English is currently available.
Manufacturing & Production Engineering DISCUSSION
I have a small CNC mill with a 6000 rpm spindle and I am cutting 6061 aluminium with a 10 mm three-flute carbide end mill. The tool catalogue gives a cutting speed in m/min and a feed per tooth in mm, but the machine wants rpm and mm/min.
What are the formulas that connect these, and what should I do when the calculated speed is higher than my spindle can reach? At the moment I am guessing, and the tool either rubs and squeals or the chips weld to the flutes.
Two formulas cover it. Spindle speed: N = (1000 × Vc) / (π × D), with Vc in m/min and D in mm. Table feed: Vf = N × fz × z, where fz is the feed per tooth and z the number of flutes.
Take Vc = 300 m/min, which is within the range tool makers give for carbide in wrought aluminium: N = 300,000 / (π × 10) = about 9550 rpm. With fz = 0.05 mm and 3 flutes, Vf = 9550 × 0.05 × 3 = about 1430 mm/min. Use the values from your own tool's catalogue, since they depend on the coating, the grade and the flute geometry.
When the spindle cannot reach the calculated speed, run it at its maximum and recalculate the feed from that speed so the feed per tooth stays the same. At 6000 rpm the actual cutting speed is π × 10 × 6000 / 1000 = 188 m/min, which is still perfectly workable in aluminium, and the feed becomes 6000 × 0.05 × 3 = 900 mm/min.
The mistake to avoid is keeping the rpm low and also dropping the feed "to be safe". Chip thickness is what matters to the tool. Too thin a chip means the edge rubs instead of cutting, which makes heat and the squeal you describe.
Chips welding to the flutes is a heat and chip evacuation problem, common in aluminium. Things that help: a cutter made for aluminium (2 or 3 flutes, polished or with a suitable coating, high helix), compressed air or a little mist or flood coolant to clear the chips, and not recutting chips in deep slots. A full-width slot is the worst case because the chips have nowhere to go; take slots in shallower passes, or use a smaller cutter and open the slot with a side-milling path.
Once aluminium has stuck to a cutting edge the tool cuts badly from then on, so inspect the flutes before blaming the numbers.
One refinement for light side cuts. The catalogue feed per tooth assumes a radial engagement of about half the cutter diameter or more. With a small radial width ae the chip is thinner than the programmed fz, and you can compensate with fz_prog = fz × D / (2 × √(D × ae - ae²)).
For D = 10 mm and ae = 1 mm: √(10 - 1) = 3, so the factor is 10 / 6 = 1.67, and a target chip of 0.05 mm needs a programmed 0.083 mm per tooth, about 1500 mm/min at 6000 rpm. On a light machine, work up to that in steps rather than jumping straight to it.
Check that the machine has the power and rigidity for the cut. Metal removal rate is Q = ap × ae × Vf. With a 5 mm depth, 5 mm width and 900 mm/min, Q = 22,500 mm³/min, or 375 mm³/s. Taking a specific cutting energy of roughly 0.8 W·s/mm³ as a ballpark for aluminium alloys, that is about 300 W at the cutter, before spindle and drive losses.
Small hobby-class mills usually run out of rigidity before power. If you hear chatter, reduce the radial width or the tool stick-out first and keep the feed per tooth; shortening the stick-out makes a large difference because tool deflection grows with the cube of the length.
