Sheet Metal Workflow Overview

Overview#

Sheet metal parts are made from a flat sheet that is cut (laser, plasma, waterjet, punch) and then bent on a press brake. The central problem of sheet metal CAD is that the same part exists in two states: the formed 3D shape and the flat blank that must be cut. Fusion handles this with a dedicated Sheet Metal tab in the Design workspace. Features in this tab know about material thickness, bend radius, bend allowance, and reliefs, so Fusion can unfold the part into an accurate flat pattern and refold it again.

The basic workflow looks like this:

1. Choose or create a sheet metal rule (thickness, bend radius, K-factor, relief and corner settings).
2. Create a base shape with a Flange (base flange from a sketch) or by using Convert to Sheet Metal on an existing solid.
3. Add edge flanges and contour flanges to build the walls.
4. Add cuts, holes, and corner treatments. Use Unfold / Refold when you need to cut across bends.
5. Create a flat pattern and export a DXF for the fabricator.

This page gives the map. The following pages go into each command in depth.

Note: Sheet metal tools are part of the standard Design workspace. Personal-use licences have limits on some export and manufacturing features; check Autodesk's current licence comparison. DXF export of a flat pattern has historically been available in personal-use, but "verify in your version" since licence terms change.

Where to find it#

• Workspace: Design.
• Tab: Sheet Metal (next to Solid, Surface, Mesh, Plastic, Sheet Metal, Utilities in the default layout; the exact tab order depends on your version and extensions).
• Panels: Create (Flange, Fold, Rip and Create Flat Pattern), Modify (Unfold, Sheet Metal Rules, Convert to Sheet Metal and other editing tools), plus the shared Construct / Inspect / Insert / Select panels. Autodesk's help gives the paths Design > Sheet Metal > Create > Flange, Create > Fold, Create > Create Flat Pattern and Modify > Unfold. Refold appears on the tab while unfold mode is active.
• When you create the first flange in a component, Fusion assigns a sheet metal rule. You can see and change it in the Browser on the component.

Step by step#

This is a complete first part, a simple L-bracket with a hole, to establish the whole workflow.

1. Open a new design. Make sure the active component is the one that should become sheet metal (use Create Component from the Assemble menu if you are starting an assembly).
2. Switch to Sheet Metal > Create > Flange. The flange command's type is chosen automatically depending on what you select: a closed sketch profile gives a base flange; a sheet metal edge gives an edge flange; an open sketch profile gives a contour flange.
3. Before sketching, open Modify > Sheet Metal Rules and check what rule is active. Set your thickness and bend radius to your fabricator's values. See the rules page.
4. Sketch a 60 mm by 40 mm rectangle on the XY plane and finish the sketch.
5. Start the Flange command, select the rectangle, and confirm the thickness is correct. Click OK. You now have a base flange.
6. Run Flange again, select one 60 mm edge, set height to 25 mm and angle to 90 degrees. Click OK.
7. Sketch a 6 mm circle on the base face and cut it with Extrude (Cut). In a sheet metal body, normal Extrude cuts work and the feature is recognised when flattened.
8. Choose Create > Create Flat Pattern, select the stationary face and click OK. A Flat Pattern node appears in the Browser. Inspect the flat length, then click Finish Flat Pattern to return to the folded model.
9. Export the pattern as DXF (see the DXF page).

Options reference#

The workflow stages and the commands that serve them:

Tips and pitfalls#

Tip: Decide your material and thickness first. Everything in sheet metal depends on thickness; changing it late can break corner reliefs and flanges.

Tip: Use user parameters (for example T = 1.5 mm) and tie flange heights and slot widths to them. Sheet metal features respond to parametric edits like any other Fusion feature.

Warning: A solid modelled with plain extrudes is not sheet metal. Fusion cannot unfold it. Either rebuild with flanges, or use Convert to Sheet Metal (see the bend and corner page).

Warning: Timeline order matters. If the model changes after the flat pattern was made, the Browser shows an Out-Of-Date icon; activate the pattern or choose Update Flat Pattern. If topology changed heavily, delete and recreate it.

Tip: Check that features still work after parametric changes: Unfold the model briefly (and Refold) to see whether it flattens without self-intersection.

Planning a part before touching a command#

Good sheet metal models are planned like the physical process. Before you open the Flange dialog, answer these questions.

1. Material and thickness. Choose from what the shop stocks, for example 1.5 mm or 2.0 mm for mild steel, 1.6 mm or 2.0 mm for aluminium.
2. Process. Laser cutting then brake forming, punching, or waterjet. This sets minimum hole sizes (about equal to the thickness for laser, larger for punching) and corner relief styles.
3. Fold sequence. Can the press brake reach every bend? A shallow U-channel is easy; a deep narrow box needs the tool to enter an opening, which may not be possible.
4. Datum faces. Which faces mate with other parts? Dimension those faces directly.
5. Joining method. Screws, rivets, welding. This affects corner treatments (welded corners may use weld-style reliefs).

Fold-sequence check by arithmetic#

On a 2 mm part with a 2 mm radius, the shop's minimum flange is about 4 x 2 + 2 = 10 mm. A tray with 30 mm walls and a 10 mm return has a return that is exactly at the limit, and the return must clear the opposite wall when the tool presses. A 25 mm deep, 40 mm wide U-channel with returns usually cannot be formed with standard tooling, since the return would collide with the punch on the second bend. Ask the shop, or reorder the bends in your design (a Z-shape forms more easily than a closed box).

Two build strategies#

After the first feature, add features in the order a fabricator would think: bends, then cut-outs, then local features (embosses, extruded holes), then the flat pattern.

Timeline and parameters#

• Create user parameters for thickness and the key radii, and reference them in sketches (Modify > Change Parameters). The rule's thickness is separate, so keep them in step.
• Name features: Base, Wall_L, Wall_R, Vent_slots. When a flat pattern fails, a named timeline is much faster to diagnose.
• Roll the timeline marker back when diagnosing. The failing feature is usually the first one after the marker that shows a warning icon.

Common failures and fixes#

Practice exercise#

Build an L-bracket with two holes, verify its flat length by hand, then test a rule change.

1. Create a rule: 2 mm steel, 2 mm inside radius, K-factor 0.35, Bend Relief Round (width 2 mm, depth 4 mm). Use thickness and radius parameters in your design if you wish.
2. Sketch a 60 x 40 mm rectangle on XY and make a base flange. Add one edge flange on a 60 mm edge: 25 mm height, Outer faces datum, 90 degrees.
3. Add two 5 mm holes in the base, 12 mm from the bend line (2.5 x 2 + 2 = 7 mm is the minimum clear distance for distortion).
4. Compute the expected flat length: outside lengths 40 + 25 = 65 mm minus outside setback 4 mm per leg (2 x 4 = 8 mm) plus bend allowance 1.5708 x (2 + 0.35 x 2) = 4.24 mm, giving about 61.2 mm. Create a flat pattern and Measure; compare.
5. Change the K-factor to 0.5, update the flat pattern, and record the new length (about 61.7 mm).
6. Export the DXF and open it in a viewer to confirm one bend line and two holes.

Expected result: a flat length near 61.2 mm with K = 0.35, rising by roughly 0.5 mm at K = 0.5, a DXF with an outline, two circles and one bend line, and a short written note of any discrepancy.

Related#

• Sheet metal rules
• Flange (base and edge)
• Contour flange
• Bend and corner treatments
• Unfold and refold
• Flat pattern and DXF export
• Design for manufacture