About Section Domes
A section dome replaces a planar surface with a sculptured surface. This surface can be defined by a sweep or a blend.
The swept dome uses two perpendicular cross sections to create the sculptured surface. The blended dome uses parallel sections blended together to create the new surface. With the blended dome, you can use a reference profile to help generate the sections.
Before creating the section dome feature, consider the following restrictions:
• The surface to be domed must be horizontal when you sketch the sections.
• Specify the sketching plane for the section dome as you would normally sketch on a part. Because the cross sections must be perpendicular to the profile, it may be necessary to reorient the view between sketches using the View option.
• Material is added or removed while a section dome is created, depending on how high or low the section is sketched in relation to the specified surface. For example, if the sections are attached to the surface, some material around the edges will be removed.
• Sections should not be tangent to the sides of the part.
• You cannot add a dome to a surface that is filleted along any edge. If you want a fillet, add the dome first, then fillet the boundary.
• It is not necessary to have the same number of segments for each section.
• Sections should be at least as long as the surface and do not have to be attached to the surface.
• Sections must be sketched to be open.