Sweeps must follow these rules (Taken from SolidWorks Help on Sweep Rules):

• The profile must be closed for a base or boss sweep feature; the profile may be open or closed for a surface sweep feature.
• The path may be open or closed.
• The path may be a set of sketched curves contained in one sketch, a curve, or a set of model edges.
• The path must intersect the plane of the profile.
• Neither the section, the path, nor the resulting solid can be self-intersecting.
• The guide curve must be coincident with the profile or with a point in the profile sketch.

Circular Profile Along Simple Path

Doing a sweep with a circular path along a simple path is straightforward because circular profiles are built into the sweep tool. This makes it so this kind of feature only requires one sketch to create a new feature and doesn’t require any sketches when only modifying a feature (see SolidWorks Help: Creating Rods and Tubes with a Circular Profile). This type of feature would be common for parts made from wire, such as springs and paper clips, or solid cylindrical bar stock that is bent, such as rebar configurations.

To do this type of sweep, first sketch your path on the plane that will get you your desired orientation. A paper clip path sketch is shown above in figure 6.23 (construction lines were added to dimension the sketch based on the wire diameter of the steel used for the paper clip). Then, you must exit the sketch and choose the sweep option. In the property manager for sweep, select the “Circular Profile” option and click your path sketch for the path selection box. Finally set your size and confirm. If you expect your sweep to be all one piece, such as with the paper clip, then select the “Merge Tangent Faces” option.

Tubular Profile Along a Simple Path

Doing a tubular profile along a simple path is 90% like that of a circular profile except the thin-feature option in the sweep command is employed. We can see this through the handrail example shown below that the steps are the same as the circular profile sweep: Create a simple path sketch on the plane you desire to achieve correct orientation, exit the sketch, sweep with the circular profile and thin-feature options checked.

Custom Profile Along a Simple Path

Creating a custom profile along a simple path allows you the most control over your sweep because you can make the profile any way you want and the path. However, there are more steps to doing this kind of sweep. This sweep requires two sketches: a profile sketch and a path sketch of which must be intersecting the profile sketch. You can make sure of this intersection using a new relation called the Pierce Relation.

The process of creating a swept feature with a custom profile sketch and a path sketch is first creating the path sketch and then exiting the sketch. Then you make your profile sketch making sure to add a pierce relation between the relevant line on the path sketch and the appropriate point on your profile sketch. Then you choose the Swept Boss/Base tool from the CommandManager, select your profile sketch for the profile selection box, your path sketch for the path section box, set up your settings and confirm.

Profile Swept Along a Helical Path

A helix is a spiral in a 2 dimensional direction (see SolidWorks Help: Helix for more information). Examples of helixes in action are springs, threads, slinks, coils, oil grooves etc. You as a mechanical designer will most of the time use helixes for threads and springs. Within SolidWorks, there is a helix tool that allows you to automatically generate a 3D sketch of a helix for use in swept boss/bases (like with springs and coils) or swept cuts (like threads).

The helix and Spiral tool is located under the Curves dropdown on the features tab of the CommandManager. To create a helix, you first need a circular sketch, so the first step to creating the helix is starting a sketch on a plane that will represent the end of the helix. Then, you can go straight to the helix command to set your parameters for the helix.

When your helix is finished, if your profile is just circular, you go straight into the sweep command and proceed as you would for a circular profile along a simple path to complete your swept feature. If you require a custom path, you would create the path sketch, exit the sketch, and then proceed as you would for a custom profile simple path sweep.

This text continues in SolidWorks 2.