4.7 Nodal Supports

Supports are used to transfer loads applied on a structural system into the foundations. Without any supports, all nodes would be free and could be displaced or rotated unhindered. If you want a node to act as a support, at least one of its degrees of freedom must be restricted by a spring or blocked. In addition, the node must be part of a surface or member. The boundary conditions of members must be considered as well, in order to exclude double releases on the supported nodes.

Nodal supports are required in order to apply imposed deformations.

It is possible to provide nodal supports with nonlinear properties (failure criteria for tensile or compressive forces, working and stiffness diagrams).

To open the following dialog box, go to the menu and select Insert → Model Data → Nodal Supports → Graphically or use the toolbar button shown on the left.

The following support types are predefined and can be selected from the list:

• Hinged (YYY NNY)
• Rigid (YYY YYY)
• Sliding in X' (NYY NNY)
• Sliding in Y' (YNY NNY)

After clicking [OK], you can assign the selected support type to nodes in the graphic.

Use the [New] button to create another type of support. The dialog box shown in Figure 4.90 is displayed.

Singular supports can only be defined on nodes. Enter the node number into the table column or the text box of the dialog box, or select it graphically.

Each nodal support has a local coordinate system. It is oriented parallel to the global axes X, Y, and Z by default. You can use the shortcut menu of a nodal support to display the support coordinate systems.

Use the User-defined axis system option to rotate the support's local axis system. Different options are available in the list.

It is possible to rotate the support about the support axes X', Y', and Z', to refer to a user-defined coordinate system or to certain nodes. In addition, you can align the support according to the position of a member or a line. In each case, it it possible to define the objects graphically in the work window by using .

The support rotation is displayed in the dynamic dialog graphic.

Often, real structural conditions are inaccurately represented by a nodal support, for example when the support zone has large dimensions. Such support conditions can be represented in RFEM by special column macro elements considering material and geometry of the column. RFEM calculates the spring stiffnesses and adjusts the support conditions. Due to the realistic modeling, you can avoid singularities that would be produced in a single FE node when a rigid support is defined.

The Model of support can be realized in three different ways, each symbolized in the dialog graphic:

• With the Elastic surface foundation model, a surface is cut out internally in the column dimensions and supported elastically. The foundation coefficients are calculated from the column's geometry and material data.
• With the Elastic nodal support model, a surface is also cut out. This surface is only supported at one node, however. The support is modeled by means of translational and rotational springs, which are calculated from the column geometry and its material. Internally, the surface thickness is duplicated to account for higher bending rigidity within the column area.
• The Node support with adapted FE mesh model corresponds to the elastic nodal support, but no springs are applied to the punctiform supports.

When modelling as an "Elastic surface foundation" or "Elastic nodal support", you have to enter the data for the column that is required to determine the spring stiffnesses. The column head's geometry can be Rectangular or Circular. If there is a steel cross-section as the Column cross-section, the cross-section can be set in the [Library] after activating the check box in the second line.

The Column material can be selected in the list of the defined materials or created with [New] (see Chapter 4.3). The Column height H influences the constants of the vertical and rotational springs. The Support conditions at the column head or column base have some influence on the determination of the translational and rotational springs of the support, just like the possible shear stiffness of the column.

The spring constants C that result from the column parameters are listed on the right in the dialog box.

To define a support, select the corresponding option in the dialog box or table. The check mark indicates that the corresponding degree of freedom is blocked and the node displacement in the corresponding direction is not possible.

If you do not want to define supports, clear the corresponding check box. Then, RFEM sets the constant of the translational spring to zero in the Nodal Support dialog box. It is always possible to modify the spring constant in order to display an elastic support of the node. In the table, enter the constant directly into the table column.

Assigning nonlinear support properties is described below.

Restraints are defined analogously to supports. The check mark indicates once again that the corresponding degree of freedom is blocked and the node displacement in the corresponding direction is not possible. In the same way, constants for rotational springs can be defined once the check box is cleared. In the table, enter the spring constant directly into the corresponding table column.

The following support properties are assigned to the buttons:

Table 4.3 Nodal support buttons

Button	Support Type
	Rigid
	Hinged with restraint about Z'
	Sliding in X' and Y' with restraint about Z'
	Sliding in X' with restraint about Z'
	Sliding in Y' with restraint about Z'
	Sliding in Z' and Y' with restraint about Z'
	Free

To control the transfer of internal forces in detail, it is possible to provide nodal supports with nonlinear properties. The list of nonlinearities includes the following options:

• Failure of component if support force or moment is negative or positive
• Complete failure of support if support force or moment is negative or positive
• Partial activity
• Diagram
• Friction depending on remaining support forces

The nonlinear properties can be accessed in the dialog box and table via the list (see Figure 4.90 and Figure 4.91). For each support's degree of freedom, you can specify whether and which forces or moments are transferred at the supported node.

Nonlinear effective supports are displayed with a different color in the graphic. In the table, support elements with nonlinear properties are indicated by a blue check box.

Both options represent an easy way to control whether the support can only take positive or negative forces/moments: If a force or a moment acts in the prohibited direction, that particular component of the support fails. The remaining retentions and restraints stay effective.

The negative or positive directions refer to the forces or moments that are placed in the nodal support with regard to the respective axes (they do not refer to the reaction forces of the support). Thus, algebraic signs result from the direction of the global axes. If the global Z-axis is oriented downwards, the load case "Self-weight" results in a positive support force P_Z.

In contrast to the abovementioned failure of a single component, the support fails completely once the component is ineffective.

To access the following dialog boxes, use the [Edit Nonlinearity] button in the dialog box or in the table, which are to the right of the list.

The support's effect can be defined separately for the Positive and Negative Zone. The sign convention is described in the previous paragraph. In addition to complete activity or complete failure, the support can be set to only be effective when it is displaced or rotated to a certain degree (in this case, a translational or rotational spring has to be defined in the Nodal Support dialog box beforehand). Furthermore, Tearing (failure of support when exceeding a certain force or moment) and Yielding (effective only until force or moment is reached) can be set in combination with a Slippage.

Look at the dynamic Activity Diagram to check the support properties.

The support's effect can be defined separately for the Positive and Negative Zone. First, define the number of steps (i.e. definition points) for the working diagram. Then, enter the abscissa values of the displacements or rotations with corresponding support forces or moments into the list.

There are several options for the Diagram after last step: Tearing for support failure on exceeding, Yielding for restricting the transfer to a maximum allowable support force or moment, Continuous like in the last step, or Stop for the restriction to a maximum allowable displacement or rotation followed by a rigid or restrained support activity.

Use the four friction options to set the transferred support forces to be in relation to the compressive forces that act in a different direction. Depending on your selection, the friction depends on only one support force or on the total force of two simultaneously acting support forces.

Click the button to open a dialog box where you can define the Friction Coefficient μ.

The following relation exists between axial force and friction force of the support:

$P_{\text{Support}}=\mu ·P_{\text{Axial force}}$

For restraints about the axes X' and Y', there is the additional entry Scaffolding in the list. With this option, it is possible to model the structural behavior of support plates at scaffoldings or bracings. This function is described in the following technical article:
https://www.dlubal.com/en/support-and-learning/support/knowledge-base/000973