CNC Is Commonly Used With 8 Shop Formulas: What Each One Tells You

• 1
  Cutting Speed and Spindle Speed
• 2
  Feed Rate and Chip Load
• 3
  Cutting Power and Spindle Torque
• 4
  Material Removal Rate and Machining Time
• 5
  Theoretical Surface Finish and Where It Breaks Down
• 6
  How CNC Is Commonly Used Across Part Types and Materials
• 7
  The 8 Formulas, What They Predict and Their Limits

Cutting speed is the surface speed of the tool edge against the material, written as V = π × D × n ÷ 1000. Here D is the cutter or workpiece diameter in millimeters, n is spindle speed in rpm, and V comes out in m/min. The constant 1000 only converts millimeters to meters. In imperial shops the same idea runs as V = π × D × n ÷ 12, with D in inches and V in surface feet per minute.

The practical version works backward. You pick V from the material and tool grade, then solve n = 1000 × V ÷ (π × D). A Ø10 mm carbide end mill running 120 m/min turns at roughly 3,820 rpm. The same cutter in 6061 aluminium can run 300 m/min, which lands near 9,550 rpm. The formula does not care about the machine.

This is where the first boundary shows up. Spindle speed on a real machine is capped. A 12,000 rpm spindle cannot reach the number for a Ø3 mm cutter in aluminium, and a 4,000 rpm spindle cannot reach it for most small tools. When the calculated n exceeds the spindle limit, you stay at the limit and accept the lower surface speed. Feed per tooth carries the rest.

Diameter matters more than most people expect. Halve the tool diameter and surface speed halves at the same rpm. That is why small tools burn up: the edge is moving slower than the chip load assumes, rubbing instead of cutting. If a Ø2 mm tool keeps dulling, check the actual surface speed before blaming the coating.

Feed rate ties spindle speed to how much material each tooth removes. The form is F = n × z × fz, where n is rpm, z is the number of flutes, and fz is feed per tooth in mm. A 4-flute cutter at 3,820 rpm with fz = 0.05 mm gives 764 mm/min. Write the units down every time. Mixing inches and millimeters here is the most common arithmetic error on the floor.

Chip load is not a free variable. It has a floor and a ceiling set by the tool and the material. Below the floor the edge rubs, work-hardens the surface and wears fast. Above the ceiling the tool deflects, the finish tears and something breaks. For a Ø10 mm carbide end mill in 6061, a working band is roughly fz = 0.03–0.08 mm. In 304 stainless the band narrows to about 0.02–0.05 mm.

Radial and axial depth change the picture. Full-width cuts in a slot load the tool differently from a 30 percent stepover in a trochoidal path. When you increase depth of cut, reduce fz first. The cutting force scales with chip cross-section, and the tool shank only has so much stiffness.

Watch the chip, not the screen. Thin powdery chips mean you are under the floor. Blue chips with a heavy burr mean you are over it. The formula gives you a starting point within about 20 percent. The machine, the holder and the workpiece rigidity settle the rest.

Cutting power estimates how much energy the cut needs, written as P = (ks × ap × f × V) ÷ (6000 × η). Here ks is specific cutting force in N/mm², ap is depth of cut in mm, f is feed per revolution in mm, V is cutting speed in m/min, and η is machine efficiency. The 6000 constant is a unit conversion. The result is in kW.

Specific cutting force is the number people get wrong. It is not a material constant in the textbook sense. It rises as chip thickness falls, which is why a light finishing pass can need almost as much power per unit volume as a heavy roughing pass. Typical working values are around 700 N/mm² for aluminium, 1,500 N/mm² for mild steel, and 2,000–2,500 N/mm² for stainless and titanium alloys.

Check the result against the spindle nameplate. A 15 kW spindle running at 80 percent efficiency delivers about 12 kW to the cut. If the formula says 14 kW, the machine will stall, trip the drive, or slow the spindle and break the tool. Derating by 20 to 30 percent for continuous cuts is normal practice, not caution.

Torque usually becomes the real limit before power does. At low rpm, power looks fine on paper while torque is exhausted. Large-diameter face mills and tapping operations are the classic cases. If the spindle bogs down at 300 rpm but runs clean at 2,000 rpm, you are torque-limited, and no feed adjustment fixes that.

Material removal rate is the simplest of the eight: MRR = ap × ae × F, where ap is axial depth, ae is radial width of cut, and F is feed rate. All three in the same length unit. A cut of 2 mm axial, 5 mm radial at 764 mm/min removes about 7,640 mm³ per minute. This number drives cost estimates and tool life planning.

Machining time follows from the same inputs. Time = L ÷ F, where L is the total tool path length including approach and retract. Add tool change time and rapid moves and you have a realistic cycle estimate. For a part with 12 tools and 4 setups, the non-cutting time often runs 30 to 50 percent of the total. Ignoring it makes quotes look optimistic.

MRR is a trade, not a score. You can raise it with more depth, more width or more feed, and each one pushes tool load, spindle power or chatter risk in a different direction. The efficient path is usually higher ap and ae with a lower radial engagement, not the reverse. Trochoidal and dynamic paths exist because they keep MRR up while holding radial load down.

Roughing and finishing want different targets. Roughing pushes MRR and accepts Ra 3.2 μm or coarser. Finishing drops to ae of 0.2–0.5 mm, raises surface speed, and aims for Ra 0.8–1.6 μm. Running one set of numbers for both stages wastes either time or finish quality.

Theoretical roughness follows Ra ≈ fz² ÷ (32 × r), where fz is feed per tooth and r is the tool corner radius, both in the same unit. A 0.05 mm chip load on a 0.8 mm corner radius predicts about Ra 0.1 μm. That number is almost never achieved in a real cut, and the gap is the useful part of the formula.

The equation assumes a perfect circular tool path with no deflection, no runout and no vibration. In practice runout of 10 μm on a multi-flute cutter means one tooth does most of the work. Its actual chip load is higher than the average, so the real finish tracks the worst tooth, not the mean. Measure runout with a dial indicator before you trust any finish prediction.

Corner radius is the lever you control. Going from r = 0.4 mm to r = 1.2 mm at the same feed cuts theoretical Ra by two thirds. That is why a small radius tool leaves a rougher floor even with identical parameters. The trade is that a larger radius needs more axial force and can chatter on thin walls.

Use the formula to rank options, not to promise a number. It tells you that halving feed improves finish roughly fourfold and that a bigger radius helps more than a slower feed in many cases. It cannot tell you whether the part will sing at 8,000 rpm. That is a stiffness problem, and it is solved with support, not arithmetic.

CNC is commonly used on parts where tolerance, repeatability and material properties beat what casting or molding can hold. A bracket with a ±0.005 mm bore, a manifold face that must seal, a heat sink with 0.5 mm fins: these are milling and turning jobs. The formulas above size the process, and the process decides whether the part is economical.

Material drives the numbers hard. Aluminium 6061 and 7075 tolerate high surface speed and generous chip load. Stainless 304 and 17-4PH work-harden, so the chip load floor is higher and light rubbing passes are counterproductive. Titanium TC4 and Inconel sit at the other end: low surface speed, modest chip load, and heavy coolant or high-pressure through-tool delivery. The same formula gives very different inputs.

Geometry sets the boundary more often than material. Deep pockets, thin floors and long unsupported walls limit depth of cut long before spindle power does. A part with a 0.8 mm wall cannot be roughed at the MRR the spindle allows. In those cases the answer is a different strategy, not a different number: smaller radial engagement, more passes, and sometimes a change in how the part is held.

Five-axis work changes the arithmetic in a useful way. Tilting the tool keeps the effective cutter diameter and the engagement angle steadier around a contour, which holds chip load close to the programmed value. That is why a 5-axis path often finishes a curved surface in one setup at Ra 0.8–1.6 μm where a 3-axis job needs two setups and hand blending. The formulas still apply. The path just keeps their assumptions truer.