FANUC 31i-B J710 involute interpolation: diagnosing PS0241 and PS0242
When G02.2 or G03.2 alarms, distinguish an unavailable feature from missing block data or a path that enters the base circle.
Contents
When G02.2 or G03.2 alarms, distinguish an unavailable feature from missing block data or a path that enters the base circle.
What J710 adds
J710 lets the CNC interpolate an involute directly, for example when machining a gear-tooth profile. FANUC lists A02B-0327-J710 for the 31i-B and A02B-0326-J710 for the 31i-B5. This article covers planar involute interpolation on the Model B machining center, not entitlement to S853 helical involute interpolation. A minimum software revision was not verified. Give FANUC or the machine builder the control model, CNC software series and revision, machine serial number and installed option record so they can confirm compatibility and install the option through authorized service. Parameters and postprocessor settings do not grant entitlement.
Reconstruct the base circle offline
G02.2 is clockwise involute interpolation; G03.2 is counterclockwise. Select the plane with G17, G18 or G19. In G17, X and Y specify the endpoint, I and J point from the start to the base-circle center, and R is the base-circle radius, not the radius of a circular move. I and J remain signed increments in G90. Recover the programmed start from the preceding blocks, then add I and J to locate the center. Offline example: with center (0,0) and R = 20 mm, an endpoint of (18,0) mm is only 18 mm from the center; it is inside the base circle. There is no need to run that block. An endpoint outside the circle does not by itself establish a valid curve.
Use the alarm number to choose the next check
PS0010 (IMPROPER G-CODE) can indicate an unavailable corresponding option or an unsupported code. Check the full alarm block and the G-code table for the actual control. For PS0241 (ILLEGAL FORMAT IN G02.2/G03.2), look for omitted endpoint words in the selected plane, missing center data or a missing R. For PS0242 (ILLEGAL COMMAND IN G02.2/G03.2), check whether the start or end is inside the base circle. If the programmed geometry clears the circle and the alarm appears only with G41/G42, inspect the D offset and compensated cutter-center path in offline simulation. Do not remove compensation from a production program just to try it. Missing or nonpositive R can also lead to PS0241 or PS0242.
Sources
- FANUC CNC Function Catalogue (2024, p. 177)
- FANUC B-64484EN-2/03 Machining Center Operator’s Manual (§2; §3.1, pp. 15–23)
- FANUC B-64485EN/01 Maintenance Manual (PS alarms 0241–0242)