FE meshed walls

If walls have been modeled as meshed, when the structure is analyzed they will initially adopt the mesh type and size specified in Structure Properties. You can however override these in order to apply a user defined mesh to individual walls if necessary. Extra consideration of the analysis model may be required if openings have been placed within meshed walls.

By default FE meshed walls are created with isotropic analysis properties. Orthotropic properties can be specified if required to model walls that are assumed to be predominantly "one-way spanning", such as masonry wall panels and cross-laminated timber (CLT) panels.

Mesh type and size guidelines for FE walls

When creating walls, you first have to choose whether to use the mid-pier or meshed modeling option. Since mid-pier walls have a number of limitations the expectation is that in most cases the meshed option will be preferred.

Assuming you choose the meshed option, you then also need to consider what is an appropriate mesh size, and what type of 2D element (i.e. QuadDominant, Quad, or Triangular) is most appropriate. The defaults in Tekla Structural Designer are:

wall mesh horizontal and vertical size: 1m (3')
2D element type: QuadDominant

Benchmarking quad and triangular meshes against the equivalent mid-pier model and theory

A small laterally loaded wall model is investigated in order to benchmark the quad and triangular mesh types against an equivalent mid-pier model and theoretical results.

Model definition

A 12 tall x 6 long x 0.2 thick cantilever wall is subjected to a horizontal tip load of 100 and vertical tip load of -1000.

E = 13.4x10⁶

G = 5583x10³

P = 100

L = 12

h = 6

t = 0.2

Assumptions

Flexural and shear deformations are included.

Theory

Lateral deflection of vertical cantilever with rectangular section of length L, shear area A_vx and horizontal tip load P:

Substituting for the wall thickness, t and depth, h this becomes:

Note: The first term accounts for the deflection due to flexure, the second term accounts for the deflection due to shear. A usual reference for this is: https://en.wikipedia.org/wiki/Timoshenko%E2%80%93Ehrenfest_beam_theory

Models

Three models are initially considered as follows:

FE meshed wall (quad elements - default mesh size)
FE meshed wall (triangular elements - default mesh size)
Mid-pier wall

The FE meshed model parameters are then varied to investigate potential mesh sensitivity.

Note: Because the model consists of a single panel the QuadDominant and Quad meshing options result in identical meshes of quad elements only. In more complex models the QuadDominant option will result in a predominantly quad mesh, but with occasional triangular elements inserted where necessary.

Key results


Result	Theoretical formula	Theoretical value	FE meshed quad elements	FE meshed tri elements	Mid-pier
Mesh size			72 elements	170 elements	N/A
Lateral Support Reaction	-P	100	100	100	100
Support Moment	PL	-1,200	-1,200	-1,200	-1,200
Lateral Deflection		0.001409	0.001380	0.001333	0.001409

Comment on above results

As is to be expected, the lateral deflection reported for the mid-pier model exactly matches the value predicted by beam theory. What may at first seem surprising is that the lateral deflections reported for both the meshed models are slightly different. It must be borne in mind that while the answer given by beam theory is an accepted close approximation, it is assuming that plane sections remain plane, so a small difference in the deflection results when using an FE meshed model might be expected.

Mesh sensitivity study (quad elements)

To investigate the sensitivity of the lateral deflections to mesh size the analysis is repeated using a range of mesh sizes.


Result	Beam Theory	Quad elements
Result	Beam Theory	8 shells	72 shells (default)	288 shells	1152 shells

Lateral Deflection	0.001409	0.001334	0.001380	0.001386	0.001388

As shown above, the results for quad elements do not indicate any significant mesh sensitivity over a wide range of mesh sizes.


Result	Beam Theory	Triangular elements
Result	Beam Theory	22 shells	170 shells (default)	666 shells	2652 shells

Lateral Deflection	0.001409	0.001065	0.001333	0.001373	0.001384

The above results for triangular elements show a much greater mesh sensitivity. The model with 666 shells is the first that could be regarded as a reasonably converged result.

Conclusion

When using FE meshed elements for walls, quad elements are to be preferred as they are not particularly sensitive to the mesh size that is adopted. The same can not be said to be true for triangular elements. For this reason we would suggest using either the Quad dominant, or Quad only mesh types, for walls, with the Tri only mesh type being non-preferred.

While mid-pier walls have been shown to give accurate results for this simplistic example, they have significant limitations in real models, one of the main ones being that they do not cater for wall openings. For that reason they are also not generally recommended.

Adjust the wall mesh parameters specified in structure properties

Initially, the same mesh parameters are applied to all meshed walls in the structure. In order to adjust these, see the following instructions.

Go to the Project Workspace.
In the Structure tree, click Structure.
Go to the Properties window.
If necessary, in Wall Mesh Type, change the shape of the wall mesh:
- QuadDominant: (Default) mainly consists of quadrilateral 2D elements, but may use occasional triangular elements to create a better mesh.
- QuadOnly: only consists of quadrilateral 2D elements.
- Triangular: only consists of triangular 2D elements.
  
  Note: The Triangular option is not generally recommended for modeling walls. While for out of plane results there is little difference between quads and triangular elements, for in-plane results triangular elements are constant stress and quads are bi-linear.
Adjust the horizontal and vertical sizes of the wall mesh according to your needs.

Apply different mesh parameters to individual walls

If you need to apply different wall mesh parameters to specific walls, you can override the model mesh properties, and modify the properties of the individual wall. For more information, see the following instructions.

In the model, select the walls that you want to modify.
Go to the Properties window and locate the parameters under the Meshing heading.
Select Override model's
If required, in Wall Mesh Type, change the shape of the wall mesh:
- QuadDominant
- QuadOnly
- Triangular
Adjust the horizontal and vertical sizes of the wall mesh according to your needs.

Review the wall mesh before the analysis

In order to review the existing slab mesh in your model before running a particular analysis, see the following instructions.

In the Status bar at the bottom of the window, click Solver View.

The solver view opens.
Right-click anywhere in the solver view.
In the context menu, go to Solver models.
In the list, select the solver model appropriate to the analysis that you want to run.

If the wall mesh is applicable to the selected solver model, it is displayed.

Note:
The wall mesh is not displayed in the working solver model. This is because the working solver model displays the model in its form before any analysis, and 2D elements are only formed during the analysis.