How to Run a 5 Axis CNC Machine
This guide is for machinists and process engineers who already run 3-axis mills and need to move onto simultaneous 5-axis work. It covers setup order, work offsets, tool setting, dry runs and the in-cut checks that keep a part inside ±0.005 mm. Read it once before you touch the control, then keep it open at the machine.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
Key takeaways
What changes when you run a 5 axis machine
A 3-axis mill moves in X, Y and Z. A 5-axis machine adds two rotary axes, usually A and C, or B and C on a trunnion. Those two rotations let the tool reach the part from an angle instead of only from the top. That single change removes most of the setup count on complex parts.
The practical benefit is not speed. It is fewer setups. Every time a part moves to a new fixture, you add stack-up error. On a 4,000 mm aerospace housing, three setups can push a true position callout out of tolerance before any cutting starts. Running the part in one setup keeps the datums fixed.
The trade-off is that the machine now has five moving elements that can each drift. One bad rotary offset shows up as a taper, a shifted hole pattern or a wall that is not square. The steps below exist to catch those errors before the spindle reaches the part.
Setup time on a 5-axis machine is longer than on a 3-axis machine. That is normal. Budget 2–4 hours for a first-article fixturing job on a new part, and do not rush the dial-in. Most scrap blamed on the program is actually an offset error from the first 30 minutes.
If your part is prismatic, has four or fewer faces and holds ±0.05 mm, a 3-axis machine will finish it faster. 5-axis work pays back on contoured surfaces, deep pockets with undercuts, and parts that need four or more faces machined.
- 1Rotary axesA and C tilt and rotate the part; B and C move the head on a gantry.
- 2Setup countMost parts drop from 3–4 setups to 1 or 2.
- 3Error sourcesRotary centerline, post-processor output and thermal growth.
Read the drawing and pick the setup before you touch the control
Open the model and find the datum features the drawing calls out. Those are the surfaces that must touch the fixture. If the drawing calls A, B and C datums, your first op should machine or seat on at least two of them. Anything else and you are measuring from the wrong place.
Check the tightest tolerance on the print. If it is ±0.005 mm, you need a machine with a rotary table that repeats inside a few microns. Our Ø400 mm rotary tables hold that band, but the fixture still has to be rigid enough not to spring under load.
Look for undercuts, deep pockets and features that cannot be reached from the top. Those are the features that justify 5-axis work. Mark them and plan which ones run in 3+2 and which ones need simultaneous motion. Most parts are 80% 3+2 and 20% simultaneous.
Pick the tooling before you pick the toolpath. A long reach tool will chatter in a rotated cut, because the load direction changes as the table turns. Keep tool length-to-diameter under 4:1 for simultaneous cuts, and under 6:1 for 3+2 positions.
Write down the order of operations. Rough, semi-finish, finish, then the rotated features. If you finish a surface and then rotate the table to cut somewhere else, chips from the second cut will land on the finished face.
Dial in the rotary centerline and work offsets
The rotary centerline is the single most important number on the machine. On a trunnion, that is the intersection of the A axis and the C axis. If it is off by 0.02 mm, every rotated feature is off by 0.02 mm in a direction that changes with the table angle.
Set the centerline with a test bar and an indicator, not by trusting the last operator's saved value. Sweep the bar at 0° and at 90°, and split the difference. Repeat until both readings agree within 0.005 mm. On a machine that runs 24 hours, check it weekly and after any crash.
Set the work offset from the fixture, not the vice jaw. Touch off on a ground surface that is part of the fixture. If you touch off on a raw casting, the offset inherits the casting's draft angle and you lose 0.05–0.1 mm before the first chip.
Use a probe where the machine has one. A spindle probe on a 5-axis machine saves 30–60 minutes per setup and removes most of the arithmetic errors. Probe the fixture, then probe the stock, and let the control compute the offset.
Store offsets in named work coordinate systems, not in G54 alone. On a pallet machine, G54.1 P1 through P6 keep each pallet's offsets separate. Mixing them is a common cause of a part cut 10 mm off in Z.
Simulate and dry run before the first cut
Run the program through simulation with the actual fixture and tool holders modeled. Simulation catches the collisions that a backplot misses: the holder hitting the trunnion, the table hitting the enclosure, the tool shank hitting the fixture clamp.
Check the post-processor output on a short section. Rotate the table to a known angle and verify that the machine position matches what the CAM software shows. A post that outputs the wrong rotary direction will scrap the part on the first rotated move.
Dry run with the Z offset raised 50 mm. Watch the tool path at 20–30% rapid override, then at full rapid. Listen for the servos loading up. A rotary axis that sounds rough at full rapid will not hold position during a simultaneous cut.
Set the feed override low for the first cut. 30–50% on entry, then bring it up once you hear the cut settle. On aluminum, a 12 mm carbide end mill running 3,000 rpm and 1,500 mm/min should sound steady. If it squeals, the tool is rubbing, not cutting.
Keep one hand on the feed hold. The first 30 seconds tell you whether the tool is engaged or rubbing. If the chip looks like dust instead of a curl, stop and check the feed per tooth.
- 1Simulate with fixtureModel clamps and holders, not just the part.
- 2Verify the postOne wrong rotary sign scraps the whole part.
- 3Dry run at +50 mmWatch full rapid before you trust the offsets.
Step by step: how to run a 5 axis cnc machine
Follow the order. Skipping ahead is the most common cause of scrap.
- 11. Machine warm-upRun the spindle at 2,000 rpm and exercise both rotary axes through full travel for 15–20 minutes. Cold ballscrews and a cold spindle grow 0.01–0.03 mm in the first hour. On a machine that sat overnight, warm-up is not optional.
- 22. Fixture and dial-inMount the fixture and indicate it to 0.005 mm or better. Check that the fixture clears the trunnion at 90° and -90° rotation. Slide a 0.5 mm shim through the gap; if it catches, the fixture will crash when the table tilts.
- 33. Set rotary centerlineSweep a test bar at A0 and A90. Adjust the saved centerline until the two readings split within 0.005 mm. Record the value and the date. Do this before you set any work offset.
- 44. Set work offsetsTouch off or probe the fixture datum. Set X, Y and Z in G54. If the part has a known stock allowance, add it to Z now. Verify each axis with a scratch pass before running the program.
- 55. Measure and load toolsMeasure every tool on the presetter and load the values. Check the longest tool for clearance through the full rotary range. A tool that clears at A0 can still hit the table at A90.
- 66. Dry runRun the program with Z raised 50 mm at 25% rapid override. Watch every rotary move. Stop and fix anything that looks close. Then run again at full rapid.
- 77. First articleCut at 40% feed override. Measure the first two or three critical features before letting the cycle finish. If true position is out, stop and recheck the rotary centerline before adjusting the program.
- 88. In-process checkMeasure one critical feature every 20–30 parts. Log the reading. If it drifts more than half the tolerance band, stop and recheck offsets. Do not run to the end of the shift on a drifting process.
When to use 3+2, simultaneous, or stay on 3-axis
Pick the mode that matches the geometry, not the machine's maximum capability.
| Part feature | Best mode | Typical tolerance | Watch out for |
|---|---|---|---|
| Flat faces, 4 sides or fewer | 3-axis | ±0.05 mm | Setup stack-up, not the machine |
| Angled holes on one face | 3+2 | ±0.02 mm | Rotary repeatability at the index |
| Contoured blade or impeller | Simultaneous | ±0.01 mm | Tool length and chatter |
| Deep pocket with undercut | 3+2 plus long reach | ±0.02 mm | Tool deflection at depth |
| Port or organ pipe bore | Simultaneous | ±0.01 mm | Post output and surface blend |
| Large housing, 4,000 mm | 3+2 on a big trunnion | ±0.05 mm | Thermal growth over long cycle |
| Prototype, 1–10 parts | 3+2 | ±0.02 mm | Fixture cost per part |
| High-volume bracket, 10,000+ | 3-axis or mill-turn | ±0.05 mm | Cycle time, not axis count |
Frequently asked questions
Do I need a post-processor to run a 5 axis cnc machine?
Yes. A generic post will output the wrong rotary signs or the wrong pivot distance, and the first rotated move will scrap the part.
Get a post built for your exact machine model and kinematic configuration. Then prove it on a simple test block with known angles before you run a real part.
What is the difference between 3+2 and simultaneous 5-axis cutting?
In 3+2, the rotary axes move to a position and lock. The machine then cuts like a 3-axis mill from that angle. It is rigid and easy to program.
In simultaneous cutting, all five axes move at once. That is needed for contoured surfaces, but the load direction changes constantly, so tool length and holder stiffness matter much more.
How do I know if my rotary centerline is drifting?
Cut a test feature at A0 and the same feature at A90. Measure the offset between them. If it grows over a week, the rotary encoder or the mechanical centerline has moved.
On a machine running two shifts, check the centerline weekly and after any hard stop or crash.
Can I run a 5-axis part on a 3-axis machine?
Sometimes, if the part has four or fewer faces and the tolerances are looser than ±0.05 mm. You will need more setups and more fixtures.
Once the part has contoured surfaces or needs five faces in one setup, the stack-up error from extra setups usually costs more than the 5-axis rate.
What tolerance should I expect from a production 5-axis run?
On a well-maintained machine with a rigid fixture, ±0.005 mm is achievable on critical features. General surfaces usually run at ±0.02 mm.
Surface finish depends on the toolpath stepover. For a fine finish, stepover of 0.1–0.2 mm gives Ra 0.2–0.8 μm on aluminum.
How long does it take to learn how to run a 5 axis cnc machine?
A machinist who already runs 3-axis mills can handle 3+2 work in a few weeks. Simultaneous cutting takes longer because the failure modes are different.
The fastest path is to run one simple contoured part end to end, from setup to first article, with someone checking the offsets.
Send the drawing before you cut the first part
Our engineers review your model and fixture plan, flag the features that need simultaneous motion, and quote the run in 12 hours. 16 simultaneous 5-axis centers, ±0.005 mm, no minimum order quantity.
12-hour quote and DFM±0.005 mm tolerance100% inspection before shipmentNDA on request
More machining notes
We publish setup notes, tooling trials and inspection data from the factory floor.
