The 'Mesh Settings' dialog manages the general specifications for generating the FE mesh. You can open this dialog using the Mesh Settings entry in the Calculate menu or the list button
.
General
In the General tab, you can adjust the default mesh size that RFEM uses when generating the FE mesh.
General Settings
The 'Target length of finite elements' controls the mesh size with which the FE mesh is generated. The shorter the FE length, the finer the mesh and the more accurate the results generally are. However, the amount of data and the calculation time also increase, because additional equations must be solved for each additional FE node. A fine mesh also leads to singularity effects becoming more pronounced.
For special boundary conditions (for example, the same number of nodes in close proximity on opposite surface edges), it is possible that the meshing algorithm ignores the target length and instead generates a regular mesh.
The 'Maximum distance between a node and a line' specifies the distance of a node from a line at which it is automatically integrated into the line. If the distance of the node is greater than this limit value, RFEM creates a new FE node.
Options
The 'Prefer independent mesh' check box allows you to generate specific FE meshes for surfaces or solids with integrated objects. For example, for a slab on a soil massif, the solid of the soil massif can be represented with a coarser FE mesh than the slab. The number of finite elements is significantly reduced in this way.
Members
The Members tab controls how the FE mesh is generated on members.
If necessary, you can adjust the 'Number of divisions' for result diagrams, for special member types, and for determining extreme values. If you increase the divisions, you achieve a refined result diagram. In most cases, however, the default settings prove to be sufficient.
The value of 'Divisions for result diagrams' influences the graphical result diagram of members that have no further FE mesh division, for example due to an FE mesh refinement or connected surface. With a division of 10, the length of the longest member in the system is divided by 10. This system-related division length is then used to determine the graphical result diagrams at the intermediate points for each member.
The 'Divisions for straight members with the material category Concrete' have an influence on the nonlinear reinforced concrete calculation of members in the cracked state. Thus, the Concrete Design add-on can, among other things, determine the stiffness (uncracked/cracked) in each finite element for the deformation analysis.
The 'Activate member divisions for large deformation analysis, structure stability, dynamic analysis' option allows you to also divide beam members by intermediate nodes for analyses according to the large deformation analysis or with regard to stability and dynamics, and thus capture them with higher accuracy. In this case, the number of divisions for 'special member types' is applied (second input field above).
With the 'Division by nodes lying on members' option, FE nodes are created at member locations where other members connect to the member but have no connection to the member.
Surfaces
The Surfaces tab controls how the FE mesh is generated on surfaces.
The most accurate results are determined for finite elements that come close to a square. For a square, the ratio of the diagonals D1/D2 is = 1. As the 'Maximum ratio of FE rectangle diagonals', the limit value ΔD of this diagonal ratio is preset to 1.8. If you reduce the value, more triangle elements will be created. A value that is too large, in turn, leads to elements with very acute or very obtuse angles being generated. This can lead to numerical problems.
A curved surface is covered by planar elements in the FE mesh. The inclination angle α defines the 'Maximum inclination of a single quadrangle element out of the plane'. This value describes the angle between the normals of two elements (see image Inclination angle α). If the allowable inclination angle is exceeded, a subdivision into triangle elements is performed.
The 'Mesh refinement along lines' function for surface models of the '2D | XY | Slab' type is still in progress.
With the 'Integrate unutilized objects into surfaces' option, you can also generate FE nodes at objects that have no further function for a surface (for example, free nodes without support or load, construction lines in surfaces). This function is deactivated by default so that statically insignificant objects do not distort the FE mesh.
You can influence the 'Shape of finite elements' using three selection fields:
- Triangles and quadrangles: default setting
- Only triangles: variant if quadrangles lead to a heavily distorted mesh
- Only quadrangles: option for increased result accuracy
You have further control options with the 'Generate identical squares where possible' and 'Triangles for membranes' check boxes.
With the 'Oriented FE mesh' option, RFEM tries to adapt the FE mesh to the boundary lines of the surfaces. You can specify this type of FE mesh generation separately for each surface (dialog 'Edit Surface', tab 'Mesh refinement').
An oriented mesh is formed exclusively from quadrangles. In general, an oriented mesh provides "more accurate" results. Since fewer unknowns also occur in the equation system, this method is recommended for mesh generation.
Solids
The Solids tab controls how the FE mesh is generated on solids.
If you activate the 'Mesh refinement on solids with close nodes', RFEM performs a mesh refinement for solids whose nodes are very close to each other. In this way, the nodes are correctly captured with the FE mesh. The mesh size of the solid results from the smallest distance between the nodes.
The 'Maximum number of elements' represents the upper limit of the generated 3D elements.
The 'Target length of finite elements for solids of the soil type' check box is accessible when the Geotechnical Analysis add-on is activated (license required). This allows you to specify a specific default mesh size LFE for soil massifs and generate coarser solid meshes without "mesh refinements".
Quality Criteria - Surfaces
The Quality Criteria - Surfaces tab manages the quality specifications for generating the 2D elements.
Quality Criteria
In this section, various criteria are specified that are checked after generating the FE mesh. If you deactivate a criterion, RFEM does not perform the corresponding check.
For each check type, you can specify from which value a 'warning criterion' and a 'failure criterion' exist.
Color Display
After generating the FE mesh, the 'Number of elements' that meet the quality criteria is displayed, as well as possibly those where a problem exists. This allows you to assess the quality of the FE mesh.
The quality of the FE mesh can also be checked on the model: In the 'Navigator - Display', activate the Mesh quality in the 'FE mesh' category.
Quality Criteria - Solids
The Quality Criteria - Solids tab manages the quality specifications for generating the 3D elements.
Quality Criteria
In this section, various criteria are specified that are checked after generating the FE mesh. If you deactivate a criterion, RFEM does not perform the corresponding check.
For each check type, you can specify from which value a 'warning criterion' and a 'failure criterion' exist.
Color Display
After generating the FE mesh, the 'Number of elements' that meet the quality criteria is displayed, as well as possibly those where a problem exists. This allows you to assess the quality of the FE mesh.
Wind Simulation
The Wind Simulation tab is displayed when the 'Wind Simulation' add-on for the CFD simulation RWIND is activated in the Model Base Data.
The parameters are described in the chapter Mesh Settings - Wind Simulation of the RWIND manual.
