Part Modeling > Tweak Features > Section Domes > To Create a Blended Section Dome with No Profile
To Create a Blended Section Dome with No Profile
You can create a blended section dome feature without using a profile. In this case, the system creates the domed surface by blending parallel sections.
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 and No Profile.
5. Select the planar surface to turn into a dome.
6. Specify a sketching plane for the first section and sketch the first section. When selecting a sketching plane, the viewing direction arrow indicates the positive direction for offset sections.
7. When finished creating sections, click OK to exit Sketcher.
8. Enter the distance between the first section and the new section to sketch. The orientation of the sections is the same. Sketch the new section and click OK. At least two sections must be used for this option. Note that the previous sections are toggled to a light gray color when you sketch the new section.
Be sure to orient the start points of the sections so the correct points are connected for the dome. The start point is displayed as a small circle on the sketch. To reorient the start point, click Sketch > Setup > Feature Tools > Start Point.
9. If other sections are required, enter yes to continue and create new sections as needed. If no other sections are required, answer no to the prompt. The dome is generated.