# 4.12 Orthotropic Surfaces and Membranes

General description

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 following figure shows the general stiffness matrix of an orthotropic surface in RFEM.

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.

You can find detailed information about Orthotropy in an English document that you can request from Dlubal Software.

An orthotropy is not entered directly but set as a parameter when defining a surface. When you create 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 Stiffness Multiplication Factors).

In the Stiffness Matrix tab, the respective elements of the matrix are displayed (see Figure 4.120).

During the RFEM 4 import, stiffness matrix elements are adjusted according to Equation 4.1.

Orthotropy Type

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.

Constant thickness

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.

Effective Thicknesses

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'.

No stresses are calculated for orthotropic surfaces: The different stiffness coefficients would cause "blurred" results because they refer to an average value of the thickness. These stresses do not correspond to the orthotropy model.

Stiffness Matrix

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

With this option, you can also customize generated coefficients (e.g. a coupling or ribbed floor).

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.

Coupling

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, enter the parameters of coupling thickness dp, 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:

Unidirectional ribbed plate

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 dp, rib height dr, 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.

Bidirectional ribbed plate

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 dp, rib height dr, rib spacing a, and rib width b for the directions x' and y' according to the scheme.

Trapezoidal sheet

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 bt, and bottom flange width bb according to the scheme.

Hollow core slab / Unidirectional box floor

Hollow units built in a ceiling reduce the self-weight, but produce orthotropic structural behavior. RFEM determines stiffnesses from the geometry parameters for slab thickness dp or total profile height h, and top/bottom flange width dp, rib or void spacing a, as well as 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.

Grillage

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 dp, rib spacing ax' and ay', as well as rib width bx' and by', which you have to specify according to the scheme shown in the Grillage dialog tab.

You can find details regarding the determination of stiffness components from geometric specifications in an English document that you can request from Dlubal Software.

Orthotropy Direction β

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.

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

Stiffness Multiplication Factors

You can reduce stiffnesses globally with the factor k, or individually for bending, torsion, shear, and membrane elements of the matrix (see Equation 4.16).

All stiffness elements

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

Bending stiffness elements

Use the factor kb 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.

Torsion stiffness elements

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.

Shear stiffness elements

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

Membrane stiffness elements

Use the factor km 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.

Literatur
 [4] Ivan Němec and Vladimír Kolář. Finite Element Analysis of Structures - Principles and Praxis. Shaker Verlag, Aachen, 2010.