Independent CNC repair and technical reference Contact

FANUC 0i-TF Plus J731: G35/G36 circular threading and PS5058

Published Updated

For PS5058, check whether the arc changes its major axis. If G36 behaves unexpectedly, check its assignment first.

Contents
  1. What J731 does
  2. Arc geometry and G36 assignment
  3. Distinguish PS5058 from PS0010
  4. Authorized setup and verification
  5. References

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

Related technical articles

FANUC 31i-B J710 involute interpolation: diagnosing PS0241 and PS0242FANUC 0i-F Plus J770: G31 P90 continuous high-speed skip and alarms PS5068 and PS0369FANUC 0i-TD S889: How G50.9 outputs an auxiliary function during axis motion