Online manuals, introductory examples, tutorials, and other documentation.
4.23 FE Mesh Refinements
If no FE mesh refinements have been defined, the FE mesh is generated with the preset target FE length. The global parameters of the FE mesh are described in Chapter 7.2.2.
The concept of the FE-mesh generator does not allow retroactive adjustments to the mesh. However, you can use FE mesh refinements to influence the mesh generation for specific areas. With this, a user-defined discretization is done, which may be required, for example, in nooks, for connections of members to surfaces, or for a dynamic analysis of members.
The settings in this dialog section or table column allow you to control, which objects are included by the FE mesh refinement and how the refinement is carried out. Different options are available for selection.
Define a radial refinement area around a node that is extended in all spatial directions.
Instead of a circular refinement area, you can specify a rectangular zone for refinement.
Define regular spacings of FE nodes on a line.
The FE mesh of a line can be refined in regular intervals. This type of refinement is especially useful for lines with member properties.
The finite elements adjoining the line can be divided by a defined number of n rows. In this way, you can, for example, cover boundary areas of surfaces with a refinement. This type of refinement is comparable to the FE mesh refinement generation along lines generation option (see Chapter 7.2.2) available for 2D plates.
Specify a lateral length of finite elements that is set as the target mesh size for the entire surface.
Conversely, this type of refinement can also be used for surfaces with low significance for the analysis: As a "refinement", enter a mesh size that is larger than the global target FE length.
FE mesh refinements can also be defined for solids to influence the generation of 3D elements.
In the text box of the dialog box or the column of the table, enter the numbers of the objects that the refinement of the FE mesh should be applied to. In the New FE Mesh Refinement dialog box, you can use to select the objects graphically.
When you select a circular refinement around a node, you have to specify the radius of the refinement area. In addition, you have to define the Target FE Length in the center (Inner) and at the periphery (Outer) of the circle. If the FE length on the boundary of the refinement area corresponds to the global target length, RFEM gradually refines the mesh from the outside to the inside.
If there is a major difference between the inner and outer FE length, specify a broader radius. In this way, you can avoid generating acute-angled triangular elements within the refinement area.
When you select a rectangular refinement around a node, you have to define the area of refinement by its side length. In addition, you have to specify the Target FE length in the center (Inner).
When you select a line refinement by division, you have to define the number of division nodes. Then, the defined number of equally spaced FE nodes is generated on the line.
When you select a gradual line refinement, you have to define the number of rows n. Then, RFEM divides the finite elements of the surface that directly adjoin the line into the corresponding number of rows. Thus, a refinement in direction of the line is generated.
If the refinement on a line, surface, or solid has been selected, the target FE length for the corresponding object must be entered.