Note
This element is typically used for modeling prismatic and non-prismatic tapered structural members that are relatively long compared to section dimensions. The element can be also used as load-transfer elements connecting other elements having differing numbers of d.o.f.

In-span concentrated loads, distributed loads, temperature gradient loads and prestress loads can be applied to beam elements.

A beam element has 6 d.o.f. per node reflecting axial, shear, bending and torsional stiffness. When shear areas are omitted, the corresponding shear deformations of the beam element are ignored.

The beam element is formulated on the basis of the Timoshenko beam theory (a plane section initially normal to the neutral axis of the beam remains plane but not necessarily normal to the neutral axis in the deformed state) reflecting shear deformations. If the ratio of the section depth to length is greater than 1/5, a fine mesh modeling is desirable because the effect of shear deformations becomes significant.

The torsional resistance of a beam element differs from the sectional polar moment of inertia (they are the same for circular and cylindrical sections). You are cautioned when the effect of torsional deformation is large, as the torsional resistance is generally determined by experimental methods.

Beam and truss elements are idealized line elements, thus their cross-sections are assumed to be dimensionless. The cross-sectional properties of an element are concentrated at the neutral axis that connects the end nodes. As a result, the effects of panel zones between members (regions where columns and beams merge) and the effects of non-alignment of neutral axes are not considered. In order for those nodal effects to be considered, the beam end offset option or geometric constraints must be used.

The tapered section may be used when the section of a member is non-prismatic. It may be desirable to use a number of beam elements to model a curved beam.

When members are connected by pins or slotted holes (<Figure 2> (a) and (b)), the Beam End Release option is used.

Note that a singularity error can result in a case where a particular degree of freedom is released for all the elements joining at a node, resulting in zero stiffness associated with that degree of freedom. If it is inevitable, a spring element (or an elastic boundary element) having a minor stiffness must be added to the corresponding d.o.f.

         (a) Pin connection                                          (b) Slot-hole connection

(c) When multiple beam elements are pin connected at a node

Note
When several beam elements are pin connected at a node, the degree of freedom for at least one element must be maintained while the ends of all other elements are released in order to avoid singularity.

   (d)   When elements having different d.o.f. are connected

<Figure 2> Examples of end-release application

The rigid beam element can be effectively used when elements having different degrees of freedom are connected. The rigid effect is achieved by assigning a large stiffness value relative to the contiguous beam elements. In general, a magnitude of 105 ~ 108 times the stiffness of the neighboring elements provides an adequate result, avoiding numerical ill conditions

<Figure 2> (d) illustrates the case where a beam member is joined to a wall. The wall element may be a plane stress or plate element. The nodal in-plane moment corresponding to the beam element's rotational degree of freedom will not be transmitted to the planar element (plane stress or plate element) because the planar element has no rotational stiffness about the normal direction to the plane. The interface will behave as if the beam was pin connected. In such a case, a rigid beam element is often introduced in order to maintain compatible connectivity. All degrees of freedom of the rigid beam at the beam element are fully maintained while the rotational and axial displacement degrees of freedom are released at the opposite end.

 

Note 1
Thick and Thin plates are distinguished by whether or not shear deformation is considered. Refer to "Important Aspects of Element Selection" of Analysis Manual.

 

Note 2
This element can be used to model the structures in which both in-plane and out-of-plane bending deformations are permitted to take place, such as pressure vessels, retaining walls, bridge decks, building floors and mat foundations.

Pressure loads can be applied to the surfaces of the elements in either the GCS or ECS.

A plate element can be either quadrilateral or triangular in shape where its stiffness is formulated in two directions, in-plane direction axial and shear stiffness and out-of-plane bending and shear stiffness.

The out-of-plane stiffness used in MIDAS/Civil includes two types of elements, DKT/DKQ (Discrete Kirchhoff elements) and DKMT/DKMQ (Discrete Kirchhoff-Mindlin elements). DKT/DKQ were developed on the basis of the Kirchhoff Thin Plate theory. Whereas, DKMT/DKMQ were developed on the basis of the Mindlin-Reissner Thick Plate theory, which results in superb performances on thick plates as well as thin plates by incorporating appropriate shear strain fields to resolve the shear-locking problem. The in-plane stiffness of the triangular element is formulated in accordance with the Linear Strain Triangle (LST) theory, whereas the Isoparametric Plane Stress Formulation with Incompatible Modes is used for the quadrilateral element.

The user may separately enter different thicknesses for an element for calculating the in-plane stiffness and the out-of-plane stiffness. In general, the self-weight and mass of an element are calculated from the thickness specified for the in-plane stiffness. However, if only the thickness for the out-of-plane stiffness is specified, they are calculated on the basis of the thickness specified for the out-of-plane stiffness.

Similar to the plane stress element, the quadrilateral element type is recommended for modeling structures with plate elements. When modeling a curved plate, the angles between two adjacent elements should remain at less than 10? Moreover, the angles should not exceed 2~3?in the regions where precise results are required.

It is thus recommended that elements close to squares be used in the regions where stress intensities are expected to vary substantially and where detailed results are required.

<Figure 3> Example of plate elements used for a circular or cylindrical modeling

 

Note
This element can be used for modeling membrane structures that are subjected to tension or compression forces in the plane direction only. Pressure loads can be applied normal to the perimeter edges of the plane stress element.

The plane stress element may retain a quadrilateral or triangular shape. The element has in-plane tension, compression and shear stiffness only.

Quadrilateral (4-node) elements, by nature, generally lead to accurate results for the computation of both displacements and stresses. On the contrary, triangular elements produce poor results in stresses, although they produce relatively accurate displacements. Accordingly, you are encouraged to avoid triangular elements at the regions where detailed analysis results are required, and they are recommended for the transition of elements only (<Figure 4>).

Singularity errors occur during the analysis process, where a plane stress element is joined to elements with no rotational degrees of freedom since the plane stress element does not have rotational stiffness. In MIDAS/Civil, restraining the rotational degrees of freedom at the corresponding nodes prevents the singularity errors.

When a plane stress element is connected to elements having rotational stiffness such as beam and plate elements, the connectivity between elements needs to be preserved using the rigid link (master node and slave node) option or the rigid beam element option.

Appropriate aspect ratios for elements may depend on the type of elements, the geometric configuration of elements and the shape of the structure. However, aspect ratios close to unity (1:1) and 4 corner angles close to 90?are recommended. If the use of regular element sizes cannot be achieved throughout the structure, the elements should be square shaped at least at the regions where stress intensities are expected to vary substantially and where detailed results are required.

Relatively small elements result in better convergence.

<Figure 4> Crack modeling using quadrilateral/triangular elements

Note
This element can be used to model a long structure, having a uniform cross section along its entire length, such as dams and tunnels. The element cannot be used in conjunction with any other types of elements.

Pressure loads can be applied normal to the perimeter edges of the plane strain element.

Because this element is formulated on the basis of its plane strain properties, it is applicable to linear static analyses only. Given that no strain is assumed to exist in the thickness direction, the stress component in the thickness direction can be obtained through the Poisson's effect.

The plane strain element may retain a quadrilateral or triangular shape. The element has in-plane tension, compression and shear stiffness, and it has tension and compression stiffness in the thickness direction.

Similar to the plane stress element, quadrilateral elements are recommended over the triangular elements, and aspect ratios close to unity are recommended for modeling plane strain elements.

Refer to Create Element>Plane Stress Element.

Note
This element can be used for modeling a structure with axis symmetry relative to the geometry, material properties and loading conditions, such as pipes, vessels, tanks and bins. The element cannot be used in conjunction with any other types of elements.

Pressure loads can be applied normal to the circumferential edges of the axisymmetric element.

Because this element is formulated on the basis of its axisymmetric properties, it is applicable to linear static analyses only. It is assumed that circumferential displacements, shear strains and shear stresses do not exist.

Similar to the plane stress element, quadrilateral elements are recommended over the triangular elements, and aspect ratios close to unity are recommended for modeling axisymmetric elements.

Refer to Create Element>Plane Stress Element.

 

 

Note
This element is used for modeling three-dimensional structures, and its types include tetrahedron, wedge and hexahedron.

Pressure loads can be applied normal to the surfaces of the elements or in the X, Y, and Z-axes of the GCS.

The use of hexahedral (8-node) elements produces accurate results in both displacements and stresses. On the other hand, using the wedge (6-node) and tetrahedron (4-node) elements may produce relatively reliable results for displacements, but poor results are derived from stress calculations. It is thus recommended that the use of the 6-node and 4-node elements be avoided if precise analysis results are required. The wedge and tetrahedron elements, however, are useful to join hexahedral elements where element sizes change.

Solid elements do not have stiffness to rotational d.o.f. at adjoining nodes. Joining elements with no rotational stiffness will result in singular errors at their nodes. In such a case, MIDAS/Civil automatically restrains the rotational d.o.f. to prevent singular errors at the corresponding nodes.

When solid elements are connected to other elements retaining rotational stiffness, such as beam and plate elements, introducing rigid links (master node and slave node feature in MIDAS/Civil) or rigid beam elements can preserve the compatibility between two elements.

An appropriate aspect ratio of an element may depend on several factors such as the element type, geometric configuration, structural shape, etc. In general, it is recommended that the aspect ratio be maintained close to 1.0. In the case of a hexahedral element, the corner angles should remain at close to 90? It is particularly important to satisfy the configuration conditions where accurate analysis results are required or significant stress changes are anticipated. It is also noted that smaller elements converge much faster.

 

 

Some results seem strange to me. In the attached model, left side is without drilling DOF, and the right is with. Yet still, both produce bending moment (I was expecting the left to be 0 at the connection with the plates, thus, beam behaving as simply supported). Where is this bending moment coming from? Also, notice that this diagram is only obtained if the section of the beam is very small (2mm x 2mm). For any decent size section, the stiffness of the drilling degree of freedom appears to be negligible, as the bending moment diagram is almost perfectly 'simply supported'. Is it supposed to provide any adequate stiffness, or is it more of a 'no singularity problem' tool, just so there is some minimum stiffness provided'?

A1. A: As you observed, the plate element without drilling dof is assigned a very small rotational stiffness so that no singularity problem can occur. There is additional information below.

Plate element without drilling vs. plate element with drilling
- Plate element without drilling
Typical plate elements have three translational and two rotational dof at a node. These element types produce very reliable results as long as we use undistorted and square-shaped elements. But when we use relatively long rectangular elements, shear locking problem can occur, which cause very stiff response. So, incompatible mode was added. This is the explanation about plate element without drilling in Gen.

- Plate element with drilling
The above element types may give inaccurate results for the distorted mesh. In order to reduce the mesh distortion sensitivity and enhance the coarse mesh accuracy, we have introduced plate element with drilling degrees of freedom. This element type is particularly convenient in the analysis of shell structure and available at some sophisticated CAE software e.g. Abaqus, Nastran. The deficiencies of this element type are the zero energy mode (hourglass deformation) and that the node rotations are not true rotations. The boundary conditions of these elements have a high influence in the results. The rotations should be fixed at the boundaries because the node rotations are not true rotations. 

A1. There are mainly three methods for performing forward Construction Stage analysis. All three with their procedure and limitation are mentioned below.

Depending on the requirements and suitability you can choose your analysis method.