5-Axis Machining Basics

How Does a 5 Axis CNC Machine Work?

A 5-axis machining center adds two rotary axes to the usual X, Y and Z. That lets the tool reach five sides of a part in one setup, at almost any angle. This guide explains the mechanics, the CAM setup and the cutting steps, so you can judge whether your part belongs on a 5-axis machine or a 3-axis one.

Get Instant Quote Talk to an Engineer

16 simultaneous 5-axis centers±0.005 mm tolerance12-hour quote + DFMNo minimum order quantity

On this page

Key takeaways

Three linear axes plus two rotaryX, Y and Z move the tool or table; two rotary axes tilt the part or the spindle so the cutter approaches from a new direction without a second setup.

Two control modesSimultaneous mode moves all five axes at once; 3+2 mode locks the rotary axes and cuts with the three linear axes only.

The post-processor matters as much as the ironA 5-axis toolpath is useless if the CAM post is not matched to the machine kinematics and the control's RTCP function.

One setup, fewer error stacksFive-sided access in a single fixturing removes the re-datuming that drives most tolerance loss on multi-setup work.

Mechanics

What the Five Axes Actually Do

Start with the linear axes. X, Y and Z are the same on any machining center: three perpendicular directions of relative motion between the tool and the workpiece. On a 3-axis vertical mill the part stays put and the spindle moves. That is fine for a cube with features on one face. Flip the part and you introduce a new datum, a new clamp, and a new stack of positional error.

The two extra axes are rotary. One turns about the Z axis, usually called C on a trunnion machine or B on a swivel-head machine. The other tilts about X or Y, called A or B. Together they let the cutter normal to a surface that faces sideways, undercut, or at a compound angle. The part does not need to be repositioned by hand.

Machine layout decides what you can actually hold. A trunnion table carries the part on a rotating cradle; the table swings and spins, which suits compact parts up to roughly Ø400 mm. A swivel-head machine moves the spindle instead, so heavy or long parts stay still and the head reaches around them. Both layouts do the same math, but they fail differently. Trunnion machines lose stiffness as the table tilts away from vertical. Swivel heads lose reach in deep pockets.

So how does a 5 axis CNC machine work in one sentence? The control solves a kinematic chain that keeps the tool tip on the programmed path while two rotary axes change orientation. When the part tilts 30°, the linear axes must compensate for the new tool-tip position. Miss that compensation and every angled feature lands in the wrong place.

1
3 linear + 2 rotaryX, Y, Z for position; A/B and C for orientation.
2
Trunnion vs swivel headTable tilts for small parts; head tilts for heavy or long ones.
3
Kinematics drive accuracyRotary positioning error multiplies over the distance from the pivot.

Control

RTCP: The Part Most Explanations Skip

Rotational tool center point, or RTCP, is the control function that keeps the tool tip fixed in space while the rotary axes move. Without it, the CAM system would have to recalculate the linear position for every single rotary increment, and any small mismatch between the CAD model and the real pivot offsets would show up as a gouge or a witness mark.

With RTCP active, you program the tool tip and the surface normal. The control does the rest. On a Fanuc or Siemens control this appears as G43.4 or TRAORI respectively. If your post does not output it, the machine runs in what is effectively 3+2 mode even if all five axes are moving.

Pivot offsets are the practical problem. The distance from the rotary axis centerline to the tool tip changes with tool length, and it changes again when you swap a holder. Every setup needs those offsets measured and entered. A 0.02 mm error in a pivot offset can throw an angled bore out by 0.1 mm at 200 mm from the pivot. That is why we probe the tool and the fixture, not just the part.

The CAM side has to match. A post-processor built for a trunnion machine will produce the wrong rotary signs on a swivel-head machine. The symptom is subtle: the part cuts fine on one face and mirrors on the opposite side. Check the post against the machine model before you trust the first article.

1
G43.4 / TRAORIFanuc and Siemens codes that enable RTCP.
2
Pivot offset error scales0.02 mm offset error becomes 0.1 mm at 200 mm reach.
3
Post must match kinematicsWrong post shows up as mirrored features, not as an alarm.

Trade-offs

When 5-Axis Helps and When It Hurts

The strongest case for 5-axis is setup reduction. If a part needs features on four or five faces, a 3-axis route means four or five fixtures, four or five datum references, and a positional error stack at every transition. Moving that part to a trunnion machine removes the re-clamping. That is often worth more than any single-axis accuracy gain.

The second case is surface quality on curved geometry. A ball nose cutter held normal to a contoured surface keeps a consistent step-over and a consistent effective cutting speed. Tilt it away from normal and the contact point shifts, leaving witness lines and uneven finish. On a compound-curve surface, a 3-axis machine simply cannot hold the normal across the whole patch.

The third case is undercut and deep cavity access. A short, stiff tool tilted into a pocket reaches areas a straight tool cannot. This is where 5-axis earns its keep on molds, impellers and housings with internal ribs.

The counter-case matters just as much. Simultaneous 5-axis toolpaths run slower, because the rotary axes have finite acceleration and the control must stay ahead of the kinematics. On a simple part you can add hours of cycle time for no geometric benefit. If a feature is reachable in 3+2, cut it in 3+2. Positional 5-axis gives you the access without the feed-rate penalty.

There is also a size limit. Rotary tables lose stiffness as the part grows, and long parts on a trunnion need counterweighting. On our floor, 5-axis work is practical up to Ø400 mm on the rotary table, while larger parts go on mill-turn centers or 3-axis machines with dedicated fixtures.

1
Use 5-axis forMulti-face parts, compound curves, undercuts, one-setup access.
2
Avoid simultaneous 5-axis forFlat plates and simple prisms that 3+2 cuts faster.
3
Size ceilingRotary table work stays practical around Ø400 mm.

Materials and finish

Materials, Speeds and Finish on a 5-Axis Machine

Aluminium is the comfortable case. 6061-T6 and 7075 cut fast at high spindle speeds, and the light cutting load means the rotary axes are not fighting much force. Typical finishing passes land between Ra 0.8–1.6 μm with a sharp carbide cutter and a consistent step-over. If you need better, a separate finishing pass at Ra 0.2–0.8 μm is achievable on a well-trammed machine.

Stainless and titanium change the picture. 316L and 17-4PH work-harden, so a tilted cutter that rubs instead of cutting will damage the surface. Keep the tool engaged, use climb milling, and watch the chip color. TC4 (Ti-6Al-4V) generates heat at the cutting edge, so coolant delivery through the tool matters more than on aluminium. A 5-axis machine with a tilted tool can sometimes reach a pocket that would starve a straight tool of coolant.

Inconel and tool steel push the rotary axes hard. The cutting forces transmit through the trunnion, and any backlash or clamp flex shows up as chatter on the contoured surfaces. On this material we favor 3+2 over simultaneous cutting, because the locked rotary axes give a stiffer loop.

Plastics and carbon fibre behave differently again. PEEK and PA cut cleanly but generate stringy chips that wrap the tool. Carbon fibre dust is abrasive and needs extraction. On a 5-axis machine, the ability to tilt the cutter helps control chip evacuation in deep pockets, which matters more than most people expect.

1
Aluminium6061-T6, 7075, 6082 — fast, stable, good finish.
2
Stainless and titanium316L, 17-4PH, TC4 — keep the tool engaged, control heat.
3
Inconel and tool steelFavor 3+2 for stiffness over simultaneous motion.
4
Plastics and compositesTilt for chip evacuation and dust extraction.

Workflow

Step by Step: Programming and Running a 5-Axis Job

The sequence we follow from model to first article.

1
1. Check the model for machinabilityLook for tool reach before you write a path. Flag any pocket deeper than 3× the cutter diameter. Confirm there is a valid setup orientation where the tool approaches normal to every surface. Fix undercuts in CAD, not on the machine.
2
2. Choose the setup orientation and stockPlace the stock so the rotary axes have clearance through the full motion range. Allow 3–5 mm of stock on machined faces for a first article, then reduce on production runs. Verify the part does not sweep outside the machine envelope at maximum tilt.
3
3. Build the CAM setup with the correct kinematicsLoad the machine model, not a generic 5-axis template. Set the rotary limits and the pivot offsets. Generate the toolpath and check the rotary axis travel does not wrap past its limit mid-cut.
4
4. Select the post and enable RTCPPost to G43.4 or TRAORI, depending on the control. Verify the output includes the pivot offset call. Simulate the posted G-code, not just the CAM path, so you catch post errors.
5
5. Prove the offsets on the machineProbe the tool length and the fixture. Measure the actual pivot offset and enter it. Do not trust the nominal value from the machine builder. Run a test cut on scrap and check an angled feature with a dial indicator.
6
6. Cut the first article and inspectHold conservative feeds on the first part, around 70% of calculated feed rate. Inspect an angled bore and a contoured surface. Compare against the CAD model at the pivot-relative distance, since that is where rotary error shows up first.
7
7. Lock the program and document the offsetsRecord the pivot offsets, the tool list, and the fixture position. On repeat runs, re-probe rather than reuse the numbers. Thermal drift on a trunnion machine over a long run is real, especially on aluminium.

Orientation strategy

Simultaneous 5-Axis vs 3+2 vs 3-Axis

Pick the mode by feature geometry and tolerance, not by machine availability.

Mode	Axis motion	Typical use	Watch out for
3-axis	X, Y, Z only	Prismatic parts, one-face features	Multiple setups add datum error
3+2 (positional)	Rotary locks, then XYZ cut	Angled faces, holes, pockets	Rotary clamp flex under load
Simultaneous 5-axis	All five move together	Blends, impellers, contoured surfaces	Slow feed rates, longer cycle time
3+2 on a 5-axis machine	Rotary held, XYZ cut	Short runs needing five-sided access	Tool reach at extreme tilt

The verdict

Use simultaneous 5-axis when the geometry demands it; use 3+2 when the part only needs access. If your part has four or five machined faces or a compound curve, 5-axis wins on setup count and finish. If it is flat and prismatic, it does not.

Get Instant Quote Talk to an Engineer

FAQs

Frequently Asked Questions

What is the main advantage of 5-axis over 3-axis machining?

One setup instead of several. A part with features on five faces stays clamped once, so you eliminate the datum changes and error stacks that come with re-fixturing.

The second gain is tool orientation. Holding a cutter normal to a curved surface gives a consistent step-over and a cleaner finish than a 3-axis pass can produce.

Is 5-axis machining suitable for prototyping?

Yes, and it is often the cheaper route for a complex prototype. One setup means one fixture and a shorter lead time than a multi-setup 3-axis sequence.

We run no minimum order quantity, so a single prototype and a 10,000-part run go through the same process. A first article may still need a second pass if the pivot offsets need fine-tuning.

What materials can be machined on a 5-axis machine?

The same metals as any other machining center: aluminium 6061 and 7075, stainless 303, 304, 316L and 17-4PH, steel 1018, 1045 and 4140, titanium TC4, Inconel, copper and brass alloys.

Plastics such as POM, PEEK, PC and ABS also run well. The limit is stiffness, not material type. Very soft or very thin parts can deflect under the rotary motion, so they may need extra support.

How is 5-axis different from 3+2 axis machining?

In 3+2, the rotary axes position the part and then lock. Cutting happens with the three linear axes only. The rotary axes are not moving during the cut, so the machine loop stays stiff.

In simultaneous 5-axis, all five axes move together. That is required for compound curves and blends, but it slows the feed rate and puts more demand on the control.

Which industries benefit most from 5-axis machining?

Aerospace, medical devices, robotics and automotive work see the most benefit, because their parts combine complex geometry with tight tolerances.

Aerospace housings and brackets often need five-sided access. Medical instruments and implants need contoured surfaces. Robotics joints need compound angles that are hard to fixture on a 3-axis machine.

How do I know if my part should be cut on a 5-axis machine?

Count the faces that need machining. If it is four or five, or if any feature sits at a compound angle, a 5-axis setup will usually beat a multi-setup 3-axis route.

If the part is a flat plate or a simple prism with features on one or two faces, 3-axis or 3+2 will cut it faster and cheaper. Send the model and we will confirm which route fits before quoting.