CNC Machining Parameters: How to Set Them, Section by Section
Every CNC cut is the result of the same handful of numbers — spindle speed, feed rate, and how deep and how wide the tool engages the material. Get them roughly right and a machine cuts metal all day. Get them wrong and you get burnt tools, chattering cuts, scrapped parts, or a broken end mill in the first five seconds. The difference between those outcomes is rarely talent: it is a repeatable method for setting and then tuning parameters.
This is the reference guide of the machining-parameters topic. It explains the parameter system, gives the conversions you will use constantly, and then walks operation by operation — roughing, finishing, slotting, drilling, turning, thin walls, difficult alloys — because the right recipe changes with the job. Definitions of the terms used here (feed rate, chip load, radial engagement and the rest) live in the CNC glossary; if you need the wider process picture first, start with what CNC machining is.
The parameter stack: what you are actually setting
Four numbers describe almost any cut. They are not independent levers — they are one system, and changing any of them shifts the load, the heat and the finish everywhere else.
| Parameter | What it is | What it controls |
|---|---|---|
| Cutting speed | How fast the cutting edge moves through the material | Heat, tool life, surface quality |
| Spindle speed | The RPM the machine runs, derived from cutting speed and tool diameter | The practical setting you dial in |
| Feed rate | How fast the tool advances into the work | Chip thickness, cutting forces, finish, cycle time |
| Depth of cut (axial) / radial engagement | How far the tool engages along the spindle axis and sideways | Material removal rate, tool load, chatter, deflection |
The mental model to hold onto: cutting speed is chosen by the material, spindle RPM is then calculated from it and the tool diameter; chip load (feed per tooth) is chosen by the tool, and feed rate is then calculated from it, the RPM and the number of flutes. Depth and width of cut are chosen by the operation — roughing wants the most material removed, finishing wants the least damage done.
The two most common beginner mistakes come from breaking this system: treating spindle RPM as the thing you “look up” (it isn’t — cutting speed is), and setting a feed rate without reference to chip load (which is how tools rub instead of cut).
The two conversions that drive everything
You will use two formulas on every job. Learn them once and the numbers stop being magic.
Cutting speed → spindle speed. Cutting speed (surface speed) is expressed in surface feet per minute (SFM) or metres per minute, and it is the same for a given material and tool regardless of tool size. Convert it to RPM with the tool diameter:
- Metric: RPM = (cutting speed in m/min × 1000) ÷ (π × tool diameter in mm)
- Imperial: RPM = (SFM × 12) ÷ (π × tool diameter in inches), or the common shortcut RPM = SFM × 3.82 ÷ tool diameter
Smaller tools need more RPM to reach the same surface speed — which is why a 3 mm end mill spins at many times the RPM of a 25 mm one doing the same material. When a spindle cannot reach the RPM a small tool wants, the cutting speed is effectively capped and the parameters must be reduced to match.
Chip load → feed rate. On a mill, the meaningful number is the thickness each flute removes per revolution — the chip load or feed per tooth. Feed rate follows:
- Feed (mm/min) = RPM × feed per tooth × number of flutes
- Feed (in/min) = RPM × feed per tooth × number of flutes
Turn that around and you have the check that catches most mistakes: chip load = feed rate ÷ (RPM × flutes). If the number that comes out is implausibly small, the tool is rubbing, not cutting. Turning uses a different convention — feed per revolution (mm/rev or inches/rev) rather than per tooth — because a single-point tool cuts with one edge.
Two secondary rules are worth memorising. Material removal rate (MRR) is axial depth × radial engagement × feed rate — the number roughing chases. And when radial engagement drops below roughly half the tool diameter (trochoidal paths, and much finishing), chip thinning kicks in: the chip each tooth takes is thinner than the feed-per-tooth suggests, so feed should be raised to restore a real chip — that is precisely the trick high-efficiency milling exploits.
Where the starting numbers come from
Nobody should derive cutting speeds from first principles on the shop floor. You start from two places and let the tool prove or correct them.
- Tool manufacturer data is the best source. Every serious cutting-tool maker publishes starting speeds and chip loads for their tools by material, and those numbers already account for their tool geometry and coating. When a catalogue is available, use it.
- General machinability charts fill the gap. The principle underneath every chart is simple: cutting speed tracks how easily the material cuts. Free-machining aluminium runs hot and fast; brass and mild steel sit in a moderate band; stainless, titanium and nickel alloys run slow, and hardened tool steel slower still. Carbide cuts at several times the speed of high-speed steel; coated tools at a premium over uncoated.
Typical starting points for carbide end mills look roughly like this — treat them as starting points only, and let the toolmaker’s data override them:
| Material | Cutting speed (carbide, starting) | Relative machinability |
|---|---|---|
| Aluminium alloys | High | Very easy — speed-limited by spindle and tool |
| Brass / bronze | Medium–high | Easy |
| Mild steel | Medium | Moderate |
| Stainless steel | Low–medium | Hard — work-hardens |
| Titanium alloys | Low | Very hard — springy, hot, work-hardens |
| Hardened tool steel | Very low | Very hard — slow and abrasive |
Chip load starts small and scales with tool size: tiny tools take a light feed per tooth, bigger tools a heavier one. The ranges published by toolmakers for a given tool diameter are the right frame; general tables for “¼-inch vs ½-inch tool” are only ever a proxy for the actual tool in your holder.
Two corrections apply before you start. Harder setups — thin workholding, long tool overhang, a light machine — all force the numbers down, because the parameters are only ever as good as the stiffness behind them. And high-performance coated tooling earns a step up from base values, while HSS earns a step down.
A repeatable method for setting parameters
Set the four numbers in order, cut, and then tune one variable at a time. In practice:
- Choose the tool and the material, and look up the toolmaker’s cutting speed and chip load for that material.
- Convert cutting speed to RPM using the tool diameter (the first formula).
- Convert chip load to feed rate using the RPM and the number of flutes (the second formula).
- Set axial depth and radial engagement for the operation — deep and wide for roughing, light for finishing — and make sure the machine and holder can take the load.
- Prove the cut out: a dry run first, then a cut in air or on a test piece if the job is expensive.
- Read the result and tune. Chips, sound, finish and tool wear each tell you which way to move (below). Change one variable, cut again, and let the evidence decide.
Most shops that “just can’t get parameters to work” are skipping step 6 — they set numbers from a chart and never tune them to their actual machine, holder and material heat.
How each operation changes the recipe
The starting method is the same everywhere, but every operation bends it toward its own goal.
Roughing chases material removal rate. Run the tool deep enough and engaged widely enough that it is actually removing metal, using the machine’s stiffness and spindle power as the ceiling. Climb milling on a rigid CNC. You want the biggest chip the machine and holder can take without chatter — chips that come off hot and blue are a machine cutting hard; fine dust is a machine rubbing and wasting its time.
Finishing chases size and surface. Drop to a light depth of cut and light radial engagement, and remember that surface finish is set mostly by feed — for a given tool, a coarser feed leaves a rougher surface. A sharp, consistent tool at a moderate feed beats a dull tool at a desperate feed every time. On a ball nose finishing a contour, the stepover between passes sets the cusp height, so tight stepovers are the price of a smooth 3D surface.
Slotting is the hardest case in milling, because the tool is fully buried — radial engagement is the full tool width, so the tool has no room to shed chips and the load is at its peak. The answer is to shorten the effective engagement: take a shallower axial depth, peck or use a high-efficiency strategy that engages less than the full width, and never assume a slot can run the same parameters as a shoulder cut.
High-efficiency milling (HEM / trochoidal) flips the roughing logic: a very light radial engagement (a fraction of the tool diameter) at high axial depth and raised feed. The tool cuts a thin, cool, uniform chip and removes metal surprisingly fast — this is the modern default for pockets and slots, and it is why chip thinning matters: feed must rise to compensate for the thin engagement, or the tool rubs.
Drilling follows its own rhythm. Spot-drill to stop the drill wandering, then drill. Deep holes need peck drilling to break and clear chips; through-spindle coolant or a pecking cycle handles the rest. Feeds are expressed per revolution and are gentler than milling chip loads; speeds are lower than an end mill would run in the same material because the drill’s cutting edges are buried.
Tapping and threading reward restraint. Rigid tapping runs at a modest speed matched to the tap and the control’s ability to synchronise; thread milling is the flexible alternative that uses a normal mill toolpath. Force neither — taps break on feed/speed mismatch more than on anything else.
Turning changes the conventions: the workpiece spins and the tool feeds per revolution (mm/rev), and constant surface speed (CSS) keeps the cutting speed constant as the diameter shrinks during facing — critical, because a face cut runs from large to small diameter in one pass. Depth of cut on a lathe is the radial bite into the bar, and the same roughing-versus-finishing logic applies.
Thin walls and long-reach tools are governed by deflection, not by speed. A thin wall or a long end mill deflects under cutting force, so reduce radial engagement to cut with a lighter force and leave the finishing passes light and even. Chatter here is a geometry problem as much as a speed problem — the fix is often a shorter tool or a different strategy, not just a lower RPM.
Difficult and work-hardening alloys (stainless, titanium, nickel) punish a tool that stops cutting. Keep the edge engaged with a real chip at all times, run at the modest speeds the material demands, use a moderate chip load, and where needed cut with reduced radial engagement to keep the edge in fresh material. Let a tool dwell or rub in work-hardened material and you will find out why it is called work-hardening.
When the machine and setup become the limit
The parameters a chart suggests are only available if the machine can deliver them. The real ceiling on any cut is the weakest link in the chain: spindle power and top RPM, the rigidity of the machine and the holder, the strength of the workholding, and the reach of the tool. A long tool in a light holder on a thin-walled part will chatter at a fraction of the speed the same tool would manage in a stub holder on a stout vise.
Chatter is the signal that you have hit a structural limit, and the answer is almost never “just lower the speed.” Often the productive fix is to change the engagement — lighter radial engagement, a shorter or stiffer tool, better workholding — rather than to slow everything down. Treat the machine and setup as part of the parameter problem, not as a fixed backdrop.
Reading the result and tuning one variable at a time
The cut itself tells you what to do next. Learn to read it:
- Chips are the best sensor. Thick, curled, even chips mean the tool is cutting properly. Fine dust or discoloured powder means rubbing and heat. Chips the wrong colour for the material and coolant tell you the speed is too high or the tool is dull.
- Sound is second. A steady cut has a rhythm. Chatter — a harsh, rattling tone — means a structural or engagement problem (above). A squeal can mean rubbing.
- Surface and tool wear are the slow indicators. A rough or burned finish, and edge wear or chipping on the tool, both point back at the parameter that caused them.
When something is off, change one variable at a time, cut, and judge. Too much heat → reduce cutting speed. Tool rubbing → raise the feed or chip load, not the speed. Chatter → lighten radial engagement or shorten the tool before touching speed. Burnt corners on a slot → the tool is dwelling or the slot engagement is too heavy. Because the parameters form one system, changing two at once leaves you unable to say which one fixed it.
Keep a record of what worked: material, tool, machine, and the parameters that cut cleanly. That record is worth more than any chart, because it is tuned to your machine, your holders and your materials.
Frequently asked questions
What is the difference between cutting speed and spindle speed? Cutting speed is how fast the cutting edge moves through the material, and it is chosen by the material. Spindle speed is the RPM you set on the machine, and it is calculated from cutting speed and tool diameter. You change the tool size, you change the RPM to keep the cutting speed the same.
How do I calculate spindle RPM for a given feed or speed? RPM = cutting speed ÷ (π × tool diameter), with units consistent: metric RPM = (m/min × 1000) ÷ (π × mm), imperial RPM = SFM × 3.82 ÷ inches. Feed then follows from chip load: feed = RPM × feed-per-tooth × number of flutes.
What should the feed rate be for milling? Set it from the chip load (feed per tooth) the toolmaker recommends for the tool diameter and material, not from a standalone “feed rate” guess: feed = RPM × feed-per-tooth × flutes. If the resulting chip load is implausibly thin, the tool is rubbing.
Why is my tool chattering? Chatter is usually a stiffness and engagement problem, not purely a speed problem. Lighten the radial engagement, use a shorter or stiffer tool, or improve the workholding — then adjust speed if the tone persists. Dropping speed alone often just slows the chatter down.
Why does my end mill rub instead of cut? The chip load is too low — the tool is spinning faster or feeding slower than the chip thickness it needs, so it polishes the material instead of cutting it and burns itself doing it. Raise the feed (or the feed-per-tooth), not the speed.
What parameters should I use for aluminium vs steel? Aluminium cuts at high cutting speed with a healthy chip load; steel runs at a fraction of that speed. The general principle is that cutting speed follows machinability — but always start from toolmaker data for the specific tool and adjust from the chips, not from a remembered number.
Do I set feeds and speeds in CAM or on the machine? In CAM — that is where the tool, material and operation are defined, and where you can simulate. The machine control then runs what the program says. The skill is the same either way: know the conversions, start from data, and tune one variable at a time until the chips are right.
Bottom line
Machining parameters are a system, not a list of magic numbers. Cutting speed comes from the material, spindle speed and feed are derived from it and the tool, and depth and width of cut come from the operation. Start from toolmaker data, convert carefully, prove the cut, and then read the chips and tune one variable at a time — respecting the stiffness of your machine, holder and setup as the real ceiling. Do that, and the same four numbers will serve you from a first prototype to a thousand-part production run.
This guide is part of the CNC Media guides library — practical reference content for the shop floor, kept current as tooling and strategies evolve.