About the Shell Feature
The shell feature hollows out the inside of the solid, leaving a shell of a specified wall thickness. You can specify surfaces to remove from the shell. If you do not select a surface to remove, a closed shell is created, with the whole inside of the body hollowed out, with no opening to the inside. In this case, you can later add the necessary cuts or holes to achieve proper geometry. If you flip the thickness side (for example, by entering a negative value, or by clicking 
on the Shell tab), the shell thickness is added to the outside of the body.
on the Shell tab), the shell thickness is added to the outside of the body.When defining a shell, you can select surfaces and assign a different thickness to them. You can specify independent thickness values for each such surface. However, you cannot enter negative thickness values, or flip the thickness side, for these surfaces. The thickness side is determined by the default thickness of the shell.
The shell feature allows you to select the adjacent tangent surfaces. This enables you to remove or offset (independently or with different thickness) the surfaces that are tangent to their neighboring surface at one or more boundaries. At the tangent edge, where the separation of the shell offset occurs, a normal capping surface is constructed to close the gap.
You can also exclude one or more surfaces from being shelled by specifying the surfaces in the Exclude surfaces collector. This process is called partial shelling. You can also exclude surfaces with adjacent tangent surfaces. The system cannot shell geometry that is normal to the surfaces specified in the Exclude surfaces collector.
When the shell is created, the body geometry that was made of solid features before you create the shell feature is hollowed out. Therefore, the order of feature creation is very important when you use shell. See the example in the links.
You can shell all the bodies in the model, or selected bodies.
To access the shell feature, click > 
Shell.
Shell.