Advices for mesh generation

Visual assessment #

The assessment of an FE-mesh is based essentially on three criteria:

  • Regularity
    • For all constructional elements a regular distribution and form of the elements should be preferred
  • Number of mesh elements between forcing nodes/lines
    • Floors: at least two mesh elements between forcing nodes/lines
    • Walls: at least two mesh elements in height, in many cases it can hardly be prevented that only one element is created in width or between openings, but in many cases it can hardly be prevented that only one element is created in width or between openings
  • Geometric form of mesh elements
    • Triangular mesh: equilateral triangles are optimal, acute-angled triangles with a smallest angle below 15° should be circumvented (heavily distorted elements) 
  • Quadrilateral mesh: squares are optimal, acute-angled quadrangles with a smallest angle below 30° should be circumvented (heavily distorted elements)

Automatic Mesh Check #


The automatic “mesh check” searches for heavily distorted elements, that can cause a reduced result quality. If heavily distorted elements are found, they are marked in the model. If necessary the display of “surface centers” has to be switched on (quick access button “graphic symbols”, on the bottom right).


Heavily distorted elements can be prevented in many cases by modifying the model. They are mostly caused by acute-angled components and closely spaced nodes. In some cases individual hevily distorted elements can be hardly avoided or only at great expenses. Although heavily distorted elements influence the result in their immediate proximity, they don’t influence the result in the rest of the model. Individual heavily distorted elements can be accepted, if they are not located at critical places in the model.

Automatic & Manual Mesh Refinement #


The parameter for mesh generation offer the option to use an “adaptive mesh size”. This applies to all selected domains. In many cases, the mesh is refined too strongly or in too many places. This can lead to an unnecessarily big set of equations and therefore to an unnecessarily long calculation time. To optimize the mesh generation, it’s recommended to refine the mesh manually.

If the mesh is deleted and rebuilt (e.g. for modifications on the model), all manual mesh refinements will be lost and have to be redone. The option for automatic mesh refinement is saved with the mesh parameters and will be used again when the model is remeshed.

Manual mesh refinement #

Manual mesh refinements are used to create locally smaller elements in a domain. They can be used to optimize the result quality and/or the calculation time.


The “uniform refinement” is used to refine manually generated rectangular elements, by defining the maximal edge length of the elements. It use for triangles is also possible but it normally leads to undesirable results.


With the “Refinement by bisection”, new nodes are created at the center points of the
mesh elements. 




“Refinement around nodes” divides the mesh adjacent to the selected nodes with the specified division ratio.


“Refinement along a line” divides the nodes adjacent to the chosen lines with the specified division ratio.

Mesh optimization #

The mesh substantially influences the result quality and the calculation time. In many cases it is useful to apply different mesh sizes to individual domains, in order to optimize the model.


The mesh is generated element by element. Consequentially, the parameters for mesh generation
(e.g. mesh size) remains constant for the whole domain. To define different mesh sizes for individual
parts of domains, the domain can be divided. Alternatively, the mesh can be refined manually.

If different mesh sizes are to be used in a model, the mesh generation is done in multiple steps. For each step, only domains are selected with the same mesh parameters.

The option “Create mesh only for unmeshed domains” excludes domains from mesh generation, that have already been meshed. For these domains the mesh remains uncanged.

Cut a Domain #

If a surface is divided into several domains, the parameters for mesh generation can be defined individually for each domain.


If a domain is divided by the function “cut a domain” after it has been defined, all other properties are preserved.

  • Supports and edge hinges
  • Load definition
  • Parameter for reinforcement, steel and timber design

Procedure & sequence #

When generating a mesh with different mesh sizes for individual domains, the transition from one mesh size to another should always be located in the domain with the greater mesh size. This can be achieved by an appropriate order of mesh generation.

To mesh individual domains with different mesh sizes, it is recommended to begin with the smallest mesh size and to increase the mesh size with every step.