Home » How to use Swept Cut in SolidWorks?

How to use Swept Cut in SolidWorks?

In this article, we are going to explain what is Swept Cut and how to use it.

Swept Cut is used to cut a solid body by sweeping a closed profile or a tool body along a path. It is similar to Swept Boss/Base except for the fact that Boss/Base adds material and Swept cut simply cuts the material.

There are 3 types of Swept Cut:

  1. Sketch Profile: Creates a swept cut by moving a 2D profile along the defined path.
  2. Circular Profile: Cuts material by moving a circular profile along the defined path.
  3. Solid Profile: Removes material by moving a solid body along the defined path. The most common usage is in creating cuts around cylindrical bodies and is useful for end mill simulation.

1. Sketch Profile:

1. To create a Swept Cut, we must have a Solid Body. Open a part file that has a Solid Body. For this tutorial, we are going to use a simple extruded cylinder.

2. Now let’s create a Profile that will represent the section of the swept cut and a Path along which we want our cut to sweep. The Sketch01 (highlighted in sky-blue) represents our Path and Sketch02 is our Rectangular profile.

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Note: The Profile must be closed for a swept cut feature. The profile may be open or closed for a surface sweep feature. The Path can be open or closed.  

Tip: The Profile or Path can be a set of sketched curves or lines that you made in a 2D or 3D sketch (Non-planer 3D sketches are not allowed), a curve, or a set of model edges (Yes, you can directly select faces, edges, and curves from your model too).

3. Go to Insert-> Cut->Sweep or select Swept Cut present in the Features Tab.

4. Choose the Sketch Profile option under the Profile and Path menu. Now select the profile and the path to create the swept cut.

The following controls are available when the path extends through a profile, as it is in our case:

  • Direction 1: Creates a sweep for one side of the path.
  • Bidirectional: Creates a sweep that extends in both directions of the path from a sketch profile.
  • Direction 2: Creates a sweep for the other direction of the path.

5. Click the Green Checkmark and you’ll have your Swept cut.

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A Thin feature option is also available in which the profile lines are thickened and used to cut instead of using the entire interior region of the profile to cut the solid body.

2. Circular Profile:

1. This method is similar to the Sketch profile but in this step, you don’t need to sketch the profile.

We are going to use a cylindrical extruded solid body and a Helix as a path in this example.

2. This time select the Circular Profile option under the Profile and Path menu. Now select the path and the diameter of the circular profile.

3. Click Green Checkmark to complete the process.

3. Solid Profile:

1. Create a Solid Body that will act as a tool and it is going to cut everything it touches on the main body as it travels on the path.

The tool body must be convex, not merged with the main body, and consist of one of the following:

  • A revolved feature that consists of analytical geometry only, such as lines and arcs.
  • A cylindrical extruded feature.

For this example, we are going to use a Revolved feature to create the tool. Make sure to uncheck the Merge Result option to keep the tool body as a separate body.

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Note: The path must be tangent within itself (no sharp corners) and begin at a point on or within the tool body profile.

2. Now initialize the Swept cut feature and select Solid Profile under the Profile and Path menu. Choose the tool body as Profile and the Helix as the Path.

Tip: If the preview is not available, Check the Show preview option under the Options menu.

3. Click on the Green Checkmark. It may take some time to finalize the cut as it requires more computational power than the above methods. Also, the tool body will get absorbed/deleted by the Swept Cut feature automatically and you’ll be left with the original main body.

So in this quick tutorial, you learned how to use the Swept Cut tool in SolidWorks.