Overview#
When your cutter is controlled by G-code rather than by a vendor's vector-import software (typical for waterjets, plasma tables and many industrial lasers), you generate toolpaths in the Manufacture workspace. For flat-sheet cutting Fusion offers the 2D Profile operation: you select contours (edges, faces or sketch curves), and Fusion outputs a path along them with the right direction, lead-ins and lead-outs, tabs, kerf compensation and cutting order, then a post processor converts it into your machine's G-code.
According to Autodesk's help, the 2D Profile operation (Fabrication > Cutting > 2D Profile, formerly called Waterjet) is used for 2-axis machines without rotary tools: laser cutters, waterjets, plasma cutters and wire EDM. Autodesk describes laser as generally the most accurate with the smallest kerf, waterjet as moderate, and plasma as generally the least accurate with the largest kerf.
Availability: the 2D Profile help pages do not mark the operation as an extension feature. Nesting, by contrast, requires the Fusion Manufacturing Extension (see the nesting page).
Note: not confirmed in Autodesk's documentation: whether 2D Profile can output tilted-head or taper-compensated waterjet motion. The reference describes a 2-axis contour only; ask your waterjet vendor about taper compensation.
Where to find it#
- Workspace: switch the workspace drop-down from Design to Manufacture.
- Setup: Manufacture workspace, Setup tab, New Setup. (Older versions: Setup panel on the main toolbar.)
- 2D Profile: Manufacture workspace toolbar, Fabrication tab, Cutting panel, 2D Profile (path as given in Autodesk's help).
- Tools: Fusion Library > Sample Tools; pick a laser cutter, waterjet or plasma cutter. Use the New Waterjet/Plasma/Laser icon to create your own.
- Simulate: Actions > Simulate (or Simulate with Machine).
- Post Process: Actions > Post Process; choose the machine-specific post.
- Nesting: Fabrication > Nest (next page).
Step by step#
1. Create the setup#
- In the Manufacture workspace choose Setup, New Setup.
- Operation Type: choose the type that suits your machine; the setup dialog options are described in the Setup tab (milling and cutting) reference.
- Orientation: pick the Z axis normal to the sheet face. Set the Y axis along the machine's long axis. For a flat pattern, select the top face as the Z axis face.
- WCS origin: choose the corner of the stock where the machine's zero is. Many plasma and waterjet tables use the lower left corner of the sheet.
- Stock: set the sheet size (for example 1220 x 610 mm) and thickness. Offsets can be zero if the stock is exactly the model. Model: select the bodies to cut, or leave the default for all.
2. Add the 2D Profile operation#
- Click Fabrication > Cutting > 2D Profile.
- Tool tab: Click Select. If you have no tool, expand Fusion Library > Sample Tools and choose a laser cutter, waterjet or plasma cutter tool. Edit it to set the cutting feedrate, lead-in feedrate, lead-out feedrate and quality control option, which are the cutting data the tool reference lists. For router work choose milling operations instead (next pages).
- Geometry tab: With Contour Selection active, click a face, edge or sketch curve. Contiguous edges are chained automatically, and selecting a face lets you filter All, Outer or Inner loops (and open or closed contours). Check the contour arrows: for internal geometry (holes) the arrows should be counterclockwise and for the outer contour clockwise, per Autodesk's help. Click an arrow to flip. The direction, together with the Sideways Compensation setting, decides which side of the line the compensation lands.
- Geometry tab, Tabs: Enable the Tabs checkbox if you need holding tabs. Set Tab Width and Tab Positioning (By distance, with a Tab Distance value, or At points, where you pick each tab location).
- Passes tab: Set Sideways Compensation (Left, Right or Center, viewed from the cut direction) and Compensation Type (In computer or In control). With In computer, Outer Corner Mode (Roll around corner, Keep sharp corner, Keep sharp corner with loop) is available. Preserve Order keeps your selection order; otherwise Fusion optimizes it, and waterjet toolpaths machine inside boundaries first by default. Smoothing and Feed Optimization (reduced feed at corners) are also here.
- Linking tab: Enable Keep Nozzle Down (Autodesk help says this avoids retracts and moving over previously cut areas) and tune Maximum Stay-Down Distance, Cut Stock Clearance and Force Retract for Inside Cut. Set the lead-in (Lead-In Radius, Lead-In Sweep Angle, Linear Lead-In Distance) and lead-out (same as lead-in, or its own values), and a Piercing Clearance (distance from the profile at which to pierce, added to the lead-in distance). Heights (clearance, retract, top) are on the Heights tab.
- Click OK. Fusion generates the toolpath.
3. Order the cuts#
- Cut inside features first, outside last, so the part is held in the sheet until the end. Use multiple 2D Profile operations (one for holes and inner contours, one for outer contours), or reorder the operations in the Browser by drag and drop.
- For many small parts, sort by nearest neighbor to reduce rapid motion, or use the nesting output, which preserves a sensible order.
- Place the pierce points and lead-ins in waste material, never on the finished part's edge.
4. Simulate and verify#
- Select the Setup in the Browser and click Actions > Simulate.
- Watch the toolpath on the stock. Check that the lead-ins start on the scrap side, tab positions are right, kerf offset is on the waste side, and no path crosses cut parts (a risk for plasma torch tip-ups and waterjet nozzle collisions with warped parts).
- Check the cut order and the estimated time.
5. Post process#
- Select the setup or operations, Post Process.
- Choose the post from the library that matches your machine (Autodesk's post library lists vendor-specific posts; check for yours). Review the options: output folder, program number and units.
- Save the NC file and open it in a text editor to check the header, units, M-codes for beam on/off and the end-of-program sequence.
- Run it in the machine's simulator or in "air cut" mode with the torch or laser off before cutting material.
Options reference#
| Option | Tab | What it does | Notes |
|---|---|---|---|
| Tool (laser, waterjet, plasma) | Tool | Cutting, lead-in and lead-out feedrates, quality control | From Sample Tools or your own library |
| Cutting Mode | Tool | Through (auto, high, medium, low quality), Etch, Vaporize | Etch uses the geometry as the centerline with no width compensation; default Through - auto |
| Quality Control | Tool | Machine uses feeds, or machine uses quality | Some posts ignore the tool feedrate when quality is used |
| Contour selection | Geometry | Faces, edges or sketches to cut | Arrow direction matters; filters for open/closed contours and inner/outer loops |
| Side | Geometry | Offset inside or outside the geometry | Only works when Sideways Compensation is Left or Right |
| Tabs | Geometry | Keep parts attached | Tab Width, Positioning (By distance, At points), Tab Distance |
| Sideways Compensation | Passes | Left, Right or Center | Center is forced by Etch mode |
| Compensation Type | Passes | In computer or In control | See the kerf page; control compensation is done on finishing passes only |
| Outer Corner Mode | Passes | Roll around corner, Keep sharp corner, Keep sharp corner with loop | Only with In computer |
| Preserve Order | Passes | Cut in selection order | Unticked: Fusion optimizes |
| Lead-in / lead-out | Linking | Radius, sweep angle, linear distance | Place in scrap |
| Piercing Clearance | Linking | Pierce away from the profile | Added to lead-in distance |
| Keep Nozzle Down | Linking | Avoid retracts between cuts | Use only when the path will not hit tipped-up parts; set Maximum Stay-Down Distance |
| Finishing Overlap | Steps in help | Overlap at entry to clear material | From Autodesk's how-to steps |
| Heights | Heights | Clearance, retract and top heights | Offsets from model, stock or selection |
| Cutting order | Browser | Order of operations | Inside first, outside last |
| Feedrates | Tool | Cutting, lead-in and lead-out feed | Taken from machine charts; power is not an option in the reference |
Special cases#
Note: the Special cases below are general shop guidance, not Autodesk data.
Small holes with plasma and waterjet. Holes smaller than about the thickness do not come out round. Use a slower feed for small holes (feed-reduced "small hole" parameters in some posts and controllers), or drill them afterward.
Sharp corners. Real beams lag at sharp corners. Many industrial controllers slow down automatically. Fusion's Feed Optimization options (Maximum Directional Change, Reduced Feed Radius, Reduced Feed Distance, Reduced Feedrate, Only Inner Corners) can also reduce feed at corners. Corner radii of 0.5 to 1 mm can improve quality (general guidance).
Common-line cutting. Parts that share an edge are cut once, saving time and material. This needs a nest where parts share boundaries and a toolpath that selects the shared edge once; handle with care on plasma where heat builds.
Taper. Waterjets leave a V-shaped kerf. Taper compensation is not described in the 2D Profile reference (see the Note above).
Piercing. For plasma and waterjet, pierce points should be in scrap with a lead-in. For brittle stock (glass, stone) pierce at low pressure or from the edge.
Engraving, scoring. The Cutting Mode Etch makes a visible mark without cutting through, by controlling jet power and feedrate, with the geometry as the centerline. Support depends on the machine and post.
Tips and pitfalls#
Tip: Name operations clearly (
holes,outer,scribe) and set colors. When you debug, it makes the order obvious.
Tip: Create your own tool entries in a local library with measured kerf and feed for each material and thickness, for example
Plasma 45A 3mm mild steel. Reuse them across projects.
Tip: Always run the post output in the controller's dry run or simulate mode.
Warning: Post-processor output varies by machine. Never run G-code from an untested or generic post on a production machine without a dry run.
Warning: Flipping a contour arrow changes the side of kerf compensation. If the part comes out undersized or oversized by exactly one kerf, check the direction.
Warning: Toolpaths are associative with the model. If you change the design, regenerate toolpaths and check that the contour selection did not drop edges.
Practice exercise#
In the Manufacture workspace, make a setup for a 100 x 100 mm plate with a 30 mm hole in the middle and 3 mm thickness. Add a laser, waterjet or plasma tool from Sample Tools with kerf 1.0 mm. Create two 2D Profile operations: the hole first, then the outer contour. Add a lead-in (for example a 2 mm lead-in radius) in the scrap for each (the hole's lead-in in the hole's waste disk, the outside lead-in outside the part). Simulate. Expected result: the hole cut first, the outer contour second, the path offset by half the kerf on the waste side, and generated NC code that begins with the hole. Change the outer contour direction arrow and see how the simulation changes.
Related#
- Kerf and tolerances
- Nesting parts on sheets
- Materials and cutting settings
- Sheet metal flat patterns for cutting