5-Axis CNC Machining
5-axis CNC machining tilts and rotates the part or the head so the tool reaches every face and stays short and rigid on complex surfaces.
- Part
- Cutting
- Revised
- 2026-08-11
At a glance
- Family
- Mechanical
- Typical tolerances
- ±0.005 in (±0.13 mm) standard; ±0.001 in (±0.025 mm) precision; single-setup work avoids the 0.002–0.005 in (0.05–0.13 mm) datum shift multi-setup machining carries
- Surface finish
- 125 µin Ra (3.2 µm) as-machined; 32–63 µin (0.8–1.6 µm) with finishing passes; 16 µin (0.4 µm) achievable on contours
- Typical volumes
- 1–500 parts typical; dedicated production cells run higher
- Lead time
- 5–15 business days for prototypes; 3–6 weeks for production quantities
- Materials
- Metal, Plastic, Composite
What it is
5-axis CNC machining adds two rotary axes to the three linear ones so the cutter can approach the work from almost any direction. It runs in two distinct modes: 3+2 positional, where the rotaries index and lock and the machine then cuts exactly like a 3-axis mill, and simultaneous 5-axis, where all five axes move together to sweep a tool along a curved surface.
The engineering value is less about exotic geometry than about setup elimination — five faces machined in one fixturing with no datum shift between them — and tool shortening, because tilting the head lets a short, rigid cutter reach into a cavity that a 3-axis machine could only touch with a long, deflecting tool.
Tolerances match 3-axis work at ±0.005 in (±0.13 mm) standard and ±0.001 in (±0.025 mm) precision; what improves is the positional relationship between features on different faces. Typical parts: impellers, turbine blades, aerospace brackets, mold cores, orthopedic implants and anything with compound-angle holes.
How it works
- Machine configuration. A trunnion machine rotates the part on an A/C table and suits small to medium work; a swivel-head machine rotates the spindle on a B axis and suits large or heavy parts; hybrids split the rotation between head and table. The configuration decides the working envelope and how much the part weighs into the accuracy budget.
- CAM programming. Toolpaths are generated with explicit tool-axis control, gouge checking against the full surface model, and collision checking of holder, spindle nose, fixture and machine castings. Full kinematic simulation is standard practice, not an optional step.
- Post-processing and kinematics. The control's tool-center-point management keeps the tool tip on the programmed point while the rotaries move, so the programmer works in part coordinates instead of machine coordinates.
- Fixturing. The part is held on a minimal footprint — a dovetail fixture, tombstone or sacrificial tab of 0.25–0.50 in (6–13 mm) — so five sides stay open to the tool.
- Roughing in 3+2. Bulk removal is done with the rotaries locked, which is more rigid and lets the machine run 3-axis feed rates.
- Simultaneous finishing. Ball-nose or barrel cutters sweep the contour. Residual cusp height follows h ≈ s²/(8R) for stepover s and effective cutter radius R — so a barrel cutter with a large-radius flank produces the same scallop as a ball nose at several times the stepover.
- Probing and inspection. In-process probing re-establishes the part origin after roughing and checks critical features before the part comes off the machine, since refixturing to inspect defeats the point of single-setup work.
Design guidelines
Prefer 3+2 to simultaneous
Any face that is planar or can be reached along a fixed tool axis should be programmed as 3+2. Simultaneous motion is for surfaces where the tool axis must change during the cut — blades, blends, impeller flanks. 3+2 is more rigid, faster and easier to verify.
Design in the clamping stock
Add a 0.25–0.50 in (6–13 mm) sacrificial boss or dovetail tab to the model, and note where it may be removed. Without it, the shop has to guess a holding scheme and often ends up adding a setup — the exact cost the process was chosen to avoid.
Keep tool overhang short
The reason to tilt is rigidity. Keep tool length-to-diameter under 4:1 wherever the geometry allows; deflection scales with the cube of overhang, so an 8:1 tool deflects roughly eight times as much under the same load as a 4:1 tool.
Internal radii still follow the 3-axis rule
Rotary axes do not make corners sharp. Internal vertical corner radius should be at least 1/3 of the pocket depth, and the same radius should be reused so one cutter finishes the part.
Dimension compound-angle features with GD&T
Holes and bosses on compound angles should be located with true position from a clear datum reference frame, not with chained angular dimensions — see GD&T symbols. Use standard hole and thread sizes from the drill size chart and tap drill chart, and put a spotface normal to the hole axis wherever a fastener head must seat.
Specify finish only where it is functional
As-machined contours run 125 µin Ra (3.2 µm), finishing passes give 32–63 µin (0.8–1.6 µm), and 16 µin (0.4 µm) is achievable — but finishing time is set by stepover, so a blanket fine-finish callout across a whole impeller is expensive (surface finish chart).
| Material | Suitability | Watch for |
|---|---|---|
| 7075 / 6061 aluminum | Excellent | Most aerospace 5-axis work; high removal rates |
| Ti-6Al-4V | Common but slow | 100–200 SFM; heat management and tool wear dominate |
| Inconel 718 / 625 | Difficult | Very low speeds, ceramic or coated carbide tooling |
| 17-4 PH, 15-5 PH stainless | Good | Machine in condition A, then age |
| P20 / H13 tool steel | Good | Mold and die cores; often finished by EDM |
| PEEK, Ultem | Excellent | Implant and fixture work; stable and clean-cutting |
| Carbon fiber laminate | Abrasive | Diamond tooling, dust extraction, no coolant contamination |
| Feature | Recommended | Limit | Why |
|---|---|---|---|
| Tool length : diameter | ≤ 4:1 | ~6:1 tilted | Deflection grows with overhang cubed |
| Clamping stock | 0.25–0.50 in (6–13 mm) | None | Something has to hold the part |
| Internal corner radius | ≥ 1/3 pocket depth | Tool radius | Rotary axes do not sharpen corners |
| Finishing stepover | Set by cusp h ≈ s²/(8R) | — | Halving the scallop costs 40% more passes |
| Undercut access | Reachable with a tilted tool | Lollipop cutter needed | Tool body must clear the surface |
Cost drivers
5-axis time bills at a higher rate than 3-axis, and the programming behind it takes longer because every move has to be collision-checked against the whole machine. The process pays for itself through setup count, not through hourly rate.
Setups avoided. A part needing five faces machined takes three or four setups on a 3-axis machine, each with its own fixture, offsets, inspection and datum shift. If one 5-axis setup replaces three 3-axis setups, it usually wins outright — and it removes the 0.002–0.005 in (0.05–0.13 mm) of stack-up those setups introduce.
Finishing stepover. On contoured surfaces, cycle time is dominated by the number of finishing passes. Because cusp height goes with the square of stepover, doubling the allowable scallop lets the stepover grow about 40% and removes roughly 30% of the passes.
Programming and simulation. A one-off impeller can carry more programming hours than machine hours.
Fixture design. Purpose-built dovetail and tombstone fixtures are a real line item on the first order and free on every reorder.
Four ways to take cost out:
- Model the clamping tab yourself so the shop is not designing workholding on your behalf.
- Keep surfaces 3+2-machinable wherever function permits; save simultaneous motion for the surfaces that need it.
- Apply a fine surface finish callout only to sealing, bearing and aerodynamic surfaces.
- If the part has fewer than three machined faces, quote it as 3-axis milling instead — 5-axis capability you do not use is still on the invoice.
Questions
6 questionsWhat is the difference between 3+2 and simultaneous 5-axis machining?
In 3+2 machining the two rotary axes index to an angle and lock, and the machine then cuts as a rigid 3-axis mill from that orientation. In simultaneous 5-axis all five axes move together so the tool axis changes continuously along the cut. 3+2 is faster, more rigid and easier to verify; simultaneous is required only for surfaces such as impeller flanks and turbine blades where the tool axis must change during the cut.
Is 5-axis machining more accurate than 3-axis?
The achievable tolerance on any single feature is about the same — ±0.005 in (±0.13 mm) standard and ±0.001 in (±0.025 mm) precision. What improves is the relationship between features on different faces, because they are cut in one fixturing instead of being re-datumed, removing the 0.002–0.005 in (0.05–0.13 mm) of stack-up that each additional setup introduces.
When is 5-axis machining worth the higher hourly rate?
When it replaces multiple setups or lets a much shorter tool reach a deep feature. A part needing four or five machined faces typically takes three or four 3-axis setups, each with fixturing, offsets and inspection. One 5-axis setup replacing three 3-axis setups usually costs less overall despite the higher machine rate.
How do I control surface finish on a 5-axis contour?
Finish on a swept surface is set by the residual cusp between passes, approximated by h ≈ s²/(8R) for stepover s and effective cutter radius R. Because the relationship is quadratic, halving the cusp height requires about 40% more passes. Barrel or circle-segment cutters present a much larger effective radius than a ball nose and reach the same cusp height at several times the stepover.
Do I need to design a fixture for a 5-axis part?
You should at least model the clamping stock. Adding a 0.25–0.50 in (6–13 mm) sacrificial boss or dovetail tab and noting where it can be removed lets the shop hold the part on a minimal footprint with five sides open. Without it, workholding gets improvised and often adds the second setup the process was meant to eliminate.
Does 5-axis machining allow undercuts?
It allows features that a fixed vertical tool axis cannot reach, which covers many geometries described as undercuts, because the tool can be tilted to approach from the side. True internal undercuts still need a lollipop or T-slot cutter, and the whole tool body — not just the tip — has to clear the surrounding surfaces.