FANUC 0i-TF Plus J731: G35/G36 circular threading and PS5058
For PS5058, check whether the arc changes its major axis. If G36 behaves unexpectedly, check its assignment first.
Contents
What J731 does
FANUC lists circular thread cutting on the 0i-TF Plus as option A02B-0349-J731. The tool follows an arc while F specifies the thread lead along the major axis of that arc. This is not G02.1 Circular Thread Cutting B. The details below apply to the cited 0i-F Plus lathe documentation; the minimum software release was not verified.
Arc geometry and G36 assignment
In the G18 ZX plane, G35 is clockwise and G36 is counterclockwise when assigned to circular threading. X/Z specify the endpoint. Use I/K for the center relative to the start or R for the radius. Optional Q is the start-angle shift in integer units of 0.001°, without a decimal point. Read the existing 3405#3 setting: 0 assigns G36 to automatic X tool compensation, while 1 assigns it to counterclockwise circular threading. This is a command assignment, not an entitlement. Do not use live motion to identify the assignment. Before relying on Q, read 3451#0 (GQS) to confirm that start-angle specification is enabled.
Distinguish PS5058 from PS0010
For PS5058 (G35/G36 FORMAT ERROR), FANUC documents two geometry checks: the arc must not switch between X and Z as its major axis, and travel along the major axis must not be zero. An arc from a Z-dominant region into an X-dominant region can therefore fail even with a correct endpoint and radius. Review the full arc geometry offline against figures 4.10(b)–(d). PS0010 (IMPROPER G-CODE) is the manual’s general rule for an unlisted G code or a missing corresponding option. Check the reported block, the code assignment and the installed options before drawing a conclusion.
Authorized setup and verification
Give FANUC or the machine builder the model and serial number, software series and release, installed options and current use of G36. Ask the authorized provider to confirm compatibility and configure the machine. Review existing programs that use G36 for automatic X tool compensation before any reassignment. Follow builder procedures to verify tool motion and spindle synchronization before cutting.
References
- FANUC CNC Function Catalogue · p. 198, Circular Thread Cutting
- FANUC 0i-F Plus Operator’s Manual B-64694EN/01 · Chapter 3, p. 32; §4.10, pp. 79–82
- FANUC 0i-F Plus Connection Manual (Function) B-64693EN-1/01 · p. 995, PS5058
- FANUC 0i-F Plus Descriptions B-64692EN/01