requires the AI contour control option. /03 is a manual edition, not a software revision; the minimum software revision was not verified, and this order code must not be transferred to 31i-B Plus. Have FANUC or the builder check the complete CNC model, software series/revision, installed options and compatibility before authorized installation and acceptance. Parameter changes do not confer a license; AI contour control alone does not prove that J777 is configured.
Zeros select axes, not a return-to-zero move
The documented format is G05.1 Q2 Xp0 Yp0 Zp0, with up to three basic axes or axes parallel to them. Zero selects a participating axis; this entry block causes no axis movement, even in absolute mode. Do not put other G codes in the G05.1 block. G05.1 Q0 or RESET cancels the mode. Check surrounding motion blocks: a nonmoving entry block does not make the whole program safe. Establish G43/G44 tool length compensation before entering smoothing; cancel smoothing with Q0 before cancelling tool length compensation, and do not change its amount while smoothing is active.
Follow the alarm cause, not the option name
The maintenance manual defines PS5085 (SMOOTH IPL ERROR 1) as a syntax error in the smoothing block, and PS1990 (SPL:ILLEGAL AXIS COMMAND) as an invalid axis specified by G5.1 Q2. Reference-return commands such as G28 or G30 in smoothing mode can produce PS5110 (IMPROPER G-CODE (AICC MODE)). Combining it with G43.4/G43.5 tool center point control is prohibited in this edition and can produce PS5421. These point to format, axes or mode conflicts, not uniformly to missing J777. The evidence does not establish one inevitable alarm number for absent J777; verify that response for the actual software rather than importing another series’ alarm table.
If there is no alarm, inspect the executing block
Smoothing depends on segment length, changes in direction, modal state, selected axes and the CNC’s internal judgment. Parameters 8486, 8490 and 8487 govern length limits and angle assessment; no recommended values or adjustment procedure are supplied here. Diagnostic 5000#0 indicates actual activity in the current block, not a permanent license flag. One active block followed by an inactive block is an analytical scenario, not our machine test: preserve the corresponding blocks and modes, then compare geometry and eligibility before attempting another option installation or loosening thresholds.
Verification boundary
Qualified personnel must verify the path, compensation and stopping conditions through the builder’s trial procedure. No machine testing or machine-specific installation procedure is claimed. The links below are third-party mirrors of manufacturer documents; the manufacturer must confirm applicability to the actual machine.