Part Modeling > Tweak Features > Section Domes > To Create a Blended Section Dome with a Single Profile
To Create a Blended Section Dome with a Single Profile
1. Set the allow_anatomic_features configuration option to yes to make the Section Dome command available on the All Commands list.
2. Add the Section Dome command to the desired user-defined group on the ribbon.
* For information about customizing the ribbon, see the Related Links.
3. Click Section Dome. The OPTIONS menu appears.
4. Click Blend, click One Profile, and then click Done.
5. Select the surface from which to make a dome.
6. To create the profile, select a sketching plane, sketch the profile, and select OK.
7. To create the first section, select a sketching plane that is perpendicular to the profile. The viewing direction of the section indicates the positive offset direction for additional sections. After orienting the sketching plane, the system displays a set of crosshairs at the intersection of the sketching plane and the profile.
When you sketch the section, the system displays a circular start point at the beginning of the sketch. All start points for additional sections should be lined up. When you have finished with the sketch, click OK.
8. To sketch the next section, select the sketching plane and sketch the section. At least two sections are required for a blended dome.
9. If another section is required for the dome, answer Yes to the prompt asking if you want to proceed to the next section, then sketch the next section. Note that the previous parallel sections toggle to a light gray color. If no other section is required for the dome, answer No to the prompt to complete the dome.
* A dome is always created over the entire specified surface. If the sections are sketched where they do not cover the entire surface, the dome is extended as necessary to complete it.