Element Library

In FrontISTR, the element groups shows in Table 4.1.1 can be used for analysis. Since HEC-MW is used to input the mesh data into FrontISTR, the following descriptions of the element library is based on the description of HEC-MW. The element library is shown in Figure 4.1.1, and element connectivity and the definitions of the surface number are shown in Figure 4.1.2.

Table 4.1.1: Element Library List

Element Types	Element No.	Description
Line element	111	Two node link element
	112	Three node link element
Plane element	231	Three node triangular element
	232	Six node triangular quadratic element
	241	Four node quadrilateral element
	242	Eight node quadrilateral quadratic element
Solid element	301	Two node truss element
	341	Four node tetrahedral element
	342	Ten node tetrahedral quadratic element
	351	Six node pentahedral element
	352	Fifteen node pentahedral quadratic element
	361	Eight node hexahedral element
	362	Twenty node hexahedral quadratic element
Connector element	511	Two node connector element (spring, dashpot)
Interface element	541	Quadrilateral cross section linear element
	542	Quadrilateral cross section quadratic element
Beam element	611	Two node beam element
	641	Two node beam element (with four 3-dof nodes)
Shell element	731	Three node three-dimensional linear element
	732	Six node three-dimensional quadratic element
	741	Four node three-dimensional linear element
	743	Nine node three-dimensional quadratic element
	761	Three node three-dimensional linear element (with six 3-dof nodes)
	781	Four node three-dimensional linear element (with eight 3-dof nodes)

Figure 4.1.1: Element Library

Structural and Plane Elements in Analyses Considering Large Deformation

In an analysis that considers large deformation (geometric nonlinearity), that is, a static or dynamic analysis with NONLINEAR in !SOLUTION (including TYPE=NLSTATIC and TYPE=STATICEIGEN), some beam, shell and plane elements cannot be used or can be used only under a condition. For a model that contains an element that cannot be used, the analysis stops after it starts with the message Element type not supported for nonlinear static analysis.

Element type	Treatment in an analysis considering large deformation
741	In nonlinear static analysis, finite rotation is handled when the material is elastic (!ELASTIC). The Total Lagrange formulation is used by default, and specifying CAUCHY in !ELASTIC selects the Updated Lagrange formulation. The Updated Lagrange formulation does not support an orthotropic material or a laminate with an orthotropic layer. In nonlinear dynamic analysis, finite rotation is not supported, and the element can be used only when INFINITESIMAL is specified for the material.
731, 743	Can be used only when INFINITESIMAL is specified for the material. The element is treated as infinitesimal deformation.
231, 232, 241, 242	Can be used only when INFINITESIMAL is specified for the material. The element is treated as infinitesimal deformation.
611, 641, 761, 781	Cannot be used. The analysis stops even when INFINITESIMAL is specified for the material.

Element 741 is the only shell element that handles finite rotation. To treat a thin-walled structure with large rotation in an analysis that considers large deformation, model it with 741. Beam elements and the elements with 3-dof nodes cannot be used in an analysis that considers large deformation, so represent a beam-like member with solid elements. INFINITESIMAL and CAUCHY are parameters of the material keywords. See !ELASTIC for details.

(Line Element)

(Triangular Plane Element)

Surface No.	Linear	Quadratic
1	1 - 2	1 - 6 - 2
2	2 - 3	2 - 4 - 3
3	3 - 1	3 - 5 - 1

(Quadrilateral Plane Element)

Surface No.	Linear	Quadratic
1	1 - 2	1 - 5 - 2
2	2 - 3	2 - 6 - 3
3	3 - 4	3 - 7 - 4
4	4 - 1	4 - 8 - 1

(Tetrahedral Element)

Surface No.	Linear	Quadratic
1	1 - 2 - 3	1 - 7 - 2 - 5 - 3 - 6
2	1 - 2 - 4	1 - 7 - 2 - 9 - 4 - 8
3	2 - 3 - 4	2 - 5 - 3 - 10 - 4 - 9
4	3 - 1 - 4	3 - 6 - 1 - 10 - 4 - 8

(Pentahedral Element)

Surface No.	Linear	Quadratic
1	1 - 2 - 3	1 - 9 - 2 - 7 - 3 - 8
2	4 - 5 - 6	4 - 12 - 5 - 10 - 6 - 11
3	1 - 2 - 5 - 4	1 - 9 - 2 - 14 - 5 - 12 - 4 - 13
4	2 - 3 - 6 - 5	2 - 7 - 3 - 15 - 6 - 10 - 5 - 14
5	3 - 1 - 4 - 6	3 - 8 - 1 - 13 - 4 - 11 - 6 - 15

(Hexahedral Element)

Surface No.	Linear	Quadratic
1	1 - 2 - 3 - 4	1 - 9 - 2 - 10 - 3 - 11 - 4 - 12
2	5 - 6 - 7 - 8	5 - 13 - 6 - 14 - 7 - 15 - 8 - 16
3	1 - 2 - 6 - 5	1 - 9 - 2 - 18 - 6 - 13 - 5 - 17
4	2 - 3 - 7 - 6	2 - 10 - 3 - 19 - 7 - 14 - 6 - 18
5	3 - 4 - 8 - 7	3 - 11 - 4 - 20 - 8 - 15 - 7 - 19
6	4 - 1 - 5 - 8	4 - 12 - 1 - 17 - 5 - 16 - 8 - 20

(Connector Element)

To connect two nodes by a discrete spring or dashpot, the 2-node connector element (element type 511) is used. A connector element gives only stiffness or damping between the two nodes it connects; it has no shape, no cross section and no mass.

A connector element can represent four kinds of characteristics, which are determined by the material assigned to the element.

• Axial spring — a spring acting along the axis connecting the two nodes. Its direction follows the deformation of the model. It is given by !SPRING_A.
• Spring with specified degrees of freedom — a spring connecting a specified degree of freedom of one node with a specified degree of freedom of the other node. Its direction is determined by the degree-of-freedom numbers and does not follow the deformation. A different spring constant can be given for each direction. It is given by !SPRING_D.
• Axial dashpot — damping acting along the axis. It is given by !DASHPOT_A.
• Dashpot with specified degrees of freedom — damping connecting specified degrees of freedom. It is given by !DASHPOT_D.

A spring contributes to the stiffness matrix and a dashpot to the damping matrix. Therefore a spring is effective in static, dynamic and eigenvalue analysis, whereas a dashpot is effective only in implicit dynamic analysis, in which the damping matrix is assembled, and has no effect in static analysis.

To place a spring between a node and the ground instead of between two nodes, use the spring boundary condition (!SPRING) rather than a connector element. It requires no element and elastically supports a degree of freedom of a node.

A connector element is defined in the mesh data as an element of type 511, and a section of section type INTERFACE is given to its element group. The spring constant and the damping coefficient are given as a material in the analysis control data. See !SPRING_A for details.

(Beam Element)

(Beam Element with 3-dof nodes)

Nodes 1 and 2 for translational DOF, nodes 3 and 4 for rotational DOF.

(Triangular Shell Element)

Surface No.	Linear	Quadratic
1	1 - 2 - 3 [front]	1 - 6 - 2 - 4 - 3 - 5 [front]
2	3 - 2 - 1 [back]	3 - 4 - 2 - 6 - 1 - 5 [back]

(Triangular Shell Element with 3-dof nodes)

Node 1, 2 and 3 for translational DOF, nodes 4, 5 and 6 for rotational DOF.

Surface No.	Linear
1	1 - 2 - 3 [front]
2	3 - 2 - 1 [back]

(Quadrilateral Shell Element)

Surface No.	Linear	Quadratic
1	1 - 2 - 3 - 4 [front]	1 - 5 - 2 - 6 - 3 - 7 - 4 - 8 [front]
2	4 - 3 - 2 - 1 [back]	4 - 7 - 3 - 6 - 2 - 5 - 1 - 8 [back]

(Quadrilateral shell Element with 3-dof nodes)

Nodes 1, 2, 3 and 4 for translational DOF, nodes 5, 6, 7 and 8 for rotational DOF.

Surface No.	Linear
1	1 - 2 - 3 - 4 [front]
2	4 - 3 - 2 - 1 [back]

Figure 4.1.2: Connectivity and Surface Number