The adaptive meshing technique in
Abaqus
combines the features of pure Lagrangian analysis and pure Eulerian analysis.
This type of adaptive meshing is often referred to as Arbitrary
Lagrangian-Eulerian (ALE) analysis. The
Abaqus
documentation often refers to “ALE adaptive
meshing” simply as “adaptive meshing.”
ALE adaptive meshing is a tool that makes
it possible to maintain a high-quality mesh throughout an analysis, even when
large deformation or loss of material occurs, by allowing the mesh to move
independently of the material. ALE adaptive
meshing does not alter the topology (elements and connectivity) of the mesh,
which implies some limitations on the ability of this method to maintain a
high-quality mesh upon extreme deformation. Refer to
About Adaptivity Techniques
for a comparison between ALE adaptive meshing
and other
Abaqus
adaptivity methods.
ALE adaptive meshing is distinct from the
pure Eulerian analysis capability in
Abaqus/Explicit.
The pure Eulerian capability supports multiple materials and voids within a
single element, which allows effective handling of analyses involving extreme
deformation (such as fluid flow). In contrast,
ALE elements are always 100% full of a single
material; while this formulation limits the deformation of material in the
model to the deformation of the elements, it allows more precise definitions of
material boundaries and more complex contact interactions. For more information
on pure Eulerian analysis, see
Eulerian Analysis.
Although the adaptive meshing techniques and the user interface are similar
in
Abaqus/Explicit
and
Abaqus/Standard,
the use-cases and the level of functionality are different. Adaptive meshing in
Abaqus/Explicit
is intended to model large-deformation problems. It does not attempt to
minimize discretization errors in small-deformation analyses. Adaptive meshing
in
Abaqus/Standard
is intended for use in acoustic domains and for modeling the effects of
ablation, or wear, of material. A comparison between the adaptive remeshing
functionality in
Abaqus/Explicit
and
Abaqus/Standard
is provided in this section.
can often maintain a high-quality mesh under severe material deformation
by allowing the mesh to move independently of the underlying material; and
maintains a topologically similar mesh throughout the analysis (i.e.,
elements are not created or destroyed).
In
Abaqus/ExplicitALE
adaptive meshing:
can be used to analyze Lagrangian problems (in which no material leaves
the mesh) and Eulerian problems (in which material flows through the mesh);
can be used as a continuous adaptive meshing tool for transient analysis
problems undergoing large deformations (such as dynamic impact, penetration,
and forging problems);
can be used as a solution technique to model steady-state processes
(such as extrusion or rolling);
can be used as a tool to analyze the transient phase in a steady-state
process; and
can be used in explicit dynamics (including adiabatic thermal analysis)
and fully coupled thermal-stress procedures.
In
Abaqus/StandardALE
adaptive meshing:
can be used to solve Lagrangian problems (in which no material leaves
the mesh) and to model effects of ablation, or wear (in which material is
eroded at the boundary);
can be used to update the acoustic mesh when structural preloading
causes significant geometric changes in the acoustic domain; and
can be used in geometrically nonlinear static, steady-state transport,
coupled pore fluid flow and stress, and coupled temperature-displacement
procedures.
Activating ALE Adaptive Meshing
Adaptive meshing can be applied to an entire model or to individual parts of
a model. A Lagrangian adaptive mesh domain will be created, so that the domain
as a whole will follow the material originally inside it, which is the proper
physical interpretation for most structural analyses. Additional options are
provided for controlling the mesh. In
Abaqus/Explicit
analyses you can define Eulerian boundaries to allow material to flow into or
out of the domain modeled.
To take full advantage of all the adaptive mesh features in
Abaqus,
it is important to understand the concepts of adaptive mesh domains, boundary
regions, boundary edges, geometric features, and mesh constraints. These
concepts are explained in
Defining ALE Adaptive Mesh Domains in Abaqus/Explicit
and
Defining ALE Adaptive Mesh Domains in Abaqus/Standard.
Instructions for applying boundary conditions, loads, and surfaces to adaptive
mesh boundaries are also provided in those sections.
ALE Adaptive Meshing and Remapping in Abaqus/Explicit
and
ALE Adaptive Meshing and Remapping in Abaqus/Standard
outline the methods used to move the mesh and to remap solution variables to
the new mesh. These sections also present options for controlling these
algorithms. Although the default methods have been chosen to work well for a
wide variety of problems, you may wish to override the defaults to balance the
robustness and efficiency of adaptive meshing or to extend the use of adaptive
meshing to relatively difficult or unusual applications.
Adaptive meshing is of great value in a variety of problems.
Abaqus/Explicit
and
Abaqus/Standard
each employ adaptive meshing in ways that provide the greatest value within the
particular solver.
Uses in Abaqus/Explicit
In problems where large deformation is anticipated the improved mesh
quality resulting from adaptive meshing can prevent the analysis from
terminating as a result of severe mesh distortion. In these situations you can
use adaptive meshing to obtain faster, more accurate, and more robust solutions
than with pure Lagrangian analyses.
Adaptive meshing is particularly effective for simulations of metal forming
processes such as forging, extrusion, and rolling because these types of
problems usually involve large amounts of nonrecoverable deformation. Because
the final shape of the product can be drastically different from the original
shape, a mesh that is optimal for the original product geometry can become
unsuitable in later stages of the process when large material deformation leads
to severe element distortion and entanglement. Element aspect ratios can also
degrade in zones with high strain concentrations. Both of these factors can
lead to a loss of accuracy, a reduction in the size of the stable time
increment, or even termination of the problem.
Uses in Abaqus/Standard
You can use adaptive meshing to enable acoustic domain meshes to follow the
large deformations of the bounding structure. In other applications you can use
adaptive meshing and adaptive mesh constraints to model arbitrarily large
amounts of ablation of material away from the domain.
Adaptive meshing of acoustic regions greatly extends the utility of acoustic
analysis procedures.
Abaqus
can be used to model the response of a coupled structural-acoustic system
subjected to structural preloads. By default, the structural-acoustic
calculations are based on the original configuration of the acoustic domain.
This approximation is adequate as long as the boundary between the fluid and
structure does not experience large deformation during application of the
preload. However, when the geometry of the acoustic domain changes
significantly as a result of structural loading, the original acoustic
configuration must be updated. An example is the interior cavity of a tire
subjected to inflation, rim mounting, and footprint pressure loads.
The acoustic elements in
Abaqus
do not have mechanical behavior and, therefore, cannot model the deformation of
the fluid when the structure undergoes large deformation.
Abaqus/Standard
solves the problem of computing the current configuration of the acoustic
domain by periodically creating a new acoustic mesh that uses the same topology
as the original mesh but with the nodal locations adjusted so that the
deformation of the structural-acoustic boundary does not lead to severe
distortion of the acoustic elements.
The geometric changes associated with the new acoustic mesh are then taken
into account in a subsequent coupled structural-acoustic analysis. However, it
is assumed that the material properties of the fluid, such as the density, do
not change as a result of mesh smoothing.
Adaptive meshing can also model effects of ablation, or wear, by enabling
you to define boundary mesh motions independent of the underlying material
motion. An example is the wearing of a tire during its life, an effect that can
significantly affect the performance of the structure.
Comparison of ALE Adaptive Meshing in Abaqus/Explicit and Abaqus/Standard
Adaptive meshing in
Abaqus/Explicit
is generally more robust and provides more features for controlling the mesh
than does adaptive meshing in
Abaqus/Standard.
ALE Adaptive Meshing in Abaqus/Explicit
Adaptive meshing in
Abaqus/Explicit
is designed to handle a large variety of problem classes, and employs a variety
of smoothing methods, with controls that you can use to tailor the adaptivity
to specific problems. The
Abaqus/Explicit
implementation allows you to do the following:
to create entirely Eulerian models;
to improve the quality of the mesh initially, before deformation begins;
and
to define tracer particles, which enable tracking and output of
material-based results quantities.
ALE Adaptive Meshing in Abaqus/Standard
Adaptive meshing in
Abaqus/Standard
uses a single smoothing algorithm that works well for structural acoustic
analyses and the modeling of ablation processes. The
Abaqus/Standard
implementation of adaptive meshing has the following limitations:
Initial mesh sweeps cannot be used to improve the quality of the initial
mesh definition.
The method is not intended to be used in general classes of
large-deformation problems, such as bulk forming.
Diagnostics capabilities are currently limited.
Illustrative Examples
To illustrate the value of adaptive meshing, simple examples of transient
and steady-state forming applications follow. For simplicity, two-dimensional
cases are shown. In each case
Abaqus/Explicit
is used in the simulation.
Axisymmetric Forging
In this example a well-lubricated rigid die of sinusoidal shape moves down
to deform a blank of rectangular cross-section (see
Figure 1).
A blank and a sinusoidal die.
The indentation depth is 80% of the original blank thickness. Material
extrudes upward and outward (radially) as the blank is indented. The die is
modeled with an analytical rigid surface, and the blank is modeled with
axisymmetric continuum elements in a regular mesh configuration. The blank is
assumed to have elastic-plastic material properties.
A pure Lagrangian analysis of this problem does not run to completion
because of excessive distortion in several elements, as shown in
Figure 2.
The contact surface cannot be treated correctly because of the gross distortion
of the elements at the troughs of the sinusoidal rigid surface.
Eventually, the purely Lagrangian analysis will terminate because of
excessive element distortion.
Adaptive meshing allows the problem to run to completion. A Lagrangian
adaptive mesh domain is created for the entire blank.
Abaqus/Explicit
automatically chooses suitable defaults for adaptive meshing; hence, the
adaptive mesh approach requires only two additional input lines:
Figure 3 and Figure 4 show the deformed mesh at various stages of the forming analysis. Because the mesh
refinement is maintained on the areas of the secondary surface that contact the die
troughs as the material flows radially, contact conditions are resolved correctly
throughout the analysis.
Deformed configuration at an intermediate stage of the
analysis. Deformed configuration upon completion of the analysis.
Steady-State Rolling Example
This example shows how adaptive meshing can be used in a steady-state
simulation to allow the flow of material through Eulerian boundaries on the
problem domain. A steel plate is passed through a symmetric roll stand to
reduce its height by 50%. This simulation is run until it reaches steady-state
conditions.
Figure 5
and
Figure 6
show the initial and final (steady-state) configurations in a purely Lagrangian
model of this problem.
The initial configuration of the roller and the undeformed blank in
the pure Lagrangian model. The final steady-state configuration in the pure Lagrangian
model.
Figure 7
shows this problem modeled using an Eulerian adaptive mesh domain, where
material flows through the mesh.
The initial Eulerian adaptive mesh domain.
Only the region near the roller is modeled. The exact location of the free
surface does not need to be known to set up the problem: it is created in a
likely location, and the final steady-state position is found as part of the
solution. Although not shown, a focused mesh can be used to capture steep
strain gradients directly beneath the roller. The Eulerian domain reaches the
same steady-state solution as obtained with the Lagrangian approach.
The Eulerian adaptive mesh domain is created by defining an inflow and an
outflow boundary on the adaptive mesh domain. Adaptive mesh constraints are
applied normal to these boundaries so that material will flow through the mesh
(see
Defining ALE Adaptive Mesh Domains in Abaqus/Explicit).
Frictional contact between the roller and the blank pulls material through the
adaptive mesh domain.
The problem is set up by making the following modifications to the input
file for the pure Lagrangian analysis:
HEADING
...
ELSET, ELSET=BILLET
...
ELSET, ELSET=INFLOW
...
ELSET, ELSET=OUTFLOW
...
NSET, NSET=INFLOW
...
NSET, NSET=OUTFLOW
...
SURFACE, NAME=INFLOW, REGION TYPE=EULERIAN
INFLOW, S1
SURFACE, NAME=OUTFLOW, REGION TYPE=EULERIAN
OUTFLOW, S2
***************************
STEPDYNAMIC, EXPLICITData line to specify the time period of the step
...
ADAPTIVE MESH, ELSET=BILLET, CONTROLS=ADAPT
ADAPTIVE MESH CONTROLS, NAME=ADAPT
ADAPTIVE MESH CONSTRAINT, TYPE=DISPLACEMENT
INFLOW, 1, 1, 0.0
100, 2, 2, 0.0
OUTFLOW, 1, 1, 0.0
...
END STEP
