CNC Parameter Guide: How Cutting Settings Shape Your Part

• 1
  Key points before you read further
• 2
  What a CNC parameter actually controls
• 3
  Why the same parameters behave differently on aluminium and steel
• 4
  Reading the machine: what the sound and chips tell you
• 5
  Machine capability and setup limits that override the numbers
• 6
  Starting values and where to adjust first
• 7
  Step by step: dialing in a new job
• 8
  Parameter starting ranges by material and operation

A CNC parameter is a number the controller uses to move the machine or compensate for geometry. Some parameters are cutting values you program per operation, such as feed rate and spindle speed. Others are machine constants set at commissioning, such as backlash compensation or servo gain. This CNC parameter guide deals with the first group, because those are the ones a process engineer can still change when a job is on the table.

The cutting values work as a set. Feed rate is the linear speed of the tool through the material, usually in mm/min. Spindle speed is rotation, in rpm. Divide feed by (speed × number of flutes) and you get chip load, the thickness of material each tooth removes per revolution. That single derived number explains most of what happens at the edge: too thin and the tool rubs, too thick and it snaps.

Depth of cut and stepover describe engagement. Axial depth is how deep the tool sinks along its axis. Radial stepover is how much of the cutter diameter is buried in the side wall. Both raise cutting force, but radial engagement raises it faster. Reducing stepover from 50% to 25% of diameter often lets you double the feed and still cut stably.

Tool offset sits in a different category. It tells the controller where the tool edge really is relative to the programmed path. Length offset handles the Z position, radius offset handles the side wall. Get them wrong and every dimension shifts by a constant, which is why offset errors look like a size problem rather than a cutting problem.

Aluminium 6061 and 7075 cut at surface speeds that would burn a high-speed steel cutter in steel. On a 10 mm carbide end mill, 6061-T6 commonly runs at 300–500 m/min surface speed, which on a 10 mm tool is roughly 9,500–16,000 rpm. That is only usable on a spindle rated for it. Many 3-axis machines top out near 8,000–12,000 rpm, so the achievable surface speed is set by the machine, not the material chart.

Steel 4140 and 4340 sit far lower, often 120–180 m/min with coated carbide. Stainless 316 and 17-4PH are lower still and work-harden if the tool dwells. The practical rule is to keep the chip load up and never let the cutter rub. A light pass at low feed on 316 is worse than a heavier pass at correct feed, because the rubbing pass hardens the surface and dulls the next tooth.

Titanium TC4 (Ti-6Al-4V) adds heat management to the list. It conducts heat poorly, so the edge absorbs it. Surface speeds of 40–70 m/min with generous coolant and a rigid setup are typical. Inconel is slower again. When a shop quotes a long cycle time for these alloys, the parameters are usually the reason.

Plastics invert some of the logic. POM and PEEK cut fast but melt if the chip cannot clear. Feed per tooth around 0.1–0.2 mm and an air blast often work better than flood coolant, which can trap chips in a deep pocket. ABS and PC are softer and need sharp edges to avoid a gummy finish.

Chip shape is the cheapest diagnostic you have. On aluminium, a proper chip is a short comma or a 6–9 shape that breaks and clears. Long stringy chips mean the feed is too low for the speed, so the edge is rubbing. Fine powder means the feed is far too low or the tool is dull. On steel, chips that come off blue and thin usually mean the edge is overheating.

Sound is next. A steady hum across the cut is normal. A rhythmic thump once per tooth usually points to runout or a loose insert. A high-pitched squeal that starts mid-pass is chatter, and chatter almost always traces back to radial engagement or tool overhang rather than to the spindle speed itself. Shorten the overhang before you touch the speed.

Surface finish records the outcome. Ra 1.6–3.2 μm is a normal as-machined result. Ra 0.8–1.6 μm needs a controlled finishing pass with a consistent chip load. Ra 0.2–0.8 μm usually needs a separate finishing strategy, sometimes a smaller tool with a light stepover, or a secondary operation. If the finish changes across the same face, the problem is rigidity or thermal drift, not the feed number.

Measure the part before you change anything. If size drifts in one direction over a run, suspect thermal growth in the spindle or the tool pulling out of the holder. If one feature is wrong and the rest are correct, suspect the offset. Only when dimensions are right and the surface is wrong should you start editing cutting parameters.

Parameter charts assume a rigid setup. On a machine with 4,000 × 400 × 150 mm travel, a long slender part flexes under the same cutter that cuts cleanly on a 500 × 500 × 450 mm machine. The fixture, not the controller, sets the ceiling. That is why a proven program can fail when it moves to another cell.

Spindle taper and holder quality matter as much as rpm. A tool held with 0.02 mm runout will cut a different width than the same tool held with 0.005 mm runout. Runout loads one flute harder, and that flute fails first. Check runout at the tool tip, not at the holder face.

Coolant strategy changes the usable window. Through-spindle coolant lets deep holes and pockets run at higher feed because chips leave the cut. Without it, you either reduce feed or accept recutting. On a 16 simultaneous 5-axis center, the extra axes let you tilt the tool and keep a consistent engagement angle on a curved surface, which is often a bigger gain than any single parameter tweak.

Roughly 127 high-precision CNC machines across the shop mean a job may be routed to a 3-axis, 4-axis, mill-turn or 5-axis platform. Each platform has a different stiffness and spindle range, so the same part number can carry two parameter sets and still be correct.

For roughing aluminium 6061 with a 10 mm carbide end mill, a workable window is 350 m/min surface speed, 0.08–0.12 mm feed per tooth, 50% radial stepover and axial depth up to 1× diameter. If the machine lacks the rpm, reduce the diameter rather than the chip load. A 6 mm tool at the same chip load is a better answer than a 10 mm tool run at half feed.

For finishing, reduce stepover first, not feed. A 0.2–0.5 mm stepover with a maintained chip load produces the Ra 0.8–1.6 μm band. Lowering feed instead tends to smear the surface and shorten tool life. On stainless, keep the finishing pass continuous so the tool never dwells in one spot.

When a cut is unstable, the order of adjustments is: shorten tool overhang, reduce radial stepover, then adjust speed. Increasing feed slightly can also settle chatter, because it changes the tooth-passing frequency. Work through that list before rewriting the program.

For drilling, peck depth and feed per revolution control chip evacuation. A peck of 1× diameter on steel and 2–3× diameter on aluminium usually clears chips without wasting cycle time. Tapping torque scales with hole size, so pilot diameter and lubricant matter more than spindle speed on small taps.