Tool Feed Method for CNC Machining: 5 Checks Before You Cut

• 1
  Key takeaways
• 2
  Start With the Tool Feed Method for CNC Machining Direction: Climb or Conventional
• 3
  Set Feed per Tooth, Not Just Feed Rate
• 4
  Match the Path Shape to Radial Engagement
• 5
  Choose the Method by Material and Feature
• 6
  Step by Step: Locking the Feed Method in CAM
• 7
  Feed Method Quick Reference

Every program starts with a direction choice, and it is the cheapest decision to get wrong. In climb milling the cutter tooth enters at the thickest part of the chip and exits at zero thickness. That is the standard for finishing on a machine with a preloaded ball screw. Heat leaves with the chip, the cut pushes the work away from the tool, and surface finish lands in the Ra 0.8–1.6 μm band on aluminium and mild steel.

Conventional milling does the opposite: the tooth rubs before it bites. On a tight machine this costs you tool life and finish. On a worn machine with 0.02 mm of backlash it can actually be the safer choice, because the cutter does not get pulled into the work. If you hear a rhythmic knock on a roughing pass, the direction is fighting the backlash.

Three cases where conventional wins. First, hot-rolled or cast stock with hard scale on the surface, where the tooth would otherwise chip on entry. Second, manual or converted machines that still carry measurable backlash in X and Y. Third, finishing an interrupted cut on a thin wall, where climb pull would deflect the part. Outside those, stay with climb.

One more note on entry angle. A tool that enters at 90° to the surface takes the full load in one instant. A ramp or helix entry spreads it over 5–15° of arc. On a 6 mm carbide end mill in 6061, a 2° ramp at 1,200 mm/min is a reasonable starting point. Watch the first 20 mm of the cut, not the whole pass.

• 1
  Climb by defaultPreloaded ball screws, finished surfaces, thin floors.
• 2
  Conventional by exceptionHard scale, visible backlash, interrupted finishing cuts.

Feed rate in mm/min is an output, not an input. The input is feed per tooth, fz, and the formula is simple: feed rate = fz × number of teeth × rpm. Change any one of the three and the chip you actually cut changes with it. That is why copying a feed rate from a tool catalogue page usually fails. The catalogue assumes a radial engagement and a tooth count that may not match your setup.

For aluminium 6061 with a 3-flute carbide end mill, a working fz is 0.05–0.10 mm per tooth on a light finishing pass. For a 12 mm cutter at 8,000 rpm that puts you near 1,600 mm/min. Stainless 304 asks for 0.03–0.05 mm per tooth and more coolant, often flood plus a high-pressure jet through the spindle. Titanium Ti-6Al-4V sits lower again, around 0.02–0.04 mm per tooth, because the material work-hardens if the tooth rubs instead of cutting.

The error we see most often is running a light radial pass with a heavy depth of cut while keeping the finishing fz. The chip gets thin, the tooth rubs, and the edge wears on the flank instead of the rake. Chips come off as dust or small slivers rather than proper comma shapes. If your chips look like powder, raise fz before you touch spindle speed.

Speeds come from surface speed, and the coating sets the ceiling. Uncoated carbide in 6061 runs 300–500 m/min. TiAlN-coated tools in 4140 run 120–180 m/min. Aluminium-specific coatings with high silicon content in the binder run higher and resist built-up edge. If the machine has an encoder that reports actual spindle speed, compare it against commanded speed on the first part. A 2% gap means the drive is slipping, and every feed calculation is off by that amount.

• 1
  Formulafeed rate = fz × teeth × rpm
• 2
  Chip shape is the gaugeComma-shaped chips: fz is right. Dust: fz is too low.

The path shape controls how much of the cutter is in the material at any moment. A straight full-width slot runs at 100% radial engagement with the cutter buried. Heat builds, chips recut in the slot, and a 12 mm cutter in steel will not survive long. A trochoidal path replaces the slot with a series of wide arcs at 8–15% radial engagement and takes the depth in a few passes. The same slot gets cut with a fraction of the cutting force.

Chip thinning is the reason the trochoidal path works with a higher feed. When radial engagement is small, the chip at the entry is thinner than the nominal fz, so you must raise fz to keep the chip thickness at the target. At 10% radial engagement on a round insert, the correction factor is roughly 2.5. That is why trochoidal programs often show feeds that look aggressive next to a conventional slotting program. They are not aggressive. The chip is the same thickness.

Use trochoidal paths for deep pockets, long slots and any pocket deeper than one diameter. Use a simple contour pass for shallow pockets under 0.5 × diameter, where the arc overhead is not worth the extra code. Adaptive clearing in most CAM systems will pick trochoidal geometry for you once you set the engagement limit. Set the limit at 15% for steel and 25% for aluminium as a starting point.

The exception is a slot that must finish at full width in one pass on a thin part. There, a trochoidal path can push the wall sideways. Climb contour with a rough pass and a separate finishing pass at 5% radial engagement holds the wall better, even if it takes longer. For parts where wall thickness is under 1 mm, we run the finish pass on a 4-axis or 5-axis setup so the cutter approaches along the wall rather than across it.

• 1
  Full-width slot100% engagement, high heat, avoid on steel.
• 2
  Trochoidal8–15% engagement, higher fz, deep pockets.

The material narrows the choice before the feature does. Aluminium 6061 and 7075 tolerate climb milling, high fz and aggressive trochoidal paths. Stainless 304 and 17-4PH work-harden at the surface, so the tooth must always cut below the hardened layer. That means a minimum chip thickness, no dwell, and no rubbing passes. Titanium behaves the same way but with lower speeds and more attention to coolant delivery.

Inconel and other nickel alloys push you toward lower radial engagement and lower surface speed. A 10 mm carbide cutter in Inconel 718 may run at 40–60 m/min surface speed with 5–8% radial engagement. Tool life is measured in minutes, not hours, and the feed method should be conservative on entry. Ramp angles stay under 2°.

Features decide the last step. Thin floors under 1 mm deflect under climb pull, so support them or finish with light conventional passes. Deep bores over 4 × diameter need a long-reach cutter, and long-reach cutters chatter at high fz. Drop fz by 30–40% and raise rpm to stay in the stable zone. For a bore that must hold ±0.005 mm, leave 0.15 mm on the wall and take it in a single finishing pass with a sharp, coated tool.

Medical and aerospace parts often carry a drawing note on surface finish, not just dimension. Ra 0.2–0.8 μm calls for a finishing pass with a wiper or a small-nose radius tool, low fz and a climb direction. If the note is Ra 0.8–1.6 μm, a normal finishing pass will hold it. We inspect on a CMM and provide reports on request, so the finish and the feed method get checked against the same drawing.

• 1
  AluminiumHigh fz, climb, trochoidal for deep pockets.
• 2
  Stainless and titaniumMinimum chip thickness, no rubbing, flood coolant.
• 3
  InconelLow surface speed, low radial engagement, ramp under 2°.