TUTORIAL 5

In this tutorial, you will create a Swept Flange feature. The Swept Flange tool allows you to create a sheetmetal feature by sweeping a profile along the path.

1. Open a new SOLIDWORKS part file.
2. On the CommandManager, click Sketch tab > Sketch.
3. Click on the top plane.
4. On the CommandManager, click Sketch tab > Arc drop-down > Centerpoint Arc
5. Select the origin point of the sketch.
6. Move the pointer downwards, and then specify the start point of the arc, as shown.

1. Move the pointer in the anti-clockwise, and then click to define the end point of the arc, as shown.

1. Create a vertical centerline, as shown.

1. Press and hold the Ctrl key, and then click on the two end points of the arc and the centerline.
2. On the PropertyManager, click the Symmetric icon.
3. Click OK.

1. Add dimensions to the sketch, as shown.

1. Click Exit Sketch on the CommandManager.
2. Change the View Orientation to Isometric.
3. On CommandManager, click the Features tab > Reference Geometry drop-down > Plane.
4. Select the arc and anyone of its endpoints.
5. Click OK on the Plane PropertyManager.
6. Start a new sketch on the newly created plane.
7. Draw the sketch profile, as shown.

1. Click Exit Sketch on the CommandManager.

Next, you need to activate the Swept Flange tool and create the swept flange. By default, the Swept Flange tool is not displayed on the CommandManager. To add this command to the CommandManager, right click on the CommandManager, and then select Customize. On the Customize dialog, click the Commands tab, and then select Sheet Metal from the Categories list. Next, click and drag the Swept Flange button from the Buttons area, and then release it on the CommandManager; the Swept Flange button is added to the CommandManger.

1. On the Menu bar, click Insert > Sheet Metal > Swept Flange.
2. Select the profile and path from the graphics window.
3. Click OK to create the swept flange.

1. Save and close the part file.