4.12 Orthotropic Surfaces and Membranes

Orthotropic surfaces have different stiffnesses in direction of the local surface axes x and y. Use orthotropic surface properties to model, for example, glued-laminated girders or ribbed floors. Orthotropic properties can be set for plane and quadrangle surfaces.

You can define orthotropic properties via material (material orthotropy with invariable geometry), geometry (irregular shape of surface with isotropic material), or as a combination of both.

The general stiffness matrix of an orthotropic surface in RFEM is as follows.

$\left[\begin{array}{c}{m}_x\\ m_y\\ m_{xy}\\ v_x\\ v_y\\ n_x\\ n_y\\ n_{xy}\end{array}\right]=\left[\begin{array}{cccccccc}{D}_{11}& D_{12}& D_{13}& 0& 0& D_{16}& D_{17}& D_{18}\\ & D_{22}& D_{23}& 0& 0& D_{26}& D_{27}& D_{28}\\ & & D_{33}& 0& 0& D_{36}& D_{37}& D_{38}\\ & & & D_{44}& D_{45}& 0& 0& 0\\ & & & & D_{55}& 0& 0& 0\\ & & \text{sym.}& & & D_{66}& D_{67}& D_{68}\\ & & & & & & D_{77}& D_{78}\\ & & & & & & & D_{88}\end{array}\right]·\left[\begin{array}{c}{\kappa }_x\\ {\kappa }_y\\ {\kappa }_{xy}\\ {\gamma }_{xz}\\ {\gamma }_{yz}\\ {\epsilon }_x\\ {\epsilon }_y\\ {\gamma }_{xy}\end{array}\right]$

Orthotropic surfaces can be calculated according to the linear static analysis, second-order analysis, or large deformation analysis. In case of matrices with pure membrane coefficients, only a large deformation analysis is possible.

An orthotropy is not entered directly but set as a parameter when defining a surface: When creating a new surface, define the Stiffness as Orthotropic or Membrane orthotropic (see Chapter 4.4). Then the [Edit parameters] buttons shown on the left become active in the dialog box and table.

The dialog box is divided into several tabs, which depend on the selected Orthotropy Type.

In the Stiffness Multiplication Factors dialog section, you can either reduce stiffnesses globally using the factor k, or individually for bending, torsion, shear, and membrane stiffness elements (see paragraph Stiffness Multiplication Factors).

In the Stiffness Matrix tab, the respective elements of the matrix are displayed (see Figure 4.121).

You can define orthotropic surfaces through material and geometry parameters or directly with coefficients of the local stiffness matrix. Depending on your specifications, tabs of the dialog box change.

The orthotropy types are described on the following pages. For each definition type, you have to specify the Thickness that you want to apply for determining the self-weight.

RFEM uses the orthotropic material properties that have been defined in the Material Model - Orthotropic Elastic 2D dialog box (see Figure 4.48). This type is only suitable for homogenous surfaces of equal thickness whose material has distinctive orthotropic properties.

In the Effective Thicknesses dialog tab, you can define different thicknesses in the directions x' and y' to represent unequal stiffness conditions.

The self-weight is not determined from the thicknesses entered in this dialog box; instead, RFEM uses the surface thickness entered in the Edit Surface dialog box or in Table 1.4 Surfaces.

RFEM displays the moduli of elasticity and shear for the material that is used (see Chapter 4.3) so that you can check corresponding data. Alternatively, it would be possible to control the orthotropic properties by means of material settings and to define the same thicknesses for the directions x' and y'.

The coefficients of the local stiffness matrix can be defined manually.

The [Info] button provides information about the relevance of coefficients in the stiffness matrix.

If the axes of the orthotropy are not consistent with the axes of the coordinate system of elements, you have to transform the matrices (see [4], page 305 - 313).

If you find out that the stiffness matrix is not positively definite when checking data before performing calculations, appropriate adjustments of coefficients are required.

Use this setting to model connections between surfaces or members, which are represented by coupling elements consisting of isotropic or orthotropic materials.

In the Coupling dialog tab, you can enter the parameters for coupling thickness d_p, coupling spacing a, and coupling width b according to the scheme. A realistic coupling model is given when the distance a is larger than the width b of the coupled elements.

The effective thickness d* is determined according to the following equation:

$d^{*}=d_p\frac{b}{a}$

The orthotropic properties of a ribbed floor are based on the principle of an uniaxially stressed T-beam ceiling. RFEM determines the stiffnesses from the geometry parameters of slab thickness d_p, rib height d_r, rib spacing a, and rib width b, which you have to specify according to the scheme shown in the Unidirectional Ribbed Plate dialog tab.

Please note that crack development (e.g. state II for concrete) is not taken into account when the stiffnesses are determined. Only isotropic materials are allowed.

This type of ceiling is characterized by webs that cross each other orthogonally in a uniform grid, thus dividing the floor into coffers. As with ribbed floors (see above), the orthotropic properties can be described by means of the geometry. You need to specify the stiffness parameters for two directions.

In the Bidirectional Ribbed Plate dialog tab, specify the parameters for slab thickness d_p, rib height d_r, rib spacing a, and rib width b for the directions x' and y' according to the scheme.

The option to display trapezoidal sheets as surfaces with orthotropic properties considerably facilitates the modeling of surfaces. RFEM determines the stiffness coefficients from the geometry parameters of the cross-section. Only isotropic materials are allowed.

In the Trapezoidal Sheet dialog tab, specify the parameters for the sheet thickness t, total profile height h, rib spacing a, top flange width b_t, and bottom flange width b_b according to the scheme.

Hollow units built in a ceiling reduce the self-weight, but produce orthotropic structural behavior. RFEM determines the stiffnesses from the geometry parameters for the slab thickness d_p or total profile height h, and the top/bottom flange width d_p, the rib or void spacing a, as well as the void diameter or rib width b. You have to specify these parameters according to the scheme shown in the Hollow Core Slab dialog tab.

Like for the remaining geometric orthotropies (effective thickness, trapezoidal sheet, unidirectional and bidirectional ribbed plate, grillage), only isotropic materials are allowed.

It is not only possible to display a grillage as a member model but also as an orthotropic surface. As for the remaining geometric orthotropies, only isotropic materials are allowed.

RFEM determines the stiffness coefficients from the geometry parameters for slab thickness d_p, rib spacing a_x' and a_y', as well as rib width b_x' and b_y', which you have to specify according to the scheme shown in the Grillage dialog tab.

The orthotropic direction refers to the surface's local axes x and y. The angle β describes the rotation of the x'-axis to the local x-axis of the surface. It is responsible for transforming the matrices available in the Transformed Stiffness Matrix dialog tab.

Use the Display navigator or the shortcut menu of a surface to display the coordinate systems of surfaces in the graphic (see Figure 4.122).

The positive angle β is defined clockwise around the positive local z-axis of the surface.

You can reduce stiffnesses globally with the factor k, or individually for bending, torsion, shear, and membrane elements of the matrix (see Equation 4.20).

All coefficients of the stiffness matrix are globally multiplied by a factor.

Use the factor k_b to adjust the coefficients D₁₁, D₁₂, D₂₂, and D₃₃ of the stiffness matrix, which represent the bending components. Entering factors between 0 (no flexural resistance) and 1 (full flexural resistance) is allowed.

The text box k₃₃ allows you to control the factor for torsional rigidity D₃₃ about the axes x' and y'. The input ranges from 0 (no twisting rigidity) to 1 (full twisting rigidity). For example, a small value is recommended for composite constructions with semi-rigid connections.

The factors k₄₄ and k₅₅ affect the coefficients D₄₄ and D₅₅ of the matrix (shear components).

Use the factor k_m to adjust the coefficients D₆₆, D₇₇, D₆₇, and D₈₈ of the stiffness matrix, which represent the axial force components. The input of factors between 0 (no membrane stiffness ) and 1 (full membrane stiffness) is allowed.