The Manufacture Workspace

Overview#

The Manufacture workspace is where Fusion turns a finished 3D model into instructions a CNC machine can run. It is a CAM (computer-aided manufacturing) environment that lives in the same document as your design. That single-document arrangement is the most important idea in this section: your toolpaths are associative with the model. If you change a fillet radius, a hole diameter, or the height of a boss in the Design workspace, the toolpaths that reference that geometry can be regenerated against the new shape instead of being rebuilt from scratch.

The workspace covers several manufacturing processes: subtractive (milling, turning, drilling, and water jet, laser or plasma cutting through the Fabrication tab), additive (FFF, SLA/DLP, MJF, SLS and metal powder-bed processes), and inspection (part setting, part alignment, geometric and surface inspection). This section of the guide concentrates on subtractive work, namely milling and turning, and on the supporting pieces that make toolpaths safe and productive: setups, stock, tool libraries, feeds and speeds, simulation, and post processing.

A typical CAM job in Fusion follows a fixed rhythm:

1. Model the part (and, if useful, the fixturing) in the Design workspace.
2. Switch to Manufacture and create a Setup that defines the machine type, work coordinate system (WCS), and stock.
3. Pick tools from a library, or create new ones.
4. Add operations (face, pocket, contour, drill, and so on) in a sensible order.
5. Generate toolpaths and review them with Simulate.
6. Post process the result into G-code for your specific controller.
7. Print a setup sheet for the operator.

You will repeat steps 2 through 6 for each fixturing orientation (each "side" of the part).

Tip: Treat the Manufacture workspace as a planning tool as much as a programming tool. Time spent thinking about holding, datum choice and operation order before you click anything is worth more than any advanced strategy option.

Where to find it#

Use the workspace switcher at the top left of the Fusion window (the button labeled Design, Manufacture, and so on) and choose Manufacture. The entry is called Manufacture.

If a document has never been used for CAM, the Browser has no setups yet; create one with Milling > Setup > New Setup (or the equivalent in the Turning, Additive or Fabrication tab). Existing setups appear in the Browser under a Setups node.

Keyboard access: there is no global shortcut to jump to the workspace, but many command shortcuts (such as S for the Shortcut Search / toolbar search in Fusion) behave the same in every workspace. Use the search to find a command by name.

The window layout#

Toolbar tabs and panels#

In the Manufacture workspace the toolbar tabs are organised by process, and each tab is split into panels. Autodesk's help names the process tabs Milling, Turning, Additive, Fabrication and Inspection. Each tab has its own Setup panel (for example Milling > Setup > New Setup, Additive > Setup > New Setup). Operations such as Face or 2D Contour are not on tabs of their own: they are panels inside the Milling tab.

Panels and command placement vary between releases, so if a command is not where described use the toolbar search. Which strategies are available depends on your licence and extensions (see the manufacturing extensions page).

Browser#

The Browser (left) is the project tree for CAM. Top to bottom, a populated document typically shows:

• Document Settings (including Units) and Named Views (shared with Design).
• Models: the component hierarchy from the Design workspace, with visibility toggles (including the model Origin).
• Setups: one entry per setup. Expanding a setup shows its operations, folders and patterns.
• NC Programs: groupings of setups or operations that will be posted together.

Status icons appear beside setups, folders, operations and NC programs. Autodesk lists these states: error, contains a child with an error, warning, contains a child with a warning, out of date, valid with no errors (for a toolpath this means both the toolpath and its in-process stock are generated), contains notes, queued to generate, and currently generating. When parent and child both have problems, the icon shows the most severe in the order errors, then out of date, then warning. A yellow exclamation triangle means the toolpath generated with warnings (double-click it, or right-click > Show Log, to read them); a red exclamation mark means the toolpath is out of date. Hover over any icon for a tooltip with the message. Generate brings operations up to date.

Canvas#

The canvas displays the model in the same navigation scheme as Design. Toolpaths are drawn over the model in color. In Autodesk's examples the start is a red arrow, rapid moves are yellow, lead-in and lead-out moves are green, cutting moves are blue, and the end is a green arrow. Stock appears as a translucent body when the Stock visibility is turned on.

The setup's WCS appears as a small triad at the origin. You will see it constantly, and learning to read it (red = X, green = Y, blue = Z) is fundamental.

Documents, data and the Design link#

When you enter Manufacture, you are not working on a copy. The model, the Setups and the operations all live in the same Fusion document. Consequences:

• Version history captures both design and CAM changes.
• Moving or renaming components can break toolpath references, in the same way it can break constraints. If you must restructure the model after programming, check each operation's geometry selections.
• References such as "Select the contour of this pocket" are stored as selections of faces or edges. If a face is deleted or its topology changes drastically, the selection may become invalid. The operation will show an error, and you reselect the geometry.
• Keeping the design parametric (design history captured) makes later edits easier to track; CAM still works in a direct-modeling document.

Tip: If several people work on the same part, separate roles by component: keep a "Fixture" component with vise, soft jaws and clamps next to the "Part" component. In the Setup dialog you choose which models are the part (Model) and which are Fixture. This gives you accurate collision checking in Simulate without modifying the part.

Setups, folders, and operations#

A Setup is the container. It records the machine, WCS and stock; every operation inside inherits those. A Folder inside the setup groups operations (for example "Roughing", "Finishing"), and can hold shared parameters. A Pattern repeats operations at multiple positions. Operations are individual toolpaths; 2D milling operations have tabs such as Tool, Geometry, Heights, Passes, and Linking (other strategies add or rename tabs).

The next pages cover each one in detail. For now, internalize the hierarchy:

Document
  Setups
    Setup 1 (machine, WCS, stock)
      Folder: Roughing
        2D Adaptive Roughing
      Face
      2D Pocket
      Drill
    Setup 2 (flip side)
      ...
  NC Programs

Step by step: your first pass through the workspace#

1. Open any simple part in Design. A block with a pocket and a few holes works well (see the practice exercise).
2. In the workspace switcher, choose Manufacture.
3. Click Milling > Setup > New Setup. Leave the type as milling, select the model body, and accept defaults for now. Click OK. A Setup appears in the Browser.
4. Expand the Setup. It is empty because no operations exist yet.
5. Click Milling > 2D > 2D Offset Roughing (called 2D Pocket in older releases). The dialog opens with tabs: Tool, Geometry, Heights, Passes, Linking.
6. On the Tool tab, click Select. The tool library dialog opens. Choose a flat end mill.
7. On the Geometry tab, click the floor of the pocket (or the pocket's bottom edges). The pocket contour highlights.
8. Click OK. A toolpath generates, and the operation appears under the Setup.
9. Click Milling > Actions > Simulate to watch the tool remove stock.
10. Return to Design at any time with the workspace switcher; the CAM data stays in place.

Options reference: key Manufacture UI elements#

Tips and pitfalls#

Tip: Name your Setups meaningfully ("Op1 - top, vise" and "Op2 - flip, soft jaws"). When you post a program for a shop floor operator, "Setup 1" tells them nothing.

Tip: Right-click items in the Browser for shortcuts such as Generate, Simulate, Show Log and Duplicate. Learning the right-click menu is one of the biggest speed-ups in Fusion CAM.

Warning: A toolpath that looks right on the screen is not proven safe. Always run Simulate with stock and, when available, with machine and fixture components, before you post. Posting does not check for collisions with your holder, vise, or machine.

Warning: Do not assume the part and the stock share an origin. The WCS and stock position are set in the Setup, and a mistake there moves every toolpath in the setup.

Warning: Strategy names have changed across releases (2D Pocket is now 2D Offset Roughing, Pocket Clearing is now 3D Offset Roughing, Adaptive Clearing is now Adaptive Roughing). If a command is not where described, use the toolbar search.

Note: Which strategies and options your licence includes is covered on the manufacturing extensions page; check Autodesk's current licence comparison for your account.

Practice exercise#

Create an 80 x 50 x 20 mm block in Design. Add a rectangular pocket 40 x 25 mm and 8 mm deep, and two 6 mm through holes. Switch to Manufacture.

Create one Setup with default settings. Add a 2D Offset Roughing operation using a 10 mm flat end mill, then a Drill operation using a 6 mm drill. Generate both and run Simulate.

Expected result: the pocket appears in the stock simulation at the correct depth, the holes pass through, and the Browser shows two valid operations under one Setup. Then return to Design and change the pocket depth to 10 mm. Back in Manufacture the pocket operation should show the out-of-date icon; Generate it and confirm the toolpath cuts the new depth.

Related#

• Setups and stock: defining the container for all operations
• WCS and orientation: choosing the origin and axes
• Tool libraries: selecting and managing cutters
• Extrude (Solid modeling section): the modeling operations your toolpaths will follow