Open topic with navigation

Orthotropic properties of slab members

The procedure to define an orthotropic slab

1. Open service Structure.

2. Start any function for the input of a slab member (plane 2D member, wall, shell member).

3. The property dialogue opens on the screen.

4. Fill in the required parameters.

5. Set the FEM model parameter to orthotropic.

6. A new item appears in the dialogue: Orthotropy.

7. Click the three-dot button [...] in this added line.

8. A dialogue with orthotropy parameters is opened on the screen.

9. Input correct values.

10. Confirm with [OK].

11. Confirm the slab-property-dialogue.

12. Input the slab member.

 If required the orthotropy parameters can be parameterised using the "slab bending stiffness" and " point stiffness" parameter-types. The units of these parameters are MNm and MN/m, respectively.

IMPORTANT: The direction of orthotropy is in general defined by the x-axis of the finite element. If the orthotropic 2D member has been input using function Plate, it is possible to control the direction of orhotropy. The local x-axis of each finite element follows the direction of the local x-axis of the plate. If the local x-axis of the plate is rotated, the direction of orthotropy rotates as well. On the other hand, if the plate is input using function Shell, it is not possible to control explicitly the direction of local x-axis of individual finite elements. Therefore, if orthotropy is to be applied in your model, it MUST be defined for Plates and not for Shells.

Orthotropy parameters

There are two cases of orthotropy :

1. physical orthotropy caused by different moduli in the x and y direction, i.e. a real material property due to the technology of material production (various layers, wood, etc.)

2. technical or shape orthotropy of ribbed plates / walls

a) Physical orthotropy

First we describe the parameters for the physical orthotropy. The orthotropic material is defined by the following physical constants:

h E1 E2 G12 G13 G23

The value of 21 is determined as follows :

v21 = v12 * E2/E1

The shear modulus G12 is determined using Kirchoff’s plate:

The parameters G13 and G23 are necessary because Mindlin’s plate element is used, with a substantial influence of shear forces qx and qy on the deformations.

We assume a plate/wall with a uniform thickness h.

The parameters entered in the program are calculated from these physical constants as follows:

A. For a plate element

For a plate element the angle Beta between the direction 1 (for which the orthotropy parameters are entered) and the local x direction of the element can be entered.

B. For a wall element

C. For a shell element

A shell element is a plate / wall element and possesses both kinds of physical constants with no additional constants.

b) Technical orthotropy

For technical or shape orthotropy we refer to P. Timoshenko, S. Woinowsky, Theory of plates and shells, McGraw Hill, second edition, 1987. The relation between the bending moments and the curvature of an orthotropic plate is given by the following relation:

The definition of moments an curvatures are as follows:

The following notations are used in the program:

D11 = Dx

D22 = Dy

D33 = 0.5 Dxy

D12 = Dx

D44 and D55 are added because Mindlin elements with shear force deformation are used. In many cases there are no simple formulas to calculate these stiffnesses. Shear force deformation is neglected (as by other FEM elements) when big values are entered for this two constants. Further a recommendation how to calculate these factors in some practical cases is given.

Determination of rigidities in various specific cases:

The expressions given for the rigidities are subject to slight modifications according to the nature of the material employed. In particular, all values of torsional rigidity Dxy based on purely theoretical considerations should be regarded as a first approximation, and a direct test must be recommended in order to obtain more reliable values of the modulus G. Usual values of the rigidities in some cases of practical interest are given below:

b.1) Isotropic plate

An isotropic plate with constant thickness is defined by : thickness h, modulus of elasticity E and Poisson coefficient :

b.2) Reinforced concrete slabs

Let Es be Young’s modulus of steel, Ec that of the concrete, c Poisson’s ratio for concrete, and n = Es / Ec. For a slab with two way reinforcement in the directions x and y we can assume:

In these equations, Icx is the moment of inertia of the slab material, Isx that of the reinforcement taken about the neutral axis in the section x = constant, and Icy and Isy are the respective values for the section y = constant.

It is obvious that these values are not independent of the state of the concrete. For instance, any difference of the reinforcement in the directions x and y will affect the ratio Dx / Dy much more after cracking of the concrete than before.

b.3) Slab reinforced by a set of equidistant ribs

In this case the orthotropic plate theory can only give a rough idea of the actual state of stress and strain of the slab.

With :

E = modulus of the material (for instance, concrete)

I = moment of inertia of a T section of width a1

Az = shear surface of a T section of width a1

C = torsional rigidity of one rib

= h / H 

When you enter this T section a geometric section, I, Az and C are calculated automatically by the program.

Then we may assume:

with D’xy the torsional rigidity of the slab without the rib

You can check this by taking the ribs not into account. The solution must be the same as for isotropic plates in section b.1.

b.4) Gridworks

The gridwork consists of two systems of parallel beams spaced equal distances apart in the x and y directions and rigidly connected at their points of intersection. The beams are supported at the ends, and the load is applied normal to the xy plane. If the distances a1 and b1 between the beams are small in comparison with the dimensions a and b of the grid, and if the flexural rigidity of each of the beams parallel to the x axis is equal to I1 and that of each of the beams parallel to y axis is equal to I2, the coefficients are as follows:

For all types of elements the thickness which is taken into account for the calculation of the dead weight must be entered in the Load t field. This thickness is multiplied with the density of the selected material.

For more information we refer to a separate section: "Library of Orthotropy".

Parameters for 2D-1D upgrade

The user who use SCIA Engineer function 2D-1D upgrade, want can specify additional stiffness coefficient (K^xy, K_yx). These coefficient represents stiffness in torsion in the x or y directions.

Torsion moment along main span of 1D beam is calculated by the following formula :

The assumption is that torsion moment extends along the whole span of 1D beam. The stiffness coefficients are used ONLY for results of 2D/1D upgrade (Internal forces on beam, export to the new project and export to the template).

Open topic with navigation