A summary of CNC parameters commonly used for CNC machine tools

• 1
  Key takeaways
• 2
  What CNC parameters actually control
• 3
  Cutting speed, feed rate and depth of cut
• 4
  Tolerance, surface finish and material removal rate
• 5
  When the numbers stop working
• 6
  Why the setup decides the outcome
• 7
  How we set parameters on the floor
• 8
  Typical CNC parameters by material and operation

Every cut on a CNC machine tools comes down to a small set of numbers. Spindle speed, feed rate, depth of cut, stepover, coolant, and the geometry of the cutting edge. The control turns those into motion, but the physics underneath is simple: a cutting edge shears material, generates heat, and wears out.

The useful way to read a CNC parameters table is not to memorize values. It is to understand which lever does what. Speed and feed trade off against each other through chip load. Depth of cut drives cutting force. Stepover drives the number of passes and therefore cycle time.

A parameter that is right for 6061 aluminium is wrong for 316 stainless. Thermal conductivity, work hardening, and chip formation all change the window. That is why a shop running a wide material list keeps separate starting points rather than one universal chart.

One more thing worth stating early. CNC parameters describe the cut, not the part. Two shops can run the same values and produce different results because of machine rigidity, tool holder quality and how the workpiece is held.

• 1
  SpeedSurface speed at the cutting edge, in m/min or SFM
• 2
  FeedAdvance per tooth or per revolution, in mm/min or IPM
• 3
  Depth of cutRadial and axial engagement of the cutter
• 4
  Chip loadFeed per tooth; the value that ties speed and feed together

Cutting speed is written as surface speed, not spindle RPM, because the same RPM means different edge speeds on a Ø6 mm end mill and a Ø50 mm face mill. In aluminium we commonly run 300–600 m/min with carbide. Mild steel sits around 120–200 m/min. Stainless and titanium drop to 40–90 m/min because the heat stays in the edge.

Feed rate is quoted as feed per tooth. A three-flute Ø10 mm cutter at 0.05 mm per tooth and 8,000 rpm gives 1,200 mm/min. Push the chip load too low and the edge rubs instead of cutting, which work-hardens stainless and kills tool life faster than a heavy cut would.

Depth of cut is the roughing lever. On a rigid setup we take axial depths up to one tool diameter and radial engagement of 30–50 percent. Many light passes add tool changes and heat without removing material faster. On thin walls or long overhangs, the opposite applies.

Stepover matters as much as depth. A 10 percent stepover on a finishing pass spreads wear across the flute and holds a better finish. A 70 percent stepover in a corner overloads the cutter. High-efficiency roughing paths keep radial engagement low and axial engagement high for that reason.

Spatial tolerance describes how closely the machine can place a feature where the drawing says it should be. On our 5-axis centers we hold ±0.005 mm (±0.0002 in) on critical features. Standard work usually lands between ±0.01 and ±0.05 mm, which is where most industrial parts actually need to be.

Surface finish is measured as Ra, the arithmetic mean roughness. As-machined aluminium typically comes off at Ra 1.6–3.2 μm. A careful finishing pass with a sharp tool gets Ra 0.8–1.6 μm. Below Ra 0.8 μm you are usually looking at a secondary operation, not a parameter change.

Tolerance and finish are separate costs. A bore that must be ±0.005 mm can still be turned with a coarse finish if the drawing allows it. A cosmetic face at Ra 0.4 μm may need no tight tolerance at all. Read the drawing before assuming both are needed.

Material removal rate ties the three together: depth times stepover times feed. It predicts cycle time, not quality. Chasing a high removal rate on a finishing pass is how parts end up out of tolerance.

Chatter is the clearest sign that a parameter set has hit a wall. The tool and workpiece start vibrating at a natural frequency, leaving a rippled surface. Reduce radial engagement or change spindle speed first. Adding a heavier cut sometimes settles it, which feels wrong until you see the stability lobe diagram.

Tool runout is the quieter problem. A cutter with 0.03 mm of runout loads one flute harder than the others. The feed rate that looked conservative on paper becomes aggressive on that one edge. Good holders and a dial indicator catch this before it becomes a broken tool.

Deep pockets and long tools shift the limit again. A Ø6 mm cutter sticking 60 mm out of the holder has a fraction of the stiffness of the same cutter at 20 mm. On jobs like that we cut parameters by 30–50 percent and accept the extra time.

Heat is the other boundary. Titanium and Inconel do not carry heat away from the edge, so surface speed has to drop and coolant flow has to be high. Running aluminium speeds on Ti-6Al-4V destroys tools in minutes.

A parameter table assumes a rigid machine, a sharp tool in a good holder, and a workpiece that does not move. Break any of those and the numbers stop predicting anything. We have seen a 20 percent feed increase work fine on one fixture and chatter on the next one.

Workholding is usually the weak link. Thin plates deflect under clamp pressure. Tall parts vibrate. A part held in a soft jaw on 5 mm of material behaves differently from the same part in a dedicated fixture.

Tool holder quality shows up in runout and in how quickly the edge dulls. Hydraulic and shrink-fit holders hold runout under 0.005 mm. A worn collet chuck can triple that, and the operator compensates by slowing everything down.

So the honest summary is this. CNC parameters give you a starting point and a vocabulary for troubleshooting. The craft is in reading the cut, listening to the spindle, and knowing which number to move when the surface changes.

We keep a per-material starting sheet for aluminium, stainless, steel, titanium and plastics. It lists surface speed and chip load bands per operation. The programmer picks a band, then the machinist adjusts on the first part.

For prototypes and short runs we bias toward tool life rather than cycle time, because a broken tool costs more than a slower pass. On 10,000-part runs we re-time the job after the process is proven, sometimes cutting cycle time by a quarter.

Inspection closes the loop. With 100 percent inspection before shipment, a drifting dimension shows up as a trend rather than a surprise at the end of the run. That data goes back into the parameters.

We hold ±0.005 mm on critical features and Ra 0.2–0.8 μm when a drawing calls for it. Both are achievable, but both cost time. Sending us a drawing with those values marked only where they matter keeps the quote honest.