FANUC 31i-B R578: is the rotary command in degrees or developed distance?
Two controls can both accept G07.1 and still interpret the subsequent rotary-axis number differently.
Contents
Two controls can both accept G07.1 and still interpret the subsequent rotary-axis number differently.
Base cylindrical interpolation and the R578 extension
FANUC lists A02B-0327-J816 for base cylindrical interpolation and A02B-0327-R578 for cylindrical interpolation by plane distance command on the 31i-B. The extension for 31i-B5 is A02B-0326-R578. R578 extends working cylindrical interpolation; it does not replace it. These operating notes are for Model B; a minimum CNC software revision was not verified. Ask FANUC or the machine builder to check prerequisites and entitlement using the machine serial number, software series and revision, and installed option record, then arrange authorized installation and acceptance.
Check the rotary words inside the mode, not the entry radius
Model B path parameter 3454 bit 2 (DTO) describes the input interpretation: 0 is angle; 1 is developed-plane distance in the active metric or inch input units. This setting is not an option license. In either case, the G07.1 entry block takes a positive workpiece radius on the rotary-axis address; the exit block uses zero on that same axis. Keep entry and exit in their own blocks. Offline example: with a 50 mm radius, 90° corresponds to about 78.54 mm along the developed surface; 90 mm would instead be about 103.13°. When comparing machines, read DTO and the input units and inspect the postprocessor output without changing the parameter or running an old program.
An alarm and a wrong path call for different checks
If G07.1 gives PS0010 (IMPROPER G-CODE), check the control’s G-code table, the entire alarm block and whether the base cylindrical function is available. PS0010 does not establish that R578 is missing: the extension introduces no separate G code. For PS0175 (ILLEGAL G07.1 AXIS), check for a negative entry radius, more than one axis in the block, an axis not configured to support the function, or an attempt to cancel it on an axis that is not in the mode. For PS0176 (ILLEGAL G-CODE USE(G07.1 MODE)), look for a prohibited code such as G00 in the mode. If the path is wrong without an alarm, check angles versus developed distances in offline simulation rather than accepting the lack of an alarm as proof of correct units.
Sources
- FANUC CNC Function Catalogue (pp. 182–183)
- FANUC B-64484EN/03 Operator’s Manual (§3; §4.9.1–4.9.2, pp. 66–70)
- FANUC B-64490EN/04 Parameter Manual (p. 181, 3454#2 DTO)
- FANUC B-64485EN/01 Maintenance Manual (PS0175, PS0176)