How to Mill a Large Arc Surface With a Small Cutter Head

• 1
  Key takeaways
• 2
  Why a small cutter head can mill a large arc surface
• 3
  Choosing the cutter and holder for arc work
• 4
  Raster or trace: picking the pass pattern
• 5
  Speeds, feeds, and stepover ranges that work
• 6
  Common errors and how to catch them early
• 7
  Step by step: milling the arc with a small cutter head
• 8
  Raster vs trace: which pass pattern fits your arc

A cutter head smaller than the arc radius is not a limitation. It is a geometry choice. The tool contacts the surface along a short chord, and the surface between passes is built up from overlapping chords. If the stepover is small enough, the envelope of those chords sits inside the tolerance band of the arc.

The math is simple. Chord error across a contact patch grows with the square of the stepover and shrinks with the cutter radius. Halve the stepover and you cut the scallop to roughly a quarter. That is why a Ø12 mm ball nose with a 1 mm stepover can hold a large arc better than a Ø50 mm face mill with a 10 mm stepover, even though the big cutter looks like the obvious tool.

This is the same reason mold shops finish deep ribs with small ball nose cutters. The cutter does not need to match the arc. It needs to sample the arc at a fine enough pitch. When you mill a large arc surface, you are really controlling sampling density.

There is a catch. Small cutters are flexible, and large arcs are long. A Ø12 mm tool hanging 120 mm out of a holder will deflect under load, and the deflection changes as the tool moves around the arc. The pass pattern has to account for that.

Use a ball nose for the finishing pass on any arc that is not flat across its width. A bull nose with a small corner radius can work on shallow arcs, but the flat land in the middle of the tool leaves a witness line where the passes meet. Ball nose cutters have a single contact point, so the scallop is predictable.

Match the cutter radius to the smallest concave radius in the arc. A cutter larger than the concave radius cannot reach the bottom of the curve. For a 300 mm radius arc, a Ø20 mm ball nose is fine. For a tight blend at the end of the arc, you may need to step down to Ø8 mm or Ø6 mm.

Holder choice matters as much as cutter choice. A shrink-fit holder gives the best runout and the shortest gauge length. A hydraulic holder is a close second and easier to change. Avoid a collet chuck on a long reach job unless the overhang is under 4× diameter.

Coating depends on the material. Uncoated carbide works on aluminium. TiAlN or AlCrN helps on stainless and tool steel, where edge buildup and heat are the main wear drivers. For aluminium with a high silicon content, a diamond coating is worth the cost.

• 1
  Ball nose over bull noseOne contact point means a predictable scallop on curved surfaces.
• 2
  Cutter radius under concave radiusOtherwise the tool cannot reach the bottom of the curve.
• 3
  Shrink-fit or hydraulic holderLower runout and shorter gauge length than a collet chuck.
• 4
  Coating by materialUncoated for aluminium, TiAlN or AlCrN for stainless and steel.

Raster passes run back and forth across the arc in straight lines. The tool axis stays vertical, which keeps the setup simple and the program short. The trade-off is that the effective stepover changes as the arc curves. On a shallow arc, the change is small. On a deep arc, the scallop height at the edges can be two or three times the scallop in the middle.

Trace passes follow the arc itself. On a 3-axis machine, this means the tool tip stays on the arc while the tool axis stays vertical, which causes the contact point to shift and the effective cutting speed to change around the curve. On a 5-axis machine, the head tilts to keep the contact point near the tool tip. That gives a more even scallop and a longer tool life.

For a shallow arc under 15° of total wrap, raster is usually faster and good enough. For a deep arc or a full radius, trace with a tilted head is the better choice. If you do not have 5-axis capability, you can still trace on a 3-axis machine, but reduce the stepover at the edges by 30–50% to compensate.

Either way, cut in one direction. Climb milling on both the forward and return pass doubles the tool life and keeps the chip load consistent. Conventional milling on the return pass will rub, work-harden stainless, and leave a different surface finish on half the arc.

Start from surface speed, not spindle speed. For aluminium 6061 with a coated carbide ball nose, 300–500 m/min is a reasonable range. For 17-4PH stainless, drop to 60–120 m/min. For titanium Ti-6Al-4V, 40–80 m/min. These are starting points, not limits. The arc geometry will tell you if you are close.

Feed per tooth on a finishing pass should be small enough to keep the chip thin. On a Ø12 mm ball nose in aluminium, 0.05–0.10 mm per tooth is typical. In stainless, 0.03–0.06 mm per tooth. If the chip is blue or the surface has a burnished look, you are rubbing, not cutting.

Stepover sets the scallop height. For Ra 1.6 μm on a Ø20 mm ball nose, a stepover of 1.5–2.0 mm is a good starting point. For Ra 0.8 μm, drop to 0.8–1.2 mm. For Ra 0.2–0.8 μm, you are in polishing territory, and a stepover under 0.5 mm is normal. Check the result with a profilometer before committing to a long run.

Depth of cut on the finishing pass should be light: 0.1–0.3 mm radial engagement. The roughing pass should leave 0.3–0.5 mm of stock on the arc, no more. Heavy finishing cuts on a long tool will deflect and leave a visible step at every pass boundary.

The most common error is a witness line at the pass boundary. It comes from tool deflection, thermal growth, or a stepover that is too large for the finish callout. If the witness line is a step, the stepover is too big. If it is a color change, the tool is rubbing or the chip load is too light.

Taper on the arc is another frequent problem. It shows up as a different radius at the top and bottom of the cut. Causes include tool wear on one side of the ball, a tilted spindle, or a workpiece that moved during the cut. Check the tool with a dial indicator before blaming the program.

Chatter on a large arc is usually a stiffness problem, not a speed problem. A long tool overhang, a thin workpiece, or a fixture that only clamps at the corners will all chatter. Reduce the overhang, add a support under the arc, or switch to a smaller stepover and a higher feed to get out of the chatter frequency.

Scrap happens when the arc is cut to the wrong radius. This is almost always a setup error, not a CAM error. Verify the tool length offset, the work offset, and the rotary table center before the first pass. On a part that takes hours to rough, a five-minute check is cheap insurance.