G-code arcs (G2 and G3) look smooth on screen but can make a machine stutter, dwell, or gouge if the controller and the motion planner disagree about how to handle them. Arc acceleration smoothing is the set of rules, in firmware and in CAM output, that keeps the machine flowing through curves instead of treating every arc segment as a separate event. Understanding these rules lets you cut curves faster, quieter, and more accurately.
Why arcs need special handling
An arc command describes a curve, but the machine's steppers move in straight micro-steps, so the controller must convert the arc into many tiny linear moves, a process called arc interpolation or segmentation. Each segment is a velocity change the planner must evaluate against acceleration limits. On a tight arc at high feed, the required centripetal acceleration can exceed the machine's limits, forcing the planner to slow down, sometimes drastically, and on machines with limited lookahead the slowdown happens too late, causing overshoot or corner rounding.
The second issue is data starvation. CAM programs often output arcs as thousands of tiny line segments instead of true G2/G3 commands. A controller with a small motion buffer can run out of moves to plan ahead on dense segment streams, causing the machine to hesitate at exactly the moment it should be flowing. True arc commands compress the same geometry into far fewer blocks, which is why emitting arcs from CAM matters.
Controller-side smoothing settings
Most modern firmware includes arc-specific handling. GRBL-based controllers have an arc tolerance setting that controls how finely arcs are subdivided; a looser tolerance means fewer segments and smoother motion at the cost of tiny chordal deviation from the true arc. Junction deviation or cornering settings govern how much the machine slows for direction changes, and arcs benefit from the same lookahead that smooths corners.
The practical tuning approach: set the arc tolerance so the chordal error stays well under your part tolerance, often a few hundredths of a millimeter, then verify with a test cut of concentric arcs at your normal feed rates. If the machine sounds labored or the surface shows faceting, the segments are too coarse or the planner is starving; if it crawls through curves that should flow, acceleration limits or overly conservative junction settings are the bottleneck.
CAM output rules for clean arcs
Configure the CAM postprocessor to emit true G2/G3 arcs wherever the geometry is genuinely circular, rather than linearizing everything. Set the postprocessor's arc fitting tolerance to match the part: tighter for precision bores and mating curves, looser for decorative profiles. Watch for CAM systems that break arcs at quadrant boundaries or emit full circles as two semicircles; both are fine for the machine as long as the segments join tangentially.
Be wary of arc commands with extremely small radii at high feed rates. The planner may not be able to honor the programmed feed on a tiny arc without exceeding acceleration limits, so it slows down, which changes chip load and can rub the cutter instead of cutting. Forcing a feed reduction on small-arc features in CAM, or splitting tiny arcs into a separate slower operation, keeps cutting conditions consistent.
Acceleration limits and curve feed
The fundamental relationship is that the maximum feed through an arc of radius r without exceeding the machine's acceleration limit a is proportional to the square root of a times r. Halve the radius and the sustainable feed drops by about thirty percent. This is physics, not a setting, and it means small radii always cost speed. The smoothing rules do not repeal this; they just keep the machine as close to the limit as safely possible instead of oscillating around it.
When tuning, raise acceleration limits cautiously and test with arcs, not straight lines. A machine that rapids beautifully in straight lines can still shake itself on tight curves. Listen for resonance and watch the cut surface: chatter marks on curves that do not appear on straight cuts point at acceleration or jerk settings, not the tool.
Verification cuts that tell the truth
Cut a test piece with a range of arc radii, from generous sweeps down to tight inside corners, at your production feeds. Measure the radii with calipers or a radius gauge and inspect the surface finish. Systematic undersize on small arcs indicates the planner is cutting corners, literally; faceting indicates coarse segmentation; chatter indicates acceleration or rigidity issues.
Log the settings that pass the test for each material and tool combination you run regularly. Arc behavior changes with feed, depth of cut, and machine wear, so a smoothing setup is a living configuration, not a set-and-forget value. Revisit it when you change spindles, upgrade firmware, or notice curve quality drifting.
Arc acceleration smoothing is about respecting what the machine can physically do through a curve and giving the planner clean data to work with. Emit true arcs, set segmentation tolerance to your part tolerance, tune acceleration against real curve cuts, and slow down deliberately for tiny radii. Curves will cut faster, quieter, and truer, which is the whole point of having a CNC in the first place.
Related Guides
- Subprogram Looping and Macro Calls in Fanuc G-Code: Repetitive machining, drilling a bolt circle, milling a pocket pattern, engraving a row of labels, does not need repetitive code. Fanuc G-code
- Polar Coordinate Interpolation Setup in Grbl: Most CNC work lives in Cartesian coordinates: X left-right, Y front-back, and the machine interpolates straight lines and arcs between points. But
- Modal Group Interactions in Fanuc Turning Cycles: Fanuc canned cycles for turning, the G70 through G76 family, are powerful shortcuts, but they interact with modal G-code groups in ways that surprise
- G91 Incremental Subroutines for Repetitive Milling: Repetitive milling, a row of identical pockets, a grid of holes, a pattern of slots, is where hand-written G-code earns its keep, and G91 incremental