Milling cutting parameters, speeds and feeds with the power check included
Enter the material, the coating on the tool, its diameter and tooth count, and the depth of cut, and read the cutting speed, spindle rpm, feed per tooth, feed rate, chip thinning correction and the cutting power the spindle actually has to supply. The tool clips the result to your machine's real rpm and power, not just what the material table recommends.
Open the cutting parameters calculator A free account opens this tool. The interface is in English and nothing you enter leaves your browser.How it works
Three steps from material to a checked, machine safe cutting regime.
Pick the material, coating and tool geometry
Choose one of five materials, aluminium 6061, mild steel S235, stainless 304, grey cast iron or brass C360, then the coating on the tool, uncoated carbide, TiN or TiAlN, since coating moves the safe cutting speed range without changing the material. Enter the tool diameter and the number of flutes.
Enter the depth of cut and either the catalogue speed or your own
Give the axial depth of cut ap and the radial depth ae. Use the catalogue cutting speed for the material and coating, or switch to a manufacturer specific value if your tool's data sheet gives one that differs from the general purpose carbide range shown here.
Read rpm, feed rate, chip thinning and the power check
The tool converts cutting speed to spindle rpm through the diameter, works out feed per tooth and minute feed rate, applies the radial chip thinning correction if ae is under half the diameter, and runs the Kienzle model to check the cutting power against your machine's rated spindle power and drive efficiency.
Five materials, three coatings, one power model
Each material carries its own cutting speed range, feed per tooth range and Kienzle force constants.
Built to catch the mistakes speed alone will not show you
Most cutting parameter mistakes are not about picking a number that looks wrong, they are about a second number moving invisibly when you only touch the first.
Diameter is the missing link between rpm and cutting speed
Cutting speed Vc and spindle rpm are not the same number: Vc equals pi times diameter times rpm divided by 1000. The same rpm gives a very different Vc for a 6mm and a 20mm cutter, because the larger tool's edge sweeps a longer path per revolution. Changing rpm alone without checking the resulting Vc is a common source of a cutting speed nobody actually chose.
Radial chip thinning, both directions
When the radial depth of cut is under half the tool diameter, each tooth sees a thinner chip than the programmed feed per tooth suggests, following a correction factor of 2 times the square root of (ae/D times (1 minus ae/D)). At 10 percent radial engagement the real chip is only about 60 percent of the programmed value, and compensating means raising feed per tooth, not lowering it, the opposite of most operators' first instinct.
Cutting force rises as the chip gets thinner
The Kienzle model puts specific cutting force as a function of chip thickness raised to a negative exponent specific to the material, so a thinner chip needs more force per unit area, not less. Halving the rpm while leaving the feed rate untouched raises feed per tooth and, through this model, raises cutting force too, the opposite of the 'slower must be gentler' assumption that leads operators to make the problem worse under load.
Climb versus conventional, and what the tool leaves out
Climb milling avoids the rubbing that conventional milling causes at the start of each tooth's engagement, especially valuable on work hardening materials like stainless 304, but it needs a machine drive with no backlash. The tool does not model tool life, chatter stability lobes or the specific dynamics of your machine and holder, and says so rather than pretending a single power number covers them.
Frequently asked questions
What is the difference between cutting speed and spindle rpm?
Cutting speed Vc, in metres per minute, is how fast the cutting edge moves along its circular path. Spindle rpm is how many times per minute the tool turns. They are linked by the diameter through Vc equals pi times D times rpm divided by 1000, so the same rpm gives a different Vc for a small and a large tool, and picking rpm without checking the resulting Vc against the material's recommended range is a common mistake.
Why does the tool warn about feed per tooth being too low, not just too high?
Every cutting edge has a finite radius at a microscopic scale, and below a minimum chip thickness the edge stops cutting cleanly and starts rubbing the surface instead. Rubbing generates heat right at the contact zone, wears the edge faster than normal cutting, and on work hardening materials like stainless 304 it hardens the very surface the next tooth has to cut. Each material in the tool carries a minimum recommended feed per tooth for this reason, not only a maximum.
If the tool chatters, should I just slow the spindle down?
Not necessarily. Chatter is usually a resonance between the tooth engagement frequency and the natural frequency of the tool, holder, spindle and workpiece taken together, described by stability lobe theory. Because of this, a higher rpm can sometimes fix chatter better than a lower one, by moving the operation into a different stable band. This calculator does not compute the stability lobes for your specific machine, since that needs a modal test, not a general catalogue table.
Why does reducing rpm without touching the feed rate make things worse?
Feed per tooth equals the feed rate divided by the number of flutes times rpm, so cutting rpm by 30 percent while leaving the programmed feed rate unchanged raises feed per tooth automatically, by roughly 43 percent in a typical steel example. Through the Kienzle force model that raises cutting force by around a third for the same material, the opposite of the 'slower means gentler' reaction most operators reach for first. Reducing rpm and feed rate together, proportionally, keeps feed per tooth and force unchanged while cutting speed and heat generation both fall.
Does coating make the material easier to cut?
No, the material is identical either way. A coating like TiN or TiAlN raises the temperature the cutting edge can tolerate before it degrades, which is why the recommended cutting speed range moves up with a better coating, from roughly 90 metres per minute uncoated to about 170 with TiAlN on mild steel in the tool's table. The workpiece material's own hardness and thermal behaviour do not change.
What does the tool not tell me?
It checks whether the cutting force, power and chip thickness for a given regime are reasonable right now, not tool life measured in minutes of cutting or number of parts, chatter stability for your specific setup, or the effect of coolant type and tool wear partway through a shift. Those depend on data this calculator does not have, and it says so rather than implying otherwise.
Other tools
Part of the EduFacturing tool set for CNC machining and manufacturing.
The rest of the tool set
A free account opens the full set: cutting data, milling tolerances, quoting, printability checks and the rest.
Create a free accountFree account. No card, no trial period.