FANUC 31i-B5 S996: the two I/J/K triplets in G43.9 and alarm PS5464
In a subsequent motion block while G43.9 mode is active, the plain I/J/K gives tool-axis direction; the separate I/J/K after literal ,L2 gives the surface normal.
Contents
In a subsequent motion block while G43.9 mode is active, the plain I/J/K gives tool-axis direction; the separate I/J/K after literal ,L2 gives the surface normal.
Check S996 and TCP against the machine record
Cutting Point Command (S996) extends tool center point control so the program can specify the contact point on the workpiece. This article covers the non-Plus 31i-B5 machining center. FANUC lists A02B-0326-S996 and includes it in A02B-0326-R677 (High-Speed Smooth TCP) for that model. The catalogue does not show what is fitted on any particular machine. B-64482EN/03 p. 22 identifies the machining-center TCP prerequisite. No minimum CNC software revision was verified. Give FANUC or the builder the machine serial number, controller model, software series and revision, and option record; use their authorized service to confirm prerequisites and activate the option.
Identify each direction in the motion block
G43.8 (Type 1) specifies posture through rotary-axis coordinates or increments. In a subsequent motion block while G43.9 (Type 2) mode is active, plain I/J/K gives the tool-axis direction at the block endpoint. The separate I/J/K following literal ,L2 gives the cutting-surface normal there. Both directions are expressed in a coordinate system fixed to the table. On an offline copy, verify the frame used by the CAM postprocessor. Check that it has not output a machine-frame normal or put the tool-axis direction in the ,L2 field. Do not jog a rotary axis to test those assumptions.
Separate an unavailable command from an invalid cutting-point condition
PS0010 (IMPROPER G-CODE) is generic: the control may not accept the G code or its corresponding option may be unavailable. Check the full block and the machine’s entitlement record. PS5464 (ILLEGAL COMMAND IN G43.8/G43.9) does not establish a missing license. The maintenance manual lists three cases: the angle between the tool length offset direction and the surface normal exceeds 90°; the tool radius offset is smaller than the tool corner-R offset; or a rotary axis is moved by manual intervention on a tool-rotation-type machine. Check a program copy, the offset table and the operating history before changing anything on the machine.
Sources
- FANUC CNC Function Catalogue (2013, pp. 330 (S996) and 332 (R677))
- FANUC B-64482EN/03 Descriptions (p. 22; §8.11, pp. 278–279)
- FANUC B-64487EN/05 Operation and Maintenance Handbook (pp. 89–90)
- FANUC B-64485EN/01 Maintenance Manual (Appendix A, p. 663 (PS5464))
- FANUC B-64484EN-2/06 Machining Center Operator’s Manual (§2 (PS0010))