CNC Machining Tool Cutting Parameters: A Working Guide

• 1
  Key takeaways
• 2
  What CNC machining tool cutting parameters actually control
• 3
  Cutting speed and feed per tooth: the pair that decides tool life
• 4
  Axial and radial depth: where force and chatter come from
• 5
  Tool geometry: the constraint that sets the ceiling
• 6
  Coolant and chip evacuation: the parameters that are not in the table
• 7
  A practical order for setting parameters on a new job
• 8
  Starting cutting parameters by material and operation

Four numbers describe almost every metal-cutting operation: cutting speed (surface speed, m/min or sfm), feed per tooth (mm/tooth or in/tooth), axial depth of cut, and radial width of cut. Everything else, spindle rpm, table feed in mm/min, is calculated from those four plus the tool diameter and flute count.

The reason engineers care is that each number maps to a different physical effect. Surface speed controls temperature at the cutting edge. Feed per tooth controls chip thickness and therefore whether the edge cuts or rubs. Axial depth controls the length of engaged edge. Radial width controls how much the tool bends.

Change one and the others shift. Raise surface speed 30 percent and edge temperature climbs, so tool life drops even though the cycle got shorter. Raise feed per tooth without raising speed and the chip thins relative to the radius, which can push the tool into rubbing instead of shearing.

So a parameter set is a balance, not a lookup value. The tables later in this page give starting ranges for common materials; the rest of the page explains which direction to move when the cut misbehaves.

Surface speed is the speed of the cutting edge relative to the workpiece, not the spindle rpm. For a Ø12 mm end mill at 4,000 rpm, surface speed is roughly 150 m/min. For a Ø50 mm face mill at the same rpm, it is over 600 m/min, which is why large tools run slow.

Feed per tooth is the thickness of material each edge removes per revolution. On aluminum with a 3-flute cutter, 0.05–0.10 mm/tooth is a common starting range. On 4140 steel with a 4-flute cutter, 0.03–0.08 mm/tooth is more typical. Below the low end, the edge tends to rub.

Rubbing is the failure mode most people misread. The tool makes noise, the finish looks smeared rather than cut, and the edge wears faster than expected. The instinct is to slow down. The correct move is usually to raise feed per tooth so the tool bites.

There is a floor here worth remembering: chip thickness must be large enough to clear the edge radius. On a coated carbide insert with a 0.02 mm edge hone, feed per tooth below roughly 0.03 mm means the hone rubs the surface instead of the rake face cutting it.

• 1
  Aluminum 6061150–400 m/min surface speed, 0.05–0.10 mm/tooth feed
• 2
  Stainless 304 / 316L60–120 m/min, 0.04–0.08 mm/tooth, generous coolant
• 3
  Steel 414090–180 m/min, 0.03–0.08 mm/tooth, watch chip color
• 4
  Titanium Ti-6Al-4V30–60 m/min, 0.03–0.07 mm/tooth, sharp edges only

Depth of cut is split into two directions. Axial depth (ap) is how deep the tool goes along its axis. Radial width (ae) is how much of the diameter is engaged in the cut. A common roughing strategy is to take a large axial depth with a small radial width, which spreads wear along more of the flute and keeps radial force low.

Radial engagement is the bigger chatter lever. On a 12 mm end mill, going from 3 mm radial to 6 mm radial roughly doubles the bending load, and the tool deflection scales with the cube of the unsupported length. That is why deep pockets chatter even at conservative speeds.

A practical starting point for roughing is 50–70 percent of the tool diameter axially and 25–40 percent radially on a rigid setup. On a long-reach tool, drop radial engagement to 10–15 percent and raise spindle speed instead. The material removal rate can stay similar while the tool stops singing.

Aspect ratio matters more than absolute depth. A Ø10 mm tool sticking 100 mm out of the holder has a 10:1 ratio and will deflect under loads a 3:1 tool would shrug off. If the geometry forces a long reach, expect to reduce radial width, not just spindle speed.

Flute count decides chip clearance. A 3-flute cutter in aluminum has more room between flutes than a 6-flute cutter, so it evacuates chips better and allows higher feed per tooth. A 6-flute cutter in steel has more edges in the cut at once, which spreads load and improves finish but limits chip room.

Helix angle controls how the cutting force is directed. A 45° helix pulls chips up and out of the cut, which suits deep pockets and aluminum. A 30° helix puts more force into the workpiece and less into the spindle, which suits thin-walled parts where deflection matters.

Corner radius is often the difference between a tool that lasts and one that chips. A sharp corner concentrates stress and is the first thing to fail in interrupted cuts. A 0.4–1.0 mm corner radius spreads that load and is worth the trade in minimum internal corner size.

Coating choice follows the material. TiAlN coatings survive high temperatures in steel and stainless. ZrN and uncoated polished tools work better in aluminum because aluminum tends to stick to TiAlN at high speed. Diamond-like coatings suit abrasive composites and graphite.

• 1
  Aluminum2–3 flutes, 45° helix, polished or ZrN, no coating build-up
• 2
  Steel and stainless4–6 flutes, 30–38° helix, TiAlN or AlTiN coated
• 3
  Titanium4 flutes, sharp edge, AlTiN, no honing
• 4
  Thin wallsLower helix, fewer flutes, lighter radial engagement

Coolant does two jobs: it removes heat and it clears chips. On shallow cuts in aluminum, flood coolant mostly clears chips. On deep holes in stainless or titanium, heat removal is the point, and through-spindle pressure matters far more than total flow.

Chip recutting is a silent parameter killer. If a chip stays in the cut, the edge cuts it a second time, which doubles the load on that tooth and usually causes chipping. This shows up as random edge damage that no speed or feed change fixes until the chip leaves.

Air blast plus minimum quantity lubrication works well in aluminum and plastics where thermal load is low. It fails in titanium and Inconel, where the heat has nowhere to go and the edge reaches temperatures that break down the coating.

The engineering meaning is simple: if you cannot evacuate the chip, no parameter set will hold tolerance. Fix the chip path before tuning speed and feed. On deep pockets, that may mean a different tool, not a different number.