Overview#
A contour flange turns an open sketch profile (lines, arcs, splines) into a sheet metal body with every corner automatically becoming a bend. It is the quickest way to make U-channels, Z-brackets, hat sections, hems and curved covers. In Fusion it is part of the same Flange command, selected by picking an open profile. It can be a new standalone body or joined to an existing sheet metal edge.
Use contour flange when the cross-section is the part (a channel extruded along its length). Use edge flanges when you are adding walls to an existing sheet.
Where to find it#
- Design > Sheet Metal > Create > Flange, then select an open sketch profile.
- Orientation and Direction options appear for contour flanges. Width type options apply when the contour flange is joined to an existing sheet metal edge, where they work as for edge flanges.
- Multiple open profiles can be selected if they lie on the same plane; each contour flange creates a new body.
Step by step#
- Create a sketch on a plane and draw the profile as an open chain of lines and arcs. You can draw sharp corners; Fusion adds bends from the rule. The profile is a reference side of the sheet; the thickness is added relative to it according to the Orientation option (see below).
- Do not close the profile. Finish the sketch.
- Start Flange and select the profile.
- Set the Distance (the length of the extrusion of the profile, giving the channel length). Choose Direction: One side, Two sides, or Symmetric.
- Choose Orientation: Side 1, Side 2 or Center, which decides on which side of the profile line the metal thickness is added.
- Choose Operation: New body or New component.
- Optionally enable Bend override to use a bend radius different from the rule for this feature.
- Click OK. Every vertex in the profile becomes a bend at the rule radius.
To attach to an existing edge, sketch the open profile on a plane normal to the edge, and select the sheet metal edge and the profile in either order. Autodesk's help confirms this workflow: the flange width type and related settings work as for edge flanges, orientation works as for contour flanges, and Override rules and Miter corners are available.
Options reference#
| Option | What it does | Notes/default |
|---|---|---|
| Profile | Open chain of lines, arcs, splines | Must be open; avoid self-intersection |
| Distance | Length the profile is swept | Parametric |
| Direction | One side, Two sides, Symmetric | Two sides lets each direction differ |
| Orientation | Side 1, Side 2, Center | Where the metal lies relative to the sketch line |
| Operation | New body, New component | |
| Sheet metal rule | Rule for the component | Appears once if none assigned |
| Override rules | Bend, relief and corner overrides | Per feature; the standalone dialog offers a Bend override for the radius |
| Flange width type | Full edge, Symmetric, Two sides, Two offsets | Only when joined to an existing edge |
Tips and pitfalls#
Tip: Dimension the sketch on the side you will see on the drawing (inside or outside). Use Orientation so the sketch line is the face you dimensioned. This keeps overall sizes right when you later change the thickness.
Tip: Sharp sketch corners get bends automatically. If you want a specific radius at one spot only, use an arc in the sketch, or use Override on the feature.
Warning: Bends in the profile that are tighter than the rule radius allows, or segments shorter than the minimum flange, will fail or produce unbendable geometry. Keep every straight segment at least a few times the thickness plus radius.
Warning: Splines are allowed but are not manufacturable by a press brake. A spline-based contour is fine for rolled or hydroformed parts; for brake-formed parts use lines and arcs.
Tip: Closed profiles will not work. If the profile accidentally closes, delete one segment.
Sketching profiles that behave#
The profile is the product. A few rules produce reliable contour flanges.
- One plane, one open chain. Multiple profiles are accepted only if they lie on the same plane. Each is a separate chain and each flange creates a body.
- Lines and arcs for press-brake parts. Every sharp vertex becomes a bend at the rule radius. Arcs become rolled sections. Splines are accepted but cannot be formed on a press brake.
- Dimension the segment lengths, not the vertex positions. A hat section is easier to parametrise as 20, 15, 10 than as coordinates.
- Choose the dimensioned side. The sketch line represents one face of the sheet (the face is chosen by Orientation: Side 1, Side 2 or Center). Dimension the face the drawing will quote.
How sketch lengths turn into flat length#
For a sketch line along the inside face with a 1.5 mm sheet, 1.5 mm inside radius and K-factor 0.35, each 90 degree bend consumes:
bend allowance = angle x (inside radius + K x thickness) = 1.5708 x (1.5 + 0.35 x 1.5) = 3.18 mm
A hat section with a 20 mm top, two 15 mm walls and two 10 mm feet, dimensioned to the outside virtual sharps, has five straight segments totalling 10 + 15 + 20 + 15 + 10 = 70 mm and four 90 degree bends. For each bend the outside setback is radius + thickness = 3.0 mm per side, so the bend deduction is 2 x 3.0 - 3.18 = 2.82 mm. Four bends remove 11.28 mm, giving a flat length of about 70 - 11.28 = 58.72 mm. Fusion computes this; use the arithmetic to check that the flat pattern is plausible.
Orientation, direction and distance#
- Orientation decides which side of the sketch line the metal lies on. Side 1 and Side 2 put the thickness on one side; Center splits it equally.
- Direction decides how the profile is swept: One side, Two sides (different distances each way) and Symmetric.
- Distance is the length of the sweep. For a 100 mm channel, enter 100 mm, or tie it to a parameter.
When you must keep a stable outside dimension while the thickness may change, choose the orientation that leaves the dimensioned face on the sketch line.
Joining a contour flange to an existing edge#
This is how you make a complex lip, hem, return or stiffening profile on a plate.
- Make a base flange, for example 200 x 100 mm, 2 mm thick.
- Sketch an open profile on a plane normal to one long edge: for example a 15 mm vertical leg, a 10 mm horizontal return and a 5 mm down-turn. Draw it so one end touches the edge.
- Start Flange and select the edge and the profile (either order).
- Set the flange width type, for example Full edge, or Two offsets to stop 10 mm from each end.
- Tick Miter corners if neighbouring flanges meet.
- Click OK.
Check the flat pattern; a return that folds back over itself needs a hem or an appropriate gap, and the shop must be able to form it (see the design-for-manufacture page).
Common failures and fixes#
| Symptom | Cause | Fix |
|---|---|---|
| The profile will not select | It is closed or on a different plane | Delete a segment; keep all chains on one plane |
| Flange fails with self-intersection | Segments too short for the radius | Lengthen segments above (radius + thickness) |
| The part is the wrong overall size after a thickness change | Orientation chosen on the wrong side | Edit Orientation so the dimensioned face stays on the sketch line |
| Bends are tighter than the rule | A sketch arc with a smaller radius | Use sharp vertices and let the rule set the radius, or use Bend override |
| Cannot join to the edge | The profile is not normal to the edge | Re-sketch on a plane normal to the edge |
| Flat pattern is not buildable | Spline profile or nested hem | Rework the profile with lines and arcs |
Contour flange versus other ways of building the same part#
| Part | Best command | Reason |
|---|---|---|
| Constant cross-section channel, angle or hat | Contour flange | One sketch gives all bends |
| Plate with four walls | Base flange + edge flanges | Walls are tied to the plate edges and miter together |
| Plate with a stiffening return along one edge | Base flange + contour flange joined to the edge | Complex profile on an existing edge |
| A single wall of a plate | Edge flange | Simplest, controlled by height and angle |
| Rolled or curved cover | Contour flange with arcs | Arcs become rolled sections |
If you find yourself sketching many profiles that differ only slightly, consider building one contour flange and editing the sketch parametrically, rather than creating separate features. Name the sketch dimensions (for example leg_a, leg_b, foot) so the part can be driven from the Change Parameters table, which makes it easy to match a catalogue of sizes.
A final check on any contour flange is the minimum leg length. As a starting guide, the straight length between two bends should be at least about four times the thickness plus the bend radius, so a 1.5 mm part with 1.5 mm radius needs 7.5 mm or more between bends; smaller legs may be unformable or require special tooling. Ask your fabricator for the exact value, which depends on the die width.
Practice exercise#
Build a hat section, check its flat length, then join a return to a plate.
- Make a rule with 1.5 mm thickness, 1.5 mm inside radius, K-factor 0.35.
- Sketch an open hat profile with 20 mm top, two 15 mm walls and two 10 mm feet, all dimensioned as outside lengths. Make a contour flange 100 mm long.
- Create the flat pattern and measure the flat width. Compare with the hand estimate in the maths section above (about 58.7 mm; yours will differ slightly depending on your datum choice, so record the difference).
- Change the rule's K-factor to 0.5 and note how the flat width changes.
- On a new body, make a 200 x 100 x 2 mm base flange and join a 15 mm leg + 10 mm return contour flange to one long edge, with Full edge width. Check the flat pattern.
- Edit the join to Two offsets so the flange stops 10 mm from each end.
Expected result: a hat section with a flat width near 58 to 60 mm, which grows or shrinks by a few tenths of a millimetre when the K-factor changes, and a plate with a formed return that stops short of the ends in step 6.