C5. Boundary Conditions
C5. Boundary Conditions
C.5.1 General case
The boundary conditions are determined by the degrees of freedom that can be fixed or not at the nodes located at the boundaries of the structure (supports, cuts ...).
The notions of reference frames and boundary conditions are closely related here. The orientation of a boundary condition (forces, moments, imposed displacements, accelerations...) will depend on the orientation of the current reference frame when it is implemented or on the entity (node, element) upon which it is applied.
In what concerns the coordinate systems, a distinction must be made between the ones linked to elements and the ones linked to the nodes.
Usually, by default, the node coordinate systems are identical to the global coordinate system. However, a different coordinate system can be assigned to one or several nodes in order to be able apply a boundary condition to the node(s) in a particular orientation. Simple graphical controls of the orientation of nodal loads (forces, moments, imposed displacements) enable visualizing the correct definition of these nodal coordinate systems.
For the elements, the local coordinate systems are generally linked to the main orientations defined during the creation of the element. Simple graphical controls of the orientation of the loads applied to the elements (such as pressure) allow visualizing the good definition of these element systems.
The boundary conditions must ensure the stability of the structure with respect to the loads applied and be representative of its overall behavior. Stability must systematically be reached in the 6 global components X, Y, Z, RX, RY, and RZ, even if the loads are applied only to a few directions.
Stability following a translation is always achieved by blocking at least one node in the direction of this translation.
Stability about an axis is achieved either by fixing one node in rotation (along the axis of rotation) or by blocking two nodes in translation in a plane perpendicular to the rotation.
It is important to check that the reactions in the fixed directions are zero in order to have numerical stability.
Example:
Objective: loading of a slab supported by 4 columns ;

The slab is modeled with solid elements (elements with nodes having 3 degrees of freedom UX, UY, and UZ),

Boundary conditions: fixing the nodes at the supports in the vertical direction UZ = 0.0,

Problem: some software will not perform the calculation because of instabilities,

Additional boundary conditions: 2 fixed nodes in the transverse direction OY + 1 fixed node in the transverse direction OX.
Summary:

4 nodes fixed in the OZ direction – the 4 supports are fixed vertically, which turns the slab stable in rotation/OX and rotation/OY,

2 nodes fixed along OY – stability of the slab in translational/OY and rotational/OZ,

1 node fixed along OX  stability of the slab in translation/OX.
We will check that at the nodes following UX and UY, the RX and RY reactions are zero.
Example of the minimum stability of a Zloaded slab
Be careful: the slab is loaded only in Z, but to ensure the stability of the calculation the translational motion in X and Y and the rotation around Z must be blocked. In this case, 2 points were blocked in Y and 1 point in X. (NB: stability in Z requires a minimum of 3 nonaligned points blocked in Z).
In a 3D model, an embedding means that the 3 rotations and the 3 translations are blocked.
In practice, without giving any choice to the user, the software can proceed in two ways to block the displacements:

A method that is always numerically stable, which consists in suppressing the DOF in the solution of the problem because its value is zero (see Part 2  A.1  in this case, a 5×5 matrix is used).

A second method consists in numerically placing a very stiff spring in the fixed direction so that the displacement is numerically close to zero. (see Part 2  A.1  in this case, a 9×9 matrix is used by adding terms of very different relative values).
It is important to understand how the software proceeds to be able to detect possible numerical instabilities that can lead to a halt in the calculations or unbalanced results.
C.5.2 Modelling different types of supports
Generally, the supports can be considered as fixed, except when the ground intervenes in the behavior of the structure, i.e. when there is a static or dynamic interaction between the soil and the structure (SSI). For instance, to model a soft ground generating differential settlements at the supports, or to define a seismic behavior.
Structures are based on three types of foundations: shallow foundations (isolated or spread footings), foundation slab, or deep foundations (piles, wells, bars, rigid inclusions, ...).
Illustration of shallow foundations, foundation slabs, and deep foundations.
C.5.2.1 Shallow foundations – For supports under columns
Shallow footings are modeled using punctual supports. They can be modeled in 3 different ways:
Illustration: clamped support, hinged support, and elastic support
Clamped support: the 6 degrees of freedom are blocked.
Hinged support: movements are blocked and rotations are free.
Elastic support: the support is defined by 6 elastic springs (one per degree of freedom), or stiffness or impedance matrices.
Stiffness of the elastic supports
To calibrate the stiffness of the elastic supports, the stiffness at the interface between the footing and the soil is required. This interface stiffness (usually denoted kv) is taken from the geotechnical report.
The term Kz (static stiffness of the spring against a vertical force) is obtained by the formula Kz = kv x S, with S the surface of the footing.
The terms KR are deduced from the formula KRi (in N.m/rad) = Ii x kv with Ii the inertia (in plane) around the axis of rotation i of the footing.
For a rectangle, we will find the terms Iy=b.a³/12 and Ix=a.b³/12, a and b being the dimensions in plane.
VIEW IN PLANE OF THE FOOTING
Particular attention will be paid to the notions of longterm, shortterm and seismic stiffnesses provided by the geophysicist, which differ significantly.
C.5.2.2 Shallow foundations – For supports under thin walls
Thin walls are generally modeled by plate or shell elements. Two types of models can be defined for the support.
Method 1: By defining linear supports distributed under the thin wall. This case is similar to that of the columns (see above) by distributing the punctual stiffnesses linearly along the wall, or to that of foundation slabs (see §5.2.3 below), but considering only one direction of calculation.
Method 2: By modeling a single central support to recover an overall torsor at the foot of the thin wall for designing the foundations. A rigid bar at the base of the thin wall is then necessary to distribute the forces. The support conditions are identical to those of the columns (embedded or elastic or with stiffnesses).
In both cases, the units for the introduced stiffness should be verified to remain consistent with the physical units provided by the geophysicist: are they N/m, N/m², N/m³? Is it also N.m/rad or N.m/deg? (or derived units: kN, MN...)
C.5.2.3 Concrete slab foundations
The support of the foundation slab on the ground is modeled by placing springs under its various nodes. The spring stiffnesses are then calculated according to the same principle as for isolated footings. They can be differentiated according to the loading zones. Be careful, the stiffness must be proportional to the surface area of the node (a possible issue in the case of an irregular meshing, if this assignment is not automatic in the software).
Some software also offer "surface" springs on plates. In any case, one must verify using a unitary case the good concordance between forces and displacements.
Soil modeling using a spring system
In reality, the horizontal stability of the foundation slab is ensured by the friction between the concrete and the soil, and a possible lateral abutment. For the model, either horizontal surface springs under the concrete base or springs on the periphery (punctual or distributed) will be chosen, depending on the internal verifications that must be carried out.
Caution: for models with horizontal surface springs, the horizontal stiffness is related to the friction between the foundation slab and the soil with possible slippage. In the case of a shrinkage study, an overestimation of this horizontal stiffness will artificially constrain the invert and may generate significant and unrealistic tensile stresses.
C.5.2.4 Pile Foundations
Pile foundations can be modeled using 3 methods.
Method 1: each pile is modeled using a beam on an elastic soil (or elastic linear supports). The horizontal soil stiffnesses depending on the characteristics of the soil layers (Kx and Ky) are generally determined by the geophysicist (pay attention to the mesh and the concordance of the units). A vertical support is positioned at the base of the pile to represent the point stiffness.
Method 2: (intermediate but little used) each pile is modeled by an elastic support (or matrix) characterized by 6 stiffnesses that are generally calculated by the geophysicist.
Method 3: It is possible to replace a complex foundation by its stiffness or flexibility matrix, which integrates the overall configuration of the footing with the set of piles.
The foundation will be modeled in the general model by an elastic support at node A, whose 6 stiffnesses will have been calculated beforehand from a local foundation model. See the example below.
Because of the coupling between horizontal displacements and rotations in deep foundation systems, there is no apparent reason to neglect the crossterms (nondiagonal) of the stiffness matrix. However, very few software allow considering the whole matrix, which is a problem. It must be demonstrated on a casebycase basis that the "diagonalization" of the matrix has no significant impact on the stresses and displacements of the structure.
Methods 2 and 3 allow the size of the model to be limited, especially in the case of many piles. On the other hand, the first method gives the stresses in the piles directly.
More generally, in global models, piles or groups of piles are modeled by springs (method 3). It is only for designing the piles themselves that one may want to model vertical beams with springs (method 1). Specific software can also be used.
In any case, it is important to remember to include in the Kx or Ky coefficients all the normative requirements such as the group effect.
Finally, if the piles are calculated by an entity other than the one in charge of the superstructure model, iterations may be necessary to achieve the convergence of efforts.
Example of calculation of a stiffness matrix.
Data: 1.20m diameter piles, Concrete Young Modulus E= 30000MPa, Ksoil= 6495(kN/m)/m, footing height 2.00m.
Geometry
Unitary results (1kN or 1kN.m) introduced
Results:
Displacements under the loads = flexibility matrix [S]
Stiffness matrix [K]=[S]1  (units : KN, KN.m, m and rad)
(The matrices are easily inverted using a spreadsheet).
An indication that the cross terms were not considered: a pile of height 10m and section 5.00×1.00m², E=32000MPa is added to the previous model. The same stack is modeled with a 6component elastic embedding, which are the terms of the diagonal of the matrix above. A force of 1000kN longitudinal (respectively transverse) is applied at the top:
In this case, a deviation of about 13% on the longitudinal displacement (respectively 17% on the transverse displacement) is obtained  the flexibility of the pile comes into play but it is identical in both cases. It is up to the engineer to judge the impact of this possible simplification.
One of the topics that must be addressed in the general hypothesis report is related to the simplifications that will be accepted or not for the SSI calculation. On the one hand, they are related to the consideration of the short and long term modules of the soil (ratio of 2 on K) and of the concrete constituting the structure (ratio of 3 on E). On the other hand, they are related to the constitutive laws introduced for the soil (linear, with several slopes, with a possible plasticization step). Depending on the software used, wanting to integrate all these factors can be very complex, leading to the assembly of several differentiated models and the need to carry out certain verifications manually (replacement of plasticized springs by an equivalent force, for example). In some cases, it may be interesting to perform a range calculation, distinguishing between resistance and deformation verifications.
Illustration of the complexity of the constitutive law of soil springs
C.5.3 Modeling of support devices
There are two ways to model the support devices of a structure:

either as a support, with the degrees of freedom and flexibility parameters of the device. In this case, the support reactions are recovered,

or as a bar element with several modeling possibilities (described below).
In any case, the support devices must be placed at the real location (transverse and vertical offsets), otherwise, large errors will occur.
It should be noted that the behavior of the support devices can be a source of nonlinearity (sliding supports, for example) and may require a de facto nonlinear calculation.
Example of a bridge pile model including the elastomeric bearings.
If bar elements are used, there are several possible choices:

some software propose elements resembling connections that can reproduce the characteristics of the bearings (it is not strictly speaking a bar),

one can also use "spring" elements between two bars, if the software allows it,

one can define a "shear beam", i.e. a bar that is very rigid in bending but with a calibrated deformability to the shear force. The software must necessarily consider the shear deformation (option not activated by default in some software). It is defined for this bar a weightless section, an elevated inertia, a strong straight section, and a section reduced to the shear efforts, allowing to find an equivalence of the support device (for the GS/h bar ⇔ G'S'/T for the support device),

finally, we can use a classic bar, working in flexion, embedded in the bottom and free at the top. It is defined for this bar, a weightless section, a section reduced to the shear efforts, and a calibrated inertia is then defined to have a global deformation equivalent to that of the apparatus (for the 3EI/h3 bar ⇔ G'S'/T for the support apparatus ).
Regardless of the method, the element must have an overall behavior equivalent to the characteristics of the supporting devices, as defined by the standards for supporting devices (NF EN 1337 series) and it must not introduce any moment neither in the deck or in the pile (other than that related to the thickness of the device).
The illustration below shows rigid extensions allowing to model the top of a pile supporting two isostatic spans, simply connected by a flooring.
Modeling details of a pile supporting two isostatic spans
No Comments