The same tool on the same machine can produce hundreds of parts with one set of cutting parameters and only a handful with another. The most important variables that determine tool life are the cutting parameters the operator controls directly. In this article we explain how they affect tool life and outline an optimization approach you can apply on the shop floor.
Basic cutting parameters
- Cutting speed (Vc, m/min): The peripheral speed of the cutting edge relative to the workpiece.
- Spindle speed (n, rpm): Calculated from cutting speed and tool diameter.
- Feed per tooth (fz, mm/tooth): Related to the chip thickness each flute removes per revolution in milling. Turning uses feed per revolution (fn, mm/rev).
- Axial depth of cut (ap) and radial width of cut (ae): Define the contact area between tool and material.
vf = fz × z × n
Q = (ap × ae × vf) / 1000 [cm³/min]
Q is the metal removal rate and the most direct indicator of productivity.
The Taylor tool life equation
The relationship between cutting speed and tool life is described by the classic Taylor equation:
Here T is tool life, and C and n are constants specific to the tool–material pair. For carbide tools, n is typically in the range of 0.2–0.3. Assuming n = 0.25, increasing cutting speed by 20% cuts tool life roughly in half:
That is why, when you want more productivity, the first move should usually be to increase feed or depth of cut rather than cutting speed. Their effect on tool life is more limited.
Feeds that are too low also hurt
Reducing feed too much to protect the tool can backfire. When chip thickness drops below the cutting edge radius, the tool rubs and ploughs instead of cutting. The result is more heat, work hardening in stainless steels and superalloys, and faster wear.
When the radial width of cut is smaller than half the tool diameter, the actual chip thickness is thinner than the programmed feed per tooth (radial chip thinning):
In trochoidal and high-efficiency milling strategies, feed per tooth is increased to compensate for this effect.
The effect of depth and width of cut
As axial depth of cut (ap) increases, a longer section of the cutting edge is engaged; because the load spreads over a larger area, the effect on tool life is usually limited. Radial width of cut (ae), on the other hand, determines how long the edge stays in contact with the material and therefore how hot it gets. In full slotting, the edge cuts for half of every revolution and has little time to cool. With low radial engagement, the edge cuts briefly and cools for longer.
That is why modern high-efficiency milling strategies combine low ae, high ap and increased fz to keep metal removal rates high while protecting tool life.
Machine power and torque limits
Before increasing parameters, check whether the machine can handle the load. The net cutting power required in milling can be estimated as:
Here kc is the specific cutting force of the material (N/mm²), which varies with chip thickness; tool manufacturers list it by material group in their catalogs. The calculated power must stay below the spindle’s available power at that speed. At low speeds torque is the limit; at high speeds, power is.
Reading wear patterns
A used cutting edge often shows clearly which parameter is wrong:
| Wear type | Likely cause | First correction |
|---|---|---|
| Flank wear | High cutting speed, abrasive material | Reduce Vc, choose a more wear-resistant grade |
| Crater wear | High temperature, diffusion | Reduce Vc, choose a suitable coating |
| Built-up edge (BUE) | Low cutting speed, sticky material | Increase Vc, use a sharp positive geometry |
| Notch wear | Work-hardened surface, constant depth-of-cut line | Vary ap, change the entering angle |
| Edge chipping | Vibration, interrupted cut, excessive feed | Improve rigidity, choose a tougher grade |
| Thermal cracks | Sudden temperature changes | Apply coolant continuously or machine dry |
Parameter optimization on the shop floor
- Start with the manufacturer’s catalog values and reduce them if machine or fixturing conditions require it.
- Define the tool life criterion: flank wear (VB), part count, dimensional or surface limit. ISO 3685 uses an average VB of 0.3 mm as a common criterion in turning tests.
- Change one parameter at a time: feed and depth first, then cutting speed.
- Record the results: parameters, part count, wear appearance, cycle time.
- Decide based on cost per part; the longest tool life is not always the most economical solution.
Coolant type, pressure and direction also directly affect tool life. Especially in titanium and nickel-based alloys, high-pressure coolant extends tool life by carrying heat away from the cutting zone. We cover these materials in our article on machining titanium and Inconel in aerospace.
