Fadal CNC machining: what the platform does well

• 1
  How Fadal CNC machining actually works
• 2
  Part geometry that suits a Fadal
• 3
  What tolerance a Fadal can hold
• 4
  Materials and the cutting-force question
• 5
  Five checks before you send the drawing
• 6
  Fadal versus a modern 5-axis center

Fadal CNC machining means running a part on a Fadal vertical machining center. The classic configuration is a 40-taper spindle on box ways, driven by a Fanuc-compatible control that reads G-code the same way most American shops learned it. Nothing exotic. The control stores programs in memory, runs macros, and handles a fourth-axis indexer through a simple rotary table command.

The mechanical side matters more than the electronics for finish quality. Box ways are hardened and ground steel on cast iron, with a wide bearing surface. That gives high rigidity in the cut but limits rapid speeds. Linear-rail machines accelerate faster and hold tighter positioning at high feed. Box ways resist chatter at low speed and heavy radial engagement, which is exactly where a 40-taper spindle does its best work.

Spindle speed is the other boundary. Most Fadal spindles top out around 7,500 to 10,000 rpm. Compare that to a modern 5-axis center running 15,000 to 20,000 rpm and the gap is clear. Small cutters under Ø3 mm need high rpm to hit a sane surface speed. On a Fadal they run slow, which means low feed per tooth and a finish that is harder to control.

So the platform fits a shape, not a category. Thick ribs, deep pockets in aluminum, castings that need one setup, weldments that need facing. It does not fit tiny features or mirror finishes. If you read a spec sheet that calls Fadal CNC machining good for everything, that sheet is wrong.

• 1
  Rigid in the cutBox ways and a 40-taper spindle handle heavy radial load without chatter
• 2
  Moderate spindle speed7,500–10,000 rpm suits Ø6 mm and larger cutters
• 3
  Simple controlFanuc-compatible G-code, easy to post from most CAM packages

Start with the feature size. If the smallest internal radius is Ø6 mm or larger and the deepest pocket is under four times the cutter diameter, a Fadal will cut it cleanly. Below that, you are running a small cutter at low rpm and the finish suffers. A Ø2 mm end mill at 8,000 rpm gives a surface speed of about 50 m/min in aluminum. That is workable but slow, and tool life drops.

Next look at the number of faces. A Fadal with a fourth-axis rotary table, typically Ø400 mm, can machine four sides in one setup. That removes three refixturing steps and the stack-up error that comes with them. On parts with tight bore-to-bore relationships, that matters more than spindle speed. One setup, one datum, one tolerance chain.

Deep cavities are the known weak point. Without high-pressure through-spindle coolant, chip evacuation in pockets deeper than 50 mm gets unreliable. We see this on mold inserts and hydraulic manifolds. Options exist: peck cycles, air blast, external coolant lines aimed into the pocket. They work, but they add cycle time.

Thin walls are the other limit. Aluminum walls under 1.5 mm deflect when the cutter pushes on them. A Fadal has the rigidity to take a light finishing pass, but the wall itself is the spring. Plan on multiple light passes, or move the part to a machine with higher rpm and lower cutting force.

• 1
  Good fitPockets with radii Ø6 mm and up, four-sided parts, heavy stock removal
• 2
  Workable with planningPockets 50–80 mm deep, walls 1.5–3 mm thick
• 3
  Poor fitFeatures under Ø3 mm, mirror finishes, walls under 1 mm

A well-maintained Fadal holds ±0.025 mm (±0.001 in) on position across a typical 750 × 1,150 × 550 mm envelope. That is the honest number for the platform in production, not the brochure number. Tighter than that, you are fighting thermal growth, ballscrew wear, and the resolution of the older control.

Tolerance is not one number though. It splits into position, size, and form. Position is where the feature sits relative to a datum. Size is the bore diameter or slot width. Form is roundness, flatness, straightness. A Fadal does position and size well. Form depends on the cutter and the setup as much as the machine.

For a bore that must hold ±0.005 mm, plan on a boring head with an in-process touch-off, or a reaming operation with a fixed-size tool. Do not expect a interpolated circle to land inside ±0.005 mm on any 40-taper machine. That is not a Fadal problem. It is how interpolation works.

Surface finish follows the same logic. Ra 1.6–3.2 μm comes off the machine with a normal finishing pass. Ra 0.8–1.6 μm takes a dedicated finish pass with a sharp tool and controlled feed. Below Ra 0.8 μm you are into polishing or a different process. Nobody reaches Ra 0.2 μm with a standard end mill.

• 1
  Position±0.025 mm typical across the envelope
• 2
  BoresUse a boring head or reamer for ±0.005 mm
• 3
  FinishRa 1.6–3.2 μm as machined, Ra 0.8–1.6 μm with a finish pass

Aluminum is where a Fadal earns its keep. 6061-T6, 7075, 2024, and 6082 all machine fast on this platform. The rigid frame lets you take a 6 mm radial depth of cut at 8 mm axial with a Ø12 mm three-flute cutter, and the machine does not flinch. That is real stock removal, not a light pass.

Steels are a different conversation. 1018, 1045, 4140, and 4130 cut fine at moderate speeds. Tool steel and 17-4PH stainless are harder on the spindle and the tooling. Expect lower feeds and more frequent tool changes. The machine handles it, but the cycle time you quoted on aluminum will not hold. Recalculate.

Titanium and Inconel are the edge case. Ti-6Al-4V and Inconel 718 generate high cutting temperatures and work-harden quickly. A 40-taper spindle at 8,000 rpm can cut them, but you need heavy coolant, conservative feeds, and sharp tooling. If your part is mostly titanium, the economics usually favor a machine with higher rpm and through-spindle coolant.

Plastics and composites are easy on the machine and hard on the setup. POM, PEEK, ABS, and carbon fibre all cut with light chiploads and sharp tools. The risk is melting, not force. Keep the chipload up and the rpm down. A Fadal is actually well suited to this, because its lower rpm range sits right where plastics cut cleanly.

• 1
  Aluminum6061-T6, 7075, 2024, 6082 — heavy radial cuts, short cycle times
• 2
  Steel and stainless1018, 4140, 17-4PH cut well but slower
• 3
  Titanium and InconelPossible, but the economics often point elsewhere