Surfaces

Surfaces describe the geometry of planar or curved structural components whose surface dimensions are significantly larger than their thicknesses. The stiffness of a surface results from its material and thickness. When generating the FE mesh, 2D elements are created for surfaces. These are applied for the calculation in the surface's centroidal axis.

To enter a surface, you can use existing boundary lines. If you describe the surface graphically using the options in the Navigator context menu or the toolbar buttons (see image Buttons for Planar Surfaces), the definition lines are automatically created after defining the surface parameters and clicking OK in the dialog box.

The Basic tab manages elementary surface parameters. By selecting check boxes, additional tabs are added where you can make the specific specifications.

Stiffness Type

The stiffness type controls in which way internal forces can be absorbed or which properties are assumed for the surface. Various types are available for selection in the list.

Standard

The surface transfers moments and membrane forces. This approach describes the general behavior of a homogeneous and isotropic surface model. The stiffness properties of the surface are direction-independent.

Without Thickness

The surface has no stiffness. This type is to be used for the boundary surfaces of a solid.

Rigid

With this stiffness type, very stiff surfaces can be modeled in order to model a rigid connection between objects.

Membrane

The surface has a uniform stiffness in all directions. However, only membrane forces in tension (n_x, n_y) and membrane shear forces (n_xy) are transferred. For compressive forces, shear forces, and moments, the affected surface elements fail.

Without Membrane Tension

Only moments and membrane forces in compression are transferred. For membrane forces causing tension, the affected surface elements fail (example: hole bearing).

Load Transfer

With this type, surface loads can be applied to areas that are not filled with surfaces, such as wind loads on windows or the members of a hall. The load of this surface is distributed to the edges or the integrated objects. If member loads are generated, the load is converted into the global directions related to the true member lengths (load directions X_L, Y_L, Z_L). The surface itself has no stiffness.

The criteria for the load transfer can be defined in the Load Transfer tab.

The 'load transfer direction' describes the direction(s) in which the load should be applied to the objects. The list offers options for an isotropic distribution based on an FEM analysis as well as for an orthotropic arrangement on surface strips that are applied in one or both local surface axes for determining the load influence width.

With the 'Isotropic | FEM' option, RFEM uses a separate partial model to determine the load distribution, in which the surface is represented by a rigid surface element. All objects integrated into the surface (members, line and nodal supports, lines connected to model elements, couplings or nodes, etc.) are replaced by rigid lines or rigid nodal supports. The reactions of this partial model are then applied as loads for the 3D calculation of RFEM. If certain objects should not transfer loads, you can specify them in the 'Without Effect on' section.

For the load transfer via surface strips, you can define how RFEM should perform the 'load distribution'. By default, the load is distributed to the adjacent objects with a variable progression. However, if you want to achieve a constant load progression, select the corresponding entry in the list. The difference between the two variants is contrasted in the following image.

The input options for the 'surface strip width', the 'smoothing factor', and the 'minimum number of strips on the surface' are accessible if the Advanced Distribution Settings check box is activated in the 'Options' section. Adjustments are only required for problematic load distributions. The effect of these parameters is explained in the technical article Advanced Distribution Settings for Load Transfer Surfaces using an example.

For the load transfer surface, you can also define a 'basis weight' in order to take into account, for example, the self-weight of a glazing.

In the 'Without Effect on' section, you can exclude members, lines, and nodes from the load transfer (for example, bracings). Define the objects individually or select a template object that lies parallel to the unloaded members or lines.

Once the boundary lines of the surface are defined, the loaded members, lines, and nodes are specified in the 'Loaded Objects' section. If you want a specific load distribution, select the Load Distribution Factor check box in the 'Basic' tab. You can then define the factors for the load-transferring objects individually in the Load Distribution Factors tab.

For the load transfer via surface strips, you can take into account the 'member eccentricity' or the 'section distribution' in order to correctly capture the geometric position of a member or its course (see chapter Cross-Section). The 'neglect rotational equilibrium' check box is not activated by default. This means that the moment from the surface loads is formed about the center of gravity and compared with the moment from the member loads about the center of gravity. For nodal loads, however, this option is irrelevant. The following image shows how a free line load is distributed to the opposite members with and without taking the rotational equilibrium into account.

Stiffening

With this stiffness type, the stabilizing effects of trapezoidal sheeting, purlins, and bracings can be taken into account easily and realistically in the modeling.

A stiffening surface is not considered as an object with a stiffness effect. Rather, it represents the geometric basis for defining the members and objects lying in the stiffening surface and for determining their stiffening effect. Therefore, for a stiffening surface, the Deactivate for Calculation check box is automatically selected and cannot be deselected.

The criteria of the stiffening surface can be defined in the Stiffening, Parameters, and Tolerances tabs.

Stiffening

Two stiffening types are available for selection, which differ fundamentally.

• Surface

The stiffening effect of a trapezoidal sheeting is represented by an orthotropic surface that is connected to the attached members via rigid couplings. The stiffness of the fasteners is taken into account by line hinges in the rigid couplings.

With the 'stress direction', you define the orientation of the trapezoidal sheeting. It influences the orientation of the orthotropic surface and is taken into account when defining the orthotropy properties. The x and y axes refer to the local xyz axis system of the surface.

In the 'Members Connected to Surface' section, the members that are considered as secondary beams and longitudinal beams of the trapezoidal sheeting are automatically entered. These are all members within the defined Tolerances in the plane of the stiffening surface and perpendicular or parallel to the stress direction of the trapezoidal sheeting.

The 'Without Effect on' section offers the option to exclude certain members from the automatic assignment as connected members.

• Member Support

The stiffening effect of trapezoidal sheeting, purlins, or bracings is captured by member supports on the attached members, for which corresponding member shear panels and rotational restraints are created.

With the 'stiffening direction', you define the orientation of the trapezoidal sheeting or the purlins. The x and y axes refer to the local xyz axis system of the surface.

In the 'Supported Members' section, the members that bound the exterior span of the stiffening surface or lie closest to a boundary of the stiffening surface or are located in an inner bay of the surface are automatically entered. The Tolerances apply in the plane of the stiffening surface and for the orientation perpendicular to the stiffening direction.

The 'Without Effect on' section offers the option to exclude certain members from the automatic assignment as connected members.

Result Surface

This stiffness type makes it possible to convert stresses and forces of other objects into surface internal forces using an integration method. This allows you, for example, to determine the membrane and bending stresses of a solid, which are to be designed with different partial safety factors.

Further criteria for integrating results can be defined in the Result Surface tab.

In the 'Integrate Stresses and Forces' section, select whether the results should be captured purely object-related or also geometrically within an area. In the 'Include Objects' section, define the relevant surfaces and solids. Alternatively, select 'All' objects and then exclude certain elements in the 'Excluded from Inclusive Objects' section.

If the results of a certain area "below" and "above" the surface are to be integrated, you can define the relevant distances in the 'Parameters' section. They refer to the local z axis perpendicular to the surface plane.

Geometry Type

The geometry type describes the formal concept of a surface. Various types are available for selection in the list.

Planar

For a planar surface, all boundary lines lie in one plane. Various shapes of planar surfaces are accessible via the list button.

You can define the surface graphically (after clicking OK in the dialog box) by dragging a rectangle, circle, etc. If you 'select the boundary', RFEM automatically recognizes the surface as soon as a sufficient number of boundary lines is fixed.

Quadrangle

In its basic form, this surface type describes a general four-sided surface. Straight lines, arcs, polylines, and splines are possible as boundary lines. This allows curved surfaces to be modeled.

In the 'New Surface' dialog box, define the boundary lines of the quadrangle surface. If the closed surface cannot be formed by four lines, more than four lines are also permitted. In the 'Quadrangle' tab, the four corner nodes are then specified. They control how the curved surface is spanned.

NURBS

NURBS surfaces are formed from four closed NURBS lines (see chapter Lines). This allows almost any freeform surfaces to be modeled.

In the 'New Surface' dialog box, define the boundary lines of the NURBS surface. The respectively opposite pairs of NURBS lines must have the same number of control points so that the order of these NURBS lines is "compatible". In the 'NURBS' tab, you can then influence the shape of the surface via the 'control point weights'. The coordinates of the selected control point are specified in the 'Coordinates - Control Point' section.

Trimmed

If surfaces intersect, you can quickly create the intersection: Select the surfaces and then open the context menu. Various options are available for selection.

With the 'Create Intersection' option, only the intersection line is generated. If you select one of the 'Split by Intersection' options, RFEM creates partial surfaces and assigns them the type 'Trimmed'. You can then delete components if, for example, you want to remove protruding surfaces.

Rotated

A rotated surface is created when an existing line is rotated about an axis. RFEM creates the surface from the start and end nodes as well as the rotated definition points of the line. New lines are generated in the process.

In the 'Rotated' tab, define the boundary line of the surface to be rotated. Specify the rotation angle α. You can determine the points of the rotation axis via the coordinates or graphically using the button .

Pipe

A pipe surface is created when the center line of the pipe is rotated at a radius about this axis. New lines are generated in the process: two circles and a polyline parallel to the pipe axis.

In the 'Pipe' tab, define the radius of the pipe. This value describes the distance from the pipe axis to the center of the surface. Specify the number of the center line or select the pipe axis graphically using the button .

If the pipe cross-section is conical, activate the 'Different Radius at End' check box and enter the corresponding value.

Spline with Minimum Curvature

With this geometry type, you can create a curved surface using control nodes that lie on or outside the surface. For example, terrain surfaces can be modeled in this way.

Define the 'coordinate system' of the reference plane and enter the 'sample coordinates in the coordinate system'. These points represent the control nodes of the spline surface. Then define the 'boundary lines of the reference plane' or select the lines graphically using the button .

Thickness with Material

In the list of existing thicknesses, select the appropriate type or define a new thickness (see chapter Thicknesses).

Material of Thickness

The material of the thickness defined in the section above is preset. If necessary, you can select a different material in the list of already created materials or define a new one (see chapter Materials). This material is then assigned to the thickness type.

Hinges

With a hinge, the transfer of internal forces along a line of the surface can be controlled (see chapter Line Hinges. After selecting the check box, you can define the hinge type in the 'Hinges' tab.

Supports

If the surface is elastically supported, you can select or redefine the surface support in the 'Support' tab (see chapter Surface Supports).

Release

To decouple the model at the surface, you can select or redefine a surface release in the 'Release' tab (see chapter Surface Releases).

Eccentricity

With an eccentricity, a vertical offset of the entire surface can be modeled (see chapter Surface Eccentricities). You can define the offset type in the 'Eccentricity' tab.

Load Distribution Factor

For a surface of the Load Transfer type, it is possible to define distribution factors for the load-transferring objects. If you select the check box, you can assign these factors individually in a new tab.

The loaded objects of the load transfer surface are preset in one row. Each object is assigned the factor 1.00, so that all objects contribute equally to the load transfer. If you want a specific distribution, click in the next free row and select the line or member. Then assign the appropriate 'distribution factor'.

Mesh Refinement

The mesh size of the FE mesh can be adapted to the geometry of the surface (see chapter Surface Mesh Refinements). It is thus independent of the general mesh settings. In the 'Mesh Refinement' tab, you can select or redefine the surface mesh refinement.

Specific Axes

Every surface has a local coordinate system. As a rule, it is aligned parallel to the global axes. However, the coordinate system can also be defined by the user – separately for input and output.

Input Axes

The orientation of the input axes is important, for example, for orthotropy and foundation properties or the effect of a surface load.

The list in the 'Category' section offers various options for adjusting the axis position:

• Angular rotation: Rotation of the xy surface axes about the z axis by the angle α
• Axis parallel to lines: Orientation of the x or y axis along a line
• Axis directed to point: Orientation of the x or y axis to the intersection of a line with the surface
• Axis parallel to coordinate system: Orientation of the axes to a user-defined coordinate system

You can determine the reference objects graphically using the button .

The 'Reverse Local Axis z' check box allows you to orient the z and y axes in opposite directions.

Result Axes

Currently, the orientation of the result axes is only possible 'Identical to the Input Axes'.

Grid for Results

Every surface is covered with a grid that is used for the result output in the tables. It enables an output independent of the FE mesh at regular, adjustable result points.

By default, a Cartesian surface grid with a uniform grid point spacing of 0.5 m in both directions is preset. If necessary, you can adjust the 'grid spacings' in the x-direction (b) and in the y-direction (h), perform a 'grid rotation', or change the 'grid origin'. For circular surfaces, the 'Polar' grid type offers an alternative for the numerical result output.

If the 'Adjust Automatically' check box is selected in the 'Options' section, the grid points are adapted to the new geometry when the surface is changed.

In the 'Points' section, you can check the coordinates of the generated grid points. Changes in the table are not possible.

Integrated Objects

RFEM usually recognizes all objects automatically that lie in the surface but were not used for the surface definition.

The numbers of the nodes, lines, and openings assigned to the surface are specified in the 'Integrated Objects in Surface' section.

If an object is not recognized, you should integrate it manually: Deactivate the automatic object detection. The input fields in the 'Integrated Objects in Surface' section are now accessible. Add the missing object number or use the button to determine the object graphically.

Activate Load Transfer

The check box makes it possible to distribute the load of the surface – regardless of its stiffness type – using a load transfer surface. In this way, the surface acts in the model through its stiffness. The distribution of the load to the adjacent objects, on the other hand, is controlled by the parameters that you can define in the Load Transfer tab. This function is primarily relevant for surfaces of the Beam Panel thickness type.

Deactivate for Calculation

The check box offers the option of not considering the surface in the calculation, for example, to simulate construction stages or to examine a modeling variant. In this case, the stiffness, boundary conditions, and loads of the surface are not applied.

Information | Analytical

This section is displayed as soon as you have defined the boundary lines of the surface. It provides an overview of important properties of the surface such as surface area, solid, and mass as well as the position of the surface's center of gravity and the orientation of the surface. Openings are taken into account accordingly.