6.4 Surface Loads

Surface loads act on all 2D elements of a surface (see Chapter 4.4).

To apply a surface load, a surface must already be defined.

If a surface is divided into surface components because of an intersection (see Chapter 4.22), the surface load does not act on components that are set inactive. Openings are omitted from the surface load as well.

The number of the surface load is automatically assigned in the New Surface Load dialog box but can also be changed there. The numerical order is not important.

In this text box, define the numbers of the surfaces on which the load acts. You can also select them graphically by using .

If you have selected the graphical input by clicking the toolbar button, you have to enter the load data first. You can select the relevant surfaces one by one in the work window after clicking [OK].

Define the type of load in this dialog section. Certain parts of the dialog box and columns of the table are disabled depending on your selection. The following load types can be selected:

The parameters for surface and member loads due to shrinkage can be defined in a separate dialog box, accessible with the button (see Figure 6.25).

Shrinkage as a time-dependent change in volume without external load action or effects of temperature can be classified into drying shrinkage, autogenous shrinkage, plastic shrinkage, and carbonation shrinkage. The shrinkage ε_cs(t,ts) at the moment of the considered concrete age t is determined from the essential influencing variables in the shrinkage process (relative humidity RH, effective structural thickness h, concrete strength f_cm, type of cement Z_Type, age of concrete at beginning of shrinkage t_s).

Click [OK] to transfer the value to the New Surface Load dialog box as the axial strain ε.

The load can act on the surface as Uniform, Linearly variable, or Radial.

Define load values for three nodes. The nodes are used to define a plane.

If the surface load is variable in the direction of an axis of the global coordinate system, load values of two nodes are required. The nodes may lie outside of the stressed surface, provided that FE nodes are generated there (i.e. the nodes are not allowed to be free).

For radially acting forces and temperature loads, you have to define the axis of the radial distribution in a separate dialog box. Use the button to open the dialog box.

The load can act in the direction of the local surface axes x, y, z or the global axes X, Y, Z.

Loads that act perpendicular to the surface are usually defined as local in direction z. Examples of application are wind loads that act on roof surfaces or internal pressure on tank shells.

To display the axes, use the Display navigator where you select Model → Surfaces → Surface Axis Systems x,y,z. You can also use the shortcut menu of a surface (see Figure 4.122).

The orientation of the local surface axes is irrelevant for the calculation according to the linear static analysis, if the load acts in direction of an axis of the global coordinate system XYZ. For nonlinear calculations, however, differences between locally and globally defined loads are possible: If the load is defined with a global direction of action, it keeps this direction when finite elements start to twist. In case of a local direction of action, however, the load twists according to the distortion of elements.

The load is converted to the projection of the surface in one of the directions of the global coordinate system. Select this option to define a snow load on the projected ground-plan area of a roof, for example.

The graphic in the lower right of the dialog box illustrates the projected surfaces.

In this dialog section or these table columns, the load values and, if applicable, the assigned nodes are managed. The text boxes are labeled and accessible depending on the previously activated selection fields.

Enter the load values into these fields. Adjust the signs according to the global or local orientations of axes.

If a linearly variable load is selected, you have to specify several load values. The dialog graphic in the upper right corner illustrates the load parameters.

If a linearly variable load is selected, specify three nodes on which the load magnitudes can be determined. The nodes are used to define a plane. You can also select nodes graphically with .

It is possible to create loads from area weights of materials that act as laminated layers. In this way, you can easily determine the structure of floorings or floor coverings., for example

You can access the function in the New Surface Load dialog box (Figure 6.23) by using the button to the right of the text box of the magnitude. In the shortcut menu, select Multilayer Composition.

The Multilayer Composition Library opens where you can select material layers or define new compositions.

The concept of the multilayer database matches that of the material library (see Chapter 4.3). Use the and buttons to create or modify user-defined multilayer compositions.

The Layers can be composed individually. Moreover, you can use the button to access the material library (see Chapter 4.3).

RFEM determines the area weight (table column E) from the Thickness and Specific Weight. An arrow shown in the dialog graphic indicates the current layer.

Confirm all dialog boxes with [OK] to import the area weight into the initial dialog box. A green triangle appears in the text box (see graphic shown on the left in the page above), indicating the parameterized input value. Click the triangle to once more access the input parameters for modifications.