FANUC polar interpolation slows near the center: C-axis speed limits and mode boundaries
The 0i-TF manual explains speed constraints near the center during polar coordinate interpolation. Calculations illustrate their scale, alongside restrictions on G12.1/G13.1, compensation state and coordinate-system changes.
Contents
During face-contour machining near the rotary center, actual feedrate can fall significantly even when the programmed F value is unchanged. First examine path geometry and C-axis speed demand; do not immediately attribute the behavior to inadequate drive performance.
Command semantics on the 0i-TF
Section 3.1 of the public mirror of the original FANUC B-64604EN-1/01 manual explains that polar coordinate interpolation converts a contour described in Cartesian coordinates into linear- and rotary-axis motion. G12.1 enters the mode and G13.1 cancels it. This article is limited to the 0i-TF with the relevant axes and function correctly configured; it does not provide a complete machine-ready program.
Why speed limiting becomes more likely near the center
Pages 20–21 explain that the required C-axis velocity component increases as the tool approaches the workpiece center. The control automatically adjusts feedrate when permitted limits are exceeded. The manual's geometric relationship gives the following speed-scale check:
F＜rmin×ωmax×π÷180. Here rmin is the minimum distance from the tool center to the rotary center in mm; ωmax is the maximum C-axis cutting angular velocity in deg/min; F is in mm/min. This is not a cutting recommendation for a material or tool.
For calculation only, assume ωmax＝3600 deg/min. At rmin＝10 mm, the right-hand side is about 628.3 mm/min; at a distance of 1 mm, it is about 62.8 mm/min. With the same angular-speed capability, the corresponding sustainable linear-speed scale differs by a factor of ten. Actual motion also depends on axis acceleration/deceleration and control settings.
Additional restrictions on mode switching
Pages 18–20 of this edition require the rotary center and coordinate reference to be checked and restrict coordinate-system changes within the mode. G12.1/G13.1 cannot be switched while G41/G42 compensation is active. Do not simply delete a command after an alarm and resume machining; first examine the complete relationship between compensation vectors and mode transitions.
Distinguish expected speed limiting from an anomaly
| Observation | Check first |
|---|---|
| Slowing occurs only near the center | Closest distance, path direction and C-axis speed demand |
| The same geometric path behaves differently after a setup change | Rotary center, coordinate reference and workholding orientation |
| An alarm occurs when entering or leaving the mode | Compensation state, coordinate changes and program transitions |
For comparisons, retain the same program segment, current coordinates and actual axis states. Do not raise axis speed limits to eliminate slowing without evaluating machine capabilities. Other functions are covered in the OPTION section.