Diagnosing common issues with FE meshing

The first stage of successfully carrying out a finite element analysis is the formation of a valid finite element mesh. The Masterframe FE module utilises an auto-generation algorithm to form the mesh and for the majority of structural layouts this will be able to form a valid mesh. However, there are circumstances where the algorithm will be unable to create a valid mesh topology, which will lead to either a failure to form a mesh error message and no mesh, or the software will encounter invalid element shapes and the analysis will fail to run, despite the display of a mesh on the structure. In each case, the underlying issue is geometrical. It should be noted, however, that is the geometry of the mesh based on the constraints and restrictions placed on the mesh, rather than the geometry of the FE surface boundary, and issues can arise with the mesh even when the overall geometry of the FE surface boundary would appear to be quite simple.

The requirements of a valid FE mesh

The aim of the FE mesh is to provide a valid discretization of a structure that represents the overall geometry of the structure and incorporates the relevant support conditions and constraint conditions imposed by other structural elements (which may or may not themselves be modelled as FE surfaces). This requires that the FE mesh has the following properties:

1.The finite elements around the perimeter of the surface have their outer edge aligned with the boundary of the FE surface

2.Nodes within the plane of the FE surface are picked up within the FE mesh such that the corners of elements in the vicinity of the node coincide with the node

3.The connection between adjacent finite elements is such that the corners of the elements coincide such that adjacent elements share a common edge

4.Where FE surfaces meet, such as at the junction between slabs or between slabs and walls, there must be compatibility in the finite elements along the common boundary line such that nodes meet at corners and so that two elements that meet along the boundary share a common edge.

5.The edges of the finite elements along the line of attached beams, or where the mesh is set to mesh to members, align with the beam or member

6.The finite elements remain 4-sided in shape.

A typical example of a valid mesh is shown below. The example is made up of two FE surfaces with a common boundary at the middle of the slab. The FE mesh is automatically generated by the software using a meshing algorithm which attempts to form a mesh which complies with the above requirements.

Fig.1 Basic mesh layout

The more constraints on the mesh topology, the more complex the required mesh geometry and the difficult the task of finding a valid FE mesh.

Some of the typical constraints that can be created in a mesh are discussed below. In most cases, these constraints do not cause issues by themselves and it is only when used in combination and in significant numbers that issues tend to occur that affect the mesh and then lead to a finite element mesh arrangement that cannot be analysed.

Nodes in the FE surface

Since nodes in the plane of the FE surface (internally or on the surface boundary) need to be picked up by corner nodes of finite elements, nodes will affect the size and shape of the mesh, particularly where nodes lie within a short distance of other nodes. This leads to a local reduction in the mesh size, but the mesh algorithm will then transition back to the user defined global mesh size.

Fig. 2 Effect of closely spaced nodes on mesh size

A common cause for nodes in close proximity is where vertical elements above and below the surface do not fully align and consideration should be given to amending the geometry of the model to avoid this.

Nodes on the boundary of an FE surface will likewise have an influence on the size of the finite elements and hence the mesh, particularly if the node spacing is less than the global mesh size.

Fig. 3 Reduction in mesh size along boundary of FE surface due to node positions

A frequent situation whereby nodes are created close to the boundary of an FE surface is where columns are modelled inboard of the slab, to model the centroid of the column such that the edge of the column will display aligned with the slab edge when viewing the 3D view. This is often done in combination with the use of the column/slab stiff regions, which modifies the mesh to account for the column cross section and modifies the stiffness of the elements within the column footprint to better model the slab and column interaction. Unless it is intended to use the FE slab design module, in many cases it is more effective to model the column on the slab boundary.

Fig. 4 FE surface with columns positioned inboard of the boundary

Where nodes are associated with structural elements, it may not be possible to simplify the arrangement of the nodes. However, where nodes are not associated with structural elements such that they are not structurally necessary, they should be removed to reduce any unnecessary constraints or restrictions on the mesh.

Mesh to members adjacent to surface boundary

Where the mesh has been set to mesh to members, or where the member is an attached beam, and the member is located close to the edge of the FE surface, the mesh is reduced in size such that the elements local to the beam are able to fit within the gap between the member and boundary. This is similar to the case of nodes at small distance, but the effect now occurs over a length. An example is shown below.

Fig. 5 Reduction in mesh size occurring due to a member adjacent the FE surface boundary

The need to retain compatibility between finite elements edges and nodes means that the effect of the mesh size reduction affects an area around the member.

Where the member is located very close to the finite element surface the mesh can be forced to be extremely small, increasing the difficulty in forming a valid mesh.

Opening near slab boundary or edge

To form a valid mesh in the gap between the edge of an opening and a FE surface boundary, the mesh must be made up of a strip at least one finite element in width. Where the boundary of an opening occurs close to the edge of an FE surface this can then require a reduced mesh size in the strip between the opening and the surface boundary. The need to transition smoothly from a reduced mesh size to the global mesh size means this width of the strip between the opening and surface edge will affect the size of the mesh beyond the dimensions of the opening.

Fig. 6 Reduction in mesh size occurring due to opening near slab edge

Coincident FE surfaces adjacent boundaries

Similar to members and attached beams adjacent an FE surface boundary, coincident FE surfaces form a geometric restriction on the mesh as the finite element size is restricted by the dimension of the gap between the coincident surface and the boundary. However, the geometry of the coincident FE surface can add some additional restrictions on the mesh which can further restrict the geometry of the mesh.

An example is shown below: -

Fig. 7 Reduction in mesh size occurring due to a coincident FE surface adjacent a slab edge

The effect of the reduced mesh size also influences the mesh to the coincident surface. In the above example, the width of the walls and the nodes that form the geometry of the wall will influence the mesh in both the wall and slab.

Surfaces wrapping around another surface edge or boundary

When using an FE surface to model a base to a wall, the meshing algorithm will start the mesh at a point on one side of the common boundary and follow the line of this boundary which produces a mesh that ‘wraps’ around the intersection of the surfaces. An example is shown below.

Fig. 8 Base slab mesh wrapping round the intersecting (vertical) surfaces

Where the resulting mesh geometry for the wrap around mesh becomes difficult it can become more challenging to produce a valid mesh that can accommodate the various restraints on the mesh topology.

Large FE surfaces

When FE surfaces are representing large structural elements, for example large area floor slabs, particularly when the FE surface has a large number of constraints from other structural elements or geometry, the issues encountered in meshing can be due to the difficulty of forming a mesh in the large FE surface itself. This is more likely when the FE surface has edges that are not parallel or has a lot of internal constraints which are not parallel to the boundary, requiring the mesh to align in different orientations at different constraints.

Fig. 9 Example of a large FE surface with numerous geometric constraints

In such cases it may be necessary to divide the large FE surface into smaller regions. This does not require the FE surface being divided into smaller FE surfaces, rather introducing additional dummy members into the surface and then using the Local Surface Mesh options and selecting the Mesh to Internal Members options. This creates smaller sub regions within the surface that are used as part of the meshing algorithm.

User defined mesh properties

In addition to geometric constraints on the FE mesh, there are a number of user defined parameters which affect the topology of the mesh. These options are:

Default mesh size (Global option) : defines the basic mesh size

Mesh column/wall stiff region (Global option): modify the mesh globally to include stiff regions for all wall and columns

Mesh to members inside FE surfaces (Global option): mesh to members in all FE surfaces across the whole model

Local mesh intensities (Local option): specify modified mesh size at specific locations

Local surface mesh options (Local): define modified mesh size and/or mesh to members on a surface-by-surface basis

Slab stiff column/wall regions (local): define specific stiff regions per FE surface

Meshing problems

Meshing issues arise when constraints combine such that the meshing algorithm is unable to form a mesh which conforms to the requirements outlined in the “The requirements of a valid FE mesh” section above. The most common issue relates to the shape of the finite elements and will generate a warning message noting a bad element shape and the warning message will note the affected nodes.

An example of a Zero stiffness warning message and highlighted nodes is shown below

Fig. 10 Example of highlighting of bad FE mesh shape

Fig. 11 Close up of bad element shapes

In some circumstances the meshing algorithm will be unable to produce a mesh for an FE surface or part of the surface and this will generate an error message stating that “Mesh Generation for Region xx failed”, where xx is an index number for the FE surface or part of a surface. As part of the meshing algorithm, individual FE surfaces are subdivided into regions and the meshing proceeds on a region-by-region basis.

Resolving FE mesh problems

Unfortunately, since problems with the FE mesh are often related to combinations of constraint conditions, there is not a simple step-by-step process whereby all meshing issues can be resolved. Each occurrence of a meshing problem needs to be looked at from the perspective of the model geometry, mesh size and additional constraints and reviewed. Often the location of invalid shaped nodes will give some clue as to the location of the problematic constraint and can give some indication of the general area to review first.

Some initial steps to try to resolve meshing issues are:

Change the global mesh size – this can include making the mesh larger as well as smaller.

Change the Local Surface Mesh Options default mesh size – changes the mesh on the affected FE surface but leaves other     surfaces unchanged

Check the radius of influence for any defined Local Mesh Intensities to ensure compliance with the recommended minimum       radius

Turn off the global Mesh column/wall stiff region and Mesh to members options

The Local Mesh sizes, Local Surface Mesh Options and Slab Stiff Regions options are accessed by going to Analysis > FE Surface Meshing Options. For more details on these options, refer to the relevant section in the FE manual.

Changing the global mesh size can improve the coordination between the basic mesh and the refined or reduced mesh caused by other constraints. However, simply decreasing the global mesh size can lead to increased analysis times which may not be desirable for large models.

Reviewing the radius of influence for local mesh intensities ensures that the FE mesh is not attempting to transition between a reduced mesh size and the global mesh too quickly. The larger the radius the more gradual that transition in element size and this makes the task of developing a valid mesh easier.

Removing global mesh settings reduces globally assigned constraints and can reduce the complexity of the mesh. It does not remove specific constraints applied locally. If remeshing resolves the issue then this would suggest that globally applied constraints represent too much constraint on the mesh topology and indicate that a more targeted approach to applying mesh constraints may help to reduce the mesh complexity. For example, stiff regions applied to internal columns are less effective than for edge columns since the bending moments from the slab are often balanced in the internal column case and so it may be worth considering only using stiff regions on the perimeter columns.

If the above steps do not resolve the meshing problem, then a more detailed assessment of the constraints on the FE surfaces is required. Again, no set algorithm or steps can be defined and each problem has to be reviewed individually, but the following steps may be required

Remove any unnecessary nodes i.e., delete nodes that do not serve a specific purpose

Review local mesh intensities for both radius of influence and mesh size

Review nodes associated with structure that does not align correctly by using the Show and Merge Coincident Nodes tool. Areas where this occurs can be identified visually due to the very dense mesh in the region

Review the alignment of structure placed close to the edge of FE surfaces and consider simplifying where possible.

Where an FE surface is wrapping round another surface, “break” the wrapping effect by introducing internal members and using the Mesh to Internal members option from the Local Surface Mesh Options

Consider simplifying the surface geometry in areas where the boundary forms a sharp point (boundaries form an acute angle) or where curves have been modelled with many short facetted members and so requires a large number of nodes in close proximity.

Review the positioning of openings within a surface where the boundary of the opening is in close proximity to the boundary of the FE surface. Where openings are extremely close to the slab, consideration should be given to eliminating the very thin strip of FE surface between the opening and surface edge.

For large FE surfaces with changes in orientation and significant numbers of internal restraints (mesh-to-members or intersecting FE surfaces) it may help to sub divide the surface with dummy members to create a small number of mesh regions. This is done by adding new dummy members (no structural properties so no effect on the analysis) and using the Local Surface Mesh options by setting the Mesh to Internal Members option to ‘Selected’ and adding the new dummy members.

Fig. 12 Additional Dummy Members (shown in red) used to create additional sub regions to assist in FE mesh formation

Conclusion

A key step in any FE analysis is the discretization of the structure by the formation of a valid FE mesh. However, the FE mesh must comply to certain constraint conditions while also conforming to the geometric restrictions formed by the structure itself. The larger the number of constraints on the mesh, the more challenging it is to produce a valid mesh layout. Part of the power of FE lies in the ability to model complex geometries but this means that there is no simple step-by-step approach to resolving meshing problems when they occur. Some experimentation with meshing parameters may be required and, in some cases, it may be necessary to consider a degree of simplification of the geometry of the problem to allow the formation of a valid mesh.