This element is a general purpose quadratic shell element. The node numbering and the direction of the normal to the surface is shown in Figure 38.
In CalculiX, quatratic shell elements are automatically expanded into 20-node brick elements. The way this is done is illustrated in Figure 39. For each shell node three new nodes are generated according to the scheme on the right of Figure 39. With these nodes a new 20-node brick element is generated: for a S8 element a C3D20 element, for a S8R element a C3D20R element.
Since a shell element can be curved, the normal to the shell surface is defined in each node separately. For this purpose the *NORMAL keyword card can be used. If no normal is defined by the user, it will be calculated automatically by CalculiX based on the local geometry.
If a node belongs to more than one shell element, all, some or none of
the normals on these elements in the node at stake might have been defined by the user (by
means of *NORMAL). The
failing normals are determined based on the local geometry (notice, however,
that for significantly distorted elements it may not be possible to determine
the normal; this particularly applies to elements in which the middle nodes
are way off the middle position). The number
of normals is subsequently reduced using the following procedure. First, the
element with the lowest element number with an explicitly defined
normal in
this set, if any, is taken and used as reference. Its normal is defined as
reference normal and the element is stored in a new subset. All other
elements of the same type in the set
for which the normal has an angle smaller than with the
reference normal and
which have the same local thickness and offset are also included in this
subset. The elements in the subset are considered to have the same
normal, which is defined as the normed mean of all normals
in the subset. This procedure is repeated for the elements in the set
minus the subset until no elements are left
with an explicitly defined normal. Now, the element with the lowest
element number of all elements left in the set is used as
reference. Its normal is defined as
reference normal and the element is stored in a new subset. All other
elements left in the set
for which the normal has an angle smaller than
with the
reference normal and
which have the same local thickness and offset are also included in this
subset. The normed mean of all normals
in the subset is assigned as new normal to all elements in the subset. This procedure is repeated for the elements left until
a normal has been defined in each element.
This procedure leads to one or more normals in one and the same node. If only one normal is defined, this node is expanded once into a set of three new nodes and the resulting three-dimensional expansion is continuous in the node. If more than one normal is defined, the node is expanded as many times as there are normals in the node. To assure that the resulting 3D elements are connected, the newly generated nodes are considered as a knot. A knot is a rigid body which is allowed to expand uniformly. This implies that a knot is characterized by seven degrees of freedom: three translations, three rotations and a uniform expansion. Graphically, the shell elements partially overlap (Figure 40).
Consequently, a node leads to a knot if
In addition, a knot is also generated if
Beam and shell elements are always connected in a stiff way if they share common nodes. This, however, does not apply to plane stress, plane strain and axisymmetric elements. Although any mixture of 1D and 2D elements generates a knot, the knot is modeled as a hinge for any plane stress, plane strain or axisymmetric elements involved in the knot. This is necessary to account for the special nature of these elements (the displacement normal to the symmetry plane and normal to the radial planes is zero for plane elements and axisymmetric elements, respectively).
The translational node of the knot (cfr REF NODE in the *RIGID BODY keyword card) is the knot generating node, the rotational node is extra generated.
The thickness of the shell element can be defined on the *SHELL SECTION keyword card. It applies to the complete element. Alternatively, a nodal thickness in each node separately can be defined using *NODAL THICKNESS. In that way, a shell with variable thickness can be modeled. Thicknesses defined by a *NODAL THICKNESS card take precedence over thicknesses defined by a *SHELL SECTION card. The thickness always applies in normal direction. The *SHELL SECTION card is also used to assign a material to the shell elements and is therefore indispensible.
The offset of a shell element can be set on the *SHELL SECTION card. Default is zero. The unit of the offset is the local shell thickness. An offset of 0.5 means that the user-defined shell reference surface is in reality the top surface of the expanded element. The offset can take any real value. Consequently, it can be used to define composite materials. Defining three different shell elements using exactly the same nodes but with offsets -1,0 and 1 (assuming the thickness is the same) leads to a three-layer composite.
The treatment of the boundary conditions for shell elements is straightforward. The user can independently fix any translational degree of freedom (DOF 1 through 3) or any rotational DOF (DOF 4 through 6). Here, DOF 4 is the rotation about the global x-axis, DOF 5 about the global y-axis and DOF 6 about the global z-axis. No local coordinate system should be defined in nodes with constrained rotational degrees of freedom. A hinge is defined by fixing the translational degrees of freedom only.
For an internal hinge between 1D or 2D elements the nodes must be doubled and connected with MPC's. The connection between 3D elements and all other elements (1D or 2D) is always hinged.
Point forces defined in a shell node are modified if a knot is generated (the reference node of the rigid body is the shell node). If no knot is generated, the point load is divided among the expanded nodes according to a 1/2-1/2 ratio for a shell midnode and a 1/6-2/3-1/6 ratio for a shell endnode. Concentrated bending moments or torques are defined as point loads (*CLOAD) acting on degree four to six in the node. Their use generates a knot in the node.
Distributed loading can be defined by the label P in the *DLOAD card. A positive value corresponds to a pressure load in normal direction.
In addition to a temperature for the reference surface of the shell, a temperature gradient in normal direction can be specified on the *TEMPERATURE card. Default is zero.
Concerning the output, nodal quantities requested by the keyword *NODE PRINT are stored in the shell nodes. They are obtained by averaging the nodal values of the expanded element. For instance, the value in local shell node 1 are obtained by averaging the nodal value of expanded nodes 1 and 5. Similar relationships apply to the other nodes, in 6-node shells:
In 8-node shells:
Element quantities, requested by *EL PRINT are stored in the integration points of the expanded elements.
Default storage for quantities requested by the *NODE FILE and *EL FILE is in the shell nodes. The same averaging procedure applies as for the *NODE PRINT command. By using the OUTPUT=3D parameter in the first step one can trigger the storage in the expanded nodes. This has the advantage that the true three-dimensional results can be viewed in the expanded structure, however, the nodal numbering is different from the shell nodes.
Finally, in thin structures two words of caution are due: the first is with respect to reduced integration. Due to the small thickness hourglassing can readily occur, especially if point loads are applied. In that case, full integration might be necessary. Secondly, thin structures can easily exhibit large strains and/or rotations. Therefore, most calculations require the use of the NLGEOM parameter on the *STEP card.