When Using a 5-Axis CNC to Machine Such Small Parts

• 1
  Why 5-Axis CNC Small Parts Are Rarely Limited by the Machine
• 2
  Workholding: The First Thing That Breaks on Tiny Parts
• 3
  Tool Runout and Deflection Decide the Tolerance
• 4
  Heat, Coolant, and Why Small Parts Move
• 5
  Material Behaviour Changes at Small Scale
• 6
  Setup Sequence for Small Parts on a 5-Axis Machine
• 7
  5-Axis CNC Small Parts vs 3-Axis: Which Setup Fits

A 5-axis CNC machine does not know how big the part is. It moves a spindle along a path and the path is written in the CAM file. A 12 mm aluminium bracket and a 400 mm housing run on the same machine with the same controller. The travels are not the problem because the part sits in the middle of a much larger envelope.

The limit shows up somewhere else. On a small part, the ratio of tool diameter to feature size gets close to one. A Ø3 mm end mill cutting a 3.2 mm pocket has almost no room to clear chips. The tool rubs instead of cutting, and rubbing turns into heat in a place where there is very little material to absorb it.

Mass matters too. A 20 g aluminium part heats up far faster than a 2 kg one under the same cutting energy. Its dimensions move while the tool is still in the cut. This is why a 5-axis job on small parts often fails on finish and tolerance long before it fails on reach or axis count.

So the question is not whether a 5-axis machine can reach the part. It can. The question is whether the setup, the tool, and the coolant can hold the part still and cold enough for the tolerance to mean anything.

• 1
  Reach is easyA Ø400 mm rotary table and 4,000 mm travels cover any small part.
• 2
  Chip clearance is hardSmall pockets and deep slots trap chips against the cutter.
• 3
  Heat is harderLow mass means fast thermal growth and fast contraction.

Cutting force scales with depth of cut and tool engagement, not with part size. A 400 mm housing in a vise resists that force with its own mass. A 15 mm cube does not. If the vise jaw pressure is low, the part lifts. If the jaw pressure is high, the part deforms and springs back when you release it.

The fix is to stop relying on the vise. Glue fixtures, also called glue chucking, bond the blank to a flat plate with cyanoacrylate or a hot-melt adhesive. The whole bottom face becomes the fixture. Cutting force goes straight into the plate, and there is no jaw pressure to distort the part.

For parts with a flat back, a vacuum chuck works the same way with less cleanup. For parts that need five-sided access, a dovetail blank leaves a small tab that you cut off in a second op. The tab costs one extra setup and removes almost all chatter risk.

There is a limit. Glue fixtures do not like heavy roughing or hot chips. If you need to remove half the blank in one pass, use a soft-jaw pocket cut to the part profile and leave 0.3 mm of stock for a finishing pass after stress relief.

• 1
  Glue chuckingBest for thin plates and parts under 30 mm.
• 2
  Dovetail blankBest when all five faces need machining.
• 3
  Soft jawsBest for small runs with a simple outside profile.

A 0.01 mm runout on a Ø3 mm tool is 0.3 percent of the diameter. On a Ø12 mm tool it is 0.08 percent. The same holder error hurts four times more on the small tool. That is why small-part work lives or dies on tool holders, not on the machine's positioning accuracy.

Use a shrink-fit or hydraulic holder for anything under Ø6 mm. Both hold runout under 0.005 mm at 3× diameter. A standard ER collet chuck is fine for roughing but will drift once the collet nut wears. Check runout with a dial indicator before every finishing pass, not once a month.

Deflection follows the same logic. A Ø2 mm carbide end mill at 3× diameter depth has a length-to-diameter ratio of 3, which is stiff. The same tool hanging 30 mm out has a ratio of 15, and it will bend under a normal finishing load. Keep tool overhang under 5× diameter whenever the geometry allows, and reduce stepover instead of increasing overhang.

If the part has deep ribs or narrow slots, a necked tool with a relieved shank reaches further without the full-length stiffness penalty. The relief costs some rigidity, so take lighter radial passes: 3 to 5 percent of tool diameter for the finishing pass.

• 1
  Under Ø6 mmShrink-fit or hydraulic holder, runout under 0.005 mm.
• 2
  OverhangKeep below 5× diameter for finishing passes.
• 3
  Necked toolsReach deep slots, but cut lighter radially.

Aluminium expands about 23 μm per metre per degree Celsius. A 20 mm feature grows 0.46 μm for every degree it warms. That sounds small until you remember that a dry cut can raise the part temperature 10 to 20 °C in a few seconds. Now the feature moved 5 to 9 μm, which is the whole tolerance budget.

The answer is not to cut slower. Cutting slower puts more heat into the part because the tool rubs longer. The answer is to cut faster and smaller. High spindle speed, light radial engagement, and a fast feed keep the heat in the chip, and the chip leaves with the heat.

On small parts, air blast or minimum quantity lubrication usually beats flood coolant. Flood coolant on a 15 g part can chill it unevenly, and the part moves as the coolant flows around it. Air blast removes chips and keeps the temperature stable without the thermal shock.

If the job needs flood coolant for chip evacuation, let the part sit in the machine for a few minutes before the finishing pass. The part and the fixture reach the same temperature, and the last pass cuts a stable size. This single pause fixes more small-part tolerance problems than any machine upgrade.

• 1
  Air blastBest for light finishing on aluminium and brass.
• 2
  MQLGood chip evacuation with little thermal shock.
• 3
  FloodUse for deep pockets, but let the part stabilise first.

6061-T6 aluminium is the default for 5-axis CNC small parts. It machines clean, holds a good finish, and does not build up on the cutter at the surface speeds a small tool needs. 7075 gives more strength but is more prone to chipping on thin walls, so keep the wall above 0.8 mm unless the design demands less.

Stainless 303 and 17-4PH behave differently. 303 is free-machining and fine for small parts, but it work-hardens if the tool dwells. Keep the feed per tooth up and never let the cutter rub. 17-4PH in the H900 condition is strong and stable, but it needs sharp tools and a rigid setup because the cutting forces are higher than aluminium at the same volume.

Plastics are the opposite problem. POM and PEEK cut well but move with temperature, and they scratch easily. Use a sharp, polished tool with a high rake angle and air blast. Never use coolant on POM; it absorbs moisture and grows after machining.

Titanium Ti-6Al-4V is where small-part 5-axis work gets expensive. The tool wears fast, the heat stays in the cut, and the material springs back. Expect to change tools more often and to keep the radial engagement under 5 percent of diameter.

• 1
  6061-T6Default choice for small aluminium parts.
• 2
  303 stainlessFree-cutting, but do not let the tool dwell.
• 3
  POM and PEEKAir blast only, no coolant.
• 4
  Ti-6Al-4VLight radial engagement, frequent tool changes.