ALE Adaptive Meshing and Remapping in Abaqus/Explicit

In an adaptive meshing increment, a new, smoother mesh is created by sweeping iteratively over the adaptive mesh domain. During each mesh sweep, nodes in the domain are relocated—based on the current positions of neighboring nodes and elements—to reduce element distortion. In a typical sweep a node is moved a fraction of the characteristic length of any element surrounding the node. Increasing the number of sweeps increases the intensity of adaptive meshing in each adaptive meshing increment. The default number of mesh sweeps is one.

ADAPTIVE MESH, MESH SWEEPS=number of sweeps

The process of mapping solution variables from an old mesh to a new mesh is referred to as an advection sweep. At least one advection sweep is performed in every adaptive mesh increment. Ideally, an advection sweep will be performed only once, after all mesh sweeps for the increment are complete. However, numerical stability of the advection sweep is maintained only if the difference between the old mesh and the new mesh is small. Therefore, if after a mesh sweep the total accumulated movement of any node in the domain is greater than 50% of the characteristic length of any adjacent element, an advection sweep is performed to remap the solution variables from the old mesh to the intermediate mesh. Mesh sweeps will continue until the specified number is reached or until the movement of any node again exceeds the 50% threshold. At this time an advection sweep is performed again to map variables from the last intermediate mesh to the new intermediate mesh. The cycle will continue until the number of mesh sweeps reaches the specified number.

The number of advection sweeps per adaptive mesh increment required for each adaptive mesh domain is determined automatically by Abaqus/Explicit; you cannot override this automatic calculation. The number of advection sweeps is printed by default to the message (.msg) file (see Output and Diagnostics for ALE Adaptive Meshing in Abaqus/Explicit).

For problems without spatial adaptive mesh constraints or Eulerian boundary regions, the default frequency for adaptive meshing is 10, and the default number of mesh sweeps is 1. The default values are usually adequate for low- to moderate-rate dynamic problems and for quasi-static process simulations undergoing moderate deformation. If the frequency or number of mesh sweeps is too low, excess element distortion may cause the analysis to terminate before the mesh is adapted; or, if a solution can be obtained, it may not be as accurate as the solution that could be obtained with a higher quality mesh. In virtually all cases, however, performing adaptive meshing at any frequency will reduce the distortion of elements (and, thus, improve the quality of the solution) compared to a pure Lagrangian analysis.

For high-rate impact problems undergoing large amounts of deformation, it may be necessary to increase the frequency of adaptive meshing or the number of mesh sweeps. It is generally less expensive to increase the number of mesh sweeps slightly before increasing the frequency, as long as the number of advection sweeps remains small.

For problems involving explosions taking place over just a few hundred increments, adaptive meshing is usually required at every increment. It may also be necessary to increase the frequency of adaptive meshing for quasi-static process simulations that involve large amounts of flow per increment.

For problems in which the deformation per increment is small, a high-quality mesh can be maintained by performing adaptive meshing only every 25–100 increments. For these problems the additional cost of adaptive meshing is negligible.

When an adaptive mesh domain contains Eulerian boundary regions or has spatial adaptive mesh constraints, the default frequency of adaptive meshing is 1. This default frequency is conservative and is chosen primarily because spatial mesh constraints are applied only during adaptive mesh increments. Thus, between adaptive mesh increments the mesh may drift from its prescribed location, which may affect the solution. However, drift from adaptive mesh constraints will always be eliminated in the next adaptive mesh increment: it will not accumulate.

For problems in which the speed of deformation or the speed of material flow from element to element is much less than the material wave speed, the frequency typically can be increased to 5 or higher. This class of problems includes most steady-state process simulations, where the drift of the mesh from the prescribed location is negligible over a few increments. By performing adaptive meshing less often, steady-state simulations become competitive with their corresponding transient simulations. For Eulerian domains in which the speed of the deformation or material flow is high, such as in dynamic shock problems, the default frequency of 1 should be used.

Volume smoothing relocates a node by computing a volume-weighted average of the element centers in the elements surrounding the node. In Figure 1 the new position of node M is determined by a volume-weighted average of the positions of the element centers, C, of the four surrounding elements. The volume weighting will tend to push the node away from element center C1 and toward element center C3, thus reducing element distortion.

Figure 1. Relocation of a node during a mesh sweep.

Volume smoothing is very robust and is the default method in Abaqus/Explicit. It works well for both structured and highly unstructured domains. (A structured domain is one that contains no degenerate elements and where every node is surrounded by four elements in two dimensions or eight elements in three dimensions.)

Laplacian smoothing relocates a node by calculating the average of the positions of each of the adjacent nodes connected by an element edge to the node in question. In Figure 1 the new position of node M is determined by averaging the positions of the four nodes, L, connected to M by element edges. The locations of nodes L2 and L3 will pull node M up and to the right to reduce element distortion.

Laplacian smoothing is the least expensive smoothing algorithm and is commonly used in mesh preprocessors. For low to moderately distorted mesh domains, the results of Laplacian smoothing are similar to volume smoothing. For domains with boundaries of complex curvature, volume smoothing generally results in a more balanced mesh.

Equipotential smoothing is a higher-order method that relocates a node by calculating a higher-order, weighted average of the positions of the node's eight nearest neighbor nodes in two dimensions (or its eighteen nearest neighbor nodes in three dimensions). In Figure 1 the new position of node M is based on the position of all the surrounding nodes, L and E.

The weighted averaging for the equipotential smoothing method is fairly complex and is based on the solution of the Laplace equation. Equipotential smoothing tends to minimize the local curvature of lines running across a mesh over several elements. Although this tendency can be desirable for gently curving domains, it can inhibit the ability of equipotential smoothing to reduce element distortion in highly deformed and locally curved domains.

Equipotential smoothing can be performed only for nodes that are surrounded by a locally structured mesh. Nodes that are surrounded by an unstructured mesh are moved with an equivalent amount of volume smoothing when equipotential smoothing is chosen.

The default smoothing method in Abaqus/Explicit is volume smoothing. To choose an alternate smoothing method or to combine smoothing methods, you specify the weighting factor for each method. When more than one smoothing method is used, a node is relocated by computing a weighted average of the locations predicted by each chosen method. All weights must be positive, and their sum should typically be 1.0. If the sum of the chosen weights is less than 1.0, the mesh smoothing algorithm will be less aggressive at each adaptive mesh increment. If the sum of the chosen weights is greater than 1.0, their values are normalized so that their sum is 1.0.

ADAPTIVE MESH CONTROLS, NAME=name
volume smoothing weight, Laplacian smoothing weight, equipotential smoothing weight

ADAPTIVE MESH CONTROLS, NAME=name
0.5, 0.0, 0.5

The conventional forms of the basic smoothing methods do not perform well in highly distorted domains. To ensure the robustness of adaptive meshing, Abaqus/Explicit uses geometrically enhanced forms of the basic smoothing algorithms by default. The enhanced forms are recommended for all adaptive mesh applications. However, since the basic smoothing algorithms are used by many finite element preprocessors, their conventional forms are provided as an option.

ADAPTIVE MESH CONTROLS, NAME=name, 
GEOMETRIC ENHANCEMENT=NO

For adaptive mesh domains without any Eulerian boundary regions, the default objective of the mesh smoothing methods is to minimize mesh distortion while improving element aspect ratios, at the expense of diffusing initial mesh gradation. The uniform mesh smoothing objective is recommended for problems with moderate to large overall deformation.

ADAPTIVE MESH CONTROLS, NAME=name, 
SMOOTHING OBJECTIVE=UNIFORM

Alternatively, the smoothing methods can attempt to preserve initial mesh gradation while reducing element distortion as the analysis evolves. This objective is the default for adaptive mesh domains with one or more Eulerian boundary regions. The graded mesh smoothing objective is recommended only for adaptive mesh domains with reasonably structured graded meshes undergoing low to moderate overall deformation. Element distortion will be minimized, but the aspect ratios of adjacent elements will be maintained approximately. Mesh gradation is particularly useful in steady-state problems where overall deformations are small and a focused mesh is used in a specific area to capture high solution gradients.

ADAPTIVE MESH CONTROLS, NAME=name, 
SMOOTHING OBJECTIVE=GRADED

If an adaptive mesh domain has no Eulerian boundary regions, then, by default, the mesh sweeps are based on current nodal locations, which account for material motion accumulated since the last adaptive mesh increment. This approach is generally the best for Lagrangian problems that undergo large overall deformation.

ADAPTIVE MESH CONTROLS, NAME=name, 
MESHING PREDICTOR=CURRENT

Mesh sweeps can be based on the locations of nodes at the end of the previous adaptive mesh increment. This technique is recommended for problems that are Eulerian in nature, where material flow is significant compared to overall deformation. Therefore, it is the default for adaptive mesh domains with one or more Eulerian boundary regions. This approach will result in a virtually stationary mesh.

ADAPTIVE MESH CONTROLS, NAME=name, 
MESHING PREDICTOR=PREVIOUS

Second-order advection is used by default for all adaptive mesh domains. It is recommended for all problems, ranging from quasi-static to transient dynamic shock. An element variable, $\varphi$, is remapped from the old mesh to the new mesh by first determining a linear distribution of the variable in each old element, as illustrated in Figure 2 for a simple one-dimensional mesh.

Figure 2. Second-order advection.

The linear distribution of $\varphi$ in the middle element depends on the values of $\varphi$ in the two adjacent elements. To construct the linear distribution:

1. A quadratic interpolation is constructed from the constant values of $\varphi$ at the integration points of the middle element and in its adjacent elements.

2. A trial linear distribution, ${\varphi }_{trial}$, is found by differentiating the quadratic function to find the slope at the integration point of the middle element.

3. The trial linear distribution in the middle element is limited by reducing its slope until its minimum and maximum values are within the range of the original constant values in the adjacent elements. This process is referred to as flux-limiting and is essential to ensure that the advection is monotonic.

Once the flux-limited linear distributions are determined for all elements in the old mesh, these distributions are integrated over each new element. The new value of the variable is found by dividing the value of each integral by the new element volume. (See Figure 3 for a first-order example of this calculation.)

Figure 3. First-order advection.

ADAPTIVE MESH CONTROLS, NAME=name, ADVECTION=SECOND ORDER

First-order advection is simple and computationally efficient; however, it tends to diffuse sharp gradients over time, especially in transient dynamic analyses or other problems that require fairly frequent adaptive meshing. Therefore, this technique should be used only as a computationally efficient alternative for quasi-static simulations that do not require frequent adaptive meshing.

Figure 3 illustrates the first-order method for a portion of a one-dimensional mesh. An element variable, $\varphi$, is remapped from the old mesh to the new mesh by first assuming a constant value of the variable for each old element. These values are then integrated over each new element. The new value of the variable is found by dividing the value of each integral by the new element volume.

ADAPTIVE MESH CONTROLS, NAME=name, ADVECTION=FIRST ORDER

The element center projection method is the default method used to advect momentum and requires the fewest numerical operations. The element momentum is calculated first for the old mesh based on the mass and velocity of the element nodes. The element momentum is then advected from the old mesh to the new mesh by the same first- or second-order algorithms used for advecting element variables. Finally, the element momentum on the new mesh is assembled at the nodes using a projection. The element center projection method requires the advection of only two or three extra variables in two dimensions or three dimensions, respectively.

ADAPTIVE MESH CONTROLS, NAME=name, 
MOMENTUM ADVECTION=ELEMENT CENTER PROJECTION

The half-index shift method is computationally more intensive than the element center projection method, but it may result in less wave dispersion for some problems. This method first shifts each of the nodal momentum variables from the nodes surrounding an element to the element center. The shifted momentum variables are then advected from the old mesh to the new mesh by the same first- or second-order algorithms used for advecting element variables, providing momentum variables at the center of the new elements. Finally, the momentum variables at the element centers in the new mesh are shifted back to the nodes. The half-index shift method requires the advection of 8 or 24 extra variables in two or three dimensions, respectively, which can increase the cost of each advection sweep significantly.

ADAPTIVE MESH CONTROLS, NAME=name, 
MOMENTUM ADVECTION=HALF INDEX SHIFT