How to Invert a 5 Axis CNC Machine
The machine never turns upside down. To invert a 5 axis cnc machine means reorienting the workpiece so a new set of faces reaches the tool, then rebuilding the coordinate system around it. This guide is for engineers and programmers who need second-side access on deep cavities, undercuts, and closed pockets.
In this article
- 1
- 2
- 3
- 4
- 5
- 6
- 7
- 8
Key takeaways
What it means to invert a 5 axis cnc machine
A 5-axis machine moves the tool along X, Y, and Z while two rotary axes tilt the part or the head. On a trunnion machine those are usually A and C. On a swivel-head machine they are A and B. Inversion does not use that hardware to turn the machine over. It uses the rotary axes plus a new work offset to present a face that was facing away from the spindle.
The practical limit is travel, not imagination. If the part is long, the rotary table may not have room to swing it. A Ø400 mm rotary table with a 500 mm part hanging off center will hit the column before the second face is horizontal. Check the swing envelope before you promise a setup.
There is also a stiffness limit. A part held 300 mm out from the table on a tall fixture behaves differently than one clamped 40 mm out. Chatter shows up first on the second side, because the fixture is usually less rigid than the vise that held side one.
So the real question is not whether the machine can reach the face. It is whether the part can be held rigidly, located repeatably, and probed accurately in the new orientation.
- 1Rotary axes do the reachingA and C, or A and B, tilt the part or head to expose the face.
- 2Work offset does the locatingA new G54-style offset ties the re-clamped part back to the model.
- 3Fixture does the holdingThe second fixture decides the achievable tolerance, not the spindle.
Plan the inversion before the first cut
Decide the sequence on paper. Which faces get cut on side one, which on side two, and which features bridge both. Any dimension that crosses the inversion needs a datum that survives the move. If a bore on side one is the locating feature for side two, cut that bore first and cut it accurately.
Pick datum features that are stable and reachable. A machined face plus two dowel holes works well. So does a bored hole with a matched spigot, or a ground pad with a shoulder. Avoid using a raw casting surface as a datum. Draft angle and scale variation will move the part by 0.1 mm or more.
Think about access for the probe. If the datum is inside a pocket that the probe cannot reach without a long stylus, the setup will be slow and noisy. Move the datum to an edge or an external pad when the geometry allows.
Finally, decide how much stock to leave. Leaving 0.3 mm on the second-side faces gives you room to correct a small misalignment with a spring pass. Leaving 0.02 mm leaves no room at all and forces a re-clamp.
- 1Cut the bridge datum firstAny feature used for side-two location must be finished on side one.
- 2Avoid raw surfaces as datumsCasting draft and scale can shift location by 0.1 mm or more.
- 3Leave correction stock0.2–0.3 mm on side-two faces allows a spring pass if needed.
Fixture design for the second orientation
The second fixture does the hard work. It must locate the part from the datums you cut on side one, and it must hold it without distorting the geometry you already finished. Clamp on stock, on a sacrificial boss, or on a face that will be cut later. Never clamp across a thin finished wall.
For repeatability better than ±0.005 mm, use dowel pins or a matched spigot rather than relying on vise jaws. Vise jaw pressure varies with the operator and with chip buildup. Pins locate the same way every time. GreatLight's engineering team designs and machines these fixtures in-house as part of the process.
In high-mix work, modular tombstone systems on pallet changers let one operator load side two while the machine cuts side one on another pallet. That cuts idle time. It also means the fixture must be self-locating, because the operator is not standing at the spindle checking it.
Watch for chips. A chip trapped under a locating pad lifts the part by its own thickness. Air blast the pads and the part before every clamp, and check the pads for dents once a week.
- 1Locate on pins, not jawsPins repeat to ±0.005 mm; jaw pressure does not.
- 2Clamp on stock, not finished wallsThin finished sections distort under clamp load.
- 3Blast pads before clampingA 0.1 mm chip becomes a 0.1 mm position error.
Rebuild the coordinate system in the CAM file
Model the fixture, not just the part. If the CAM file shows the part floating in space, the post will not catch a collision between the tool holder and the fixture body. Add the fixture, the clamps, and the tombstone. It takes an hour and saves a crash.
Set the second-side work offset at the datum features, not at the corner of the stock. The stock corner is saw-cut and may be off by 0.5 mm. The datum you machined is the truth.
Use the rotary axes deliberately. On a trunnion, tilting A to 90° and rotating C to 0° is a different setup from leaving A at 0° and rotating C. The first gives more tool clearance; the second keeps the part closer to the table center and reduces the swing radius. Pick based on which face you are cutting.
Keep the tool list short for side two. Every tool change is a chance for a chip to land on a datum. If you can finish side two with four tools instead of seven, do it.
- 1Model the fixtureCollision checking only works if the CAM file includes it.
- 2Offset from datums, not stockSaw-cut stock can be off by 0.5 mm or more.
- 3Fewer tools, fewer chipsEach tool change risks contaminating a locating surface.
Holding tolerance across the inversion
Every inversion adds a stack of errors: fixture location, clamp distortion, probe repeatability, and thermal drift. On a good pinned setup the total is 0.01–0.02 mm. If the drawing calls for ±0.005 mm across both sides, the setup has to be better than the tolerance, not equal to it.
Temperature matters more than most shops admit. A 300 mm aluminium part grows about 0.007 mm per °C. If side one is cut in the morning and side two after lunch, the part has moved. Let the part stabilize for 30 minutes before the witness cut, or keep the shop within ±1 °C.
Probe repeatability sets the floor. A clean stylus on a machined surface repeats to about 0.002 mm. The same stylus on a rough casting repeats to 0.02 mm or worse. That is why the datum has to be machined.
If the numbers do not close, do not chase them with cutter compensation. Find the physical cause: a chip, a loose pin, a clamp that moved the part. Compensation hides a mechanical problem and it will come back on the next part.
- 1Budget the error stackFixture, clamp, probe, and thermal errors add up to 0.01–0.02 mm.
- 2Let the part stabilizeAluminium moves about 0.007 mm per °C over 300 mm.
- 3Fix causes, not symptomsCutter comp cannot fix a chip under a locating pad.
Step by step: how to invert a 5 axis cnc machine part
- 1Finish the bridge datums on side oneCut the locating face, dowel holes, or spigot bore to final size before the part moves. Hold bore position to ±0.005 mm. If the datum is off, side two is off by the same amount.
- 2Probe and record the side-one positionTouch off the datum features in the machine coordinate system and save the values. Note the stock condition on the faces that side two will cut. A 0.2–0.3 mm stock allowance is a good working range.
- 3Release the clamps and clean every surfaceAir blast the fixture pads, the part, and the locating pins. Inspect the pads for dents or embedded chips. A single 0.1 mm chip under a pad tilts the part and shows up as a taper on the second side.
- 4Re-clamp in the second fixtureSeat the part on the pins or spigot by hand first, then apply clamp force. Tighten in a cross pattern to avoid rocking the part off the primary datum. Do not over-torque small clamps; 5–8 N·m is usually enough for M6 hardware.
- 5Re-probe the datums and rewrite the offsetProbe the same features again. The control should compute a new work offset that puts the part back into the model position. If the correction is larger than 0.05 mm, stop and find out why before cutting.
- 6Take a 0.05 mm witness cutSkim a known surface and measure it. This confirms the offset is correct with real chips flying. If the witness cut is off, correct the offset and repeat the skim. Do not start the finishing pass on an unverified offset.
- 7Run side two with the stock allowance in placeRough leaving 0.3 mm, then semi-finish leaving 0.1 mm, then finish. On thin walls, take lighter radial cuts: 0.3–0.5 mm radial engagement at 8,000–12,000 rpm in aluminium keeps deflection low.
- 8Inspect both sides before unclampingCheck the cross-inversion dimensions while the part is still located. If a bore on side one must align with a pocket on side two, measure it now. Re-clamping after unclamping costs a full setup.
When to invert, when to choose another route
Compare the part geometry against the setup options before committing to a second orientation.
| Part condition | Invert on 5-axis | Better alternative |
|---|---|---|
| Deep cavity with undercut walls | Yes, tilt and reach | None; 3-axis cannot reach |
| Long part over 500 mm | Check swing envelope first | Use 4-axis with tailstock |
| Thin wall under 1.5 mm | Risky on second clamp | Machine both sides from one orientation |
| Tolerance tighter than ±0.005 mm | Only with pinned fixtures | Single-setup 5-axis, no inversion |
| High mix, low volume | Modular tombstone pallets | Dedicated fixture per part |
| Raw casting datums | Not recommended | Machine datums first, then invert |
| Closed internal pocket | No access after inversion | Split the part or use EDM |
The verdict
Invert when the second face is unreachable any other way and the geometry can survive a second clamp. If a single-setup 5-axis pass can reach the feature, take it; every extra orientation adds error and time.
Frequently asked questions
Do you physically turn the machine upside down?
No. The machine stays on its foundation. Inversion is a workpiece strategy: you reorient the part, rebuild the work offset, and use the rotary axes to reach the new faces.
The word comes from the idea that the part's hidden side becomes visible, not from any movement of the machine frame.
How much tolerance can I hold across two orientations?
With machined datums, pinned fixtures, and probing, ±0.005 mm is achievable on a stable part. Realistic production numbers are often 0.01–0.02 mm because of clamp distortion and thermal drift.
If the drawing demands tighter than that across both sides, machine the critical features in one orientation instead.
What is the biggest cause of failure after inversion?
A chip under a locating pad. It lifts the part by its own thickness and tilts it. The result is a taper that looks like a machine geometry problem.
Air blast the pads and the part before every clamp, and inspect the pads weekly for dents.
Can I invert a part on a 4-axis machine?
Yes, if the second set of faces is reachable by rotating about one axis. A 4-axis setup with a tailstock is often stiffer than a 5-axis trunnion for long parts.
You lose the second rotary axis, so faces that need compound angles will not be reachable without a second fixture.
Should I leave stock on the second side?
Leave 0.2–0.3 mm on faces that will be finished after the inversion. That gives you room to correct a small misalignment with a spring pass without recutting the whole surface.
Leaving 0.02 mm removes that option. Any offset error becomes a visible step.
How long does a second-side setup add?
On a pinned fixture with probing, the clamp and offset rebuild takes 10–20 minutes. A dedicated fixture designed for the part is faster than adapting a general-purpose vise.
If the part needs a new fixture designed and machined, add 1–3 days depending on complexity.
Send us the part and the drawing
We review the geometry, tell you whether one setup or two is the right route, and quote it with a DFM note inside 12 hours.
12-hour quote±0.005 mm100% inspectionNDA on request
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
