Four axis CNC machining guide

• 1
  What the fourth axis actually adds
• 2
  Parts that belong on a four-axis machine
• 3
  Boundaries and failure modes to design around
• 4
  How a four axis CNC machining job runs
• 5
  Fixturing and datums on the rotary table
• 6
  3-axis vs 4-axis vs 5-axis: which fits the part

A 3-axis mill moves the tool in X, Y and Z. The part stays bolted in one orientation, so any feature on a side face needs a second setup. A four axis CNC machining setup adds one rotary axis, usually the A axis turning around X, and sometimes a B axis around Y. The spindle still moves in three linear directions, but the part can now index or rotate while the tool is cutting.

That single rotation changes the geometry you can reach. Holes on four faces, slots that wrap around a shaft, and flat pads at different angles can all be cut without unclamping. On a long part such as a 4,000 mm extrusion, the rotary table holds one end and a tailstock supports the other, so the tool can travel the full length while the part turns.

The axis is not free. A rotary table adds mass, and the controller has to keep the part rigid while the cutter pushes sideways. On our Ø400 mm rotary tables, we keep turning diameters under about 350 mm when the part is long, so the setup stays stiff enough for ±0.005 mm work.

Indexing is the common mode. The table rotates to a position, locks, and the tool cuts as if it were a 3-axis move. Simultaneous motion is the harder mode, where the A axis turns while X, Y and Z move together. That is what produces a smooth blend across a curved face, and it needs a CAM toolpath that treats all four axes as one motion.

The clearest candidates share one trait: features that repeat around a centerline. A drive shaft with keyways and cross holes, a valve body with ports on three sides, a manifold with angled faces, a camera housing with bores on four sides. If the drawing shows the same operation on more than two faces, a fourth axis usually removes a setup.

Setup count is where the money is. Every additional 3-axis setup costs a fixture, a re-zero, and a chance to lose datum. On a part with features on four sides, moving from four setups to one can cut machining hours by 30 to 50 percent and tighten the relationship between features, because everything is cut from the same zero.

Long, slender parts benefit twice. The rotary table and tailstock support the workpiece along its axis, which reduces chatter compared with a vise holding one end. A 500 mm shaft that sings in a vise often cuts cleanly when it is supported at both ends.

The fourth axis also improves surface finish on curved geometry. When the tool stays tangent to a cylindrical face instead of stepping over it in Z, the scallop height drops. We hold Ra 0.8–1.6 μm on turned-and-milled surfaces without a separate finishing operation in many cases.

• 1
  More than two facesFeatures on three or four sides of one part.
• 2
  Round or near-round partsShafts, sleeves, hubs, and bodies with a centerline.
• 3
  Wrapped featuresSlots, pockets or engravings that follow a curve.
• 4
  Long partsLengths up to 4,000 mm with tailstock support.

A fourth axis does not reach everywhere. Deep cavities in the middle of a large block still need a long tool, and the rotary table does not help if the feature faces the wrong way. If a part has undercuts on five sides, or organic contoured surfaces that blend in every direction, the extra reach of a simultaneous 5-axis center is the honest answer.

Rotary work also raises the bar for workholding. A part that hangs far from the chuck acts like a lever, and the cutting force bends it. Keep the unsupported overhang short. When a part is too short to reach the tailstock, we use a fixture plate on the rotary table instead, which restores stiffness but adds a setup.

Tolerance stacking is another trap. If the rotary table has any runout, every indexed face inherits it. We check the table before a tight job and keep turning errors inside ±0.005 mm. On parts where two opposite bores must be coaxial, it is usually better to bore them in one continuous pass than to index 180° and hope.

Cutting tools matter too. Long reach end mills deflect, so we prefer stub tools with a flute length just long enough for the feature. A tool with 4× diameter reach will hold size; a tool at 10× will not, no matter how good the machine is.

It starts with the model and the datum. We pick one zero that works for every face, usually the centerline of the part or a primary bore, and build the CAM setup around it. This is the step that decides whether the job runs in one setup or three.

Next comes the fixture. For shaft-type parts, a three-jaw chuck or collet on the rotary table plus a tailstock center. For blocky parts, a tombstone or a dedicated fixture plate. The fixture has to clear the toolpath on all indexed positions, so we check for collisions in CAM before cutting metal.

Then the toolpath. Roughing runs at high feed with a large cutter. Finishing on curved surfaces switches to simultaneous mode, where the A axis turns in step with the linear axes. Feeds and speeds come from the material: 6061 aluminium runs fast and wet, 17-4PH stainless runs slower with more coolant, titanium runs slow with high pressure.

Finally, inspection. Because the part is cut in one setup, the first article check focuses on feature-to-feature relationships, not just individual dimensions. We inspect 100 percent before shipment and can supply reports on request.

• 1
  One datumAll faces cut from the same zero point.
• 2
  Fixture clears the pathCollision-checked in CAM first.
• 3
  Simultaneous only where neededIndexed cutting is faster and stiffer.
• 4
  Check relationshipsCoaxiality and angular position matter most.

Workholding decides the outcome more than the spindle does. On a rotary table, the part must be supported against both cutting force and its own weight as it turns. A heavy block clamped on one end will sag when indexed 90°, and the error shows up as a taper on the far face.

For round parts, a collet or a bored soft jaw gives the best concentricity. For rectangular parts, a fixture plate with dowel pins locates the blank repeatably, and the pins are cut in place on the machine so they match the table's true center. That is how we hold ±0.005 mm across indexed faces.

Datum choice follows one rule: pick the surface that other features are measured from. If the drawing dimensions everything from a bore, that bore is the zero. If it dimensions from an outside face, use that. Changing datums mid-job is the fastest way to build in error.

Tailstock support is not optional on long parts. It removes the whip that appears when a slender shaft turns at speed. With support at both ends, we can hold concentricity on a 4,000 mm part that would otherwise need a second operation.