This blog will show three basic examples of how to use the Swept Boss/Base feature in SolidWorks. There are two main requirements to create a Swept Boss or Base: A closed profile and a path. This first example will show how to create a sweep using a circular profile and an open relatively linear path. Figure 1, below, shows the profile drawn on the front plane and the sweep path drawn on the top plane. It is important to make sure that the starting point of the path lies on the same plane as the profile. Also, notice how the center of the circle profile is centered on the start of my path. This ensures that the sweep will be centered to my profile; however, any location contained inside the profile, including the boundary, can be used to generate a sweep.
Figure 1: Profile and Path
Once your profile and sketch are defined, select the Swept Boss/Base command on the features tab as seen in Figure 2.
Figure 2: Swept Boss/Base Command
The command window will then appear on the left side of the screen. Click on the boxes under the Profile and Path section and select your profile and path sketches as seen in Figure 3. A preview of your sweep will appear to further verify your intended feature.
Figure 3: Command Manager & Execution
The green check mark on the top left of the command manager will execute the command and reveal the finished model as seen in Figure 4.
Figure 4: Example 1 Finished Model
This first example shows the basics of generating a sweep feature. Examples 2 and 3 dive into more complex geometry and some other capabilities of this command. Figure 5 shows the cross profile and the slot-shaped path used for the sweep in Example 2.
Figure 5: Example 2 Profile and Path
Selecting the Swept Boss/Base command and the two sketches above as the profile and path accordingly, Figure 6 shows the initial preview of the sweep. Expanding the options drop down in the command manager, as indicated by the red arrow in Figure 6, SolidWorks allows you to change the orientation of the profile along the sweep by assigning a profile twist. The profile twist can be specified by a twist value, direction vector, or by applying tangency to adjacent faces. In this example, a profile twist value of 720 degrees (also available in radians or revolutions) was set and can be seen in Figure 7.
Figure 6: Example 2 Command Manager and Preview
Figure 7: Assigning a Profile Twist
After hitting the green check, the resulting model from the sweep feature is shown in Figure 8.
Figure 8: Example 3 Model
This final example will cover how to setup and execute a sweep using guide curves. Guide curves in comparison to profile twist allow for a varying profile size along the path of the sweep. Figure 9 shows separate sketches of the square profile, line path, and the additional guide curve drawn on the same plane as the path. Make sure when adding a guide curve to a sweep that the pierce constraint is used to connect the start of the curve to the edge of the profile (see Figure 9). In utilizing guide curves, it is also crucial that profile of the sweep is not fully constrained otherwise the sweep will fail. In this example, the height of square profile is constrained but not the width.
Figure 9: Adding a Guide Curve Sketch
After sketching the profile, path, and guide curve on separate sketches, enter the Swept Boss/Base command manager and add in the profile and path designated in Figure 9 above. Select the guide curve drop down and, in the box, select the guide curve sketch from the feature tree (see Figure 10). Since the width of the profile is not constrained, it can follow the guide curve as it is swept down the intended path. After executing the command, the resulting model is seen in Figure 11.
Figure 10: Adding a Guide Curve in the Command Manager
Figure 11: Example 3 Model
That’s all for now! You now know the basics of the Swept Boss/Base. If you like the content or have questions, signup for our email list to stay in the loop for solutions or weekly content.