Part Modeling > Tweak Features > Radius Domes > To Create a Radius Dome
To Create a Radius Dome
The Radius Dome option allows you to create a dome feature. A radius dome deforms a surface and is parameterized by one radius and one offset distance.
It is useful for creating qualitative deformations on a surface. If you want more precise control over the geometry, use a section dome feature.
1. Set the allow_anatomic_features configuration option to yes to make the Radius Dome command available on the All Commands list.
2. Add the Radius Dome command to the desired user-defined group on the ribbon.
* For information about customizing the ribbon, see the Related Links.
3. Click Radius Dome.
4. Pick a surface to dome. The surface to dome must be a plane, torus, cone, or cylinder.
5. Select a datum plane, planar surface, or edge that is normal to the sketch plane to which to reference the dome arc.
6. In the Radius of dome box, type the dome radius, and click . The radius value can be positive or negative, resulting in a convex or concave dome.
The domed surface is created using two dimensions—the radius of the dome arc, and the distance from the arc to the reference datum plane or edge. The radius of the dome is the radius of an arc that passes through the two edges of the domed surface. Thus, a larger radius value results in less elevation from the original surface. The placement dimension affects the dome steepness. The closer the dome arc to the middle of the domed surface, the less the dome elevation.
On non-rectangular surfaces, the dome is trimmed to the part edges.