Bend, Rip and Corner Treatments

Overview#

Three families of tools deal with the places where flat metal turns or meets itself:

• Fold (the command was called Bend in older releases and Autodesk's help still says "Fold (Bend)") bends an existing flat sheet metal flange along straight sketch lines, adding a true bend with the rule's radius and bend allowance.
• Convert to Sheet Metal applies a rule to an ordinary solid so that sheet metal tools work on it.
• Rip separates the material along an edge or at a corner so that a closed shape can be unfolded (a box has to be cut open at its corners before it can lie flat).
• Reliefs and corner treatments are small cuts and gaps that stop the metal tearing or colliding where bends end or meet. They come from the sheet metal rule (bend relief, 2-bend corner, 3-bend corner) and can be overridden per feature.

Command names were confirmed against Autodesk's Fusion help, except Rip, whose dialog labels could not be confirmed (see below).

Where to find it#

• Design > Sheet Metal > Create: Flange, Fold, Rip, Create Flat Pattern. Modify holds Unfold and Sheet Metal Rules; Refold appears on the tab while you are in unfold mode.
• Sheet Metal Rules (Modify panel) for default relief and corner shapes.
• The Override toggles inside the Flange dialog for local control.

Step by step#

Fold (bend a flat flange along a sketched line)#

1. Draw a sketch on the face of a sheet metal flange. Draw one straight line for each fold. Each line must lie in a plane parallel to the stationary face.
2. On the Sheet Metal tab choose Create > Fold.
3. Select the face that will be the Stationary side, then the sketch lines. When folding across several lines, select the line farthest from the stationary side first.
4. Set the Bend angle, measured relative to the stationary side, and use Flip to reverse the direction.
5. Set the Bend line position: Start (bend begins at the line), Center (bend centered on the line) or End (bend ends at the line).
6. Choose Bend relief On or Off for each fold, tick Corner relief to add corner reliefs where needed, and use Override rules if this fold needs different settings.
7. Click OK. The flange folds, the sharp sketch line becomes a cylindrical bend and the flat pattern gains a bend line.

Unlike Flange, Fold does not add material; it bends what is there. It is the quick route to a mounting tab or hook on an existing plate.

Convert to Sheet Metal (solid to sheet metal)#

If you have a thin-walled solid, Convert to Sheet Metal applies a sheet metal rule to it. You pick a wide face, and Fusion detects the thickness from that face and stores it in the rule; this thickness cannot be edited afterward. Use it for imported thin bodies before adding flanges or creating a flat pattern.

Rip#

1. Run Rip (Sheet Metal tab).
2. Choose the rip type. The Fusion API exposes three ways to define a rip: along an edge, between two points (each a vertex or a point along an edge) and by face. The dialog labels for these were not found in Autodesk's published help, so check the type names in your build.
3. Select the edge, points or face. The gap comes from the rule's Minimum gap (Autodesk's field for the space left at a miter, rip or seam).
4. Click OK.

A closed box, for example made from edge flanges that overlap at the corners, needs the corner either mitred (the Miter corners option in the edge flange) or ripped with a controlled gap. Without that, the flat pattern cannot be produced.

Corner relief control#

1. Open Sheet Metal Rules and edit the corner settings: 2-Bend Corner Relief (two bends meeting) and 3-Bend Corner Relief (a box corner, shown in the flat pattern view).
2. Choose the shape. For 2-bend corners the shapes are Round, Square, Tear, Trim to bend, Linear weld, Arc weld and Laser weld; Round and Square take a Size, and Round also has a Placement of Tangent or Intersection. For 3-bend corners the choices are No replacement, Intersection, Full round and Round with radius.
3. For one troublesome corner, use the Flange dialog's 2-bend corner override or 3-bend corner override.

Options reference#

Tips and pitfalls#

Tip: Use Round bend reliefs for laser-cut parts; square corners concentrate stress and may crack on hard materials.

Tip: If a feature fails with "self-intersection" near a corner, look at the corner gap and relief first, rather than the flange heights.

Warning: A relief that is shallower than the bend radius will leave a stress riser and may not unfold properly.

Warning: Do not rely on the flat pattern to show you tearing risk; check relief against the shop's rules in the design for manufacture page.

Tip: After a Rip, use Unfold briefly to confirm the part can truly flatten before adding more features.

Reliefs: what each shape is for#

A bend relief is the notch cut at the end of a bend where it meets an unbent edge. Without it, the flat tab beside the bend tears when the neighbouring metal is stretched.

Relief size follows simple proportions. A common starting point is a width of about one thickness and a depth equal to the bend radius plus about one thickness, so that the cut extends past the tangent line of the bend. For 1.5 mm steel with a 1.5 mm radius, that gives a 1.5 mm wide, 3 mm deep relief. The rule also has a Remnant, the minimum material left beside the relief. These numbers are starting points; follow your shop's guidance.

Corner reliefs in detail#

A 2-bend corner occurs where two flanges meet at a corner, as in an open box. The options in the rule:

• Round and Square cut a hole centred on the corner, with a Size measured in the unfolded body. Round has a Placement of Tangent (tangent to the flange edges) or Intersection (centred on the flange intersection).
• Tear leaves no relief.
• Trim to bend, Linear weld, Arc weld and Laser weld are sized by the bending area; the weld types leave shapes meant for welded corner seams.

A 3-bend corner appears when three bends meet. Its settings only show in flat pattern view: No replacement, Intersection (extend the flanges to meet), Full round (extend, then add a full round) and Round with radius (extend, then add a fillet of the specified radius). The Radius overrides the rule's relief radius.

Worked example: choosing corners for a 2 mm aluminium box#

Box 100 x 60 x 40 mm, 2 mm sheet, 2 mm inside radius, four walls from edge flanges, laser cut and brake formed. Settings: bend relief Round with width 2 mm, depth 4 mm; 2-bend corner Round, Size 4 mm, Placement Tangent; Minimum gap 0.5 mm. The round corner relief leaves 4 mm holes at each corner of the flat pattern, which also absorb small bending errors. If you plan to weld the corners instead, use Linear weld on the 2-bend corner and leave the gap at 0.2 mm to 0.5 mm per the welder's request.

Miter corners, rip and seams compared#

If a closed shape cannot flatten, the problem is nearly always a missing rip or corner treatment, not the flange heights.

Common failures and fixes#

Practice exercise#

Compare four ways of handling box corners and a fold.

1. Set up a 1.5 mm steel rule with a 1.5 mm bend radius and Minimum gap 0.5 mm. Make a 100 x 60 mm base flange.
2. Add four edge flanges 30 mm tall on all sides without Miter corners. Try Create Flat Pattern and note what happens at the corners.
3. Edit the flanges to tick Miter corners, and create the flat pattern. Measure the gap at a corner; it should be about 0.5 mm.
4. Delete the flat pattern, undo the miter, and instead edit the rule's 2-bend corner relief to Round, Size 3 mm, Placement Tangent. Create the flat pattern again, and compare the corner shape.
5. Sketch a line 20 mm from one short end on the base face and use Fold at 90 degrees with Bend line position Center. Check the flat pattern for the added bend line.

Expected result: the first flat pattern fails or overlaps, the mitred one has 0.5 mm gaps, the relief version has 3 mm round holes at the corners, and the Fold adds a bend line at the sketched position. Record which treatment you would choose for a laser-cut, welded and a brake-formed part, and why.

Related#

• Flange: base and edge
• Sheet metal rules
• Unfold and refold
• Design for manufacture