Both triangular and quadrilateral shell elements are available currently in the software. Either can be linear or parabolic order. Shell elements are used to model thin structures where the thickness is significantly smaller than the dimensions in the other directions.
Linear Triangular Shell
Parabolic Triangular Shell
Linear Quadrilateral Shell
Parabolic Quadrilateral Shell
Elemental Geometry
The element x-direction is defined as shown in the images above for shell elements. Notice that when automeshed the G1 and G2 grid points (used to define the element x-direction) can be defined randomly throughout a mesh, hence the requirement to define a material x-direction to align the element output. Elemental z is defined from the node ordering. This can be either clockwise or counter-clockwise. G1-G2-G3 defines the element z-direction using the right-hand rule for the linear triangular shell. Element y is calculated from element z and element x.
Formulation Options
There are two orders of elements available for triangular and quadrilateral elements in the software: linear and parabolic. Linear triangular elements have three nodes while parabolic triangular elements have 6 nodes. Linear quadrilateral elements have 4 nodes while parabolic quadrilaterals have 8 nodes.
Degrees of Freedom
Shell elements support five (5) degrees of freedom per node with a stiffness based degree of freedom in the out-of-plane rotational degree of freedom. Users do not typically change this value, but can be done so as an advanced change to the K6ROT parameter under Parameters in the model tree. This stiffness is only mentioned here to point out that this is not a true degree of freedom for the element and should not be treated as such.
Additionally, a full six (6) degree of freedom shell element can be used globally by setting the parameter SHELLRNODE to ON under Parameters in the model tree. The changes described above are for advanced users, and should not be made unless the user knows the full extent of what they are doing.
Element Output
All shell element results are in the element coordinate system. It is important to note this because if a directional stress is desired, users must map the direction of the element x-direction using a material orientation. The default element x-direction is based on the node order of the shell elements. Because the auto mesher “connects the dots” in a consecutive fashion, the element x-directions can end up pointing in many different ways throughout a plane. Output for shells consists of a top and bottom value. This is useful because the top may be in compression while the bottom is in tension. Top and bottom is signified by the element z-axis. This vector can be viewed by right-clicking on Total Elements, then Normal Display and Vector or Color. Element normal vectors can be reversed.
Color Option – Yellow Defines the Top
Vector Option – Vectored Side Defines the Top