Overview#
Turning rotates the workpiece while a stationary tool removes material, producing round parts: shafts, pins, bushings, pulleys, threaded studs, and so on. In Fusion, turning uses the same Manufacture workspace as milling but a different Setup type, a different coordinate convention, and a different set of operations.
Good turning programs start with a good revolved model. A part that is essentially a profile revolved around an axis (see the Revolve command in the Solid modeling section) is ideal. Features that are not rotationally symmetric, like flats, cross holes and keyways, are either milled on a mill-turn machine with live tooling, or on a separate mill setup.
The workflow mirrors milling: Setup, tools, operations, simulation, post. The details differ in these ways:
- The spindle axis is Z, X is the radial direction. Whether X is output as diameter or radius depends on the post and machine.
- Tools are inserts in holders with specific cutting-edge geometry, not rotating cutters.
- Feeds are typically per revolution, and the tool's cutting data has a Use Constant Surface Speed checkbox (CSS), in which case the NC controller determines speed from the cutting diameter.
- Operations work from a 2D profile (the part's silhouette) rather than faces and pockets.
Where to find it#
- Turning > Setup > New Setup, with Operation Type Turning or Mill/Turn (selecting a machine defines the type).
- Turning tab > Turning panel: Turning Profile Roughing, Turning Profile Finishing, Turning Adaptive Roughing, Turning Face, Turning Groove, Turning Single Groove, Turning Thread, Turning Chamfer, Turning Trace and Turning Part. Groove roughing and finishing have their own topics. The Part Handling panel holds Subspindle Grab, Subspindle Return and Bar Pull; Actions has Simulate; Manage has the Tool Library.
- Tool Library: turning tools (Turning general, boring, grooving, threading) are in the Fusion Library's Turning Tools (Metric / Inch) libraries.
Turning toolpaths are described by Autodesk in the help without an extension flag on the strategy pages checked here; the sub-spindle and part-handling topics should be checked against your licence (see the manufacturing extensions page).
The turning Setup#
Operation type and machine#
Choose Operation Type: Turning (or Mill/Turn). If you have a lathe machine definition, selecting it defines the operation type. The machine configuration determines available spindles, turret and canned cycles via the linked post.
Work coordinate system#
Autodesk's turning WCS settings:
- Z Axis (Rotary Axis): select a cylindrical face or a sketch line along the part centreline. Z is almost always on the centreline and should point away from the chuck/clamping side; use Flip Z Axis if it points into the part.
- X Axis: select an edge or sketch line; Flip X Axis flips it.
- Origin: Stock front, Stock back, Model front, Model back, Selected point or Chuck front.
- Safe Z: the Z retract position, referenced to the WCS origin or the stock, with an offset; each operation can override it on its Passes tab.
- Spun Profile: for parts that also need milling features, approximates a 2D profile for 2-axis turning.
A typical choice is the origin on the centreline at the front face, so the front face is Z0 and the part toward the chuck is negative Z.
Stock#
Turning commonly uses Fixed size cylinder, Relative size cylinder, Fixed size tube, Relative size tube or From solid. Fixed cylinder takes Stock diameter and Length with a Model position (offset from front, centre, offset from back); relative cylinder takes Radial, Frontside and Backside stock offsets. For a second turning setup, From preceding setup has a Continue rest machining option.
Chuck and fixtures#
You can model the chuck and jaws as a Fixture to see collisions highlighted in stock simulation. The WCS Chuck front origin option references the chuck position.
Turning tools#
Tool types include:
| Tool | Typical use |
|---|---|
| General turning (OD) | Roughing and finishing outer diameters, profiling |
| Boring bar (ID) | Machining existing holes, internal profiles |
| Grooving | Cut grooves, O-ring seats, facing grooves |
| Threading | External and internal threads |
| Parting / cut-off | Separate the part from the bar |
| Drill | Center drilling and drilling along the axis |
| Live tools | Milling and drilling on mill-turn (extension) |
For turning tools, the Setup tab of the tool editor has 90-degree interval orientation options (and a custom angle box) to match how the tool is mounted on the machine. Accurate holder geometry matters for collision checks. Insert shape codes (CNMG and similar) are standard ISO designations; the Fusion Library's turning tools are named by insert and holder code, for example CNMT09T308 - DCLN-R.
Turning operations#
Turning Profile Roughing#
Removes as much stock as quickly as possible to leave a shape close to the desired geometry. Turning Mode selects Outside Profiling or Inside Profiling. Further topics cover groove suppression, grooving of grooves, depth of cut, skipping wall passes and angled entry moves.
Steps:
- Turning > Turning > Profile Roughing.
- Tool: pick an OD (or ID for Inside Profiling) insert holder.
- Geometry: select the profile or leave the default. A profile is generated from the model silhouette in the turning setup.
- Passes: set the cycle, depth of cut and stock to leave.
- Linking: set lead-in/out and retracts (including Retract and Approach in X).
- Generate.
Turning Adaptive Roughing removes bulk stock in small overlapping passes that follow part contours; it commonly uses grooving tools cutting in both directions, and is useful for complex shapes.
Turning Profile Finishing#
Produces the required shape and surface finish with shallower cuts at a slower feedrate than roughing; the number of cuts depends on finish and material. It has Outside and Inside modes, groove suppression, holder and insert clearance, and a Cutting Direction option.
Turning Face#
Removes stock from the end of the part to produce a flat surface perpendicular to the rotational axis. No geometry selection is needed. Options include Facing direction and Number of toolpath passes.
Turning Groove and Single Groove#
Turning Groove creates grooves on the OD, ID or face (Outside and Inside grooving) with roughing and finishing passes; tool orientation lets you groove angled areas. Turning Single Groove creates a groove of width equal to the insert's groove width at selected positions, useful for a clearance groove behind a thread. Turning Trace follows a model contour or sketch to machine complex geometry such as undercut grooves (gouge checking applies to the tool tip only).
Turning Thread#
Creates cylindrical and conical threads, right or left hand, on the outside or inside. Definition Method is Manual, Automatic (selects Fusion-generated threads) or Standard (predefined thread parameters such as pitch and major diameter). Select the faces for the thread and optionally confinement boundaries. To output a canned threading cycle, tick Use Cycle on the Passes tab, which may limit some features.
Turning Part (parting off)#
Also called cut-off. No geometry selection is needed; the toolpath is created at the back of the model specified in the Setup. It is usually the last operation in a setup. A part catcher collects the part on suitable machines. Turning Chamfer adds chamfers.
Drilling and boring on the lathe#
The Drill operation (shared with milling) works for axial holes. Peck cycles depend on the post (general guidance: G74 on Fanuc-style lathes). A center drill first prevents walk. Boring uses Turning Profile Roughing or Finishing with Inside Profiling and an internal tool; there is no separate turning Bore operation.
Speeds and feeds in turning#
On the turning tool's cutting data, Use Constant Surface Speed makes the NC controller determine speed: the rpm rises as the tool approaches the centreline. With it cleared, you enter a fixed Spindle Speed. Cap the rpm for CSS jobs (general guidance; a maximum spindle speed field is the usual way, check your tool's fields), because the theoretical rpm at zero diameter is unbounded.
The following are general industry starting points, not Autodesk data; use insert vendor data:
- Feed per revolution: roughly 0.1 to 0.4 mm/rev roughing and 0.05 to 0.15 finishing; finishing feed should stay under about half the nose radius.
- Carbide insert surface speeds: mild steel 150 to 250 m/min, stainless 100 to 180, aluminum 300 to 600.
Step by step: a simple stepped shaft#
- Model the shaft in Design by revolving a profile (see the Revolve page): total length 80 mm, with a 30 mm diameter section, a 20 mm diameter section, a chamfer and a groove.
- In Manufacture create a Setup, Operation Type: Turning, select the model, stock mode Fixed size cylinder 32 mm x 90 mm. Select the cylindrical face for Z Axis (Rotary Axis), flip if needed, and set the origin to Stock front or Model front.
- Add Turning Face with a general OD tool.
- Add Turning Profile Roughing, stock to leave 0.3 mm, stepdown 2 mm.
- Add Turning Profile Finishing with the same or a dedicated finishing tool.
- Add Turning Groove for the groove.
- Add Turning Part to cut off.
- Simulate. Post using a lathe post.
Options reference#
| Option | What it does | Notes/default |
|---|---|---|
| Operation type | Turning vs. milling | Chosen when creating the Setup |
| Z Axis (Rotary Axis) | Along spindle axis | Origin on centreline |
| Stock mode | Cylinder or tube | Frontside / backside offsets |
| Tool orientation | Mounting orientation (90-degree steps or custom) | Tool Setup tab |
| Use Constant Surface Speed | Controller varies rpm with diameter | Otherwise fixed Spindle Speed |
| Feed per revolution | Feed per spindle turn | General values above |
| Stepdown | Depth of roughing pass | Up to insert capability |
| Stock to leave | Finish allowance | Passes tab |
| Turning Mode | Outside or Inside Profiling/Grooving/Threading | Strategy dialog |
| Definition Method (thread) | Manual, Automatic, Standard | Turning Thread |
| Use Cycle (thread) | Output a canned threading cycle | Passes tab |
| Safe Z | Z retract position | Setup; overridable per operation |
| Part-off | Cuts part from bar | Last operation in a setup |
Tips and pitfalls#
Tip: Revolve your lathe parts from a single sketch profile. The same sketch can drive CAM geometry selection, keep dimensions parametric, and make changes simple.
Tip: Set a spindle speed limit for CSS jobs, especially when facing to center. The theoretical rpm at zero diameter is infinite.
Warning: Insert nose radius compensation is critical on tapers and arcs. Without it the profile is off by an amount that increases with the nose radius. Set the tool orientation correctly in the tool and check how the post outputs compensation.
Warning: X in diameter vs. radius. Posts and controllers differ. A radius value interpreted as a diameter is a half-size mistake. Verify with a test cut or a dry run.
Warning: Check chuck, jaw and tailstock clearances in simulation. Rapid moves in turning pass very close to the chuck.
Note: not confirmed in the Autodesk turning topics checked: which mill-turn, sub-spindle and live-tooling features need an extension.
Practice exercise#
Revolve a 25 mm diameter by 60 mm long pin with a 2 mm x 45-degree chamfer at the front, an 18 mm diameter step over the last 20 mm, and a 3 mm wide, 1 mm deep groove. Create a turning Setup with stock 28 mm x 70 mm. Add face, rough, finish, groove, and part-off operations.
Expected result: the simulation shows the face cleaned, the bar reduced to profile with a thin finish skin removed by the finishing pass, a clean groove, and a successful part-off with no collision with the chuck.
Related#
- Setups and stock
- Tools and tool libraries
- Feeds and speeds
- Revolve (Solid modeling section)