Defining ALE Adaptive Mesh Domains in Abaqus/Standard
ALE adaptive meshing in Abaqus/Standard:
maintains a topologically similar mesh;
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 in static stress/displacement analysis, steady-state transport analysis,
coupled pore fluid flow and stress analysis, and coupled temperature-displacement
analysis;
can be used only in geometrically nonlinear general analysis steps; and
is available only for acoustic elements and a subset of the solid elements.
You can apply ALE adaptive mesh smoothing to an entire
model or to individual parts of the model as a step-dependent feature. Adaptive meshing for
solid elements in Abaqus/Standard uses a subset of the adaptive meshing functionality available in Abaqus/Explicit.
You must specify the portion of the original mesh that will be subject to adaptive meshing.
Modifying an ALE Adaptive Mesh Domain
By default, all adaptive mesh domains defined in the previous analysis step remain
unchanged in the subsequent step. You define the adaptive mesh domains in effect for a
given step relative to the preexisting adaptive mesh domains. At each new step the
existing adaptive mesh domains can be modified and additional adaptive mesh domains can be
specified (except in Abaqus/CAE, where only one adaptive mesh domain can be in effect for a given step).
Removing an ALE Adaptive Mesh Domain
If you choose to remove any adaptive mesh domain in a step, no adaptive mesh domains will
be propagated from the previous step. Therefore, all adaptive mesh domains that are in
effect during this step must be respecified.
Splitting ALE Adaptive Mesh Domains
Abaqus/Standard may subdivide each adaptive mesh domain that you specify such that
all elements in an adaptive domain refer to one element property definition; and
all elements in an adaptive domain are of similar type (such as hybrid elements with
linear pressure).
If Abaqus/Standard subdivides the adaptive mesh domains that you specified, each of the adaptive mesh
domain subdivisions will have a new name, which will be used for output and diagnostic
purposes. The new names will be formed by concatenating the name of the user-specified
element set, a number identifying the subdivision, and the step number. Each of the
subdivisions will be further examined to ensure that all the elements in a subdivision are
subjected to the same body forces. You may be asked to modify the definition of the
adaptive mesh domain to satisfy this requirement.
ALE Adaptive Mesh Regions
Each adaptive mesh domain has an interior region and a boundary region. The boundary region
may include distinct kinks that take the form of geometric edges or corners. The nodes on
the boundary region are, therefore, further separated into free surface nodes, edge nodes,
and constrained nodes. Different updating rules are applied to nodes in these different
regions. These regions are created automatically by Abaqus/Standard. You can control the detection of the geometric features. In addition, mesh constraints
can be applied to any node in the adaptive mesh domain.
Since acoustic elements do not have displacement degrees of freedom, their treatment for
adaptive meshing includes some additional considerations. The acoustic adaptive domain must
be connected to the structural domain using a surface-based tie constraint with the
secondary surface defined on the acoustic domain. Thus, an acoustic adaptive domain has an
additional boundary region that is connected to the structural domain. These secondary
surface nodes are updated based on the displaced configuration of the main surface nodes on
the structural domain, without permitting relative sliding between the surfaces. The
displacements of the main surface defined on the structural domain, together with nonzero
adaptive mesh constraints, serve as the forcing function that drives adaptive mesh smoothing
of an acoustic adaptive domain. The mesh smoothing algorithm will produce no changes in the
acoustic adaptive domain if these displacements are zero.
Nodes in the interior region are defined as nodes that are surrounded entirely by
elements in the adaptive mesh domain. By default, the new position of an interior node is
computed from the positions of the adjacent nodes that are connected through element edges
to the node in question. These nodes can move in any direction.
To control the displacement of these nodes, you can apply an adaptive mesh constraint in
any direction.
ALE Adaptive Mesh Boundary Regions
The boundary region is that part of the surface of the adaptive mesh domain that is not
constrained to other elements in the mesh. The nodes on the boundary region are further
separated into surface nodes, edge nodes, corner nodes, and constrained nodes.
Surface, Edge, and Corner Nodes
Surface nodes are defined as nodes at which the surrounding surface facets have the
same normal vector within a user-defined angle. These nodes are constrained against
movement in the normal direction, but sliding in any tangential direction is permitted.
The new position of a surface node is computed from the positions of the adjacent nodes
that are connected through the edges of the surface facets to the node in question.
Edge nodes are nodes in a three-dimensional model at which the surrounding surface
facets have two different normals and where the vectors along two of the surface edges
are colinear. Nodes on an edge can slide only along the edge. The new position of an
edge node is computed from the positions of the two adjacent nodes along the edge.
Corner nodes are nodes at which all the surrounding surface facet normals are
different. These nodes are constrained against all mesh smoothing movement.
You can control the displacement of these node types on the boundary region by applying
an adaptive mesh constraint in any direction.
Constrained Nodes in an Acoustic Adaptive Domain
A surface-based tie constraint can be used to connect two acoustic surfaces together.
When both the main and secondary nodes of the tie constraint belong to the same adaptive
mesh domain, the main surface nodes are updated according to the rules for surface,
edge, and corner nodes. An adaptive mesh constraint can be applied at main surface
nodes. Secondary nodes are updated by applying a tie constraint. Adaptive mesh
constraints cannot be applied at secondary surface nodes.
Mesh smoothing is not applied to these nodes when the main and secondary nodes belong
to different acoustic adaptive mesh domains.
The classification of boundary region nodes as surface, edge, and corner nodes is performed
based on the identification of geometric features in the mesh's configuration at the start
of a step where adaptive mesh domains are defined and is updated as the analysis proceeds
and the configuration changes. You can define the criteria that Abaqus/Standard uses in classifying geometric features through adaptive mesh controls.
Controlling the Detection of Geometric Edges and Corners
Geometric features are identified initially as edges on boundary regions where the angle
between the normals on adjacent element faces is greater than the initial geometric
feature angle, (), as shown in Figure 1. The default value for the initial geometric feature angle is . Setting will ensure that no geometric edges or corners are formed on the
boundary of the adaptive mesh domain. You can define adaptive mesh controls to change the
value of the angle that will be used to recognize geometric features.
Controlling the Activation and Deactivation of Geometric Edges and Corners
Abaqus/Standard allows geometric features, and consequently the updating rules applied at a node, to
change during the analysis. For example, nodes are constrained to lie along a discrete
geometric edge unless the angle forming the geometric edge becomes less than the
transition geometric feature angle, (). The default value for the transition feature angle is . If the angle across the geometric edge becomes less than , the boundary surface is considered to be flattened sufficiently for the
feature to be deactivated, and the mesh is allowed to slide freely on the surface.
Geometric corners are allowed to flatten in a similar fashion. In addition, surfaces that
are initially flat might develop edges or corners during the simulation. This logic allows
great flexibility in mesh adaptation while preserving geometric features in the model.
Setting will ensure that no geometric edges or corners are ever deactivated. You
can change the transition feature angle using adaptive mesh controls.
Abaqus/Standard will issue a warning message when geometric features are activated or deactivated.
Mesh Constraints
In most adaptive mesh problems the motion of nodes in the mesh is determined by the mesh
smoothing algorithm, with constraints imposed by the domain boundary and the boundary region
edges. However, there might be cases when you will want to define the motion of the nodes
explicitly. You might also want to keep certain nodes fixed, to move nodes in a particular
direction, or to force certain nodes to move with the material.
Adaptive mesh constraints give you the flexibility to define the motion of the node
explicitly.
Applying Spatial Mesh Constraints
Spatial mesh constraints are applied to define the motion of the nodes explicitly.
Spatial mesh constraints allow full control over the mesh movement and can be applied to
any node except those that have Lagrangian mesh constraints applied to them.
You can also prescribe the spatial mesh constraints via user subroutine UMESHMOTION. The user subroutine
allows you to let the spatial mesh constraints depend on available nodal or material point
information.
Defining Mesh Constraints That Vary with Time
The prescribed magnitude of a nonzero mesh constraint can vary with time during a step
according to an amplitude definition (see Amplitude Curves).
Applying Spatial Mesh Constraints in Local Directions
Mesh constraints are applied in local directions if a transformed coordinate system is
used at a node (Transformed Coordinate Systems); otherwise,
they are applied in global directions.
Applying Lagrangian Mesh Constraints
Lagrangian mesh constraints on a node are used to indicate that mesh smoothing should not
be applied; that is, the node must follow the material.
Spatial Mesh Constraint Considerations
When you decide on the type of spatial adaptive mesh constraint, (displacement, velocity,
or specified with a user subroutine), you should consider the guidelines below.
Choosing between Displacement and Velocity Adaptive Mesh Constraints
Displacement and velocity mesh constraints differ in their application. Displacement
constraints define a node’s displacement relative to its original coordinates, while
velocity constraints define a node’s velocity relative to the motion of the material.
You will use a displacement constraint to control a node’s motion to a specific
coordinate location, while you will use a velocity constraint to control a node’s motion
relative to the Lagrangian motion. Therefore, a constant velocity adaptive mesh
constraint does not in general lead to a constant velocity of the node relative to its
original coordinates.
Applying Spatial Adaptive Mesh Constraints to Model Material Ablation
Your spatial mesh constraint is applied without regard to the current material
displacement at the node. This behavior allows you to prescribe mesh motion that differs
from the current material displacement at the free surface of the adaptive mesh domain,
effectively eroding, or adding, material at the boundary. Using adaptive mesh
constraints this way is an effective technique for modeling wear or ablation processes.
As described above, in common ablation modeling cases you will use the velocity form of
the constraint. In addition, for general boundary shapes the most effective interface
for ablation is user subroutine UMESHMOTION, where you can apply
spatial mesh constraints to the nodes on the free surface in general ways according to
solution-dependent variables, if needed. The user subroutine interface provides a local
coordinate system that is normal to the free surface at the surface node, enabling you
to describe mesh motions in this local system.
Modifying ALE Adaptive Mesh Constraints
By default, all adaptive mesh constraints defined in the previous analysis step remain
unchanged in the subsequent step. You define the adaptive mesh constraints in effect for a
given step relative to the preexisting adaptive mesh constraints. At each new step, the
existing adaptive mesh constraints can be modified and additional adaptive mesh
constraints can be specified.
Removing ALE Adaptive Mesh Constraints
If you choose to remove any adaptive mesh constraint in a step, no adaptive mesh
constraints will be propagated from the previous step. Therefore, all adaptive mesh
constraints that are in effect during this step must be respecified.
Contact
When surfaces are defined for large-sliding contact, adaptive meshing might relocate the
nodes on the surfaces. If the bodies in contact are sliding or deforming considerably, you
might want to use Lagrangian mesh constraints on the boundary of the surfaces to prevent the
surfaces from sliding from their intended place.
For small-sliding contact Abaqus/Standard assumes that the reference configuration does not change significantly. If the reference
configuration does not change significantly, the amount of adaptive meshing on these
surfaces should be small and the contact quantities computed based on the reference
configuration should continue to remain valid (Abaqus/Standard updates the tangent planes if nodes change positions). Hence, Abaqus/Standard will allow the nodes on the contact surface to move as needed by the mesh smoothing. You
should apply Lagrangian mesh constraints in cases where nodes are intended to remain
nonadaptive.
Initial Conditions
Initial temperatures and field variables can be defined on any region subjected to adaptive
mesh smoothing. However, these variables will not be remapped from the original to the
updated configuration.
Loads
For elements with displacement degrees of freedom, no restrictions are made to loads
applied to adaptive mesh domains. In cases where loads are intended to follow the material
motion, Lagrangian mesh constraints must be applied to the nodes on the boundary of the
surface on which distributed loads are applied to prevent the surface from sliding. This
will allow adaptive meshing to occur inside the surface while maintaining the location of
the distributed load.
All the nodes on which concentrated loads are applied become nonadaptive.
Special consideration is given to nodes on which boundary conditions are applied. No
adaptive meshing is done in the direction in which the boundary condition is applied, but
adaptive meshing is carried out in other directions. When a boundary condition on any degree
of freedom is removed (see Boundary Conditions) in a step, the
node becomes nonadaptive, since Abaqus/Standard will ramp off the corresponding reaction force or flux over the duration of the step.
Boundary conditions on scalar degrees of freedom will cause the node to become
nonadaptive.
The boundary conditions that can be applied to an acoustic domain are described in Acoustic, Shock, and Coupled Acoustic-Structural Analysis. These boundary conditions cannot be applied in any
analysis procedure in which mesh smoothing can be performed.
Predefined Fields
There are no restrictions on applying prescribed temperatures or field variables in an
adaptive mesh domain, but these nodal values are not remapped when adaptive meshing is
performed. Therefore, predefined fields that are not constant might not be meaningful in an
adaptive mesh domain.
Material Options
For elements with displacement degrees of freedom all material models that are isotropic
and homogeneous can be used in an adaptive domain. Material options that have anisotropic
behavior such as anisotropic materials (see Defining Fully Anisotropic Elasticity), jointed
material models (see Jointed Material Model), and concrete
material models (see Concrete Smeared Cracking) cannot be used
in an adaptive mesh domain.
For acoustic elements the relevant material models are described in Acoustic, Shock, and Coupled Acoustic-Structural Analysis. Mesh smoothing assumes that the geometric changes in the
acoustic domain do not lead to changes in material properties, such as fluid density.
Elements
Adaptive mesh domains can be defined for all acoustic first-order and second-order planar,
axisymmetric, and three-dimensional elements in Abaqus/Standard and for a limited number of other elements. Table 1
provides a list of supported elements.
Acoustic elements will typically undergo adaptive meshing during static procedures and then
participate in subsequent acoustic procedures in their updated configuration.
Deformable elements that are declared rigid cannot be part of adaptive mesh domains.
Elements in the adaptive domain cannot contain embedded elements or rebars.
Symmetric results transfer cannot be done from an axisymmetric model that had solid
elements in an adaptive domain.
Import cannot be done from a model that had solid elements in the adaptive domain.
It is not meaningful to drive a submodel using the nodes from a global model that were
part of an adaptive mesh domain.
Only enhanced hourglass control can be used with reduced-integration elements.
When used with acoustic elements, adaptive mesh smoothing must be applied in steps
prior to a coupled structural-acoustic analysis. It cannot be applied during a
large-displacement dynamic analysis.
Mesh smoothing assumes that the geometric changes in the acoustic domain do not lead to
changes in material properties, such as fluid density.
The coupling between the fluid and structure must be defined using a surface-based tie
constraint with the secondary surface defined on the acoustic domain.
Nodes in the adaptive domain that are involved in constraints such as multi-point
constraints (General Multi-Point Constraints) and
equations (Linear Constraint Equations) should be
made nonadaptive by applying Lagrangian constraints.
Input File Template
Applying ALE Adaptive Meshing for Acoustic
Analysis
HEADING
…
ELEMENT, TYPE=…, ELSET=ACOUSTIC
Data lines to define acoustic elementsELEMENT, TYPE=…, ELSET=SOLID
Data lines to define structural elementsSURFACE, NAME=TIE_ACOUSTIC
Data lines to define the acoustic surface interface with the structural meshSURFACE, NAME=TIE_SOLID
Data lines to define the solid surface interface with the acoustic meshTIE, NAME=COUPLING
TIE_ACOUSTIC, TIE_SOLID
…
STEPSTATICADAPTIVE MESH, ELSET=ACOUSTIC, MESH SWEEPS=10
…
END STEP
**
STEPSTEADY STATE DYNAMICS, DIRECT
…
END STEP
Applying ALE Adaptive Meshing in Other Uses
HEADING
…
ELEMENT, TYPE=C3D8, ELSET=..
Data lines to define solid elementsNSET, NSET=LAG
Data lines to define nodes that should be nonadaptiveNSET, NSET=SPATIAL
Data lines to define nodes that will have spatial adaptive mesh constraints appliedELEMENT, TYPE=…, ELSET=SOLID
Data lines to define structural elementsSTEP, NLGEOM=YESSTATICADAPTIVE MESH, ELSET=SOLID, MESH SWEEPS=10
ADAPTIVE MESH CONSTRAINT, CONSTRAINT TYPE=LAGRANGIAN
LAG
ADAPTIVE MESH CONSTRAINT, CONSTRAINT TYPE=SPATIAL, USER
SPATIAL
END STEP