Overview#
When a part is made by cutting a flat blank and bending it, the 2D fabrication work is the flat blank: its outline, holes, slots, relief cuts and the lines that mark where the bends go. Fusion's sheet metal tools compute that blank from the 3D model using the sheet metal rule (thickness, bend radius, K-factor or bend allowance, relief type). The same blank then goes to a laser, waterjet, plasma or turret punch, and then to a press brake.
The detailed sheet metal modeling workflow (flanges, contour flanges, bends, corners) belongs to the sheet metal section of this guide. This page focuses on the fabrication hand-off: what the flat pattern contains, how to check it for cutting, how to configure bend lines and layers, what a shop wants to see, and how a flat pattern connects to nesting and toolpaths in Manufacture.
Where to find it#
- Create Flat Pattern: Sheet Metal tab, Create > Create Flat Pattern. You select the stationary face, and Fusion creates a Flat Pattern node in the Browser and displays the flat. Finish Flat Pattern (or Exit Flat) returns to the folded model; the Activate Flat Pattern radio button in the Browser switches between the two states. Only one flat pattern is allowed per sheet metal component.
- Flat pattern environment: With the flat pattern activated, the toolbar offers Export DXF. The flat pattern has its own timeline, so you can add manufacturing features (such as tabs) that do not affect the folded model, per Autodesk's help.
- DXF options: The Export Flat Pattern As DXF dialog offers a unit type (default is the design's units), Convert splines to polylines with a Tolerance, and the visible geometry options Center lines (bend center lines) and Extent lines (bend extent lines).
- Sheet metal rules: Managed in the Sheet Metal rules library (create, edit, override); see the sheet metal section.
- Manufacture workspace: A flat pattern can be used as a manufacturing model or used as input to nesting. Nest Preparation lets you pick shapes that are sheet metal parts or other bodies.
Step by step#
Create and check the flat pattern#
- Make sure your part is a sheet metal body (it uses a sheet metal rule). If it was modeled as a regular solid, re-model it using the sheet metal flange tools.
- Choose the correct rule. Check thickness, bend radius, K-factor (the rule's linear type uses a K-factor; typical values of roughly 0.33 to 0.5 are general guidance, and your shop may specify its own), bend relief shape (Round, Straight or Tear) with width, depth and remnant, and the 2-bend corner relief shape (Round, Square or Tear). A wrong K-factor produces a flat pattern whose bent dimensions miss by a fraction of a millimeter per bend.
- In the Sheet Metal tab, click Create > Create Flat Pattern. Select the stationary face from which all flanges are unfolded, then click OK. A folded model must have at least one flat surface.
- Inspect the pattern. Check that holes near bends are not distorted (holes closer than about two to three thicknesses to a bend deform), that relief cuts exist at bend ends, and that corners have gaps.
- Measure: use Inspect, Measure on the flat pattern to confirm overall width and length against your own calculation using the bend allowance formula if you want a cross-check.
- Edit if needed. Per Autodesk's help, changes made in the Flat Pattern environment do not affect the folded model, so you can add manufacturing features such as tabs there; changing the formed model is preferable where the feature belongs to the part.
Export#
- Right-click the flat pattern in the Browser and choose Activate, then click Export DXF on the toolbar.
- In the Export Flat Pattern As DXF dialog choose the unit, tick Convert splines to polylines (and set a tolerance) if your cutter does not support splines, and choose whether to include Center lines and Extent lines.
- Click OK, name the file, set the type to DXF and save. According to Autodesk's help, outer profiles, interior profiles, bend center lines, bend extent lines and text are each assigned to a different layer; open the DXF and verify.
- Send the DXF to the shop with a separate drawing or notes stating material, thickness, finish, grain direction (for some stock), and bend directions and angles (the DXF does not carry these).
The flat pattern and DXF export pages in the sheet metal section cover the command in more detail.
From flat pattern to toolpaths#
- In Manufacture, create a Setup on the flat pattern face (Setup, Orientation: select a Z axis from the flat pattern's top face).
- Add a 2D Profile operation (Fabrication > Cutting > 2D Profile) with a laser/plasma/waterjet tool.
- For geometry select the flat pattern face edges (outer and inner contours) with contour selection. Use the direction arrows (outside clockwise, inside counterclockwise per Autodesk help).
- Ignore bend lines for cutting. If the flat pattern's DXF or sketches include bend lines as geometry, do not select them for cutting. Marking bends on a laser requires a separate scribe or engraving operation with its own settings.
- Use Tabs, lead-ins and kerf compensation as discussed in the toolpath page.
Nest multiple parts#
- Prepare shapes using the Nest Preparation dialog, include sheet metal bodies, set material and thickness. See the nesting page.
- Create a nest study and export nests as DXF or generate toolpaths from them.
Options reference#
| Item | What it does | Notes/default |
|---|---|---|
| Sheet metal rule: Thickness | Sheet thickness | Matches gauge or measured stock |
| Sheet metal rule: Bend radius | Inside bend radius | Check the tooling at the shop |
| K-factor / bend allowance | Position of the neutral axis | General guidance 0.33 to 0.5; shops often provide their own |
| Bend relief shape, width, depth, remnant | Cut at bend ends | Round, Straight or Tear |
| 2-bend corner relief | Gap where two bends meet | Round, Square or Tear |
| Stationary face | Face from which all flanges are unfolded | Chosen when creating the flat pattern |
| Center lines (DXF) | Bend center lines | Separate DXF layer |
| Extent lines (DXF) | Bend extent lines | Optional; useful for the press brake operator |
| Convert splines to polylines (DXF) | Replaces splines with polylines within a tolerance | Use if the laser does not support splines |
| Flat pattern edit features | Manufacturing features added in the flat state | Do not affect the folded model |
Fabrication checks for sheet metal#
Note: the figures in this list are general design-for-manufacture guidance, not Autodesk data.
- Minimum hole diameter at least equal to the material thickness for laser, 1.5 to 2 times for plasma, and typically at least equal to thickness for waterjet. Smaller holes should be drilled or punched.
- Hole to edge distance at least 1 to 2 times thickness to avoid bulging.
- Hole to bend distance: at least 2 to 3 times thickness plus bend radius, otherwise the hole deforms when bending.
- Slot width at least equal to thickness.
- Bridge between features (web width) at least equal to thickness.
- Tab and slot self-locating features designed with 0.1 to 0.2 mm clearance per side.
- Bend relief depth at least equal to thickness plus bend radius plus a small amount.
- Grain direction: for stainless and aluminum alloys with strong grain, bends perpendicular to the rolling direction are safer.
These are general design-for-manufacture guidelines. Your fabricator's manual overrides them.
Tips and pitfalls#
Tip: Ask the shop for their K-factor or bend deduction table and create a custom sheet metal rule that matches it. This avoids tolerance errors on formed parts.
Tip: Keep the 3D model as the source of truth; re-export the flat pattern after any change. The flat pattern is associative and updates with the model.
Tip: Check the flat pattern for self-intersections. Parts with overlapping flanges may fail to flatten; add relief or open corners.
Warning: Do not scale the DXF to fix a size mismatch. If dimensions seem wrong, fix the sheet metal rule and re-export; scaling hides a real error that will repeat at the bends.
Warning: Some shops reject DXFs that contain bend lines. If yours does, untick Center lines and Extent lines in the export dialog.
Warning: Variable thickness materials such as coated steel have nominal vs actual thickness. Use the thickness the shop specifies.
Practice exercise#
Model an L-bracket: a 60 x 40 mm base flange and a 30 mm tall flange, 2 mm thickness, 2 mm bend radius, with two 5 mm holes in each flange. Create a sheet metal rule with a K-factor of 0.4. Create the flat pattern, measure its overall length, and compare with a hand calculation: flat length = 60 + 30 - 2*(R + T) + BA, where BA = bend angle in radians x (R + K x T), assuming the 60 and 30 mm are outside dimensions. Export as DXF with Center lines ticked. Expected result: a flat pattern about 86.4 mm long (if the dimensions are outside dimensions; check your own value), DXF with one outer contour, four holes, and a bend center line on a separate layer. Then change thickness to 3 mm and confirm the flat pattern updates.
Related#
- Flat Pattern and DXF Export (section 08)
- Sheet metal rules (section 08)
- Unfold and refold (section 08)
- Exporting DXF and SVG
- Nesting parts on sheets