Creating a sheet metal component

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In Fusion, a sheet metal part starts out as a flat piece of metal with a consistent thickness.

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A flange feature consists of a face and bend connected to an existing face along an edge.

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In the Design workspace, switch to the Sheet Metal toolbar.

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Click the Create menu to access tools related to sheet metal creation, such as New Component, Flange, and Create Flat Pattern.

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In the Modifier group, you find tools such as Unfold and Sheet Metal Rules.

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To create and work with a sheet metal component, such as an outlet box, start with a blank workspace.

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On the Sheet Metal toolbar, Create group, click New Component.

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In the New Component dialog, the Type defaults to Sheet Metal.

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Decide if the component will be an External or Internal component, then enter a name, such as “Outlet Box”.

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You have the option to set the Sheet Metal Rule.

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For this example, leave the default Stainless steel (in) rule selected, and then click OK.

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A new component is added to the Browser, with an icon that looks like a sheet metal part.

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From the Create group, click Create Sketch, then select the XZ plane.

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To start drawing the first profile, on the Sketch toolbar, expand the Create menu, and select Rectangle > Center Rectangle.

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Starting from the origin, create a rectangle that is 2 in by 3 in.

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In the Sketch Palette, click Finish Sketch.

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Now, you can use the Flange tool, which is a combination of four tools in one.

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The Flange tool can be used to create a sheet metal base flange, an edge flange, a contour flange,

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or a lofted flange, based on the profiles you select.

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From the Create group, click Flange.

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Select the profile to add thickness and create a sheet metal base flange, based on the specified sheet metal rule.

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In the Flange dialog, you can specify the Orientation you want the sheet metal to extrude to: Side 1, Side 2, or Center.

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For this example, select Side 1, and then click OK.

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You can create a bend in this new body using edge flange.

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Click Flange again and select the upper-right edge of the base flange.

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Specify the Height of the bend—in this case, 2.5 in.

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The bend is automatically created according to the bend rules.

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You can also select multiple edges at the same time.

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In the Flange dialog, click Add selection set, then select the opposite edge.

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You can set other options, such as the Angle of the bend, Height Datum and Bend Position.

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A sample block is shown here as a reference, to enable you to see these options more clearly.

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The block is 2 in wide and 2.5 in tall.

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If the Height Datum is set to Inner Faces, the 2.5 in height is measured from the inside face to the top of the part,

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so it extends above the sample block.

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If you select Outer Faces, the 2.5 in is measured from the outside or the bottom of the sheet metal part to the top.

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With the Bend Position set to Inside, the edge flanges are inside the 2-inch width,

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and with Outside selected, these areas of the part are outside of the 2-inch width.

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Selecting Adjacent starts the bends adjacent to the two-inch width, and with Tangent selected, the bends are tangent to the 2-inch width.

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Typically, you use Inside or Outside bend positions.

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You can also Flip directions of the bend, set Miter Corners, or Override the sheet metal rules.

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Click OK to accept the parameters and create the new flanges.

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You can draw an open profile and turn it into a sheet metal part using a contour flange.

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For this example, click Create Sketch and select the top face of the left flange.

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In the Create group, click Line.

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Draw an angled line that runs along the existing sheet metal part, then down and to the right, with another extension line to the right.

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Click Finish Sketch.

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Back on the Sheet Metal toolbar, Create group, click Flange.

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Select the open profile, start to drag the height down, and then click OK.

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Notice that the corners of the sheet metal part are bent accordingly.

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Even though you created a sharp-edged sketch, this was created as a new body, so you can move it down if you want.

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The last tool, the join flange, enables you to join sheet metal parts together, even if they are not touching.

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Click Create Sketch and select the right face of the last flange you added.

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In the Create group, click Line and draw an angled line that runs up and to the left with another extension line.

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Click Finish Sketch.

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Once again, on the Sheet Metal toolbar, Create group, click Flange.

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First, click to select the new profile, then select the top edge of the open flange sheet metal part.

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Click OK, and they are automatically joined together.

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Again, even if your profile is not touching the sheet metal part, it will still extend and join.

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This is a great way to create features, such as hems.

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Now, you can add two more flanges on the other edges.

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Click Flange again, select the two remaining edges on the base of the box, and drag up.

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Click an existing flange to grab its height.

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Make sure that the Height Datum is set to Inner Faces and the Bend Position is Inside.

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Click OK.

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Depending on the first set of vertical flanges, you may need to offset the side faces to provide clearance when you bend the edges.

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Right-click, and from the Marking menu, select Press Pull.

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Select the four faces on the side of the left and right flanges.

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Set an offset of 0.03 in, then click OK.

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Click Flange again.

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Click the inside edge of the side flange.

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Click and drag the height to about 0.5 in.

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Based on the preview, you can change any settings, such as the Bend Position.

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In this case, set it to Outside.

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This flange will not take up the whole distance along the edge.

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Select a different Edge option in the flange dialog:

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Full Edge extends the full distance of the edge.

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Symmetric enables you to specify a distance for the length of the flange symmetrically.

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Note that the distance is half of the flange length.

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Two Sides gives you the option to specify the length of the flange using two distances, such as 0.25 up and 0.75 down.

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Two Offsets enables you to specify a distance from a reference point or plane.

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In this example, select Symmetric, and then set the Distance value to 0.4 in.

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To do the same on the other side, click Add Selection Set, then select the opposite edge.

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Again, select Symmetric and enter a Distance of 0.4 in.

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Add another selection set, and this time, rotate the view to select the other two edges.

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Select the first edge, then press and hold Ctrl as you select the second edge.

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Set the same Edge and Distance.

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Once complete, click OK.

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You also can create an automatic miter flange.

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Click Flange again, then select the four top inner edges.

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With the Miter Corners option selected in the dialog, when you drag the arrow, the corners are automatically mitered.

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Click Cancel to cancel the command.

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Add some symmetric flanges on the top for screw mounts.

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Click Flange and select the top edges on the front and back.

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Set edge 1 to Symmetric, the Distance to 0.2 in, and the Height to 0.5 in.

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Set edge 2 to Symmetric and the Distance to 0.2 in.

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Set the Height Datum to Inner Faces and the Bend Position to Inside.

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You can override the sheet metal rules by selecting Override Rules.

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Then, select Bend Relief Override, which enables you to change the Relief Shape to Straight.

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Click OK.

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You can also use regular modeling tools, such as Fillet, Chamfer, and Offset.

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In the Modify group, click Fillet, select the corner edges on the new tabs,

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and set the Radius to 0.2.

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Click OK.

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Use the Hole tool to add a couple of holes that reference the curved edges.

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Press H to start the Hole command.

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Select the top surface of one of the flanges, then select the curved edge.

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Set the Hole Diameter to 0.2 in and make sure the hole cut out goes through the part by dragging the arrow.

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Click OK.

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Press H again, and this time, select the opposite flange face and curved edge.

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Once the hole is placed, click OK.

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The outlet box is mostly complete.

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Now you can unfold it to see what it would look like flat.

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In the Modify group, click Unfold.

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Then, select a stationary entity, or the face that will stay fixed while the other bends unfold against it.

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You have the option to unfold only selected bins, but in this case, select Unfold all bins to unfold the entire part.

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Click OK.

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You can still make changes to the sheet metal part in its unfolded state.

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Create a new sketch and select the top face of the central flange.

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Expand the Create menu, and select Slot > Center to Center Slot.

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Draw a slot that crosses over multiple bends across the middle of the box.

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Click Finish Sketch.

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From the Create group, click Extrude and extrude the slot profile through the unwrapped pattern.

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Click OK.

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This cuts the slot through the material.

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On the Sheet Metal toolbar, click Refold Faces.

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When the part refolds, you can see how the slot folds with it.