5-Axis CNC Machining
Also: 5-axis machining, five-axis machining, 5-axis milling, 3+2 machining, simultaneous 5-axis, multi-axis machining, full 5-axis
5-axis CNC machining tilts and rotates the part under the spindle so complex parts are cut in one setup: impellers, aerospace structures, implants and multi-face housings.
292 shops tagged 5-axis among 5,104 CNC machining companies in the Noramark directory
A 5-axis machine adds two rotary axes to the three linear ones, on a trunnion table, a tilting head, or one of each. It runs in two modes. In 3+2 (positional) machining the part is tilted to an angle and locked, then cut as on a 3-axis mill; this covers most job-shop 5-axis work, including compound-angle holes and faces. In simultaneous 5-axis all five axes move together so the tool follows a contoured surface at a constant lean, which is how impellers, blisks, turbine blades and complex mold surfaces are finished.
One setup for five faces means the true position between faces is the machine's positioning accuracy, typically 0.025 mm (0.001"), instead of a stack of fixturing errors across three or four flips. The head can tilt to reach into a pocket with a short, stiff tool, so deep walls finish cleaner with less chatter. Profile on contoured surfaces holds 0.05-0.1 mm (0.002-0.004") with care. The hourly rate is roughly double 3-axis, at $125-250 in the U.S., but fewer setups and less fixturing often make the part cheaper overall once it has features on three or more faces.
The work envelope is smaller than a 3-axis machine of the same footprint because the trunnion takes room, and the part must be held from below with five faces exposed, which means dovetail fixtures, vacuum chucks or a sacrificial tab. Programming and collision simulation take longer than a bracket deserves, so simple parts stay on 3-axis. Very large flat plates and long parts do not fit inside the tilt envelope.
At a glance
| Typical tolerances | Standard ±0.05 mm (±0.002") on features cut in one setup, ±0.013 mm (±0.0005") with care; true position of ±0.025 mm (±0.001") between features on different faces, because they share a setup. Profile tolerance on simultaneous-finished contoured surfaces of 0.05-0.1 mm (0.002-0.004") with care; angular features held to ±0.05° routinely. |
|---|---|
| Size limits | Trunnion-table machines common in job shops take parts up to about 500-800 mm (20-32") diameter and 400-500 mm (16-20") tall, with 200-500 kg on the table. Gantry and head-tilt machines for aerospace structures run to 3-6 m (10-20 ft). The tilt range limits reach: a deep pocket beside a tall wall may still need a long tool. |
| Surface finish | As-machined 0.8-1.6 µm Ra (32-63 µin) on walls and floors; 0.4-0.8 µm Ra (16-32 µin) on simultaneous-finished contoured surfaces with a fine stepover. Cusp height on ball-nose finishing is set by the stepover; 0.01 mm (0.0004") is achievable and costs machine time. Bead blasting or hand polishing hides tool paths on visible surfaces. |
| Lead time | Prototypes in 5-10 business days; production in 3-8 weeks. Programming and fixture design front-load the schedule, so the first piece takes longer than on 3-axis while repeat orders run faster. |
Typical of U.S. job shops; confirm with the shop for your part.
Materials
Aerospace aluminum (7075, 7050, 2024), titanium and nickel alloys (Ti-6Al-4V, Inconel 718 and 625) and PH stainless (17-4, 15-5) make up most 5-axis work, along with 6061 for housings and manifolds, 316 for medical and food parts, 4340 and H13 for dies and tooling, and PEEK and Ultem for implants and electrical parts. Titanium and Inconel cut at a fifth to a tenth of aluminum feed rates and wear tools fast; thin-walled aerospace parts in any alloy are roughed, stress relieved and finished.
What drives the cost
- Machine rate: 5-axis time runs $125-250 per hour in the U.S., roughly double 3-axis
- Programming and simulation: complex surfaces and collision checking take CAM hours that a simple bracket does not need
- Material: titanium, Inconel and PH stainless cut at a fraction of the speed of aluminum and wear tools fast
- Workholding: custom fixtures, dovetails or vacuum chucks that leave five faces clear
- Tolerances below ±0.025 mm (±0.001") and profile tolerances on contoured surfaces
- Quantity: one-off parts carry the whole programming cost
- Inspection: contoured surfaces need a CMM or a scanner against the model, not a caliper
When to use it
- Parts with features on three or more faces, where one setup saves fixturing and holds true position
- Compound angles: holes and faces that are not square to any datum
- Contoured surfaces: impellers, blades, manifolds, orthopedic implants, molds and dies
- Deep pockets and tall walls that a tilted, shorter tool can finish without chatter
- Aerospace structural parts machined from plate, where one monolithic part replaces an assembly
When not to
- Simple prismatic parts with features on one or two faces: 3-axis milling is cheaper per hour and just as accurate
- Round parts: a lathe or mill-turn center makes them faster
- Very large flat plates or long parts that will not fit inside the tilt envelope
- High volumes of a casting-shaped part: cast or forge near net and machine only the datums
Design tips
- Leave one face free for workholding, or add a sacrificial tab or dovetail the shop can grip and cut off at the end.
- Model surfaces as true geometry, not faceted meshes; the CAM system drives the tool along the CAD surface.
- Use profile tolerances with a datum scheme on contoured surfaces; a plus-minus dimension on a curved face is ambiguous.
- Add wall-to-floor fillets sized to a standard bullnose or ball cutter (1-3 mm radius) so the surface finishes in one pass.
- Check that every feature can be reached within the machine's tilt range, usually ±90° to ±120° on a trunnion.
- Keep walls above 1 mm (0.040") in aluminum and 1.5 mm (0.060") in titanium, and expect a rough, stress-relieve, finish routing on thin-wall parts.
- Send native CAD or STEP with critical surfaces flagged; a 2D drawing cannot carry a free-form surface.
Frequently asked questions
- What is the difference between 3+2 and simultaneous 5-axis machining?
- In 3+2 the two rotary axes tilt the part to an angle and lock while the three linear axes cut, which handles multi-face and compound-angle parts. In simultaneous 5-axis all five axes move at once so the tool follows a contoured surface. Most job-shop 5-axis work is 3+2; impellers, blades and organic surfaces need simultaneous.
- Is 5-axis machining more expensive than 3-axis?
- Per hour, yes: about $125-250 versus $75-150 in the U.S. Per part it is often cheaper for anything with features on three or more faces, because one setup replaces three or four and the tolerance stack disappears. For a part with features on one face it is simply a dearer 3-axis machine.
- What tolerances can 5-axis machining hold?
- ±0.05 mm (±0.002") is standard and ±0.013 mm (±0.0005") is achievable with care. True position between features on different faces holds about ±0.025 mm (±0.001") because they are cut in one setup. Profile on contoured surfaces holds 0.05-0.1 mm (0.002-0.004").
- What parts need 5-axis machining?
- Impellers, blisks and turbine blades; orthopedic implants; aerospace ribs, spars and fittings machined from plate; mold cores and cavities with undercuts; manifolds and housings with ports at compound angles; and any part where the tolerance between faces cannot survive several setups.
