C2. Modeling of the main elements

C.2.1 Creating the geometry

The first stage of modeling consists of creating the geometry of the model by defining points, lines, boundaries, areas, and volumes. The notions of nodes, elements, and meshes are associated with finite elements.

In some software, the geometry can be defined before creating nodes, elements, and meshes. In others, the geometry is established outside the software, using diagrams or Excel spreadsheets, and the nodes, elements, and meshes are then defined directly in the software.

In any case, the sign conventions used by the software must be known at the start of the modeling (direction of gravity in the global coordinate system, sign convention for bending moments, forces, and stresses).

Some general notions:

Nodes: their presence is essential at the supports, the joints, and the boundaries between geometries. Depending on the software, nodes should also be present where the data will be extracted. Please refer to § D.3.2 for more information. Depending on the software, a node must also be provided at each load application point. Finally, depending on the phenomena one wants to quantify, for example for large displacements or dynamic calculations, intermediate nodes must be defined on the beams to accurately represent them. Defining the points of the geometry means incorporating all these node requirements. However, the number of nodes must be limited to keep the model as light as possible.
Structural elements: in most non-solid models (bars, plates, shells ...), the elements will be modeled at their average fiber. This is the safest method for the good transmission of forces between elements and the consideration of secondary effects. In the case of beams for which the loads are located on a particular face (bridge secondary beams, for example), it is possible to define the element at this face and to create an offset, if the software does not do it automatically. The positioning of the average fiber of the elements with offsets is discussed in § C.7 ~~Offsets.~~Offsets. In the case of beams of variable height, the mean fiber is no longer a straight line, which leads to multiple local coordinate systems for the different inclinations and can complicate the exploitation of the results. If the arch effect is not considered, the model can be simplified by keeping the neutral fiber straight-lined.
See also the calculation examples for beam grids for which simplifications can be admitted (Link to the ~~examples)~~examples).

C.2.2 Degree of simplification: shafts and openings

Depending on the study phase and the type of calculation carried out (for example stability or load reactions), not all the openings will necessarily be modeled.

The case of buildings.

For buildings, when the openings are considered, it is advised to integrate into the geometry the shafts of non-negligible sizes and the ones which may affect the behavior of the structure (at least in the bracing elements). The latter will be cut according to the intersection wall/wall, wall/floor, shafts, to have a mesh as regular as possible.

In the case of modeling a building, the shafts are defined as a function of:

their size (any shaft in a wall or slab whose largest dimension is less than 1m is commonly neglected).
their spatial distribution - small but closely spaced openings can be considered as a single opening whose dimensions correspond to the perimeter of the envelope.
their influence on the force transmission.

Particular attention must be paid to the lintels of doors in structural walls (and bracings). Indeed, these lintels might have numerous openings, so they may no longer be able to fulfill their structural role. Consequently, the model must be adapted.

When the openings are not known, the modeling of buildings subjected to horizontal forces (wind, earthquake) must consider conservative measures concerning the large shafts (generally for ventilation). It is often necessary to reduce the thickness of the lintels fictitiously or even to remove them from the model.

Example of how to model a group of openings:

Example of a structure with close openings... which clearly cannot be neglected.

Case of steel construction. The CNC2M recommendations for the dimensioning of steel beams with openings in the web according to NF EN 1993 states that an isolated opening with a maximum dimension less than 10% of the height of the web of the beam is not considered significant. When modeling these openings, the same rule can be applied. Nevertheless, this opening must be considered when verifying the resistance of the cross-section according to NF EN 1993.

In the cases where there are wall collaborations with diaphragms made of ribbed plates, according to EN 1993-1-3 § 10.3.4, small regularly distributed openings whose cumulative surface area represents up to 3% of the total surface area may be arranged without any calculation of the diaphragm. It is doable as long as the total number of connections points of the panels constituting the diaphragm is respected. Thus, from a modeling point of view, such openings may not be considered.

C.2.3 Degree of simplification: curvature, slope, ...

When modeling the geometry, at the structural element scale, the curved elements will have to be represented as accurately as possible, knowing that the meshing phase will discretize these curvatures by a succession of straight segments, depending on the mesh size chosen and the nodes already defined. The part of the Eurocodes NF EN 1993-1-6 dealing with the strength and stability of shell structures gives some indications on how to take curvature into account.

For bridges, the effects of slope, curvature, and skew angle must be considered, and their non-inclusion in the model must be justified. For common straight structures, since the slope is normally limited at the design stage, it can generally be neglected. On the other hand, for curved structures:

depending on the level of the supports and the hyperstatic degree of the structure, the slope cannot be neglected.
whether the structure is curved over all or part of its length, the centrifugal force and the slope must be considered. It should be noted that the standard NF EN 1991-2 indicates that the centrifugal force, including dynamic effects, can be neglected if the radius of curvature of the pavement in the plan is greater than 1500m.
curvature and skew angle create non-negligible torsional moments in the structure even when the traffic is transversely centered on the structure.

To establish an order of magnitude, a structure can be considered as being of low sensitivity:

to the skew angle when it remains greater than or equal to 70 degrees.
to curvature when the angle between two adjacent supports is less than 0.3 rad.

However, it is difficult to establish general rules and the reader is invited to consult the design guides specific to each type of work (PRAD, PIPO, PICF, ...).

Illustration of the angle between two supports

The example of a girder grid "Modelling the same structure using different ~~approaches"~~approaches" (in Part 3) illustrates the effects of skew angle and slope on an example of girder bridges.

C.2.4 Degree of simplification: Alignment of structural walls of variable thickness

In the case of a building, a vertical alignment of the elements is recommended to ensure a simple load transmission. However, various requirements (sheltered equipment, available space, etc.) can lead to certain offsets from one level to another. A simplification of the geometry during the modeling can however be made (mainly to avoid excessively heterogeneous mesh) by aligning the vertical elements and even the horizontal elements.

This simplification results in a good representation of the overall functioning of the structure provided that the recommended constructive arrangements are respected. However, it is necessary to make a local verification of the proper functioning of the transfer of forces and to reintegrate the actual offsets in this local verification.

Similarly, for steel structures, in the presence of footings or tubes of variable thickness (ferrule for example), a single average plan is usually used.

For example, a tank composed of shells of different heights and thicknesses will be modeled with cylindrical surfaces with:

an identical radius equal to an equivalent average radius.
appropriate thicknesses according to the height (shell thickness).

The value of the equivalent mean radius can be defined according to the Seismic Guide for Storage Tanks DT108. This guide brings examples on how to determine an equivalent uniform thickness, which allows defining the value of the equivalent mean radius = Internal radius of the ferrule + Uniform equivalent half-thickness (see example below):

C.2.5 The use of symmetries

As discussed in Part 1 A2. The dimensionality of the model, when the structure presents a plane or planes of symmetry in its geometry, it can be very interesting to limit the calculation time and the size of the model by using this symmetry and model only a part of the structure. Appropriate boundary conditions must be applied on the plane of symmetry.

However, it is important to highlight the fact that the loading must also be symmetrical, and that the solution obtained will be symmetrical (for example, the antisymmetric natural frequencies will not appear).

Example 1: 4-span symmetrical bridge

The spans are 60/100/100/60m long. The bridge is symmetrical with respect to its midpoint.

One could be tempted to model half of the bridge, by placing a symmetry support condition at the center (on the right side of the figure, vertical translation blocked, rotation blocked):

Symmetrical load case:

In this case, the results are identical for both structures.

Case of asymmetrical loading:

In this case, there is a significant difference in the results:

The examination of the bending moment influence lines on the second support in both configurations provides an immediate explanation:

Example 2: Foundation mat

Square-shaped foundation slab modeled with shell elements.

The nodes have 6 degrees of freedom (ux, uy, uz, rx, ry, rz).

Because of its shape, it contains planes of symmetry. The following plane of symmetry was chosen as shown in the figure below:

The foundation slab can then be subjected to a loading that is either symmetrical or antisymmetrical.

For example:

if a bending moment is applied around the Y-axis, the loading is symmetrical.
on the other hand, if a bending moment is applied around X in the forward direction, the foundation slab turns upwards on the side with nodes Y>0 and downwards on the side with nodes Y<0. The loading is then antisymmetrical.

The conditions that must be applied to the nodes on the plane vary.

In the first case, the nodes located on the plane of symmetry will be:

free for translations ux, uz, and rotations around y.
blocked for translations uy and rotations around x and z.

In the second case (antisymmetric loading), the nodes located on the plane will be:

blocked for translations ux, uz, and rotations around y.
free for translations uy and rotations around x and z.

It is important to note that considering the different types of loading, in this case, leads to creating two models differing only by the boundary conditions associated with the loading, which is not prohibitive.

In the case of dynamic calculations of a soil volume, particular attention should be paid to the lateral boundary conditions of the block to correctly translate the conditions of non-reflection of the waves (see Part 1, chapter F.8). The definition of these spring-damper element systems is outside the scope of this guide.

Even if computing resources are very powerful nowadays, the use of symmetry remains an approach that can be very useful for complex calculations and/or for large models. It presents several delicate aspects that need to be understood.

C.2.6 Modeling of the foundations

Most of the time, the soil is modeled by support conditions (simple supports or clamps).

Before modeling the foundations and the soil in detail, the sensitivity of the structure to the flexibility of its foundations must be assessed.

If the structure is sensitive, the soil must be considered:

either indirectly through elastic supports or stiffness matrices, the parameters of which should be calibrated elsewhere.
or directly by modeling a certain volume of soil (soil portion + boundary elements). Note that this type of calculation requires special software.

In the case where the reliability of the soil parameters is low and/or their variability is high, it is recommended to perform a range calculation.

In some cases, having to model the structure with its foundations is a regulatory obligation. Refer to the NF-EN-1998-5 §6 standard.

For more details on boundary conditions, refer to § C.5 Boundary conditions.

C.2.7 Modeling of bracing by bars

Beware! In the case of steel structures, some very slender elements (braces or cables) can only work in traction. If the modeling does not take this into account, the strength and stiffness of the bracing are overestimated for both static and modal calculations.

Example of a simple braced structure

“As-built" modeling of a braced frame, but without considering the fact that the bracing bars will buckle as soon as they are put in compression:

In this case:

the horizontal deflection is 4.4 cm,
the maximum force in the diagonals is 321kN.

Because of the buckling of compressed diagonals, for the overall behavior, one diagonal out of two should be removed, ideally those that are compressed, but this is not a requirement:

In this case, the displacement increases from 4.4 to 7.6cm. Thus, the stiffness of this pier is divided by 7.6/4.4=1.73, which may have consequences on the verification of deformations and the calculation of proper natural frequencies for the seismic calculation (Error of the order of 1.730.5 =1.31).

Consequently, the efforts in the diagonals increase from 321 to 641kN, which is logically about twice as much.

C.2.8 Structural Zoom - Local Model

This is for example the case for spacers of mixed slabs, support zones of complex structures, or an arch/deck embedding in a bowstring bridge.

Sometimes the entire structure is modeled using beam elements except for a part modeled using plate elements. In this model, which incorporates beam and plate elements, it is necessary to check carefully that the transmission of forces from one to the other is carried out correctly (for example by ensuring the sufficient rigidity of fictitious connecting elements). See C.6.7.

Global modeling with beam elements (pseudo-volumetric view)

Local modeling with plate elements (view of average surfaces)