Constructing the Swept feature

1. On the CommandManager, click Sketch > Sketch.
2. Select the plane created normal to helix.
3. On the View (Heads Up) Toolbar, click View Orientation > Normal To.

1. Draw circle of 4 mm diameter.

1. On the CommandManager, click Sketch > Display/Delete Relations > Add Relations.
2. Click on the center point of the circle and helix.
3. On the PropertyManager, under the Add Relations section, select Pierce.

1. Click OK.

1. Click Exit Sketch and change the view orientation to Isometric.
2. To construct a Swept feature, click Features > Swept Boss/Base on the CommandManager.
3. Select the circle to define the profile.
4. On the PropertyManager, click in the Path selection box and select the helix to define the path.
5. Leave the default settings and click OK to construct the Swept feature.
6. On the View Heads-Up toolbar, click the Visibility drop-down and turn off the Plane and Curves icons.

1. Save and close the file.

You need to make sure that the size of the cross section is not larger than the curves on the path, the resulting geometry will intersect and the Swept will fail.

Note: In the above figure, the cross-section plane is normal to the path.

In SOLIDWORKS, you can create a profile anywhere along the path. For example, create a profile at the middle of the path, as shown. Activate the Swept tool and select the profile and path. On the PropertyManager, use the Direction 1, Birectional, and Direction 2 icons to Swept the profile.

Direction 1

Direction 2

Birectional

In SOLIDWORKS, you can select the face of a model to define the swept profile.