Corner Closure in Fusion Sheet Metal
Autodesk has added some new functionality into the Sheet Metal commands. We will highlight these new commands by creating a sheet metal dustpan.
Create the Aluminum Inch Dustpan Component
Create a new component and set its type to Sheet Metal. Choose the sheet metal rule named aluminum inch, and name the component dustpan.
Create a centered rectangle with the R shortcut key for the Rectangle command. Start with a 12" by 12" rectangle.
Use the Flange command to give the part its sheet metal thickness. Select the back wall and set the flange height to 2 in.
To form the top of the dust pan, select the top edge, right-click, and choose Flange. Set the height to 5 in and the angle to 80 degrees so the top pitches upward.
Add an Open Hem
Use the Hem command from the Create menu to add strength and rigidity. Select the edge, then change the hem type to Open Hem. This lets you control the spacing.
The gap starts at thickness. Change it to the formula:
thickness / 8
The hem length starts at thickness * 4. Change it to:
thickness * 6
The smaller gap brings the hem close to flat, while the longer length adds more support.
Work on only one side of the dust pan for now. The 12 by 12 starting rectangle helps show the overall shape. The body can be split and mirrored after the features are complete.
Build the Angled Side with Project Intersect and Join By Bend
The angled side needs to meet the lower part of the dust pan. A regular flange on the edge cannot match the needed angle. If the flange extends too far, it intersects the other geometry.
Create a sketch on the edge face of the hem. Use Project Intersect, then select the whole body. Fusion projects the body where it intersects the sketch plane.
Use the projected edges to draw the new side shape. Offset the first edge by 0.09, then offset the second edge by the same amount. The three-dot menu remembers recent values, so the second offset can reuse 0.09.
Continue the sketch by drawing down and across. Add a construction line from the front point to the projected edge. This keeps the point perpendicular to the projection.
Add the needed angle and set it to 155 degrees. Align the front point with the front edge, then leave the remaining geometry as drawn.
Finish the sketch and use Flange on the profile. The model now contains two separate sheet metal bodies.
Connect the Bodies with Join By Bend
The new Join By Bend command joins two edges with a bend. Select the two edges that should connect. Fusion changes the hem length slightly so the edges meet with a bend.
This makes the angled shape possible without forcing the flange to extend into the other body.
For fabrication, we will spot weld along the joined surface. Create a flange on the upper edge and drag it to preview the result. Change the extent from a distance to To Object, then select the target face. Fusion creates the flange at the correct distance for a spot weld along the top.
Repeat the same process on the other edge. Select the face as the object reference so the flange reaches the correct location.
Close the Dust Pan Corners with Corner Closure
The new flanges leave one wide opening and another offset opening at the corners. Corner Closure refines these intersections.
Select the two edges at the top corner. The command provides Symmetric Gap and Overlap Gap options. It also includes relief shapes such as Round, Square, and Tear.
Choose Laser Weld for the relief shape. Then set the gap width to:
thickness / 8
The smaller gap brings the walls closer together and creates a tighter corner. The Corner Closure edge and relief settings show the effect of these choices.
Apply the same Laser Weld corner closure to the bottom corner. Select both edges and use thickness / 8 again.
Compare Symmetric Gap and Overlap Gap
In the video, I show another example by selecting two inside edges and changing the formula to:
thickness / 4
With Symmetric Gap, the two edges stay separated by a gap. With Overlap Gap, one face moves across the other face.
You can flip which face overlaps and control the overlap amount. The setting can range from zero to 50% and then to a full overlap. The selected relief shape also changes the result. Round, Square, and Tear each produce a different corner.
Add Handle Mounting Flanges and Mirror the Dust Pan Body
Add a hem along the inside edge for more strength. Keep the same gap and length settings used for the earlier hem.
Next, create a flange on the edge where the handle will attach. A full-edge flange overlaps nearby geometry, so change the flange type to Two Offsets.
Fusion warns that the flange intersects the body, but it also lets you choose a new reference. Clear the original reference, then select the inside face instead of the outside edge.
Set the offset from the inside face to -0.1. This gives enough clearance from the nearby geometry. Set the overall height to 0.5 in.
Create this feature on only one side. The other side will come from the mirror.
Split the Body
Switch to the Solid tab and choose Split Body. Use the vertical center plane as the splitting tool. The starting rectangle was centered, so this plane divides the dust pan correctly.
Remove the unwanted half. Then return to the Sheet Metal tab.
Before mirroring, add one more hem to an edge.
Use Sheet Metal Fillet Before Mirroring
The finished body still has sharp corners. Fusion adds both Sheet Metal Fillet and Sheet Metal Chamfer commands for sheet metal edges.
A regular Fillet lets you select an edge that can cause problems when the part is laid out flat. The issue appears when Fusion tries to create orthographic shapes for the flat pattern.
Sheet Metal Fillet is more specific. It refuses the edge that the regular Fillet accepted, while allowing other orthographic edges. This helps prevent the wrong edge from being selected.
Set the fillet value to 0.2 and round the selected edges. Add another fillet to the rear edge and one more edge to reduce sharp corners.
The fillet was added after the mirror in the first attempt. To place it before the mirror, delete the fillet and drag the timeline marker before the mirror feature. Create the fillet again, then move to the end of the timeline and repeat the mirror command.
The final mirror also carries the fillets to the other side. The matching Sheet Metal Chamfer command is part of the same new sheet metal enhancement, although this edge treatment uses fillets.
Check the Part with Unfold Sheet Metal Part
Before creating the handle, check whether the dust pan can unfold correctly.
Choose Unfold Sheet Metal Part and select a planar face as the reference. Then select Unfold All Bends.
If the part lays flat and all bends unfold, the sheet metal body is manufacturable. A flat result also shows that the part has no overlapping faces that would stop it from folding back together.
Create the Handle with Project Intersect and Contour Flange
Right-click and create a new component. Set it as a Sheet Metal component, use the same sheet metal rule, and name it handle.
Create a sketch on the mid plane. Use Project Intersect again and select the entire dust pan body. Fusion projects the body where it intersects the sketch plane.
Use the projected shape to trace the handle. Mock up the overall profile and make it touch the front of the dust pan.
Use collinear constraints to align the handle lines. One line can be placed slightly off the target, then forced to be collinear with it.
To align a point with another line, draw a construction line between them. Make that construction line collinear with the target line. This brings the point into alignment without using a horizontal constraint.
Create a tangent arc for the rounded handle shape. Change the line type back to regular before drawing the arc. Add a tangent constraint at the second connection as well.
Control the overall handle shape with a dimension. Set its total height to 4.
Create the Handle Flange
Select the handle profile and use the Contour Flange command. Set the distance to 0.75, then change the direction to Symmetric so the flange extends 0.75 in both directions.
Check the side setting before accepting the feature. Side 1 places the handle outside the dust pan. Side 2 would place it inside, which is not the desired result.
Some of the handle will later be bent, rolled, or hammered. To remove sharp edges where the handle is held, add a hem to both handle edges at the same time. Use the formula:
thickness / 8
The completed handle can be spot welded to the back and the front of the dust pan.
Test the 5 in, 6 in, and 8 in Top Flange Changes
Activate the top-level component to view the finished dust pan. The strengthening hems run around the part and make the body sturdy.
Return to the top flange and change its height from 5 in to 6 in. The dust pan updates, and the handle grows slightly so it stays aligned with the front.
The handle updates because Project Intersect uses information from the dust pan body when creating the handle. Change the flange again, this time from 6 in to 8 in, and the handle grows with the new length.
Use undo and redo to compare the two versions and see how the connected features respond.
The Finished Fusion Sheet Metal Dust Pan
The completed design shows how the new functionality added into Fusion Sheet Metal can make your designs look better and be easier to design. Its features remain editable through the timeline, which keeps later design changes tied to the same dust pan.
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