# Finite elements

# 2D Plate

The 2D plate element has almost the same properties as the 3D plane shell element with one important difference: it is capable only of calculation of bending effects. The following section contains only the differences.

The element is planar, the plane of the structure is the XY plane, its loads are perpendicular to its plane. It is capable of calculation of bending and torsional moments and cross-directional shear forces. Degree of freedom of nodes are 3, w is the displacement in Z direction, φx and φy are rotation around X and Y axis, respectively. Interpolation of the displacement function is quadratic. The element with 8 nodes is well-known in the literature as serendipity element.

At definition of bedding (surface supports) it is possible to set them to resist only pressure (see non-linear calculation).

Material of the plate is orthotropic, relationship between strains and stresses are as follows:

Since the matrix of the material constants are symmetrical:

v_{rs} / v_{sr} = E_{r} / E_{s}

The k constant in the last row is the Winkler-type bedding factor. The element is loadable in the same way as the 3D plane shell element, according to common sense.

Results:

- w, φ
_{x}, φ_{y}are displacement and rotations of nodes, - M
_{x}, M_{y}are specific bending moments in the global X-Y coordinate system, - M
_{xy}is torsional moment, - T
_{x}, T_{y}is cross directional shear forces,

F_{z} is bedding (support) surface distributed forces.

The extremes of the stresses can be calculated from the above mentioned internal forces according to the following relationships (t is the thickness of the plate):

σ_{x} = 6 M_{x} / t^{2}, σ_{y} = 6 M_{y} / t^{2}

τ_{xz} = 3 T_{x} / (2t), τ_{yz} = 3 T_{y} / (2t), τ_{xy} = 6 M_{xy} / t^{2}

# 2D Wall

The 2D wall element, (also called disk element) has almost the same properties as the 3D plane shell element but it is capable only of calculation of the membrane effect. The following section contains only the differences.

The element is planar, the plane of the structure is the XY plane, its loads act in its plane, too. Degree of freedom of the nodes is 2: u and v, displacements in the X and Y directions. Interpolation of the displacement function is quadratic. The element with 8 nodes is well-known in the literature as serendipity element.

The element is capable of calculation on plane stress or plane strain state. Material of the plate is orthotropic, relationship between strains and stresses are as follows:

- In case of plane stress state:

- In case of plane strain state:

Results:

The result of the calculation for a given element in the nodes are as follows:

- σ
_{x}, σ_{y}are normal stresses in the X-Y plane - σ
_{ζ}is normal stress in the Z direction (only in case of plane strain state) - τ
_{xy}is shear stress, - σ
_{1},σ_{2},σ_{3}are principal stresses, - σ
_{VM}is the so called von Mises stress, which is calculated according to the following form:

The internal forces in the nodes of the connected elements are averaged over every region one by one. The sign rule of the internal forces:

# 2D Beam

The 2D beam element is a prismatic element with two nodes and straight axis. It is capable of calculation of beam-grids lying in the X-Y plane, loaded in Z direction, and in case of bent 2D slab structures for modelling of stiffening ribs and lintels. The applied (Timoshenkó-type) bar element has three degrees of freedom: w, the displacement in the global Z direction and φX, φY rotations. The shear deformations are taken into consideration similarly to the 3D element. Interpolation of the displacement function is implemented by polinomes of the third degree.

In the case of bent slab structures the element can be eccentric in the global Z direction, as it is represented in the following picture. In this case the bar element behaves like an element with inertia increased by the Steiner part, which gives correct results for the displacement of the slab structure from engineering point of view. However in this case the internal forces of the elements are calculated as a 3D bar element.

The possible loads and the results are appropriately the same as in case of the 3D beam element.

# 3D Shell

The 3D slab element is an isoparametrical, thick shell element with eight or six nodes, which can be used for modelling of spatial structures containing parts with plane centre surfaces. The element is capable of calculation of membrane (in-plane) and bending (perpendicular to plane) displacements and matching same time (engaged) internal forces. The number of degree of freedom is six per node: u, v, w displacements and φX, φY, φZ rotations, referring to the X, Y, Z directions of the global coordinate system. Interpolation of displacement functions is implemented by second order functions. In all elements beside the eight nodes on the perimeter there is a ninth node in the centre of the element, which is invisible to the user. The interpolation function belonging to the ninth node is the so called bubble-function, which is zero on the perimeter of the element. It only has a role in the elimination of numerical problems during the calculations (shear locking, membrane locking). Applying the thick shell theory makes it possible to calculate the shear effect more accurately perpendicular to the plane.

As a result of application of shell theory (or more accurately Kirchoff hypothe- sis referring to displacements) the rotation stiffness of the structure perpendicular to the centre plane is zero. It only has effect if the analyzed structure is a plane slab. In this case the rotation around the normal direction of the plate has to be fixed in at least one point additional to the statically determined support of the slab. It is unnecessary, if the structure itself fixes this rotation, i.e. beams or columns connected to the slab, or the structure contains more connected slabs with not parallel centre plane. If the whole structure is in one plane, it is more practical to use wall or plane plate element, because it eliminates the above mentioned problem, moreover the number of degree of freedom of the structure is much lesser at the same element division and calculation accuracy. The thick- ness of the element can vary linearly. The elastic surface bedding is taken into consideration according to the linear Winkler model, which also allows the bed- ding factor to vary linearly.

Application of the element requires the usage of three different Descartes coordinate systems. Coordinates of nodes, certain type of loads and node displacements among the results are defined in the global (structural) X, Y, Z system. The calculated internal forces can be defined in the local (region) x, y, z system, where z is the normal direction of the region and finally the r, s, z system defines the main directions of orthotropy.

In case of orthotropic material the r, s axes lying in the centre plane define the material main directions. In this system the relationship between deformations and stresses is the following (Hook law):

The thermal expansions in direction of r, s axes developed by T temperature:

In case of isotropic material two material constants, E and u define the elastic material property:

Loads:

- Gravity (dead) loads, in the downward vertical direction, by default the global -Z,
- Forces and moments acting on one point, in any point of the structure,
- Linearly varying line load,
- Linearly varying surface load (pressure),
- Thermal load linearly varying align the surface and align the element thickness,
- Support motions at the rigid or elastic surface and point supports.

Results:

- Displacements and rotations in the global (X, Y, Z) coordinate system,
- Eight internal force and five stress coordinates in the local (x, y, z) coordinate system.

Calculated internal forces (force and moment referring to unit length):

- M
_{x}, M_{y}bending moments, - M
_{xy }torsional moment, - T
_{x}, T_{y}cross directional shear force, - N
_{x}, N_{y}, N_{xy}membrane forces.

Variation of stress coordinates along the thickness can be calculated from the internal forces according to the following relationships:

where t is the element thickness.

# 3D Beam

The beam element is an element with two nodes which has a straight axis. It is usable for analysis of spatial trusses and structures containing bars among others. The number of degree of freedom is six per node: u, v, w displacements and φX, φY, φZ rotations, referring to the X, Y, Z directions of the global coordinate system. The applied (Timoshenko) bar theory also makes it possible to take into consideration the shear deformations. Interpolation of displacement and rotation functions are implemented by the third order polynomials.

Application of the element requires the usage of four different Descartes coordinate systems. Coordinates of nodes, certain type of loads and node displacements among the results are defined in the global (structural) X, Y, Z system. The x, y, z local coordinate system fits to the node, where x is parallel with the axis of the bar element, and y, z define the plane of the cross-section. The calculated internal forces can be defined in the x', y', z' axes, origined from the centre of gravity, which are parallel with x, y, z, respectively. In the plane of the cross- section x and h axes, originated from the centre of gravity, define the cross-sectional main directions.

Cross-section of the element is arbitrary but its size and orientation is constant along one element. Since the node (connection point) and the centre of gravity can be different in a cross-section, this element is capable of analysis of structures containing bars with eccentric connections.

A typical structure for this case is a ribbed slab. In this case the node of the rib (bar) element is on the centre plane of the slab but the centre of gravity of the bar can differ from it.

Loads:

- Gravity (dead) loads, in the downward vertical direction, by default the global-Z,
- Forces and moments acting on one point, in any point of the structure,
- Linearly varying line load,
- Thermal load linearly varying align the length and align the cross-section,
- Support motions at the rigid or elastic point supports.

Results:

- Displacements and rotations in the global (X, Y, Z) coordinate system,
- Six internal forces in the local (x', y', z') coordinate system, with its origin in the centre of gravity,
- M
_{y}, M_{z}bending moments, - M
_{x}torsional moments, - V
_{y}, V_{z}shear forces, - N
_{z}normal force.

# 3D Solid

These 3D elements are isoparametric solid elements with 4/10 nodes (Tetra), 6/18 nodes (Wedge) or 8/27 nodes (Brick), which can be used for modeling of spatial structure. The number of degree of freedom is three per node: u, v, w displacements. Interpolation of displacement functions is implemented by linear (4/6/8 node) or second-order (10/18/27 node) function (standard/fine). The numerical integration method is performed in a full manner for element stiffness. The element node numbers and the integration schemes are the following:

4 node tetra element, parametric coordinate system, node numbering and integration point (1 pc)

10 node tetra element, parametric coordinate system, node numbering and integration points (15 pcs)

6 node wedge element, parametric coordinate system, node numbering and integration points (9 pcs)

18 node wedge element, parametric coordinate system, node numbering and integration points (18 pcs)

8 node brick element, parametric coordinate system, node numbering and integration points (8 pcs)

27 node brick, parametric coordinate system, node numbering and integration points (27 pcs)

Application of the element requires the usage of two different Cartesian coordinate systems.

- Coordinates of nodes, certain type of loads and nodal displacements among the results are defined in the global (structural) X, Y, Z system.
- The x, y, z system defines the main directions of orthotropy. In this system the relationship between deformations and stresses is the following (based on Hooke’s law):

The connection between the local and global coordinate system is the following:

The thermal expansions in direction of x, y, z axes developed by temperature:

In case of isotropic material two material constants, E and ν define the elastic material property:

where:

Loads:

- Gravity (dead) loads, in the downward vertical direction, by default the global -Z
- Forces acting on one point, in any point of the structure, in global system
- Linearly varying line load, in global system
- Linearly varying surface load (pressure), in global system
- Thermal load linearly varying align the elements
- Shrinkage load, in x, y, z direction
- Support motions at the rigid or elastic surface and point supports.

Results:

- Displacements in the global (X, Y, Z) coordinate system
- Six stress components in the global (X, Y, Z) coordinate system.

# Point Support

The element is a point-like elastic support element with 6 degrees of freedom, meant in local coordinate system. In the general case it can be defined by 3-3 stiffnesses against motions and rotations. It is possible to make the element to resist only compression (see non-linear calculation). In case of infinitely rigid supports the program modifies the stiffness coefficients in order to avoid numerical problems and substitutes them with proper values for the calculation.

The element can be loaded by support motion but only if it resists both tension and compression. The results of the elements are line reaction forces and moments in the local coordinate system of the element. The reaction forces are positive in case of extension of the spring, and negative at compression.

# Line Support

Spatial, line aligned, elastic support element with 6 degrees of freedom per node.

The element is isoparametric, has 3 nodes in order to fit the surface elements, al- ways meant in local coordinate system. The degrees of freedom for a node of the element: u, v, w, φx, φy, φz. There is possibility to make the element resist only tension (see non-linear calculation). In case of infinitely rigid supports the pro- gram modifies the stiffness coefficients in order to avoid numerical problems and substitutes them with proper values for the calculation.

The 3D element can be defined by 3-3 stiffnesses against motion and rotation which are constant along the given line. In the 2D modules (i.e. Plate, Wall) only the appropriate stiffnesses can be defined and only they are considered during the calculation. For example, in the Wall module only stiffnesses against motion in x and y directions can be defined.

The element can be loaded by support motion but only if it resists both tension and compression. The results of the elements are line reaction forces and moments distributed along the length of the element according to quadratic function. They are always meant in the local coordinate system of the element. The reaction forces are positive in case of extension of the spring, and negative at compression.