Understand CNC Machining Parameters
Cutting speed, feed, depth of cut, stepover and tool geometry set the result before the spindle turns. This guide explains how each parameter moves surface finish, tolerance and cycle time, so you can read a setup sheet and argue with it.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
Understand CNC machining parameters: cutting speed and feed
Two numbers dominate every milling or turning operation: surface speed (Vc, in m/min or sfm) and feed per tooth (fz, in mm/tooth). Surface speed is how fast the cutting edge travels through the material. Feed per tooth is how far the edge advances per revolution divided by the number of flutes. Multiply them correctly and you get chip load, which is the real number the tool feels.
Surface speed mostly drives heat and tool wear. Push aluminum at 300–500 m/min and the chips carry heat away fast. Push titanium at the same speed and the edge fails in minutes, so Ti-6Al-4V typically runs at 40–60 m/min with high-pressure coolant. Feed per tooth controls chip thickness and therefore cutting force.
Too light a chip load rubs instead of cuts. The edge work-hardens the surface, especially on 304 stainless and 17-4PH, and the next pass cuts through a harder skin. Too heavy a chip load overloads the flutes and the part moves in the vise. Both extremes show up as poor finish and drifting dimensions, not as a clean tool break.
A practical starting point for 6061-T6 with a 10 mm carbide end mill: 350 m/min, 0.05 mm/tooth, four flutes. For 304 stainless with the same tool: 120 m/min, 0.03 mm/tooth. Run one test cut, measure the chip, then adjust. Thin, silver chips on aluminum mean you are close. Blue or powdery chips mean back off.
Depth of cut, stepover and tool load
Axial depth of cut (ap) is how deep the tool bites along its axis. Radial width of cut (ae) is the stepover, the side engagement per pass. These two numbers decide how much of the flute is in the material, which sets deflection and heat. A tool buried 2 mm deep and 0.5 mm wide behaves very differently from one cutting 0.5 mm deep and 8 mm wide.
Modern CAM strategies trade depth against width. High-efficiency milling uses light radial engagement, often 5–10% of tool diameter, with axial depth up to 1–2× diameter. The small radial bite keeps the chip thin and the heat low, so you can remove material fast on a 27-machine 3-axis floor without stalling the spindle.
On thin walls and long tools, deflection beats everything else. A 6 mm end mill hanging 60 mm out of the holder will spring away from the cut no matter how good the numbers look. Reduce stepover, take a finishing pass with a 0.2 mm radial bite, or move to a shorter tool. On a part held in soft jaws, the same cut can lift the workpiece instead of cutting it.
For roughing, aim to keep the tool engaged but not buried. On 6061 with a 12 mm end mill, 1.5 mm axial and 6 mm radial is a safe start. For 4140 steel, drop to 0.8 mm axial and 4 mm radial. Climb milling is the default on CNC machines with backlash-free ball screws; conventional milling only makes sense on older machines or when breaking through a hard scale.
How stepover and tool radius set surface finish
Theoretical surface roughness in milling comes from the scallop left between passes. A ball nose tool with radius R and stepover ae leaves a cusp height h roughly equal to ae² divided by 8R. Halve the stepover and you cut the cusp to a quarter. That single relationship explains why finishing passes are slow.
To hit Ra 0.8–1.6 μm on a typical aluminum part, a 6 mm ball tool at 0.2 mm stepover is usually enough. For Ra 0.2–0.8 μm, drop the stepover to 0.05–0.1 mm and use a fresh tool. Worn edges smear the surface and leave a torn finish that no polishing step fully hides.
Tolerance is a different problem. Achievable tolerance depends on machine geometry, thermal stability and fixturing, not on the finishing pass alone. A machine that holds ±0.005 mm on a 100 mm aluminum part may only hold ±0.02 mm on a 300 mm steel part that heats up during the cut.
Sharp internal corners are the classic trap. A Ø6 mm cutter cannot produce a corner radius below 3 mm, and a square corner needs EDM or a relieved tool. Design the corner radius at least 1 mm larger than the tool radius if you want a clean, repeatable cut.
Tool geometry, coating and when it changes the answer
Tool material and coating shift the usable window more than any single feed number. Uncoated carbide suits aluminum and most plastics. TiAlN and AlTiN coatings handle steel and stainless at higher speeds but fail fast on aluminum because of the aluminum pick-up on the coating. DLC coatings are the opposite: they work well on aluminum and poorly on steel.
Geometry matters just as much. A two-flute tool clears chips in deep pockets and slots but leaves a rougher floor. A four-flute tool finishes better and feeds faster but needs more chip room. Variable helix tools reduce chatter on long reach cuts. For tapping, spiral flute tools pull chips out of blind holes; spiral point tools push them forward and suit through holes.
Rigid setups forgive bad numbers. A tool held in a shrink-fit holder with 25 mm of gauge length will hold size far better than the same tool in a worn collet chuck at 80 mm. Before you tune feeds and speeds, check runout. Anything above 0.01 mm TIR on a finishing tool shows up in the finish.
Plastics and composites need their own logic. PEEK and carbon fibre wear carbide quickly, so use diamond-coated or polished tools and keep the chip load high enough to avoid rubbing. Melting, not tool wear, is usually the failure mode on ABS, PC and PMMA.
When parameter tuning stops helping
Some problems are not parameter problems. Chatter that survives three feed changes is usually a stiffness problem: too much tool overhang, a weak vise, or a thin floor in the part. Adding a support, shortening the holder or switching to a smaller radial bite does more than any speed change.
Thermal drift is the other silent one. A spindle running for hours grows, and a part that measured on size at 8 a.m. can drift out of tolerance by noon. On tight jobs, rough in the morning, let the part cool, then finish. That sequence costs one setup but saves scrap.
Material condition matters too. 6061-T6 from one mill can cut differently from the same alloy at another. Hardness variation in castings and forgings shows up as a changing finish across the part. If the finish changes halfway through a pass, suspect the material, not the program.
Finally, know when to stop tuning. If the part meets the drawing and the cycle time is competitive, extra optimization adds risk without adding value. The goal is a stable process you can repeat on the next order, not the fastest single run.
Starting parameters by material and operation
Values are starting points for carbide tooling. Adjust after the first test cut and confirm against your own machine.
| Material | Roughing (Vc / fz) | Finishing stepover | Typical result |
|---|---|---|---|
| 6061-T6 aluminum | 350 m/min / 0.05 mm | 0.2 mm ball, 6 mm | Ra 0.8–1.6 μm |
| 7075 aluminum | 300 m/min / 0.05 mm | 0.15 mm ball, 6 mm | Ra 0.8–1.6 μm |
| 304 stainless | 120 m/min / 0.03 mm | 0.1 mm ball, 6 mm | Ra 0.8–1.6 μm |
| 17-4PH stainless | 100 m/min / 0.03 mm | 0.1 mm ball, 6 mm | Ra 0.8–1.6 μm |
| 4140 steel | 150 m/min / 0.04 mm | 0.15 mm ball, 8 mm | Ra 1.6–3.2 μm |
| Ti-6Al-4V | 50 m/min / 0.02 mm | 0.1 mm ball, 6 mm | Ra 0.8–1.6 μm |
| Inconel 718 | 30 m/min / 0.015 mm | 0.08 mm ball, 6 mm | Ra 1.6–3.2 μm |
| POM / PEEK | 400 m/min / 0.06 mm | 0.2 mm ball, 6 mm | Ra 0.8–1.6 μm |
Which parameters to change first
If the finish is bad, cut stepover first; if the tool breaks, cut feed per tooth; if dimensions drift, fix fixturing and thermal stability before touching speed. Change one variable at a time and keep a record of what worked.
Common questions on machining parameters
Can I run the same parameters on a 3-axis and a 5-axis machine?
The cutting numbers are the same, but the 5-axis setup changes the effective stiffness. With the part tilted, gravity and the rotary table add load paths that a flat 3-axis setup does not have. Start conservative on the first 5-axis run and confirm the finish before pushing feed.
Short tools still win. On a 5-axis machine you can often reach a feature with a shorter tool than on a 3-axis setup, and that alone lets you raise the feed.
How do I know if my chip load is right?
Look at the chip. On aluminum, a thin, curled, silver chip means the load is in range. A powdery chip means rubbing, so raise feed per tooth. A thick, blue chip means too much heat, so reduce surface speed or increase coolant pressure.
On steel, a short, comma-shaped chip is normal. Long stringy chips wrap around the tool and cause poor finish, so break the chip with a higher feed or an insert with a chip breaker.
Does coolant always help?
No. Flood coolant helps on steel, stainless and titanium because it removes heat from the edge. On some cast irons, coolant causes thermal shock and cracks the insert, so dry cutting is preferred.
On aluminum, high-pressure coolant clears chips from deep pockets, which matters more than cooling. On plastics, air blast is often better than liquid coolant.
What surface finish can I expect from a standard as-machined part?
A normal milled or turned surface sits around Ra 1.6–3.2 μm. A finishing pass with a sharp tool and small stepover reaches Ra 0.8–1.6 μm. Below Ra 0.8 μm you need a dedicated finishing strategy or a secondary process.
If the drawing calls for Ra 0.2–0.8 μm, plan for a separate finishing operation with a fresh tool, not a tweak to the roughing pass.
How many test parts should I run before production?
One test cut tells you whether the tool survives. A first article tells you whether the dimensions hold across the feature set. On tight-tolerance parts, run the first article, measure it fully, then adjust and run a second before releasing the run.
For a 10,000-part order, the cost of two scrap parts is irrelevant next to the cost of a process that drifts at part 4,000.
Do these numbers apply to turning as well?
The same logic applies, but the geometry differs. On a lathe, feed is per revolution, not per tooth, and depth of cut is measured radially. Surface speed is still the main driver of tool life.
For turning 304 stainless, 180 m/min with 0.2 mm/rev and 1.5 mm depth of cut is a reasonable start. Insert grade and chip breaker matter more on a lathe than on a mill.
Send us the drawing and the material
We review the geometry, pick the parameters and tell you what finish and tolerance the part can actually hold. Quotation and free DFM analysis within 12 hours.
12-hour quote100% inspection±0.005 mm toleranceNo minimum order quantity
More machining notes from GreatLight
We publish setup notes, tooling trials and inspection data from the factory floor.
