About Shells and Plates
A shell is a thin-walled structure in 3D where a simple form is assumed for the variation of the displacement through the thickness. Using this approximation, it is possible to develop a model for the deformation that is more similar to a 2D plane stress condition than to a full 3D state.
For a shell to give accurate results it is important that the structure can really be described as being thin-walled. When modeling using shells you should in general model the faces at the midplane of the real geometry. You can use the offset setting if the midsurface of the shell does not coincide with the boundary of your geometry.
Plates are similar to shells but act in a single plane and usually with only out-of-plane loads. The plate and shell elements in COMSOL Multiphysics are based on the same formulation. The Plate interface for 2D models is a specialization of the Shell interface. In the following, the text fully describes the Shell interface, and the Plate interface is mentioned only where there are nontrivial differences.
A Shell interface can be active either on free surfaces embedded in 3D or on the boundary of a solid 3D object. In the latter case, it can be used to model a reinforcement on the surface of a 3D solid. A Plate interface can only be active on domains in 2D.
To describe a shell, you provide its thickness, a possible offset, and the elastic material properties.
The element used for the shell interface is of Mindlin-Reissner type, which means that transverse shear deformation is accounted for. It can thus also be used for rather thick shells. It has an MITC formulation where MITC means mixed interpolation of tensorial components. A general description of this element family is in Ref. 1.
The dependent variables are the displacements u, v, and w in the global x, y, and z directions, and the displacements of the shell normals ax, ay, and az in the global x, y, and z directions.
Figure 5-1: The degrees of freedom in the shell interface. N is the normal vector in the original configuration and n is the normal in the deformed state.
The degrees of freedom represent the displacements on the reference surface. The reference surface is the boundary where the shell element mesh is created. If an offset property is used, the reference surface differs from the physical shell midsurface. The displacement vector on the midsurface, u, can be expressed as
where uR is the displacement on the reference surface (the displacement degrees of freedom) and ζ0 is the offset. The rotational displacement a is the same on both midsurface and reference surface.
For input and output, the Shell interface to a large extent replaces the displacements of the shell normals by the more customary rotations θx, θy, and θz about the global axes. For a geometrically linear analysis, the relation between normal displacement and rotation vector is simple: where n is the unit normal of the shell.
For a standard plate analysis only three degrees of freedom are needed: the out-of-plane displacement w and the displacements of the shell normals ax and ay. It is also possible to activate all six degrees of freedom, so that any type of analysis of a shell initially positioned in the xy-plane can be performed using the Plate interface. Using six degrees of freedom is the default, but three degrees of freedom can be selected instead for efficiency.
Also for plates, the rotations θx, θy (and possibly θz) are used to a large extent.
When six degrees of freedoms are used in the Plate interface, there must be enough constraints to suppress any in-plane rigid body motions.
In the Shell interface, the coordinates are usually denoted with lower case letters (x, y, z). If a Solid Mechanics or Membrane interface is present in the same model, then it becomes necessary to make a difference between the material frame and the spatial frame (Material and Spatial Coordinates). In this case the coordinates in the Shell interface changes to (X, Y, Z).