Infinite Elements

The node numbering for infinite elements must be defined such that the first face is the face that is connected to the finite element part of the mesh.

The infinite element nodes that are not part of the first face are treated differently in explicit dynamic analysis than in other procedures. These nodes are located away from the finite element mesh in the infinite direction. The location of these nodes is not meaningful for explicit analysis, and loads and boundary conditions must not be specified using these nodes in explicit dynamic procedures. In other procedures these outer nodes are important in the element definition and can be used in load and boundary condition definitions.

Except for explicit procedures, the basis of the formulation of the solid medium elements is that the far-field solution along each element edge that stretches to infinity is centered about an origin, called the “pole.” For example, the solution for a point load applied to the boundary of a half-space has its pole at the point of application of the load. It is important to choose the position of the nodes in the infinite direction appropriately with respect to the pole. The second node along each edge pointing in the infinite direction must be positioned so that it is twice as far from the pole as the node on the same edge at the boundary between the finite and the infinite elements. Three examples of this are shown in Figure 3, Figure 4, and Figure 5. In addition to this length consideration, you must specify the second nodes in the infinite direction such that the element edges in the infinite direction do not cross over, which would give nonunique mappings (see Figure 6). Abaqus will stop with an error message if such problems occur. A convenient way of defining these second nodes in the infinite direction is to project the original nodes from a pole node; see Projecting the Nodes in the Old Set from a Pole Node. The positions of the pole and of the nodes on the boundary between the finite and the infinite elements are used.

Figure 3. Point load on elastic half-space.

Figure 4. Strip footing on infinitely extending layer of soil.

Figure 5. Quarter plate with square hole.

Figure 6. Examples of an acceptable and an unacceptable two-dimensional infinite element.

The nodes of acoustic infinite elements need to be defined only for the face that is connected to the finite element part of the mesh. Additional nodes are generated internally by Abaqus in the direction of the “node ray” (see Figure 1). The node rays, which are discussed earlier in this section in the context of defining the reference point, define the sides of the acoustic infinite elements.

In plane stress and plane strain analyses when the loading is not self-equilibrating, the far-field displacements typically have the form $u=\ln \left(r\right)$, where r is distance from the origin. This form implies that the displacement approaches infinity as $r\to \mathrm{\infty }$. Infinite elements will not provide a unique displacement solution for such cases. Experience shows, however, that they can still be used, provided that the displacement results are treated as having an arbitrary reference value. Thus, strain, stress, and relative displacements within the finite element part of the model will converge to unique values as the model is refined; the total displacements will depend on the size of the region modeled with finite elements. If the loading is self-equilibrating, the total displacements will also converge to a unique solution.

In direct-integration implicit dynamic response analysis (Implicit Dynamic Analysis Using Direct Integration), steady-state dynamic frequency domain analysis (Direct-Solution Steady-State Dynamic Analysis), matrix generation (Generating Structural Matrices), superelement generation (Using Substructures), and explicit dynamic analysis (Explicit Dynamic Analysis), infinite elements provide “quiet” boundaries to the finite element model through the effect of a damping matrix; the stiffness matrix of the element is suppressed. The elements do not provide any contribution to the eigenmodes of the system. The elements maintain the static force that was present at the start of the dynamic response analysis on this boundary; as a consequence, the far-field nodes in the infinite elements will not displace during the dynamic response.

During dynamic steps the infinite elements introduce additional normal and shear tractions on the finite element boundary that are proportional to the normal and shear components of the velocity of the boundary. These boundary damping constants are chosen to minimize the reflection of dilatational and shear wave energy back into the finite element mesh. This formulation does not provide perfect transmission of energy out of the mesh except in the case of plane body waves impinging orthogonally on the boundary in an isotropic medium. However, it usually provides acceptable modeling for most practical cases.

During dynamic response analysis the infinite elements hold the static stress on the boundary constant but do not provide any stiffness. Therefore, some rigid body motion of the region modeled will generally occur. This effect is usually small.

In many applications, especially geotechnical problems, an initial stress field and a corresponding body force field must be defined. For standard elements you define the initial stress field as an initial condition (Defining Initial Stresses) and the corresponding body force field as a distributed load (Distributed Loads). The body force cannot be defined for infinite elements since the elements are of infinite extent. Therefore, Abaqus automatically inserts forces at the nodes of the infinite elements that cause those nodes to be in static equilibrium at the start of the analysis. These forces remain constant throughout the analysis. This capability allows the initial geostatic stress field to be defined in the infinite elements, but it does not check whether or not the geostatic stress field is reasonable. If the initial stress field is due to a body force loading (such as gravity loading), this loading must be held constant during the step. In multistep analyses it must be maintained constant over all steps.

You must remember that when infinite elements are used in conjunction with an initial stress condition, it is essential that the initial stress field be in equilibrium. In Abaqus/Standard any procedure that determines the initial static (steady-state) equilibrium conditions is suitable as the first step of the analysis; for example, static (Static Stress Analysis); geostatic stress field (Geostatic Stress State); coupled pore fluid diffusion/stress (Coupled Pore Fluid Diffusion and Stress Analysis); and steady-state fully coupled thermal-stress (Fully Coupled Thermal-Stress Analysis) steps can be used. To check for equilibrium in Abaqus/Explicit, perform an initial step with no loading (except for the body forces that created the initial stress field) and verify that the accelerations are small.